Project Options - Class Generation

Modified by Jason Howie on Mar 13, 2015
Contents

Parent page: WorkspaceManager Dialogs

The Class Generation tab of the Options for PCB Project dialog.

Summary

This tab of the Options for PCB Project dialog enables you to configure and control class generation. Classes are a logical collection of a particular type of design object. For example, a group of related components could be grouped into their own Component Class which could then be used as the basis for creating a targeted rule. This tab provides controls to determine which classes are automatically generated, and which user-defined classes are generated, when the source schematic documents are synchronized with the PCB design document.

Access

This is one of multiple tabs available when configuring the options for a project – accessed from within the Options for PCB Project dialog. This dialog is accessed by:

  • Clicking Project | Content | , from the main menus in the Schematic Editor, or the PCB Editor.
  • Right-clicking on the entry for the project itself, on the Projects panel, and choosing Project Options from the context menu.

Options/Controls

Automatically Generated Classes

  • Generate Net Classes for Buses - enable this option to automatically generate a net class for each bus in the design. The members of a class will be the individual constituent nets of the bus (from which that class was generated).
A generated net class will be named using the name of the bus.
  • Generate Net Classes for Components - enable this option to automatically generate a net class for each component in the design. The members of a class will be the associated nets to which the pins of the component (from which that class was generated) are connected.
A generated net class will be named using the designator of the component, in the format <ComponentDesignator>_Nets.
  • Generate Net Classes for Named Signal Harnesses - enable this option to automatically generate a net class for each named signal harness in the design. The members of a class will be the nets associated to the signals gathered by the named signal harness (from which the class was generated).
A named signal harness is one that has a net label attached to it. A generated net class will be named using the name of the net label attached to the signal harness.
  • Sheet-Level Class Generation - this region of the tab allows you to control the automatic generation of component and/or net classes at the individual schematic sheet level. All source schematic sheets for the project are listed, with the following information presented for each:
    • Sheet Name - the name of the schematic document.
    • Full Path - the absolute path to the folder in which the document resides.
    • Component Classes - enable this option to have a component class generated for the sheet.
    • Net Classes Scope - use this field to determine whether to have a net class generated for the sheet and, if so, the scope of generation. The field's drop-down provides the following choices:
      • None - do not generate a net class for this sheet.
      • Local Nets Only - do generate a net class for this sheet, but only containing member nets that are local to the sheet.
      • All Nets - do generate a net class for this sheet, containing all member nets associated with the sheet (local, and those that go elsewhere).
Enable/disable component class generation, or set the scope for net class generation en-masse, using commands available from the right-click context menu for a column. Multiple sheet entries can be selected using standard multi-select techniques (Ctrl+click, Shift+click, click&drag).
For components and/or nets on the top sheet, the respective component and/or net class will be named using the schematic document name. For components and/or nets on child sheets, the respective component and/or net classes will be named using the sheet symbol designators.
The text at the bottom of this region dynamically changes based on the choices made, and provides a summary of which classes will be automatically generated.

User-Defined Classes

  • Generate Component Classes - enable this option to generate user-defined component classes, when the design is transferred to the PCB. Component classes are manually defined on the schematic by adding a ClassName parameter to targeted components, and setting its value to the desired class name.
  • Generate Net Classes - enable this option to generate user-defined net classes, when the design is transferred to the PCB. Net classes are manually defined on the schematic through use of the Net Class directive. To make a net a member of a Net Class, attach a Net Class directive to the relevant wire or bus (or a blanket) and set the value of the its ClassName parameter to the desired class name.
Note: To generate classes (automatic and/or user-defined) when transferring the design to the PCB, you must ensure that the respective Comparator settings have been set to , on the Comparator tab of the Options for PCB Project dialog. For net classes, this is the Extra Net Classes comparison type, found in the Differences Associated with Nets category. For component classes, this is the Extra Component Classes comparison type, found in the Differences Associated with Components category.

 

In addition, you must ensure that the respective ECO settings have been set to , on the ECO Generation tab of the Options for PCB Project dialog. For net classes, this is the Add Net Classes modification type, found in the Modifications Associated with Nets category. For component classes, this is the Add Component Classes modification type, found in the Modifications Associated with Components category.

 

You are reporting an issue with the following selected text and/or image within the active document: