I'm using KiCAD version 5, and I have an issue with it. Previously, I've been using OrCAD up until the point to where I needed multiple layers for my board. So, I redesigned my components, but I'm having an issue with my SOT-23 footprint.

Previously, in OrCAD, there were no problems. I managed to design my part, and in the layout, the ground plane managed to fill in the gaps between the pads as shown in the image below. You can see my pad here, and my soldermask clearances are 0.1 mm for all sides. It passed the DFM checks with no issues.

enter image description here

However, when working in KiCAD, I can't seem to get my copper plane to go in between the gaps. The pads are the same size, but I can't view the soldermask, so my rough workaround is to change the net pad clearance to be 0.1 all around, so it fits with my old part from OrCAD. However, it still doesn't solve the issue of the planes going in between the pads. How can I resolve this issue without affecting the other components of my board (is it possible to do this on a part-by-part basis)? Also, is there a way to view the soldermask layer? I see the mask layer as an option, but it doesn't show on the component. Perhaps being able to see the soldermask on my components might be helpful for this issue.

enter image description here

  • \$\begingroup\$ I am not a KiCad user, but try adding the soldermask layer to the board stack up. And look for an engineering rule for minimum web size to get the plane to go between. And after making the changes you probably have update polygons. \$\endgroup\$
    – Tyler
    Commented Aug 13, 2018 at 17:55

1 Answer 1


KiCad (version 5) works on a maximum required clearance model. That means that it will select the smallest clearance possible from the combination of requirements. In your case, although your pad has small enough clearance, I suspect that your zone fill has a higher clearance set.

In the image below, you'll need to set two things: the clearance and the minimum width. Because you want the copper to flow between the pads, you'll need the width to be smaller than the space available between pads (when including their clearance.

Zone settings

You said that you don't want this to affect other things on the board. In that case, you can set the minimum clearance for other elements using the "Design Rules -> Net Class Editor" clearance setting. Then, as long as your other footprints are set to a clearance of "0" (and their pads are set to "0"), it will use the netclass value.

Viewing the Soldermask

To view the soldermask, you need to have the soldermask layer enabled (and probably selected). The check-mark enables it but because it is drawn behind the pads, they typically obscure the layer unless you also click on it to make it the front-most layer drawn.

Soldermask view

  • \$\begingroup\$ Thanks for your answer. I tried playing around with a dummy project to try and put your tips into action, and I was wondering if it would be better to change the default clearance (in the design rules editor) to be the smallest value rather than the clearance in the ground plane properties? Sometimes it feels that whatever change I try to make, it affects everything whether I have it at the copper zone or not. Also, I tried what you said about showing the soldermask layers, but it doesn't seem to work. I can't make it the front-most layer just by clicking on it as you shown. \$\endgroup\$ Commented Aug 13, 2018 at 19:09
  • 1
    \$\begingroup\$ That could be a matter of preference. You should consider the clearance values to be limits. As in answering the question "What is the smallest value I would allow for this element?" That way, you build up the system based on the inherent limitations. \$\endgroup\$
    – Seth
    Commented Aug 13, 2018 at 19:29
  • 1
    \$\begingroup\$ Also, you can only select the soldermask layer when you are in the footprint editor main window or pcbnew main window. Not in the "Pad Properties" window. If it is still not showing, then edit the footprint and ensure that the "F.Mask" technical layer is enabled for the pad. \$\endgroup\$
    – Seth
    Commented Aug 13, 2018 at 19:31

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.