Copyright: Copyright© 1997 by SolidWorks Corporation
Citation: Copyright© 1997 by SolidWorks Corporation.  All rights reserved.


3 Point Arc

Creates an arc through three points (start, end and midpoint).

To create a 3 point arc:

1	Click [image] or Tools, Sketch Entity, 3 Point Arc.

2	Point where you want the arc to start.

3	Press the mouse button and drag to where you want the arc to end.

4	Release the mouse button.

5	Drag the arc to set the radius and to reverse the arc, if necessary.

6	Release the mouse button.


Activate View/Activate Sheet

Activates a drawing view or drawing sheet.

To activate a drawing view:

In a drawing, double-click on the view or sheet you want to activate, or right-click on a view or sheet and click Activate View or Activate Sheet.


Assembly Mating

The entities and components that you selected for mating are listed in the Items Selected window. Examine the list to make certain that it is correct; scroll horizontally to see the entire list, if necessary.

1	Select the desired Mate Type and Alignment Condition . (Only those types and conditions that are valid for the selected features are available.)

2	In the Workbench area, click Preview. The parts move to the mating relation that you specified.

3	If this mating relation is acceptable, click Apply; if not, click Undo and try again.

To change the mating relation, click the name of the mate in the FeatureManager design tree, and select Edit Definition. Make your changes in the Assembly Mating dialog box.

See also Edit Mating Relations .


Mating Types

You can establish a mating relation between the faces, edges, vertices, or reference planes of components. The valid mating relations are:

•	Coincident: positions selected faces, edges, and planes (in combination with each other or combined with a single vertex) so they share the same infinite line. Positions two vertices so they touch.

•	Perpendicular: places the selected items at a 90 degree angle to each other

•	Tangent: places the selected items in a tangent mate (at least one item must be a cylindrical surface)

•	Concentric: places the selected cylinders so that they share the same center point

•	Parallel: places the selected items so they lie in the same direction and remain a constant distance apart from each other

•	Distance: places the selected items with the specified distance between them

•	Angle. places the selected items at the specified angle to each other


Alignment Condition

You can  specify an alignment condition for the mating relations. The conditions are:

•	Aligned: places the selected items so the solids are on the same side of the plane

•	Anti-Aligned (On): places the selected items so the solids are on opposite sides of the plane

•	Closest: makes the items aligned or anti-aligned, based on which position they are closest to at the beginning.


Add-Ins

Allows you to use other compatible software products that are installed on your computer with SolidWorks.

To use another software application along with SolidWorks:

1	Click Tools, Add-Ins.

The list of installed, compatible software shows in the dialog box.

2	From the list, select one or more applications that you want to use.

3	Click OK to add the application; click Cancel to close the dialog box without adding another application.


Add Relations

Creates geometric relations (like tangent or perpendicular) between sketch elements, or between sketch elements and planes, axes, edges, or vertices.

These are the same relations that are created automatically as you sketch (see Automatic Relations) and by the Mirror Sketch Elements sketch tool.

To remove a relation, use Display/Delete Relations .

To create a relation:

1	In a sketch, select the item(s) to relate.

At least one of the items must be a sketch element. The other item(s) can be either a sketch element or an edge, face, vertex, origin, plane, axis, or sketch curve from another sketch that forms a line or arc when projected on the sketch plane.

2	Click [image] or Tools, Relations, Add.

3	Select the relation you want to add, then click OK.

Available relations depend on the items you select:

To add  this relation...	Select...	Result:
Horizontal or Vertical	One  line or two points .	The line becomes horizontal or vertical (as defined by the current sketch space). Points are aligned horizontally or vertically.
Collinear	Two lines .	The two items lie on the same infinite line.
Coradial	Two arcs .	The two items share the same centerpoint and radius.
Perpendicular	Two lines .	The two items are perpendicular to each other.
Parallel	Two lines.	The two items remain parallel.
Tangent	An arc , ellipse , or spline , and a line , arc , ellipse , or spline .	The two items remain tangent.
Concentric	Two arcs , or a point and an arc .	The circles and/or arcs share the same centerpoint.
Midpoint	A point and a line .	The point remains at the midpoint of the line.
At Intersection	Two lines or one point .	The point remains at the intersection of the lines.
Coincident	A point and a line, arc , or ellipse .	The point lies on the line, arc, or ellipse.
Equal Length/Radii	Two lines , or  two arcs.	The line lengths or radii remain equal.
Symmetric	A centerline and two points , lines , arcs , or ellipses .	The items remain equidistant from the centerline, on a line perpendicular to it.
Fix	Any item.	The item’s size and location are fixed. However, the end points of a fixed line are free to move along the infinite line that underlies it. Also, the endpoints of an arc or elliptical segment are free to move along the underlying full circle or ellipse.
Pierce	A sketch point and an axis, edge, line, or spline.	The sketch point is coincident to where the axis, edge, or reference curve pierces the sketch plane.
Merge Points	Two sketch points.	The two points are merged into a single point.
Note	When you create a relation to a line, the relation is to the infinite line, not just the sketched line segment or the physical edge. As a result, some items may not physically touch when you expect them to.

Similarly, when you create a relation to an arc segment or elliptical segment, the relation is actually to the full circle or ellipse

Also, if you create a relation to an item that does not lie on the sketch plane, the resulting relation applies to the projection of that item as it appears on the sketch plane.

Additional relations are created automatically when you use the  Offset Entities Tool  and the Convert Entities Tool .


Align Drawing View

Reorients a drawing view by aligning a model edge horizontally or vertically, or in relation to another drawing view. Also, breaks view alignment relations that are automatically formed.

To reorient a drawing view:

1	In a drawing view, click the model edge you want to align.

2	Click Tools, Align Drawing View, then either Horizontal Edge or Vertical Edge. The selected view will rotate.

– or –

Click Tools, Align Drawing View, then either Horizontal To Another View or Vertical To Another View. Then click the view to which you want to align the current view. The selected view will snap into alignment.

To restore the position of a view that you aligned to another view:

1	Select the view.

2	Click Tools, Align Drawing View, Default Alignment. The selected view returns to its original position.

In a Standard 3 View drawing, the top and side views are aligned to the front view. The top view can only move vertically; the side view can only move horizontally. To move these views independently, you must break the alignment.

To break the alignment to another view:

Select a view and click Tools, Align Drawing View, Break Alignment.

To move the view, click the green border (not its handles) and drag.


Align Grid

Aligns the sketch grid with the model edge that you select.

To align the grid to a model edge:

1	Open a sketch on a model face.

2	Click Tools, Sketch Tools, Align Grid.

3	Click the model edge to which you want to align the grid.

4	Click Apply to apply the change.

The grid shifts to align with the edge you selected and the origin is placed at the end of the edge closest to where you clicked.

5	Click OK to accept the change and close the dialog box.

– or –

Click Close to close the dialog box. If you previously clicked Apply, the change is saved; if you did not click Apply, the dialog closes without change.

See also Grid/Units .


Align Ordinate

Aligns ordinate dimensions in a drawing.

To align ordinate dimensions:

1	Right-click a dimension value.

2	Select Align Ordinate from the menu.

The rest of the ordinate values in the set align to 0.0 ordinate dimension of the set.

See also Ordinate Dimension , Add to Ordinate Dimension


Aligned Section

Creates a section view through a model, or portion of a model, that is aligned with the selected section line.

To create an aligned section view:

1	Double-click the drawing view to activate it.

2	Click [image] or Tools, Sketch Entity, Line and draw the section line. The section line should be two connected lines at an angle to each other.

3	Click [image] and select the line to which you want to align the view.

4	Click [image] or Insert, Drawing View, Aligned Section. This converts the lines into a section line, with arrows indicating the direction of the view.

5	If necessary, double-click on the section line to reverse the direction of the section view.

You can edit section lines by dragging them to make them longer or shorter, and then clicking [image] or Edit, Rebuild.

To change the section line label or the direction of the view, right-mouse click the line and select Properties. Make your changes, then click Rebuild.

See Section Line Properties  for more information.

See also Crosshatch Options .


Annotations

Lets you select the types of annotations to use, and lets you turn the display of annotations, feature dimensions, and reference dimensions on or off.

To select the display of annotations and/or dimensions:

1	In the FeatureManager design tree, right-mouse click Annotations.

2	Select from the following:

•	Details - Opens the Annotations Properties dialog so you can specify the annotation types to display.

•	Display Annotations - A shortcut to turn annotation display on or off.

•	Show Feature Dimensions - A shortcut to turn feature dimension display on or off.

•	Show Reference Dimensions - A shortcut to turn reference dimension display on or off.


Annotation Properties

Lets you select the types of annotations that you want to display.

To select the types of annotations to display:

1	In the FeatureManager design tree, right-mouse click Annotations and select Details.

2	From the Annotation Properties dialog, select the annotation types to display:

Cosmetic Threads

Datums

Datum Targets

Feature Dimensions

Reference Dimensions

Geometric Tolerances

Notes

Surface Finish

Welds

- or -

Click Display All Types to show all kinds of annotations available for that part or view.

3	Change the values in the Text Scale edit box to change the scale of the text used in the annotation.

4	Select from the following options:

•	Always display text at the same size. When this is checked, all  annotations and dimensions are displayed at the same size regardless of zoom. Note that drawings have this option disabled and always zoom the text height.

•	Display items only in the view in which they are created.

•	Display Annotations / Display Assembly Annotations.

•	Display Annotations for all components. This option is available in an assembly only.

5	Click OK to accept your changes; click Cancel to exit the dialog without saving the changes.


Arc

See 3 Point Arc, Centerpoint Arc, Tangent Arc.


Arrange Icons

Lines up all minimized document icons in evenly spaced rows at the bottom of the SolidWorks window.

To arrange minimized document icons:

Click Window, Arrange Icons.


Assembly Feature

Creates a feature that exists only in the context of the assembly. You can either make an extruded cut, a revolve, or a simple hole.

To create an assembly feature:

1	Position all of the assembly components as desired.

2	Set the scope to the desired parts. (See Feature Scope.)

3	To make a cut feature, select a sketch plane, and sketch a profile of the new feature. (To make a revolve, you must sketch a profile and a centerline.)

4	Click Insert, Assembly Feature, Cut and select either Extrude or Revolve.

5	Click OK.

– or –

3	To make a simple hole, click where you want to create the hole.

4	Click Insert, Assembly Feature, Hole, Simple and specify the hole Diameter and Depth.

5	 Click OK.


Attach Dimensions

In an imported .DXF or DWG drawing, globally attaches dimensions to the nearest reasonable sketch entities.

To attach dimensions:

With an imported .DXF or DWG drawing active, click Tools, Dimensions, Attach Dimensions.


Automatic Relations

Specifies whether geometric relations are automatically created as you add sketch elements.

To turn automatic relation creation on or off:

Click Tools, Sketch Tools, Automatic Relations. A check mark next to the menu item means that relations will be created automatically as you sketch.

As you sketch, the cursor changes shape to show you which relations can be created: Horizontal, Vertical, Parallel, Perpendicular, Tangent, Midpoint, and Coincident.

See also Add Relations .


Automatic Solve

Specifies whether SolidWorks should automatically do the computation to solve the sketch geometry of your part as you create it.

To turn automatic computation on or off:

Click Tools, Sketch Tools, Automatic Solve. A check mark next to the menu item means that computations are solved automatically.

When you are in the process of changing many dimensions in an active sketch, you may want to turn off the Automatic Solve option temporarily.


Auxiliary

Creates an auxiliary view, unfolded from a drawing view along a selected edge.

To create an auxiliary view:

1	In a drawing view, select the edge that you want to use as the axis for unfolding the auxiliary view. (To unfold horizontal or vertical projections, use the Projection command.)

2	Click [image] or Insert, Drawing View, Auxiliary.


Axes

Toggles the display of user-defined axes on or off.

To turn axis display on or off:

Click View, Axes. A check mark next to the menu item means axes are visible (except for axes you have hidden individually).

To hide or show an individual axis:

1	Right-click on the axis or on its name in the FeatureManager design tree.

2	Click Hide or Show.

See also Temporary Axes .


Axis

Creates an axis in a part or assembly.

To create an axis:

1	Click [image] or Insert, Reference Geometry, Axis.

2	Select from the Options to make an axis box.

•	One Axis. Select View, Temporary Axes , and then select the axis.

•	Two Planes. Select View, Planes, and then select two construction planes (while holding the Ctrl key).

•	Two Points. Select two sketched points or two vertices.

•	One Line. Select one line.

•	One Surface. Select one cylindrical surface.

3	Verify that the items listed in the Valid Items for an Axis box correspond to your selection(s).

4	Click OK.

Note	Axis display must be turned on (see Axes) to see the new axis.


Balloon

Inserts balloons in drawing, assembly, or part documents. If you previously inserted a bill of materials in an assembly drawing, the balloons label the parts in the assembly and relate them to items on the bill of materials. The balloon leader attaches to the place where you click.

You can specify the default balloon style and size on Tools, Options, the Detailing tab.

To insert a balloon:

1	Click  [image] or Insert, Annotations, Balloon.

2	Click on a part in a drawing view.

A balloon that contains a number corresponding to the part number on the bill of material attaches to the part that you clicked.

3	To move the balloon or leader arrows, drag them with the Select tool.

To change the balloon or its contents:

1	Double-click on the balloon

– or –

right-mouse click the balloon and select Properties from the menu.

2	In the Balloon Note Text block, you may specify that the note text is an Item Number, a Quantity, or Custom text.

3	If you choose Custom text, you can do one of the following:

•	enter text in the text box,

•	click the Add Symbol button and select a symbol from the Symbol dialog,

•	click [image] and embed a hyperlink in the balloon. (A hyperlink is indicated when a cursor passing over the balloon dynamically changes to a hand.)

4	If you select a balloon style of Circular Split Line, you may choose different note text for the Upper and Lower balloon. (See the Balloon block at the bottom of the dialog box.)

5	Select from the following leader options:

•	Angle. Scroll to an angle for the leader display.

•	Leader. Options are Display with Leader and/or Display with Bent Leader. When you select these options, you may select the position of the leader anchor: Closest, Left, or Right.

•	Arrowhead Style. When you select Display with Leader, you may also select an arrowhead style from a pull-down list.

6	In the Balloon block, you can select a balloon Style from the pull-down list: Circular, Triangle, Hexagon, Box, Diamond, Circular Split Line, Pentagon, or None.

7	You can select a balloon Size of Tight Fit, expandable to tightly fit any custom text you type in, or of a size to accommodate from one to five characters.

8	In the Font block, you can deselect the Use Document’s Font checkbox if you want a font of a different style and size. Click the Font button and make your selections from the Choose Font dialog box.

9	Make the changes in the Note dialog and click OK.

See also Bill of Materials ,  and Insert Model Annotations .


Balloon Properties

Lets you set the default style and size of the balloons used in assembly, drawing, and part documents.

To set default balloon properties:

1	Click Tools, Options.

2	Click the Detailing tab.

3	Click the Balloons button in the Notes block.

In the Balloon Properties dialog, you can select properties for balloons used for Notes or balloons associated with a bill of materials, BOM Balloons.

4	From the Style pull-down list, select either: Circular, Triangle, Hexagon, Box, Diamond, Circular with Split Line, Pentagon, or None.

5	From the Size pull-down list, select a balloon size of Tight Fit, expandable to tightly fit any custom text you type in, or of a size to accommodate from one to five characters.

6	If you select the Circular with Split Line style for a BOM Balloon, you can select the type of text that goes into the Upper and Lower halves of the balloon. You may specify that the note text is either an Item Number, a Quantity, or Custom text.


Baseline Dimension

Creates baseline dimensions in a drawing.

To create a baseline dimension:

1	Click the Dimension tool [image],  then press the right mouse button and select Baseline.

- or -

Click Tools, Dimensions, Baseline.

2	Click the edge you want to use as a baseline.

3	Click each of the edges or vertices you want to dimension.

4	Click to place the dimensions.

Note	Baseline dimensions are reference dimensions. You cannot change their values or use them to drive the model.


Bill of Materials

Lets you insert a bill of materials into the drawing of an assembly.

Note	To insert a bill of materials in a drawing, you must have Microsoft Excel installed on your computer.

To insert a bill of materials:

1	With a drawing view selected, click Insert, Bill of Materials.

2	Specify the information to include in the bill of materials by clicking the radio button in front of one option:

•	Show parts only. Select this option to list only parts in the bill of materials.

•	Show top level subassemblies and parts only. Select this option to list top level assemblies and parts in the bill of materials.

3	Select from the following options:

•	Use Summary Info title as part number.  If you assigned a part identifier number in the title box of the Summary Info for the part, you can use that identifier in the bill of materials.

•	Add new item by extending top border of table.  New components are added at the top of the bill of materials instead of at the bottom.

A bill of materials is displayed that lists the parts in your assembly.

4	Insert any additional information or columns in the spreadsheet using the appropriate Excel commands and icons.  See Custom Columns in a Bill of Materials .

5	Click a corner of the spreadsheet to change its size.

6	Click anywhere outside the spreadsheet to close it.

7	Double-click on the spreadsheet to open it again for editing.

To move the bill of materials:

1	Click on the spreadsheet. Your cursor should change to its Move shape [image].

2	Hold the left mouse button and move the cursor to where you want to place the bill of materials.

3	Release the mouse button.

To update the bill of materials:

1	Click in the drawing view originally selected to create the bill of materials.

2	Click Insert, Bill of Materials.

The existing bill of materials updates to include any new components that you added to the assembly; components that you deleted are removed from the bill of materials.

Note:  To make sure that the Bill of Materials updates automatically whenever a change is made to the assembly, click Tools, Options, and select the Drawings tab.  Then select the Automatic update of BOM option and click OK.

See also Balloon and Custom Columns in a Bill of Materials .


Custom Columns in a Bill of Materials

You can add more information such as Material, Vendor Number, Cost, etc. to the open part or subassembly document by clicking File, Properties, and selecting the Custom tab. (See Summary Info - Custom  for information about specifying custom properties on the part or subassembly property sheet.)

Then, you can add columns for these properties to your bill of materials template found in \install_directory\lang\english\Bomtemp.xls. When the bill of materials is inserted into an assembly drawing, it will be automatically populated with the values for the properties you defined on the property sheet.

To add custom columns to the bill of materials:

1	Open the file \install_directory\lang\english\Bomtemp.xls (in Excel).

2	In the first empty cell in the first row (E1, if this is first time you have edited this file), enter the column heading that you want to use for the custom property you want to display in that column, and press Enter. (The column heading does not need to match the custom property name.)

3	Click the cell to select it, then click Insert, Name, Define and type in the name of the custom property that you want to appear in this column.  Click OK.

This name is listed in the Names in workbook list for the selected cell. This name must match the name of the custom property from the part or subassembly document.

4	Click Add, then click OK.

The bill of materials will now include the added column, with the values specified in the custom file properties of the parts or subassemblies included in the assembly document.


Boss/Base

Creates a feature that adds material by extruding a profile for a specified distance.

You can extrude in one or two directions and add a draft while extruding.

An extrusion extends the sketched profile as either a solid feature or a thin feature.

To create a boss:

1	Create a sketch and draw the profile you want to extrude, or select an existing sketch that contains a profile. The profile must be closed and cannot intersect itself.

2	Click [image] or Insert, Boss, Extrude (or Insert, Base, Extrude, if this is the first feature in the part).

3	Select the Type, and specify the Depth if necessary.

4	Click Reverse Direction, if necessary.

5	To add a Draft, select the Draft While Extruding box. Enter a draft Angle and check Draft Outward, if necessary.

6	To extrude the feature in both directions from the sketch plane, select Both Directions, then select Direction 2 from the Settings for: box, and repeat steps 3 through 5 for the other direction.

7	Set the Extrude As: box to Solid Feature or Thin Feature. (Click Thin Feature for more information.)

8	Click OK.

See also Revolved Boss/Base .


Cascade

Arranges all SolidWorks document windows so they overlap with all their title bars visible.

To cascade document windows:

Click Window, Cascade.


Cavity

Within an assembly, creates a mold cavity in a part.

To create a mold cavity:

1	Create and save a part in which to insert a cavity. This is the mold.

2	Create and save a part to shape the cavity.

3	Open a new assembly.

4	Insert both parts into the assembly as assembly components.

5	Save the assembly.

6	Select the shape part, and use mating conditions to position the shape part over the mold part where you want to locate the cavity.

7	Right mouse click on the larger (mold) part, and select Edit Part from the menu.

8	Select the shape part in the FeatureManager design tree and click Insert, Features, Cavity.

The Design Component box displays the name(s) of the cavity shape component(s).

9	Select the Scaling Type:

•	About Component Centroids -- scales each part added to the cavity about its own centroid.

•	About Component Origins -- scales each part added to the cavity about its own origin.

•	About Mold Base Origin -- scales each part added to the cavity about the origin of the mold base part.

10	Adjust the Scaling Factor as appropriate for your casting material. The scaling factor is expressed as a percent (+/- 20%) of the size of the cavity part.

Note	The formula used to determine the size of the cavity is:

cavitysize = partsize * (1 + scalingfactor)

11	Click OK.

The mold part now has a cavity within.

Note	Multiple shape components may be inserted in the mold to create several cavities in a single part.


Centerline

Creates a centerline. Centerlines are used to create symmetrical sketch elements (see Mirror Sketch Elements) and revolved features (see Revolve), or as construction geometry.

To create a centerline:

1	Click [image] or Tools, Sketch Entity, Centerline.

2	Point where you want the line to start.

3	Press the mouse button and drag to where you want the line to end.

4	Release the mouse button.


Center Mark

Creates axis lines for showing center marks on circles that can be used as a reference points for dimensioning in a drawing. You can also use center marks on sketch geometry in a drawing.

To create a center mark:

Click [image] or Insert, Annotations, Center Mark, and click the circle.

To change the display attributes of individual center marks:

1	Right-mouse click the center mark and select Properties.

2	Click to uncheck Use document’s defaults.

You can set the default size of center marks and choose whether or not to display extended axis lines.

3	Make the changes that you want and click OK to accept the changes; click Cancel to close the dialog box without saving any changes.

To set your default preferences for center marks, click Tools, Options and select the Detailing tab.


Centerpoint Ellipse

Creates an ellipse from a centerpoint, start point, and end point.

To create a centerpoint ellipse:

1	Click Tools, Sketch Entity, Centerpoint Ellipse.

2	Point where you want to place the center of the ellipse.

3	Press the mouse button, drag and release to define one axis of the ellipse.

4	Press the mouse button and drag to define the second axis.

5	Release the mouse button. The circumference guideline remains.

6	Press the mouse button and drag to set the length and direction of the ellipse.

7	Release the mouse button.

See also Ellipse .


Centerpoint Arc

Creates an arc from a centerpoint, start point, and end point.

To create a centerpoint arc:

1	Click [image] or Tools, Sketch Entity, Centerpoint Arc.

2	Point where you want to place the center of the arc.

3	Press the mouse button and drag to where you want to place the start point of the arc.

4	Release the mouse button. The circumference guideline remains.

5	Press the mouse button and drag to set the length and direction of the arc.

6	Release the mouse button.

See Also Tangent Arc, Three-Point Arc


Chamfer Feature

Creates a beveled edge feature on selected edges.

To create a chamfer feature:

1	Click [image] or Insert, Features, Chamfer.

2	In the Chamfer Feature dialog box, click in the Items To Chamfer window.

3	On the model, select the edges, faces, or loops to chamfer. (You can also do this as the first step.)

4	Examine the Items to Chamfer list to make certain that you have selected the entities that you intended.

5	Set the chamfer Distance and the chamfer Angle.

An arrow appears that points in the direction in which the distance is measured.

6	If necessary, select Flip Direction.

7	Click OK.


Change Parameter Value

To change a parameter:

1	Enter a value for the parameter in the New Value edit box.

2	Click OK to accept the changed value and click Rebuild.

- or -

Click Cancel to close the dialog and not save any changes.


Drawing View Properties

Provides information about the drawing view and the model or assembly that it is from. The Drawing View Properties dialog also lets you specify the view’s scale,  dimension type, and configuration.

To access the Drawing View Properties dialog:

Right-mouse click in a drawing view and select Properties from the menu.

To change the scale of a drawing view:

1	Click the Use sheet’s scale box to remove the check mark.

2	Change the scale ratio value in the Scale boxes. (The default scale ratio is 1:2.)

3	Click OK.

To specify a different view orientation for a Named View:

Under Model Information, select a standard or user-defined view from the Named View list.

Note:	The entire part or assembly is displayed at the scale of the selected view, even if the selected view orientation in the part or assembly displays a zoomed-in view.

To specify the configuration to use:

From Configuration Information, select one of the following:

•	Use model’s “in-use” or last saved configuration.

- or -

•	Use named configuration.  If you want to use a configuration that you previously created and named, select the configuration from the pull-down list.

Select Show in exploded state to use an exploded view.

To specify the dimension type:

From Type of Dimensions Created in This View,  select either Projected or True (Isometric).

To align a broken view with the broken view that it was derived from:

Click Align breaks with parent if you want to the break gap in both views to be aligned. (Click Edit, Rebuild, if necessary.)


Check Entity

Lets you do a complete geometry check of an active model, including invalid edges, and faces, or short edges.

To check a model for correct geometry:

1	With a part document active, click Tools, Check.

2	In the dialog box, select the entity type that you want to verify. Click either Check body, Check feature, or Check selected item.

3	If you clicked Check selected item, select a face on the part.

4	Select the problem(s) that you want to check for: Invalid face(s), Invalid edge(s), and/or Short edge(s).

5	If you clicked Short edge(s), you can specify an edge length in the scroll box.

6	Click Highlight all results to display the errors with highlighting.

7	Click OK.

The dialog box does not close when you click OK, so you can check additional entities.

The Item to check box displays the item that you selected.

The What’s wrong list displays the items that are either invalid or too short.

Messages provide a description of the results, and the graphics area displays the invalid items with arrows and highlighting (if you specified Highlight all results).

8	Click Cancel to close the dialog.


Choose Font

Lets you specify the font style and size to use.

To specify the default font for all new parts, assemblies, or drawings:

1	Click Tools, Options.

2	Select the Detailing tab.

3	Click Note Font to specify the font used for notes in drawings.

4	Click Dim Font to specify the font used for dimensions.

5	Make selections from the following options, and click OK.

•	Font.  Use the scroll arrows to select from a variety of type faces available on your system.

•	Font Style.  Use the scroll arrows to select from Regular, Italic, Bold, or Bold Italic font styles.

•	Height.  Set the font measurement system to either Units or Points.
If Units is selected, the value is interpreted as the actual height of the tallest character in the font set. Select the Units value box and enter a new value.
If Points is selected, the font height includes ascenders and descenders, so the character size is actually smaller than the corresponding character when measured in Units. Use the arrows to scroll to the point size you want to use.

•	Effects.  Select Strikeout, Underlining or both, if desired.

•	Sample. The Sample box displays your font selections.


Component Line Font

Lets you change the line font style of edges on each of the components in an assembly drawing.

To change the font style of component edges:

1	Right-mouse click a component in a drawing view and select Component Properties.

2	Select from the Type of Edge list box.

3	Select a line style and weight from the Line Style and Line Weight scroll boxes.

The line you selected is displayed in the Preview box.

4	Click OK to use the line font in the component you selected.


Circle

Creates a circle.

To create a circle:

1	Click [image] or Tools, Sketch Entity, Circle.

2	Point where you want to place the center of the circle.

3	Press the mouse button and drag to set the radius.

4	Release the mouse button.


Circular Pattern

Creates multiple instances of a feature spaced uniformly around an axis.

If you modify the original feature, all instances in the pattern are updated to reflect the change.

To create a circular pattern:

1	Create a feature that you want to replicate.

2	Create an axis around which to pattern the feature.

For information about how to create an axis, see Reference Axis .

3	Select the axis, and Ctrl-select the feature(s) to pattern.

4	Click Insert, Pattern/Mirror, Circular Pattern.

5	Specify the Spacing and the Total Instances of the feature.

6	Click Vary Sketch if you want the pattern to change as it is repeated. See Vary Sketch for more information.

7	Click OK.

To delete pattern instances, see Pattern Deletion .

See also Linear Pattern .


Vary Sketch

Use the Vary Sketch option if you want the pattern to change its dimensions as it is repeated. For example, you may want to maintain a specific distance between the edges of the base part and the patterned features.

In this example, the first feature (the hole feature) is patterned three times.

•	When Vary Sketch is not checked, the pattern remains the same regardless of the defining geometry.

•	When Vary Sketch is checked, the pattern maintains its relation to the sloping edge, based on the dimensions and constraints of the first instance of the pattern.

To create a variable pattern:

1	Create a sketch for the first feature in the pattern, observing the following recommendations:

•	The feature sketch must be constrained to the boundary that defines the variation of the pattern instances. For example, in the illustrated pattern, the angled top edge of the first feature is parallel and dimensioned to the angled edge on the base part.

•	The feature sketch should be fully defined.

2	Double-click one of the feature dimensions and click the spinbox arrow to change the dimension.

This gives you a preview of the way this dimension will drive the feature when you create the pattern. Try a different dimension for a different result.

3	When you are satisfied that the dimensions are correct and the pattern will repeat as you wish, click Insert, Cut, Extrude (or Insert, Boss, Extrude) to create the first feature.

4	In the FeatureManager design tree, select the feature to repeat.

5	Click Insert, Pattern/Mirror, Linear Pattern (or Circular Pattern).

6	Click the dimension that you want to use to drive the pattern. Notice the preview arrow.

7	Click Reverse Direction if the arrow points in the wrong direction.

8	Click the Vary Sketch checkbox.

9	Specify the values for the Spacing and Total Instances of the pattern.

10	Click OK to create the pattern.


Close

Closes the currently active document.

To close a document:

Click File, Close. If there are unsaved changes in the document, you will be asked if you want to save them.

If other documents are open that are dependent on the current document, you will be asked if you want to save them as well.


Close All

Closes all open documents. If a new or changed document has not been saved, the program asks you to confirm whether you want to save the document or rebuild the part.

To close all documents:

1	Click Window, Close All.

2	Respond to confirmation requests from the program to save or not save documents when they are closed.


Close Sketch to Model

Closes a sketch with an open profile, using existing model edges.

To use an open profile sketch to extrude using existing model edges:

1	Open a sketch on a model face.

2	Sketch an open profile with endpoints that are coincident with model edges on the same face boundary.

3	Click Tools, Sketch Tools, Close Sketch to Model.

The Close Sketch with Model Edges dialog appears.

Notice that an arrow points in the direction in which the sketch will close. (The extruded boss will either be within the sketch lines or outside of the sketch lines, as shown in the illustration.)

4	Click Reverse direction to close sketch, if necessary.

5	Click Yes when the arrow points in the correct direction; click No to exit the dialog.

6	Click Insert, Boss, Extrude (or Insert, Cut, Extrude) and specify the End Conditions in the Extrude Feature dialog box.

7	Click OK to make the extrusion.


Color Options

  To specify the color display of view modes .

  To specify the color display of lines, borders, text, and so on .

  To specify the color display of features .


Color -- Lines, Text, and Borders

To set the colors used to display lines, text, borders, and so on:

1	Click Tools, Options and click the Color tab.

2	Click the View System Defaults checkbox.

3	In the System region, scroll the list to select the line type, border style, dimension text, an so on for which you want to edit the color representation.

4	Click Edit to change the color used to display the selected line or item.

5	Select a color from the color palette or define a custom color. Click OK.

6	To restore the original default color settings, click Reset All.

7	Select the scope of the application in the Apply To: box.

•	Active Document - the document that you are currently working on

•	System Defaults - all new documents that are created

•	All Possible - the current document as well as all new documents

8	Click OK to accept the changes; click Cancel to discard the changes and exit the dialog box; click Reset All to return to the installed system defaults.


Color -- View Mode

To set the colors used to display model lines and shaded surfaces in view modes:

1	Click Tools, Options and click the Color tab.

2	In the System region, select the view mode for which you want to edit the color representation: Wireframe/HLR, Shaded, or Hidden.

– or –

Click the Apply same color to Wireframe/HLR and Shaded box if you want to use the same color for those view modes.

3	Click Edit to change the color used to display the selected view mode.

4	Select a color from the color palette or define a custom color. Click OK.

5	To restore the original default color settings, click Reset All.

When you edit the color of the Shaded mode, you can click Advanced and use the slider controls to change the lighting condition values:

6	Select the scope of the application in the Apply To: box.

•	Active Document - the document that you are currently working on

•	System Defaults - all new documents that are created

•	All Possible - the current document as well as all new documents

7	Click OK to accept the changes; click Cancel to discard the changes and exit the dialog box; click Reset All to return to the installed system defaults.


Color -- Features

To set the colors used to display features:

1	Click Tools, Options, and click the Color tab.

2	In the Features region, click the feature type for which you want to edit the color representation.

3	Click Edit and select a color from the color palette or define a custom color. Click OK and view the selection in the preview box.

4	To restore the original default color settings, click Reset Feature.

5	To specify that feature colors are not used, click Ignore Feature Colors.

6	Select the scope of the application in the Apply To: box.

•	Active Document - the document that you are currently working on

•	System Defaults - all new documents that are created

•	All Possible - the current document as well as all new documents

7	Click OK to accept the changes; click Cancel to discard the changes and exit the dialog box; click Reset All to return to the installed system defaults.

To change the color of individual part faces, see Entity Property .


Material Properties

Use the slider controls to change the display properties.  Experiment until you produce the results that you prefer.

Ambient - light reflected and scattered by other objects

Diffuse - light scattered equally in all directions on the surface

Specularity - ability to reflect light from a surface

Shininess - a glossy, highly reflective surface

Transparency -  ability to pass light through the surface

Emission - ability to project light from the surface

See also, Color -- View Mode.


Common Properties

Construction Geometries. Check the box to convert two or more sketched entities to construction geometries.


Component

Adds a component to an assembly.

To add a component:

1	With an assembly open, click Insert, Component, From File.

The Open dialog box appears.

2	Browse to the directory that contains the component you want to insert into the assembly.

3	Click Open. The cursor changes to a cross [image].

4	Click in the assembly window where you want to locate the component.

To create a new component within the context of the assembly, see New Component .

See also Move Component  and Rotate Component .


Component Properties

Lets you view or change the configuration properties of a component.

To view or change component properties:

1	Right-click the component name in the FeatureManager design tree.

2	Select Component Properties from the menu.

•	Component Name. The part name is displayed, but usually is read-only. (If you want to change a component name, you must deselect the option Update component names when documents are replaced in the Tools, Options, External References dialog. See External References .)

•	Model Document Path. The path to the part file is displayed. You can click the Browse button to search for a different part to replace the current one.

•	Instance ID. The instance is 1 for the first time the part is used in the assembly; if it is used more than once, each occurrence of the part is assigned a consecutive instance identification number.

3	Select Configuration specific properties:

If the selected component is part of a subassembly, choose which set of configuration properties to use from the following:

•	Use properties specified in configuration <configuration name> of <subassembly name>  --  The Visibility options specified for the configuration of the subassembly are used. (The options in the Visibility section of this dialog box are not available.)

•	Override properties specified in configuration <configuration name> of <subassembly name>  --  The Visibility options listed below in the Visibility section of this dialog are used.

Visibility

•	Suppress.  When this is checked, the component is suppressed and it is not an active part of the assembly. When you rebuild the assembly, this component is not used in the regeneration.

•	Show Feature Detail in FeatureManager Design Tree.  When the component is suppressed, the component’s icon in the FeatureManager design tree is displayed in gray, but the icon and the component’s name remain visible.

•	Show Model.  When this is not checked, the component is hidden. This affects the display of the component only; when you rebuild the assembly, this component still is used in the regeneration.

•	Color.  Click this button to select a color for this instance of the assembly from the Assembly Instance Color dialog box.

4	Referenced configuration. Select one of the following:

•	Use component’s “in-use” or last saved configuration.

- or -

•	Use named configuration.  If you want to use a configuration that you previously created and named, select the configuration from the pull-down list.

5	Click OK when you finish making your changes.


Assembly Instance Color

Lets you select a color for the assembly when it is in shaded mode.

Click Use Component to use the selected component’s default color.

Click Use Assembly to use the assembly’s default color.

Click Change Color to select a color from the color palette or define a custom color.

Click Advanced to set lighting display characteristics, such as transparency, shininess, etc.


Component Pattern

Lets you place a pattern of components in an assembly in one of these two ways:

 Based on a feature pattern of one of the components.

