How to have a pad with three TH holes connected with a track

Layout Footprints
1

Hello,

I am trying to make a footprint in Kicad 6.0.
This footprint would have uncommon pads which would look like this:

image
image894×550 23.5 KB

What I did is I only gave a pin number to the one Through Hole I actually want to connect my tracks with and I have created tracks to connect them together.
Unfortunately, DRC is not really happy about this solution as the tracks are violating the clearance policy.
What would be the proper way to achieve the same result without infringing DRC checks?

I am also wondering if there is a quick way to subtract these tracks from the silkscreen on the footprint. I know I can do it when generating gerber files but in the meantime it generates warning on DRC (and I would prefer not disabling default checks).

Thanks in advance for your help.

2

In the footprint, you can give the 3 pads in each row on each side the same numbers like

1 - 1 - 1…2 - 2 - 2

And connect them with tracks (as you did). DRC will be happy then.

3

You should create this footprint by adding multiples of same numbered pads (3x th pads numbered as ‘2’ overlapped by one smd rectangle pad, numbered also as ‘2’ - your current track portion. This was an example for your pad number 2).

1 Like
4

If you additionally want to include the connecting copper-segments directly into your footprint you have to draw an arbitrary Pad shape → command: “Edit Pad as graphic shape”. If you draw a simple “copper”-line you run into DRC-errors (as you have discovered).
To draw an arbitrary Pad-shape in the footprint-editor:

  • draw a simple Pad as anchor for the arbitrary Pad-shape (for instance the first Pad1)
  • select this Pad, right-mouse-click → context menu → “Edit Pad as graphic shape” (or hotkey CTRL-E"
  • observe: yellow info-message at top of screen (shows “Pad edit mode active”)
  • now draw some copper-elements around your Pad (begin with filled rectangle or circle). The copper-elements must connect with the Pad.
  • If you are satisfied with your geometric art
  • If your geometric drawing is ready for an modern art exhibition: end the “Pad edit mode” with CTRL-E.
  • The original Pad and your additional copper-shapes should now be combined into one arbitrary Pad shape

I have attached an example Kicad-project with a footprint with arbitrary shapes. Play around with this.
footprint_example.zip (12.0 KB)

2 Likes
5

Thanks it worked perfectly!

6

Many thanks to the three of you. I no longer have these DRC errors.

7

Thanks to your example I figured out how to fix my second issue with the silkscreen interfering with the tracks. I have disabled the F.Mask and F.Paste now the tracks (pads) are no longer conflicting with the silkscreen layer.

3 Likes
8

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