Creating a Package

Creating a package

A part or hierarchical block may have an underlying hierarchical description, such as an attached schematic folder. If it does, it is called a non-primitive. A part or hierarchical block that has no underlying hierarchical description is called a primitive. In Capture, this characteristic is defined in a property, called Primitive, on every part instance. You can change the Primitive property as often as you like during the design process. When a part or hierarchical block is marked as primitive, all of Capture's tools treat it as such. You cannot descend into a part or hierarchical block that is marked as primitive, even if it has an attached schematic folder.

For example, you might create a part and attach a schematic folder that describes its gates and wiring, and then attach schematic folders to some of those parts to describe their transistors. Before you create a netlist for simulation, you should specify those parts as non-primitive, so Create Netlist can descend far enough to find the transistor-level descriptions. Before you create a netlist for board layout, you should specify the parts as primitive, so Create Netlist stops at the gate-level descriptions. Bill of Materials and Cross Reference work similarly.

For part instances that have their Primitive property set to Default, you can configure Capture to treat them as either primitive or non-primitive on a design-wide basis, using the Design Template and Design Properties commands on the Options menu. This is useful when you are describing and simulating your design at varying levels of abstraction (as in a top-down design).

If you attach a schematic folder to a homogeneous part, it is attached to each part in the package, not the package itself. You cannot attach a schematic folder to a heterogeneous part.

When you attach a schematic folder to a part or hierarchical block, you can specify a full path and file name in the Library text box. So, although you can specify a library that has not been saved, you should not try to descend into the attached schematic folder until the library that contains the schematic folder has been saved.

If you do not specify a full path and file name in the Library text box, Capture expects to find the attached schematic folder in the same design as the part of hierarchical block to which it is attached. If the specified schematic folder does not exist in either the design or library, Capture creates the schematic folder when you descend the hierarchy on the part or hierarchical block.
For compatibility with future versions of Windows, Capture preserves the case of the path and filename as you specify them in the Library text box.

Using the package view

In the part editor, to view and edit all sections of a part, click the Edit Pins of All Sections button in the Property Sheet pane. The Edit All Sections dialog box opens.

Forcing multiple parts into a single package

For PCB designs, if you need to make sure that two or more parts in your design are in the same package, you use the Update Part Reference tool. First, choose a property that all the parts share and verify that the parts all have the same value for that property, then use the Update Part Reference tool.
For example, you might have several NANDs in a schematic folder and four that are in close proximity in the final product. For each of the four NANDs, create a user-defined property named COMPGROUP and set the property's value to 1. In the Combined Property String text box in the Update Part Reference dialog box, enter {COMPGROUP}.

To specify ignored package pins

The IGNORE property, available for package pins, provides a method for you to specify that certain pins on a part are ignored when the part is placed on a schematic page. Pins that have the IGNORE property assigned to them do not appear on the schematic page. These pins will also not be included on the part footprint for any downstream PCB layout tools. Also, note that ignored pins will not be included in any back annotation from a layout tool.

1. Open a part in part editor.
   The Package Properties section appears in the Property Sheet pane.
2. In the Section Pins section of the Property Sheet pane, select the Pin Ignore check box for all the pins that you want to ignore.
3. Click the Apply Pin Changes button.
4. Save the part.

To force multiple parts into a single package

1. Choose one property that the parts share and assign the same value to that property for each part. You may want to add a user-defined property to each part.
2. In the project manager, select schematic folders or schematic pages if you want to process only a portion of the design. If you want to process the entire design, leave the schematic folders or schematic pages unselected.
3. Choose Tools - Annotate.
   The Annotate dialog box appears.
4. In the Combined Property String text box, enter the property name. The name must be enclosed in braces: "{" and "}".
5. Verify that the remaining dialog box options are set the way you want them. For example, specify, among other things, whether you are unconditionally updating all references or only those that are set to the unassigned (?) reference.
6. Click OK.

Shortcut

Toolbar:

To create a multiple-part package

1. Open the library that will contain the part.
2. Choose Design – New Part.
   The New Part Properties dialog box appears.
3. In the Parts per Pkg field, specify the number of parts in the package, and also specify whether they are all the same (homogeneous) or different (heterogeneous).
4. Specify the other properties and click OK.
   The part editor opens with an empty part outline.
5. Edit the part properties as required in the Property Sheet pane.
6. Choose File – Save.
   If you are creating the part in a new library that has not yet been saved, the Save As dialog box appears to name the library file.