How to create clearance for custom footprint?

[Erol_Bayraktarov]

Hello all,
I have this issue. I have created a custom footprint for a heater board. The footprint is imported from Fusion360 in .dxf format and set on the F.Cu layer. My layout depends on me having trace clearance for this custom footprint. As shown in the screenshot bellow i don’t have trace clearance on this footprint/track. Adding keepout zones on the whole footprint is not an option since it won’t let me do the routing shown in the screenshot. How do I add it? Is there a better way to achieve what i want?
Thank you for your time and efforts.
Cheers

[iabarry]

Stagger the Vias like the pins in a Canon D connector. I will attempt an example:

A. A. A. A
…B…B…

The text editor here may not like that. This method gives more room for the Vias.

[Erol_Bayraktarov]

Yes I already thought of that but still it will be good to know if there is a way to add clearances to custom footprints such as this. I can also just do it by measuring the distance from the trace to the vias but that is a lot of manual work that I prefer not to do.

[paulvdh]

KiCad makes a clear distinction between copper tracks and graphics on a copper layer.

For clearances to be recognized properly, you need it to be copper tracks instead of graphics.

I’ve experimented with this for some 10 minutes and what I thought should work does appear to work as expected.

Do this:

1. Go to the Footprint Editor, create a new footprint in a (writable) library.
2. Place a pad in your new footprint.
3. Select the pad to highlight it, then press [Ctrl + e] to enter “pad edit mode”.
4. Footprint Editor / File / Import / Graphics
5. Place the graphics.
6. End Pad Edit Mode by pressing [Ctrl + e] again.
7. Save the footprint, assign it to a schematic symbol, put it on a PCB and verify it works.

Your graphics have now become a part of a pad, and as thus inherit pad properties such as clearance.

Do not try to make your first attempt “perfect”.
Instead, it’s better to first get familiar with this workflow and concentrate on that.
Once you have the workflow right and know how it works, it’s easy to make a real footprint.

There are some gotcha’s here.
Because your graphics are part of the pad, by default they have a cutout in the solder mask, as an SMT pad it will have solder paste, and maybe other stuff. You have to set the layers for the pad.

You want two pads in your footprint, one on each end, because those pads become the attachment points for the wires, and those pads will create a short on your PCB which KiCad will probably complain about. For this, look into how Footprits for “Net-Ties” are defined. (It’s not neat and a bit of a hack, but it works until there is a better solution).