Applied Parameters: ParameterSet=NetClass
Summary
This command is used to place a Net Class directive onto the active document. This is essentially a pre-configured Parameter Set object, which is a container for one or more parameters, and which can be associated to a net object within a schematic design. Net Class directives enable you to create user-defined net classes on the schematic. When a PCB is created from the schematic, the information in a Net Class directive is used to create the corresponding Net Class on the PCB. To make a net a member of a net class, attach a Net Class directive to the relevant wire, bus, or signal harness, and set the directive's ClassName parameter to the name of the desired class.
While Net Classes can be created fairly easily from within the PCB editor, the logical function or grouping of Nets is usually much clearer in the Schematic, and so it makes more sense to drive the process from there.
For detailed information about this object type, see
Parameter Set.
Access
This command can be accessed from the Schematic Editor by:
- Choosing the Place » Directives » Net Class command from the main menus.
- Right-clicking in the main design workspace and choosing the Place » Directives » Net Class command from the context menu.
Use
After launching the command, the cursor will change to a cross-hair and you will enter design directive placement mode.
- Position the cursor over a wire or other net object and click, or press Enter, to effect placement.
- Continue placing further directives or right-click, or press Esc, to exit placement mode.
Additional actions that can be performed during placement – while the parameter set is still floating on the cursor – are:
- Press the Tab key to access the Parameters dialog, from where properties for the parameter set can be changed on-the-fly.
- Press the Alt key to constrain the direction of movement to the horizontal or vertical axis, depending on the initial direction of movement.
- Press the Spacebar to rotate the parameter set anti-clockwise or Shift+Spacebar for clockwise rotation. Rotation is in steps of 90°.
Tips
- A newly-placed Net Class directive contains a default parameter with name ClassName, and undefined value. Simply edit this parameter's value to define the name for the net class.
- Attach a Net Class directive to a Blanket object, to create a net class whose members are the individual nets covered by that blanket. If a PCB Layout directive is also attached to that blanket, the PCB Layout directive's rule parameters will target that net class, rather than each individual net. When importing the changes into the PCB document, this results in a single design rule being created (per parameter), with a scope set to target the net class.
- To ensure Schematic defined Net Classes are propagated to the PCB, the following options must be set in the Options for PCB Project dialog:
- Enable the Generate Net Classes option located in the User-Defined Classes region of the dialog's Class Generation tab.
- On the dialog's Comparator tab, set the Differences Associated with Nets » Extra Net Classes checking mode to Find Differences.
- While attributes can be modified during placement (Tab to bring up associated properties dialog), bear in mind that these will become the default settings for further placement unless the Permanent option on the Schematic – Default Primitives page of the Preferences dialog is enabled. When this option is enabled, changes made will affect only the object being placed and subsequent objects placed during the same placement session.
Altium Designer Documentation
...
((Command Reference))_AD
((Sch Commands))_AD