 Defined locally within in the assembly


Component Pattern - Derived

Creates a component pattern based on a feature pattern of an existing component.

To derive a component pattern from an existing feature pattern:

1	Insert into your assembly a component that has a pattern feature, and a seed component that you can mate with the pattern of the other part.

2	Mate the seed component to the original feature in the pattern.

3	Click Insert, Component Pattern.

4	In the Pattern Type dialog, click Use an existing feature pattern and click Next.

The Derived Component Pattern dialog box appears.

5	Select the seed component in the FeatureManager design tree or the graphics area.

6	Click the Pattern Feature box, then click the pattern feature in the FeatureManager design tree.

7	Click Finish.


Component Pattern - Local

Lets you define a component pattern in an assembly in much the same way as you define a feature pattern in a part.

To define a local pattern for components in an assembly:

1	Insert and mate components in an assembly.

2	Click Insert, Component Pattern.

3	In the Pattern Type dialog, click Define your own pattern, and select either Linear or Circular.

4	Click Next.

The Local Component Pattern dialog box appears.

5	Select the seed component in the FeatureManager design tree or the graphics area.

6	Click the Along Edge/Dim box, click a model edge, axis, or dimension to indicate the pattern direction, and click Reverse Direction if necessary.

7	Specify the Spacing and Instances.

8	If you are creating a linear pattern in two directions, select Second Direction, and repeat Steps 5 and 6.

9	Click OK.

See also Linear Pattern and Circular Pattern.


Pattern Type

1	Click either:

•	Use an existing feature pattern (Derived) if you want to create a component pattern based on a feature pattern of one of the components.

•	Define your own pattern (Local) if you want to specify a component pattern within the assembly. If you choose to create a local pattern, select either Linear or Circular.

2	Click Next.

See also Component Pattern .


Derived Component Pattern

1	Click the seed component in the FeatureManager design tree or the graphics area.

2	Click the Pattern Feature box and then select the pattern feature in the FeatureManager design tree.

3	Click Finish.


Local Component Pattern

1	Click the seed component in the FeatureManager design tree or the graphics area.

2	Click the Along Edge/Dim box, click a model edge, axis, or dimension to indicate the pattern direction, and click Reverse Direction if necessary.

3	Specify the Spacing and Instances.

4	If you are creating a linear pattern in two directions, select Second Direction, and repeat Steps 2 and 3.

5	Click OK.

See also Linear Pattern and Circular Pattern.


Configure Document

To open a configuration of a part:

1	Click File, Open.

2	Select a part file, click the Configure check box, and click Open.

3	In the Configure Document dialog box, click Use Named Configuration and select the desired configuration.

4	Click OK.

The part opens in the selected configuration.

To open a configuration of an assembly:

1	Click File, Open.

2	Select an assembly, click the Configure check box, and click Open.

3	In the Configure Document dialog box, click Use Named Configuration and select the desired configuration.

4	To use the simplified version of the parts, check the Use specified configuration name for all part references when available check box, and enter a part configuration name.

5	Click OK.

The assembly opens in the selected configuration.

To open only the structure of an assembly:

1	Click File, Open.

2	Select an assembly, click the Configure check box, and click Open.

3	In the Configure Document dialog box, select New configuration showing assembly structure only and enter a name.

4	Click OK.

The FeatureManager design tree for the assembly appears.

See also Configuration .


Configuration

Lets you hide or suppress some features or components on a part or assembly and then name and save that configuration.

This is useful when you have a very complex part or assembly that you want to work with, but you do not want to view all its parts or features while you are working. Also, a part or assembly may rebuild more rapidly with some features suppressed, so it is efficient to suppress them temporarily.

To create and name a configuration:

1	Click the Configuration icon at the lower left of the window to change to the Configuration Manager view.

2	In the Configuration Manager tree, right-mouse click the assembly name, or part name, and select Add Configuration. The Add Configuration dialog box appears.

3	Enter a Configuration Name, and add Comments if desired.

4	Select Properties for newly inserted items as desired.

For an assembly document, select from the following properties:

•	Click Suppress part components or Hide component models if you want newly added parts to be added in the suppressed or hidden state.

•	Click Show sub-assembly component structure without features to simplify the detail for all added sub-assemblies in the FeatureManager design tree.

For a part document, check or uncheck the following property:

•	Suppress Features. When checked, new features added to the part are automatically suppressed for this configuration.

5	Select the way properties are applied (only for assemblies):

•	Click Apply properties to sub-assembly root only to apply the properties selected in Step 4 to only the top subassembly components. All subassembly child components will inherit the properties specified in the configuration of the subassembly.

•	Click Apply properties to ALL sub-assembly components to apply the properties selected in Step 4 to all added components. (If you want all components of newly added subassemblies to be suppressed, regardless of the properties specified in the subassembly configuration, choose this option.)

6	Click the Advanced button to specify how the assembly or part is referenced in a Bill of Materials.

7	Click OK.

The new configuration name appears in the tree.

8	Return to the FeatureManager design tree view, by clicking the FeatureManager icon.

9	Suppress and/or hide components for the desired configuration.

The new named configuration is created. You can create multiple configurations and recall any one from the configuration list.


Viewing an Assembly or Part Configuration

You can have several configurations of an assembly or part, and you can quickly switch between them using one of the following two methods:

To use Show Configuration:

1	Click the Configuration icon [image] to change to the Configuration Manager.

2	Right-mouse click the name of the configuration you want to view and select Show Configuration.

The named configuration becomes the active configuration, and the display updates to reflect any differences in hidden or suppressed items.

To double-click to display a configuration :

1	Click the Configuration icon [image] to change to the Configuration Manager.

2	Double-click the name of the configuration you want to view.

In case the double-click was a mistake, and because some complex configurations take a long time to display, a dialog box appears that gives you the option of canceling the display.

3	If you do not want the Confirm Show Configuration dialog box to display again during this session, click the checkbox next to Don’t ask for confirmation again during this session.

4	In the Confirm Show Configuration dialog box, click OK to see the configuration or click Cancel to abort the display.

The named configuration becomes the active configuration.


Edit Configuration Properties

You can change the properties of an assembly or part configuration.

To edit the configuration properties:

1	Right-click the configuration name, and select Properties. The Configuration Properties dialog box appears.

2	Edit the name, comments, and/or properties as desired.

3	Click OK.

To change only the name of the configuration, click-pause-click the name in the Configuration Manager tree, type the new name, and press Enter.


Edit Assembly or Part Configuration

You can edit an assembly or part configuration.

To edit an assembly or part configuration:

1	View the desired configuration.

2	Change to the FeatureManager view, and change the suppression property and/or visibility as needed.


Delete Assembly or Part Configuration

You can delete an assembly configuration or a part configuration.

To delete a configuration:

1	In the Configuration Manager, click the name of the configuration you want to delete.

2	Press the Delete key (or click Edit, Delete), and click Yes to confirm.

Note:	You cannot delete the active configuration. Deleting a configuration does not delete any feature or part.


Add Configurations
Add Configuration

1	Enter a name for the configuration in the Configuration Name box.

2	Enter a Comment that describes the configuration. (Optional)

3	Select Properties for newly inserted items as desired.

If you have an assembly, select from the following properties:

•	Suppress part components. When checked, all parts you add to the assembly will be in the suppressed state.

•	Hide component models. When checked, all components that you add to the assembly will be added in the hidden state.

•	Show sub-assembly component structure without features. When checked, any subassembly you add to the assembly will display only its icon in the FeatureManager design tree.

If you have a part, check or uncheck the following property:

•	Suppress Features. When checked, new features added to the part are automatically suppressed for this configuration.

4	Select the way properties are applied (only for assemblies):

•	Apply properties to sub-assembly root only. When selected, the properties chosen above apply to the sub-assembly root only.

•	Apply properties to ALL sub-assembly components. When selected, the properties chosen above apply to all components in the sub-assembly. (Use this option when you want to hide or suppress most of the components in a large assembly. You can then individually select the components that you want unsuppressed or visible.)

5	Click the Advanced button to specify how the assembly or part is referenced in a Bill of Materials.

6	Click OK.

 The new configuration name appears in the tree.

7	Return to the FeatureManager design tree view, by clicking the FeatureManager icon.

8	Suppress and/or hide components for the desired configuration.

The new named configuration is created. You can create multiple configurations and recall any one from the configuration list.


Advanced Configuration Properties

You can specify how a part or assembly is referenced when it is used in a Bill of Materials.

1	Under Part No. displayed when used in a Bill of Materials select one of the following:

•	Use the document name.  Specifies that the SolidWorks part or assembly name is used.

•	Use name below. When selected, an edit box opens in which you can enter a part name or number.

2	If an assembly is active, you can select:

Don’t show child components in BOM when used as sub-assembly. When checked,  specifies that the sub-assembly itself shows in the Bill of Materials.  When not checked, the child components are listed in the Bill of Materials.

3	Click OK.


Constrain All

Sets constraints on the sketch entities of an unconstrained imported .DXF or .DWG drawing.

To solve relations in an imported drawing:

1	Import a sketch from a .DXF or .DWG drawing.

2	Click Tools, Relations, Constrain All.

The command tries to solve all the apparent relations in the sketch and reports the number of constraints that were added to the sketch.


Construction Geometry

Converts sketched curves on a sketch or drawing to construction geometry.

To convert lines, arcs, or circles in a drawing to construction geometry:

1	Select a sketched line, arc, ellipse, spline or circle in a drawing.

2	Click Tools, Sketch Entity, Construction Geometry.

To convert lines, arcs, circles, ellipses or splines in a sketch or drawing to construction geometry:

1	Right-click a sketched line, arc, ellipse, spline, or circle in a sketch or drawing.

2	Select Properties, and click the Construction <entity name> checkbox in the Properties dialog box.

3	Click OK.


Convert Entities

Creates one or more sketch entities in a sketch by projecting an edge, loop, face, external sketch curve, or external sketch contour, set of edges, or set of external sketch curves onto the sketch plane.

To convert an entity:

1	With a sketch active, click on an edge, loop, external sketch curve, or other entity.

2	Click [image] or Tools, Sketch Tools, Convert Entities.

An On Edge relation is created between the new sketch curve and the entity, so the curve will be updated if the entity changes.


Copy

Copies the selected item(s) to the Windows Clipboard.

To copy:

1	Select the item(s) to copy.

2	Click [image], or Edit, Copy, or press Ctrl-C.


Move and Copy Features

You can move or copy features by dragging them in the model.

To move a feature to a new place on a model:

For example, to move a hole feature to a different face on the model, point at the hole and hold the left mouse button. Drag the feature to a different face and release the mouse button to drop the hole feature.

To create a copy of the feature:

To copy a hole feature to a different face on the model, point at the hole and hold the left mouse button. Hold down the Ctrl key while you drag the feature.


Cosmetic Threads

Represents threads on a part, assembly, or drawing.

To insert cosmetic threads on a part or drawing:

1	On a cylindrical part, click a circular edge where the thread should begin.

2	Click a circular edge and click Insert, Annotations, Cosmetic Thread.

3	In the Cosmetic Thread dialog box, select the thread to apply:

•	Select Blind to run the thread for a specified distance, and enter the distance in the value box.

•	Select Up to Next to run the thread to the next face.

4	Enter a value in the Minor Diameter/Major Diameter box.

5	In the Thread Callout box, enter thread callout text, if desired.

6	Click OK to create the thread; click Cancel to exit.


Cosmetic Thread

1	In the Apply Thread box, select the thread type:

•	Select Blind to run the thread for a specified distance, and enter the distance in the value box.

•	Select Up to Next to run the thread to the next face.

2	Enter a value in the Minor Diameter/Major Diameter box.

3	In the Thread Callout box, enter thread callout text, if desired.

4	Click OK to create the thread; click Cancel to exit.


Create File

1	To change the directory path, click Browse, navigate to a new directory, and click Save.

2	Click OK to accept the directory path, or Cancel to abandon the operation.


Crosshatch Options

Specifies a crosshatch pattern to be used on the solid interior of section views, and displays a preview of the pattern selection.

To specify a default crosshatch pattern:

1	Click Tools, Options.

2	Click the Crosshatch tab.

3	Select a crosshatch pattern from the Pattern list.

4	If necessary, set the Angle and Scale of the crosshatch pattern.

A preview of the pattern is displayed in the Type box.

5	Select the scope of the application in the Apply To: box.

•	Active Document -- the document that you are currently working on

•	System Defaults -- all new documents that are created

•	All Possible -- the current document as well as all future documents

6	Click OK to accept the changes; click Cancel to discard the changes and exit the dialog; click Reset All to return to the system defaults at installation.


Curvature

Causes surfaces to be rendered in different colors according to their local radius of curvature.

To render curved surfaces in colors:

Click View, Display, Curvature.

The curvature of the model is displayed in color as long as the menu item remains checked.

To remove the color, click View, Display, Curvature again.


Custom Header and Footer

Creates a custom header or footer for every document page that you send to the printer.

To create a page header or footer:

1	Place the insertion point in an edit box: Left Section, Center Section, or Right Section.

2	Click the appropriate button to insert the information that you want to appear in that section.

3	If appropriate, enter spaces or text between the selections.  For example, “Page &[pagenum] of &[pages]”  would print as  “Page 1 of 7” on the first page of a seven-sheet drawing.

4	Click the Font button to choose from a variety of font styles and sizes.

5	Click OK and view the result in the Header Preview and Footer Preview boxes.

6	Click Apply to accept the change. You can continue to make changes and then click OK to close the dialog.

or

Click OK to accept the change and close the dialog.

	Page number
	Total number of pages in the document
	Date of the print
	Time of the print
	Name of the file


Customize Toolbars

Customizes the toolbars to suite your style of working.

You can,

•	rearrange the buttons on toolbars,

•	move buttons from one toolbar to another,

•	duplicate buttons and place them on more than one toolbar,

•	delete buttons that you never use.

To customize your toolbars:

1	Click Tools, Customize.

2	Click the Toolbars tab for the options you can customize.

3	Make your changes and click OK.

Note:	The Web toolbar is not customizable.

Customization options:

Categories. Scroll through the list of toolbars to locate the button(s) you want to move.

Buttons. Click and drag a button from the dialog box to a new location on a toolbar, or to a different toolbar.

To delete a button from a toolbar, click and drag the button from the toolbar to the dialog box, then release the mouse button.

Description. Click a button to see the description of the button’s purpose.


Customize Drawing Template

Customizes drawing templates.

To edit the drawing template:

1	Right mouse click anyplace on the drawing sheet and select Edit Template from the menu.

2	Double-click on the text that you want to replace.

3	Enter new text in the Note dialog box.

4	Click Font to select a new font style or size, if necessary.

5	Click OK to accept the new font and new text.

Additionally, you can edit the template format by moving, deleting, and adding lines or text in the text blocks.

•	To delete, click the line or text and press the Delete key.

•	To move, click the line or text and drag to a new location.

•	To add lines, click the Tools, Sketch Entity, Line or [image].

•	To add text, click Insert, Annotations, Note or [image]. Complete steps 3, 4, and 5, and then drag the text to the correct location.

To save the template:

1	Click File, Save Template.

2	  If you want to overwrite the standard template, click OK and confirm.

- or -

If you want to save the template to a new name, click Custom Template, and Browse to a location, and enter the new  template name.  (Template files have the .drt extension.)

3	Click Save.

To end editing the template and return to working with an individual sheet, click the right mouse button and select Edit Sheet.


Customize Menus

Customizes the SolidWorks menus to suite your style of working.

To customize your menus:

1	Click Tools, Customize.

2	Click the Menus tab.

3	Click the appropriate buttons to Rename a menu item, Remove or Add a menu item, or Reset All menus to their original state.

4	Make your changes and click OK.

Customization options:

Categories. Displays the list of available menus. Select the menu that you want to change.

Commands. Displays the list of available commands on the selected menu. Select the command that you want to rename, relocate, or remove.

Change What Menu. Displays the code name of the menu that is selected.

Position on Menu. Lets you select a position from Auto, At Top, At Bottom, or Add Below one of the listed commands.

Name of Command. Displays the code name of the command that is selected.

Description. Displays the description of the selected command.


Customize Keyboard

Customizes your keyboard to suite your style of working with SolidWorks.

To customize your keyboard:

1	Click Tools, Customize.

2	Click the Keyboard tab.

3	Click the appropriate buttons to Assign a new shortcut key, Remove a shortcut key, or Reset All shortcut keys to their original state.

4	Make your changes and click OK.

Customization Options:

Categories. Displays the list of available menus. Select the menu that contains the command you want.

Commands. Displays the list of available commands. Select the command for which you want to assign or remove a shortcut key.

Press New Shortcut Key. Enter the new key or key combination.

Current Key. Displays the current shortcut key for the selected command.

Description. Displays the command description for the selected command.


Cut

Removes the selected items and places them on the Windows Clipboard.

To cut:

1	Select the item(s) to cut.

2	Click [image], or Edit, Cut, or press Ctrl-X.


Cut Extrude

Creates a feature that removes material by extruding a profile for a specified distance.

To create a solid or thin feature cut:

1	Create a sketch and draw the profile you want to extrude, or select an existing sketch that contains a profile. The profile does not have to be closed.

2	Click [image] or Insert, Cut, Extrude.

3	Select the Type.

4	Specify the Depth.

5	Click Reverse Direction, if necessary.

6	Select Flip Side to Cut if you want to remove the material outside of the profile.

7	To add a Draft angle, check the Draft While Extruding box. Enter a draft Angle and check Draft Outward, if desired.

8	If the Type you selected relies on the selection of a surface or vertex, select that item now in the graphics area.  The selection displays in the Selected Items list.

9	To extrude the feature in two directions from the sketch plane, select Both Directions, and specify settings for Direction 2 from the Settings for: box. Repeat steps 3 through 8 for the other end.

10	Specify Solid Feature or Thin Feature in the Extrude as: box.

If you are extruding the cut as a solid feature, skip ahead to Step 12. If you are extruding the cut as a thin feature, proceed to Step 11.

11	Select the Thin Feature tab at the top of the dialog box, and

•	Select a Type.

•	Specify a Wall Thickness.

•	To extrude in the opposite direction, click Reverse.

12	Click OK.

See also Loft Feature , Revolved Cut , Sweep Feature


Dangling Detail Items

Lists dangling detail items by type.

The values in the Count column indicate the number of dangling annotations of each type. You can either delete the dangling items, or leave them in the drawing to re-attach later.

To delete the dangling items:

1	Click the box in the Delete column corresponding to the annotation type you want to delete.

2	Click OK.


Datum Feature Symbol

Attaches a datum feature symbol to a selected location on a part, assembly, or drawing document.

To insert a datum feature symbol:

1	With a drawing active, click  [image] or Insert, Annotations, Datum Feature Symbol.

2	Click the surface on which you want to place a datum feature symbol.

You can place several datum feature symbols; the datum letters are assigned alphabetically (omitting I, O, Q, S, X, and Y to comply with ANSI standards).

3	To stop placing datum feature symbols, click  [image] or Insert, Annotations, Datum Feature Symbol again.

To edit the datum feature symbol, right-click the symbol and select Properties from the menu.


Datum Target Point

Locates target points on the model surface in a drawing.

To place target points on a drawing view:

1	Activate the drawing view.

2	Click [image] or Insert, Annotations, Datum Target Point.

3	Point and click the mouse where you want to place a target point.

Notice that an inferencing line is available to assist you in placing the target points in relation to each other.

You can also apply constraints (Add Relations) to the datum target point, as you can with a sketch point.

4	Click [image] again to end making target points.


Datum Target Symbol

Creates and places datum target symbols on a part or assembly document, or a drawing view.

To create a datum target symbol:

1	Click a model edge or a datum target point in a part or assembly or a drawing view.

2	Click [image] or Insert, Annotations, Datum Target Symbol.

The Datum Target Symbol dialog appears.

3	Enter a value for the Target area size box; click [image] if the value describes a diameter.

4	Click the Display target area size outside check box if you want to place the value outside the target symbol circle.

5	Enter up to three Datum Reference labels in the boxes.

6	Specify the leader style that you want:

•	Check Bent Leader, if appropriate.

•	Select an Arrowhead Style from the pull-down menu.

•	Select a Line Style from the scroll-down list. Typically, a Solid line indicates the target is on the near side; a Dashed line indicates the target is on the far side.

7	Click OK to accept the datum target symbol that you constructed; click Cancel if you do not want to accept the symbol.

To change the location of the datum target symbol, click and drag the circle.

To edit the datum target symbol, right-mouse click on the circle and select Properties from the menu. The Datum Target Symbol dialog appears.


Datum Target Symbol Dialog

To create a datum target symbol:

1	Enter a value for the Target area size box; click [image] if the value describes a diameter.

2	Click the Display target area size outside check box if you want to place the value outside the target symbol circle.

3	Enter up to three Datum Reference labels in the boxes.

4	Specify the leader style that you want:

•	Check Bent Leader, if appropriate.

•	Select an Arrowhead Style from the pull-down menu.

•	Select a Line Style from the scroll-down list. Typically, a Solid line indicates the target is on the near side; a Dashed line indicates the target is on the far side.

5	Click OK to accept the datum target symbol that you constructed; click Cancel if you do not want to accept the symbol.


Edit Definition

Allows you to change the current definition of a feature.

To change a feature’s definition:

1	Click on the feature or on its name in the FeatureManager design tree, then click Edit, Definition.

- or -

Right-click the feature or its name, then click Edit Definition.

2	Change the Depth, Distance, Radius, or other parameters as necessary.

3	Click OK.


Delete

Removes the selected item(s).

To delete:

1	Select the item(s) to delete.

2	Click Edit, Delete or press the Delete key.

If you are deleting a feature, sketch, or drawing view, a Confirm Delete dialog shows the item you are deleting and a list of its dependents. Click Yes to confirm that you want to delete the item and its dependents.

Note	If you select more than one item, clicking Yes to All deletes all of the items and all of their dependents.


Delete Design Table

Lets you delete a previously created design table in the currently active document.

To delete a design table:

1	Click Edit, Delete Design Table.

2	Confirm the deletion and click OK.

Note:  Deleting a design table does not delete any configurations created from the design table.


Derive Component Part

Derives a new part from the selected assembly component.

To derive a component part in an active assembly:

In the FeatureManager design tree, select a component and click File, Derive Component Part.


Derived Sketch

Derives a sketch from another sketch that belongs to the same part or a different part.

To derive a sketch:

1	Select the sketch from which you want to derive a new sketch.

2	Hold the Ctrl key and click the face on which you want to place the new sketch.

3	Click Insert, Derived Sketch.

The sketch appears on the plane of the selected face, and you are editing the sketch.

4	Position the derived sketch by dragging and dimensioning it to the selected face. (The derived sketch is rigid and drags as a whole entity.)

Note the following:

•	If you delete a sketch from which a new sketch was derived, you are prompted that all derived sketches will automatically be underived. Click Yes or No.

•	You cannot add or delete geometry on a derived sketch; it is always the same as its parent. However, you can re-orient it using dimensions and geometric relations.

•	When you make changes to the original sketch, the derived sketch is updated automatically.

•	To break the link between the derived sketch and its parent sketch, right-click the sketch name in the FeatureManager design tree and select Underive from the menu. (After the link is broken, the derived sketch will no longer update when a change is made to the original sketch.)


Join

To create a joined part:

1	Click the parts that you want to join in the FeatureManager design tree or the graphics window. The names appear in the Design Component list.

2	Click Hide Input Components if you want to hide the original components in the assembly document. When the input components are hidden, their icons in the FeatureManager design tree are shown in white with a grey outline.

3	Click Extend Smallest Abutting Faces if you want to fill in the spaces where the components just touch each other.

4	Click OK when the list is complete.

To edit a joined part:

1	In the FeatureManager design tree, Ctrl-click the part(s) you want to remove from the joined component, or select new components to be joined to the existing component.

2	Click OK.


Base Part

Lets you use a previously created part as the base feature for a new part.

The original part becomes a single feature in the new part. You can add new features to it, but you cannot make changes to its original features. Changes made to the original part document are reflected when you rebuild the derived part.

To create a Base Part:

1	Create a new part document.

2	Click Insert, Base Part.

3	Select an existing part file and click OK.


Design Table

Allows you to build multiple configurations of parts by driving dimension values from cells in an embedded Microsoft Excel spreadsheet. The design table is saved in the part file and is not linked back to the original Excel file. Changes you make in the part are not reflected in the original file.

Note	You must have Microsoft Excel installed on your computer to use design tables.

To create a design table:

1	Open Microsoft Excel and create a spreadsheet.

Note	This procedure describes entering the data in Excel before inserting the table. You can also insert a partially empty spreadsheet and complete editing it in SolidWorks, as described below.

2	In the first row, enter the names of the dimensions or features that you want to control.

Dimension names are in the form Dimension name @ Feature or Sketch name, or just the Feature name. For example, the default name for the depth of the first extrusion in a part is D1@Base-Extrude1.

To see a dimension’s name, right-click on the dimension, then click Properties. You can also use the Properties command to assign more meaningful names to dimensions. Dimension names are case-sensitive, so the name in the spreadsheet must match the name in the part exactly.

3	In the first column, enter the names of the design variations you want to create.

4	Fill in the dimension values in each column. For example:

D1@Base-Extrude	D2@Cut1-Extrude

Housing, rev 1	45	88

Housing, rev 2	48	94

Note	You can unsuppress a feature by putting the feature name in the first row and yes in the appropriate cell. You can suppress a feature by leaving the related cell blank.  For example, the following will suppress the feature Cut1 in the version named rev 2.

D1@Base-Extrude	Cut1-Extrude

Housing, rev 1	45	yes

Housing, rev 2	48

5	Save the spreadsheet.

6	Open the part where you want to use the design table.

7	Click Insert, Design Table.

8	Locate the spreadsheet file and click OK.

The spreadsheet appears in the part document, and the Excel menus and toolbars also appear.

9	Edit the table, if necessary. When you are finished editing, click on the part, anywhere outside the table. The SolidWorks menus and toolbars will reappear, and the part will rebuild, using the first row of dimension values in the table.

To select another configuration, click Tools, Configuration, and select a configuration from the list displayed by the SolidWorks Configurations Manager dialog.

Note	The various design table instances can be associated to drawing views.

Different design table instances can be displayed simultaneously in different drawing views.

See also Edit Design Table  and Delete Design Table .


Edit Design Table

Allows you to make changes to an existing design table.

To edit a design table:

1	Click Edit, Design Table. The table appears, and the Excel menus and toolbars also appear.

2	Edit the table. You can change the dimension values in the cells, add new columns to add design variations, or add new rows to control additional dimensions.

3	Click anywhere outside of the design table to close it.


Detach Segment On Drag

Allows detaching a segment (line, arc, ellipse, or spline) from the other entities it is attached to in a sketch.

To detach a sketch segment:

Click Tools, Sketch Tools, Detach Segment on Drag and select the entity that you want to drag away from another sketch entity.

The dragged entity detaches from any entities it shares points with.

Note	Detach Segment On Drag does not delete any relations that the sketch entity may have, so it is possible that the entity may not drag or may not drag smoothly. If this occurs, you should delete any relations before you drag/detach the entity. (See Display/Delete Relations .)


Detail

Creates a detail view in a drawing.

To create a detail view:

1	Activate a drawing view. (Double-click the view, or right-click on the view and click Activate View.)

2	From the Tools, Sketch Entity menu (or the Sketch Tools toolbar), select a sketch entity to create a closed profile around the area of the drawing that you want in the detail view.

3	Click [image] and select the closed profile.

4	Click [image] or Insert, Drawing View, Detail.

A detail circle appears in the original view and a detail view appears.

5	Click on the detail view and drag it to the desired location on the sheet.

Note	To change the detail label on the original view, double-click the label and type the new text.  Click OK.

See also Detail Circle .


Detail Circle

Lets you change the label associated with a detail circle in a drawing.

To change the label text in a detail circle:

1	Right-click the label text.

2	Select the text in the Label  box and enter new text.

3	To choose a new font style or size, deselect Use Document’s Font and click the Font button.  Use the Choose Font dialog to specify a font for the label text.

4	Click OK.

See also Detail .


Dimensions

Creates dimensions. The type of dimension (point-to-point, or angular) is determined by the items on which you click.

1	With a sketch active, click [image] or Tools, Dimensions and select from Parallel, Vertical, Horizontal.

- or -

With a drawing active, click [image] or Tools, Dimensions and select from Parallel, Vertical, Horizontal, Baseline, Ordinate, Horizontal Ordinate, or Vertical Ordinate.

- or -

Press the right mouse button and select Dimension from the menu. Right mouse click on a dimension and select the dimension type (Horizontal, Vertical, etc.) from the menu.

2	Click on the items to dimension, as shown in the table below.

3	Click again to place the dimension.

To Dimension...	Click on...	Note
Length of a line or edge	The line.
Angle between two lines	Two lines, or a line and a model edge.	If the lines are parallel, this creates a distance dimension.
Distance between two lines	Two parallel lines or a line and a parallel model edge.
Perpendicular distance from a point to a line	The point and the line or model edge.
Distance between two points	Two points.	One of the points can be a model vertex.
Radius of an arc	The arc.
Diameter of a circle	The circumference.
To change a dimension value:

1	Double-click the dimension value.

2	Type a new value, click on the arrows to set a new value, or enter a calculation in the box.

•	Click [image] to accept the current value and exit.

•	Click [image] to restore the original value and exit.

•	Click [image] to reverse the value of those parameters that are reversible, such as offset.

•	Click [image] to regenerate the model with the current value.(Not available in a sketch.)

•	Click [image] to change the spin box increment value.

Note:	When using any trig function in a dimension dialogue or an equation, the value of the angle is interpreted as radians. For example, sin(90) is evaluated as .89 (90radians) not 1.0 (90deg).

See also Horizontal Dimension, Vertical Dimension, Parallel Dimension , Baseline Dimension, Ordinate Dimension, Horizontal Ordinate Dimension, Vertical Ordinate Dimension, Equations.


Dimension Precision

To Specify the precision for dimensions:

1	Enter values for the number of decimal places and tolerance for Primary Units, Angular Units, and Alternate Units.

2	Click OK to accept your values, or click Cancel.

Note:	Only those unit types that are appropriate for the selected dimension are visible in the dialog box. For example, Angular Units are only available if the dimension you selected is angular.


Dimension Preferences

Sets the default properties for new dimensions.

To set default dimension properties:

1	Click Tools, Options.

2	Click the Detailing tab.

3	Change the settings. See Dimension Properties and Dimension Tolerance properties for details.

4	Click OK.


Display as Icon

Displays an embedded OLE object as an icon.

To display an OLE object as an icon:

1	Select the OLE object.

2	Click Edit, Object, Display as Icon.

See also Object .


Display Content

Displays the contents of an OLE object embedded in your SolidWorks document.

To display an OLE object:

1	Select the OLE object.

2	Click Edit, Object, Display Content.


Display/Delete Relations

You can view the relations on each entity by selecting the entity and clicking [image] or Tools, Relations, Display/Delete. If your sketch becomes “overdefined” or “not solved,” use Display/Delete to examine and delete relations as necessary.

To view or delete relations:

1	Click the sketch entity about which you have a question. (If no entity is selected, all relations in the sketch are listed.)

2	Click [image] or Tools, Relations, Display/Delete.

A dialog box appears that tells how many relations apply and allows you to view or delete the relations.

The Status box informs you of any conflicting relations. (The status can be Dangling, Satisfied, Overdefined, or Not Solved.)

3	Click Next or Previous to view each of the relations in turn, if there is more than one.

4	You can click the Suppressed check box to suppress or unsuppress the current relation.

5	Click Delete to delete the current relation; click Delete All to delete the relations to this entity.

You can specify search criteria for listing relations in a sketch by using the Display Constraints By box. For example, you can click Specified Criteria, and choose Dangling to list all the dangling relations in the sketch.

You can continue to display relations for any or all entities in the sketch. The dialog box remains open until you click the Close button.


Display Grid

Displays a grid on a drawing. The grid, which is optional, may be useful when you are using the sketch entities and sketch tools on a drawing.

To display a grid:

Right-mouse click on an active drawing sheet and select Display Grid from the menu.

To change the grid properties, see Grid/Units.


Dome Feature

You can add a dome feature to any model face that has a circular, elliptical, or four-sided boundary. A four-sided boundary need not be rectangular, and each side may consist of a single segment or a set of tangent segments.

To create a dome on a planar face:

1	Click [image] or Insert, Features, Dome.

2	Select a planar Dome Face in the graphics area.

3	Specify the Height, and observe the preview. The height is measured from the centroid of the selected face.

4	Click Reverse Direction to create a concave dome (default is convex).

5	If you selected a circular or elliptical face, you can select Elliptical Dome. This creates a dome whose shape is a half ellipsoid, with a height equal to one of the ellipsoid radii.

6	Click OK.


Dome

1	Select a planar Dome Face in the graphics area.

2	Specify the Height, and observe the preview. (The height is measured from the centroid of the selected face.)

3	Click Reverse Direction to create a concave dome (default is convex).

4	If you selected a circular or elliptical face, you can select Elliptical Dome. This creates a dome whose shape is a half ellipsoid, with a height equal to one of the ellipsoid radii.

5	Click OK.


Draft

Creates a feature that tapers selected model faces by a specified angle, using either a neutral plane or a parting line.

Note	You can also apply a draft angle as part of an extruded base, boss, or cut. (See Extrude.)

To draft a model face to a neutral plane:

1	Click [image] or Insert, Features, Draft.

2	In the Type of Draft box, select Neutral Plane.

3	Set the Draft Angle.

4	Click in the Neutral Plane box, and select a face or reference plane to serve as the neutral plane. The draft angle is measured perpendicular to this plane.

5	If you want the draft to slant in the opposite direction, click Reverse Direction.

6	Click in the Faces to Draft box, and select the faces to draft in the graphics area.

7	Choose an item from the Face Propagation list that describes how you want the draft to propagate across additional faces:

•	None - Draft only the selected face.

•	Along Tangent - Extend the draft to all faces that are tangent to the selected face. (The faces meet with filleted corners.)

•	All Faces - Draft all faces next to the neutral plane and extruded from the neutral plane.

•	Inner Faces - Draft all faces extruded from the neutral plane.

•	Outer Faces - Draft all faces next to the neutral plane.

8	Click OK.

To draft to a parting line:

1	With a part open that already has a split line , click [image] or Insert, Features, Draft.

2	In the Type of Draft box, scroll to select Parting Line.

3	In the Draft Angle box specify the angle that you want.

4	Click in the Direction of Pull box and click the face toward which you want the draft angle to go. A directional arrow displays; click Reverse Direction if the arrow is not pointing in the correct direction.

5	Click in the Parting Lines box.

6	Hold the Ctrl key and select the parting line on each face of the part. Use the Select Other right-mouse option as necessary. The list of selected line segments displays in the Parting Lines box.

7	Choose an item from the list that describes how you want the draft to propagate across additional faces:

•	None - Draft only the selected face.

•	Along Tangent - Extend the draft to all faces that are tangent to the selected face.

8	Click OK to complete the draft of the part.

See also Split Line .


Drawing View Orientation

Creates a part view in a drawing.

To create the view:

1	Click on a face on the part.

2	Select the direction you want the selected face to be orientated towards, then click OK.

3	Click on a second face, then select its orientation and click OK.

4	Activate the drawing window, and click where you want to place the view.


Edges Options

To set options for edge display:

1	Click Tools, Options.

2	Click on the Edges tab.

3	Change the settings (below) and click OK to accept the changes; click Cancel to discard the changes and exit the dialog box; click Reset All to return to the installed system defaults.

Hidden Edges

•	Gray or Dashed. Specifies whether hidden edges are displayed as gray lines or dashed lines in Hidden in Gray mode.

•	Select Hidden for Wireframe/HLG. Allows you to select hidden edges or vertices in Wireframe and Hidden In Gray modes.

•	Select Hidden for HLR and Shaded. Allows you to select hidden edges or vertices in Hidden Lines Removed and Shaded modes.

Part/Assembly Tangent Edge Display

•	Tangent Edges Visible – Tangent edges displayed.

•	Tangent Edges as Phantom –Tangent edges display using the Phantom style line font ( [image]).

•	Tangent Edges Removed – Tangent edges are not displayed.

Repaint After Selection in HLR. When selected, specifies that a selected feature is repainted in HLR if you click on space. When not selected, specifies that the selected feature is repainted in wireframe.

Highlight All of Selected Feature. Specifies that the entire feature is highlighted when you click on it.

