Can I get copper on just one side of a pad?

I am a new user to Kicad … using version 7

Produced my first board … had it made JLC … came out great!

So, now I am doing some refinement before making 10 of these boxes for the customer.

Question … I have one spot where a part goes through a hole and is connected to traces on the back of the board (two sided board).

Although it is a through hole, I am only soldering on the back and don’t want the pad to be on the front side of the board (long story but this part is optional and I don’t want the chance of anything touching the pad if the part is not inserted into it).

Is there a way of putting a through hole but only having copper on one side?

I thought I found it under pad properties (copper layers: connected layers only) but then I do the 3D view, it still shows a pad on both sides of the board.

I also found in the next tab (connect to copper zones: from parent footprint) … but that didn’t seem to change anything.

Is there a way of having copper on just the back side of the hole? Is it one of the setting I found or ???


You can use a SMD pad on the reverse side and a NPTH hole through it. This is mechanically weak and prone to dry joints and pad lifting compared to a normal THT pad

Suggest making the component footprint with a (nearly) zero size thru hole pad - that is Pad size = hole. you will get your PTH for strength this way ,
Then, place a second single sided pad over the zero size pad on the side you need the full pad on.

In the future, Kicad will get complex pad stacks like $ software- which enables top , middle and bottom to have their own characteristics.

Thanks for the heads up on the mechanical strength. It is for a battery holder so strength is not that important. There are four 4-40 screws holding it. It is just for the two power wires. Thanks!

Awesome idea!

The holes are for a battery holder. I am going to switch them over to a clip and holder so they can take the battery out easier. Right now they need to reach into a crowded box and almost pry it out.

I just want to make sure I give them the option of the old style holder just in case an engineer at the factory these are going to complains … or if the guys are rough on the wires and end up pulling the wires out when they change the batteries.

I like the idea of a “zero” pad. The battery should never touch these two terminals but just in case some bare metal on the batter ever touched the terminals (again probably a one in a million chance), I don’t want an issue.

Thanks so much for the advice !!!

This will make the annular ring thin / non existent, but the hole will still be in the drill file for the plated holes. Aditionally, KiCad is likely to complain about too thin annular rings. If you want a hole without plating, you have to use a “NPTH / Mechanical” pad. KiCad does not like using NPTH/Mechanical pads as part of a net. It is a bit of a strange limitation to me. Sure, it’s unusual on a dual sided PCB, but a gazillion single sided PCB’s are made without plated holes.

I have not verified it, but I’m quite certain this works:

  1. Use a NPTH / Mechanical pad to get your hole (You can disable copper layers too).
  2. Use an SMT pad for the net connection.

Both pads must have the same pad number. This is a common technique in KiCad to build up more complex pads (By lack of a fully implemented pad stack). The next problem you have to work around is that KiCad does not like it if the attachment point of an SMT pad is inside a hole. You can work around that by using an offset. KiCad does not accept an offset for a round hole. An oval hole with it’s X-size the same as it’s Y-size is also round though :slight_smile: (Rectangle, rounded rectangle, etc also work).

From another thread with the opposite problem:

Edit the pad properties and uncheck the F.Mask layer.

There will be copper on both sides of the hole, but the top pad will be covered with solder avoiding contac without losing strength.
I have never done it, anyway I would give it a try.

1 Like


Normal solder mask is not reliable as an insulating layer. If you want to attempt it anyway, then at least also draw something on the silkscreen layer, which gives 2 layers of paint. To do this reliably, you would need a reinforced mask layer or an extra insulating layer such as tape or paper designed for this purpose. (“Elephant hide” is a brand name of such paper).

Exactly my thinking! I just removed all traces that ran under parts like heat sinks. I was worried that the mask “might” not insulate. Sure it does most of the time but I don’t want it to fail on a customer.

I am one of these guys who try to make everything I build “bullet proof”.


Check with your PCB fab house to learn their requirements for Thickness.

That said, you can set Mask Thickness in the Board Stackup …

1 Like

Thanks for all the info! I will try this today. This is just one of those unusual times there there is a pad and the 9V battery is mounted very near. I normally would not put a hole in a board for no reason but I am worried someone will change there mind later and want the old style battery holder. I don’t want to re-make the board if they do.

Like I said, it would take a lot of things to go wrong to get the battery just in the right place …and then touch both terminals at once … and then have the paint scratched off to it shorts the terminals … but I have had those type of things happen out there in the field!

Just FYI … I laughed when a plant electrician told me to put my plugs in “upside down” (ground terminal up) … than a few months later, I had a small metal plate fall from a shelf … just happen to hit the two terminals on my plug that were just a bit out (not quite in all the way) … and arced for about 10 seconds before the breaker kicked.

One in a million … yest … but it did happen to me.

Thanks again !

Murphy’s First Law: Anything that can go wrong will go wrong .

I’m wondering how much of mask will be inside pad hole and may be at opposite PCB side ‘helping’ soldering to that pad.

And how much of paint.

1 Like

Corollary: Murphy’s law can fail.

I have overlooked OP’s sentence: in case the part is not mounted.

1 Like

never rely on mask for insulation… and once you throw vibration in there, the mask may quicly erode.

If Kicad complains about low or zerro annular ring, just make a rule specific to that pad or footprint to ignore the violation.


Do you know if PCB manufacturers will complain on low or zero annular ring?

It depends on the manufacturer. I rescued an old pcb from gerber files with v5. Not all copper pads were imported in pcbnew correctly so I reworked the copper and we did not noticed some pads were not present on the top layer. Fortunately the tracks were on the bottom layer.

Works well for me and I suggest you tweak the Color Settings for the Viewer and set the Alpha (opaque) to lower value

My colors are NOT set for ideal demo but good enough for you to see the Pads/Tacks that are Not visible if not connected…etc…

Perhaps useful screenshot of Wire connected to Back side

1 Like

“Do you know if PCB manufacturers will complain on low or zero annular ring?”

They will only complain about zero annular ring if there is a trace / track connecting to it.


A post was split to a new topic: Testing Forum Abilities

Awesome video !!!

I will do some playing tonight.

Just FYI … here is the prototype board I made. First board I made in 20 years. Took me a week to figure out Kicad. The customer is testing with it now (populated and in a panel). Like I said, just doing a bit of clean up. Little things like moving all the traces from under parts (like removing the one under the battery holder).

Thanks again so much for all the help!

1 Like