Currently I have created a footprint by using one large retangular pad + 2 through holes.

However the DRC picks this up as an error.

Is there a better or more correct way to do this? Or is the DRC in this case being overzealous?

Datasheet for the part: http://www.pemnet.com/fastening_products/pdf/smtradata.pdf

  • \$\begingroup\$ You are using three pads to simulate a single pad, but the DRC doesn't know this, so it is trying to warn you that you have pads hitting each other. It's not being overzealous, it's doing it's job. In this case you just have to ignore it. I don't use Kicad, but in my EDA software if I connect through hole pads to a surface mount pad with a ratline (putting on same net), then it will let me put the through holes on top of the smd pad and not give any errors. \$\endgroup\$
    – I. Wolfe
    Commented Jan 27, 2015 at 15:49

1 Answer 1


As noted in the first comment the DRC is doing precisley its job, and you should not ignore it. DRCs are somewhat magic and sometimes when they encounter an error they don't actually check for other errors, so to have an error free design... You need to have and error free design, and this does not include ignored errors.

The DRC is yelling at you because you have created three separate pads, assigned to each of them a separate number, then just stuck them one on top of the other. This violates the minimum clearance allowed between pads. What can you do about that?

  • Ignore the DRC error. That's probably the worst way to deal with it. Try to ignore your partner when there's some problem and see what happens.
  • Make some custom clearances for the specific footprint. That works, the DRC would stop complaining but you still have to connect three pins on the schematic, that's just awful.
  • In each pad setting (press 'e' when hovering on the pad) assign the three pads the same number, i.e. 1. Now that's a solution: the three pads correspond to one pin, and they actually correspond to one single physical pad

The third solution, actually, The Solution is what you want to use when drawing strange pads with strange shapes. Imagine a LDO SMD regulator with the tab connected to the central pin, the land pattern would look like a big square (thermal tab) connected to a rectangle going to the middle pin. You can do that with two overlapping smd pads that have the same pin number.

Disclaimer: when you are drawing the footprint for a large microcontroller that has many ground and vcc pins you might think you can assign all the corresponding pads the same number in order to have only one pin on the schematic. That is a bad idea\$^{\text{TM}}\$. When you draw the tracks on the board the DRC will assume that all that pads are somewhat physically connected together and won't force you to connect all of them. Of course they are physically connected but you should provide power (and a decoupling cap) to each of them.

So the rule is: you can give different pads the same pin number if and only if these pads overlap in some way OR you really, really, really know what you're doing.


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.