Dynamic Highlight from Graphics View. Specifies whether model faces, edges, and vertices are highlighted when you move the cursor over a sketch, model, or drawing.


Edit Assembly

Activates the assembly for editing after you complete editing a part in the assembly.

To return to editing the assembly,

click [image], the Edit Part tool (which is depressed while you are editing a part),

-or-

right-click the name of the assembly in the FeatureManager design tree, and select Edit Assembly,

-or-

right-mouse click in the graphics area and select Edit Assembly:<AssemblyName>.


Edit Drawing Reference

You can change the model used in a drawing. This is useful in cases where you have a group of similar parts, each requiring drawings with similar details. You can save time and produce more consistent drawings for each member of the group by taking advantage of this capability.

To edit a drawing reference and reuse the annotations:

1	Create a drawing for one of the parts in the group, setting up the various sheets and views you want.

2	Add all the annotations that are common to the group (surface finish symbols, notes, etc.). You can also include annotations that are specific to the current part, such as reference or model dimensions.

3	Save a copy of the drawing (you can use the Save As Copy option in the Save As dialog box).

4	Click File, Open, select the copy of the drawing, and click References.

5	Edit the referenced file location to select one of the other parts in the group, and click Open.

You are notified that the internal IDs of the documents do not match.

6	Click Yes to accept the document.

The Dangling Detail Items dialog box appears. The values in the Count column indicate the number of dangling annotations of each type.

7	Click the box in the Delete column corresponding to the annotation types you want to delete (dimensions, for example). Leave unchecked the boxes for the annotation types you want to reuse in the new drawing (such as notes).

8	Click OK.

9	When the drawing is displayed, you can re-attach any remaining dangling detail items.


Edit Equations

Allows you to make changes to a selected equation.

To change an equation:

1	Choose an equation in the list and select and replace values as needed.

2	Click OK to accept the changes you made; click Cancel to discard your changes and close the dialog box.

3	When you return to the graphic display, click [image] or Edit, Rebuild to apply the change.


Edit Part

Editing a part (component) while in an assembly allows you to use surrounding geometry for reference while creating new features. The sketches that you create while editing a part in the assembly may use any edge or reference a dimension to any edge or any part in the assembly. Features may use any end condition , such as Up to Surface, on another component.

To edit a part while in an assembly:

1	Right-click on a part in the FeatureManager design tree or the graphics area.

2	Click [image], or select Edit Part from the right mouse menu.

The title bar shows the name of the part in the assembly that is open for editing

Also note that the message in the lower right corner of the window indicates that you are now editing the part document even though the entire assembly is visible.

The assembly component that you are editing turns pink, and the other components turn grey, if they are in shaded view mode. (Otherwise the lines of the component you are editing turn pink.)

3	To make changes to the part, use Sketch Entity tools, Sketch Tools, Dimensions, and Relations from the Tools menu.  Click Boss, Cut, and/or Features on the Insert menu to create extrusions or features.

4	To return to editing the assembly, click [image] again, or right-click anywhere in the graphics area and select Edit Assembly:assemblyname.

Note:	When you edit a part in an assembly, do not create an Up to Next extrusion expecting to extrude to the surface of another component in the assembly. The Up to Next option only goes to the next set of surfaces on the same part. Up to Surface and Up to Vertex options can be used when you want to go up to geometry on another component in the assembly.


Edit Macro

Edits or debugs a macro that you recorded previously.

To edit a macro:

1	Click [image] or Tools, Macro, Edit.

2	Select a macro file and click OK.

3	Edit the macro. (For details, use the online help in the macro editor.)


Edit Referenced File Locations

You can edit the locations of referenced parts:

•	To select different parts for an assembly or drawing,

•	To save selected assembly parts to a new location or filename.

To edit part location:

1	In the New pathname list, select a path or filename that you want to edit.

If you want to edit all the entries on the list, click Select All.

2	You can edit the path or filename using one of the following methods:

•	Select the list entry by clicking it two times, then you can type a new path and/or filename.

•	Select a list entry and use the Browse button to change to a new drive or directory path.

•	Click the Replace button and enter a word to find and a word to replace with. (For example, change “\samples” to “\archive” to move one or all part files to the archive directory.) Click Match case if the case is significant in the search.

3	Click OK to make the changes and exit the dialog. Click Cancel to exit without saving your changes.


Add to Ordinate Dimension

Adds new ordinate values to an already defined set of ordinate dimensions.

To add ordinate dimensions:

1	Right-click one of the ordinate values and select Add to Ordinate from the right-mouse menu.

2	Click a new item to dimension, and click again to place the dimension.

3	Repeat, until all the additional items are dimensioned and placed.

See also Ordinate Dimension , Align Ordinate   , Horizontal Ordinate Dimension , Vertical Ordinate Dimension .


Edit Properties

Lets you view and edit the properties of a selected item.

To view and edit an item’s properties:

1	With the cursor over the item in the graphics window or in the FeatureManager design tree, select the right mouse button and choose Properties from the right button menu

- or -

click on the item or its name in the FeatureManager design tree and select Edit, Properties

2	Make any appropriate changes (some property values are read-only) and click OK.


Edit Sheet/Edit Template

Toggles between opening either a drawing sheet or a drawing template for editing.

To edit a drawing sheet:

Click Edit, Sheet, or right-click on the sheet and select Edit Sheet from the menu.

To edit a drawing template:

Click Edit, Template, or right-click on the sheet and select Edit Template from the menu.

To end editing the template, select Edit Sheet and return to editing the drawing sheet.

For more information about editing the drawing template, see Customize Drawing Template .


Edit Sketch

Opens an existing sketch so you can edit it.

To edit a sketch:

1	Right-click on the sketch you want to edit or on a feature built from the sketch, either in the model or in the FeatureManager design tree.

Note	For features built from multiple sketches (lofts and sweeps), right-click on the sketch in the FeatureManager design tree.)

2	Click Edit Sketch.

3	To close the sketch when you are finished editing, right-click anywhere in the sketch and click Edit Sketch or click [image],

- or -

to exit the sketch and rebuild, click  [image].


Edit Sketch Plane

Changes the sketch plane.

To change the plane of a sketch:

1	Right-mouse click the sketch in the FeatureManager design tree, and select Edit Sketch Plane.

2	Select a new plane by clicking a plane in the FeatureManager design tree or select a new face by clicking a different model face in the sketch.

3	Click Apply or click Cancel to exit without making a change.


Sketching Plane

1	Select a new plane by clicking a plane in the FeatureManager design tree or select a new face by clicking a different model face in the sketch.

Note:	If you have trouble selecting a hidden face, right-mouse click and use the Select Other option.

2	Click Apply, or click Cancel to exit without making a change.


Ellipse

Creates an ellipse.

To create an ellipse:

1	Click Tools, Sketch Entity, Ellipse or [image].

2	Point where you want to place the center of the ellipse.

3	Press the mouse button and drag to set the major axis of the ellipse.

4	Release the mouse button.

5	Press the mouse button again over the ellipse curve, and drag the minor axis of the ellipse.

6	Release the mouse button.

See also Centerpoint Ellipse .


Ellipse Properties

Displays the properties of an ellipse or centerpoint ellipse.

Start Point, End Point, and Center Point. Displays the X, Y, Z coordinates of the start point, end point, and center point.

Radius and Angle. Displays the values for Radius1, Radius2, and angle of the arc.

Defined Status. Indicates whether the ellipse is currently underdefined or fully defined.


Empty View

Allows you to insert an empty view in a drawing. You can add sketch geometry to the active view that you can drag or delete as a group. You can still edit sketch entities individually.

To insert an empty view in a drawing:

1	Click on the drawing sheet where you want to place the empty view.

2	Click Insert, Drawing View, Empty.

3	To move the view, select the view and drag the green border (not the handles).

4	Double-click the view to make it active (red border), or right-mouse click and select Activate View from the menu.

Use the Sketch Entity tools to create sketch geometry; use the Relations tools for making or deleting relations; use the Dimensions tools for dimensioning.


Entity Property

Displays the properties of a face or edge.

To view or change the name or color of a part face:

1	Right-click on a part face.

2	Select Face Properties.

3	View the color in the preview box, or change the color of the face by using one of the following methods:

•	Change the numeric values for Red, Green, or Blue, and click OK.

•	Click Use Part Color to use the default part color.

•	Click Change Color and select a color from the color blocks or the custom color palette. Then click OK.

•	Click Advanced  and use the sliders to increase or decrease advanced lighting values such as ambient, shininess, transparency, etc.

4	You can enter a name for the face in the Entity Name block, or change the name by entering a new name.

5	Click OK.

To view or change the name of an edge:

1	Right-click on a part edge.

2	Select Edge Properties.

3	You can enter a name for the edge in the Entity Name block, or change the name by entering a new name.

4	In a drawing, you select line visibility by clicking Hide Entity or Show Entity .

5	Click OK.


Equations

Creates mathematical relations between model dimensions, using dimension names as variables. When using equations in an assembly, you can set equations between parts, between a part and a subassembly, with mating dimensions, and so forth.

Note	Dimensions driven by equations cannot be changed by editing the dimension value in the model.

To add an equation:

1	Click Tools, Equations.

2	Click Add.

3	In the model or the FeatureManager design tree, double-click on the feature that contains the first dimension you want to use in the equation.

4	Click on the dimension to paste its name into the equation. (Dimension names are in the form dimension name @ feature or sketch name.)

5	Complete the equation by typing or clicking on the calculator buttons, or by clicking on other dimensions to paste their names.

Equations are solved left to right (i.e., the dimension on the left is driven by the value on the right), in the order in which they appear in the equation list.

6	Click OK. The equation will appear in the Equations window.

7	Click OK, then click [image] or Edit, Rebuild to update the model. (All equations are solved before the geometry is regenerated.)

Note:	When using any trig function in an equation or dimension dialogue, the value of the angle is interpreted as radians. For example, sin(90) is evaluated as .89 (90radians) not 1.0 (90deg).

To edit equations:

1	Click Tools, Equations.

2	Click Edit All.

3	Edit the equations. Each equation must be on a separate line, and dimension names must be enclosed in quotes.

4	Click OK to close the Edit Equations window.

5	Click OK to close the Equations window.

6	Click [image] or Edit, Rebuild.


New Equation

To create an equation:

1	In the model or the FeatureManager design tree, double-click on the feature that contains the first dimension you want to use in the equation.

2	Click on the dimension to paste its name into the equation. (Dimension names are in the form dimension name @ feature or sketch name.)

3	Complete the equation by clicking on the calculator buttons, or by clicking on other dimensions to paste their names.

Equations are solved left to right (i.e., the dimension on the left is driven by the value on the right), in the order in which they appear in the equation list.

4	Click OK. The equation appears in the Equations window.

5	Click OK, then click [image] or Edit, Rebuild to update the model. (All equations are solved before the geometry is regenerated.)

Note:	When using any trig function in an equation or dimension dialogue, the value of the angle is interpreted as radians. For example, sin(90) is evaluated as .89 (90radians) not 1.0 (90deg).


Exit

Closes the SolidWorks application.

To exit SolidWorks:

Click File, Exit.

If you have open files with unsaved changes, you will be prompted to save them.


Explode Assembly

Explodes the view of an assembly so you can look at it with the components separated. At times, it is useful to separate the components of an assembly to visually analyze their relations. When you explode an assembly, all mating relations are maintained.

An exploded view consists of one or more explode steps. An exploded view is stored with the assembly configuration with which it is created. Each configuration can have one exploded view.

To create an exploded view of an assembly:

1	Click Insert, Exploded View.

The Assembly Exploder dialog box appears, with these Step Editing Tools:

	Create a New Step
	Edit the Previous step
	Edit the Next step
	Undo changes to the currrent step
	Delete the current step
	Apply/update the current step
2	Click New Step. The Assembly Exploder dialog box expands.

3	Click an edge or face that is parallel to the direction you want to explode.

A preview arrow appears and a description of what you have selected appears in the Direction to explode along: box. If the preview arrow is pointing in the wrong direction, click Reverse direction.

4	Click the component(s) you want to explode, either in the FeatureManager design tree or in the graphics area.

The component name appears in the Components to explode: box.

5	Click Apply [image].

The component explodes from the assembly.

6	Drag the green handle to position the component as desired, or if you prefer to explode the component a precise distance, enter the distance in the Distance: box.

7	Click Apply to update the step.

8	If you are satisfied with this exploded view, click OK.

If you want to add more explode steps to the exploded view, click New Step, repeat Steps 3 through 7 until all the steps are complete, then click OK to finish the exploded view. Remember to click Apply after defining each step.

To collapse the assembly:

Right-click anywhere in the graphics window, and select Collapse.

To view the exploded view:

1	Click the Configuration Manager icon at the bottom of the window.

2	Expand the desired configuration.

3	Double-click the ExplView feature. The assembly explodes.

See also Edit Exploded View .


Auto Explode

Automatically creates an exploded view of a simple assembly with few components.

To create an exploded view using Auto Explode:

1	Click Insert, Exploded View.

2	In the Assembly Exploder dialog box, click Auto Explode. The assembly explodes.

You can edit an Auto Explode view in the same manner as any exploded view.

See also Explode Assembly.


Assembly Exploder

To automatically explode an assembly with few components:

Click Auto Explode.

To create separate explode steps for an exploded view:

1	Click New Step [image]. The Assembly Exploder dialog box expands.

2	Click an edge or face that is parallel to the direction you want to explode. The selected entity is listed in the Direction to explode along box.

3	If the preview arrow points in the wrong direction, click Reverse direction.

4	Click the component(s) you want to explode, either in the FeatureManager design tree or in the graphics area. The selections are listed in the Components to explode box.

5	If you selected a component that is part of a sub-assembly:

•	Click Entire sub-assembly to explode the selected component and all other components belonging to the sub-assembly.

•	Click Component part only to explode only the selected part, leaving the rest of the subassembly in place.

6	Click Apply [image]. The component(s) explodes from the assembly.

7	Drag the green drag handle to position the component(s) as desired, or to explode the component(s) by a precise distance, enter the distance in the Distance: box.

8	Click Apply to update the step.

9	To add more explode steps to the exploded view, repeat the process for each component or group of components. Remember to click Apply after defining each step.

10	When you are satisfied with the completely exploded view, click OK.

To edit the explode steps:

1	Select the Explode Step you want to edit, or use the [image] [image] buttons to examine and edit each step in turn.

As you select each step, the drag handle appears and the components involved are highlighted or enclosed in bounding boxes.

2	Edit the explode step by dragging the green handle, changing the distance or direction, etc., until the component is positioned as desired.

3	To change the Components to explode or the Direction to explode along, click the corresponding box, then click the desired entities to select or deselect them.

4	To clear the contents of a box and start again, click the box, then right-click in the graphics area, and select Clear Selections.

5	To undo the changes to a step, click [image].

6	Click [image] after editing each step.

7	To delete an explode step, click [image].

8	Click OK to finish the view.


Edit Exploded View

Allows you to edit the explode steps in an exploded view. Each assembly configuration can have one exploded view.

There are several ways to edit an exploded view and its steps. You can:

  Edit the Explode Steps in Turn

  Edit the Explode Steps for a single component

  Edit the Explode Steps in a Complex Assembly


Edit Explode Steps in Turn
Edit All Explode Steps in Turn

To edit an exploded view step by step:

1	Click the Configuration Manager icon at the bottom of the window.

2	Expand the desired configuration, and expand the exploded view to see the steps,

- or -

Right-click the ExplView feature, and select Edit Definition.

3	Select the Explode Step you want to edit, or use the [image] [image] buttons to examine and edit each step in turn.

As you select each step, the drag handle appears and the components involved are highlighted or enclosed in bounding boxes.

4	Edit the explode step until the component is positioned as desired.

5	Click [image] after editing each step.

6	Click OK to finish the view.


Edit Explode Steps for a Single Component

To edit the explode steps for one component:

1	Click the Configuration Manager icon at the bottom of the window.

2	Expand the desired configuration, then double-click the ExplView to explode the view.

3	Right-click the component you want to reposition in the graphics area, and select Show Explode Steps.

The drag handle(s) for the explode step(s) on the selected component is displayed.

4	Drag the component by the green drag handle to the new position.

5	Repeat as needed for each component, click Apply after editing each step, and click OK to finish the view.


Edit Explode Steps in a Complex Assembly

For complex assemblies, you may find it easier to edit the explode steps by selecting the component from the FeatureManager design tree.

To edit a complex exploded view:

1	Click the Configuration Manager icon at the bottom of the window.

2	Expand the desired configuration, then double-click the ExplView feature to explode the view.

3	Switch from Configuration Manager view to FeatureManager view by clicking the FeatureManager icon at the bottom of the window.

4	Right-click a component to reposition in the FeatureManager design tree, and select Show Explode Steps.

5	Drag the component by the green drag handle(s) to reposition as needed, then click anywhere to apply the edits.

6	Repeat Steps 4 and 5 as needed for each component, then collapse the assembly. The next time you explode the assembly, the new values are used.


External References

Specifies how assembly, part, and drawing files with external references are opened and managed.

To specify how SolidWorks manages references to external files:

1	Click Tools, Options.

2	Click on the External References tab.

3	Make any necessary changes to the options listed below.

4	Click OK to accept the changes; click Cancel to discard the changes and exit the dialog box; click Reset All to return to the installed system defaults.

External References

Open referenced documents with read-only access. Specifies that all referenced documents will be opened for read-only access by default.

Don’t prompt to save read-only referenced documents (discard changes).  Specifies that when this part is saved or closed, no attempt will be made to save its referenced documents that are opened for read-only access.

Search document folder list for external references. Specifies that the document folder list is searched to update any external references.

Folders

Show folders for: Displays documents of various types.

You can specify the search rules for locating external documents. Folders are searched in the order in which they are listed in the External References display box.

To add a new directory path to search order, click the Add button.

To delete a directory path from the External References display box, select the path listed in the External References display box, and click the Delete button.

To change the search order, select a directory path listed in the External References display box and click either the Move Up button or the Move Down button, depending on how you want to change the search order.

Assemblies

Automatically generate names for referenced geometry. (This option is off by default.)

When this option is off, you can mate to parts for which you have read/only access because you are using the internal face IDs of the parts. Unless you will use component replacement, leave this option off, especially in a multi-user environment.

When this option is on, you automatically create surface identifiers (for example: Face1, Face2) at the time you mate the part, therefore you need write access to the part, in most cases. Turn this option on if you intend to do component replacement using the same surface identifiers, remembering that you need write access to the parts you are using. (Rename the corresponding edges and/or faces on the replacement component to match the edge/face names on the original part.)

Update component names when documents are replaced. Deselect this option only if you use the Component Properties dialog to assign a component name in the FeatureManager design tree that is different from the filename of the component.


List External References

You can list out the external references of any component or  feature created in the context of an assembly.

To list the external references for a feature or component:

Right-mouse click the component in the FeatureManager design tree and select List External Refs from the right mouse menu.

Note:	Features or components that do not have external references do not have this option listed in the menu.

A dialog box appears with the following fields and types of information:

External References For:  Displays the name of the selected component or feature in the top banner or the dialog box.

Assembly.  Displays the path and name of the assembly in which the component or feature was created.

Columns:

Feature.  Lists each in-context or derived feature in the selected part.

Data.  Describes the type of derivation used within the feature, such as a derived profile, point, surfaces, etc.

Status.  The status is either In Context or Out of Context depending on whether the listing was taken while in the assembly or in the part alone.

Referenced Entity.  Displays a list of parts and assemblies the data came from.  If sketch information is referenced, both the sketch and part/assembly names are listed.  If geometry alone is used, only the part name appears.

Feature’s Component.  Displays the name of the part(s) in which the derived feature exists.


Extrude

Creates a feature that adds or removes material by extruding a profile for a specified distance.

You can extrude in one or two directions and add a draft while extruding.

An extrusion extends the sketched profile as either a solid feature or a thin feature.

To create an extruded base or boss:

1	Create a sketch and draw the profile you want to extrude, or select an existing sketch that contains a profile. The profile must be closed and cannot intersect itself.

2	Click [image] or Insert, Boss, Extrude (or Insert, Base, Extrude, if this is the first feature in the part.)

3	Select the Type, and specify the Depth if necessary.

4	Click Reverse Direction, if necessary.

5	To add a Draft, select the Draft While Extruding box. Enter a draft Angle and check Draft Outward, if necessary.

6	If the Type you selected relies on the selection of a surface or vertex, select that item now in the graphics area.  The selection displays in the Selected Items list.

7	To extrude the feature in both directions from the sketch plane, select Both Directions, then in the Settings For: box, click Direction 2 and repeat steps 3 through 5 for the other end.

8	Set the Extrude As: box to Solid Feature.

9	Click OK.

To create a thin feature extrusion:

1	Sketch a profile for the extrusion. This does not have to be a closed profile.

2	Click [image] or Insert, Base, Extrude.

3	Select the Type, and specify the Depth.

4	To add a Draft, select the Draft While Extruding box, and enter a draft Angle.

5	If the Type you selected relies on the selection of a surface or vertex, select that item now in the graphics area.  The selection displays in the Selected Items list.

6	To extrude the feature in both directions from the sketch plane, select Both Directions, then in the Settings For: box, click Direction 2 and repeat the steps above.

7	If you are extruding a closed profile sketch, you must set the Extrude As: box to Thin Feature.

8	Click the Thin Feature tab at the top of the dialog box.

9	Select the extrusion Type, and specify the Wall Thickness.

10	If you created a closed profile you can select the following options:

•	Cap Ends. Specifies that the ends of the thin feature are capped. A capped thin feature must be extruded from a closed profile sketch.  When the ends are capped, all walls of the feature are closed; the center is hollow.

•	Cap Thickness. Lets you specify the thickness of the cap. (Available only if Cap Ends is selected.)

- or -

If you created an open profile you can select the following options:

•	Auto Fillet. Automatically creates a round at the each edge where lines meet at an angle.

•	Fillet Radius. Specifies the inside radius of the round.

11	Click OK.

See also Cut Extrude


FeatureManager Design Tree

The FeatureManager design tree on the left side of the SolidWorks window provides an outline view of the active part, assembly, or drawing.  This makes it easy to see how the model or assembly was constructed or to examine the various sheets and views in a drawing.

The FeatureManager design tree and the graphics display window are dynamically linked. You can select features, sketches, drawing views, and construction geometry in either panel.

The FeatureManager design tree makes it easy to:

•	Select items in the model or assembly by name.

•	Identify and change the order in which features are created.  You can drag and drop items in the FeatureManager design tree list to reorder them.  This changes the order in which features are regenerated when the model is rebuilt.

•	Display the dimensions of a feature by double-clicking the feature’s name.

•	Rename items by slowly clicking two times on a name to select it and then entering a new name.

•	Select a feature to revert to when using Rollback, Suppress, Unsuppress, or Unsuppress with Dependents.

•	Temporarily roll the model or assembly back to an earlier state using the rollback bar .

•	View parent/child relations by right-clicking a feature in the list, then selecting Parent/Child.

See also, FeatureManager Design Tree Conventions .


FeatureManager Design Tree Conventions

The FeatureManager design tree uses the following conventions:

•	A [image] symbol to the left of an item’s icon indicates that it contains associated items, such as sketches. Click [image] to expand the item and display its contents.

•	Sketches in the FeatureManager design tree are preceded by (+) if they are overdefined; they are preceded by (–) if they are underdefined; they are preceded by (?) if the sketch could not be solved. (There is no prefix if the sketch is fully defined.) For information about sketch status, see Fully Defined Sketches .

•	Assembly components in the FeatureManager design tree are preceded by (+) if their position is overdefined; they are preceded by (–) if their position is underdefined; they are preceded by (?) if their position could not be solved; they are preceded by (f) if their position is fixed (locked in place).

•	Assembly mates are preceded by (+) if they are involved in overdefining the position of components in the assembly; they are preceded by (?) if they could not be solved.

•	In an assembly, each instance of the component is followed by a number in angle brackets <n> that increments with each occurrence.

•	If a part or feature has an external reference, its name is followed by –>.


FeatureManager Design Tree Display

Provides alternate ways to view the information in the FeatureManager design tree in an assembly document.

To display features or dependencies in an assembly:

Click View, FeatureManager Tree, By Features/By Dependencies.

•	 By Features, displays all components, features, planes, and mate groups.

•	By Dependencies, displays only the top level components and mate groups.


Feature Scope

When creating an assembly feature, you must first determine which components you want to be affected by the feature. By setting the scope, you can selectively choose the components you want the feature to impact.

If you do not set any feature scope, all the components in the assembly are assumed to be in the scope.

To set the scope:

1	In an assembly, select Edit, Feature Scope.

2	Select the components that this assembly feature will affect by clicking the components or the component names in the FeatureManager design tree.

3	The selected component names appear in the Edit Assembly Feature Scope dialog box.

4	Click OK.

•	To remove a component from the list, press Ctrl and click the component again in the graphics area or in the FeatureManager design tree.

•	To change the scope, click Edit, Feature Scope again and make additions to or deletions from the feature scope list.


Fillet
Fillet (Sketched)

Creates a tangent arc at the intersection of two sketch elements, trimming away the corner.

To create a fillet in a sketch:

1	Click [image] or Tools, Sketch Tools, Fillet.

2	Select the sketch elements to fillet. The elements must form a corner.

The items are listed in the Sketch Items to Fillet box.

3	Enter a fillet radius value.

4	Click Apply.

The dialog box stays open so you can continue making other fillets.

5	Click Cancel to close the dialog box.


Fillet/Round

Creates a fillet or round feature on selected model edges.

  Click here  for information about creating a Face Blend fillet.

To create a fillet or round:

1	Select the edges, loops, and faces you want to round.

Note	Selecting a face also selects all loops (closed profiles) on the face. To select individual loops, click on the face, then hold the Ctrl key and click on each edge you want to select.

2	Click [image] or Insert, Features, Fillet/Round.

3	Specify the fillet Radius.

4	The default setting Propagate To Tangent Faces will extend the fillet to all faces that are tangent to the selected faces. Deselect it, if necessary.

5	Select the Overflow Type (see below).

6	View the Items Selected box to be certain that you have selected the edges, faces, or loops that you intended.

7	Click OK.

To create a variable radius fillet:

1	Select the edges, loops, and faces you want to round.

2	Click [image] or Insert, Features, Fillet/Round.

3	Change the Fillet Type to Variable Radius.

4	Select Smooth Transition or Straight Transition.

5	In the Items Selected list, click Vertex1. The fillet radius appears on the model, showing which vertex is selected.

6	Enter the desired radius for the selected vertex in the Radius box.

7	Repeat steps 5 and 6 for each vertex.

8	Click OK.

Overflow Type:

•	Default. The system chooses one of the following options, depending on the geometry conditions (convexity of edges being filleted and the adjacent edges, and so on).

•	Keep Edge. Maintains the integrity of adjacent linear edges. The fillet surface is broken into separate surfaces, and the top edge of the fillet may be uneven.

•	Keep Surface. Uses the adjacent surface to trim the fillet. As a result, the fillet edge is continuous and smooth, but the adjacent edge is changed.


Face Blend

You can blend non-adjacent faces with a Face Blend fillet.

To insert a face blend fillet:

1	Select Insert, Features, Fillet/Round.

2	Change the Fillet Type to Face Blend.

3	Click the first face or set of faces to be blended. Under Items to Fillet, the selection is indicated in Face Set 1.

4	Click the Face Set 2 box, and click the face(s) to blend with.

5	Specify the Radius.

6	If you want the blend to continue along tangencies, click Propagate to Tangent Faces.

7	If any of the selected faces has a tangency which results in an ambiguity, you can use a Help Point to resolve the ambiguous selection. Click Use Help Point, then click an edge or face where you want to insert the fillet.

8	Click OK.


Find References

Locates the part or subassembly documents associated with the components in an active assembly.

To find the part or subassembly files of the components in the active assembly:

1	Click File, Find References.

The Search Results box lists the path and filename of each part file or assembly file in the assembly.

If the assembly consists of one or more sub-assemblies, the sub-assembly file and all of its component part files are displayed.

2	To copy the listed files to the current directory (or a different directory), click the Copy Files button in the dialog box.

The Choose Directory dialog lets you browse your local drive(s) or a network drive to select a directory and path to copy the file to.

3	To retain the directory structure of the file copies, click the Preserve directory structure box.

4	Click OK to complete the copy and close the Choose Directory dialog.

5	Click Close to close the Search Results dialog.


Fix/Float

Toggles the Fixed property on or off for individual components in an assembly. The first component that you add to an assembly is always fixed, initially. Components that you add later float (i.e. can translate and rotate).

•	A fixed component has a (f) before its name in the FeatureManager design tree; it cannot be moved.

•	A floating component has a (-) before its name in the FeatureManager design tree; it can move in relation to fixed components.

To Fix or Float an assembly component:

1	Right-click the component or the component’s name in the FeatureManager design tree.

2	Select Fix or Float from the menu, depending on how you want the component to behave.


Full Page

Zooms in or out so the entire drawing sheet is visible.

To see the entire sheet:

With a drawing active, click [image] or View, Full Page.


Fully Defined Sketches

Sketches may be in any of five states described below. The state of the sketch is displayed in the status bar at the bottom of the SolidWorks window.

•	Fully Defined  -- displayed as black lines. All the lines and curves in the sketch, and their positions, are described by dimensions and/or relations.

•	Overdefined  -- displayed as red lines. There are dimensions and/or relations that are either in conflict or are redundant. To view and remove conflicting relations, see Display/Delete Relations .

•	Underdefined  -- displayed as blue lines. Some of the dimensions and/or relations in the sketch are not defined and are free to change. You can point the mouse at endpoints, lines, or curves and drag them until the sketch entity changes shape.

•	No Solution Found -- displayed as pink lines. The sketch was not solved. The geometry, relations, and dimensions that prevent the solution of the sketch are displayed.

•	Invalid Solution Found -- displayed as yellow lines. The sketch was solved but will result in invalid geometry, such as a zero length line, zero radius arc, or self-intersecting spline.

With SolidWorks it is not necessary to fully dimension or define your sketches before you use them to create features. However, you should fully define your sketches before you consider the part completed.

Note:	If you wish to always use fully defined sketches, you can set that option by clicking Tools, Options, and selecting the General tab. In the Sketch section, click Use fully defined sketches.

See also Sketch Geometry Status or Sketch Dimension or Relation Status .


Sketch Geometry Status

Sketch Geometry may have any of the following states:

•	Fully defined -- black. The dimensions and relations are fully and correctly described.

•	Under defined -- blue. The dimensions and relations are not defined adequately and lines may move or change size unexpectedly.

•	Over defined -- red. This geometry is constrained by too many dimensions and/or relations.

•	Dangling -- brown, dashed. Only applies to a sketch entity which was added automatically to the sketch in the last known position of the dangling model geometry.

•	Not solved -- pink. This geometry’s position cannot be determined using the current constraints.

•	Invalid -- yellow. This geometry would be geometrically invalid if the sketch were solved.

See also Fully Defined Sketches  or Sketch Dimension or Relation Status .


Sketch Dimension or Relation Status

Sketch Dimensions or Relations may have any of the following states:

•	Dangling -- brown, dashed. A dimension that can no longer be resolved (a dimension to a deleted entity, perhaps).

•	Satisfied -- black. A dimension that is completely and appropriately defined.

•	Over Defining -- red. The dimension or relation is involved in over defining one or more entities.

•	Not Solved -- pink. The dimension or relation results in not being able to determine the position of one or more sketch entities.

•	Driven -- gray. The dimension’s value is driven by solving the sketch.

See also Sketch Geometry Status or Fully Defined Sketches .


Geometric Tolerance

Inserts Geometric Distancing and Tolerance symbols in part, assembly, and drawing documents.

To insert geometric tolerances:

1	Click [image] or Insert, Annotations, Geometric Tolerance.

2	In the first Feature Control Frame area, click GCS, then select a Geometric Characteristic Symbol and click OK.

Notice that as you make each selection, the information appears in the preview display box.

3	Enter a tolerance value in the Tolerance 1 box, and click [image] if you want to include a Diameter symbol.

4	Click MC, to choose the material condition symbol for Tolerance 1 and click OK.

5	Repeat steps 3 and 4 for Tolerance 2.

6	Enter tolerance values and material condition symbols for the Primary, Secondary, and Tertiary datums.

7	Repeat the process for the second Feature Control Frame,

- or -

Click the Composite Frame check box and complete entering values and material condition symbols.

8	Click Between Two Points if the tolerance value applies to a measurement between two points or entities.

9	If you want to enter a Projected Tolerance Zone height, click the Show PTZ check box and enter a value in the Height box. The value is displayed in the first frame’s tolerance box.

10	To specify styles for leaders, arrows and/or fonts, click the Options button.

11	When you are finished, click OK and drag the geometric tolerance frame to the desired position on your document.


Geometric Tolerance Options

Make the following selections:

•	Display with Leader. Deselect if you do not want to display a leader with the geometric tolerance control frame.

•	Display with Bent Leader. Select if you want to display the geometric tolerance control frame with a bent leader. With this selected, you can also select an All Around leader.

•	All Around. Select this symbol to indicate that the profile tolerance extends all the way around the feature to which the tolerance applies.

•	Leader Anchor: Choose the location of the leader anchor from Closest, Left, or Right sides.

•	Arrow: Select an arrow style from the scroll box, or select None to display no arrow.

•	Click the Use Document’s Font check box to use the default font, or deselect Use Document’s Font and click the Font button to choose from various font styles and sizes.

When you are finished, click OK to save your selections and exit; click Cancel to exit without saving your selections.


Headers and Footers

Lets you specify headers and footers for the active document before printing.

To specify the headers and /or footers of a document:

1	Click File, Page Setup.

2	From the Header/Footer tab,

•	Scroll the Header and Footer boxes to select predefined headers and/or footers, and view your selection in the Preview boxes.

•	Click Custom Header or Custom Footer to define your own headers and/or footers.

3	Click OK.

See Custom Header and Footer .


Helix

Creates a helix curve in a part. The helix can be used as a path or guide curve for a swept feature, or a guide curve for a lofted feature.

To create a helix:

1	Open a sketch and sketch a circle. The diameter of this circle controls the diameter of the helix.

2	Close the sketch.

3	Select the circle.

4	Click Insert, Reference Geometry, Helix.

5	Select a definition from the Defined by scroll box: Pitch and Revolution, Height and Revolution, or Height and Pitch.  (To define a helix, you specify two values, and the third value is automatically calculated.)

6	Depending on the definition, specify values for Height, Pitch, and number of Revolutions.

7	To make a tapered helix, click the Taper Helix checkbox, specify the Angle of taper, and the direction of the taper (outward or inward).

8	If necessary, specify a Starting Angle for  the first turn of the helix.

9	Click Reverse to make the helix extend backward from the point of origin.

10	Click a radio button to choose the direction of the turns (Clockwise or Counterclockwise).

11	Click OK.


Help

Provides additional information about a SolidWorks function or option, online.

To access Solidworks online help, do one of the following:

•	Click [image] on the Standard toolbar.

•	Click Help on the menu bar to access help for SolidWorks and other add-in applications that you have installed, such as PhotoWorks.

Use the Table of Contents, the Index, or the Find word search tool to locate the topic for which you need help.

To get help about a specific dialog box:

•	Click the Help button in the dialog box.

•	With the dialog box active, press the F1 key.

To access the entire help system from the specific dialog box help, click the Help Topics button.


Hidden in Gray

Displays the model with all edges that are not visible from the current view angle in gray.

To display the model with hidden lines in gray:

Click [image] or View, Display, Hidden in Gray.

Tip	Click Tools, Options to change the hidden edge color (Color tab) or to display hidden edges as dashed lines (Edges tab).


Hidden Lines Removed

Displays the model with all edges that are not visible from the current view angle removed.

To display the model with hidden lines removed:

Click [image] or View, Display, Hidden Lines Removed.


Hide/Show Dimensions

Allows you to hide or display individual dimensions in a drawing.

To hide or display dimensions:

1	Select a drawing view that contains dimensions you want to display or hide.

2	Click View, Hide/Show Dimensions. All dimensions on the selected view are displayed; hidden dimensions are in gray.

3	Click the dimensions that you want to show or hide.

4	Click the Select tool or click View, Hide/Show Dimensions again to end selecting.


Hide/Show Components

Hides or displays components in an assembly. In a complex assembly, hiding some components temporarily may make the assembly easier to understand and work with.

To hide one or more component(s):

1	Select the component(s) in the FeatureManager design tree or in the graphics area.

2	Click [image] or Edit, Hide Component(s).

The component disappears from view and the related icon in the FeatureManager design tree is grey.

