Copper Fill inside footprint


I have a microwave transition that I would like to realize as a footprint: Microstrip to GCPW. This all works great because I can set the polygon line width to 0 so the structure is exactly the same size as my dxf import from the EM Solver. The issue is now, that the ground pour does not seem to want to connect the SMD pads that I put on the footprint. You can see that it forms a clearance around the component (fill clearance is set to 0 and pad connection to “solid”. Am I doing something wrong here? Why does it not simply connect?

edit: for clarity, the clearance around the square-ish part should not exist. It should simply connect the polygon in the footprint with the fill zone in the layout. If this is not possible, what is the recommended way of doing this?


How are you designating the fill area as ground?

Use a polygon pad with zone connect set to solid. (zone connect can be set at the footprint or pad level. By default polygon pads use zone connect none as the thermal spokes option does not work for them and the devs feel users will want to use custom thermal spokes made by traces.)


I’ve never done it myself, but I believe you can design custom footprints in FreeCAD & StepUp and the main limitations of complexity would be your on fantasy and CPU cycles to crunch the numbers.

Hi all,

Thanks for the replies. I have done nothing special to designate the fill areas as ground other than allowing them to overlap with the SMD style pad.

I’ve tried the custom rect option for the pad and filled in some test values on the “Custom Shape Primitive” Tab. Unfortunately, I get an error: “Incorrect pad shape: the shape must be equivalent to only one polygon”

You can see that the polygon I created is one enclosed structure. Why is there another square around 0?

Thank you all for your help!

@Rene_Poschl how can I configure the zone connect of a pad? I don’t see the option in the footprint editor nor do I see it after I’ve placed the footprint into a layout.

best regards,

I’ve not done this and I’m away from my Kicad computer but netname set to GND might help?

right click on the pad -> preferences
And then in the second tab i think

@hermit: the zone settings are overwritten by the pad settings is this will not help at all.

Hi @hermit,
Thanks for the help attempt, but it is not possible to set a netname when editing a footprint. Net names are a concept only accessible at the board level.

However, there is good news, @Rene_Poschl was on the right track. If you place the SMD pad inside a polygon that you previously defined and then select both -> right click -> Create Pad from Selected Shapes everything works out. Now the fill in the layout properly observes the “Default pad connection” of the fill. Thanks all for your help! Kicad actually isnt half bad for microwave design…


You can draw lines, arc’s & polygons on any non-copper layer, and then select it and transform your custom graphics into a pad.

The non-copper layers have more freedom in drawing graphics on them in KiCad.
When you’ve transormed the custom graphics to a pad it will show up on the “Custom Shape Primitives” tab on the screenshot from your post #5.

Oops, dom11990 beat me to it.

1 Like

And a bit more detail about the freecad option mentioned above by somebody: Kicad StepUp: The Sketcher for Footprint generation

One final question… it appears that the fill in the layout does not respect the pad clearance settings in the second tab. I’ve set this to 0.254 but when I fill the zone it fills over the pad and effectively flows into the clearance of the central trace that runs through the footprint. This is not ideal, I need to to maintain the distance to the polygon I defined in the pad. When I set the clearance of the fill zone to the minimum clearance inside the footprint everything looks correct. @Rene_Poschl said pad takes priority over fill, I’m seeing the opposite. Is this correct?


This topic was automatically closed 90 days after the last reply. New replies are no longer allowed.