Tutorial: Real-Time Impedance and Coupling Analysis

April 22, 2019 Team EMA

Trying to find impedance and coupling issues in your design can be a tedious and time-consuming process. Finding these issues AFTER your design is completed can lead to a complete re-spin of your design, possibly making your project late and overbudget. Real-time Impedance and Coupling Analysis in OrCAD PCB Designer Professional allows you to quickly find and fix problematic traces throughout the design process. This tutorial will show you how easy it is to simulate and view impedance and coupling issues in your traces with no additional steps or modeling by utilizing the included workflow manager. If you would like to follow along, you can download the design files here.
 

Step 1: In OrCAD PCB Designer Professional, Open the Workflow Manager. 

You can do this by selecting Analyze Workflow Manager from the Toolbar. Make sure the Impedance Workflow is selected.

Note: The Analysis Workflow Manager will walk you through the necessary steps and settings to perform the Coupling or Impedance Analysis.
 


 

Step 2: Complete the Set Up for Analysis.

Under Analysis Mode select “Net Based”.

Note: The following options are available for analysis:
  • Net Based: Allows every segment of selected nets or all nets to be simulated. This Analysis Mode is selected by default.
  • Directed Group: Allows you to select specific connections between a starting component and ending component(s) and only simulate that portion of the net.  (If you need more information on Directed Groups, including the set-up, see this blog post to get a step-by-step overview)
     

Click Select Nets. This will bring up a window where you can select specific nets or all the nets in the design. Select all the nets in the design by pressing the >> button and click OK.

Note: By selecting Analysis Options, you can detect and model coplanar traces in the Impedance Analysis Parameters window.  By default, this option is not enabled.
 


 

Step 3: Run the Analysis. 

Select Start Analysis from the Analysis Workflow Manager. This will perform the analysis. The progress bar will report the status of the analysis.
 


 

Step 4: View the results.

Under View Modes select “Net Based” and “Differential Pairs”.

Note: The following Analysis Modes are available to view:
  • Net Based: Displays results for all segments or selected nets.
  • Directed Group: Displays results for the segments defined in selected directed group. This option is only available if results contain directed group data.
  • Single Ended: Displays sin
  • gle ended analysis results for both single-ended and differential pair nets.
  • Differential Pairs: Displays differential pair analysis results for differential pair nets and single-ended results for single-ended nets.
     

View the results using the Impedance Table. The Impedance table is broken down into two different views: the Summary Table and Detailed Table. The Summary Table shows the following information:

  • Net Names
  • Vias
  • No Ref
  • Color Coded Impedance Values (Ohm)
  • Minimum, Maximum, and Typical
  • Impedance Length (%)
  • Minimum, Maximum, and Typical
  • Trace Total Length
  • Trace Total Delay (nS)
  • The Detailed Table includes the following information:
  • Color Coded Impedance (Ohm)
  • Length
  • Trace Delay (pS)
  • Layer
  • Location (x;y)
Note: The Single Ended Impedance Table will also show Trace Total R (mOhm), Trace Total L (nH), and Trace Total C (pF).
 


 

View the results using Impedance Vision. Adjust the Imp [Ohm] bar to only view traces with problematic impedance values.

Note: With Impedance Vision, the color code is applied to the traces on your board.
 


 

Step 5: Select the Coupling Workflow from the Analysis Workflow Manager Window.



 

Step 6: Complete the set up the Analysis.

Under Analysis Mode select “Net Based”.
 

Click Select Nets. This will bring up a window where you can select specific nets or all the nets in the design. Select all the nets in the design by pressing the >> button and click OK.

Note: By selecting Analysis Options, you can set Coupling Analysis Parameters including the following:
  • Detect and Model Coplanar traces: Choose to include coplanar data in simulation results. By default, this option is not enabled.
  • Coupling (%): Specifies the minimum net level coupling coefficient threshold. The default value is 2%.
  • Rise Time (ps): Specifies the rise time for minimum coupled length. The default value is 50 ps.
  • GeoWindow: Set a geometry window value in design units for aggressor inclusion for the selected victim nets. All net segments within the specified distance from the selected net, across all layers, will be considered aggressors. This option is only available for coupling analysis and will allow additional potential aggressor traces to be found based on the window.


 

Step 7: Run the Analysis.

Select Start Analysis from the Analysis Workflow Manager. As with the Impedance Workflow, this will perform the analysis. The progress bar will report the status of the analysis.
 


 

Step 8: View the results.

Under View Modes select “Net Based” and “Worst Case”.

Note: The following Analysis Modes are available to view in the Coupling Analysis:
  • Net Based: Displays results for all segments or selected nets.
  • Directed Group: Displays results for the segments defined in selected directed group. This option is only available if results contain directed group data.
  • Worst Case: Displays the maximum coupling coefficient for all segments or selected nets.
  • Victim Analysis: Displays all aggressor segments for a specific victim net.

View the results using the Coupling Table. The Coupling Table is broken down into two different views- the Summary Table and Detailed Table. The Summary Table shows the following information:

  • Net Name
  • Max Coupling
  • Aggressor Net Name
  • Color Coded Coef (%)
  • Length (%)
  • Percentage of Length with Coupling Coefficient
  • >5%
  • 2-5%
  • Total Coupling Index (millimeter-%)
  • The Detailed Table includes the following information:
  • Victim Trace Ref
  • Aggressor Net
  • Aggressor Trace Ref
  • Coupling Coefficient
  • Length
  • Layer
  • Victim Segment
  • Aggressor Segment



 

View the results using Coupling Vision. Adjust the Coef [%] bar to only view traces with problematic coupling coefficient values.

Note: With Coupling Vision, the color code is applied to the traces on your board.
 


 

Step 9: In the Coupling Vision, adjust the problem routes to incorporate additional space between traces.

Note: This can be accomplished by selecting the Slide button from the toolbar and sliding the traces.
 


 

Step 10: Run the Coupling Analysis again.
This can be done by selecting Start Analysis in the Coupling Workflow Manager. Select OK in the pop-up window to replace the analysis data and view the results.
 

The analysis has completed using the adjusted traces and the coupling issues have been resolved.
 


 

Real-Time Impedance and Coupling Analysis in OrCAD PCB Designer Professional quickly analyzes a specialized selection of nets or all the nets on your board throughout your design process. With visually compelling information about the trace impedance and coupling coefficients, you can easily identify and fix problem areas on your board before design completion, saving you time and reducing errors or even complete re-spins.

Video Tutorial
 

Previous Article
Tutorial: Managing Signal Integrity Analysis Results with User Directed Groups in OrCAD
Tutorial: Managing Signal Integrity Analysis Results with User Directed Groups in OrCAD

Creating Directed Groups within OrCAD PCB Designer

Next Article
Tutorial: Real-Time Placement Analysis
Tutorial: Real-Time Placement Analysis

With designs increasing in complexity and speed, it is more important than ever to ensure your design funct...