To show the hidden component(s):

1	Select the component’s name(s) in the FeatureManager design tree.

2	Click [image] or Edit, Show Component(s).

The component reappears and the related icon in the FeatureManager design tree is now in color.

To hide or show an individual component:

1	Right-mouse click a component in the graphics area or in the FeatureManager design tree.

2	Select Hide Component from the menu.

3	Right-mouse click the component’s name in the FeatureManager design tree.

4	Select Show Component from the menu.


Show with Dependents

In an assembly, displays selected hidden components and any dependents.

To show a hidden component(s) with dependents:

1	Select the component’s name(s) in the FeatureManager design tree.

2	Click Edit, Show with Dependents.

The component and its dependents reappears and the related icon in the FeatureManager design tree is now in color.


Hide View/Unhide View

Hides or shows individual views in a drawing.

To hide or unhide a drawing view:

1	Select the drawing view.

2	Right-click the view and select Hide or Unhide from the menu.

See also Show Hidden Views .


Hole

See Hole Wizard  and Simple Hole .


Hole Callout

Inserts a hole callout in a drawing view.

To insert a hole callout in a drawing view:

1	Click a hole edge to select it.

2	Click [image] or Insert, Annotations, Hole Callout.

A dialog box appears with the dimensions of the hole already filled in.

3	Make any additions or changes to the callout information that you think are necessary.

4	Click OK when you are satisfied, or click Cancel.

To move the callout text to a new location, click and drag the text.

To make changes to the arrow, font, dimension precision, or tolerances, right-mouse click the callout text and select Properties from the menu. Make the changes in the Dimension Properties dialog box.


Hole Wizard

Creates complex holes (countersunk, counterbore, tapered, holes with drill angles, etc.) and simple hole features.

To create a hole:

1	In a part, click on the model where you want to create the hole.

2	Click [image] or Insert, Features, Hole, Wizard.

3	Select the Type from the pull-down list:

Blind	Up to Vertex

Through All	Up to Surface

Up to Next	Offset from Surface

4	Specify the Depth or Offset, if necessary.

5	If the Type you specified relies on the selection of a surface, select that item now. The selection is indicated in the Selected Items box.

6	Click Next.

7	Select the style of hole you want to create.

8	Click Next.

9	Enter the appropriate dimensions.

10	Click Finish.


Hole Wizard  -  Step 2 of 3

1	Click the diagram of the type hole you want to make.

2	Click Next to go to the next step and specify the hole dimensions.

- or-

Click Back to return to the previous step; click Cancel to exit.


Hole Wizard  -  Step 3 of 3

1	Select a dimension that you want to change and enter a new dimension.

2	Press Enter and view the results in the preview box.

3	When all of the dimensions are satisfactory, click Finish.

- or-

Click Back to return to the previous step; click Cancel to exit.


Horizontal Break

Creates a broken view (or an interrupted view) on the drawing of a long part that has a uniform cross-section. This makes is possible to display the part in a larger scale on a smaller size drawing sheet

To create a break line in a drawing:

1	Select the drawing view and click Insert, Horizontal Break.

Two break lines appear in the view.

2	Drag the break lines to where you want the breaks to occur.

3	Right mouse click inside the view border (green border) and select Break View from the menu.

The part is displayed with a gap in the part geometry; however, the dimensional values associated with the broken area reflect the correct values.

You can continue to drag the break lines to adjust them after the view is broken, if necessary.

To change the shape of the break lines, right mouse click a break line and select a line style from the menu: Straight Cut, Curve Cut or Zig Zag Cut.

To specify the width of the break gap, click Tools, Options, and select the Detailing tab. Enter a value in the Break Gap box under the Break Lines option.

See also Vertical Break .


Horizontal Dimension

Creates a horizontal dimension between two points. (The horizontal direction is defined by the orientation of the current sketch.)

To create a horizontal dimension:

1	Click Tools, Dimensions, Horizontal.

2	Click the two points to dimension.

3	Click a location to place the dimension.


Horizontal Ordinate Dimension

Creates horizontal ordinate dimensions in a drawing, measured horizontally from the entity you select first.

To create horizontal ordinate dimensions:

1	With a drawing active, click [image] and select Horizontal Ordinate from the right-mouse menu.

– or –

Click Tools, Dimensions, Horizontal Ordinate.

2	Click the first item from which all others will be measured, and click again to place the dimension.

3	Click an item to dimension, then click to place its dimension. Repeat this step until all the remaining items are dimensioned. The dimension tool remains in ordinate mode until you select another mode or another tool.

See also  Align Ordinate   , Ordinate Dimension , Vertical Ordinate Dimension , Add to Ordinate Dimension .


Insert Hyperlink

Creates a hyperlink to a document on the Internet, your local network, or on your own hard drive. Selecting the hyperlink brings the user to the associated URL (document or web site).

To embed a hyperlink:

1	Click [image] or Insert, Hyperlink.

2	Enter the path (or browse) to the document to which you want to link.

3	Click OK to accept the path.


IGES Out Selection

1	Click Complete Body to export a solid body as an IGES file,

- or -

click Selected Faces to export only those surfaces that you have selected.

2	Click OK to complete exporting to an IGES file; click Cancel to exit without exporting the file.


IGES Settings

Select an export format from the list.

Click OK to complete the format selection; click Cancel to exit.


Insert Model Annotations

Imports to the selected drawing view, annotations that currently exist on the model.

To import existing annotations to a drawing view:

1	Select a drawing view.

2	Click Insert, Model Annotations.

3	From the Insert Annotations dialog, select any of the annotation types that you want to import:

Cosmetic Threads

Datums

Datum Targets

Dimensions

Geometric Tolerances

Notes

Surface Finish Symbols

Weld Symbols

- or -

Click the All Types checkbox to import all of the annotations available for that view.

Note:	If you select Dimensions, you have the option of also importing Instance/Revolution Counts if those dimensions exist in the part or assembly.

4	From the Import From box, select one of the following options:

•	Entire Model. Displays all of the selected annotation types that exist in the model.

•	Selected Component. If this drawing is of an assembly, displays the annotations that exist on the selected component only.

•	Selected Feature. Displays the annotations existing on the selected feature only.

5	Click OK to insert the annotations; click Cancel to exit without making the changes.

Attachment points of imported annotations can be dragged, but not re-attached to another edge, face, vertex, etc.

Note	Imported annotations display in the default Imported Annotation color; reference annotations (added in the drawing) are displayed in the default Reference Annotation color. These colors are specified in Tools, Options, on the Color tab. See Color -- Lines, Text, and Borders .


Interference Detection

Checks to see whether portions of any two components in an assembly occupy the same space. The volume of interference is graphically displayed as highlighted edges showing the over-lapping portions of the components. (One volume of interference is displayed at a time.)

To check for interference in an assembly:

1	Hold the Ctrl key and select two components in the assembly.  Alternately, you can select the assembly or sub-assembly(ies) from the FeatureManager design tree.

2	Click Tools, Interference Detection.

The Interference Volumes dialog opens and the Selected Components list displays the names of the selected components.

3	Click the Coincidence as Interference checkbox if you want to consider coincidence as interference. Note:  Coincidence is the overlapping of two entities, such as a bounded plane on another bounded plane.

If there is interference,

•	The names of the components are reported in the Component 1 and Component 2 boxes

•	The interference name (Interference1, Interference 2, and so on) is reported in the Interference List. When you click an interference name, the related interference volume is highlighted in the graphics display area.

•	The volume of the interference is reported in the form of length, width, and height of the bounding box around the area of interference. These numbers are displayed on the graphic display of the component.

3	With the dialog box still active, you can reselect other components to check for interference.

4	Click Recheck to see if the newly selected components interfere.

5	Click Close to dismiss the dialog box.

When the dialog box is dismissed, the volumes are dismissed also.


Interference Volumes

Checks to see whether portions of any two components in an assembly occupy the same space.

You can decide if you want to consider coincidence as interference by clicking the Coincidence as Interference checkbox. Note:  Coincidence is the overlapping of two entities, such as a bounded plane on another bounded plane.

The Interference List displays each case of interference between two components in the assembly: Interference1, Interference 2, and so on. If no names are listed, there is no interference.

1	Click the name of an interference (Interference1, for example).

The names of the two over-lapping components in Interference1 are displayed in the Component 1 and Component 2 boxes, and the volume of interference is graphically displayed as highlighted edges that show the over-lapping portions of the components. (One volume of interference is displayed at a time.)

2	With the dialog box still active, you can reselect other components to check for interference.

3	Click Recheck to see if the newly selected components interfere.

4	Click OK to dismiss the dialog box.


Open Internet Address

Allows you to specify a Web site or document to view.  If the specified path is to a local SolidWorks document, it will be retrieved into the SolidWorks application. Other documents and Web sites will come up in your default Internet browser.

To open an Internet link:

1	Click [image] on the Web toolbar.

2	Type the address of the document, folder, or computer on the Internet, or click the Browse button and browse to the document or location that you want.

3	Click OK to continue to open the Internet address; click Cancel to end the operation and close the dialog box.


Jog

Allows the arrangement of ordinate dimensions for better viewing when ordinate values are clustered too closely. You can select individual dimensions and pull them to a more visible position. The leader line develops a jog, or bend, so it can be easily seen and still be aligned with other dimensions in the ordinate.

To arrange ordinate dimensions:

1	Right-click an ordinate dimension value and select Jog from the menu.

2	Drag the dimension in any direction.

•	The leader line has a jog in it that allows you to place it freely.

•	The menu item is checked. Selecting Jog again returns the dimension to its original place and unchecks the menu item.

3	Use the Align Ordinate command to align all the dimensions in the ordinate.


Join

Creates a new part by joining two or more parts. The Join operation removes surfaces that intrude into each other’s space and creates a single solid volume.

You create a joined part by editing a new part in the context of an assembly.

To join parts:

1	Create the parts that you want to join. Save and name the individual part files.

2	Create an assembly and insert the parts as assembly components.

3	Position and mate the components so that they touch or intrude into one another. The components should form the configuration that you want for the resulting part.

4	Save the assembly, but do not close the assembly window.

5	Click Insert, Component, New to insert a new part into the assembly, name and Save it. You are editing this new part to create the joined part.

6	Click a planar face on one of the components.

7	Click Insert, Features, Join. The Join dialog box appears.

8	In the FeatureManager design tree or the graphics window, click the parts that you want to join. The names appear in the Design Component list.

9	Click Hide Input Components if you want to hide the original components in the assembly document. (See Hide/Show Components for more information.)

10	Click Extend Smallest Abutting Faces if you want to join parts that just touch each other.

11	Click OK, and Save the part.

12	Exit Edit Part by selecting Edit Assembly from the right-mouse menu or by clicking [image].

Changes that you make to any of the original parts are reflected in the joined part. See also Editing a Joined Part.


Editing a Joined Part

To edit a joined part:

1	In the FeatureManager design tree, right-click the Join feature of the joined part and select Edit Definition.

The Join dialog box appears. Joined parts are listed in the Design Component box.

2	In the FeatureManager design tree, Ctrl-click the part you want to remove from the joined component, or select new components to be joined to the existing component.

3	Click OK.


Library Feature

Lets you build a collection of features to insert into parts that you create.

To create a library feature:

1	In a new part file, create one or more features.

2	Select the feature(s) that you want to save in the library. Select the feature(s) either in the FeatureManager design tree or in the graphics area.

3	Click File, Save As.

4	In the Save As dialog box, select Lib Feat Part Files (*.lfp) from the Save As Type menu.

5	Enter a name for the part and click Save.

To add a library feature to a part:

1	With a part open, click Insert, Library Feature. The part can be empty or it can contain an extruded base and other features.

2	In the Insert Library Feature dialog box, select the library feature to be added and click Open.

The Insert Library Feature Wizard appears along with the library feature window and the part window.

3	Select the place on the part where you want to insert the library feature.

- or -

In an empty part, select the plane where you want to place the library feature.

Note:  When you make an acceptable choice for the placement of the library feature, a green checkmark appears in the Reference region of the Insert Library Feature wizard.

4	If you are satisfied, click OK. Otherwise, click Deselect All or Cancel.

Note:	You cannot place a library feature that is a Base extrusion in a part that already has a Base extrusion. When creating your library feature, you can first make a base extrusion on which to create the library feature.


Insert Library Feature Wizard

1	Select the place on the part where you want to insert the library feature.

- or -

In an empty part, select the plane where you want to place the library feature.

Note:  When you make an acceptable choice for the placement of the library feature, a green checkmark appears in the Reference region of the Insert Library Feature wizard.

2	If you are satisfied, click OK. Otherwise, click Deselect All or Cancel.

Note:	You cannot place a library feature that is a Base extrusion in a part that already has a Base extrusion. When creating your library feature, you can first make a base extrusion on which to create your library feature.


Lighting

Adjusts the direction, intensity, and color of light in a shaded view.

To adjust lighting in a shaded view:

1	Click View, Lighting.

The Light Sources dialog opens with an Ambient light page and a Directional light page already in place. Additionally, you may select more Directional Light and Spot Light sources.

2	To add light sources, click the Add Direction or Add Spot buttons located at the bottom of the dialog box. (You may use a maximum of eight light sources in addition to the ambient light source.)

For each new light source a tabbed page is created on which you can define the characteristics of that light source. Move between the tabbed pages by clicking their tabs.

3	For directional light source pages, adjust the slider bars to specify the amount of directional light striking the model surface from positions X, Y, and Z, and move the slider to the right to increase  the effect of each of the following light source characteristics:

Ambient , Diffuse Light , and  Specular .

4	For spot light source pages, set the direction from which the light arrives and its intensity by  adjusting the slider bars to specify the amount of spot light striking the model surface from positions X, Y, and Z, and specify the following light source characteristics:

Exponent , Attenuation , Distance , and Cutoff .

5	Click Apply to see the changes as you make them. (It is best to experiment with the values until you get the results that you want.)

6	Click OK to save the changes; click Cancel to end the session without saving the changes.

The command buttons on the Light Sources pages:

•	Edit Color. Defines the color of the light striking the model surface. Select a color from the color palette or click Define Custom Color to create a custom color.

•	Use as default. Preserves the Direction, Ambient, Diffuse, and Specular settings as the default settings for new models. (Not available for Spot Light.)

•	Delete. Removes the current light source page from the dialog box. (Not available for Ambient.)

•	Disable. Click this checkbox to disable the light options and characteristics of the current page.

See also Shaded .


Line

Creates a line.

To create a line:

1	Click [image] or Tools, Sketch Entity, Line.

2	Point where you want the line to start.

3	Press the mouse button and drag to where you want the line to end.

4	Release the mouse button.


Linear Pattern

Creates multiple instances of selected features along one or two linear paths. You can specify the direction(s), the number of instances in each direction, and the distance between them.

If you modify the original feature, all instances in the pattern are updated to reflect the changes.

To create a linear pattern in one direction:

1	Click Insert, Pattern/Mirror, Linear Pattern.

2	In the Linear Pattern dialog, select First Direction, then click a model edge or a dimension to indicate the first direction for the pattern.

If the arrow that appears on the model is pointing in the wrong direction, click Reverse Direction.

3	In the FeatureManager design tree or the model, select the feature(s) that you want to copy. (If you are selecting more than one feature to copy, hold the Ctrl key while selecting.)

4	Set the appropriate values for Spacing and Total Instances. As you modify the values, a preview of the pattern is displayed.

5	Click Vary Sketch if you want the pattern to change as it is repeated. See Vary Sketch for more information.

6	Click OK.

To create the pattern in two directions:

1	Follow Steps 1 through 5 as described above.

2	Select Second Direction, then click a model edge or a dimension to indicate the second direction.

3	Set the appropriate values for Spacing and Total Instances for Direction 2.

4	Click OK.

To delete pattern instances, see Pattern Deletion .

See also Circular Pattern .


List Named Entities

Faces and edges that are named can be listed and highlighted in the model. You can specify entity names manually, or you can let the system generate them for you automatically. Automatic naming can occur when you use a face or edge either:

•	As an external reference in another part

•	To create a mate in an assembly

See Entity Property for information about manually naming faces and edges.

To automatically name model faces and edges:

On the External References tab of the Options dialog box, click Automatically generate names for referenced geometry.

Thereafter, whenever you use a face or edge as an external reference or in a mate, it is named. The name consists of the entity type and an incremental number, such as Face1, Face2, etc.

Note:    This option is OFF by default, and should be used with caution in a multi-user environment. See External References for more information.

To list and highlight named model entities:

1	In the part window, right-mouse click on the part name at the top of the FeatureManager design tree, and select List Named Entities.

2	Click an entity name in the list. The corresponding entity on the model is highlighted.


Named Entities

Click an entity name in the list to highlight the corresponding entity on the model.


Loft

1	Select the profile sketches in order in the FeatureManager design tree or the graphics window.

The sketches are listed in the Profiles box, and a preview curve connecting the selected entities is displayed.

2	If you are using guide curves, click the Guide Curve(s) box, then select the guide curve sketch(es).

3	Examine the path preview. If necessary, use the Up or Down buttons to adjust the order, or reselect the sketches to connect different points on the profiles.

4	Click Close Along Loft Direction to create a closed body along the loft direction. This connects the last sketch and the first sketch automatically.

5	Click Maintain Tangency to cause the surfaces in the resulting loft to be tangent if the corresponding segments are tangent.

6	Click Advanced Smoothing to obtain smoother surfaces. This option is available only if the loft sections have circular or elliptical arcs.

7	Click OK to create the loft, or click Cancel.


Loft Feature

Creates a feature that adds or removes material by connecting multiple cross sections.

To create a loft feature:

1	Set up the planes needed for the cross sections. (You can use existing faces and planes, or create new planes. The planes do not have to be parallel.)

2	Sketch each section on a different face or plane.

3	If you are creating the first feature in a new part, click Insert, Base, Loft. Otherwise, click Insert, Boss, Loft or Insert, Cut, Loft.

4	Select the sketches in order, picking a corresponding point on each cross section. You do not have to select the vertices precisely; the vertex closest to the selection point is used.

The sketches are listed in the Profiles box, and a preview curve connecting the selected entities is displayed.

5	If the preview curve looks wrong:

•	Use the Up or Down buttons to rearrange the sketches if they are in the wrong order.

•	If the wrong vertices are connected, click the profile once to deselect it, then click again to select a different point on the profile.

•	To clear all selections and start over, right-click in the graphics area, select Clear Selections, and try again.

6	Click Close Along Loft Direction to create a closed body along the loft direction. This connects the last sketch and the first sketch automatically.

7	Click Maintain Tangency to cause the surfaces in the resulting loft to be tangent if the corresponding segments are tangent.

8	Click Advanced Smoothing to obtain smoother surfaces. This option is available only if the loft sections have circular or elliptical arcs.

See also Guided Curve Loft .


Guide Curve Loft

You can make a loft with one or more guide curves.You position the loft profiles along the guide curve(s) at points where you want a profile change to take place.

To make a loft with guide curves:

1	Sketch the profiles.

2	Sketch one or more guide curves, or create reference curves to use as guide curves.

3	In the profile sketches, add relations between the guide curve(s) and the profiles. Use pierce or coincident relations between the guide curve(s) and vertices or sketch points on the profile.

4	If you are creating the first feature in a new part, click Insert, Base, Loft. Otherwise, click Insert, Boss, Loft or Insert, Cut, Loft.

5	Click the Profiles box, then select the profile sketches in order in the FeatureManager design tree or the graphics window.

The sketches are listed in the Profiles box, and a preview curve connecting the selected entities is displayed.

6	Click the Guide Curve(s) box, then select the guide curve sketch(es).

7	Examine the path preview, and use the Up or Down buttons if necessary to adjust the order.

8	Click Close Along Loft Direction to create a closed body along the loft direction. This connects the last sketch and the first sketch automatically.

9	Click Maintain Tangency to cause the surfaces in the resulting loft to be tangent if the corresponding segments are tangent.

10	Click Advanced Smoothing to obtain smoother surfaces. This option is available only if the loft sections have circular or elliptical arcs.

11	Click OK.

See also Notes on Creating Lofts with Guide Curves .


Notes on Creating Lofts with Guide Curves

•	The first or last section can be a point.

•	Guide curves must pass through the sketched profiles, either at the vertices or at user-defined sketch points on the profile. The guide curve splits edges of the profiles where the guide curve intersects the profile.

•	There is no limit on the number of guide curves you may use.

•	Guide curves can intersect at a sketch point or the apex of the lofted surface.

•	You can use sketched curves, model edges, or reference curves of any kind as guide curve(s).

•	If a simple loft fails or twists, it is recommended that you add a Curve Through Reference Points  as a guide curve, selecting corresponding vertices of the profiles to create the curve.

•	Guide curves can be longer than the resulting loft. Only that portion of the curve that is needed is used.

•	You can control the behavior of the loft by creating the same number of segments on all the guide curves. The end points of each segment mark corresponding points for transition of the profiles.


Make Dimension Driven?

The highlighted dimension has made the sketch over defined or unsolvable.  Select one of the following options:

•	Make This Dimension Driven  (The overdefined or unsolvable state is repaired.)

•	Leave This Dimension Driving   (The sketch remains overdefined or unsolvable. Look for other dimensions or relations that you can delete or change.)


Make Section Line

Converts a sketched line (or lines) on a drawing into a section line which can be used to create a section view. (See Section.)

To make a section line:

1	Double click the drawing view where you want to draw the section line. (This activates the view so you can draw on it.).

2	Click [image] or Tools, Sketch Entity, Line and draw the section line. You can draw connected lines.

3	Click [image] and select the line(s).

4	Click Insert, Make Section Line. This converts the selected line(s) into a section line, with arrows showing which direction the view will face.

5	To change the section line label or the direction of the view, select the line and click Edit, Properties. (Double-clicking the section line will also reverse the direction.)


Mass Properties

Displays the density, volume, surface area, center of mass, and inertia tensor of the model.

To display the mass properties of a model:

1	Click Tools, Mass Properties.

•	You can print the mass property results directly from the dialog box.

•	You can select and copy the text to the clipboard for pasting into another document.

2	Click Close to close the dialog box.


Mate

Mates components in an assembly.

To mate components in an assembly:

1	Select the desired faces, edges, vertices, or reference planes on the components.

2	Click [image] on the Assembly Tools toolbar or select Insert, Mate.

The Assembly Mating dialog box appears. To keep the dialog in place while you are working, click the push pin icon [image].

The entities and components that you selected for mating are listed in the Items Selected window. Examine the list to make certain that it is correct; scroll horizontally to see the entire list, if necessary.

3	Select the desired Mate Type and Alignment Condition. (Only those types and conditions that are valid for the selected features are available.)

4	In the Workbench area, click Preview. The parts move to the mating relation that you specified.

5	If this mating relation is acceptable, click Apply; if not, click Undo and try again.

6	When you are satisfied, close the dialog box.

To change the mating relation, click the name of the mate in the FeatureManager design tree, and select Edit Definition. Make your changes in the Assembly Mating dialog box.

See also Edit Mating Relations .


Material Condition

Inserts a material condition symbol into the Current Work Sheet in the Geometric Tolerance dialog.


Measure

Measures distance, angle, radius, and size of and between lines, points, surfaces, and planes in sketches, 3D models, assemblies, or drawings.

To use the measure tool:

1	Click Tools, Measure.

The Measure dialog box appears.

2	To keep the dialog box in place while you are working, click the push pin icon [image].

Note:  While the Measure dialog is in place, you can switch between different documents without closing the dialog. The name of the currently active document displays near the top of the Measure dialog box. If you activate a document that has items already selected, the measurement information updates automatically.

3	To turn the Measure function on or off, click the switch [image] in the corner of the dialog box.  (You can turn Measure off while you do other work on your part or assembly.)

While the Measure function is ON, the cursor is a ruler [image] with which you can select entities to measure.

4	In the Projection On region, select Screen to measure the projection on the screen, or click Plane/Face to measure the projection on a selected plane or planar face. (When Plane/Face is selected the ruler icon has a small plane attached.)

5	Select the items to measure with the ruler cursor.

The selected items appear in the Selected Entities list box, and appropriate values are displayed in the Measurements box.  New measurements update dynamically when you change selections.

If the combination of selected entities does not make sense for the measure function, the Measurements box is blank.

6	To delete an item from the Selected Entities list box, click the item’s name in the list and press the Delete key, or click the selected item again in the graphics area.

To clear all items from the Selected Entities list box, click away from the part or assembly in the graphics area.

7	Click Close to close the dialog box.


Mirror All

Creates a symmetrical part by mirroring an existing half around a planar face.

To mirror a part around a planar face:

1	Select a planar face on a part.

2	Click Insert, Pattern/Mirror, Mirror All.

A mirror image of the original part is joined to it at the selected face to make a whole part.

See also Mirror Part , Mirror Feature , Mirror Sketch Elements


Mirror Sketch Elements

Creates copies of sketch elements which are mirrored around a centerline.

When you create mirrored elements, SolidWorks applies a symmetric relation between each corresponding pair of sketch points (the ends of mirrored lines, the centers of arcs, and so on). If you change a mirrored element, its mirror image will also change.

To mirror existing items:

1	In a sketch, click [image] and draw a centerline.

2	Hold down the Ctrl key and select the centerline and the items you want to mirror.

3	Click [image] or Tools, Sketch Tools, Mirror.

To mirror items as you sketch them:

1	Select a centerline to mirror about.

2	Click [image] or Tools, Sketch Tools, Mirror. M’s appear at both ends of the centerline to indicate that automatic mirroring is active.

3	Sketch curves. The elements you draw will be mirrored automatically as you draw them.

4	To turn mirroring off, click [image] again.

See also Mirror Part , Mirror Feature , Mirror All .


Mirror Feature

Creates a copy of a feature (or multiple features), mirrored about a plane.

If you modify the original feature, the mirrored copy is updated to reflect the changes.

To mirror a feature:

1	Select a feature (or features) in the model or in the FeatureManager design tree.

2	Hold down the Ctrl key and select a plane or a face.

3	Click Insert, Pattern/Mirror, Mirror Feature.

See also Mirror All , Mirror Part , Mirror Sketch Elements


Mirror Part

Creates a new part that is the reverse of a previously constructed (and saved) part.

If you modify the original part, the mirrored copy is updated to reflect the changes. If you add features to the mirrored copy, the original part is not updated to reflect the changes.

To create a mirror part:

1	With a part document open and saved, pick a face or plane about which to mirror the part.

2	Click Insert, Mirror Part.

A new document is created with the mirrored geometry.

See also Mirror All , Mirror Feature , Mirror Sketch Elements .


Modify

Use the scroll arrows to change the value

- or -

enter a new value in this field.


Modify Sketch

Allows you to move, rotate, or scale a sketch.

To move or rotate a sketch:

1	Open a sketch or select a sketch in the FeatureManager design tree, and click [image] or Tools, Sketch Tools, Modify.

2	In the Translate region of the Modify Sketch dialog, you can enter incremental values in the X value and Y value boxes, and then press Enter. Click Position Selected Point if you want to select a point on the sketch and move that point to the specified absolute coordinates.

3	In the Rotate region of the Modify Sketch dialog, you can enter a specific rotation value, and then press Enter.

- or -

You can use the mouse cursor to move and rotate, as follows:

•	Press the left mouse button to move the sketch.

•	Press the right mouse button to rotate the sketch around the black origin symbol.

•	Point at the end points or center of the black origin symbol to display one of three  “flip” symbols on the right mouse button.  Press the flip symbol to flip the sketch on the X axis, the Y axis, or both.

•	Point at the center point of the black origin symbol, to display a point symbol on the left mouse button. Press the left button to move the center of rotation independently of the sketch.

Note	You cannot move a sketch if it has external references. (The mouse cursor has a ? on the left button.)

To scale a sketch:

Enter a decimal value in the Scale box, and press Enter.

Scale applies a uniform scale about the origin of the sketch.

Note	You cannot scale a sketch if it has external references.


Move Component

Moves an underdefined component in the assembly window.

To move with the mouse:

1	Click the component to select it.

2	Click [image] on the Assembly toolbar, or click Tools, Component, Move.

3	Hold the mouse button down and drag in the direction you want to move the component.

4	To move a different component, click its name in the FeatureManager design tree and drag it.

5	Click the Move Component tool again when finished.

See also Rotate Component Around Centerpoint and Rotate Component Around Axis .


Modify Perspective

Perspective in the real world, as well as in SolidWorks, is related to the size of the object being observed and the distance of that object from the observer. You can modify the perspective by specifying the Object sizes away value in the Perspective Information dialog box. The smaller the value, the greater the amount of perspective distortion.

To change the perspective:

1	With Perspective selected, click View, Modify, Perspective.

2	Specify the Observer Position by scrolling the Object sizes away value or by entering a value.

3	Click OK.

See also Perspective .


Modify Text of Dimension

Modifies the text of a dimension in a drawing.

The dimension value is represented by <DIM> in the middle box.

To change the text of a dimension:

1	Place the cursor in the Dimension Text box where you want to make changes. You can make the following changes:

•	Add text or symbols before or after the dimension <DIM> (in the middle box).

•	Add text or symbols above or below the dimension (in the upper or lower boxes).

•	Delete the dimension.

2	To add a symbol, place the cursor in the text box where you want the symbol to appear and click Add Symbol.

3	Select a library from the Symbol Libraries list.

4	Select a symbol name from the list, and click OK.
(The symbol’s name displays in the Dimension Text box, but the actual symbol appears in the Preview box and in the drawing.)

5	To replace the dimension value if it was deleted, click Add Value.

6	Click OK.


Pan

Scrolls the part, assembly, or drawing in the document window.

To scroll with the mouse:

1	Click [image] or View, Modify, Pan.

2	Hold the mouse button down and drag in the direction you want to scroll.

To scroll with the arrow keys:

Hold down the Ctrl key and press the Arrow keys.


Named View

Creates a drawing view with the same orientation as one of the named views in a model.

To create a drawing view to match a model view:

1	Open a drawing and a part or assembly.

2	Click [image] or Insert, Drawing View, Named View.

3	Click anywhere in a part or assembly window.

4	Select a view from the list and click OK. You can choose the current view or any named view.

5	Click in the drawing where you want to place the view.


New

Creates a new document.

To create a new part, drawing, or assembly document:

1	Click [image] or File, New, or press Ctrl-N.

2	Select either Part, Drawing, or Assembly from the list and click OK.

3	If you selected Drawing, select the template you want to use (or None) and click OK.


New Component

Creates a new component and adds it to the active assembly.

To create a new part in an assembly:

1	With an assembly active, click Insert, Component, New.

2	Enter a name for the new part in the Save As dialog and click OK.

3	In the assembly window, click a plane or face where you want to place the new part. Plane 1 of the new part will be coincident to the selected plane or face.

If the assembly is an empty document, select a plane from the FeatureManager design tree.

The sketch grid appears and the Sketch Tools and Sketch Relations toolbars are active. You are now editing a sketch on Plane1 of the new part, in the context of the assembly.

4	Sketch and dimension the new sketch.

5	Click Insert, Base, Extrude (or Revolve) to create the base feature of the new part. Use any other of the part feature commands from the Insert menu as needed, such as Boss or Cut, or something from the Features menu, such as  Fillet/Round, Chamfer, and so on, to build the part.

6	When the part is finished, click [image] or right-click in the assembly window, and select Edit Assembly to leave Edit Part mode.

The new part appears in the assembly. Its position is fully defined by an InPlace mate to the face or plane on which you created it.

Note: The default color for the new part, or a part being edited, is salmon pink if the part is in Shaded view; the default color for non-editable parts in an assembly is gray.


New Window

Creates a new window for viewing the active part, assembly, or drawing.

To open another view in a new window:

1	Click Window, New Window.

2	Adjust the size and location of the new window, as desired. (To hide the FeatureManager design tree in the new window, drag the right edge of the FeatureManager design tree to the left edge of the window.)

Note that this window is just another view of the same document. You can set the zoom, rotation, and view mode (wireframe, hidden removed/gray, or shaded) for each window independently, but any changes you make to the model will be reflected simultaneously in both windows.


Next Sheet

Displays the next sheet in a drawing.

To view the next sheet in a drawing:

Click View, Next Sheet, or click on the sheet tabs at the bottom of the drawing window.


Note

Inserts a note into a part, assembly, or drawing document. You may create a free-floating note or a note with a leader line attached to a specific point on the document.

Notes can have multiple leaders .  You can select any number of attach locations and create the note.  Also, you can add, remove, and move leaders of existing notes.

Also used for Customizing Drawing Templates .

To create a note:

1	On a document, click where you want to place the note.

Note	If you choose to attach a leader line, the leader will attach where you clicked.

2	Click [image] or Insert, Annotations, Note.

3	Type the text into the Note Text box.

4	Specify the text angle in the Angle box, or use the spinbox arrows to set the value.

5	If you want to use the font you selected in Tools, Options, Detailing for note text, leave Use Document’s Font checked.

If you want to use a different font, deselect Use Document’s Font, and click the Font button to choose from various font styles and sizes.

6	Specify the Leader display:

•	Display with Leader. Attaches the note with a straight leader line.

•	Display with Bent Leader. Attaches the note with a bent leader line.

•	Leader Anchor. Choose a default position: Closest, Left, or Right.

•	Arrow Style. Choose Open, Filled, or Simple arrowheads, Open or Filled dots, Slash, or None (for leader arrows).

7	Specify the Balloon display:

•	Style. Specifies the shape of the balloon, or None.

•	Size. Specifies either Tight Fit to the text, or a fixed size to accommodate a specified number of characters.

8	To add a symbol to the note text, click the cursor in the Note Text box where you want the symbol to appear and click Add Symbol.

Select a library from the Symbol Libraries list, then select a symbol name from the list, and click OK.
(The symbol’s name displays in the text box, but the actual symbol appears in the note.)

9	Click [image] if you want to include a Hyperlink in the note.

10	Click OK.

See also Geometric Tolerance , Balloon , Cosmetic Threads , Datum Feature Symbol , Datum Target Symbol , Surface Finish Symbol , Weld Symbols .


Offset Entities

Creates sketch curves offset from a selected edge, loop, face, external sketch curve, external sketch contour, set of edges, or set of external sketch curves by a specified distance.

 SolidWorks creates an Offset Entity relation between each original entity and the corresponding sketch curve. If the entity changes when you rebuild the model, the offset curve also changes.

To create a sketch curve offset from a model edge:

1	In a sketch, select a face or one or more connected edges.

2	Click [image] or Tools, Sketch Tools, Offset Entities.

3	Set the value in the Offset box.

4	If necessary, select Reverse to change the direction of the offset.

5	Click OK.

You can now use the offset curve to extrude a cut or a boss.

To change the size of the offset:

Change the amount of the offset by double-clicking the offset’s dimension and changing the value.


Offset Surface

Creates an offset surface from the selected surface on a model.

To create an offset surface:

1	Click Insert, Reference Geometry, Offset Surface.

2	Select the model surface(s) from which to create an offset. (Hold the Ctrl key if you are selecting more than one face to offset.)

In the Offset Face dialog box, the Items to Offset box shows the number of selected faces.

3	Specify an offset value in the Offset box.

A preview of the offset is displayed.

4	If the offset is in the wrong direction, click Reverse.

5	When you are satisfied, click OK.

For more about using surfaces, see Thicken Feature and With Surface .


Offset Face

1	Select the model surface(s) from which to create an offset.
(Hold the Ctrl key to select more than one face.)

The Items to Offset box lists the number of selected faces.

2	Specify an offset value in the Offset box.

A preview of the offset is displayed.

3	If the offset is in the wrong direction, click Reverse.

4	When you are satisfied, click OK.


Extruded Surface

Extrudes a reference surface from a sketched profile.

To extrude a surface:

1	Sketch the profile of the surface.

2	Click Insert, Reference Geometry, Extruded Surface.

3	In the Extrude Feature dialog box, on the End Condition tab, choose the Type, and specify the Depth.

4	Examine the preview. If the offset is in the wrong direction, click Reverse Direction.

5	Click OK.

See also Extrude .

For more about using surfaces, see Thicken Feature and With Surface .


Revolved Surface

Creates a reference surface by revolving a profile around a centerline.

To revolve a surface:

1	Sketch a profile and a centerline around which to revolve the profile.

2	Click Insert, Reference Geometry, Revolved Surface.If the profile is open, you will be asked if you would you like the sketch to be automatically closed.

3	Click Yes to create a closed profile, or No to leave the profile open.

4	Enter the value for Degrees, and click Reverse Direction if necessary.

5	Click OK.

See also Revolve .

