Library Menu Reference

Libraries

This option brings up the dialogue box which allows the setting up and editing of libraries.

The list in the dialogue box is a list of libraries searched when the Get option (in the Library menu) is used. You may add or remove these libraries from this list using the buttons at the side of the list.

The Add button in the dialogue allows a library not currently being searched to entered into the search list. When this option is selected a file selection dialogue appears. Select the index file (those files with .idx extensions), which belongs to the library you wish to use. The library is then added to the list box.

The Remove button removes a library from the search list. It does not delete it! Select the library you wish to remove by clicking on it in the list box, then click on the remove button.

The Edit button allows you to:
- View & Print thumbnails of the symbols
- Add new symbols to this library
- Edit existing symbols in the library

The Tidy button causes a library to be tidied up. Select a library to tidy by clicking on it in the list, then click on the Tidy button. When the library has been tidied a message box will appear informing you of this.

Libraries will need tidying after they have been extensively edited. Tidying the library will make it smaller by removing the unwanted old (now deleted) symbols in the library.

Refresh symbols from libraries

Normally symbols are saved with the design, so any changes to the libraries do not effect your design straight away.

This option causes all the libraries currently in use to be re-read, and any changes displayed in the current design. This only effects the design in the current window.

Part in Package

This option can only be used when you are editing a library symbol.

When a symbol has more than one part per package, this option allows you to edit each part individually.

Each part in the package must have the same symbol outline, but with different pins. Therefore this option only effects the pins in the symbol.

When you select a new part per package, which has not yet been defined, you will be given the option to copy over the pins in the current part into the new part. Select Yes, if you wish to have the pins in the same layout for each part in the package. This is highly recommended. Once the pins have been copied, you can edit their pin numbers using the Edit Item option in the Edit menu.

Add Pin

This option can only be selected when you are editing a library symbol.

Pins are used to show where the connections to each symbol are.

Pins of various shapes are provided, however, these shapes are for cosmetic purposes only. They do not effect how each pin is considered to be connected.

There are various types of pin. These type govern how the electrical rules checker operates. The electrical rules checker checks which pins of what type are connected together and determines whether or not this will produce a correct circuit.

All pins must have a pin number. If the device is not one that has pins numbers (such a capacitor), then what the numbers are is arbitrary - but they must all be different. Pin numbers can also include letters. This is so the pins of a Pin Grid Array device can be correctly labeled.

Pins can optionally have a name. This is not necessary however.

The pin number and name can be shown or hidden. To hide the text click on the check box next to the text in the dialogue box.

Pins of type power are special. Although they are shown when editing a symbol, when the symbol is placed in a design these pins are hidden. Once the symbol is placed in a design pins are automatically connected to the power of the same value as their name. Therefore these pins must have a name. This can be used in conjunction with the parts per package option to allow the placing of, for example, logic gates, without need to show the power connection explicitly. A power pin cannot be connected to normally, all connections to this pin will be done automatically.

A pin of type hidden will be shown when editing a symbol, as with power pins, and hidden when the symbol is placed into a design. However, the normal connections are expected to be made to this pin, even though it is unseen. The symbol design must indicate where these pins are to allow easy connection.

Each pin is associated with a part per package. A single symbol may have more than one part per package. For example a 7400, consists of 4 NAND gates. Each part has different pin numbers on each pin. To select which part per package the pin you are placing belongs to use the Part in Package option in the Library menu.

To place a pin click with the left hand mouse button in the design window. When a pin has been placed, the pin number in the dialogue box will automatically be advanced for you.

Placing can be canceled by clicking with the right hand mouse button.

Once a pin is placed the pin number is either incremented or decremented, automatically for you. The Pin Increment/Pin Decrement options in the repeat directions menu (in the Edit menu) select which way the pin number is changed.

Also if the pin name has a number at then end of it then it too is also incremented or decremented. The Name Increment/Name Decrement options in the repeat directions menu (in the Edit menu) select which way the pin name is changed.

Pins can be edited. To edit them select the Edit Item option in the Edit menu, then click on the end of the pin (the same end as you placed, and would connect a wire to).

Pins can also be moved or deleted.