Duplicate PCB for test jig

Layout
1

I need to design a test jig PCB that matches a PCB that will be tested. There are some mounting holes and PoGo Pin pads that I would like to copy to the test jig PCB.

The positions are all dimensioned, however, it would be really nice if there was some way to use the PCB to be tested as the starting layout, with all tracks etc removed, just the PoGo pads and mounting holes left.

Is it possible to do this with PCBNew? The new PCB would also need to be associated with the test jig schematic.

Thanks.

1 Like
2

Not 100% clear to me. Do you have just the physical PCB or do you have the design files for it also? If Kicad then you can do a global deletion of the tracks.

3

I have the design files.

So you suggest making a copy of the schematic and PCB files and just deleting what is not needed?

4

I have been meaning to write a plugin to do exactly this since hearing Orson’s talk at KiCon. Glad to hear I’m not the only one who would find it useful. Sorry, I realize this is completely useless to you right now.

Until then, I would copy the schematic and board like you suggested and remove everything except your test points and any alignment features. I would also flip the test points onto the opposite side of the test PCB so that you don’t have to think about mirroring. The test points on the top side of your primary PCB will then mate with the pogo pins on the bottom side of your test PCB (and vice versa, if applicable).

5

Well, it is relatively easy to rip up the tracks. I have a feeling I’m probably missing your purpose though.

image
image499Ă—524 56.9 KB

6

I would first doe as hermit suggests:

Pcbnew / Edit / Global deletions.
and then remove the Zones, & tracks. (Maybe more)

Then make a gerber file of this board, open it in Gerbview and then, back export the gerber file to a .kicad_pcb file again.

Gerbview / File / Export to Pcbnew.

During this back import you can specify a layer to export it to, but the most important thing for you is that all the pads are turned into graphical objects, and you can put these on one of the user layers.
Then they are available for reference, but can easily be hidden by disabling the layer they are on. You can snap to graphical objects if you turn on:

Pcbnew / Preferences / Preferences / Pcbnew / Magnetic Points / Snap to Graphical [Yes].

Another important step to know is that if you open Pcbnew directly from your OS (not from KiCad’s project manager), then some extra menu items are enabled. This can be used to import one PCB into the file of another PCB, for example to make a mixed panel with multiple PCB. In your case I suggest:
1). Make a new project for your test jig (pogo pins + connectors, test circuitry, etc).
2). Extract the info you want from the original PCB as I explained above.
3). Open PCBnew in stand alone mode, and open the test-jig project PCB.
4). Pcbnew / File / Append Board. And then add the extracted info from 2).
5). Save the board, and exit Pcbnew.
6). Open Pcbnew from within your test jig project and work from there.

The purpose to me is clear from the title:
“Duplicate PCB for test jig”.

The Idea (usually) is to make 2 PCB’s with THT holes big enough to accept Pogo Pins. These 2 boards are then placed 1 to 2 cm apart with those brass bushes in the mounting holes instead of screws and the pogo pins soldered in them to make a test jig. This keeps all the pogo pins vertically aligned to the boards.
On top of the brass bushes, bullet shaped centering pins are screwed, that wil center the PCB to be tested exactly on top of the Pogo Pins.

Depending on the time needed to test the boards, they are held down by hand, or some kind of clamping arrangement is added. “toggle clamps” are common.

For this to work properly, the locations of the Pogo pins must of course align with the locations of the test pads on the PCB, and the test jig is easier to make if the locations for the mounting holes and the pogo pins can simply be copied from the original PCB.

What would such a plugin add to the work flow I described above?

7

The above works, but it’s tedious, especially for larger boards. I do this manually for most of the boards I design, and it’s easily an hour or two of work when you include checking everything, even though the steps are identical each time.

But what’s worse is keeping the test jig board in sync every time you have a new revision of the primary PCB.

The workflow I’m imagining:

  • Launch plugin
  • Widget lets you to select test points manually or via pattern matching
    – e.g. refs: “TP1, TP2, TP5, TP7”
    – or “TP*”
    – or by footprint: “TestPoint:TestPoint_Pad_D1.0mm, TestPoint:TestPoint_Pad_1.0x1.0mm”
    – or “TestPoint:TestPoint_Pad_*”
    – etc.
  • Option to define replacement footprints on test PCB, e.g. for through-hole pogo pins on the test board that mate with test pads on the main board
  • Similar selection for mechanical features
  • Press Go button
  • New Your_Design_Test_Jig schematic and PCB design appear in your project
  • Edit schematic to add any connectors or test circuitry
  • Edit PCB to place connectors and route

Most importantly, I want to have a pain free workflow for updating the test board after I’ve added/removed/moved half the test points. That’s why the pattern matching is important – I want to be able to pick up new test points automatically.

I don’t mind changing the connector or rerouting the test board when necessary, but I don’t want to have to think about which test points moved, checking alignment, etc.

8

The plugin sounds like a good solution to me, I need to get this jig completed so I am going to try the manual steps described by @paulvdh.

1 Like
10

Even without any plugin ohaz’s way is still valid.

After designing a PCB, you can change the footprint links in the schematic, from “Testpoint” to “PogoPin” and re-import them in Pcbnew.

This of course does not change the schematic. For your test jig you want to use a very different schematic then for the PCB of your product.

But copying a directory with a project to another and renaming the files is not a valid nor straightforward proecess, because the project files have internal links to the other files.

11

This topic was automatically closed 90 days after the last reply. New replies are no longer allowed.