Copper Area with pure Copper for Shielding

I want an area with pure copper for connection to shielding (no footprint).
The shielding is fixed with an screw which should be connected to ground.

It’s the blue marked area in the picture. IS there an possibility to do this in the
layout section without creating an footprint?Is there something like an keepout area for

Best regards

Why is it that such a lot (majority?) of KiCad users seem to be horrified of even the Idea of making a Footprint?

I’ve read posts of user that continued here for several days for some footprint which can be made in 5 minutes.

Yup, that’s all it takes. Once you’ve done a few, you can make a (simple) Footprint in a few minutes.

And before I forget: KiCad has a few examples of these, they’re called Footprint Libraries. Have a look at for example some Footprints for mounting holes, and how they’re made.
Fiducials also have stuff on a solder mask layer.

You can probably also select a soldermask layer and draw some graphics on it (for top and for bottom), which will likely be explained in the link eelik points to.

I think the reason why are so many users are horrified is the non intuitive way of doing this.
I can give an example, I tried to solve the problem via making an footprint. I thought an easy
way should be to modify an existing. So I opened one to create an custom pad geometry via changing
it. Than the trouble starts:

I look for an custom shape -> But I can only find custom rectangle and circle…What I would need ist custom shape with combinated forms? For sure there is an way to do this, but when nobody tells you there is no logical way to find out.

So now I feel obliged to help.
Had to (re) figure out how to make something work.

  1. Footprint Editor / Place / Pad. Like so:

  2. Footprint Editor / Place / Polygon.
    Draw the Polygon over your pad like so:

(Note: Polygon is currently on silkscreen, I made it transparent).

3).Select both the pad and the polygon by dragging a rectangle around it with the mouse, then [RMB] and clik “Create Pad from Selected Shapes”.

4). Your polygon is now in the tab “Custom Shape Primitives”

Don’t try to do it using pad properties. Pads can have limited shapes.
In the footprint editor there’s a Free area draw tool which you can use for your purpose.
But if I were you, I would just create a filled zone with your geometry on the F.Mask layer to get job done.
I do this for individual “exposed copper” PCB features.

I’m not sure if this is the way to go in this particular case. Fred may be right.
It depends, as always…

If you have such a thing on each corner of the board, then you can make one Footprint (with silkscreen cutout on both sides) and flip 2 of them to the “back” to mirror them, so you do not have to draw them all individually.

Exactly, there are four of these. In each corner one. I’m still not sure if I got it right. A footprint would be cool because its an clean solution.

But how can I make an free area with the same properties?
If i use the free tool:

I never get same properties

What do you mean by “a free area”?

It was already clear from the 2nd screenshot you added later.
The Icon you mentioned is just another way to access the same. Just typing “Footprint Editor / Place / Polygon” is easier then making a screenshot. They are the same.

So I was making another custom pad.
First put some pad somewhere, then drew a polygon and a circle. Then right clicked on the circle and made it thicker, I gave it a line thickness of 2mm.

Then again, made a custom pad out of it.

If you now edit the pad, there are 2 custom shape primitives in it. The polygon, and a “ring”. You probably can add arc’s too.

Also, with the [Edit Primitive] button on the bottom, you can edit the primitives. :slight_smile:
Here I changed the radius to 5mm:

With the polygon, you can type in new coordinates for the corners with the edit function.

Also: I advise to play around a bit with how it works before you attempt to make a real footprint. Don’t worry about exact coordinates and such until you are familiar with how it all works and what you can do with it.

So I had a closer look at your first post and experimented a bit more.

A bit of a “problem” in the current version of KiCad is that you can not put lines on the edge-cuts layers in Footprints. (without a text editor).

In your particular case I would make a footprint that is solder mask only, and add a few graphics lines on a non technical layer to make it easier to align it with the edge of your PCB.
To do this:

  • Set Pad type to SMD, so no holes are drilled at all.
  • Set Copper layers to none.
  • Enable the F. and B.Mask Layers.
  • Turn off all other layers.


Then, check the results in the 3D viewer:

Thanks for your good explinations, but I actual only need the half of the circle:
How can I cut out the red marked zone so that it nicely fits in here:

I think you do not have to worry about half circles.
Everything will probably get clipped at the board edge.
Generate some gerbers and check what it looks like.
Or else, experiment with arc’s.

If you want to go real fancy, you can draw the shapes in an external program, import them as .dxf and then post process.

Footprint Editor / File / Import Outlines from .DXF

1 Like

Nice. This seems to work:

I simply will me make an rectangle and everything is fine.

In this case there’s no need for a custom shape. Just create an oval pad with SMD Aperture pad type and check F.Mask layer. The footprint covers also some area outside the board, but it doesn’t matter.

You can also just draw a graphic line on the F.Mask layer with proper thickness on the layout, without a footprint. Like this:

It takes a couple of seconds and you can duplicate it to each corner.

Or something like this, made with a circle and a rectangle shaped polygon.

Ah, just a single SMD pad may also work.

Also, if you have multiple overlapping SMD pads with the same pin number they merge into a big pad.
[ Edit: Oops, goofed up, typed too fast, Tnx eelik].

You may have problems if pads are outside of the PCB outline.

Will you post a screenshot of the final result? Maybe add some comments with tips which could be helpful for others who read this thread later?

1 Like

Pin number must not be used with aperture (non-copper) pads.

1 Like

Final result:


Thanks for the great support. Should be working I think?