BoardSurfers: Using Test Points in Allegro PCB Editor

Test points are placed on a PCB during the design process to ensure (some might say ‘test’) that the design performs as intended and provides the desired output. Test points also help ensure that the integrity of the component assembly process is not compromised.

A test point is a small area of exposed copper that is contacted by a probe. Test points provide the capability to program, test, calibrate, and set up the PCB Assembly during manufacturing. Allegro® PCB Editor supports simulating test points, which facilitates digital testing of your designs.

After routing the board, you can use the testpoint command to add test points to your design. Only certain elements in a design can be defined as test points, including vias, through pins, and cline segments. The elements that are not eligible for use with the command generate a warning and are ignored.

You can assign test points to the front, back, or both sides of the design. Multiple vias or a particular via can be defined as a test point. Additionally, a grid of vias can be used as test points as well, where you can specify a minimum spacing between the vias. If you do not specify a testpoint, Allegro PCB Editor chooses certain vias to be used as test points based on user-defined or default parameters when the command is run.

Placing Test Points Automatically

You can configure Allegro PCB Editor to place test points automatically in a design.

Use one of the following ways to facilitate automatic placement of testpoints:

• Testprep Automatic Dialog Box
• Command Line

Using the Testprep Automatic Dialog Box

Perform the following steps to generate test points automatically in a design:

1. Choose the Manufacture – Testprep – Automatic menu command.
   Alternatively, you can run the corresponding command from the Command prompt, testprep automatic.
   
   
   
   The Testprep Automatic dialog box opens.
   
   
   
   
2. You can set the test point criteria as required and indicate the Execute mode. The minimum and maximum Via displacement values control the distance when adding new vias to be used as a test point. There are additional parameters that you can define from the Testprep Parameters dialog box.
   
   
   
   
3. Click OK to generate test points.

Using the Command Line

You can also run the command directly from the command line by defining the constraints in the Allegro Command window. Use the following syntax:

testprep automatic (‘parameter name’ ‘value’)

For example, to create test points for all the nets by using the via, TSTVIA on the BOTTOM layer of a design with a minimum center-to-center spacing of 50 mils, run the following command:

testprep automatic (side back) (center_center 50) (use_via TSTVIA)

Note: Use the testprep automatic command only after routing is completed so that the vias do not contribute to routing channel congestion during the rip-up and reroute operations. Use the clean command after the testprep automatic command to minimize T-junctions and remove excess vias.

After this command is run, test points are generated in the design that you can use to track performance and efficiency during test simulations. 

Creating Test Points Manually

You can also add test points to your design manually. Follow these steps to add a test point to a design:

1. Choose the Manufacture – Testprep – Manual menu command.
   Alternatively, you can run the corresponding command from the Command prompt, testprep manual.
   
   
   
   
2. Open the Options panel to view command options.
   
   
   
3. In the Options panel, select the Mode you want to run the command in; Add, Add (Scan and highlight), Delete, Swap, or Query.
4. When you set the Mode to Add (Scan and highlight), Allegro PCB Editor checks the design for failed nets that do not have a test point associated with them and highlights those nets and their connections.
   
   
   
   
5. Click the pin, via, or cline segment where you want to place a test point.
   
   
   
   
6. To continue adding test points manually, choose Next from the shortcut menu. To exit the command, choose Done.
   
   
   
   
7. Similar to the Testprep Automatic command you can define Preferences, Text, Methodology, and Restrictions parameters in the Testprep Parameters dialog box. All the parameters applied to automatic test points are applicable to manually generated test points as well. 

Conclusion

Test points are instrumental in validating design and routing integrity and help ensure that your design efforts produce the desired results. Test points in Allegro PCB Editor help you test the functionality of your designs digitally, ensuring that the PCB Assembly can be physically tested after manufacturing and optimizing the design process.

Contact Us

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

Do SUBSCRIBE to stay updated about 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 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.