Adding Design Rule Directives to a Schematic Document
Design constraints (rules) can be defined prior to PCB layout, by adding parameters that are configured as design rule directives to the schematic source document(s). The scope of the corresponding PCB design rule, created when the design is transferred to the PCB document, is determined by the nature of the object to which the parameter (added as a rule) is assigned. The following table summarises the schematic parameter-to-PCB rule scope options that are supported:
| Add a Parameter (as a rule) to a... | From... | For a PCB rule scope of... |
| Pin | the Parameters tab of the Pin Properties dialog | Pad |
| Port | the Parameters tab of the Port Properties dialog | Net |
| Wire | the Parameters dialog, after placing a PCB Layout Directive (Parameter Set object) on the wire using the Place » Directives » PCB Layout command | Net |
| Bus | the Parameters dialog, after placing a PCB Layout Directive (Parameter Set object) on the bus using the Place » Directives » PCB Layout command | Net Class |
| Harness | the Parameters dialog, after placing a PCB Layout Directive (Parameter Set object) on the harness using the Place » Directives » PCB Layout command | Net Class |
| Blanket | the Parameters dialog, after placing a PCB Layout Directive (Parameter Set object) on the edge of the Blanket using the Place » Directives » PCB Layout command. Include a ClassName parameter to create a net class for all nets covered by the blanket, which will then be used for the rule scope. | Net Class |
| Component | the Parameters region of the Component Properties dialog | Component |
| Sheet Symbol | the Parameters tab of the Sheet Symbol dialog | Component Class |
| Sheet | the Parameters tab of the Document Options dialog ( Design » Document Options ) | All Objects |
In each case, the method of adding a rule-based parameter is the same. From the respective tab or dialog, perform the following:
- use the Add as Rule button - the Parameter Properties dialog will appear, with the Name and Type fields set to Rule and STRING respectively and uneditable
- click the Edit Rule Values button to open the Choose Design Rule Type dialog. This dialog lists each of the rule categories and types that are available in the PCB document and for which you can validly add as a rule parameter in the schematic document.
- select a rule type and click OK (or double-click on it) to open its corresponding Edit PCB Rule (From Schematic) dialog, from where you can define the constraints for the rule.
Synchronicity through Unique IDs
When adding design rule parameters to objects on a schematic, a unique ID is given to each rule parameter. The same IDs are given to the corresponding design rules that are created in the PCB. With this Unique ID, the constraints of a rule can be edited on either the schematic or PCB side and the changes pushed through upon synchronization.For example, consider adding a width rule parameter to a particular wire (associated with the net NETS2_1) on a schematic sheet, by placing a PCB Layout directive:
When you edit the default parameter entry for the directive, you will notice that the Unique ID field in the corresponding Parameter Properties dialog has a specific entry, as illustrated in the image below:
When the design change is passed on to the PCB - using the Synchronizer and generating and executing the relevant Engineering Change Order (ECO) - the rule will be created and added to the defined Width rules for the PCB and will have the same Unique ID assigned to it: