Position components in KiCad for a test rig

Question

I'm designing a test rig for a product. There's a number of test pads and a power connector on the PCB, which I want to match up with a tester device, i.e. the tester PCB should have pogo pins and the mating power connector in matching places.

The question: given the PCB of the product, how do I export from KiCad, for example, a .dxf such that it has only a few of the components? I could simply export the whole PCB as .dxf and import that to the user.dwgs layer in the tester PCB, but this will have a lot of visual noise as all components are visible. Is there a way I could export only the few selected components (test pads and power connector), or perhaps some other easy way to guarantee that the tester PCB will match with the testee.

Answer 1

...or perhaps some other easy way to guarantee that the tester PCB will match with the testee

The way I'd do it is this: -

• Save the design under a new name (say "fixture")
• Lock the mating components needed on the "fixture"
• Delete all the components apart from those needed
• Use this as the basis for your fixture design
• Develop the fixture design but,
• Make sure the component copper/pads/holes that align with the original PCB are position-locked on the fixture design.

Answer 2

It's been a while, but I add another solution.

I'm using a combination of theses tools:

• KiCad
• FreeCAD

I'm not affiliated with these products, I'm just a user. BTW, they are open source.

1. I imported the artwork into FreeCAD. Here I joined the board and all components to one solid body. It's a boolean operation (union). The command is Part Fuse. Now, it's one object and not thousands, it's now better handled within the CAD tool.

2. I duplicated the layer with pads (Cu- or Paste-mask-layer and put it on the tester-pcb. There you can design the test stuff. Align the pads and drills with the pads of your testee.

There is also a FreeCAD plugin for KiCad (a so called workbench): KiCad StepUp.
Here you can import board files from KiCad an push a design back to KiCAD.

You can also go some steps further:
You could model the whole tester pcb with all pogo pins attached, add the pcb-under-test to your design and verify how good they mate. With collision detection turned on. I haven't tried it yet by myself. But I think this could by handy if you have pogo pins with different contact length.

FreeCAD can be found here: www.freecadweb.org

The procedure is not tight to the mentioned tools. The artwork (Gerber, dxf) could be imported to any 3D-CAD-Tool.

Answer 3

You can have a look at my fork of openfixture where I added a generate_kicad.py script which is called from GenFixture when the --kicad option is added.

It generates a schematic and PCB with the pogopins placed on the PCB, and as far as I remember with 3D models for the pogopins, which were generated 3dmodels/create-steps.sh. I do not guarantee the 3D models are correct, but it suffices to update the 3dmodels/pogopins.scad script to adjust the generation thereof an regenerate them.