Using Eagle 7.6.

I have a part in a TO-5 can. The can needs to mount flush to the PCB, and I'm concerned that the copper on the top side of the standard thru-hole pads might contact the case. For various reasons can't put an insulator between the part & PCB - the part MUST be hard against the PCB.

I could make the pad's diameter really small, which would help the top side, but would provide no real estate for soldering on the bottom. So what I really want is a "single sided" pad - essentially a non-plated hole with a solder pad on the bottom side and bare board on the top.

Any suggestions as to how to best create this?

My thought was to make a zero-width (ie. filled) circle on the bottom (or pads) layer, put a slightly larger bStop filled circle on top of that, then place a 0.025" hole in the center of it all.

Any thoughts/suggestions/opinions would be appreciated, -Dave

  • \$\begingroup\$ I have never used Eagle. Usually on a TO-5 the pin has kind of a gap around it, filled with epoxy or something, where the pin goes into the can to prevent shorting between pin and can. Are you sure you need a "no-annular ring" through-hole? Anyway, you can use a very small annular ring, then place a through-hole testpad on the bottom side to kind of trick the CAD tool into making a larger annular ring on the bottom. \$\endgroup\$
    – user57037
    Jul 15, 2016 at 15:48

2 Answers 2


It's not directly possible to make a 1-sided pad in Eagle. There are a couple of ways, but both result in either DRC warnings or non-PTH holes (in one you basically do an SMD pad on the bottom, and put a non-PTH drill hole through it). So I won't go into these methods.

There is however a workable solution that I am using in one design I have that uses a TO-3 part (similar package), and that is basically to use a solder mask defined pad.

Solder mask Defined Pad

Here is the pad I am using. Basically it is a large PTH hole. I first set the annular ring to be large enough for what I need on the bottom of the board. The next step is to turn the predefined solder mask off - you do this by setting Stop to off in the properties for the hole.

With no stop mask defined, it means there will be no copper exposed - the entire pad is covered with solder mask. You are then free to draw your own solder mask definition on the tStop and bStop layers. On each of the two stop layers, draw a circle with a width of 0, and a radius to meet your requirements. Align the circles up on the centre of the hole.

In the picture above, you can see I have draw a circle on each layer. The tStop circle is only just larger than the drill hole itself to ensure that the hole doesn't get tented (blocked) with solder mask. Then on the bStop layer, the circle is large enough to expose the whole pad to allow soldering.

While this doesn't result in a single sided pad, it does mean that there won't be any shorts between the metal case and the top copper because the solder mask is in the way.

  • 1
    \$\begingroup\$ I like this - seems a LOT less hacky than other alternatives... thanks! \$\endgroup\$
    – dlchambers
    Jul 15, 2016 at 17:49
  • \$\begingroup\$ I also like this solution, but I have a question. In your example, why draw a circle on the top stop layer at all? Wouldn't omitting that circle answer the original question perfectly (creating a one-sided pad), or is there a reason to always expose a little bit of the ring on both sides? For instance, would having no top stop on the mask mean the solder mask goes through the hole and affect the other side of the board? (EDIT: I didn't understand your answer originally, and you explain that you need some stop otherwise the hole might get blocked by solder mask. Sorry.) \$\endgroup\$
    – Tristan
    Oct 23, 2017 at 1:32

I found a related question that might help you out. It seems to me that you can put down an SMT pad (round or square, whatever you want), and then drill a hole on top of it.

This related question's answer shows how to use the HOLE command in Eagle: Non Plated Through Holes in Eagle

I'm sure you'll get DRC warnings or outright errors and your board house might flag it and ask you about it. You can either ignore it, or you can define an SMT pad that has a clear center (a donut pad without a drill hole) and maybe get rid of the DRC errors. Hope that helps, -Vince


Your Answer

By clicking “Post Your Answer”, you agree to our terms of service and acknowledge you have read our privacy policy.

Not the answer you're looking for? Browse other questions tagged or ask your own question.