BoardSurfers: Optimizing RF Routing and Impedance Using Allegro X PCB Editor

Achieving optimal power transfer in RF PCBs hinges on meticulously routed traces that meet specific impedance requirements. Impedance matching is essential to ensure that traces have the same impedance to prevent signal reflection and inefficient power transfer. The key to controlling the impedance is to fine-tune the trace width, trace thickness, and dielectric height that separates the trace from the reference plane in the z-axis. A continuous reference plane beneath the signal layer is also critical in maintaining optimal impedance. Proper track-to-ground clearance on the same layer (for coplanar waveguides) is equally important for consistent impedance control.

Coplanar Wave Guide (Top View)                  Coplanar Wave Guide (Cross-Section View)

This post provides solutions to achieve optimal RF routing and impedance. It guides you on how to protect RF circuits from Electromagnetic Interference (EMI) generated in other sections of the same PCB or neighboring PCBs. It also explains how to convert RF traces to shapes for smoother editing at places where the signal bends. These solutions will help you when routing an RF PCB layout using Allegro X PCB Editor.

Guarding RF Circuits Using Via Arrays to Prevent EMI

Adding shielding on both sides of RF traces protects them from EMI. Via arrays act as a shield and guard the RF signal from the EMI generated in the adjacent circuits. Via arrays are a series of vias placed in a specific pattern around the RF signal, creating a barrier and preventing EMI.

To add via arrays to your design in Allegro X PCB Editor, do the following:

1. Choose Place – Via Array.

2. Open the Options panel.

3. Follow the settings in the Options panel and select Both sides in the Array Parameters Type list, as shown in the following image:

4. Select the RF trace in the design canvas.
A via array is displayed along both sides of the RF trace cline.

5. Tweak the via spacing settings in the Array Parameter pane to get optimal via array preview around the cline.

6. Click anywhere in the design canvas to place the array on both sides of the trace.

Adding Ground Vias to RF Planes

After adding via arrays for all the RF signals, filling large copper planes with ground vias, near the RF part of the layout, maintains a lower impedance for the PCB and improves the ground reference.

You can use the via array command to add ground vias. The following image illustrates an RF section of a PCB layout with the RF signal being guarded by vias on both sides and the ground plane stitched with Gnd vias. This visual can help you understand how vias are to be placed so that they create a barrier around the RF signal.

To learn more about using via arrays, refer to the Allegro X PCB Editor Intermediate course, Module – 3 Interactive Etch Editing, or the course video channel.

Converting RF Traces to Shapes

Typically, RF traces need tapering at necking points to ensure a smooth transition of the RF signal and to avoid abrupt changes in its width. However, when you route RF signals as arc traces, tapering is not possible at places where the trace width needs to be reduced while routing in and out of a component. The following image shows a track that sees impedance change at the neck region:

Shapes offer great flexibility for editing. Converting RF signal traces to shapes at the final stage of routing improves impedance control.

To convert RF traces into shapes for enhanced design flexibility, do the following in Allegro X PCB Editor:

1. Choose Tools – Convert – Cline/Line to Shape.

2. Modify the Options panel settings. You can keep existing clines, retain the nets, or change the shape to dynamic.

3. To identify the traces that should be converted to shapes, specify the area containing them or apply a filter based on width or layer.

4. Select the End cap style option to select a shape (square, circle, octagon, or flush) for the starting and ending edges of the clines as shown in the following image:

RF signals after getting converted to shapes appear as shown here:

Applying Mask Shapes to RF Signals

After finalizing the RF shapes, the next step is to apply mask shapes to the RF signals. This involves copying the RF shape from the signal layer to the mask layer. By doing so, you create an open mask on top of the RF signal layer. This step is crucial as it helps to maintain the characteristic impedance of the RF layout. Ignoring this step may change the characteristic impedance of the RF layout, impacting the performance of the circuit. It is important to apply mask shapes to RF signals to meet the microstrip or coplanar waveguide requirements.

Conclusion

This blog post equips you with the knowledge and techniques to navigate the complexities of an RF PCB design. By following the solutions provided, you can ensure that your RF PCB designs achieve optimal power transfer and contribute to the overall reliability and efficiency of the PCB. Implementing via arrays and transforming RF traces into shapes enhances signal integrity and protects RF circuits against EMI. To learn more about the new features of every major release, enroll in the course, Allegro X Update Training course.

Contact Us

For any feedback or topics you want us to include in our blogs, write to us at pcbbloggers@cadence.com.

Subscribe to stay updated about our upcoming blogs.

About BoardSurfers

The BoardSurfers series provides solutions to the various tasks related to the creation and management of PCB design using the Allegro X platform products. The name and logo of this series are designed to resonate with the vision of making the design and manufacturing tasks enjoyable, just like surfing the waves. Regular, new blog posts by experts cover every aspect of the PCB design process, such as library management, schematic design, constraint management, stackup design, placement, routing, artwork, verification, and much more.