Hello,
I would like to remove copper pour near pads, Can someone help me to highlight what are the options? Are there any settings in Copper Zone Properties that can be used here?
One option I am thinking is, To add keep out area.
Appreciate your help!
Yes that is one option.
Also every PAD has an optional NET clearance setting, that you could try.
What exactly are you trying to do & why ?
Also, the pour has it’s own clearance that you can set to make the clearance to all non-net copper larger.
Sure, I’ll checkout NET clearance settings to see if that works.v I just want to remove copper pour between two pads, mostly between resistor pads. It is required by one of the client.
Thanks for the suggestion.
yeah, but it also increase clearance on full board and I would prefer to keep clearance below around .6mm-.8mm, and that doesn’t remove copper for footprint above R_1210.
That’s fair. I admit, adjusting the entire zone’s clearance is a bit like using a maul where a jeweler’s hammer will do. 
What, you customer doesn’t want resistors acting like see-saws on the combined height of copper and solder mask? I thought tombstoning was a desired feature of assembly? 
Seriously, I think adjusting the net clearances (ok, this is no longer a maul, more like a mini-sledge) might help. While a keepout between the pads would work, currently KiCad doesn’t natively support zones in footprints. (You may be able to kludge them in by manually editing the footprint file with a text editor, but you risk unexpected behavior when later loading that footprint into the native footprint editor.)
I think I just realized what might work well for you. You will need to modify your footprints (and probably save them out into a custom library for future use). For my example, I loaded the R_0805_2012Metric footprint from the standard libraries. Either using math, or with a fine grid and the measurement tool, determine the spacing between the pads:
I got 0.90mm by measuring. Now edit the pad and under the Local Clearance and Settings tab change the Net pad clearance from the default zero to half the measured distance (0.45mm in my example).
Now you should see a clearance border around the pad:
Make the same setting on the other pad, and you should get this (I have both pads selected simply for contrast for the screenshot):
Save this modification out as a new footprint and update all the footprints with this new one. (I.e. go to the schematic, change the footprint field in all the necessary components, the Edit Symbol Fields... tool should help make massive changes like this. Then update the PCB from Schematic with update footprints.)
You may want to edit one of the footprints on the board in-place just to make sure the results are what you want/expect. Then if you like it apply the changes board-wide.
Excellent, comprehensive, post by @SembazuruCDE !
This will enforce a clearance of at least 0.45mm around the entire pad, not just the gap between the two pads. If this clearance is too much . . . . remember that your fill zone has a “Minimum width” parameter. The fill algorithm will not place copper fill if the available space between two features (after allowing for clearances) is less than the minimum fill width. So if the “Minimum width” in your fill zone is, say, 0.15mm you can reduce the pad clearance value in this example from 0.45mm to 0.375mm.
Dale
@SembazuruCDE Great, This will do the trick. Thank you so much for the tip really appreciate it. 
Best regards
This topic was automatically closed 90 days after the last reply. New replies are no longer allowed.