For more about using surfaces, see Thicken Feature and With Surface .


Swept Surface

Creates a reference surface by sweeping a profile along a path.

To sweep a surface:

1	Sketch the guide curves (if any are needed) and path for the swept surface on model faces, or create planes as needed for sketching.

2	Sketch the sections of the surface, and create coincident/pierce relations between the guide curve(s) and the section.

3	Click Insert, Reference Geometry, Swept Surface.

4	Click the Sweep Section box, then click the profile sketch.

5	Click the Sweep Path box, then click the path sketch, curve, or model edge for the path.

6	If you are using guide curves, click the Advanced tab. Click the Guide Curves box, then click the sketch, curve, or model edge for the guide curve(s).

7	Select options as desired under Orientation/Twist Control, Advanced Smoothing, and Maintain Tangency.

8	Click OK.

See also Sweep .

For more about using surfaces, see Thicken Feature and With Surface .


Lofted Surface

Creates a reference surface by connecting multiple cross sections.

To loft a surface:

1	Sketch the profiles (cross sections) and the guide curves (if any are needed) for the lofted surface.

2	Click Insert, Reference Geometry, Lofted Surface.

3	Click the profiles in the order in which you want them to be connected. Select corresponding segments on each profile; the vertex closest to the selection point is used to connect the profiles.

4	If you are using guide curves, click the Guide Curves box in the Loft Surface dialog, then select the guide curves.

5	Choose from the options Maintain Tangency, Close along Loft Direction, and Advanced Smoothing as desired.

6	Click OK.

See also Loft Feature .

For more about using surfaces, see Thicken Feature and With Surface .


Parallel Dimension

Creates a dimension between two parallel lines or a line and a model edge.

To create a parallel dimension:

1	Click Tools, Dimensions, Parallel.

2	Click the two parallel lines or a line and a parallel model edge.

3	Click a location for the dimension.


Object

Embeds an OLE object from another program into the active document. You can either open another program from within SolidWorks and create a new object or insert an existing file.

To create a new OLE Object:

1	Click Insert, Object.

2	Click Create New.

3	In the Object Type box, click the type of document you want to create (for example, Microsoft Excel Worksheet.) Only documents from OLE-compliant applications that are installed on your computer appear in the list.

4	Select the Display as Icon check box if you want the new object to appear as an icon in your document.

5	Click OK. A new document will appear inside your active document. The toolbars and menus for this new document will appear in place of the SolidWorks toolbars and menus.

(If you chose Display as Icon, an icon will appear in your SolidWorks document, and the parent application will open in another window.)

6	Edit the object as though you were working in the parent application.

7	When you are finished editing, click in the SolidWorks document window anywhere outside the embedded object. The SolidWorks toolbars and menus will become available again.

(If you chose Display as Icon, click File, Close or File, Close and Return in the parent application.)

To insert an existing file as an OLE object:

1	Click Insert, Object.

2	Click Create from File.

3	Click Browse, locate the file you want to insert, and click Open.

4	Select the Display as Icon check box if you want the new object to appear as an icon in your document.

5	By default, the contents of the file are saved as part of your SolidWorks document. Select the Link check box if you want to insert a picture of the file contents into your SolidWorks document. The picture will be linked to the original document, and changes made to the original file will be reflected in your document.


Offset Plane

To create a plane parallel to a plane or face, offset by a specified distance:

1	Select a plane or a planar face.

2	Specify the offset Distance.

3	Click Reverse Direction, if necessary.

4	Click Finish.


On Surface Plane

To create a plane on an angular surface:

1	Select a surface.

2	Select a plane that intersects that surface and an edge which passes through the plane.

3	If no solution is displayed, you will also need to select an edge on that surface.

4	Click Other Solutions, if necessary.

5	Click Finish.


Open

Opens an existing part, drawing, or assembly document. Also used to import files from other applications.

To open an existing file:

1	Click [image] or File, Open, or press Ctrl-O.

2	In the Open dialog box, browse through the directory structure to find the part, drawing, or assembly file that you want to open.

3	Click Open as read-only if you do not want to change or save the part.

4	Click Preview if you want to view the SolidWorks part, assembly, or drawing document without opening it.

5	Click Configure to open a specific configuration of a part or assembly.

6	Click References to see a list of the part and/or assembly documents referenced by the currently selected part, assembly or drawing. You can edit the locations of the listed files.

7	Click Open to open the document; click Cancel to exit without opening a file.

You can open existing SolidWorks files or you can select other file types to import into SolidWorks. For example, you can open IGES files as SolidWorks models, and DXF and DWG files as SolidWorks drawings.

See also Open DXF/DWG File


Open DXF/DWG File

Opens an imported DXF or DWG drawing file using the template size and units of measure that you specify.

To open a DXF or DWG drawing:

1	Click File, Open and select the filename. (In the Open dialog, be sure that the List Files of Type box displays either *.* or the appropriate file type.)

SolidWorks derives information from the incoming file and reports the sheet size and the units of the imported drawing.

2	Make any changes that are necessary and click OK.

•	Sheet Size box. Scroll to the correct sheet size.

•	Units box. Scroll to the correct units of measure.

•	Move entities onto sheet. Select this option to move the lower-left corner of the imported drawing to the origin of the SolidWorks drawing sheet. (This option is only available if SolidWorks detects that either the X or Y coordinate of the lower left-hand corner of the imported drawing is negative.)

•	Import to template.  Select this option to place all geometry in the template instead of on the sheet.

Note:

If you import the geometry to the template, thereafter you edit the geometry by selecting Edit Template from the right-mouse menu. This is the appropriate option to choose if you are importing a previously designed template that you want to name and use repeatedly for SolidWorks drawings.

If you do not import to the template, the geometry is placed on the sheet.  Thereafter, you edit the geometry by selecting Edit Sheet from the right-mouse menu.

After the drawing is imported, you can click Tools, Sketch Tools, Modify and use Translate to move the drawing to a new position. See Modify Sketch  for more information about Translate.


Open File

This command is available from within an assembly or a drawing; it does the following:

•	Opens the part file or sub-assembly file of the selected component in an active assembly.

•	Opens the part file or assembly file of the selected part or assembly in a drawing.

To open a part or assembly file:

1	Right-click a part or assembly, or its name in the FeatureManager design tree.

2	Select Open File from the menu.

The part or assembly file opens for editing.


Open Parasolid File

Imports a Parasolid file for a part or assembly in the appropriate SolidWorks window.

To open a Parasolid file:

1	Click File, Open and select the filename. (In the Open dialog, be sure that the Files of Type box displays either Parasolid files *.x_t, *.x_b, or *.*)

2	Click Open.

If the file you chose is an assembly, you are notified that a new assembly and new part files for the assembly components will be created in the directory shown. To change to a different directory, click Browse, locate the new directory, and click OK.


Ordinate Dimension

Creates ordinate dimensions in a drawing, measured from the axis you select first. The type of ordinate dimension (horizontal, vertical, or angular) is defined by the orientation of the points you select.

To create ordinate dimensions:

1	With a drawing active, click [image] and then select Ordinate Dimension from the right-mouse menu.

- or - Click Tools, Dimensions, Ordinate.

2	Click the first item from which all others will be measured (the 0.0 dimension), and click again to place the dimension.

3	Click an item to dimension, then click to place its dimension. Repeat this step until all the remaining items are dimensioned. The dimension tool remains in ordinate mode until you select another mode or another tool.

To modify ordinate dimensions:

You can modify ordinate dimensions using commands on the right-mouse menu.

1	Activate (double-click) the drawing view containing the dimensions you want to modify.

2	Right-mouse click an ordinate dimension, then select from these options:

•	Add to Ordinate Dimension. Use this option to add more dimensions later, along the same ordinate.

•	Align Ordinate. Aligns all the dimensions along the ordinate with the 0.0 ordinate.

•	Jog. Bends the leader line of a dimension and allows you to reposition it (to eliminate crowding).

To display as chain dimensions:

1	Right-mouse click on an ordinate dimension and select Properties from the menu.

2	Click the Display as chain dimension checkbox. (All the dimensions along the ordinate are affected when you select or deselect this option.)

See also Vertical Ordinate Dimension, Horizontal Ordinate Dimension.


Orientation

Rotates and zooms the model or drawing to a preset view. You can select from the standard views (Normal To, Front, Back, Isometric, and so on for a model, Full Sheet for a drawing) or add your own named views.

To select a view:

1	Click View, Orientation.

2	Double-click the name of the desired view, or select a planar face and double-click Normal To.

Note:  To keep the Orientation list open, click the [image] icon.

You can return your model or drawing to a previous view by clicking [image], the Undo button, on the View Orientation dialog box. You can undo the last 10 view changes.

To add your own named view:

1	Use the Rotate, Zoom, and Pan commands to create the desired view.

2	Click View, Orientation.

3	Click Add.

4	Enter a descriptive name for the view, and click OK. The name will appear at the top of the list of views, and you can display the view by double-clicking it.

5	To remove one of your named views from the list, select it and press the Del key.

To change the orientation of the standard model views:

1	Click View, Orientation.

2	Double-click on one of the named views to select the new orientation. For example, if you want what is currently the Left view to become the front view, double-click Left.

3	Click (do not double-click) the name of the standard view you want to assign to the current orientation of the model. For example, click Front if you want the current view to become the front.

4	Click Update. This updates all of the standard views so they are relative to this view.

To return all standard model views to their default settings:

1	In the View Orientation dialog, click Reset.

2	Respond to the message box by clicking either Yes, to restore the default settings, or No to close the dialog without restoring the default settings.


Origins

Toggles the display of the origins on and off.

To turn origin display on or off:

Click View, Origins. A check mark next to the menu item means origin symbols are visible (except for origins that you have hidden individually).

To hide or show individual origin symbols:

1	Right-click on the origin symbol in the FeatureManager design tree.

2	Click Hide or Show.


Override Dims on Drag

Lets you override dimensions by dragging sketch entities. The sketch dimensions update at the end of the drag. They remain driving dimensions and update in the assembly and in the drawing.

To override dimensions by dragging:

1	In a part sketch or a drawing, click Tools, Sketch Tools, Override Dims on Drag.

When Override Dims on Drag has a check mark next to it, you can drag sketch entities and the dimensions will update automatically in the part, assembly and drawing.

2	Click [image] or [image] to rebuild the part and exit the sketch.


Add a Named View

1	Use the Rotate, Zoom, and Pan commands to create the desired view.

2	Enter a descriptive name for the view, and click OK.

Display the named view by double-clicking on its name in the View Orientation list.

For more information about the View Orientation list, see Orientation .


Page Setup

Lets you control the appearance of printed documents and provides access to the Print Setup dialog.  Also lets you create a header and/or footer for the active document before printing.

To set the print options of a document:

1	Click File, Page Setup.

2	From the Printer tab,

•	Paper Margins.  To set paper margins, you can either

Specify margin widths in the appropriate margin boxes (Top, Bottom, Left, or Right).

- or -

Use the default margins by clicking the checkbox next to Use printer’s margins.

•	Line Weight. Specify the line weight in the appropriate line style boxes (Thin, Normal, and Thick).

•	Page Orientation. Select either Portrait (vertical page orientation) or Landscape (horizontal page orientation).

•	Scale. Use the default scale by clicking Scale to Fit or else use the Scale scroll box to specify the scale you want.

•	Print Setup. Click this button to access the Print Setup dialog box. This lets you choose your printer, paper size and set other printer properties.

3	Click OK.

To create a header and footer for the current document:

1	Click File, Page Setup.

2	From the Header/Footer tab,

•	Scroll the Header and Footer boxes to select predefined headers and/or footers, and view your selection in the Preview boxes.

•	Click Custom Header or Custom Footer to define your own headers and/or footers.

3	Click OK.

To view the changes before printing the document, click Print Preview .


Parent/Child

Displays the parents and children of a selected feature, sketch, axis, plane curve or surface.

To display parent/child relations:

1	In the model or in the FeatureManager design tree, right-click the item whose parent/child relations you want to examine.

2	Click Parent/Child.


Parameter Property

Name. The name of the parameter. To change the name, select it and enter a new name.  Click OK.


Paste

Copies the contents of the Clipboard to the current sketch, part, assembly, or drawing document.

To paste the contents of the Clipboard:

1	If necessary, select an appropriate destination for the item being pasted. For example:

•	If the Clipboard contains a sketch, select a face or a plane to paste the sketch on.

•	If the Clipboard contains an extruded or revolved feature or a hole, select a face to paste the feature on.

2	Click [image], or Edit, Paste or Ctrl+V.

Note:  When you paste a sketch, you cannot have a sketch open.


Pattern Deletion

To delete pattern instances:

1	Select the pattern instance(s) that you want to delete.

2	Press the Delete key.

3	In the dialog box, select one of the following:

•	Delete Pattern Instances. Only the selected instance(s) are deleted. The instance locations are displayed in the Instances Deleted box.

•	Delete Pattern Feature. The complete pattern is deleted, not including the initial feature.

4	Click OK to delete, or click Cancel to exit the dialog.

To restore deleted pattern instances:

1	Right-click the pattern feature, and select Edit Definition.

2	In the Instances Deleted box, select the number corresponding to the deleted instance to restore, and press the Delete key.


Performance Options

To set performance options:

1	Click Tools, Options.

2	Click on the Performance tab.

3	Change the settings and click OK if you are satisfied; click Reset All to return to the settings that you started with.

Shaded Display Quality. Controls the tessellation of cylindrical surfaces for shaded rendering output. A higher resolution setting results in slower model rebuilding but more accurate curves.

•	Coarse or Fine. Preset resolutions.

•	Custom. Allows you to choose any resolution by dragging the slider control or by entering a Deviation value.

Deviation. Reports the maximum chordal deviation in effect at the various tuning levels. The chordal deviation value is greater at the Coarse setting, and decreases as the resolution becomes more finely tuned.

Wireframe Display Quality.

Optimal. A preset quality that provides a faster redraw without greatly sacrificing the display quality.

Custom. Allows you to choose the display quality by dragging the slider control. Choose the Low end of the slider if you want to redraw the screen more quickly and the display quality is not of great importance; choose the High end of the slider for high display quality, but a slower redraw.

Note:  If you are noticing problems with your HLR image display, you may want to select a higher quality wireframe display.

Rebuild. Verification on Rebuild controls the level of error checking when creating or modifying features. For most applications, the default setting (off) is adequate, and results in faster model rebuild.

Windows95 Zooming.  Enable clipping for zoom limitation. When using SolidWorks on Windows95, there is a limit beyond which you cannot zoom in on a model. This option lets you select a portion of the model and zoom in on only the selected portion. You can zoom in on small details very closely, but the display is slower.

Transparency Quality.  Select either Low or High.  Low quality transparency (Screen Door) is similar to viewing an object through a mesh or screen; High quality transparency (Alpha Blending) is similar to looking through clear glass.


Perpendicular to Curve at Point Plane

To create a plane through a point and perpendicular to an edge, axis, or sketch curve:

1	Select an edge, axis, or sketch curve and a vertex or point, while holding the Ctrl key.

2	Click Finish.


Perspective

Displays a perspective view of the model. You use Perspective along with one of the other view types: Wireframe, Hidden in Gray, Hidden Lines Removed, or Shaded.

To display the model in perspective view:

Click [image] or View, Display, Perspective.

See also Modify Perspective


Plane

Creates a construction plane in a part or assembly.

To create a construction plane:

1	Click [image] or Insert, Reference Geometry, Plane.

2	Select the type of plane you want to create and click Next.

3	Select the appropriate number of vertices, faces, or edges for the type of plane you want to create.

4	Enter the required distance or angle, if any, and click Reverse Direction, if necessary.

5	Click Finish.

See also:

Plane at Angle

Offset Plane

On Surface Plane

Parallel Plane at Point

Perpendicular to Curve at Point Plane

Line and Point Plane

Three Point Plane


Plane at Angle

To create a plane through an edge, axis, or sketch geometry at an angle to a face or plane:

1	Select a plane or a planar face.

2	Hold the Ctrl key and select an edge, axis, or sketch line.

3	Specify the Angle between the new and existing plane.

4	Click Reverse Direction, if necessary.

5	Click Finish.


Planes

Toggles the display of planes on or off.

To turn plane display on or off:

Click View, Planes. A check mark next to the menu item means planes are visible (except for planes you have hidden individually).

To hide or show individual planes:

1	Right-click on the plane or on its name in the FeatureManager design tree.

2	Click Hide or Show.

Note:	Individual planes always appear when you select them.


Point

Creates a sketch point.

To create a sketch point:

1	Click [image] or Tools, Sketch Entity, Point.

2	Click where you want to create the point.


Parallel Plane at Point

To create a plane through a point parallel to a plane or face:

1	Select a plane or planar face and a vertex or point while holding the Ctrl key.

2	Click Finish.


Point Properties

Sketch Point. The X, Y, Z coordinates of the point.

Defined Status. Indicates whether the point is currently underdefined or fully defined.


Previous Sheet

Displays the previous sheet in a drawing.

To display the previous sheet:

Click View, Previous Sheet, or click on the sheet tabs at the bottom of the drawing window.


Print

Prints the active part, drawing, or assembly document.

To print the current document:

1	Click [image], or File, Print.

2	Review the information in the Print dialog, and make changes as appropriate.

3	Click OK.

Printer

•	Name. Select the printer’s name from the drop-down list.

•	The system provides read-only information about the printer’s status, type, and location.

•	Print to file.  Check this box to send this print to a file instead of the printer. A dialog box appears that lets you name the file to print to.

Print Range

•	All. Prints all pages of the document.

•	Pages. Prints a range of pages in your document.  Enter the first and last page that you want to print.

Copies

•	Number of copies. Select the number of copies to print from the spin box.


Print Preview

Previews the image of the active Part, Drawing, or Assembly before you send it to the printer.

To preview a print job:

Click [image], or File, Print Preview.

See also Print ,  Page Setup .


Projection

Creates a new orthographic view that is unfolded from an existing view.

To create a projection view:

1	Open the drawing that has the view you want to project.

2	Click on the view you want to project.

3	Click [image] or Insert, Drawing View, Projection.

4	Click beside the selected view on the drawing sheet to indicate the direction for the projected view. For example, to project the the right face of the selected view, click to the right of the selected view.


Projected Curve

You can project a sketched curve (either open or closed) onto a surface to create a 3D curve.

You can use the projected curve to create a path or guide curve for a swept feature or the guide curve for a lofted feature.

To project a curve onto a face:

1	Create a sketch that contains a single curve (either open or closed).

2	Click [image] to close the sketch.

3	Select the sketch.

4	Hold down the Ctrl key and select the face where you want to project the curve.

5	Click Insert, Reference Geometry, Projected Curve. The curve now appears in the FeatureManager design tree and on the selected face.

Also, you can create a 3-D curve that represents the intersection of two extruded surfaces generated by curves sketched on two intersecting planes.

To create a projected curve using sketches on two intersecting planes:

1	Create a sketch on each of two intersecting planes, closing each sketch when you are done. Each sketch must contain a single open curve.

Be sure to align the sketches such that when they are projected normal to their sketch plane the implied surfaces will intersect, creating the desired result.

2	Click to select each sketch.

3	Click Insert, Reference Geometry, Projected Curve.

The curve appears.

See also Sweep and Loft Feature


Properties

Displays the properties of a selected item.

To view an item’s properties:

1	Right-click on the item or on its name in the FeatureManager design tree.

2	Click Properties.

3	Make any appropriate changes (some property values are read-only) and click OK.

See also properties for:

Arc

Center Mark

Dimension Display

Dimension Tolerance Properties

Drawing View

Entity

Feature

Line

Point

Section Line

Spline,

Reference Geometry

To view the properties for a document:

1	Click File, Properties.

2	Make changes or additions to the Summary page and/or the Custom page.

3	Click OK.


Rebuild

Rebuilds the model with any changes that you made.

To rebuild the model:

Click [image] or Edit, Rebuild, or press Ctrl+B.


Record Macro

Creates a macro that records your mouse clicks, menu choices, and keystrokes to play back later.

To record a macro:

1	Click [image] or Tools, Macro, Record.

2	Perform the steps you want to record.

3	When you are done, click [image] or Tools, Macro, Stop.

4	Type a name for the macro and click OK to save it. (SolidWorks automatically adds the extension to the filename.)

- or -

Press Cancel in the Save Macro dialog to cancel the macro.


Rectangle

Creates a rectangle.

To create a rectangle:

1	Click [image] or Tools, Sketch Entity, Rectangle.

2	Place the cursor where you want one corner of the rectangle to appear.

3	Drag the cursor and release when the rectangle is the correct size and shape.


Redraw

Refreshes the screen, but does not rebuild the part.

To refresh the screen:

Click [image] or View, Redraw, or press Ctrl-R.

Note:  Use Redraw to refresh the screen if the graphics do not appear to be complete.


Reference Axis

Creates a reference axis (or construction axis).

To create a reference axis:

1	Select from the Options to make an axis box:

•	One Temporary Axis. Select View, Temporary Axis , and then select the axis.

•	Two Planes. Select View, Planes, and then select two construction planes (while holding the Ctrl key).

•	Two Points/Vertices. Select two sketched points or two vertices

•	One Line/Edge. Select one line or edge.

•	One Surface. Select one cylindrical surface.

2	Verify that the items listed in the Valid Items for an Axis box correspond to your selection(s).

3	Click OK.

Note:   Axis display must be turned on (see Axes ) to see the new axis.


Reference Dimensions

Creates reference dimensions on drawings.

Reference dimensions show measurements of the model, but cannot be used to drive the model and you cannot change their values.

To add a reference dimension:

1	Select the drawing view.

2	Click [image].

3	Click the item(s) you want to dimension. (See Dimension for details.)

4	Click to place the dimension.

5	Reference dimensions are shown in parentheses by default.

To specify the default for all drawings, click Tools, Options and select the Detailing tab. Select Add Parenthesis by Default.

See Detailing Options.


Relative to Model

Creates a drawing view by selecting two orthogonal faces to define an orientation.

To create the view:

1	Open a part, and open the drawing where you want to insert a view of the part.

2	From the drawing, select [image] or Insert, Drawing View, Relative to Model. A small part symbol appears on the cursor to indicate that you need to select a part.

3	Activate the part window by clicking on it or by choosing it from the Window menu.

4	Click on a face on the part.

5	Select the direction you want the selected face to be oriented towards, then click OK.

6	Click on a second face, then select its orientation and click OK.

7	Activate the drawing window, and click where you want to place the view.


Reload/Replace

Allows you to Reload or Replace documents, either locally or over the Internet.

To reload the document you are currently referencing:

1	Click File, Reload.

2	Click Open as read-only if you do not want to save any changes to the file.

3	Select either Reload or Replace.

•	Reload. Refreshes shared documents. For example, if you open a part file for read-only access and use that part while another user is making changes to the same part, you can load the new version including the changes.

•	Replace. Lets you load a new file into the SolidWorks session and replace each open reference to the current file with a reference to the new file instead. You can use the Browse button to access the new file.

4	Click OK to accept the change, or click Cancel.

Note	The reloaded part must be read-only, and not derived.


Reload Internet Document

Allows you to Reload documents, either locally or over the Internet.

To reload the document you are currently referencing:

Click [image] on the Web toolbar.

Reload refreshes shared documents. For example, if you open a part file for read-only access and use that part while another user is making changes to the same part, you can load the new version including the changes.


Reset Size

Restores an embedded OLE object to its original height and width.

To reset an OLE object to its original size:

1	Select the OLE object.

2	Click Edit, Object, Reset Size.


Resolve Result Ambiguity

The SolidWorks software has found multiple ways to solve the part. The Resolve Result Ambiguity dialog gives you the opportunity to select the solution that you want to use.

•	The Current box displays the number assigned to the highlighted solution.

•	The Out Of box displays the total number of possible solutions.

To select the solution that you want to use:

1	Click the Previous and Next buttons to highlight each possible solution in the graphics area.

2	When the solution that you want is highlighted, click the OK button. Click the Cancel button to close the dialog without selecting a solution.


Revolve

Creates a feature that adds or removes material by revolving a closed profile around a centerline. The feature may be either solid or thin walled.

To create a revolved feature:

1	Create a sketch and draw a profile and a centerline. (The profile must be closed, and it cannot cross the centerline.)

If the sketch contains more than one centerline, select the centerline you want to use as the axis of the revolution.

2	If you are creating the first feature in a part, click [image] or Insert, Base, Revolve.

Otherwise click [image] or Insert, Boss, Revolve or [image] or  Insert, Cut, Revolve.

3	From the Revolve As: box, select either Solid Feature or Thin Feature.

4	If you select Thin Feature, click the Thin Feature tab, choose a direction from the Type list box, and specify a Wall Thickness.

- or -

If you select Solid Feature, choose a direction from the Type list box and set the desired rotation angle in the Angle box.

5	The preview shows the direction of rotation. Select the Reverse check box if you want to rotate the feature in the opposite direction.

6	Click OK.

See also Revolved Surface


Revolved Boss/Base

Creates a feature that adds material by revolving a closed profile around a centerline. The feature may be either solid or thin walled.

To create a revolved boss or base:

1	Create a sketch and draw a profile and a centerline. (The profile must be closed, and it cannot cross the centerline.)

If the sketch contains more than one centerline, select the centerline you want to use as the axis of the revolution.

2	Click [image] or Insert, Boss, Revolve (or, if it is the first feature, click Insert, Base, Revolve).

3	From the Revolve As: box, select either Solid Feature or Thin Feature.

4	If you select Thin Feature, click the Thin Feature tab, choose a direction from the Type list box, and specify a Wall Thickness.

- or -

If you select Solid Feature, choose a direction from the Type list box and set the desired rotation angle in the Angle box.

5	The preview shows the direction of rotation. Select the Reverse check box if you want to rotate the feature in the opposite direction.

6	Click OK.


Revolved Cut

Creates a feature that removes material by revolving a closed profile around a centerline. The feature may be either solid or thin walled.

To create a revolved feature:

1	Create a sketch on an existing solid and draw a profile and a centerline. (The profile must be closed, and it cannot cross the centerline.)

If the sketch contains more than one centerline, select the centerline you want to use as the axis of the revolution.

2	Click [image] or  Insert, Cut, Revolve.

3	From the Revolve As: box, select either Solid Feature or Thin Feature.

4	If you select Thin Feature, click the Thin Feature tab, choose a direction from the Type list box, and specify a Wall Thickness.

- or -

If you select Solid Feature, choose a direction from the Type list box and set the desired rotation angle in the Angle box.

5	The preview shows the direction of rotation. Select the Reverse check box if you want to rotate the feature in the opposite direction.

6	Click OK.


Rib Feature

Adds a rib of a specified thickness and direction between the contour and the surrounding part.

To add a rib to a part:

1	Insert a plane that intersects the part in the direction in which you want to create the rib.

2	Sketch the contour to use for the rib.

3	Click [image] or Insert, Features, Rib.

4	From the Rib dialog, select Mid Plane to extrude the rib equally in both directions from the sketch plane, or Single Side to extrude in one direction.

5	If you chose Single Side, examine the preview and select Reverse if necessary to get the results you want.

6	Enter the thickness of the rib, and click Next >.

7	In the Rib Options dialog, examine the preview and, if necessary, select Flip side of material to reverse the direction in which material is added.

8	To add a draft, select Enable Draft and enter the draft angle. Select Draft Outward, if necessary.

9	To create a rib with multiple contours using draft angles, click the Next Reference button until the arrow shows on the contour from which you want to start the draft angle.

10	Click Finish.


Rib

Select Mid Plane to extrude the rib equally in both directions from the sketch plane.

Select Single Side to extrude in one direction.

If you chose Single Side, examine the preview and select Reverse if necessary to get the results you want.

Enter the thickness of the rib, and click Next >.


Rib Options

Examine the preview and, if necessary, select Flip side of material to reverse the direction in which the rib material is added.

To add a draft, select Enable Draft and enter the draft angle. Select Draft Outward, if necessary.

To create a rib with multiple contours using draft angles, click the Next Reference button until the arrow shows on the contour from which you want to start the draft angle.

Click Finish.


Rollback

Reverts the model to the state it was in before the selected feature was created.

Rollback also flattens sheet metal bends.  See also Bends .

To revert to an earlier state:

1	Select a feature in the FeatureManager design tree or in the graphics display area.

2	Click [image] or Edit, Rollback.

The model reverts to the state it was in before the selected feature was created.

You can now add new features or edit existing features while the model is in the rolled-back state.

3	To roll forward again, click [image] or Edit, Rebuild. (The model will not rebuild unless you answer Yes in the dialog box.)

Note:	The same rollback functionality is available for parts and assemblies by using the rollback bar in the FeatureManager design tree. The rollback bar is a wide yellow line which turns blue when selected. Drag the bar up or down the FeatureManager design tree to step forward or backward through the regeneration sequence.

To use the rollback bar:

1	Place your cursor over the rollback bar in the FeatureManager design tree. The cursor changes to a hand.

2	Click to select the rollback bar. The bar changes color from yellow to blue.

3	Drag the rollback bar up the FeatureManager design tree until it is above the feature you want rolled back,

- or -

Use the up and down arrow keys on the keyboard to move the rollback bar up or down. (Check Arrow key navigation in Tools, Options, General to enable this functionality.)

Note:	You do not have to select a feature before you move the rollback bar. Note also that the FeatureManager icons are grey after they are rolled back.


Rotate About Screen Center

Determines whether Rotate View rotates the view around the center of the screen or around the center of the part or assembly.

To set the center of view rotation:

Click View, Modify, Rotate About Screen Center. A check mark next to the menu item means that rotation will be around the screen center.


Rotate Component Around Centerpoint

Rotates an unmated component in the assembly window.

To rotate with the mouse:

1	Click the component to select it.

2	Click [image] on the Assembly toolbar, or click Tools, Component, Rotate.

3	Hold the mouse button down and drag in the direction you want to rotate the component.

The component rotates around its own centerpoint.

4	To rotate a different component, click its name in the FeatureManager design tree and drag it.

5	Click [image] again when you are finished.

See also Move Component and Rotate Component Around Axis .


Rotate Component Around Axis

Rotates an un underdefined component in an assembly around an axis, a linear edge, or a sketched line.

To rotate a component around an axis:

1	If you want to rotate around an axis, click View, Temporary Axes and select an axis,

-or-

click an edge or sketched line to rotate around.

2	Hold the Ctrl key and click the component that you want to rotate.

3	Click [image], press the left mouse button and drag to rotate in the direction you want to rotate the component.

4	Click [image] again to stop rotating.

See also Move Component  and Rotate Component Around Centerpoint  .


Rotate View

Rotates your view of the model.

To rotate the image on the screen:

1	Click [image] or View, Modify, Rotate.

2	Press the mouse button and drag to rotate the view.

Note	The Rotate About Screen Center command determines whether the view rotates around the center of the screen or the origin of the model.

Tip	Use the Arrow keys to rotate the view vertically or horizontally. (Hold down the Shift key to rotate in 90-degree increments). Hold down the Alt key and use the left-right Arrow keys to rotate clockwise or counterclockwise.


Run Macro

Opens a dialog that lets you select the macro you want to run.

To run a macro:

1	Click [image] or Tools, Macro, Run.

2	Locate the macro (.swb) file you want to run and click OK.


Save

Saves the active document to disk.

To save a document:

Click [image] or File, Save, or press Ctrl-S.

The first time that you save a new document, a dialog box opens that lets you type a new filename or accept a default filename.


Save As

Saves the active document to disk with a new name or saves it in a different format for export to another application.

To save a document with a new filename or format:

1	Click File, Save As.

The Save As dialog appears.

2	Type the new filename.

3	Click Save As Copy to save the document to a new filename without replacing the name in the active session. Documents that reference the active document will continue to reference the original file.

4	To save the file in another file format, select a format from the Save as File Type box.

You can save parts as SolidWorks part files (.sldprt), IGES files (.igs), Parasolid files (.x_t), Parasolid Binary files (.x_b), STL files (.stl), Library Feature Parts (.sldlfp), ACISTM files (.sat), or VRML files (.wrl).

You can save assemblies as SolidWorks assembly files (.sldasm), Parasolid files (.x_t), Parasolid Binary files (.x_b), or VRML files (.wrl).

You can save drawings as SolidWorks drawing files (.slddrw), DXF files (.dxf), or DWG files (.dwg).

5	Click Save to save the document with the new name and file type; click Cancel to exit without saving.


Search Results

Displays the list of part and sub-assembly documents that make up the active assembly.

To copy a listed file to a new directory:

1	Select a listed file.

2	Click the Copy Files button.

The Choose Directory dialog box provides a default of  the present directory in which you are working.  If you need to copy the file to another directory, you can browse the local directory tree or click Network to browse your network.

3	Click OK to complete the file copy.

4	Click Close to close the dialog and return to the active assembly.


Send Mail

Sends the current assembly or drawing (with or without the component parts) to another system using your electronic mail application.

To mail an assembly or drawing to another computer:

1	Click File, Send To.

2	In the Send Mail dialog box, click a radio button to select one of the following:

•	Send the current document only.

•	Send the current document and the other documents that it references.

A list of the referenced documents, the number of documents, and the combined size of the documents is displayed. Note: Mail size can cause transmission problems.

If you choose to send the assembly or drawing and referenced documents, you do not have to send all of the referenced files. You can:

•	Click a filename you do not want to send and click the Remove button. (The paper clip icon is removed.)

•	Click a removed filename and click the Attach button to replace the file. (The paper clip icon is replaced.)

•	To return all the removed files to the list, click Attach All.

3	Click OK to send your document(s).

4	Enter your mail password, the mailing address, and any other information required by your mail application.


Sketch Fillet Radius

To specify the radius of a fillet in a sketch:

1	Hold down the Ctrl key and select two sketch elements that form a corner.

2	Click [image] or Tools, Sketch Tools, Fillet.

3	Select the Radius value box and enter a value or use the arrows to scroll to a new value.

4	Click OK.


Symbol

Inserts a symbol.

To add a symbol to text:

1	Select a library from the Symbol Libraries list.

2	Select a symbol name from the list, and click OK.

The selected symbol appears in the preview box.

Note	The symbol is represented by its name in the Note Text preview box, but the actual symbol appears in the drawing note.


Template to Use/Save Template

Template to Use:

Lets you select a template style for your new drawing.

To select a new template:

1	Open a new drawing document.

2	Select either Standard Template, Custom Template, or No Template.

•	Standard Template.  Use the spin box to select from a set of standard template styles.

•	Custom Template.  Use the browse button to locate the directory and template file that you want to use.

•	No Template.  Selects a blank drawing sheet.

3	Click OK after making your selection.

Save Template:

Saves the template used to create the active drawing. If you have customized the template in any way, the template retains those changes.

To modify a drawing template:

1	Open a new drawing document, using the template you want to modify.

2	Activate the drawing sheet and modify it. For instance, you might draw a border or a title block.

3	Click File, Save Template.

4	If you want to overwrite the standard template, click OK and confirm.

- or -

If you want to save the template to a new name, click Custom Template, Browse to a location, and enter a new template name.  (Template files have the .drt extension.)

5	Click Save.

The changes that you made will appear in all new drawings created with that template.

See also Customize Drawing Template .


Scale

Scale allows you to scale the model about the centroid or about the model origin.

To scale a model:

1	With a part document active, click [image] or Insert, Features, Scale.

2	From the Scaling Type pull-down list, select either: About Centroid or About Origin.

3	Specify a scaling value in the Scaling Factor box.

4	Click OK to accept the value; click Cancel to exit the dialog without changing the scale.


Scan Equal

Scans a sketch for elements with equal lengths and/or radii, and lets you create equal length/radii relations between the elements.

To locate equal radii and line lengths:

1	In a sketch, click Tools, Relations, Scan Equal.

2	If sketch elements exist that are equal, the appropriate radio buttons are active. (For example, if two or more lines are equal, Length is active; if two or more arcs have equal radii, Radii is active; if an arc has a radii equal to a line length, Both is active.)

3	To see the equal sketch elements, click an active radio button.

•	The equal elements of the same type as the radio button that you clicked, are highlighted in the sketch.

•	The Value box displays the length or radii.

•	The Line Count or the Arc Count box displays the number of equal elements.

4	If there are additional sets of equal elements of the same type, the Find Next button is active. To highlight the additional sets, click the Find Next button.

5	Click Set Equal, if you want to create an Equal Length/Radii relation between the highlighted elements.

6	Click Close.


Section

Creates a cross section drawing view of the model.

