Design Rule Checker

Created: February 05, 2019 | Updated: August 18, 2021 | Applies to versions: 19.0, 19.1, 20.0, 20.1 and 20.2

Now reading version 20. For the latest, read: Design Rule Checker for version 21

The Design Rule Checker dialog

Summary

The Design Rule Checker dialog allows you to configure design rule checking for the board. Design Rule Checking (DRC) is a powerful automated feature that checks both the logical and physical integrity of a design. Checks are made against any or all enabled design rules and can be made online, during design, or as a batch process (with an optional 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 a batch mode design rule check always be performed prior to generating final artwork.

Online Design Rule Checking runs in the background, in real-time, flagging and/or automatically preventing design rule violations. This is especially helpful when manually routing to immediately highlight clearance and width violations.

Using validation reports defined in an assigned Output Job file provides the ability to validate your designs as an integral part of the board design release process. These validation checks will be performed on every release and the release will fail if any validation checks are not passed successfully. This gives you additional peace of mind that costly errors do not creep in to your released designs due to last-minute changes. Validation is run at the Validate Design stage of the process flow within the PCB Release view. In Design Mode, the validation checks are performed directly on your project before outputs are generated. In Release Mode, the release flow first builds a self-contained snapshot from your project that includes all project documents and external dependencies, and the validation checks are performed on this snapshot. This provides additional security that the snapshot has correctly captured all the required dependencies for your project.

Online DRC only detects new violations – violations that are created after the feature is enabled – while Batch DRC allows a check to be manually run at any time during the board design process. So while good designers know the value of the Online DRC, they also know that board design should begin and end with a Batch DRC.

Access

The dialog is accessed from the PCB Editor by clicking Tools » Design Rule Check from the main menus.

Options/Controls

The dialog's functionality is essentially divided into two areas:

Configuration of options relating to a Batch DRC.
Configuration of which rules to check, and whether those rules should be checked as part of the Online and/or Batch DRC.

These areas are reflected by, and accessed through, the folder-like entries in the left-hand pane.

Report Options

Clicking on the Report Options folder loads the right-hand side of the dialog with additional options that are available when running a Batch DRC.

DRC Report Options

Create Report File - enable this option to have a report generated after running a Batch DRC for the board.

The report is in HTML format and will be named Design Rule Check - PCBDocumentName.html. It will be automatically opened as the active document after the Batch DRC process has been completed.
Create Violations - enable this option to have violations highlighted in the design space in accordance with defined violation display settings. This option is also required to have violations appear listed in the Violations region of the PCB Rules And Violations panel.

Management of how DRC violations are displayed – using custom violation graphics and/or a defined violation overlay – is performed on the PCB Editor - DRC Violations Display page of the Preferences dialog.
Sub-Net Details - if an Un-Routed Net rule has been defined, enable this option to include sub-net details in the DRC report.

The Un-Routed Net rule should only be enabled for checking when all connections have been routed, as a connection line is effectively an "open circuit".
Verify Shorting Copper - enable this option to verify the integrity of the shorting copper in any Net Tie components used in the design. This check looks for any unconnected copper in a component (indicative of a pad not shorting the other pad(s) correctly).
Report Drilled SMT Pads - enable this option to include any SMT (Surface Mount Technology) pads that have been erroneously drilled in the DRC Report.

An SMT pad can be, for example, a short pin; flat contact; one of a matrix of balls (BGAs); a termination on the body of a component (passives); or a short lead in a gull-wing formation (QFPs).

This option is only for detecting SMT pads with holes defined in them, which was possible in legacy versions of the software. To check for vias under SMD pads, the Vias Under SMD rule (in the High Speed category) must be added to the design and enabled for Batch DRC.
Report Multilayer Pads with 0 size Hole - enable this option to include any invalid multi-layer pads found in the design. An invalid multi-layer pad is one whose hole size is zero that would otherwise make it an SMT pad.
Stop when n violations found - use this field to determine the maximum number of violations that can be detected before the batch DRC process is stopped (default = 500). Limiting the number of violations that are reported is a key strategy in keeping the checking process manageable.

