One pin on Symbol needs to map to 3 holes in footprint

I am a footprint designer noob. I am using Kicad v5.1.9. I have made 20+ schematics and PCBs and had them manufactured. So not a complete noob!

On a number of my PCBs I have a edge connector which is 52 pads by 3, where each group of 3 pads are connected together.

Originally I modified a conn_01x40 symbol to make a conn_01x52 symbol. I then placed this 3 times in the schematic. I then had to manually route the connection from pin 1 to pin 1 to pin 1 and then to the circuit. I modified the 01x40 footprint and extended it. In layout I get 3 conn_01x40 footprints. Again in layout I get the 3 connector footprints and then I have to manually wire pin1 to pin1 to pin1. I also make the same connections both sides (this causes problems with wire rip up in the latest tool so I have to use legacy mode).

I decided, enough is enough this is too much work. In the schematic I will instance only one of my 52 way connectors. So I no longer have to make 104 connections to connect to the other 2 connectors.

I modified the 52 x 01 connector by copying pad1 twice and placing them side by side. So each “pin” on the symbol maps to 3 through plate holes. I now needed to connect each set of 3 pads together. I used “graphic lines” and connected the 3 pads on both front and back copper. When loaded into the layout tool, I had problems and finally realised that the front and back copper wires in the pad apparently had a “keep out” attribute". I had no idea how to remove it.

So I searched and found a YouTube video. It explained how to make unusual shapes by copying the pad and slightly moving it (SMT). So I removed the “graphic lines” front and back copper links. I copied one of the pads and changed it to SMD (to remove the hole) and resized and moved it to link the pads.

In layout although this looks OK in the 3D viewer, I can see that layout wants me to wire the52 sets of 3 pads together. I can see the rats nest white lines. All these connections fail in DRC. I really would like this footprint to be DRC clean in order to spot the other missing connections.

I need advice as to how to make the footprint tool see the collection of 3 through plates holes and the 4 linking SMD pads as one “super” pad.

I have attached a picture from Footprint Editor and the same footprint in PCB Layout Editor.

I would be grateful; for any advice or pointers.

The SMD pad covers the center or each THT pad.


Thank you!

Although I didn’t at first understand your brief response, I went ahead and tried what I think you were suggesting. For pin 52 I deleted the small SMD pads which I added to short each pair of pads and added a new one which was large enough to cover all the centres of the three holes. I reloaded the footprint in the layout editor, and pin 52 didn’t have the whitelines.

Just for the interest of anyone reading who is wondering how long it takes to do this for all 52 pads. Once one pad had been confirmed to work as wanted, I edited the footprint text file directly using Vim, and deleted all the unwanted SMD pads, then copied the new SMD pad text definition and pasted it 51 times. I then I used some block copy of Y locations (from the through hole pad definitions) then pasted this into the Y part of the newly created SMD section. All 52 SMD pads were numbered 52, so more edits changed them from 1 to 52. I mention this just to make anyone aware that having textual definitions of footprints makes it sometimes quicker to use an editor than the GUI.

So this solution worked as I requested in that the funny shaped 3 hole pad is now a “super” pad. All DRCs are now passing.


If you turn off the mask of the SMT pad then you will have solder mask between all your pins so you won’t have to use as much solder here. Just an idea for you to use or ignore depending on the demands of your design.

1 Like

I have answered so many questions here over years that I tend to write quick, minimal posts which may not be very informative. Sorry for that.

What you tried first was reasonable. The reason it didn’t work is, as far as I can see, that KiCad’s connection finding algorithm isn’t perfect: it needs pads to overlap so that one pad’s center is within another pad’s outlines. (“Perfect” may actually be very difficult: it would need knowledge of the minimum allowed width of the copper connection which depends on the manufacturer requirements, not just on footprint requirements.)


Once when short of time I did a response and someone later replied your one line was better than my 3 paragraphs. Think of it as noise cancellation. :smiley:

Dear @eelik , certainly you have no need to apologise. You replied quickly and gave me enough of a clue to fix the problem I was facing and move forward. I hope to be getting a few new PCBs made by JLCPCB using the new footprint very very soon! I just need to finish them off.

Many thanks once again from me, and even more thanks for helping other people too. Thanks also to all other people generous with their time to help others with Kicad problems and knowledge. It’s thanks to people like you that Kicad is becoming so popular.

From your first post I recon you’re unfamiliar with the repeat function in Eeschema.

Pressing and holding (so it repeats) the [Ins] key can repeat the last added item. This is handy for making a bunch of bus entries, or adding a lot of labels to a bus (it has an auto increment function built in too).

But in your case, the solution of adding it in the PCB footprint is a better solution.

Hi @paulvdh, you’re right!

I used to place 3 “single in line 52 pin connectors” in the schematic, then connected them from top to bottom up using the repeat key. I could even add the wire connector dots in the same way. So the schematic wasn’t too much effort, but just placing a single (custom) 52 single in line pin header symbol is quick and makes the schematic a little less cluttered.

I use this key (“INS”) all the time, but I was surprised to find that one of my friends was never aware of this super time saving feature. It makes me wonder how many other features I am blissfully unware of!

I have used the new footprint quite a few times now and this is definitely a time saver. If there was the equivalent of the repeat for laying a track, this could have worked previously, but you would have to define direction, step distance, etc.

[off-topic] I was wiring a PCB last night with several identical memory chips, so all pins of the same number (except chip select) were all wired together. I would have loved a feature where I wire up all pin 1’s and then the repeat feature connects all pin 2’s then 3’s etc. :slight_smile: Perhaps if version 6 has a built in auto-router this might do close to what I want? :man_shrugging:

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