EMA Academy

Quick How-Tos

Home > EMA Academy > How-Tos > How to Add Return Path Vias when Routing High-Speed Signals

How to Add Return Path Vias when Routing High-Speed Signals

When working with high-speed signals, having a good return path is crucial for signal integrity. For some high-speed nets, return path vias should be incorporated every time a via is placed. While these can be added manually after routing is complete, it can be tedious and increase the possibility of errors. With the high-speed option in Allegro PCB Designer, return path vias can be configured and added automatically during routing.

This quick how-to will provide step-by-step instructions on how to configure and add return path vias when routing single nets with the high-speed functionality in Allegro PCB Designer.

How-To Video

Configuring Return Path Via Settings

Step 1: Open the desired design in Allegro PCB Designer with the High-Speed Option enabled.

Routing Traces in Allegro PCB Designer

Step 2: Select Route > Connect from the menu or the Add Connect icon from the toolbar.

Step 3: Click to start routing a trace.

Configuring Return Path Via Settings in Allegro

Step 4: To configure settings, right-click and select Return Path Vias > Settings.

Note: A warning may appear that the feature is in the prototype phase. Click OK.

Step 5: The Return Path Via Setup window opens. Select the ellipsis for Return Path Net to assign a net name.

Step 6: Select the desired net name and click OK.

Note: If a voltage property has been defined for nets in the design, select DC Nets to filter the nets.

Step 7: Select the ellipses for Return Path Via to select the padstack.

Step 8: Select the desired padstack and click OK.

Note: You can filter padstacks from:

  • The database
  • The library
  • What is allowed by the net’s physical constraint set
Configuring the Return Path Via Spacing in Allegro

Step 9: Set the desired via spacing under 1 Via. By default, the minimum spacing is configured.

Note: The 1 via pattern adds one return path via next to one of the trace vias. Here you can configure the:

  • Space X: Circumference-to-circumference distance of the vias.
  • Angle: The angle at which the return path via is located with respect to the trace via.
  • Mirror-Geo: Mirrors the location of the return path via as shown below.

Step 10: Click OK.

Placing Return Path Vias

Step 11: Right-click in the canvas and select Return Path Vias > 1 Via to associate the via.

Activating Return Path Vias During Routing

Step 12: Double-click while routing to activate via placement. Via placement mode will activate as normal and the return path via will attach to your cursor separate from the trace.

Placing Return Path Vias in Allegro

Step 13: Click to place the vias.

Step 14: Continue routing the trace. Right-click and select Done when finished.

Adjusting Vias

Step 15: Select Route > Slide from the menu or the Slide button from the toolbar.

Sliding Vias in Allegro

Step 16: Select one of the vias. The trace and return path via are both attached to the cursor.

Ungrouping Vias and Return Path Vias in Allegro

Step 17: To adjust each via separately, right-click and de-select Return Path Vias Group while the group is selected.

Note: If you reactivate this option after moving one of the vias, the trace and return path vias will lock together as they are.

Step 18: When finished, right-click and select Done.

Wrap Up & Next Steps

Accelerate the PCB layout for high-speed designs and quickly add return path vias while routing with the high-speed functionality in Allegro PCB Designer.  Learn more about solving common issues for high-speed designs with our e-book.

Table of Contents

How To was created with:
Share:
LinkedIn
Email
EMA Design Automation