Is it possible to have pads of a different size on top and bottom layer?

[pigeon]

Hello, just wondering if I can change the pad sizes on just one layer (in my case its to have smaller pads on one side for extra routing space.

[jmk]

Yes, you may have any size or shape pads on either layer.

Towards the bottom of the “select” menu (right mouse button click), there are various ways to edit pads in bulk on either side (or both) of the PCB.

[pigeon]

Thank you, I see there is the 3 options to change the pads, cut can seem to work out how to have the pads larger on the underside of the PCB?

[bertrand_meneroud]

You need to create a small pad through hole.
Then you can add a SMD pad to it bigger for each layer.

You must put the same pad number to each pad which are on the same pin.

[Heath_Raftery]

FWIW I recently went deep into this territory. I had some pretty tortuous requirements (recreating some complex pad stacks from an OrCAD project), and found KiCad quite capable. Here’s what I discovered:

• Every hole needs a THT pad. So if you have a complex pad with multiple holes, you’ll need to place at least two THT pads on top of each other and position one hole in each.
  • For example, here I position the pads at the same location and offset the hole in each.

• THT pads define the pad size for all layers. There are options to remove the pad on a layer if there’s nothing connected to it, but that’s determined at PCB layout time so not something you can control at the footprint level.
• SMD pads define the pad size for a single, outer layer.
• The resulting pad size is the superset of all the pad sizes that overlap.
• Because of these three points, to have different pad sizes on different layers, you will need at least one SMD pad.
• Subtly, also because of these three points, the inner layers must be the smaller of the two outer layer pads. That’s because it’s the THT pad that dictates the inner layer sizes, and to override one of the THT pad’s outer layers, a bigger SMD pad must be added.

The take-away from all that is that to have different size pads on top and bottom:

• Place the smaller pad. If it needs a hole, make it a THT pad.
• Place the larger pad on side that needs it. It must be a SMD pad.
• If you have inner layers, they will be the THT pad size, if you have a THT pad.

For example, here’s a THT pad with a larger SMD pad on the bottom:

The inner layers get the smaller THT pad size, no choice.

And lastly, for an advanced example, here’s a double THT pad with a smaller pad on top and a larger on bottom. One pad has the hole offset in the positive y direction, one in the negative.

But, you remark astutely, didn’t you say the larger THT pad will override the smaller THT pad on all layers? Ah, but I cheated! In this case I edited the .kicad_mod file by hand and changed the bottom pads from (layers "*.Cu" "*.Mask") to (layers "B.Cu" "B.Mask"), so this particular THT pad only exists on the bottom layer.

[Heath_Raftery]

BTW, this is what I love about KiCad. It makes the easy things easy and the hard things possible.

Naturally a SMD pad lives on the surface. Naturally a through hole intersects all layers. Naturally copper on copper is just more copper. Out of the box KiCad really gives you tools to make real things. If you want to get fancy, you gotta get fancy.