Polygonal SMD pad for footprint/module


I’m currently creating a footprint and the layout requires a polygonal SMD pad. To be exact, I need a parallelogram, so it’s still just a rectangle, just shifted on one end.

I have no problem with editing the footprint in a text editor if it is required.

I’m using the stable 4.0.6 but can switch to a nightly if required.

I hope anyone can help me out, thank you.

Polygonal pads are currently not supported. You can build up your pad with overlapping pads that have the same pad number. (It might be necessary to play around a bit to also get the solder mask opening to look like you want it to look.)

An example of something similar as your requirement can be found in this pull request for the official lib.

1 Like

Create the parallelogram as a group of overlapping SMD pads, where ALL of the pads have the SAME pad number. There will be at least two pads; my guess is that you will need four.

For one (or two) of the pads, place a new pad then open the “Pad Properties” dialog. (Do this by hovering the cursor over the pad and pressing “E” on your keyboard.) Specify a rectangular (or possibly trapezoidal) pad shape. Enter the approximate dimensions for the size. In the “Orientation” drop-down, select “Custom” then enter the appropriate angle value. (Yeah, you may need to spend a few minutes doing some trig calculations.)


Or use a parametric mcad tool for this task. I use the sketcher from freecad. (part design workbench.)

Thank you for the quick response.

I hoped there would be some hacky way to input polygons. But seems like I have no luck and need to calcute some hours now (yay). Now I just put together 2 trapezoids. Does the job, just takes way longer.

Another question now that it have been mentioned. Is there some way to add an area where now solder mask should be applied? There are no polygons so I thought about just adding one thick line. But unfortunately they have rounded ends.

Place a smd pad without copper/paste and only soldermask.
Leave the pad number empty.

Worked quite well, thank you!

Just found a video which exploits a hack to draw footprints on Copper.
The Idea is to first draw some graphics on the silk screen in the Footprint Editor.
Then Right Mouse Button and change the line segment to a copper layer.
The “very dangerous” part is that KiCad can not do DRC error checking and such on these line segments, so you have to check manually.

The Footprints are also text files and you probably can change the layer name of some graphics right there with an editor. (Haven’t tried).

That’s really not something you should use for pads. (no control over paste and mask layer offset. Can not connect a trace to it.)

It is ok to use for stuff like touch buttons or logos. (But for that i would go the route of svg2mod instead of manually drawing it.)

Little update from me.

The mentioning of logos made me take a look at the logos I created and I saw they are made with fp_poly.
So I made it again using polygons and a width of 0.00001. Then I put a SMD pad on top of it

I also used a polygon to create the solder mask as it will not get affected by the mask offset which you get when using a pad.

I made a picture to demonstrate both ways I did. (Taken in pcbnew.)

I must say I’m quite happy with the polygon solution and prefer it over the stacked trapezoids.
As it’s only for a connector on the board edge, I will only connect traces to the inwards of the board, so that won’t pose a problem.
Also it looks much cleaner this way :slight_smile:

Again, thanks for all the help.

Two stacked rectangular pads should be near enough. One of them rotated a little. I suspect the ends don’t really have to be horizontal.
Don’t try to use the autorouting when you have odd pads