Mounting holes (etc) and 'exclusion zone' for copper pour

Hi

I’ve noticed that the stock mounting holes allow the copper pour to encroach within the area marked with a blue circle (layer cmts.user). I would like to block the pour to outside such a zone to provide clear area for fixings. (I’m not sure what the effective difference in use is between a courtyard marking and a cuts.user marking if neither stop a pour.) Ideally I don’t want to use a pad - just a clear area with no copper. This is just one example where having an exclusion/keepout zone would be useful.

How can I do this in the footprint rather than having to edit each copper pour I do?

Also, I could not see orphan control in the copper pour settings - did I miss it? I’d like to control the keeping/dropping of orphans.

Thanks in advance

Steve

Are you talking about some video or screenshot?
Cause some of us change the layer colors, so what is blue for you might not be for us.

Copper fill is only influenced by other zone definitions, pads, tracks or board outlines/cuts (on the Edge.Cuts layer) - nothing else.

For mounting holes I use footprints, plated and unplated (examples):

z_MountPTH_3mm.kicad_mod (688 Bytes)
z_MountNPTH_3.0mm.kicad_mod (690 Bytes)

For clearances to filled zones you have to edit the net-pad clearance setting of the pad of such a footprint.

What are orphans?

Courtyard is the area around a footprint where no other courtyard should get into. It’s needed for pick&place machines to be able to assemble a board - and for humans to have some space for a soldering tip.
KiCAD doesn’t check or enforce this, it’s currently just a layout help for the user.

Cmts.User layer is yours to do what you want. Can have assembly instructions on there or some detail for the fabricator… KiCAD doesn’t care.
I use it in my personal footprints for additional information like for FPC connectors (where the cable comes out) or for SDcard slots (to show the inserted card) or for components that need to have a keep-out-area for copper fills, I mark that there too.

1 Like

blue circle (layer cmts.user)

Thanks. Ok so no ability to create a simple exclusion/keep out zone around a footprint? The problem with the settings in a copper zone is that they apply to everything in a zone. If I simply want more gap around a particular component type, e.g. a hole, I have to create an individual cut out for each and every instance or steer the copper zone around each of them. Rather more painful than it need be. The only way in a footprint to force a zone away from it is to place copper down which doesn’t make sense.

By orphans I mean unconnected “islands” which might form in a copper pour/zone due to component placement interacting with zone settings governing distance to footprints.

Regarding editing zones, is there a way to drag a corner without the corner at the other end of the line moving as well? Perhaps I am not zoomed in enough to select the exact corner but I can’t seem to correct things like a simple rectangle if I have accidentally placed a corner such that one side is too long.

That line contains the answer to your question, try reading it again. It’s not painful at all, just use a little common sense.

You cannot select to keep a zone’s isolated islands. Why would you want to?

When editing a zone you can select “Move Corner” and only that corner moves.

Apologies. I read the post hastily on my mobile phone - and not very well. That net-pad clearance setting is exactly what I was after.

Ok so default is to discard which suits me. Thanks.

“Move Corner” - thanks. I’m not finding these ‘naturally’ because KiCad isn’t recognising a right-click from my Wacom pen.

Thanks again to all of you for answering all my questions. I really appreciate it.

Hi Community,
My goal is to maximize the area of my ground plane. When I use the fill-zone option, it pours around my vias, as expected;


… though I wasn’t wanting such as large clearance around the via, per above. I was hoping for something more like this (below);

Per @Joan_Sparky;

… I thought this was the answer to my “problem”, but I’m not able to figure out how to modify the via properties to reduce the via clearance to the theoretical minimum (28mils., I figure).

Any assistance would be appreciated.

Many thanks,
Tim.

The via is not what has that large clearance set. It is the zone itself.
Every copper zone has its own clearance settings and applies that clearance to any feature of a different net. Meaning you need to check the zone properties to change the clearance between the zone and the via.


Vias however use the normal clearance assigned to the net they are part of. So if you ever really have the via as the source of the large clearance then you need to check the clearance of the net the via is assigned to.

2 Likes

@Rene_Poschl … worked like a charm (changed zone property clearance to 0.005), thanks so much. Tim.

You are aware that the zone clearance (or any other clearance) should be set in accordance with your manufacturers capabilities right?

1 Like

@Rene_Poschl … thanks very much for checking back with me on this. I may have made a poor assumption. I’m using OshPark’s four-layer service for this board, which permits track clearances of 5mils. I made the assumption that there was nothing “special” about the pour clearances vs. the standard track-to-track or track-to-pad clearances and as such set the pour clearance to 5mils, also. Was that naive?

Many thanks,
Tim.

No. I just wanted to make sure that you know that the clearance settings are driven by the manufacturers capabilities not by the designers wishes.