Request layout idea to create a cut out board

[bertrand_meneroud]

Hi,

On some board I use a 3 PCB sandwich.
On top the actual board, with some THT components (the connectors mostly).
Then on the bottom an empty PCB with the mounting hole, that allow to isolate unde the PCB and protect it.
In between I have to put a cut out board to allow the space for the pin of the THT components that sticks out.

I’m looking for a way to create the layout for the cut out board.
Currently, I copy my main PCB. I delete everything except the THT componenent.
Then I’ve created a set of footprint wich are just a cut out (so a rectangle in the edge cut layer) for each of my THT components.
I then do a search and replace to assign the new footprint.

This work. but it’s a pain to do.
So I’m lookig ofr any idea or tips to make that easier.
I’m thinking that I my write a plugin to automate that, but I havn’t taken this step yet, as I’m not proficient in python programming at all.

[retiredfeline]

One problem I see is that the pins and solder blobs may be taller than 1.6 mm, the thickness of the middle board.

Why not just forget about the middle board. Use mounting holes and nylon pillars to separate the top and bottom boards.

[bertrand_meneroud]

Hi,
I do it like that on some other case.

But on these board, I do need to isolate the pin. and my connectors pins are less than 1.6mm
It’s really to isolate the pins, mostly again dust.

[eelik]

Add the cutout graphics to the original top board footprints to some unused user layer. Plot the layer to gerber. Open it in the gerber viewer when the middle board is the active project and export the layer to the edge.cuts layer of the PCB.

If you add a copy of the outer edge of the top board to that same user layer in the top board, or plot edge.cuts together with the user layer to the gerber, you will have a complete board ready when the gerber has been exported.

[paulvdh]

You can also use FreeCAD with the KiCad StepUp workbench to exchange data between KiCad and FreeCAD. And this works both ways. You can import a PCB made with KiCad into FreeCAD, or you can make STEP files with FreeCAD (or another 3D drawing program) and attach them to a part / footprint placeholder in KiCad.

[bertrand_meneroud]

Thanks eelik, I’ll try something around that.

[Piotr]

@bertrand_meneroud

Then I’ve created a set of footprint wich are just a cut out (so a rectangle in the edge cut layer) for each of my THT components.

At beginning I understood you need a hole for each pin. Now it looks that you need one hole for IC.
Strictly rectangle hole is not easy to be made.

@bertrand_meneroud

It’s really to isolate the pins, mostly again dust.

So you have holes for pins or ICs?

[bertrand_meneroud]

I have my top PCB, with the components.
The connectors pins goes trough the PCB.
Then in the middle PCB I have a square (more or less) hole for each connector. So that the middle PCB can be flush to the top one. and the connectors pins goes trough the hole.
Finally I have a Third PCB, that has no hole and cover evrything.

from the side it looks like that :

and the middle board looks like :

But the middle board is a real pain to produce.

[eelik]

Certainly a pain if you do it one by one.

A small change to my proposed workflow: you don’t have to copy the board edge.cuts to another layer if you plot so that you plot the edge.cuts and use “plot on all layers” selection for the user layer of the footprints. If each footprint has the slot in the user layer, the result should be what we see in your latter screenshot.

[paulvdh]

Ah, an example. Now we have an idea what you want to make.

An Idea:

1. Make a project specific footprint library. Put your footprints in it.
2. Make sure the footprint links in the schematic use the links to this new library.
3. Modify a footprint to have some lines on a graphical layer. (For example copy Courtyard to User.1).
4. Sharp inner corners can not be milled. Modify them, add dogbones, etc.
5. PCB Editor / Tools / Update Footprints from Library.
6. All instances of your modified footprint now have the lines on User.1.
7. Repeat for the other footprints.
8. Add other lines that are not in the footprints for some reason.
9. Copy the graphics from Edge.Cuts also to User.1. (and make modificiations if you wish.)
10. Create output artwork: Export as DXF, Gerber, use FreeCAD/StepUp, etc.

The main advantages of making those lines parts of footprints is that you avoid alignment issues. The lines get duplicated for each footprint instance, and they also move with the footprint if the footprint gets moved. (And you can also re-use those footprint in other projects, etc).

Also, if you want your middle spacer board to have an 1.6mm thickness, you can have it manufactured as a normal / regular PCB (but without copper). To do this you can for example:

1. Copy the project (Use “Save As” from the project manager).
2. Delete everything from the Edge.Cuts layer.
3. Copy contents from User.1 to Edge.Cuts.
4. Create PCB artwork output.

Also: How tightly does that intermediate layer have to fit? If it is sandwiched between other layers, then just a few plastic strips around the perimeter and some small pieces in the center may be enough.

[bertrand_meneroud]

Yes that should work. I would need a script to get the proper gerber name at the end but that quite easy.
I didn’t do it one by one, I did use the change footprint to replace each similar footprint by it’s cut ou version. but it still far too slow, and prone to error.

[ekoeck]

Quick and dirty:
a) export the Edge.Cuts together with the F.Courtyard as .SVG
b) open the SVG in Inkscape and delete all shapes you do not want to cut out
c) import the SVG to a new project as Edge.Cuts layer
d) done.

The cutouts then will be probably a bit bigger than needed but it still might be acceptable if you don’t want to spend too much time meddling.

[bertrand_meneroud]

Yes that should do the trick.
Actually, I should have a bottom courtyard on my footprint that should do nicely.

[BlackCoffee]

With Kicad’s increasing ability and elimination of Bug’s, you can do it all in Kicad…

Video shows a ‘Summarized’ how-to-do-it (which may include other user posted steps/ideas) - I stopped it at the end of Footprint creation (though OP knows how to create Footprints, I left enough for Noob’s…). I did not fuss with exactness… This should give OP/users some ideas…

I see the video quality is poor - sorry, the good quality video was too large for posting…

After setting ‘Z’ in the Footprint (to be lower than the Top PCB…