To create a section view:

1	Double click the drawing view where you want to draw the section line. (This activates the view so you can draw on it.)

2	Click [image] or Tools, Sketch Entity, Line and draw the section line or a series of connected lines.

3	Click [image] and select the sketched line(s).

4	Click [image] or Insert, Make Section Line. This converts the line(s) into a section line, with arrows indicating the direction of the view.

5	If necessary, double-click on the section line to reverse the direction of the view.

6	Select the section line.

7	Click Insert, Drawing View, Section.

You can edit section lines by dragging them and then clicking Rebuild.

To change the section line label or the direction of the view, right-mouse click the line and select Properties . Make your changes, then click Rebuild.

The solid interior of the section view is crosshatched. To change the pattern, see Crosshatch.


Section View of Model or Assembly

Creates a section view of the model or assembly for display purposes. You cut through the model or assembly using one of the following:

•	one or more standard planes (Plane1, 2, or 3). Note:  You can pre-select a plane. If no plane is selected, Plane1 is displayed by default.

•	one or more planes that you create for the purpose (Click Insert, Reference Geometry, Plane, and create a new plane.)

•	one or more planar face(s) (Select any planar face(s) on the model.)

•	the viewing plane  (The invisible plane that is parallel to the screen you are looking through. The initial position for this plane is the center of the part body bounding box.)

You can view the section in one of two ways:

•	Click the Pre View box. When this is checked, the section view is updated each time the the dialog box information is changed. (If you change the settings frequently with a large part or assembly, the Pre View box may not be an efficient way to view the section.)

•	When the Pre View box is not checked, click the Display button to display the section view based on the current settings. You can make additional changes to the settings and click Display again.

To create a section view of the model:

1	With a part or assembly document active, click [image] or View, Display, Section View.

2	To make a section cut using a plane or face, click on one or more planes in the FeatureManager design tree, or click one or more faces on the model. The name of each selected plane or face is displayed in the Section Plane(s)/Face(s)  box.  To deselect an unwanted plane click its name in the FeatureManager design tree.

- or -

To use the viewing plane to make a section cut, click Use Viewing Plane in the Section View dialog box.

3	Click a plane in the Section Plane(s)/Face(s) box, then use the spinbox arrows in the Section Position box to move the plane and change the section cut.

4	Click the Flip the Side to View box to reverse the viewing direction of the section cut. (Not available if you are using the viewing plane.)

5	Click OK.

Note:	You can view both the section view and the complete view of the model at the same time by splitting your screen into two windows. (Drag the split controls on the bottom or right side of the window frame.) You can revolve, size, and shade the views independently.

To change the section view, click View, Modify, Section View and change the settings in the Edit Section View dialog box and/or select a different plane.


Section View

You can cut through the model or assembly using one of the following:

•	one or more standard planes (Plane1, 2, or 3)  Note:  You can pre-select a plane. If no plane is selected, Plane1 is displayed by default.

•	one or more planes that you create for the purpose (Click Insert, Reference Geometry, Plane, and create a new plane.)

•	one or more planar face(s) (Select any planar face(s) on the model.)

•	the viewing plane  (The invisible plane that is parallel to the screen you are looking through. The initial position for this plane is the center of the part body bounding box.)

You can view the section in one of two ways:

•	Click the Pre View box. When this is checked, the section view is updated each time the the dialog box information is changed. (If you change the settings frequently with a large part or assembly, the Pre View box may not be an efficient way to view the section.)

•	When the Pre View box is not checked, click the Display button to display the section view based on the current settings. You can make additional changes to the settings and click Display again.

To create a section view of the model:

1	To make a section cut using a plane or face, click on one or more planes in the FeatureManager design tree, or click one or more faces on the model. The name of each selected plane or face is displayed in the Section Plane(s)/Face(s) box.  To deselect an unwanted plane click its name in the FeatureManager design tree.

- or -

To use the viewing plane to make a section cut, click Use Viewing Plane in the Section View dialog box.

2	Click a plane in the Section Plane(s)/Face(s) box, then use the spinbox arrows to set a value in the Section Position box to move the plane and change the section cut.

3	Click the Flip the Side to View box to reverse the viewing direction of the section cut. (Not available if you are using the viewing plane.)

4	Click OK.

5	You can view both the section view and the complete view of the model at the same time by splitting your screen into two windows. (Drag the split controls on the bottom or right side of the window frame.) You can revolve, size, and shade the views independently.

To change the section view, click View, Modify, Section View and change the settings in the Edit Section View dialog box and/or select a different plane.


Section Scope

In a drawing, lets you select components to be excluded from a section view of an assembly.  During the creation of an assembly section view, use the Section Scope dialog box to exclude any components that are not necessary to the view.

To define a section view and then exclude components:

1	Double click the drawing view where you want to draw the section line.

2	Click [image] or Tools, Sketch Entity, Line and draw the section line or a series of connected lines.

3	Click [image] or Insert, Drawing View, Section. This converts the line(s) into a section line, with arrows indicating the direction of the view.

The Section Scope dialog appears and gives you the opportunity to exclude components from the section view.

4	On the drawing view, click those components that you want to exclude from the section view.

A list of the selected components appears in the Excluded Components list box.

5	To remove a component from the list, select the component and click the Delete From List button.

6	Set the Exclusion Status if the selected component is used more than once in the assembly (for example, if it is a member of a pattern, or if it is used as a component of more than one subassembly):

•	If you want to exclude all the instances of the selected component in the assembly, click Don’t Cut All Instances. In the resulting view, all instances of the selected component will be left uncut.

•	If you want to exclude only the selected instance, leave this unchecked. In the resulting view, only the selected instance will be uncut; all others will be cut.

7	Click OK.

8	If necessary, double-click on the section line to reverse the direction of the view, then click [image] or Edit, Rebuild.

Note:	To edit the section view, right-mouse click the active section view and select Properties.  Add components to the Excluded Components list box by clicking components in the section view (not the parent view). To remove a component from the list, select the component and click the Delete From List button.


Select

Selects items.

To select items:

1	Click [image].

2	Click the item that you want to select.

To select multiple items:

Hold down the Ctrl key while you click the items that you want to select.

To drag select:

In a sketch or drawing, you can drag a selection rectangle around the items you want to select.

See Also:

  Selection Filter


Select Loops

If you select a face, all loops (closed profiles) on the face are selected, too. To select individual loops, click on the face, then hold down the Ctrl key and click on the loops you want to select. This deselects the face and leaves the loops selected.

To select individual loops:

1	Select the face.

2	Ctrl-click the loop you want to select.

3	Now you can fillet only the selected loop.


Select Other

Selects items that are obscured by other items.

To select hidden items:

1	Point at the item you want to select and click the right mouse button.

2	Click Select Other.

3	Click the right button to step through the items that lie under the point where you clicked. Click the left button when the desired item is highlighted.


Selection Filter

Facilitates the selection of specific items.

To set the Selection Filter:

1	Click the arrow on the Selection Filter pull-down box.

2	Set the Selection Filter to the kind of item that you want to select: Faces, Edges, Axes, Planes, or Any Item.

With the filter set, the specified kinds of items are highlighted when you pass your cursor over them. This makes it easy for you to select only those items that you intend to select.

Note: The Selection Filter is not displayed by default.  To display the Selection Filter, click View, Toolbars and choose Selection Filter from the list.


Send To

Sends the current part document to another system using electronic mail.

To mail a part document to another computer:

1	Click File, Send To.

2	Enter your mail password, the mailing address, and any other information requested by your mail application.

To send assembly or drawing documents, see Send Mail .


Shaded

Displays a shaded view of the model. (Shaded mode is the default display mode for parts and assemblies.)

To display a shaded view:

Click [image] or View, Display, Shaded.

To control the color of shaded parts, see Color Options .

To change the color of individual part faces, see Entity Property .

To control the light intensity and direction on the shaded parts, see Lighting .


Shared Values

Links dimension values using named variables.

This enables you to set the value of several dimensions to be equal without the need for multiple equations or relations. When dimensions are linked in this way, any member of the group can be used as a driving dimension. Changing any one of the linked values changes all others to which it is linked.

The variable name you specify becomes the name of the linked dimensions, and appears in the Name box of the Dimension Properties dialog box.

To link dimension values:

1	Right-click one of the dimensions that you want to link, and select Link values.

The Shared Values dialog box appears. The Value box displays the value of the selected dimension, but you may not change it here.

2	Enter a Name. This is the variable name that will be used as the dimension name for the linked items.

3	Click OK.

4	Right-click one of the dimensions that you want to link to the first dimension, and select Link values.

5	Select the variable name from the list in the Name box, and click OK.

6	Repeat for as many dimensions as needed.

The values of the selected dimensions become linked to the first one. Changing any of the linked values causes the others to change.

To unlink dimension values:

Right-click the dimension that you want to unlink, and select Unlink value.


Sheet

Adds a new sheet to the active drawing.

To add a new drawing sheet:

1	With a drawing active, click Insert, Sheet.

2	Specify the drawing name, sheet size, scale and other drawing requirements in the Sheet Setup dialog box.

3	Click OK.

Tip	To move between sheets in a drawing, click the sheet tabs at the bottom of the drawing window, or click View, Next Sheet or View, Previous Sheet.


Bends

Creates bends in a thin-feature part.  Use this operation when creating sheet metal parts.

To create a sheet metal part:

1	Create a part by sketching the part profile, then extruding a thin-feature part.

2	Select a face to be fixed. The fixed face remains in place when the part is unbent.

3	Click [image] or Insert, Features, Bends.

4	In the Flatten Bends dialog box, enter the Default Bend Radius.

5	Select from the following bend allowance options: Use Bend Table , Use K-Factor , or Use Bend Allowance .

6	If you select K-Factor or Bend Allowance, enter a value.

7	If you want relief cuts added automatically, check Auto Relief and enter an Offset Ratio .

8	Click OK.

A bent sheet-metal part is created whose dimensions in the flattened state reflect the specified bend allowance and radius values.

To add a wall to a sheet metal part:

1	Open a sketch on the face of the part where the new wall will be attached.

2	Select the edge of the model to attach the wall to, and click [image].

3	Drag the vertices near existing bends a small distance away from the bends to allow for the bend radius.

4	Click Insert, Boss, Extrude, set the Type to Blind and specify the Depth.

5	On the Thin Feature tab, set the Wall Thickness to be the same as the base part.

6	Click OK.

     ..

Important: All walls must in place before the Sheet-Metal feature adds the bends.

It is recommended that you add all the walls as described here, before inserting bends. However, if necessary, you can rollback the model to the the last feature before the Sheet-Metal feature to add a wall. Or, if parent-child dependencies allow, you may be able to re-order a wall before the Sheet-Metal feature.

7	Click [image] or Insert, Features, Bends.

To flatten a sheet metal part:

1	In the FeatureManager design tree, click a Process-Bends item.

2	Click Edit, Rollback or drag the rollback bar above Process-Bends.

The part flattens and goes into rollback state. In this state, you can make holes, slots, and other modifications to the part surface.

To extrude a boss or cut on the flattened part:

1	Click a face on the flattened part and open a sketch.

2	Sketch a profile and extrude a cut or a boss. If you are adding a boss, click Link to Thickness to insure that the boss is the same thickness as the base.

3	Drag the rollback bar below Process-Bends.

The part rebuilds with the new feature(s) in place.

To add bends to the flattened sheet metal part:

1	In the FeatureManager design tree, click the + sign next to a Process-Bends item to expose the Flat-Sketch item beneath it in the design tree.

2	Right-mouse click on Flat-Sketch and select Edit Sketch.

3	Click [image] or [image], and sketch one or more lines across the face of the part where you want to make a bend.

4	Click [image] to close the sketch and rebuild the part.

The part rebuilds with the new bend(s) in place.

To flatten a sheet metal part that contains features added after Process-Bends:

1	In the FeatureManager design tree, right-mouse click the Process-Bends icon.

2	Select Properties.

3	In the Feature Properties dialog box, click the Suppressed checkbox.

The part flattens. In this state, you can extrude a boss or cut, or add bends as described above.

4	To rebend the part, repeat the procedure, clicking the Suppressed checkbox again to unsuppress the feature.

For information about making changes to the bends that you added, see Edit Bends .

See also Reorder Bends .


Edit Bends

You can edit bend information by using the Edit Definition option from the right-mouse menu. The scope of the changes depends upon which feature is edited. For more information, select from the following.

  Edit a single bend.

  Edit bends for an entire part.

  Edit bends listed under Flatten-Bends.

  Edit bends listed under Process-Bends.

Notes:

1)  You cannot change the bend angle for sharp bends because
      this is calculated from your model.

2)  You cannot change the bend angle and radius for round bends.
     The bend angle is calculated from the model and the bend radius
      is specified in the sketch or in the fillet.


Edit a Single Bend

To edit a single bend:

1	In the FeatureManager design tree, right-click a SharpBend, RoundBend, or FlatBend item that you want to change, and select Edit Definition.

2	On the dialog box that comes up, make changes as needed to the bend Radius, Angle, or Order. Click Bend Down to reverse the direction of the bend.

3	In the Bend Allowance region, you can un-check the Use Default checkbox if you want to change the use of the Bend Table , K-Factor, or Bend Allowance .

4	Click OK to exit the dialog and rebuild the part.


Edit Bends for Entire Part

To Edit bend parameters for the entire part:

1	In the FeatureManager design tree, select the Sheet-Metal feature.

2	Right mouse click and select Edit Definition.

3	In the Sheet-Metal dialog box, change the Default Bend Radius.

4	In the Bend Allowance region, you can change the use of the Bend Table , K-Factor, or Bend Allowance .

5	You can un-check Auto Relief or change its Offset Ratio .

6	Click OK.


Edit Bends Listed Under Flatten-Bends

To edit bend parameters for all bends listed under Flatten-Bends:

1	In the FeatureManager design tree, select the Flatten-Bends feature.

2	Right mouse click and select Edit Definition.

3	In the Flatten-Bends dialog box, change the Default Bend Radius.

4	In the Bend Allowance region, you can un-check the Use Default checkbox if you want to change the use of the Bend Table , K-Factor, or Bend Allowance .

5	Click OK.


Edit Bends Listed Under Process-Bends

To edit bend parameters for all bends listed under Process-Bends:

1	In the FeatureManager design tree, select the Process-Bends feature.

2	Right mouse click and select Edit Definition.

3	In the Process-Bends dialog box, change the Default Bend Radius.

4	In the Bend Allowance region, you can un-check the Use Default checkbox if you want to change the use of the Bend Table , K-Factor, or Bend Allowance .

5	Click OK.


Sheet Metal

1	Enter the Default Bend Radius.

2	Select from the following options: Use Bend Table , Use K-Factor , or Use Bend Allowance .

3	If you selected K-Factor or Bend Allowance, enter a value.

4	If you want relief cuts added automatically, check Auto Relief and enter an Offset Ratio .

5	Click OK to accept your input and exit the dialog, or click Cancel to exit without saving your input.


Bend Data

1	If you do not want to use the value in the Default Bend Radius box, deselect Use Default, and enter a new value in Default Bend Radius box.

2	In the Bend Allowance region, deselect Use Default if you want change the following options:

Use Bend Table , Use K-Factor , or Use Bend Allowance .

If you selected K-Factor or Bend Allowance, enter a value.

3	Click OK to accept your input and exit the dialog, or click Cancel to exit without saving your input.


Edit Bend Definition

For any individual Bend From Round, Bend From Sharp, or Bend From Flat:

1	Enter a new value for the bend Radius, or select Use Default.

2	Enter a value for the bend Angle.

3	Enter a value to indicate the bend Order.

Note:  This number specifies the order in which the bends are made in the final fabrication of the part.  The value is not used by SolidWorks, but is for your documentation purposes only.

4	Click Bend Down to reverse the direction of the bend.

5	Click Delay Update if you want to postpone rebuilding the part until you have completed your changes.

6	In the Bend Allowance region, deselect Use Default if you want change the following options:

Use Bend Table , Use K-Factor , or Use Bend Allowance .

If you selected K-Factor or Bend Allowance, enter a value.

7	Click OK to exit the dialog and rebuild the part.


Flatten Sheet Metal Part

Flattens a sheet metal part in which bends have been inserted.

If you want to add features such as holes, slots, or bend reliefs to a part with bends, you must roll back the part to the flattened state and then open a sketch on the face of the part.

To flatten a part with bends:

Click [image] to flatten.

The part flattens, revealing the bend lines. The software calculates the correct overall length of the flat sheet, compensating for the bend radius and bend allowance.

To restore bends to the part:

Click [image] again to restore the bends.


No Bends

Rolls back all  bends from a sheet metal part in which bends have been inserted so that you can make additions, such as adding a wall. (All walls must in place before the Sheet-Metal feature adds the bends.)

To roll back all bends from a sheet metal part:

Click [image] to roll back the bends up to “SheetMetal.”

The bend radius and bend allowance are rolled back. (The part is not flattened.)

To restore all bends to the part:

Click [image] again to restore the bends.


Reorder Bends

You can reorder the bends in a sheet metal part in which bends have been inserted.

To reorder bends in relation to each other:

1	Right-mouse click on Process-Bends in the FeatureManager design tree.

2	Select Reorder Bends from the menu.

3	Click a bend name in the list box and then click the Move Up or Move Down button to move the item up or down the list, into the position you want.

Repeat step 3 to move additional bends.

4	Click OK to accept the new order; click Cancel to close the dialog without reordering.


K-Factor

K-Factor is a ratio that represents the location of the neutral sheet with respect to the thickness of the sheet metal part.

Bend allowance using a K-Factor is calculated as follows:

BA = Π/2(R + KT) A/90

where:

BA = bend allowance

T = material thickness

R = inside bend radius

A = bend angle in degrees  (the angle through which the material is bent)

t = distance from inside face to neutral sheet

K = K factor which is t / T


Bend Table

A sample bend table for sheet metal operations is provided in <install.dir>\lang\english\sample.btl. To use your own bend table, copy this table and edit it to specify your required bend allowances.

The sample bend table is provided only for informational purposes. The values in this table do not represent any actual bend allowance values.

Edit the bend table using any text editor.


Auto Relief

Automatically adds relief cuts wherever needed when inserting bends. The cuts added are of the minimum size required to insert the bend and flatten the part.

When you choose the Auto Relief option, you must specify the Offset Ratio.

Offset Ratio:

Represents the distance, d, by which the side of the square relief cut extends past a bend region, expressed as a ratio of material thickness.

d = (offset ratio) * (part thickness)

(The shaded area represents the bend region.)

The value must be between 0.05 and 2.0. The higher the value, the larger the size of the relief cut added during insertion of bends.


Bend Allowance Value

You can specify an explicit bend allowance for any sheet metal bend by entering the value when you create the bend.

Note:	For a given bend radius and angle, the specified value for the bend allowance should be between the length of the inner edge and the length of the outer edge of the bend.


Sheet Setup

Lets you change the setup of the active drawing sheet.

To change the setup of a drawing sheet:

1	While in an active drawing document, click Edit, Properties.

2	You can make the following changes in the Sheet Setup dialog box:

•	Enter a title in the Name box.

•	Select a Paper Size from the drop-down list of standard paper sizes or select UserDefined to specify a custom paper size.

•	Displays the Height of the selected standard paper size, or lets you specify the custom paper size Height.

•	Displays the Width of the selected standard paper size, or lets you specify the custom paper size Width.

•	Specify the Scale. The default is 1:2.

•	Select a standard drawing template or select Custom or None.

•	Use the Browse button to locate and use a custom drawing template.

•	Select the Type of Projection that will be used if you use the Standard 3 View option on this sheet.

First Angle. Orthographic views in first angle projection.

Third Angle. Orthographic views in third angle projection (the default).

•	Specify the letter of the alphabet that will be used for the next Section Label, Detail Label, and Datum Label. The default letter is A. Successive labels are in alphabetic order.

3	Click OK.


Shell

Creates a shell feature, removing selected faces.

To create a shell feature:

1	Click on the face you want to remove, or hold down the Ctrl key and select multiple faces.

2	Click [image] or Insert, Features, Shell.

3	Make sure the correct faces are listed in the Faces to Remove list box.

4	Set the wall thickness in the Thickness box.

5	Select Shell Outward if you want the shell feature to increase the outside dimensions of the part.

6	Click OK.

To shell faces to different thicknesses:

1	After you select a face to shell and click [image] or Insert, Features, Shell, click in the Multi Thickness Faces box.

2	Click on the faces that will remain as walls of varying thicknesses.

As you click the faces, a list forms in the Multi Thickness Faces box.

3	Click each face name on the list and enter a Thickness value for each one.

4	Choose whether to shell the part inward or outward.

5	Click OK.


Show Hidden Views

Displays in gray the view outlines of hidden views in a drawing. (This command does not “unhide” the views. See Hide View/Unhide View .)

To show hidden drawing views:

Click View, Show Hidden Views.


Show Hierarchy Only

Displays only the top level components of the active assembly.

To show components only:

Right-click the assembly icon at the top of the FeatureManager design tree and select Show Hierarchy Only from the menu.

The FeatureManager display does not include planes, mates, and lower level details.

The display does show the component parts and subassemblies.

Note:  This command is the alternate of  Show Feature Detail.


Show Feature Detail

Displays components and features of the active assembly.

To show feature detail:

Right-click the assembly icon at the top of the FeatureManager design tree and select Show Feature Detail from the menu.

The FeatureManager display includes assembly features, planes, mates, and lower level details.

Note:  This command is the alternate of Show Hierarchy Only .


Simple Hole

Creates a hole feature.

To create a hole feature:

1	Click on the face where you want to create the hole.

2	Click Insert, Features, Hole, Simple.

3	Select the Type from the pull-down list:

Blind	Up to Vertex

Through All	Up to Surface

Up to Next	Offset from Surface

4	Specify the Depth or Offset, if necessary.

5	Specify the Diameter of the hole.

6	If the Type you specified relies on the selection of a surface or vertex, click that item now in the graphics area. The selection is indicated in the Selected Items box.

7	Examine the preview of the hole and select the Reverse Direction checkbox, if necessary.

8	To add a draft, select the Draft While Extruding box. Enter a draft Angle and check Draft Outward, if necessary.

9	Click OK.

To change the diameter of the hole, right-click on the hole’s name in the FeatureManager design tree, select Edit Definition, and change the diameter dimension.


Sketch

Toggles in and out of sketch mode.

To create a new sketch:

1	Select a face or a plane.

2	Click [image] or Insert, Sketch. The sketch grid appears (unless you have turned it off) and EDITING SKETCH appears in the status bar at the bottom of the SolidWorks window.

3	Use the tools on the Sketch Tools and Sketch Relations toolbars to draw and dimension the sketch.

4	When you are finished, click [image] or Insert, Sketch to close the sketch (for use in the creation of a loft or sweep, for instance), or click one of the sketch-based feature commands (e.g., Insert, Boss, Extrude) to create a feature from the sketch.

To edit a sketch:

1	Right-mouse click the sketch you want to edit or a feature built from the sketch, either in the model or in the FeatureManager design tree.

Note	For features built from multiple sketches, (lofts and sweeps), right-click on the sketch name in the FeatureManager design tree.

2	Select Edit, Sketch from the right mouse menu.

3	When you are finished editing, click [image] or Edit, Rebuild, or right-click anywhere in the sketch and select Exit Sketch from the right-mouse menu.

See also Fully Defined Sketches .


Sketch from Drawing

Transfers entities from an existing drawing to an open sketch.

You can use this function to create sketches from imported 2-D DXF and DWG (AutoCAD Release 12) files.

To insert a sketch:

1	Open the drawing that contains the curve entities you want to insert.

2	Open the part where you want to insert the entities.

3	Open a sketch and click Insert, Sketch from Drawing.

4	From the Window menu, select the drawing to make it the active window.

5	Box-select the entities with the left mouse button.

6	Return to the part window. The entities have been inserted into the active sketch in the part, and you can now edit the sketch and use it to make features.


Spline

Creates spline curves.

To create a spline:

1	Click [image] or Tools, Sketch Entity, Spline.

2	Press the mouse button and drag out the first segment.

3	Press over the end point and drag out the second segment.

4	Repeat until the spline is complete.

Note	 If Alternate Spline Creation method is selected (see General Options in the Sketch Controls section), click on each through point to create the spline, then double-click when the spline is complete.

To reshape a spline:

1	Click [image] (the Select tool).

2	Click on the spline; handles appear on the segment end points.

3	Drag the handles to reshape the spline.

Note:    An open spline is proportional by default; when you drag the endpoints, the spline retains its shape. To change the spline’s shape, or to add relations or dimensions to interior points on the spline, you must remove the proportional property. Right-mouse click the spline and select Properties from the menu. Click the Proportional checkbox to remove the check.


Split Line

Projects a sketched curve onto selected model faces. It divides a selected face into multiple separate faces so that each can be selected and modified individually.

Split line is used with the Parting Line option in the Draft feature.

To project a split line onto a planar face:

1	Open a sketch on the face of part and sketch a line to project as your split line.

2	Exit the sketch.

3	Click Insert, Reference Geometry, Split Line.

4	On the Split Lines dialog box, select Projection and click Next.

5	On the Project Split Line dialog, click the Sketch to Project box and select the sketched line in the FeatureManager design tree. The sketch item should appear in the box.

6	Click the Faces to Split box and select all the faces around the perimeter of the part that you want the split line to pass through. The number of faces should appear in the Faces to Split box.

7	If there is an interruption in the selected face (for example, if the sketch plane of the Sketch to Project lies in the area of a cut), click Single Direction to project the curve in one direction only. Click Reverse Direction if the preview indicates that the curve projects the wrong way.

8	Click Finish.

To project a split line onto a cylindrical surface:

1	With a cylindrical part open, click Insert, Reference Geometry, Split Line.

2	On the Split Lines dialog box, select Silhouette and click Next.

3	Click the Direction of Pull box.

4	In the FeatureManager design tree, click any plane that projects through the silhouette.

5	Click the Faces to Split box and click on the cylinder wall(s) to split (not the circular end face).

6	Click Finish.


Split Lines

1	Select the type of split line that you want to make.

•	Silhouette.  Creates a split line on a cylindrical part.

•	Projection.  Projects a sketch line on a surface.

2	Click Next.


Project Split Line

1	Click the Sketch to Project box and select the sketched line in the FeatureManager design tree. A sketch item should appear in the box.

2	Hold the Ctrl key and select all the faces around the perimeter of the part that you want the split line to pass through. The number of faces should appear in the Faces to Split box.

3	Click Single Direction if you want the split line to project in only one direction.

4	Click Reverse Direction to project the split line in the opposite direction.

5	Click Finish.


Silhouette Split Line

1	Click the Direction to Pull box.

2	In the FeatureManager design tree, click any plane that projects through the silhouette.

3	Click the Faces to Split box.

4	Hold the Ctrl key and click on the cylinder wall(s) to split (not the circular end face).

5	Click Finish.


Create Silhouettes

You can select the silhouette edge of a rounded surface, such as a cylinder, revolve, loft, sweep, etc., to use Convert Entities or Offset Entities, add Dimensions and/or Relations.

Note:	The Enable silhouettes option is on by default.  To verify this, click Tools, Options, and select the General tab.

You may notice that it takes a little longer to open a sketch of a complex part or assembly when the Enable silhouettes option is on.  If you have a performance problem, turn off the Enable silhouettes option and use the Create Silhouettes option from the right mouse menu.

To use the Enable Silhouette option:

1	Working with a sketch open on a model face or plane (or working in an active drawing view), drag your cursor over a cylindrical face until the cursor changes to include a small cylinder next to the pointing arrow. At this time, the cylinder’s silhouette edge becomes visible as a dashed line.

2	Select the dashed line to use with the Convert Entities or Offset Entities sketch tools, or to add Dimensions and/or Relations to your sketch.

Note:  To address cases where the generation of silhouettes is too slow, a timer has been added to the Enable silhouettes option.  After 60 seconds, an error message appears advising you to use the Create Silhouettes right mouse function described below. (You do not have to turn off the Enable silhouettes option in Tools, Options, General.)

To use Create Silhouettes for a complicated part or large assembly:

1	To improve the rebuild performance of a part or assembly, click Tools, Options, and select the General tab. In the Sketch block make sure that Enable silhouettes is not checked.

2	Working with a sketch open on a model face or plane (or working in an active drawing view), right-mouse click and select Create Silhouettes from the right mouse menu. The system tries to create silhouettes for any selected faces.

3	Drag your cursor over a cylindrical face until the cursor changes to include a small cylinder next to the pointing arrow.

4	Click on the cylinder’s silhouette edge when it becomes visible as a dashed line.


Standard 3 View

Creates three standard orthographic views on a drawing sheet.

To create a drawing:

1	Open a part or an assembly and a drawing.

2	With the drawing window active, click [image] or Insert, Drawing View, Standard 3 View.

3	From the Window menu, select the part or assembly to make it the active window.

4	Click anywhere in the part or assembly window.

The three views will appear on the drawing sheet. The type of projection (first or third angle) depends on the setting specified by the Sheet Setup command.

5	If necessary, drag the drawing views to position them on the sheet. The top and side views retain their alignment with the front view as you drag them; dragging the front view moves all three views.


Status Bar

Displays or hides the status bar at the bottom of the SolidWorks window.

To display or hide the status bar:

Click View, Status Bar.  A check mark next to the menu item means the status bar is visible.


Stop Macro

Stops recording the macro and opens a dialog so you can name the macro.

To stop recording a macro:

1	Click [image] or Tools, Macro, Stop.

2	Type a name for the macro and click OK to save it. (SolidWorks will automatically add the extension .SWB to the filename.)

- or -

Press Cancel in the Save Macro dialog to cancel the macro.


Stop Internet Jump

Stops the current jump.

To stop the current local or Internet jump:

Click [image] on the Web toolbar.


Summary Info

Allows you to enter or view summary information about the part, assembly, or drawing document.

To enter or display summary information:

1	Click File, Properties.

2	Enter the appropriate information in the boxes provided for: Author, Keywords, Comments, Title, and Subject.

Note:  If you insert a part identification number in the Title box, you can use that number automatically when you create a bill of materials in an assembly drawing that contains that part.

The system provides read-only Statistics about the document’s creation date, the date last saved, and the name of the person who saved the document last.

See also Bill of Materials .


Summary Info - Custom

Allows you to specify custom properties belonging to the part, assembly, or drawing document.

To enter custom properties:

1	Enter a Name for the property, or choose one from the list.

2	Select the Type of value the custom property will use.

3	Enter a Value for the custom property that is compatible with the selection in the Type box.

4	Click Add.

The Properties box displays the name, value and type of the custom properties.

To modify custom properties:

1	Click the property in the Name box that you want to change.

2	Edit the Type or Value as needed.

3	Click Modify.

To delete custom properties:

1	Click the property in the Properties box that you want to delete.

2	Click Delete.


Suppress

Suppresses a feature so you can work on the model with the selected feature temporarily omitted from the model. Features that are children of the selected feature are also suppressed.

To suppress a feature:

1	Select a feature in the FeatureManager design tree.

2	Click [image] or Edit, Suppress.

The feature disappears from the model view and its icon is grayed in the FeatureManager design tree.

Use Unsuppress or Unsuppress with Dependents to restore suppressed features.


Imported Surface

Imports IGES surfaces.

To bring in an IGES surface:

1	Open a new part file.

2	Click Insert, Reference Geometry, Imported Surface.

3	From the Open dialog box, select the IGES file to import and click Open.

See also Thicken Feature and With Surface .


Surface Cut

To select the direction in which you want to cut away the solid:

1	Examine the preview.

The arrow points in the direction of the solid to discard.

2	If necessary, click Flip the Side to Cut Away to reverse the direction of the cut.

3	Click OK.


Surface Finish Symbol

Attaches a surface finish symbol to the selected surface in a part, assembly, or drawing document.

To add a surface finish symbol to a part surface:

1	Click where you want to place the symbol.

2	Click [image] or Insert, Annotations, Surface Finish Symbol.

3	Construct the symbol that is appropriate for the selected surface by selecting values from the options in the Surface Finish Symbol dialog box:

•	Symbol. Select a symbol type from Basic, Machining Required, or Machining Prohibited.

•	Direction of Lay. Select the direction of the surface pattern from a pull-down list.

•	Roughness. Define the Maximum, and Minimum height deviation from the mean plane of the surface, and the Spacing between peaks and valleys that form the texture of the surface.

•	Special Requirements. Define any necessary requirements such as: Production Method/Treatment, Sampling Length, or Other Roughness Values.

•	Material Removal Allowance. Define the amount of stock to be removed by machining.

•	Leader. Check the Show Leader box to display the symbol with a leader.

•	Bent Leader. Check this box to allow the leader to have a bend.

•	Arrow Style. If a leader is displayed, you can choose the type of leader end from a pull-down list.

4	Click Rotated if you want the symbol rotated 90 degrees.

5	Click OK when you are satisfied with the surface finish symbol you defined.

To edit the surface finish symbol, right-click the symbol and select Properties from the menu, or double-click the symbol. Make changes to the Surface Finish Symbol dialog box.


Sweep Feature

Creates a feature that adds or removes material by projecting a profile along an open or closed sketched path or a model edge.

To create a simple sweep:

1	Sketch a closed, non-intersecting profile on a face or a plane, then close the sketch.

2	On another face or plane, sketch a non-intersecting sweep path that the profile will follow. Close the path sketch

The start point of the path must lie on the plane of the profile. (You may also use an existing model edge or reference curve).

3	If you are creating the first feature in a new part, click Insert, Base, Sweep. Otherwise, click Insert, Boss, Sweep or Insert, Cut, Sweep.

4	In the Sweep dialog box, click the Sweep Section box, then select the section profile either in the model or in the FeatureManager design tree.

5	Click the Sweep Path box, then select the sketch, edge, or curve that you want to use as the path.

6	Under Orientation/Twist Control:

•	Select Follow Path if you want the section to remain at the same angle with respect to the path at all times.

•	Select Keep Normal Constant if you want the section to remain parallel to the beginning section at all times.

7	If you picked an edge as the path, and you want to continue the sweep along all tangent edges, click Propagate Along Tangent Edges.

8	If you want to continue the sweep profile up to the last face encountered at the ends of the path, click Align with End Faces.

9	Click OK.

See also Guide Curve Sweep


Sweep

1	Click the Sweep Section box, then select the section profile either in the model or in the FeatureManager design tree.

2	Click the Sweep Path box, then select the sketch, edge, or curve that you want to use as the path.

3	Under Orientation/Twist Control:

•	Follow Path. Causes the section to remain at the same angle with respect to the path at all times.

•	Keep Normal Constant. Causes the section to remain parallel to the beginning section at all times.

•	Follow Path and 1st Guide Curve. The angle between the section and the path remains the same along the length of the path, and the twist is based on a vector between the path and the first guide curve. (For Guide Curve Sweep only)

•	Follow 1st and 2nd Guide Curve. The angle between the section and the path remains the same along the length of the path, and the twist is based on a vector between the first and second guide curves. (For Guide Curve Sweep only)

4	If you picked an edge as the path, and you want to continue the sweep along all tangent edges, click Propagate Along Tangent Edges.

5	If you want to continue the sweep profile up to the last face encountered at the ends of the path, click Align with End Faces.

6	Click OK to create the sweep, or click the Advanced tab to specify guide curves, or click Cancel.


Sweep - Advanced

1	Click the Guide Curve(s) box, then select the guide curve(s). Use the Up and Down buttons to rearrange the order of the guide curves if needed.

2	Under certain conditions, these additional options for sweeps with guide curves are available:

•	Maintain Tangency. If the sweep section has tangent segments, checking this option causes the corresponding surfaces in the resulting sweep to be tangent.

•	Advanced Smoothing. If the sweep section has circular or elliptical arcs, the sections are approximated, resulting in smoother surfaces.

3	To view the modifications in the profile as it moves along the path, click Show Intermediate Profiles. Use the arrows beside the Profile Number box to scroll through the profiles. (You can activate this option before creating the sweep, or by editing the definition of the sweep after it is created.)

4	Click OK to create the sweep, or click Cancel.


Guide Curve Sweep

Uses guide curves to control the intermediate profiles as the sketch is swept along the path.

To create a sweep using guide curves:

1	Create the guide curve(s), either as a sketch, a reference curve, or a model edge.

2	Create a path for the sweep. This also can be a sketch, reference curve or model edge.

3	Sketch the sweep section on a plane that is normal to the end of the sweep path.

Important: Create the profile after the path and guide curve(s). The intermediate profiles of the sweep are dependent on both the path and guide curves for their definition.

