Virtual Workshop: Design Rule Check

August 10, 2020

Duration: 15 minutes | Version Required: 17.4

With PCB complexity increasing and deadlines shortening, there is little to no room for error. While design teams often look at DFM as a “manufacturing problem,” the fact is these changes rarely get back to the design team and are often made without a full understanding of the design and its requirements; leading to design failures, production delays, etc. This can be avoided by taking DFM and DRC into your own hands, allowing you to alter any issues in engineering, where changes are can be made easily. OrCAD DRC can help you to find manufacturing errors as you design so you can be sure your product can not only be manufactured in high volumes, but electrically performs as intended.

This document is intended to provide step by step instructions on using design rule checks in OrCAD PCB Designer Professional. For this workshop, download the design files and use the provided design, DRC_Start.BRD, to follow along. To view the completed design, select DRC_Finish.BRD.

  1. Open the provided design, DRC_Start.BRD, in OrCAD PCB Designer Professional.

  1. Select Tools > DRC Browser from the menu.

  1. Select Show DRC Chart.

  1. Click the bar on the graph for additional information.
  2. Close out of the graph and minimize the DRC Browser.

  1. Back in the PCB, mouse over the DRC Marker by Via21 N004.

Note: View the text for additional information to resolve the DRC Error. This error is the result of a trace placed too closely to the via.

  1. Select Setup > Application Mode > Etch Edit from the menu.

  1. In the Find Tab, select off of DRC Error for easier selection of the trace.

  1. Click on the trace that is causing the error.

  1. Move the trace away from the via and click to place.

Note: The DRC marker is no longer visible, and the DRC error is resolved.

  1. Select Setup > Constraints from the menu.

  1. In the Worksheet Selector, select Manufacturing > Design for Fabrication > DFF Constraint Set> Copper Spacing.

  1. In the Constraint Set Window, expand Trace To and view the assigned constraints.

Note: You can manage your spacing constraints here and re-use the constraints for multiple designs. For re-use, export the constraints to spreadsheet form: Fileà ExportàConstraints.

  1. Close the Constraint Manager and open the DRC Browser. Browse to the following path: DRC > Design for Fabrication > Copper Spacing > Trace to > All via pads.


Note: You can filter the DRC errors by selecting the asterisk (*) in the desired column and selecting a filter.

  1. Click on the DRC Location.

Note: This will bring you to the location of the DRC Marker on the PCB. Remember to select DRC Error in the Find Tab to view more information when you mouse over the DRC error.

  1. Flag an error by checking the box next to the corresponding coordinates in the DRC Location.

  1. Select Review to view the flagged errors.

With design deadlines shortening and complexity increasing, you can’t afford to leave DFM and DRC in the hands of your manufacturers. OrCAD helps empower your design decisions by allowing you to find any potential manufacturing errors in real-time, as you design so you can be rest-assured your product will perform as intended and can be manufactured without issue.  

If you would like more tutorials, visit our walk-through page to view additional OrCAD and PSpice video tutorials and download design files.

Don't have OrCAD 17.4? Download the Trial Now

Previous Article
Virtual Workshop: In-Design Analysis
Virtual Workshop: In-Design Analysis

Ensuring established rules are met is essential to produce quality designs. In-design impedance & coupling ...

Next Article
Virtual Workshop: Constraint Management
Virtual Workshop: Constraint Management

Embedded rules and constraints allow PCB design intent to be conveyed clearly, reducing overall confusion a...