Design Rule Checking (DRC) is a powerful automated feature that checks both the logical and physical integrity of your design. Checks are made against any or all enabled design rules and can be made online, as you work, and/or as a batch check, with results listed in the Messages panel and a generated report. This feature should be used on every routed board to confirm that minimum clearance rules have been maintained and that there are no other design violations. It is particularly recommended that you always perform a design rule check prior to generating final artwork.

Configuring the DRC

Configuration for the check is carried out in the Design Rule Checker dialog, accessed by selecting the Design Rule Check command from the PCB Editor's Tools menu ( Tools » Design Rule Check ).

In the folder list on the left side of the dialog, each of the design rule categories whose rule types can be checked are listed under the Rules To Check folder. Click on the Rules To Check folder to list all checkable design rule types, across all categories, in the right side of the dialog.

Click on a category to list all associated (and checkable) design rule types for that category.

Enable/disable Online (where available) and/or Batch checking options for each rule type you wish to check. Use the options available from the right-click pop-up menu to enable/disable checks of all rule types, or to enable checks of all used rule types only.

Using Online DRC

To turn on the Online DRC feature, enable the Online DRC option on the PCB Editor - General page of the Preferences dialog ( Tools » Preferences ). Online Design Rule Checking runs in the background, as you work, flagging and/or automatically preventing design rule violations. Errors are highlighted in the document by outlining the violating object(s) in the current DRC Error Markers color, defined in theSystem Colors region of the View Configurations dialog ( Design » Board Layers & Colors ).

Using Batch DRC

Batch Design Rule Checking allows you to manually run a check at any time during the board design process. When setting up a batch DRC, various additional options can be defined by clicking on theReport Options folder, in the folder-tree pane of the Design Rule Checker dialog. These options include generation of a report.A batch DRC is initiated by clicking the Run Design Rule Check button, at the bottom left of the dialog. After the check has completed, all violations will appear listed as messages in the Messages panel.If the Create Violations report option is enabled, clearance, length and width errors will be highlighted on the PCB document.

DRC Reports

Enable the Create Report File option in the Design Rule Checker dialog to generate a DRC report. Options available on the PCB Editor - Reports page of the Preferences dialog allow you to specify in which format the report is generated and whether a report is automatically displayed in the main design window. The following report formats are available:

• TXT - producing the Design Rule Check - PCBDocumentName.drc file
• HTML - producing the Design Rule Check - PCBDocumentName.html file
• XML - producing the PCBDocumentName.xml file.
   

By default, TXT and HTML formats are generated, with the HTML report being displayed after generation

                                                  .

The report lists each rule that was tested, as specified in the Design Rule Checker dialog. Each violation that was located is listed with full details of any reference information, such as the layer, net name, component designator and pad number, as well as the location of the object. In the HTML format report, click on the entry for an offending object to cross probe directly to that object in the workspace.