Fancy Pads from DXF

you can get a fp from polyline pads:
TouchPad-fp.FCStd (17.0 KB)
TouchPad-fp.kicad_mod (4.5 KB)

1 Like


I don’t know anything about FreeCAD (yet)… so you convert in FreeCAD to a poly line?

have a look at

1 Like

…it seems to me, what you want is a Footprint

Verrry easy to do in Kicad

  1. Click the Footprint Editor Icon
  2. Create New Footrpint (two Icons at top left, use the First Icon)
  3. Draw your lines on the Silk layer with the Graphic Line tool (could do on other layers, too)
  4. When the lines are done, Edit each (double-click, or hover and ‘E’ for edit)
    Change the Width and select Desired Layer (most likely Top Layer)
  5. Add Pads (icon in tool strip) Could make them Square, Rect, Round, Oval, Custom)
  6. Draw Lines/Shape on Silk and other desired layers

Save it and Use it… (I did not dial-in specific details but, you get the idea.
Did Not use DXF, FreeCad or anything other than Kicad.


They shouldn’t be done like that because then they are not pads. Steps 1…5 are good, but the graphics and the pad which belong together should be combined to one custom pad. It happens by selecting them and using RMB menu -> Create Pad from Selected Shapes.

1 Like

I do it both ways - I make my PCB’s so, I often don’t bother going beyond the minimal I need. And, that should serve as a starting point for others… Generally, I only do the Pads from graphics if needed… it’s an excellent feature!

Unless you need to make a number of different configurations I’ve found its easier to calculate (excel, libracalc) the end points then just put them in by hand.

Not too long ago KiCad did not have the capability to DRC checks on graphics placed on a copper layer, and a hackish way of adding some graphics on a copper layer did work. For some time though (about a year?) KiCad generates DRC violations for track segments and pads that overlap with graphics on a copper layer.

You are of course free to do so in your own projects, but I do not like it if you teach sloppy methods to others.
Combining the graphic shapes with the pads as eelik mentioned is a very small extra step, and without that step KiCad won’t let you draw a track to the pad, because that would violate DRC.

To OP:
Drawing some graphics, then moving it to F.Cu and combining it with a pad such as described earlier does work. Your graphics are also very simple straight lines, so there is no use in being cleverer then needed, and drawing some lies in KiCad itself is just fine. No need for DXF, or even dragging in 3D.STEP files for this.

An alternative method is to just use a few SMT pads and then overlap them in the Footrpint editor to make a bigger and more complex pad.

If you put graphics on a copper layer, then it will be covered by solder mask, and this is … not recommended for switches :open_mouth:
If you combine multiple SMT pads, then the pads have cutouts in the solder mask, but also in the paste layer, which is also probably not what you want, so you have to disable the paste layer for those pads.

The photograph has a single big square cutout in the solder mask. The recommended way to do this in KiCad is with an “aperture pad”. An aperture pad is nothing special, it is just a regular pad, but with the copper layers disabled, and also with the pad number removed. Because it has no pad number, You can’t connect a track to it, and you can use use it for custom shapes on the solder mask and/or solder paste layers. Search KiCads footprint libraries for “Thermal” to get examples of this.

1 Like

Your graphics are also very simple straight lines
They are not; they have rounded ends.

The photograph has a single big square cutout in the solder mask. The recommended way to do this in KiCad is with an “aperture pad”.
That’s interesting. I was assuming that I would draw a square on the solder mask layer.

I’m going to try and do a crash course in FreeCAD. The ability to generate a pad shape from a DXF (or STEP) would be useful for me as I am familar with Fusion 360 for drawing.

All copper tracks have rounded ends in KiCad, so as far as KiCad is concerned they are just straight lines (copper tracks).

My attempt at FreeCAD stepup didn’t work out well.

I think I will have to approximate with lines for now

have a look at the FreeCAD file I have attached above

That’s better. Is there some magic going on there… naming convention Pads_Poly_… and the circle for the reference point?

there is not a full howto, but there are examples on StepUp Demo menu from where an user can get some tip…

I have also a cheat-sheet document, but it is not fully exhaustive

and the topic at the forum here

1 Like

Thanks all. I think I have learnt quite a few things.

I put a square of F.Mask over the pads to open up the area (I couldn’t see how to use Aperture)

I think I have something workable so will move on as I have a design to finish but I think I will return to Kicad StepUp when I have my next fancy requirement.

1 Like

I managed to get quite a long way with the use of KiCad StepUp. Thanks!

The only thing I could not establish is the relationship between the KiCad origins and FreeCad origins when taking sketches from different sources and then exporting them to layers back in the PCB… but close enough.

Thanks for the workbench plug-in!


In this thread: PCB shape from enclosure STEP file

I wrote:

Which is an index in into the video posted a little bit earlier in that thread.


Thanks for the pointer. Must have missed that.

My two cents (probably useful working scenario):

I create such footprints by adding many pads having the same pad number. At least I have done this for this transistor in real life:

Creating your footprint would take up to 10 minutes (only several CTRL + D operations, pad property changes (use “Push pad properties to other pads” in right mouse click menu, and some changes in pad geometries (done by simple dragging operations with mouse). I tend not to take a risk of miss-talk somewhere in long path with external tools: freecad-stepup-dxfexport-dxfimport.

I don’t remember if doing so caused any DRC mistakes. As for soldermask openings - yes, please use “SMD aperture” type pads, or just a simple graphical shapes on any layer desirable (solder mask or solder paste…). This is very useful when custom paste openings are needed on a soldering stencil (adding rectangles or “SMD aperture” type pads).

I accidentally got the idea of using duplicate pads in the footprint from one of stock footprints (I do not remember which one). See this screenshot from stock library (containing SMD aperture pads for stencil layer, I am sure there is on footprint with duplicate “real” copper pads arranged to make one big custom shaped pad):

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