Whether it is a test in school, a driver’s test, or some sort of casual mention of a test at work, the word “test” can cause normally calm people to have a sense of anxiety. On the other hand, once beyond the test you can see those same people visibly relax. Perhaps that is why when PCB designers finish assigning testpoints to their design it is easy for them to breathe a huge sigh of relief. But, once you’ve assigned those testpoints there’s still more to do.
Assigning testpoints on your PCB design is the first half of the process. Once assigned, you will need to validate the testpoint assignments and then report the testpoint information. Fortunately, Altium Designer has advanced DRC capabilities to check your testpoints and utilities for outputting testpoint information into files that are easy to use. Here’s how to proceed with those next steps once your testpoints are assigned.
A Quick Review of Setting Up and Assigning Testpoints
Just as a reminder, we are talking about testpoints on a printed circuit board that are used for automated testing during manufacturing. We are not talking about those test locations on the PCB that are provided for technicians to perform bench tests with. Automated testpoint locations are used for either bare-board (fabrication) testing, or in-circuit test (ICT) which is performed after the board is assembled.
Altium Designer gives you the ability to assign vias and pads as testpoints. This can be done manually by changing the attributes of the specific via or pad, or automatically using the testpoint manager. The testpoint manager has settings for testpoint constraints such as which nets to test, specific sized vias or pads to consider as testpoint candidates, testpoint grids, and other options.
In order for the testpoint manager to work, you must have testpoints design rules organized. These rules also apply for validating the testpoint assignments, which we will examine next. For more information on setting up and assigning testpoints, take a look at How to Use Test Points on a PCB Design in Altium Designer.
Validating Assigned Testpoints
Now that you’ve assigned your testpoints, you will want to make sure to validate them. Altium Designer will check your testpoint assignments according to the testpoint style and usage rules that you’ve set up in your design rules. Checking your testpoints is another DRC that you should run before sending your board out for manufacturing.
If you’ve made any edits to the board after assigning the testpoints it is possible that you might have affected the testpoints in one way or another and it is always a good design practice to check everything first before sending the design out.
We are going to continue with the same example design that we used in the first article on assigning testpoints.
The first thing to do is introduce an error condition to demonstrate the validation process. Originally, we had turned off the use of a testpoint grid because all of the testpoint candidates were thru-hole pads that were off-grid. In order to find an error, we are going to turn the testpoint grid back on as shown below. The testpoint design rules are found in the Design > Rules pulldown menu.
Restoring the testpoint grid in the Altium Designer rules and constraints menu
Next, enable the testpoint rules for checking by going to the Tools > Design Rules Check > Testpoint pulldown menu. In the picture below, you can see that we’ve only enabled the Batch rules “Assembly Testpoint Style,” and the “Assembly Testpoint Usage” rules. This is because in the example design we only assigned the assembly testpoints and if we were to enable the fabrication testpoint rules for checking there would be nothing to check and report on.
Additionally, we went through and disabled every other rule in the design so that we would only check the testpoint rules.
Setting up the Assembly testpoints for design rule checking
Once you have enabled the desired testpoint design rules for checking as shown in the image above, click on the “Run Design Rule Check…” button in the lower left corner of the menu. Altium Designer will run the checks on your design and open a report window for you. In the image below you can see that Altium Designer has found problems with all of the testpoints in the design, and is reporting that they are off-grid just as we intended.
Altium Designer’s testpoint design rule checking results
One of the really handy features in Altium Designer is the ability to navigate to a specific DRC error. In the image below, we have clicked on the top error in the report window. You can see how Altium Designer has zoomed into the specific testpoint that is in error. In this way, you can find and correct any testpoint errors that are reported.
Using the testpoint DRC results to navigate to the error in the design
How to Find Testpoints and Report Them
Once you’ve confirmed that all of your testpoints are correct, you can now output the testpoint data. Altium Designer gives you the ability to either output the files individually using a menu command, or you can include a set of commands in an “Output Job Configuration” file to batch process those reports along with the rest of your manufacturing outputs.
To output the testpoint files individually, go to the File pulldown menu and select either “Fabrication Outputs” or the “Assembly Outputs” and then select “Test Point Report.” Remember that Altium Designer gives you the ability to assign testpoints for bare-board testing (fabrication) or ICT (assembly), and depending on which testpoints you have assigned (or both) will determine which outputs you create.
As you can see below, both menus contain the same options making them easy to use.
Altium Designer’s Fabrication and Assembly Testpoint Setup menus
In our case we’ve only assigned ICT (assembly) testpoints to our design, so we will use the File > Assembly Outputs > Test Point Report. The assembly testpoint menu is on the right side in the image above, and you can see how we’ve changed the “Report Formats” to enable the “Text” version only. Altium Designer will also output reports as a CSV file or as an IPC-D-356A file.
The IPC formatted file also comes complete with the ability to include options like board outlines and trace information as you can see at the bottom of the menu. The Test Point Report menus also give you options for testpoint layers, units, and coordinate positions.
Once you’ve set up the options that you desire, click the OK button at the bottom of the menu. The output file, or files, will be written at the location specified in the Project > Project Options pulldown menu. The assembly testpoint file that we generated in text format is shown in the image below.
Assembly testpoint report sample
Once you’ve assigned the testpoints on your design, they won’t serve any purpose until you can generate reports on them for your manufacturer. Fortunately, Altium Designer provides you with some of the best design utilities for validating and reporting testpoint information available in PCB design software today.
Would you like to find out more about how Altium can help you when it comes time to create, validate, and report the testpoints on your design? Talk to an expert at Altium.
About the AuthorVisit Website More Content by Altium Designer