I am trying to create a non masked copper pour so that when the PCB is attached to a metal plate, it will create a chassis ground connection. It’s for an XLR input on a microphone preamp. I have tried to do a copper pour zone but cannot figure out how to leave the mask off. I have also thought about creating a connector pad on the footprint itself but I am worried about it covering up the five drill holes placed in the same area it covers. Any ideas on how best to implement this? Great site by the way. A lot of my questions have been answered thanks to this site. Kicad is an amazing product especially to be given away for free. Unfortunately the instructions on how to use it leave a bit to be desired.
I don’t know if you can copy the zone outline easily from copper pour to layer zone, so you might have to redraw it…
Anyhow… select the F.Mask or B.Mask layer.
Then activate the zone fill tool and start drawing… it will ask you with a dialog what and how you want it to go and then you can follow the outline of the un-masked shape you have in mind.
Features like fillets etc are missing afaik.
1 Like
If I’m not completely mistaken, there is an entry “duplicate zone” in the context menu. openGL mode?
1 Like
Yeah, there is … but in my version of a somewhat older KiCAD (BZR6608) it only allows copying the zone to other copper layers… dunno if it’s possible in latest nightlies to copy a zone to non-copper layers yet?
The way to draw non-copper zones is not obvious as one has to select a non-copper layer before he starts drawing.
Maybe I am missing something. When you create a fill zone on the B.Cu or F.Cu area, Do you still have to create a mask for it on the corresponding Mask layer? If not will it just be unmasked? I guess I assumed that the board was masked automatically unless told to be otherwise, like on a pad. I should tell you all that this is my first time using Kicad, so while I understand the basics enough to create a PCB, I am far from proficient in it.
Tracks and zones will be covered by soldermask automatically.
Just check the 3D view for reference… it’s really what you get if you turn on the realistic version.
For footprint pads the settings usually are made so that there will be a shape on the soldermask layer to expose the pad when the fab makes the board.
But that can be changed by the user… just edit a pad (either in the fp editor or right there in pcbnew for testing this).
You’ll see the options.
I disabled the paste and soldermask option for that pad there:
As you can see tracks or copper pour are covered automatically.
If one wants those areas to be free of soldermask one has to draw a zone on the respective soldermask layer to get them uncovered (backside of pcb here):
1 Like
Thanks for the clarification. I have just one more point I need some clarification on. If I create a copper pour in an area where other pads and through holes are located, then to expose it, I would just designate the non-masked area of the pour on the mask layer?
Whatever the zone covers/overlaps/contains (defined on F.Mask or B.Mask) will be without soldermask.
Just draw one and check the 3D view and post a screenshot if you can if you’re still in doubt.
I wish it was possible to add mask zones like this to footprints. I can draw boxes and circles on the mask layers in the footprint editor, but the only way to “fill” them is by using very thick lines. Also, FWIW, “filled” circles drawn this way do not seem to show up correctly in the 3D viewer, but the gerbers look right.
Just place mask only pads without a pin number.
(Add a smd pad, select no copper and remove the paste layer.)
A simple example with one circle:
MaskOnlyFootprint.kicad_mod (346 Bytes)
1 Like
I did that for one that needs a round mask, but I didn’t think of doing it with a rectangular pad until reading your reply, duh. Thanks!
Hello, thank for your answers. The link for download don’t work
I can’t do an rectangular zone or one shape without solder-mask. Someone would be to explain ?
The software has changed a lot in the 7 years since this thread ended. Please open a new one.
Thank You
1 Like