Q.1.2 How can I create a line parallel to another?
A.
There are several methods:
Q.1.3 How can I create a line at a specific angle?
A.
To create a line at a specific angle you must understand how to manipulate your
work axes (the little green arrows). Don't be afraid to move the work axes around your sketch for duplicating, mirroring and working at angles. When creating lines, hold the SHIFT key down to align with the work axes. You can rotate the work axes by a specific angle using the Transform Axes tool on the Workplane menu. Alternatively, you can use the Reposition Axes tool and, while holding the mouse button down, drag to set the orientation by snapping to another part of your sketch. In this way you can very quickly align the axes from an existing line and then work at that orientation. If you wish to return to an origin which is not selectable within your sketch, you can create a construction line or circle before moving the work axes around.
Q.2.1 How do I know if I am above or below the workplane?
A.
There is a visual clue to how your workplane is oriented. If you see solid arrows, then above the workplane will be up and below will be down. If you see hollow arrows, above the workplane will be down and below will be up.
Q.2.2 How do I know which is the X and Y axis on my work axes?
A.
Work axes conform to the right-hand Cartesian coordinate system. To understand this, hold up your right hand with your palm facing you and your thumb and index finger extended. Your thumb represents the X axis, your index finger represents the Y axis and your middle finger represents the Z axis.
Q.2.3 Why do I sometimes get little gaps in my shading?
A.
In the interest of fast graphical update, when making incremental changes to a model, only those edges and faces that are affected by the change are recalculated. Sometimes this can lead to tiny gaps - usually not more than a few pixels wide - between the faces of the model when shown in shaded mode. You can remove these gaps by regenerating the model from the beginning. The easiest way of doing this is by suppressing the first feature, immediately unsuppressing it, then update the design. You can suppress a feature by using the popup menu in the Features browser.
Q.2.4 Why does the shading sometimes look jagged?
A.
The curved faces of a shaded model are drawn using facets - an approximation of the surface made of tiny planar tiles. The tolerance used to calculate the accuracy of these facets is based on the size of the model and is usually such that you cannot perceive the approximation. However, when you first create a model, its overall size is not known and a default tolerance is used. If the model size is very small, you may see small errors in the facets. You can remove these by regenerating the model from the beginning. See Q.2.3 for a method of doing this.
Q.3.1 How can I prevent an open assembly or drawing from updating every time I make changes to a part?
A.
Simply minimize any assembly or drawing windows that reference the part that you are working on. Updates to the assembly or drawing will be made when their windows are next restored.
Q.4.1 How do I set up drafting standards?
A.
You can setup your preferred drafting style from various settings within the Options dialog. The Options command can be found on the Tools menu. The options that you set here are then used to supply the default properties of objects that you create from that point on. (The grayed out fields are used when the dialog controls the properties of a selected object.) The settings that you make are stored per user and will be retained across sessions.
Use the following options to set your preferred standard:
| Options Setting | ANSI Y14.5M | ISO (includes BS308) |
|---|---|---|
| Numeric/Suppress leading zeros | Yes | No |
| Numeric/Suppress trailing zeros | No | Yes |
| Numeric/Suppress sign on zero tolerance | No | Yes |
| Numeric/Use comma for decimal separator | No | If desired |
| Placement/Level | In Line | Above line |
| Placement/Orientation | Horizontal | Along line |
| Datum/Datum label style | Flippers | No flippers |
Q.4.1 How do I create text without a leader?
A.
While dragging the note using the Textual Note tool, hold the SHIFT key down. If you already have text with a leader, you can select the leader and delete it separately.
Q.4.3 How do I insert special characters in textual notes?
A.
In some rare situations, you might need to create text notes in your drawing to manually simulate dimensions that DesignWave cannot apply automatically in this release. There is no simple way to enter special symbols when you edit the text for a note on the drawing. Instead, you can open the SYMBOLS.CVD drawing and copy the text from the samples provided. The SYMBOLS.CVD drawing and a readme.txt, which explains the process for using the symbols, can be found in the Samples\Symbols sub-folder of your installation directory.
E.g. C:\Program Files\Computervision\DesignWave\Samples\Symbols
Q.4.4 How do I center a section line through a hole?
A.
When you create a section line and you want to snap to attraction points of the model, such as the center of a hole, turn the Edges check box on.
If you place the cursor just inside a hole, you will snap to its center. You can create a section line passing through the center of a hole by snapping to the hole feature center, then select the line that you have just created and drag an end while holding the SHIFT key to maintain the line direction.
Remember to turn the Edges check box back off in order to select sketch geometry so that you correctly join up the endpoints of the section line chain.
Q.4.5 How do I use text from an external text file to create multi-line text notes?
A.