Split Plane DRC Report Options

Report Broken Planes - enable this option to have the batch rule checking process look for and report broken planes. Broken planes occur when an area of a plane that has connectivity to a net becomes electrically disconnected from the rest of the plane. An example of where this may occur is a connector placed across a split plane but not connected to it. The voids around the pins join to completely cut through the plane copper, effectively breaking it into two parts.

To check for broken planes, the Un-Routed Net rule (in the Electrical category) must be enabled for Batch DRC.
Report Dead Copper larger than - enable this option to have the batch rule checking process look for, and report, dead copper regions larger than the specified area. Dead copper refers to sections of copper that have no connectivity to a net, and which also become electrically disconnected from the original parent plane. An example of where this may occur is a connector (not connected to the plane) with closely spaced pins, in which the voids around the pins join to isolate areas of plane copper from the rest of the plane. Use the associated field to specify a value for the minimum permissible area of dead copper, beyond which is considered a rule breach (default = 100 sq. mils).

To check for dead copper, the Un-Routed Net rule (in the Electrical category) must be enabled for Batch DRC.
Report Starved Thermals with less than n% available copper - enable this option to have the batch rule checking process look for and report 'starved' thermal connections larger than the specified percentage. Thermals are connections to a plane with thermal relief 'cutouts' around them to reduce heat conductivity to the plane copper. A thermal can become 'starved' when the surface area of the copper spokes connecting it to the plane is reduced by void areas. This option also checks the surface area for the thermal (not just the spokes) against any void areas that encroach into the thermal. Use the associated field to specify a value for the minimum permissible percentage of connecting copper that must remain, below which is considered a rule breach (default = 50%).
Run Design Rule Check - click this button to perform a Batch DRC in accordance with rules enabled for Batch checking and additional options defined for this type of checking.

After the check has been completed, all violations will appear in the Messages panel.

Rules To Check

The Design Rule Checker dialog, listing all rules that can be checked.

Clicking on the Rules To Check folder loads the right-hand side of the dialog with a list of all checkable rule types. Alternatively, click on a specific category (below the folder) to list only those design rule types associated to that category.

For each rule type, the following information is presented;

Rule - the type of rule.
Category - the parent category to which the rule type is associated.
Online - the current state of this rule type with respect to Online DRC (where available). Click to toggle.
Batch - the current state of this rule type with respect to Batch DRC. Click to toggle.

Enable each rule type for Online and/or Batch checking as required.

Use the right-click menu to access commands for quickly enabling/disabling all rule types for Online or Batch DRC or only those rule types that are used (defined and enabled for use).

Tips

A generated Design Rule Verification Report lists each rule that was tested during the batch checking process as specified in this 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. Click on the entry for an offending object to cross probe directly to that object in the design space.
To give further flexibility when displaying rule violations in the design space, the two violation display types – violation details (custom violation graphics) and violation overlay – have separate associated system colors. This allows you to differentiate between the two using different, distinct colors. Color assignment is performed on the Layers & Colors tab of the View Configuration panel:
1. Violation Details – uses the color assigned to the Violation Markers color in the System Colors region.
2. Violation Overlay – uses the color assigned to the DRC Error Markers color in the System Colors region.
After running a Batch DRC, double-click on a violation message in the Messages panel to cross-probe to the object(s) causing that violation in the design space.
When running an Online or Batch DRC, any rule violations will be listed in the Violations region of the PCB Rules and Violations panel.
Violations associated with a particular design object can be interrogated directly within the PCB design space. Position the cursor over an offending object, right-click then choose a command from the Violations sub-menu. Either choose to investigate an individual violation that the object is involved in, or choose to view all violations in which it is involved, using the Show All Violations command. In each case, the Violation Details dialog will appear providing detailed violation information and controls for highlighting and jumping to the offending object(s).

Printer-friendly version

If you find an issue, select the text/image and pressCtrl + Enterto send us your feedback.