Class Generation Options for a Project in Altium Designer

The Class Generation tab of the Options for Project dialog

Summary

This tab of the Options for 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 dialog is one of multiple tabs available when configuring the options for a project and is accessed from within the Options for Project dialog. To access the Options for Project dialog:

• From the PCB or schematic editor, click Project » Project Options.
• Right-click on the project name on the Projects panel, then click Project Options from the context menu.

Options/Controls

Automatically Generated Classes

• Generate Net Classes for Buses - check 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).

• Generate Net Classes for Components - check 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.

• Generate Separate Net Classes for Bus Sections - check this option to automatically generate a separate net class for each bus section. A bus section is created by specifying a bus which is actually a section of a larger bus, for example D[15..8], from the bus D[15..0].
• 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).

• Sheet-Level Class Generation - this area 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 - check 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 - generate a net class for this sheet but only containing member nets that are local to the sheet.
    • All Nets - generate a net class for this sheet that contains all member nets associated with the sheet (local and those that go elsewhere).
  • Structure Classes Generate Structure - check this option to have a structure class generated for the sheet.

User-Defined Classes

• Generate Component Classes - check 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 Rooms for Component Class - check this option to generate rooms based on the user-defined component classes. These components need to have the component parameter with 'ClassName' as its parameter name.
• Generate Net Classes - check 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 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 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.