To create a multi-line text note, edit the text and select Multi-line. You can cut or copy text from an external application and paste it into the multi-line text area. However, be aware that when copying text from some applications, such as MS Word, a paragraph is placed on the clipboard as a single very long line with no carriage returns. (You can tell by pasting the text into Notepad and experimenting with Word Wrap.) To get the desired paragraph formatting out of MS Word you can Save As with the file type Text Only with Line Breaks(*.txt). You can then open the .txt file with Notepad and copy/paste lines into the multi-line area of the dialog.
Q.4.6 Why are there three different unit selections within the Options menu?
A.
When you select Tools->Options->Units, you are provided with two selections: Model Distances and Paper Distances. Model distances controls the input units while you are in a part. Paper distances controls the input units while you are in a drawing. To see what your current unit selection is, simply look at the grid size feedback while you input geometry.
The Tools->Options->Number page controls the units that will be used to display subsequently created dimensions. This unit is stored with a dimension value and can be controlled independently to the units you use for creating lines in sketches on a part or drawing.
Q.4.7 How do I create a balloon callout?
A.
Since there is no balloon callout included yet, you must create a line and a circle to represent the balloon callout. Create the balloon by inserting a circle in the appropriate location (double-click on it to set an exact diameter). Create a line from the center of the circle to the arrowhead location. Modify the line to touch the outer edge of the circle. (Use the Select Lines tool and drag the line onto the circle.) Now double click on the line and select the Line tab from the property sheet. In the Start terminator dialog box, select Arrow. If the wrong end of the line received the arrow, simply double-click on the line again, select the Line tab and press the Swap button. To create the text, select the Textual Note tool and, while holding down the SHIFT key, position the text in the circle. (You will notice that by default the Textual Note tool creates a label, but by holding down the SHIFT key you will get text. The shift key also affects how GD&T are placed!) Double click on the text to edit.
TIP: If you have multiple balloons, you can resize one circle to the correct diameter, then with this circle selected, choose the Pick Up Properties tool from the Edit pulldown menu and select Radius. Now you can make all the circles you want have this radius by selecting them (use SHIFT key to add selections) and choosing Apply Properties from the Edit pulldown menu.
This technique of property reassignment can also be used with dimensions!
Q.4.8 How can I selectively turn off crosshatching?
A.
DesignWave does not distinguish between a shaft and a cylinder. Therefore, when creating section views, crosshatching is generated for a shaft just like any other cylinder feature. Often, in assembly views, shafts are not shown crosshatched. Currently it is not possible to delete a crosshatch object, but you can make it invisible by editing its properties and setting the spacing to the maximum of 1m. Be aware that with the spacing set at this distance, you will not be able to select the crosshatch to change it back later.
Q.4.9 How do I dimension a cone?
A.
ANSI Y14.5 indicates three allowable methods for dimensioning cones: as a callout note, as an angular dimension between the walls and as an angular dimension to the horizontal or vertical. DesignWave currently supports the first of these methods (see online documentation topic Dimensioning the Angle of a Cone). The other dimension styles can be created by using the line tool for the dimension and leader lines. You can cut and paste the text from a callout created by the first method to maintain associativity, or you can create your own callout to hold the value. See the online help topic Creating Tabular Dimensions for more information on cutting and pasting dimension text and Q.4.3 for information on embedding a degree symbol in a text string.
Q.4.10 How do I dimension in degrees-minutes-seconds?
A.
This presentation method is not supported in this release. If you wish to display this style, you can insert your own text notes into any dimension callout group and delete the original dimension value. See Q.4.3 for information on embedding a degree symbol in a text string.
Q.4.11 Where is the Not-To-Scale option for dimensions?
A.
This is intentionally not supported, since all dimension values created in DesignWave reference the model geometry directly. Even if a dimension spans different views of a part, the dimension value is still true for the distance being represented. If you do need to cheat the system for a special case you can use the Insert Callout Note method to substitute NTS dimension text and use the line tool to add an underline. You will need to leave some room so that the line doesn't get hidden by the text blanking.
Q.4.12 How do I dimension axial center lines in pipe sections?
A.
This type of center line is currently not supported. Use the line tool to draw the center line as fragments. Be sure to use a new sketch and not one already used for defining the section lines. See Defining Section Views in the online help for more information on sections and sketches.
Q.4.13 How do I dimension the major radius of a swept profile (pipe bend)?
A.
This is currently not supported. The radial dimension line must be drawn using the line tool. You can add an arrow terminator to the line via its properties. The dimension text value can be placed using textual note tool.
Q.4.14 How do I dimension a blend at the junction between two cylinders?
A.
At this release, the radial dimension tool does not support dimensioning the blend angle that forms the saddle feature created at the junction of two cylinders, such as a small pipe welded to the side of a larger pipe. You will need to create a dimension using the line and text note tools.