Pay special attention to the use of Horizontal or Vertical relations. Because of the way the section changes as it sweeps along the path, you may need to adjust the Orientation/Twist Control to achieve the desired effect.

4	Create Pierce relations in the profile sketch, where the guide curve intersects the profile at a vertex or a sketch point.

5	If you are creating the first feature in a new part, click Insert, Base, Sweep. Otherwise, click Insert, Boss, Sweep or Insert, Cut, Sweep.

6	On the Sweep tab, click the Sweep Section box, then select the profile sketch in the FeatureManager design tree or in the graphics area.

7	Click the Sweep Path box, then select the path sketch, curve, or model edge.

8	Under Orientation/Twist Control:

•	Follow Path and 1st Guide Curve. The angle between the section and the path remains the same along the length of the path, and the twist is based on a vector between the path and the first guide curve.

•	Follow 1st and 2nd Guide Curve. The angle between the section and the path remains the same along the length of the path, and the twist is based on a vector between the first and second guide curves.

9	On the Advanced tab, click the Guide Curve(s) box, then select the guide curve(s). Use the Up and Down buttons to rearrange the order of the guide curves if needed.

10	Under certain conditions, these additional options for sweeps with guide curves are available on the Advanced tab:

•	Maintain Tangency. If the sweep section has tangent segments, checking this option causes the corresponding surfaces in the resulting sweep to be tangent.

•	Advanced Smoothing. If the sweep section has circular or elliptical arcs, the sections are approximated, resulting in smoother surfaces.

11	To view the modifications in the profile as it moves along the path, click Show Intermediate Profiles. Use the arrows beside the Profile Number box to scroll through the profiles. (You can activate this option before creating the sweep, or by editing the definition of the sweep after it is created.)

12	Click OK.

See also Notes on Creating Sweeps with Guide Curves


Notes on Creating Sweeps with Guide Curves

•	The path and the guide curves may differ in length. The sweep length is determined by the shortest overlapping distance between the path and all the guide curves.

•	Guide curves may meet at a common point, which is the apex of the swept surface.

•	If a profile is symmetrical, symmetry is maintained even as the section varies due to the guide curve.

•	If a guide curve has no Pierce relation with a sketch point, no edge on the sweep will follow the guide curve.

•	You can use sketched curves, model edges, or reference curves of any kind as guide curves.


Tangent Arc

Creates an arc, tangent to a sketch element.

To create a tangent arc:

1	Click [image] or Tools, Sketch Entity, Tangent Arc.

2	Press the mouse button over the end point of a line, arc, ellipse, or spline.

3	Drag out the arc to the desired shape.

4	Release the mouse button.


Tangent Edges Visible

In a model, assembly, or drawing document, if you selected Hidden in Gray or Hidden Lines Removed, you can choose to display tangent edges as a solid line.

To display tangent edges as a line:

Click View, Display, Tangent Edges Visible. The transition edge between rounded or filleted surfaces displays as a line.


Tangent Edges with Font

In a drawing document, if you selected Hidden in Gray or Hidden Lines Removed, you can display tangent edges with the default line font that you select in Tools, Options, Edges.

To display tangent edges with font:

Click View, Display, Tangent Edges With Font. The transition edge between rounded or filleted surfaces displays as a line using the default font for tangent edges defined in Tools, Options, on the Line Font page.


Tangent Edges Removed

In a model, assembly, or drawing document, if you selected Hidden in Gray or Hidden Lines Removed, you can choose to not display lines for tangent edges.

To not display tangent edges:

Click View, Display, Tangent Edges Removed. The transition edge between rounded or filleted surfaces and other surfaces is not displayed.


Tangent Edges as Phantom

In a model or assembly document, if you selected Hidden in Gray or Hidden Lines Removed, you can select Phantom lines for tangent edges.

To display tangent edges as phantom lines:

Click View, Display, Tangent Edges as Phantom to display the transition edge between rounded or filleted surfaces as a line using the Phantom style line font ( [image]).


Temporary Axes

Displays all temporary axes in a part or assembly.

To display temporary axes:

Click View, Temporary Axes.

Note:	Every cylindrical entity has a axis; axes of this type are temporary. To convert a temporary axis to a reference axis, click Insert, Axis. See Reference Axis.


Edit Thicken

Changes the thickness or direction of the thickness feature on the surface of an imported IGES part.

To change the thicken feature:

1	Right-click the feature’s name in the FeatureManager design tree and select Edit Definition from the menu.

2	Change the Thickness value as necessary.

3	Select either Thicken Side 1, Thicken Side 2, or Thicken Both Sides.

4	View the preview graphic and click OK when you are satisfied.


Text

Creates text on a part as either an extruded boss or a cut.

Note:	Text aligns with the x-axis of the sketch plane and proceeds in the direction of the increasing x value.

To insert text on a model face:

1	Click a model face where you want to insert text, and open a new sketch.

2	Click Tools, Sketch Entity, Text.

The cursor becomes a “Note” cursor.

3	Click on the model face where you want the text to begin.

The Text dialog box opens.

4	Type your text into edit box.

5	Click the checkbox to use the document’s default font, or click the Font button and choose a font style and size. The text displays in the fonts that you select.

6	Click the arrows next to the Scale box to increase or decrease the scale of the text.

7	Click OK when you are satisfied with the appearance of the text.

8	To change the orientation or location of the text before extruding it:

•	Exit the sketch and click Tools, Sketch Tools, Modify. or [image]. The cursor changes to the shape of a mouse. The left mouse button moves the text, the right mouse button rotates the text.

•	Use the mouse to position the text.

•	When you are finished, click Tools, Sketch Tools, Modify. or [image] again.

1	Click Insert, Boss, Extrude or Insert, Cut, Extrude, and set the Depth value.

2	Click OK to extrude the text.

See also:

  To move extruded text

  To edit extruded text


Editing Extruded Text

To edit extruded text:

1	Right-mouse click the text sketch in the FeatureManager design tree and select Edit Sketch.

2	Right-mouse click on the text and select Properties from the menu.

3	Change the text or the font and click OK.

4	Exit the sketch and click Edit, Rebuild or [image].


Moving Extruded Text

To change text orientation and location after making the extrusion:

1	With the sketch closed, select the text sketch in the FeatureManager design tree.

2	Click Tools, Sketch Tools, Modify or [image].

The cursor changes to the shape of a mouse; the left mouse button moves the text, the right mouse button rotates the text.

3	Using the mouse, position the text.

4	Click Tools, Sketch Tools, Modify or [image] to exit.

5	Click Edit, Rebuild or [image].


Thicken Feature

Thickens a selected reference surface.

To thicken a surface:

1	Click the surface(s) that you want to thicken.

2	Click Insert, Base (or Boss), Thicken.

3	Change the Thickness value as necessary.

4	Select either Thicken Side 1, Thicken Side 2, or Thicken Both Sides.

5	View the preview graphic to see if your selection is correct for your purpose.

6	When you are satisfied with your selection, click OK.

To cut an existing solid by thickening a surface:

1	Select the surface and the solid to be cut.

2	Click Insert, Cut, Thicken.

3	Change the Thickness value as necessary.

4	Select either Thicken Side 1, Thicken Side 2, or Thicken Both Sides.

5	View the preview graphic to see if your selection is correct for your purpose.

6	When you are satisfied with your selection, click OK.

To change the thickened or cut feature, right-click the feature’s name in the FeatureManager design tree and select Edit Definition from the menu.

For information about creating a reference surface, see Extruded Surface , Revolved Surface , Swept Surface , Lofted Surface , and Offset Surface .

To import an IGES surface, see Imported Surface .


Thin Feature

The thin features dialog box lets you define the characteristics of extruded thin features..

•	Type. Type lets you specify whether to extrude the thin feature in One Direction, Mid-plane, or Two Directions.

•	Wall Thickness. Use the spin box to specify the thickness of the thin feature wall.

•	Reverse. Lets you reverse the extrusion of the wall thickness.

If you created a closed profile you can select the following options:

•	Cap Ends. Specifies that the ends of the thin feature are capped. A capped thin feature must be extruded from a closed profile sketch.  When the ends are capped, all walls of the feature are closed; the center is hollow.

•	Cap Thickness. Lets you specify the thickness of the cap. (Available only if Cap Ends is selected.)

If you created an open profile you can select the following options:

•	Auto Fillet. Automatically creates a round at each edge where lines meet at an angle.

•	Fillet Radius. Specifies the inside radius of the round.


Three Point Arc

See 3 Point Arc.


Three Point Plane

To create a plane through three points:

1	Select three vertices or points while holding the Ctrl key.

2	Click Finish.


Curve Through Reference Points

Creates a 3D spline curve through points or vertices located on one or more planes. You can use this curve as a path for a sweep or as a guide curve for a loft or sweep.

To create a curve through points:

1	With a sketch active, use [image] (the point tool) to place points to guide the curve, or use existing vertices.

2	Close the sketch.

3	Select a different plane and open a new sketch.

4	Place additional points on the second plane and close the sketch.

5	Click Insert, Reference Geometry, Curve Through Reference Points.

The Curve dialog box opens.

6	Click the Spline Points box, then select the points and/or vertices in the order in which you want to create the curve. You can use the arrow keys to rotate the view to assist in selecting the points.

As you select, the number of sketch items and/or vertices is listed in the Spline Points box.

7	If you want to close the curve, click the Curve Closed box.

8	Click OK to create the curve.


Curve Through Free Points or From a File

Creates a 3D spline curve from a set of points. There are two ways to generate a point list for this purpose:

 You can create a curve one point at a time , observing the effect on the resulting curve as you go along.

 You can use previously created text file containing a list of points.


Curve Through Free Points

To create a curve one point at a time:

1	Click Insert, Reference Geometry, Curve Through Free Points.

2	In the Curve File dialog box, double-click any cell in the first row to activate the cell.

3	Enter the coordinates for X, Y, and Z (double-click to activate each cell). Notice that the value in the Point column automatically is set to 1. The numbers in the Point column define the order in which the points will be connected.

4	Double-click in the next row, and enter the coordinates. Notice the preview of the curve in the graphics area.

5	Repeat Step 4 to continue adding as many points as needed. The larger the number of points, the greater your control of the resulting curve.

6	If necessary, you can insert a new point between existing points. Drag the cursor across the cells to select the row where you want the new point to occur, then click Insert. A new row is added, and all the points below the selected row move down.

7	If desired, you can save the curve file for re-use. Click Save or Save As, navigate to the desired location, and specify the filename. If you do not specify an extension, the SolidWorks application adds the extension .sldcrv.


Curve From a File

To create a curve from a file:

1	Create a point file using a text editor, spreadsheet, or other utility. (Save spreadsheet data as a text file.) The point file should be a three-column, tab- or space-delimited list of X, Y, and Z coordinates.

Note:	Created outside of a sketch, the X, Y, and Z coordinates are interpreted with respect to the Plane1 coordinate system.

2	Click Insert, Reference Geometry, Curve Through Free Points.

3	Use the Browse button to locate the file, then click Open.

4	The coordinates from the file are displayed in the Curve File dialog box. Notice the numbers in the Points column, indicating the order in which the points will be connected.

5	Examine the preview of the curve, and edit the coordinates if necessary, until you are satisfied with the result. Double-click in any cell, then edit the value.

6	Click OK.


Curve File

•	To open and use a previously created text file of points, click the Browse button and locate the file you want to use.

- or -

Create new set of coordinates by double-clicking cells in the X, Y, and Z columns and  entering a point coordinate in each one. (Created outside of a sketch, the X, Y, and Z coordinates are interpreted with respect to the Plane1 coordinate system.)

Note:	The numbers in the Point column define the order in which the points are connected.

•	To change coordinates, double-click in a cell and enter a new value.  (As you enter values, notice the preview of the curve is displayed in the graphics area.)

•	To add a new row, double-click in a cell in the row below the last numbered row.

•	To insert a new row, drag the cursor across a row to select it, then click the Insert button. A new row is inserted above the selected row.

•	To delete a row, drag the cursor across a row to select it, then press the Delete key.

•	Examine the preview of the curve until it is satisfactory, then click OK to create the spline curve.

•	To save the curve file for re-use. Click Save or Save As, navigate to the desired location, and specify the filename. If you do not specify an extension, the SolidWorks application adds the extension .sldcrv. (You can also use .txt as the extension.)

Note:	The curve file must be in text format.  You can use spaces or tabs between the columns of X, Y, and Z coordinates.  An easy way to create the file in the correct format is to use the Notepad accessory supplied with Windows.


Curve

1	While holding the Ctrl key, select sketch points in the order in which you want to create the curve. Use the arrow keys to rotate the view to assist in selecting the points.

As you select, the number of sketch items and/or vertices is listed in the Spline Points box.

2	If you want to close the curve, click the Curve Closed box.

3	Click OK to create the curve.


Tile Horizontally -- Tile Vertically

Arranges and shrinks the open SolidWorks document windows so they are all visible.

To tile the document windows:

Click Window, Tile Horizontally to display the windows horizontally on your screen.

Click Window, Tile Vertically to display the windows vertically on your screen.

Note:  If you have many SolidWorks documents open, the display will be both vertical and horizontal.


Toolbars

Displays or hides toolbars. See Standard, View, Sketch, Sketch Tools, Sketch Relations, Macro, Dependency Editing,  Features, Assembly ,Drawing,  Web toolbars and Selection Filter .

To display or hide a toolbar:

1	Click View, Toolbars.

2	Click the checkboxes to select each toolbar you want to display.

3	Click OK to make the changes and close the dialog; or click Cancel.

To move a toolbar:

Toolbars can be either "docked" (attached to one of the edges of the SolidWorks window) or "floating."

1	Point at the space between the buttons on the toolbar and drag the toolbar to the desired location. If you drag it to an edge of the SolidWorks window, the toolbar docks to that edge automatically.

2	To change a toolbar’s orientation (from horizontal to vertical), drag the toolbar near a horizontal or vertical edge of the window before placing it in the desired location.

To display large size toolbar buttons:

Click View, Toolbars and select Large Buttons from the Toolbars dialog box.

To show tooltips:

Click View, Toolbars and select Show Tooltips from the dialog box. When checked, a small note pops up to identify each tool icon that you pause your cursor over.

For information about customizing your toolbars, see Customize Toolbars .


Trim/Extend

Trims or extends a sketch element.

Use Trim/Extend to:

•	Trim a line, arc, ellipse, or circle to its intersection with a line, arc, circle, ellipse, spline, or centerline.

•	Extend a line, arc, or centerline to meet a line, arc, circle, ellipse, spline, or centerline.

•	Delete the portion of a line that lies between two intersecting lines.

To trim a sketch element:

1	Click [image] or Tools, Sketch Tools, Trim/Extend.

2	Click the portion of the sketch element you want to remove.

To extend a sketch element:

1	Click [image] or Tools, Sketch Tools, Trim/Extend.

2	Click on an endpoint of a sketch element that you want to extend (a line, arc, or centerline).

3	Drag the endpoint to a second sketch element. When the second element is highlighted, release the mouse button; the first element will extend to meet the second.

To extend one or two endpoints -- a shortcut:

1	Click [image] or Tools, Sketch Tools, Trim/Extend.

2	Hold the Ctrl key and click the sketch element you want to extend (line, arc, or centerline).

The sketch element extends to intersect with the next sketch element that is available. It extends both ends of the sketch element if there are possible intersections at both ends.

If there are other possible intersections with additional sketch elements beyond the first intersection, repeatedly Ctrl-clicking the extending sketch element causes it to continue to grow until there are no more sketch elements with which it can intersect.


Undo

Reverses recent changes you have made, when possible.

To undo your last action:

Click [image] or Edit, Undo, or press Ctrl-Z.

To Undo multiple operations:

1	Click [image] (to the right of the Undo button) to see the list of actions that are available to undo. The most recent actions are at the top of the list.

2	Click on any action on the list. The action you select and all actions above it on the list are reversed.

Note:  Use Undo if your sketch pulls out of shape when you drag an edge.

See also VIEW_ORIENTATION for a description of using the Undo option on the View Orientation box to undo view rotation, translation, and scale.


Unsuppress

Unsuppresses a suppressed feature.

If the feature has suppressed parents, the parents will also be unsupressed.

To unsuppress a feature:

1	Select the suppressed feature in the FeatureManager design tree.

2	Click [image] or Edit, Unsuppress.


Unsuppress with Dependents

Unsuppresses a feature and all its dependents.

To unsuppress a feature and its dependents:

1	Select the suppressed feature in the FeatureManager design tree.

2	Click [image] or Edit, Unsuppress with Dependents.


Update Units

You made a change to the units of measure used in this document.  Review the changes indicated in this dialog box.

Click OK to accept the changes and close the dialog.

- or -

Click Cancel to close the dialog without saving any changes.


Options

Allows you to customize SolidWorks options and set default values.

To set preferences:

1	Click Tools, Options.

2	Click on the appropriate tab (General, Color, and so on) for the settings you want to change.

3	Change the settings and click OK.

See General, Color , Edges, Import/Export Settings , External References , Material Properties , Performance, Grid/Units , Line Font, Detailing, Crosshatch, Drawings, and Planes  options.


Vertical Break

Creates a broken view (or an interrupted view) on the drawing of a long part that has a uniform cross-section. This makes is possible to display the part in a larger scale on a smaller size drawing sheet

To create a break line in a drawing:

1	Select the drawing view and click Insert, Vertical Break.

Two break lines appear in the view.

2	Drag the break lines to where you want the breaks to occur.

3	Right mouse click inside the view border (green border) and select Break View from the menu.

The part is displayed with a gap in the part geometry; however, the dimensional values associated with the broken area reflect the correct values.

You can continue to drag the break lines to adjust them after the view is broken, if necessary.

To change the shape of the break lines, right mouse click a break line and select a line style from the menu: Straight Cut, Curve Cut or Zig Zag Cut.

To specify the width of the break gap, click Tools, Options, and select the Detailing tab. Enter a value in the Break Gap box under the Break Lines option.

See also Horizontal Break .


Vertical Dimension

Creates a vertical dimension between two points. (The vertical direction is defined by the orientation of the current sketch.)

To create a vertical dimension:

1	Click Tools, Dimensions, Vertical.

2	Click the two points to dimension.

3	Click a location to place the dimension.


Vertical Ordinate Dimension

Creates vertical ordinate dimensions in a drawing, measured vertically from the entity you select first.

To create vertical ordinate dimensions:

1	With a drawing active, click [image] and select Vertical Ordinate from the right-mouse menu.

– or –

Click Tools, Dimensions, Vertical Ordinate.

2	Click the first item from which all others will be measured, and click again to place the dimension.

3	Click an item to dimension, then click to place its dimension. Repeat this step until all the remaining items are dimensioned. The dimension tool remains in ordinate mode until you select another mode or another tool.

See also  Ordinate Dimension ,  Align Ordinate , Horizontal Ordinate Dimension.


Web Toolbar

Displays or hides the Web toolbar.

To access the Web toolbar when it is hidden:

Click [image] on the Standard toolbar to display the Web icons.

Click [image] again to hide the Web toolbar when it isn’t needed.


Weld Bead

Adds a weld bead to components.

To add a weld bead to components in an assembly:

1	Mate the components.

2	Click Insert, Assembly Feature, Weld Bead.

3	In the Weld Bead Type dialog box, select the desired weld bead type from the list. Notice the symbol and the illustration for the selected type.

4	Click Next.

5	In the Weld Bead Surface dialog box:

•	In the Surface Shape box, select the desired surface shape.

•	In the Top Surface Delta box, enter the desired top surface delta.

•	If you selected Backing Run type, enter the Bottom Surface Delta.

•	If you selected Fillet type, enter the Radius.

6	Click Next.

7	In the Weld Bead Mate Surfaces dialog box, select faces as follows:
(required selections depend on the Weld Bead Type you chose.)

•	Click in the Contact Faces box. Select the faces of the components where you want the weld bead to be added.

•	Click in the Stop Faces box. Select the faces (usually four faces) where you want the weld bead to start and stop.

•	Click in the Top Faces box. Select the faces from which to measure the Top Surface Delta.

8	Click Next.

9	In the Weld Bead Part dialog box, accept the default weld bead part name (bead1.sldprt, for example) or rename the part as desired. Click Browse if you want to save the weld bead part to a different directory.

10	Click Finish.

The new bead component is created and added to the assembly.

To change the weld bead parameters:

1	Expand the bead component in the FeatureManager design tree.

2	Right-click the WeldBead feature and select Edit Definition.

3	Repeat Steps 3 through 10 making changes as desired.


Weld Bead Type

1	Select the desired weld bead type from the list. Notice the symbol and the illustration.

2	Click Next.


Weld Bead Surface

1	In the Surface Shape box, select the desired surface shape.

2	In the Top Surface Delta box, enter the desired top surface delta.

If you selected Backing Run type, enter the Bottom Surface Delta.

If you selected Fillet type, enter the Radius.

3	Click Next.


Weld Bead Mate Surfaces

1	Select the mate faces. Selections required depend on the Weld Bead Type you chose.

•	Click in the Contact Faces box, then select the faces of the components where you want the weld bead to be added.

•	Click in the Stop Faces box, then select the faces (usually four faces) where you want the weld bead to start and stop.

•	Click in the Top Faces box, then select the faces from which to measure the Top Surface Delta.

2	Click Next.


Weld Bead Part

1	Accept the default weld bead part name or rename the part as desired. Click Browse if you want to save the weld bead part to a different directory.

2	Click Finish.


Weld Symbols

Creates symbols to provide weld specifications on your part, assembly, and drawing documents.

To create a weld symbol:

1	Click an edge on the part or assembly where you want to indicate a welded joint.

2	Click [image] or Insert, Annotations, Weld Symbol.

3	In the Dimension boxes, enter the values for the weld dimensions.

4	Click the Weld Symbol button and select a symbol type from the list of standard symbols.

5	Choose other options as needed, such as Symmetric, Peripheral, Field or site weld, or Contour.

6	To specify the welding process, click Indication of welding process and enter the text in the box.

7	Choose a Leader Anchor style.

The symbol is displayed in the preview box as you select symbols and add appropriate dimensions and values.

8	Click OK.


ANSI Weld Symbol

Creates symbols to provide weld specifications on your part, assembly, and drawing documents.

To create a weld symbol:

1	Click an edge in the drawing view  where you want to indicate a welded joint.

2	Click [image] or Insert, Annotations, Weld Symbol.

3	In the boxes beside the Weld Symbol button, enter the weld dimensions.

4	Click the Weld Symbol button and select a symbol type from the list of standard symbols.

5	Specify other options as needed, such as Finishing Method, Contour, Joint with Spacer, Groove angle, Root opening, or Field or site weld.

6	To specify the welding process, click Specification process and enter the text in the box.

7	Choose a Leader Anchor style.

The symbol is displayed in the preview box as you select symbols and add appropriate dimensions and values.

8	Click OK.


Wireframe

Displays all the edges of the model.

To display the model in wireframe:

Click [image] or View, Display, Wireframe.


Witness/Leader Display

Controls the display of witness lines and leader lines.

•	Click the check boxes to select or deselect the Witness Lines display options for the first and second witness lines.

•	Click the check boxes to select or deselect the Leaders display options for the first and second leader lines.

•	Click the check boxes to select or deselect the Display with broken leaders or Smart display of witness lines options.

You can observe the behavior of the lines in the Preview box as you select and deselect the display options.

Click OK to accept the display you selected, or click Cancel to exit without accepting.


With Surface

Creates a cut through a solid with a surface.

To cut with a surface:

1	Insert a surface into an active part document.

2	Create a sketch and extrude a base around the imported surface.

The surface should extend to both edges of the solid, or beyond.

3	Select the surface and click Insert, Cut, With Surface.

4	Select the direction of the cut.

5	Click OK.

For information about creating a reference surface, see Extruded Surface , Revolved Surface , Swept Surface , Lofted Surface , and Offset Surface .

To import an IGES surface, see Imported Surface .


Zoom In/Out

Zooms in and out.

To zoom in or out:

1	Click [image] or View, Modify, Zoom In/Out.

2	Press the mouse button and drag up (toward the top of the screen) to zoom in, or drag down to zoom out.

Tip	Press z to zoom out or Shift-Z to zoom in.


Zoom to Area

Zooms in on a portion of the view that you select by dragging a bounding box.

To zoom in to a selected view:

1	Click [image] or View, Modify, Zoom to Area.

2	Point at one corner of the area you want to enlarge.

3	Press the mouse button and drag the bounding box diagonally to enclose the area.

4	Release the cursor.


Zoom to Fit

Zooms in or out so the entire model, assembly, or drawing sheet is visible.

To see the entire model:

Click [image] or View, Modify, Zoom to Fit.


End Condition

The End Condition dialog lets you define the characteristics of extruded features created with the Extrude, Simple Hole, or Hole Wizard functions:

•	Type determines how far the feature extends.

If you choose Blind or Mid-Plane, specify the Depth.

If you choose Offset from Surface, specify the Offset dimension. Click Reverse Offset, if appropriate.

•	Reverse Direction. Lets you extend the feature in the opposite direction from that shown in the preview.

•	Flip Side to Cut. Appears only when you are extruding a cut. By default, material is removed from the inside of the profile. Flip Side lets you sketch the portion that you want to remain, and remove all material outside of the profile.

•	Draft While Extruding.  Lets you add a draft to a feature while you extrude it. Set the draft Angle, and check Draft Outward, if necessary.

•	Selected Items. If the Type that you specified relies on the selection of a surface or vertex, click that item now in the graphics area. The selection is displayed in the Selected Items box.

•	Both Directions. Lets you extend the feature in both directions from the sketch plane.

•	Settings for: Lets you specify the settings for Direction 1, then, if you specified Both Directions, scroll to Direction 2 and specify the settings for the second direction.

•	Extrude As: Select either Solid Feature or Thin Feature.

If you select Solid Feature, click OK to complete the extrusion.

If you select Thin Feature, click the Thin Feature tab at the top of the dialog box and complete the specification of the feature on the next page. See Thin Feature .


End Condition

1	 Select the hole Type to determine how far the feature extends.

•	If you choose Blind or Mid-Plane, specify the Depth.

•	If you choose Offset from Surface, specify the Offset dimension. Click Reverse Offset, if appropriate.

2	To extend the feature in the opposite direction from that shown in the preview click Reverse Direction.

3	If you selected Up to Surface, Offset from Surface, or Up to Vertex, you must select a surface or vertex. View the Selected Item box to be sure your selection is complete.

4	Click Next.


End Type

The Type determines how far an extruded feature extends.

Blind	Extends the feature from the sketch plane for a specified distance. • Specify a Depth.
Through All	Extends the feature from the sketch plane through all existing geometry.
Up to Next	Extends the feature from the sketch plane to the next surface that intercepts the entire profile. (The intercepting surface must be on the same part.)
Up to Surface	Extends the feature from the sketch plane to the selected surface. • Click on a face to specify the surface.
Offset from Surface	Extends the feature from the sketch plane to a specified distance from the selected surface. • Click on a face to specify the surface. • Specify an Offset.
Mid Plane	Extends the feature from the sketch plane equally in both directions. • Specify a Depth. (This is the total depth of the extrusion, not the depth in each direction.)
Up to Vertex	Extends the feature from the sketch plane to a plane that is parallel to the sketch plane and passing through the specified vertex.


Arc Properties

Start Point, End Point, and Center Point. The X, Y, Z coordinates of the start point, end point, and center point.

Radius and Angle. The radius and angle of the arc.

Defined Status. Indicates whether the arc is currently underdefined or fully defined.

Construction Arc. Converts a sketched arc to a construction arc used in the creation of the model geometry.


Crosshatch Properties

Lets you make an immediate change to the crosshatch pattern for a surface, component, or view.

To change the crosshatch pattern for a surface, component, or view:

1	Right-mouse click on a crosshatched face in a part or assembly drawing.

2	Select a new crosshatch pattern.

3	View the changed crosshatch pattern in the Preview box.

4	Change the crosshatch angle and/or scale, if necessary.

5	Scroll the Apply To: box and select one of the available application modes:

View. All instances in the currently active section view.

Component. All faces on the currently selected component in an assembly.

Region. The currently selected surface only.

6	Click Apply to make the crosshatch change, or click Cancel.

7	Click OK to exit.

To remove the crosshatch for a specific layer (Region, Component, or View), select the layer and click the Remove Crosshatch check box. (The checkbox is only available for layers from which the crosshatch can logically be removed.)

The crosshatch is removed a layer at a time.  For example, if you remove the crosshatch from a region, any crosshatch applied earlier to the whole component is then revealed. If you remove crosshatch from a component,  the default crosshatch for the view is revealed.

See also Crosshatch Preferences .


Dimension Properties

To access the dimension properties dialog:

Right-mouse click a dimension and select Properties.

You can view and/or make changes to the following options:

Value. The current value of the dimension. To change, select the value and enter a new value or use spin box arrows.

Name. The name of the dimension (used in equations and design tables). To change, select the name and enter a new name.

Full Name. The dimension name plus the name of the feature or sketch the dimension is associated with. (Read only)

Arrows

•	Sets style of dimension arrows: Open, Filled, or Simple arrows, Slash Mark, or Filled Dot, Open Dot, or None.

•	Sets placement of arrows: Inside, Outside, Smart Arrows, or Follow Document.

(Smart Arrows specifies that arrows automatically appear outside of witness lines if the space is too small to accommodate the dimension text and the arrowheads.)

Display Precision

•	Use document’s precision. When checked, the default precision selected for the document is used.
When not checked, allows you to specify the precision with the Dimension Precision dialog box.

Font

•	Specifies either:

Use document’s font,

or provides a Font button that allows the selection of a new font type, style, and size. See Choose Font.

Display…

•	Lets you control the display of dimension lines and witness lines. See Witness/Leader Display .

Modify Text...

•	Lets you modify the dimension by adding Prefix or Suffix text and symbol(s). See Modify Text of Dimension.

Tolerance...

•	Lets you modify the dimension tolerance display and values.  See Dimension Tolerance Properties.

Driven. Specifies that the dimension of a sketch curve is driven by other dimensions and conditions.

Read Only. When checked, specifies that the dimension cannot be changed.

Display with parenthesis. Specifies whether to display reference dimensions in a drawing with parenthesis.

Diameter dimension. Specifies that arc dimensions are always diameter dimensions and not radius dimensions. Note: To convert a diameter dimension to a radius dimension, deselect this checkbox.

Display second arrow. Specifies that a second arrow is used for radial dimensions when Outside arrows are selected.

Foreshortened radius. Specifies that the radius dimension line is foreshortened when the centerpoint of a radius is outside of the drawing or interferes with another drawing view.

Dimension to inside of arc. Specifies that dimensions to arcs are always to the inside of the arc.

Display as chain dimension. Displays ordinate dimensions with an arrow from the base point to the dimension position. The measurement of the dimensions is from the base ordinate (the 0.0 mark). (These dimensions look best when all ordinates are aligned.)

Display as Dual Dimension. Allows the display of dimensions in two kinds of units.

Display with solid leader. Specifies the display of dimensions with solid leaders.

Display as linear dimension. Allows the display of a radius dimension as a linear dimension.

When you are dimensioning arcs and circles to each other, the following options are available:

First Arc Condition:  Center, Min, Max.  Allows you to select the first arc dimension parameter that provides the dimension you want.

Second Arc Condition:  Center, Min, Max. Allows you to select the second arc dimension parameter that provides the dimension you want.


Dimension Tolerance

Tolerance Display. Lets you specify the type of tolerance to display: None, Basic, Bilateral, Limit, Symmetric, MIN, MAX or Fit.

Tolerance Values. Lets you specify the Maximum Variation and/or Minimum Variation values as appropriate for the type of tolerance that you selected.

Linear or Angular Tolerance. Indicates the type of dimensions to which the current changes apply.

Font. Lets you specify the font to use for the dimension tolerance text.

•	Click Use dimension’s font if you do not want to change the font size for the dimension tolerance text.

•	To change the size of the dimension tolerance text, select either

•	Font Scale. Enter a number from 0 to 10.0 to scale the font.

•	Font Height. Enter a value to specify the font height.

Click OK to accept your changes and close the dialog; click Cancel to close the dialog without saving any changes.


Feature Properties

Name. The name of the feature. To change the name, select it and enter a new name.  Click OK.

Suppressed. Indicates whether the feature is currently suppressed.

Created By. The system name of the person who created the feature.

Date Created. The date and time when the feature was created.

Last Modified. The date and time when the part was last saved.

Color.  Click this button to change feature colors through the Entity Properties dialog box. (To change transparency or shininess, use the Advanced button in the Entity Property dialog box.)


Material Properties

Specifies the material properties of the selected part.

To specify material properties:

1	Click Tools, Options and click the Material Properties tab.

2	Select the text in the Properties, Density box, and enter the appropriate density specification.

3	Click OK to accept the changes; click Cancel to discard the changes and exit the dialog box; click Reset All to return to the installed system defaults.


Line Properties

Start Point and End Point. The X, Y, Z coordinates of the start point and end point.

Length. The length of the line.

Defined Status. Indicates whether the line is currently underdefined or fully defined.

Construction Line. Check the box to convert the sketch line to a construction line.


Reference Geometry Properties

Name. The name of the plane or axis. To change the name, select it and enter a new name. Click OK.


Resolve Ambiguity

Choose a file from the list and click OK or Cancel.


Section Arrows

1	Specify the Height, Width, and the Length of the section arrows used in drawings.

2	If you are using ANSI standards,  you have the option of selecting Alternate Section Display. With this type of display, the section line does not display across the drawing view; the arrow ends display appropriately at the ends of the section cut.

3	Click OK to apply your selection, or click Cancel.

Alternate Section Display

Normal Section Display


Section Line Properties

Label. The letter that is associated with this section line. Edit by selecting the letter and entering a new label.

Change direction of cut. Reverses the direction of the section line cut.

Scale with model changes. The section line changes size parametrically with the model. This could result in a section cut that is not what you intended, however. The default for this option is off.

Partial section. If the section line does not go all the way across the view, selecting this option causes the section view to include only the portion of the model crossed.

Display only surface cut. Displays a simplified view with surfaces behind the section line removed. Only the surface(s) cut by the section line are displayed in the section view.

Font. When checked, displays the same font style and size as the rest of the document. When not checked, allows you to click the Font button and specify the font style and size to use.


Spline Properties

Which Point. Click the arrows on the scroll box and the points of the corresponding spline segments are highlighted.  As the points are highlighted, the X, Y, Z coordinates of each segment are displayed.

Status. Indicates whether the spline is currently underdefined or fully defined.

Proportional.

•	When Proportional is selected, if you drag a spline endpoint the entire spline moves or resizes proportionately.

•	When Proportional is not selected, if you drag an endpoint only the local area of the spline changes shape.

•	Whether or not Proportional is selected, if you drag a spline point that is not an endpoint, only the local area of the spline changes shape.

Construction Spline. Check the box to convert the sketched spline to a construction spline.


General Options

To set general options:

1	Click Tools, Options.

2	Click on the General tab.

3	Select options from the following list and make the changes that you prefer.

4	Click OK to accept the changes; click Cancel to discard the changes and exit the dialog box; click Reset All to return to the installed system defaults.

Model

Input dimension value

Single command per pick

Show dimension names

Show errors every rebuild

FeatureManager Design Tree

Scroll selected item into view

Name feature on creation

Arrow key navigation

Dynamic highlight

View Rotation

Arrow keys

Mouse speed

Sketch

Use fully defined sketches

Alternate spline creation

Display arc centerpoints

Display entity points

Infer from model

Prompt to close sketch

Create sketch on new part

Enable silhouettes

Override dimensions on Drag

Automatic relations

Overdefining Dimensions

Prompt to set driven state

Set driven by default

General

Open last used documents at startup

Number of backup copies per document

Maximize on open

Use English language  Lets you change to using English if you specified another language during the SolidWorks installation.


Detailing Options

Lets you set properties for detailing and dimensioning in your parts, assemblies, and drawings.

To set detailing properties for all part, assembly or drawing documents:

1	Click Tools, Options.

2	Click the Detailing tab.

3	Change the detailing options to meet your standard detailing style, and click OK.

Dimensioning Standard

•	Specifies the standard to use: ISO, ANSI, DIN, JIS, and BSI.

•	Display with Broken Leaders. Specifies the display of dimensions with broken leaders.

•	Dual Dimensions Display. Allows the display of dimensions in two kinds of units.

•	Display datums per 1982.  Click this checkbox to use the 1982 standard for the display of datums.  Note:  Available only if you use the ANSI dimensioning standard.

•	Trailing Zeros. Select one of three settings:

Smart – Trailing zeros are trimmed for whole metric values. (Conforms to ANSI and ISO standards.)

Show – Dimensions have trailing zeros up to the number of decimal places specified in Tools, Options, Grid/Units .

Remove – All trailing zeros are removed. Specifies that metric whole dimensions have trailing zeros up to the number of decimal places specified.

Note:  Tolerances are not affected by this option.

Arrows

•	Specifies Height and Width of arrowheads, and Length of outside arrows.

•	Specifies style of dimension arrows (Open or Filled arrowheads, Simple Arrow, Open or Filled dots, Slash, or None).

•	Sets placement of dimension arrows in relation to the witness lines (Inside, Outside, or Smart.)

Note: Smart arrows appear outside of witness lines if the space is too small to accommodate the dimension and the arrowheads.

•	Display 2nd Outside Arrow (Radial). Specifies that two outside arrows are displayed with radial dimensions.

Break Lines

•	Break Gap.  Specifies the size of the gap between break lines in a broken view (or interrupted view) in a drawing.

Center Marks

•	Size. Specifies the size of Center Marks, used with arcs and circles in drawings.

•	Show Lines. Specifies whether the center mark lines are displayed.

Witness Lines

•	Sets the Gap and Extension of witness lines.

Datum Feature Symbols

Specify the letter of the alphabet that will be used for the next Datum Feature Symbol. The default letter is A. Successive labels are in alphabetic order.

Sections . Click this button to specify the Height, Length, and Width of section arrows. Note:  The Sections button is available when you are in a drawing.

Annotations Properties . Click this button to specify the annotations Display Filter and set annotations properties.

Dimensions

•	Dim Font. Lets you specify the font, font style and font size used for the text in dimensions. See Choose Font .

•	Tolerance. Specifies the type of tolerance to display: None, Basic, Bilateral, Limit, Symmetric, MIN, MAX or Fit. See Dimension Tolerance Properties .

•	Add Parentheses By Default. Specifies that reference dimensions in drawings are displayed within parentheses.

•	Snap Text to Grid. Specifies that the placement of dimension text snaps to the grid in a drawing or a sketch.

•	Use System Separator. Specifies that the default system decimal separator is used in the display of decimal numbers. (To set the system default use Control Panel, International (or Regional Settings), Number Format, Decimal Separator.) To set a decimal separator different from the system default, click to deselect, and enter the symbol that you want to use (usually the period or the comma).

•	Center text.  Specifies that the dimension text is centered between its witness lines.

•	Precision. Sets the dimension precision and tolerance values for  Primary Units, Angular Units, and Alternate Units.

Notes

•	Note Font. Lets you specify the font type and size used for notes.

•	Balloons . Lets you specify the balloon style, size, and text for Notes Balloons and BOM (bill of materials) Balloons.

•	Leader Anchor. Specifies to which side of the text the leader attaches: Left, Right, or the side Closest to the attach point.

•	Display Notes with Bent Leader. Specifies whether notes are displayed with a bent leader.

•	Bent Leader Length. Specifies the distance between the leader bend and the text of the note.

View System Defaults.

•	When checked, the system default for each of the options is displayed; when not checked the option selections used by the active document are displayed.

Apply To:  Select an option from the pull-down list, as follows:

•	System Defaults. Applies the selections that you made to all new documents that you create.

•	Active Document. Applies the selections that you made to only the currently active document.

•	All Possible. Applies the selections that you made to both the system defaults and currently active document.


Drawings Options

Lets you set options for drawings.

To set options for drawings:

1	Click Tools, Options.

2	Click the Drawings tab.

3	Change the options to meet your needs, and click OK.

Default Sheet

•	Sheet Scale. Specifies the default drawing scale for those cases when you choose No Template from the Template to Use dialog.

Type of Projection

Specifies either First Angle or Third Angle projection for those cases when you choose No Template from the Template to Use dialog.

Default Display

•	Specifies the way models or assemblies are displayed in drawings:

Wireframe – All edges are displayed.

Hidden in Gray – Displays visible edges normally; displays hidden edges in gray.

Hidden Lines Removed – Displays only edges that are visible at the chosen angle; obscured lines are removed.

•	If you selected Hidden in Gray or Hidden Lines Removed, select one of the following modes for viewing tangent edges:

Tangent Edges Visible – The transition edge between rounded or filleted surfaces displays as a line.

Tangent Edges With Font – The transition edge between rounded or filleted surfaces displays as a line using the default font for tangent edges defined in Tools, Options, on the Line Font page.

Tangent Edges Removed – The transition edge between rounded or filleted surfaces and other surfaces is not displayed.

Automatic placement of imported dimensions from model.

When checked, specifies that imported dimensions are automatically placed at an appropriate distance from the geometry in the view.

Display drawing view borders.

When checked, displays borders around individual drawing views.  This is the default.

Automatic scaling of 3 view drawings.

If checked, when you insert a Standard 3 View drawing, the three views are scaled to fit on the drawing sheet, regardless of the paper size selected.

Automatic update of BOM.

When checked, if a Bill of Materials exists in a drawing of an assembly it is automatically updated when relevant changes are made to the assembly.

Detail Item Snapping

•	Infer when dragging corner.  When you click a corner and drag a detail item (for example, a note or dimension), the corner you clicked can infer to the corners of stationary detail items, and vice versa.

•	Infer when dragging center.  When you click the inside of a detail item (a note or dimension) and drag it, the center can infer to the center of stationary detail items, and vice versa.

Detail View Scaling

Specifies the scaling for detail views. The scale is relative to the scale of the original drawing.


Import/Export

Specifies how SolidWorks files are translated for import and export.

To set options for importing and exporting files:

1	Click Tools, Options and select the Import/Export tab.

2	Change the settings and click OK if you are satisfied; click Reset All to return to the settings that you started with.

IGES

Output to

•	Settings For. Lists the format types for various mechanical design application programs to which SolidWorks can export IGES files: Standard, ANSYS, COSMOS, MasterCAM, SURFCAM, SmartCAM, and TEKSOFT.

•	Pop-up Dialog Box Before File Saving. If Trimmed Surfaces is also selected, the Settings For: list appears every time you save an IGES file so you can select a different format type. (You do not have to change the Options each time you export an IGES file to a new format.)

Output as

•	Trimmed Surfaces. Specifies the output of trimmed surfaces.

•	Curves (3D). Specifies the export of 3D curves. The solid body is converted to 3D wireframe representation. Select either B-Splines or Parametric Splines depending on the entity types required by the system to which you are exporting.

•	Duplicate Entities. Select this option to export composite curves (entity type 102) to any of the available export formats.

Trim Curve Accuracy

•	Normal. Select this option when smaller file size is preferred and high curve accuracy is not needed.

•	High. Select this option when high curve accuracy is essential; the file size is larger than when using the Normal setting.

See also IGES Entity Types and IGES Export Format Types .

Parasolid

Assembly.  Select one of the following: (For export only.)

•	Flatten Assembly Hierarchy. A file containing a flattened hierarchy consists of a top level assembly and one level of parts.  All subassemblies are eliminated.

•	Maintain Assembly Hierarchy. A file which saved the assembly hierarchy consists of assemblies, sub-assemblies, and parts, and the structure mirrors the original assembly and its nested subassemblies.

Output as.  Select one of the following:

•	Version 9 file. Outputs parasolid transmit file in Version 9 format.

•	Version 8 file. Outputs parasolid transmit file in Version 8 format.

DXF/DWG Output

•	Version.  Select R12, R13, or R14. This allows you to specify if a file saved with a .dxf or .dwg extension will be in R12, R13, or R14 format.

•	Fonts.  Select either Truetype Fonts or AutoCAD STANDARD only.

ACIS (.sat)

•	Version. From the pull-down list, select the ACIS version to use when saving files in ACIS format.

•	Units. Specify the units of measure to use for ACIS files.

STL

Click the STL Options button to specify your preferences for STL output.


STL

Specifies your preferences for STL output.

Output Format:

•	Select either Binary or ASCII as the file format.

Quality. Controls the tessellation of non-planar surfaces for Stereolithography (STL) output. A lower deviation setting produces a more finely tessellated STL file.

•	Coarse or Fine. Preset resolutions.

•	Custom. Allows you to specify the resolution by dragging the Total Quality and Detail Quality slider controls or by entering values for Deviation and Angle Tolerance.

Total Quality

•	Deviation. Reports the maximum chordal deviation in effect at the various resolution levels. The chordal deviation value is greater at the Coarse setting, and decreases as the resolution becomes more fine.

Detail Quality

•	Angle Tolerance. Controls smaller detail tessellation.  Use a value from 0.5 to 30 degree.  A lower value gives greater small detail accuracy, but takes longer to generate.

Preview.  Select this option to see a preview of the model with the tessellation triangles visible.

Show STL Info Before File Saving. Displays a faceted model preview in the part window and displays a dialog box with the following information:  Triangles (number), binary file size, file format, and the directory path and file name.


IGES Entity Types

IGES Entity Type	Entity Name
144	Trimmed (parametric) surface
142	Curve on a parametric surface
128	Rational B-spline surface
126	Rational B-spline curve
122	Tabulated cylinder
120	Surface of revolution
118 Import only	Ruled surface
112 Export only	Parametric spline curve
110	Line
102	Composite curve
100	Circular arc


IGES Export Format Types

Trimmed Surfaces

Export Format Types	Exported IGES Entity Types
Standard	144, 142, 128, 126, 122, 120, 110, 102, 100
ANSYS	144, 142, 128, 126, 110, 102, 100
COSMOS	144, 142, 128, 126, 110, 102, 100
MasterCAM	144, 142, 128, 126, 110, 102, 100
SurfCAM	144, 142, 128, 126, 110, 102, 100
SmartCAM	144, 142, 128, 126, 110, 102, 100
TEKSOFT	144, 142, 128, 126, 110, 102, 100
3D Curves - Wireframe Representation

Type of 3-D Curve	Exported IGES Entity Types
B-splines (entity 126)	126, 110, 102*, 100
Parametric splines (entity 112)	112, 110, 102*, 100

*Exported only if you select the Duplicate Entities option in IGES Preferences.


Grid/Units

To specify the grid and units settings for documents:

1	Click Tools, Options.

2	Click on the Grid/Units tab.

3	Change the settings and click OK.

Grid

•	Properties

Display Grid

Dash

Automatic Scaling

Major Grid Spacing

Minor Lines Per Major

•	Snap Behavior

Snap to Points

Snap Points Per Minor

Snap to Angle

Snap Only When Grid is Displayed

Units

•	Length Unit

Units Type

Decimal Places

Fractions Denominator

•	Angular Unit

UnitsType

Decimal Places

•	Spin Box Increments

Length

Angle

View System Defaults. When checked, the system default for each of the options is displayed; when not checked the option selections used by the active document are displayed.

Apply To:  Select an option from the pull-down list, as follows:

•	System Defaults. Applies the selections that you made to all new documents that you create.

•	Active Document. Applies the selections that you made to only the currently active document.

•	All Possible. Applies the selections that you made to both the system defaults and currently active document.


Planes Options

Lets you specify default plane names for parts and assemblies. For example, you may want to name the planes Front, Top, and Right, instead of Plane1, Plane2, and Plane3.

To set new default names for planes:

1	Click Tools, Options.

2	Select the Planes tab.

3	Enter the new names in the boxes that correspond to the original plane names.

4	Click OK.

To return to the original names, click Reset All.


Line Font

To set the default style and weight of lines for selected edge types in a drawing:

1	Click Tools, Options.

2	Click on the Line Font tab.

3	Change the settings and click OK.

Default Line Font Properties

Type of Edge

Line Style

Line Weight

Preview

View System Defaults. When checked, the system default for each of the options is displayed; when not checked the option selections used by the active document are displayed.

Apply To:  When in a drawing, select an option from the pull-down list, as follows:

•	System Defaults. Applies the selections that you made to all new drawing documents that you create.

•	Active Document. Applies the selections that you made to only the currently active drawing.

•	All Possible. Applies the selections that you made to both the system defaults and currently active drawing.

Note:  If you make changes to this page when you are not in a drawing, the changes apply to the next drawing that you create (System Defaults).

To set the line weight value for the three types of lines, see Page Setup.


No help available
No help is available for the selected topic.


No help available
No help is available for the selected topic.


Edit Mating Relations

Allows you to make the following changes to a mating relation:

•	Distance between the mated components, for distance mates

•	Angle between mated components, for angle mates

•	Alignment (aligned or anti-aligned) on mates that imply a direction

•	Flip dimension to other side changes the direction in which the distance is measured

To edit a mating relation:

1	Right-mouse click the mate you want to edit in the FeatureManager design tree, and select Edit Definition.

2	Select the desired Alignment Condition . (Only those conditions that are valid for the selected features are available.)

3	In the Workbench area, click Preview. The parts move to the mating relation that you specified.

4	If this mating relation is acceptable, click Apply; if not, click Undo and try again.


Geometric Characteristic Symbols

Inserts a geometric characteristic symbol into the Current Work Sheet in the Geometric Tolerance dialog.


Line and Point Plane

To create a plane through a line, axis, or shetch line and a point:

1	Select an edge, axis or sketch line and a vertex or a point while holding the Ctrl key.

2	Click Finish.


SolidWorks API

The SolidWorks API is an OLE programming interface to SolidWorks.  The API contains hundreds of functions that can be called from Visual Basic, VBA (Excel, Access, and so forth), C, C++, or SolidWorks macro files. These functions provide the programmer with direct access to SolidWorks functionality such as creating a line, extruding a boss, or verifying the parameters of a surface.

For a detailed description of the API and the syntax used to call each function, please refer to the API online help file.  This help file, API_HELP.HLP is located in the ..\SAMPLES\APPCOMM\ subdirectory of your SolidWorks installation.  Also included in the ..\SAMPLES subdirectory are several Visual Basic and C++ example projects.  Feel free to use these projects as a reference or as a starting point for your own applications.

You can also find a detailed description of the API functions on the SolidWorks web page (www.solidworks.com) under the Technical Support area.


Microsoft Office Compatible

SolidWorks is a Microsoft Office Compatible product.  This means that the SolidWorks toolbars, menus, and accelerator keys are similar to the ones used by the Microsoft Office suite of applications, including Microsoft Word, Microsoft Excel, Microsoft Access, and PowerPoint.

If you already know how to use Microsoft Office, you will find that you already know how to do many of the similar tasks in SolidWorks.

SolidWorks and Microsoft hope that these many similarities will make it easier for you to use our products together and with other Microsoft Compatible products.  Look for the Microsoft Office Compatible logo when you select new software to purchase.

For more information about the Microsoft Office Compatible program, and for a complete list of Microsoft Office Compatible products,

in the United States, call Microsoft Customer Service at 1-800-426-9400

- or -

outside the United States, contact your local Microsoft office.

See also:

  SolidWorks and Microsoft Office Compatible Features

  SolidWorks Interaction with  Microsoft Office


SolidWorks and Microsoft Office Compatible Features

The following are some of the many SolidWorks features that are compatible with Microsoft Office:

Toolbars and Menus

•	SolidWorks has toolbars that are similar to Microsoft Office toolbars, containing many of the same functions and arranged in the same order.

•	The toolbar buttons graphically describe the task they are associated with. For example, you can click the pair of scissors to cut a region of selected text.

•	The SolidWorks toolbars provide ToolTips. When you pause your mouse cursor over a toolbar button, a small note pops up to identify the button. If you wish to disable ToolTips, click View, Toolbars and uncheck the Show ToolTips option.

•	You can customize your toolbars, menus, and keyboard by selecting Customize from the Tools pull-down menu.

•	You can move and hide the SolidWorks toolbars in the same ways that you can move and hide the toolbars in many Microsoft Office products.

Additional Features

•	SolidWorks uses drag and drop action with the mouse cursor, as well as dragging to change the size of both windows and sketch entities.

•	You can choose how you want to view your open documents by tiling or cascading windows, as with other Windows compatible products.


SolidWorks Interaction with  Microsoft Office

SolidWorks interacts with Microsoft Office tools:

•	Using Microsoft’s OLE, you can link or embed SolidWorks part, assembly, or drawing documents in Microsoft products such as Word, Microsoft Excel, and PowerPoint.

•	You can use Microsoft products such as Microsoft Excel to insert data into SolidWorks documents.

•	You can send SolidWorks part, assembly, or drawing documents over the network using Microsoft’s mail application, as well as other Microsoft Office compatible mail products.


Display Grid

Turns the sketch grid on or off.


Dash

Toggles between solid and dashed grid lines.


Automatic Scaling

Automatically adjusts display of the grid when you zoom in and out.


Major Grid Spacing

Specifies the space between major grid lines.


Minor-Lines Per Major

Specifies the number of minor grid lines between major lines.


Snap to Points

Turns grid snap on or off. When snap is on, points that you sketch or drag snap to the nearest intersection of grid lines (or to intermediate points, if Snap Points Per Minor is greater than 1).


Snap Points Per Minor

Specifies the number of snap points between minor grid lines.


Snap only when grid is displayed

Turns on grid snap only when Display Grid is turned on. (Available only from the Tools, Options, Grid/Units tab dialog.)


Angular Unit Selection

From the pull-down menu, select either Degrees, Deg/Min, Deg/Min/Sec, or Radians.

If you select Degrees or Radians, specify the number of decimal spaces.


Type of Units

From the pull-down menu, select Millimeters, Centimeters, Meters, Inches, Feet, or Feet and Inches.

If you select Inches, or Feet and Inches as your unit of measure, select Decimal or Fractions.


Decimal

Specify the number of  (0 to 10).


Fractions

Specify the default Denominator. (Only dimensions that are evenly divisible by this denominator are displayed as fractions.)


Length Increment

Enter the number of units to add or subtract when you click on a spin box arrow to change a linear dimension value.


Angle Increment

Enter the number of degrees to add or subtract when you click on a spin box arrow to change an angular dimension value.


Type of Edge
Type of Edge - Select an edge type from a list of line types: Visible Edges, Hidden Edges, Sketch Curves, and so on.


Line Style
Line Style - Choose a style from the pull-down menu, such as:  Solid, Dashed, Phantom, and so on.


Line Weight
Line Weight - Select Normal, Thin, or Thick lines from the pull-down menu.


Preview
Preview - Displays the selected line font.


Drawing Name
Drawing Name - Enter a title for the drawing in the Name box.


Drawing Paper Size
Drawing Paper Size - Select a standard paper size from the pull-down menu, or choose User Defined and enter dimensions for the paper width and height.


Drawing Paper Width
Drawing Paper Width - Enter the width dimension of your drawing sheet.


Drawing Paper Height
Drawing Paper Height - Enter the height dimension of your drawing paper.


Drawing Scale
Drawing Scale - Enter the drawing scale to use.  The default scale is 1:2.


Drawing Scale
Drawing Scale - Enter the drawing scale to use.  The default scale is 1:2.


Drawing Template
Drawing Template - Select one of the drawing templates in the pull-down list, or select None or a custom template.  If you select Custom, use the Browse button to find the template.


Find a Custom Drawing Template
Find a Custom Drawing Template - Use the Browse button to find a drawing template on your local drive or across the network.


First Angle Projection
First Angle Projection - Select this button to use orthographic views in first angle projection if you use the Standard 3 View drawing on this sheet.


Third Angle Projection
Third Angle Projection - Select this button to use orthographic views in third angle projection if you use the Standard 3 View drawing on this sheet.


 Single command per pick

This option specifies that sketch and dimension tools deselect after each use. (Double-clicking a tool causes it to remain selected for additional use.)


Use fully defined sketches

To specify that sketches must be fully defined before using them to create features, select this check box.


Alternate spline creation

To create splines by clicking on through points select this check box.  The default method of creating splines is to drag out the spline segments.


Display arc centers

To turn the display of arc centerpoints on or off in a sketch, select this check box.


Infer from model

To specify that inferencing lines that relate to the lines and vertices of the underlying part are displayed when you are sketching on a face of an extruded part, select this check box.


Input dimension value

To specify that the modify spin box is automatically displayed for the input of a new dimension value, select this check box.  Otherwise, you must double-click on the dimension value to display the spin box.


Use English language

If you specified the use of another language during the SolidWorks installation, you can change to English by selecting this check box.

Note that you must exit and re-start SolidWorks for this change to take place.


Create sketch on new part

To specify that the part window opens with the sketching area and sketch tools immediately available when you select New, Part, select this check box.


Scroll Selected Item into View

Specifies that the FeatureManager design tree should automatically scroll to display the feature icon that is related to the selected items in the graphics area.


Angle Snap Value

Specifies the number of degrees between snap points when sketching.


Snap to Angle

Select this check box to specify that sketched lines snap to a pre-defined angle.  The inferencing cursor displays the specified angle as you sketch.


Change Value for Red

Change the color of the selected face by changing the numeric value for red.  The color displays when you select Shaded view.


Change Value for Green

Change the color of the selected face by changing the numeric value for green.  The color displays when you select Shaded view.


Change Value for Blue

Change the color of the selected face by changing the numeric value for blue.  The color displays when you select Shaded view.


Use Part Color

To use the default part color for the selected face when in Shaded view, click this button. The part color is displayed in the preview box.


Change Color

To change the color for the selected face when in Shaded view, click this button.  Select a color from the color blocks or create a color with the custom color palette.


Name of Entity

To add or change a name for a part face or edge, place the cursor in the edit box and enter a new name.


Hide Entity

When you are working in a drawing, select an edge and click this button to hide the edge entity.


Show Entity

Pass your cursor over the drawing view to reveal hidden entities with  dynamic highlighting. Select a highlighted edge and click this button to show the edge entity.


Decimal Places

Specify the number of decimal places (0 to 10).


Decimal Places, Angular Dimension

Specify the number of decimal places (0 to 10).


Ambient Light

Light that is scattered so greatly that it seems to come from all directions. For example, the light in a room with white walls has a high degree of ambient light because the light reflects off the walls and objects in the environment; a spot-lighted area has little ambient light because the light is focused in a narrow beam.


Directional Light

Light that comes from a source that is infinitely far away from the surface. The light travels from one direction. (The sun is a real-world example of directional light.) The direction of the light source is apparent to the viewer.

Adjust the slider bars to specify the amount of directional light striking the model surface from positions X, Y, and Z.


Spot Light

A restricted and focused light that emits in a cone-shaped beam that is brightest at its center; a spot-lighted area has little ambient light because the light is focused in a narrow beam.


Diffuse Light

Light that comes from one direction, but once it strikes the surface the light scatters equally in all directions so it appears equally bright no matter where the observing eye is located.


Specular

Light that comes from one direction and tends to bounce off the surface in a particular direction. Specularity indicates that the surface is shiny. A dull surface has no specularity; a glossy surface has high specularity.


Exponent

The property that results in a more or less concentrated beam of light. A higher spot exponent results in a more focused light source. Move the slider to the right to increase the light concentration.


Attenuation

The property that decreases the intensity of light as the distance from the light source increases. The three boxes (a, b, and c) hold values that are used in an equation to arrive at an attenuation factor. The distance from the light source is represented by d in the attenuation factor equation.


Distance

The distance from the light source to the surface of your model. Use the scroll arrows to increase or decrease the distance. (This value is represented by d in the attenuation factor equation.)


Cutoff

The property that restricts the shape of the light cone. The maximum value is 180; reduce the value to reduce the spread of the light cone.


Ambient

Adjust the slider bars to specify the amount of ambient light that strikes the model surface from positions X, Y, and Z. Move the slider to the right to increase the effect of the ambient light.


Coincident. Positions the selected items so they overlap, occupying the same space.


Perpendicular. Places the selected items at a 90 degree angle to each other.


Tangent. Places the selected items in a tangent mate. You must select at least one cylindrical face.


Concentric. Places the selected cylinders so that they share the same center point.


Parallel. Places the selected items so they lie in the same direction and remain a constant distance apart from each other.


Distance. Places the selected items with the specified distance between them.


Aligned. Places the selected items so the solids are on the same side of the plane.


Anti-Aligned (On). Places the selected items so the solids are on opposite sides of the plane.


Closest. Makes the items aligned or anti-aligned, based on which position they are closest to at the beginning.


 Angle. Places the selected items at the specified angle to each other.


Displays the Height of the selected standard paper size, or lets you specify the custom paper size Height.


Displays the Width of the selected standard paper size, or lets you specify the custom paper size  Width.


Use the Browse button to locate and use a custom drawing template.


Specify the letter of the alphabet that will be used for the next Section Label. The default letter is A. Successive labels are in alphabetic order.


Specify the letter of the alphabet that will be used for the next Detail Label. The default letter is A. Successive labels are in alphabetic order.


Specify the letter of the alphabet that will be used for the next Datum Label. The default letter is A. Successive labels are in alphabetic order.


Composite Frame.  A composite frame allows for the location of a profiled feature or circular pattern and, at the same time, the control of form and orientation. The entire frame is doubled in height; the top half is the locating tolerance zone, and the bottom half is the form and orientation (or feature-related) tolerance zone. The first compartment of the feature control frame holds a geometric characteristic symbol that is common to both.


Projected Tolerance Zone.  A tolerance zone that is recommended when there are variations in perpendicularity of threaded or press-fit holes which could cause interference when mating a part. The PTZ is located at true position and extends away from the primary datum at the threaded feature.


Line

A line can be a line or centerline in the sketch, or an external entity (edge, plane, axis, or sketch curve in an external sketch) that projects as a line in the sketch.


Arc

An arc can be an arc or circle in the sketch, or an external entity that projects as an arc or circle in the sketch.


Point

A point can be a point in the sketch, or an external entity (origin, vertex, axis, or point in an external sketch) that projects as a point in the sketch.


Ellipse

An ellipse can be an ellipse in the sketch, or an external entity that projects as an ellipse in the sketch.


Spline

A spline can be a spline in the sketch, or an external entity that projects as a spline in the sketch.


Reverse direction to close sketch

Notice that an arrow points in the direction in which the sketch will close. The extruded boss will either be within the sketch lines or outside of the sketch lines.

1	Click Reverse direction to close sketch, if necessary.

2	Click Yes when the arrow points in the correct direction; click No to exit the dialog.


Datum Feature Symbol

To change the label, enter a new letter in the Label box.

To display the symbol with a filled triangle at its base, click the check box.

To display the symbol with a shoulder (a bend), click the check box.

Click OK to save your changes; click Cancel to exit without saving the changes.


Prompt to close sketch

 With this option selected, if you make a sketch with an open profile that can be closed with the model edges to extrude a boss, the system puts up a dialog, Close Sketch with Model Edges? You can choose to use the model edges to close the sketch profile and you can select the direction in which to close the sketch. The Extrude Feature dialog then appears automatically.


Enter feature name on creation
Name feature on creation

When you create a new feature, the feature name in the FeatureManager design tree is automatically selected and ready for you to enter a name of your choice.


Open last used documents at startup.

Select either Always or Never. Select Always if you want the convenience of having the documents that you used most recently open automatically when you start SolidWorks.


Maximize on open

 When checked, each document is opened to its largest size within the SolidWorks window.


Chordal Deviation

When representing a cylindrical surface, the curve of its shape is actually represented by straight lines arranged to approximate the curve. Chordal deviation measures the distance between each straight line and the apex of the arc of the imaginary circle. When the resolution is low, there are fewer straight lines, the representation is rough, and deviation between the line and the arc is greater. When the resolution is high, there are many straight lines, the representation is smoother, and the deviation between the line and the arc is smaller.


Configure

Click this checkbox to open a specific configuration of a part or assembly.


Preview

Click this checkbox to see a graphic preview of the selected part, assembly or drawing document without opening the document.


References

Lists the part and/or assembly documents referenced by the currently selected assembly or drawing.  You can edit the locations of the listed files.


All Faces


None


Along Tangent


Inner Faces


Outer Faces


Arrow key navigation

Lets you use the arrow keys to traverse the FeatureManager design tree, and expand or collapse the design tree and its contents, as follows:

Up arrow - scrolls up the design tree

Down Arrow - scrolls down the design tree

Left arrow at top of design tree - collapses the design tree

Right arrow at top of design tree - expands the design tree

Left arrow on an item in the tree - collapses the item to hide its contents

Right arrow on an item in the tree - expands the item to display its contents, if any

Space Bar - selects the highlighted item


Show errors every rebuild

If errors are present in the model, displays an error message each time the model rebuilds.


Override dimensions on drag

Lets you override dimensions by dragging sketch entities. The dimension updates after the drag is completed.

(Also available from the menu: Tools, Sketch Tools, Override dims on drag.)


Automatic relations

Specifies whether geometric relations are automatically created as you add sketch elements.

 (Also available from the menu: Tools, Sketch Tools, Automatic Relations.)


Prompt to set driven state

When checked, specifies that when you add an overdefining dimension to a sketch, a dialog box asks you if the dimension should be driven. (The default is to ask.)

Set driven by default. When checked, specifies that when you add an overdefining dimension to a sketch, the dimension is set to be driven by default.

Note:	The Prompt to set driven state checkbox can be used alone or with the Set driven by default checkbox. Depending on the choice of checkboxes you can have one of four different behaviors when you add an overdefining dimension to a sketch.

1  A dialog box appears that defaults to driven.

2  A dialog box appears that defaults to driving.

3  The dimension comes in driven.

4  The dimension comes in driving.


Set driven by default

When checked, specifies that when you add an overdefining dimension to a sketch, the dimension is set to be driven by default.

Note:	This checkbox can be used alone or with the Prompt to set driven state checkbox. Depending on the choice of checkboxes you can have one of four different behaviors when you add an overdefining dimension to a sketch.

1  A dialog box appears that defaults to driven.

2  A dialog box appears that defaults to driving.

3  The dimension comes in driven.

4  The dimension comes in driving.


Enable silhouettes

With this option, silhouettes are selectable and you can do the following operations on silhouettes: Convert Entities, Offset Entities, Add Relation, and Dimension.

Note	Enabling silhouettes may effect performance when activating a sketch for editing if the model is complicated.


Show dimension names

Displays the dimension’s name as well as its value.


Display entity points

Specifies the display of the endpoints of sketch entities as filled circles. The color of the circle indicates the status of the sketch entity, as follows:

Black = Fully defined

Blue = Under defined

Red = Over defined

Green = Selected

Note	Over defined and dangling points are always displayed, regardless of the Options setting.


Arrow keys

Lets you specify the angle increment for view rotation when you use the arrow keys to rotate the model.


Mouse speed

Lets you set the speed of rotation when you use the mouse to rotate the model or assembly component. If you move the slider to the left, you get finer control and slower rotation.


Dynamic Highlight

Specifies that the geometry in the graphics area (edges. faces, planes, axes, etc.) is highlighted when the cursor passes over the item in the FeatureManager design tree.


Number of backup copies per document

Lets you specify the maximum number of backup copies you want to save of part, assembly or drawing documents. Scroll to 0 (for none) or up to the maximum number of backups you want to save. The name of a backup copy is "Backup (n) of original filename and extension."


Instance/Revolution Counts

When this is checked, all dimensions that correspond to the number of pattern instances in a linear or circular pattern, or the number of revolutions in a helix will be imported into this drawing view (if they exist in the part or assembly). The default is that these dimensions are not imported because dimensions of this type generally have little value.


Multiple Leaders

To use multiple leaders:

1	Click each place on the drawing where you want the note leaders to attach.

2	Click [image] or Insert, Annotations, Note.

3	Enter the note text, and click OK.

The note appears with leaders attached to all the places you clicked.

4	Click on the note and drag it to the location where you want it to remain.

To add an additional leader to a note:

1	Hold the Ctrl key and select the arrowhead of an existing leader.

2	Drag the arrowhead.

A new leader takes shape.

3	Drag the new leader to point to a new location.

To delete a leader:

Select the arrowhead and press the Delete key.


Do Not Repeat Confirmation Message

This message gives you the opportunity to abort the action you requested.

Click OK to continue; Click Cancel if you want to abort the action.

If you do not want the message to display again during this session, click the checkbox next to Don’t ask for confirmation again during this session.


Standard Toolbar

The Standard toolbar controls file management and model regeneration.

	New
	Open
	Save
	Print
	Print Preview
	Cut
	Copy
	Paste
	Undo
	Rebuild
	Redraw
	Web Toolbar
	Help


View Toolbar

The View toolbar controls your view of the model.

If any View icons are not included on your default View toolbar, you can customize the toolbar by adding any of the icons below.  See Customize Toolbars for more information.

	Zoom to Fit
	Zoom to Area
	Zoom In/Out
	Rotate View
	Pan
	Wireframe
	Hidden in Gray
	Hidden Lines Removed
	Shaded
	Section View
	Perspective


Sketch Tools Toolbar

The Sketch Tools toolbar provides sketch entities and sketch tools to use in a sketch or a drawing. (Note that the Convert Entities and Offset Entities tools are not available in drawings.)

	Line
	Centerpoint Arc
	Tangent Arc
	3 Point Arc
	Circle
	Ellipse
	Spline
	Rectangle
	Point
	Centerline
	Convert Entities
	Mirror
	Fillet
	Offset Entities
	Trim/Extend


Sketch Toolbar

The Sketch toolbar controls selection, sketch creation, sketch modification, and the sketch grid.

	Insert/Edit Sketch
	Grid/Units
	Select
	Modify


Dependency Editing Toolbar

The Dependency Editing toolbar controls feature dependencies.

	Rollback
	Suppress
	Unsuppress
	Unsuppress with Dependents
	Rebuild


Sketch Relations

The Sketch Relations toolbar controls dimensions and other geometric relations.

	Dimension
	Add Relation
	Display/Delete Relations


Macro Toolbar

The Macro toolbar controls macro recording, playback, and editing.

	Run Macro
	Stop Macro
	Record Macro
	Edit Macro


Assembly Toolbar

The Assembly toolbar controls the movement and mating of components.

	Show Components
	Hide Components
	Rotate Component Around Centerpoint
	Rotate Component Around Axis
	Move Component
	Edit Part
	Mate


Drawing Toolbar

The Drawing toolbar provides tools for creating drawing views, notes, and symbols.

	Note
	Surface Finish Symbol
	Geometric Tolerance
	Balloon
	Center Mark
	Datum Feature Symbol
	Hole Callout
	Weld Symbols
	Datum Target Point
	Datum Target Symbol
	Detail
	Section
	Aligned Section
	Projection
	Standard 3 View
	Auxiliary
	Named View
	Relative to Model


Web Toolbar

The Web toolbar provides support for working over the Internet.

	Stop Internet Jump
	Reload Internet Document
	Insert Hyperlink
	Open Internet Address


Features Toolbar

The Features toolbar provides tools for creating model features.  The set of features icons is very extensive so not all of them are included on the default Features toolbar.  You can  customize this toolbar by adding and removing icons to suit your working style and frequent tasks.  See Customize Toolbars for more information.

	Boss
	Revolved Boss
	Cut Extrude
	Revolved Cut
	Fillet
	Chamfer
	Rib
	Plane
	Axis
	Scale
	Shell
	Draft
	Hole Wizard
	Insert Bends
	Dome
	Flattened
	No Bends


Enter your input in this field.


Enter your input in this field.


Closes this dialog and saves any changes you have made.


Closes this dialog without saving any changes you have made.


Click this button to make your choice.


Choose an item from the list.


Enter your input in this field.


Choose an item from the list.


Enter your input in this field.


Choose an item from the list.


Closes this dialog and saves any changes you have made.


Closes this dialog without saving any changes you have made.


Click this button to make your choice.


Enter your input in this field.


Closes this dialog and saves any changes you have made.


Closes this dialog without saving any changes you have made.


Click this button to make your choice.


Choose an item from the list.


Click this button to make your choice.


Click this button to make your choice.


Click this button to make your choice.


Click this button to make your choice.


Click this button to make your choice.


Click this button to make your choice.


Click this button to make your choice.


Click this button to make your choice.


Choose an item from the list.


Closes this dialog and saves any changes you have made.


Closes this dialog without saving any changes you have made.


Click this button to make your choice.


Closes this dialog without saving any changes you have made.


Click this button to make your choice.


Click this button to make your choice.


Click this button to make your choice.


Click this button to make your choice.


Click this button to make your choice.


Click this button to make your choice.


Click this button to make your choice.


Choose an item from the list.


Choose an item from the list.


Choose an item from the list.


Choose an item from the list.


Choose an item from the list.


Choose an item from the list.


Check your desired options.


Check your desired options.


Choose an item from the list.


Click this button to make your choice.


Click this button to make your choice.