Any way to have clearance from the copper of the mounting hole to the edge of the board? I was not able to find any way to pull it back between the board setup and footprint override settings.
Unfortunately no 
It would be FANTASTIC if KiCAD could do something like this as right now the only way to manage this is
- move such pads inboard
- custom pad creating a chord
- discuss with the fabricator to instruct them to pull the copper back
- YOLO it and risk burred copper due to the routing bit
Right now with Mentor Xpedition we are doing #3
1 Like
I don’t see this as a significant problem.
Just draw a small zone in the corner, drop a pad with a small annular ring, and assign it to the zone’s net (presumably ground). Then fill with no thermal clearance.
Probably take 30 seconds per corner.
Got it, thank you! Hopefully it’ll be added at some point, but I wanted to make sure I wasn’t missing a setting somewhere.
Clipping pads by the board edge is generally a very bad Idea. The method from 3Dogs is good though. Just use a smaller pad that fits, and add a copper zone around it.
1 Like
in general, the fabricator will pull that copper back for you to whatever minimum they need.
sort of idea #3.5 from above.
you can also try the “margin” layer to bring the copper back from the edge.
That is a very flawed assumption. The results vary between the manfacturer modyfing your gerbers to do the pull back, but you can also get PCB’s with smeared copper and shorts on their edges, and other manufacturers may bluntly refuse your PCB’s, or start mailing you to ask what the intention is.
And for me those are all bad options. I don’t like them modifying my gerbers. I don’t want bad PCB’s and I don’t want delays, or waste their time. I.e: The only good way is to pay a bit attention to what you do and generate quality data, that goes though the process without further issues.
1 Like
In general I agree with you, I have a note in my fab drawing that says they’re not allowed to change anything without approval.
but… for this particular thing with mounting holes near the edge I think letting the fabricator pull the copper back is ok. because you wouldn’t (shouldn’t) have put any traces under or inside the mounting hole anyway. so if any of the bad things you mention happen it won’t make a difference in the final board. If I was making 10000 of something I’d do it differently.
When using edge plating, pulling back the copper from the edge would ruin the board. With castellated holes the copper also goes right up to the edge of the PCB. There are a lot of different ways people want their boards made. Assumptions go wrong, and if it goes wrong because a PCB manufacturer made a faulty assumption annoying. If it goes wrong because you’re to lazy yourself, it’s a good lesson to be more attentive the next time.
you’re going off-topic. we were talking about mounting holes, not edge plating or castellated boards… those are different things.
You’re attempting to defend an undefendable position. Gerber files don’t have mounting holes nor pads. They just have copper features (except for the lastest Gerber standard, which is rare it the wild).
You are relying on your PCB manufacturer interpreting the gerber files in some particular way. That is already beyond what they should do.
But I agree it’s a senseless conversation. Is it OK for you if I delete the last couple of posts from this thread?
I disagree. your run of the mill fab will take your gerber’s and mask as per your design and then you don’t actually get what you designed for, especially with higher weight copper.
Higher quality fab houses will work with you throughout and will modify the GERBER’s to align with their process AND will feed back their artwork so you sign off (usually a simple XOR). 99% the only difference is every single copper shape is slightly larger to manager their etching process so you get very close to what you ask and it is acceptable… every now and again they do something to assist them but have misinterpreted your needs resulting in an artwork modification that needs correcting…
I had this 2weeks ago with a 12layer flexi-rigid and the fab sent back the artwork and they had add copper balancing to manage their process and unfortunately where they had placed the shapes resulted in two key tracks having a copper-copper creep distance of ~0.5mm when I needed > 2mm for safety reason. Once their process was understood and why they needed balancing (we took all the copper away…), we added the copper balancing in a controlled manner.
I agree it’s complicated.
First you disagree, and then you give an example of how a modification by a manufacturer broke your board design.
Also with solder stencils. Some manufacturers make the stencil as ordered. Others do weird things with it. What sort of stencil do you get if you order like this:
It’s a hit and miss, For one project it may work, for another project the stencil may be worthless, and you don’t know what they did.
I also agree that good communication between you and your board designer is a big positive. But you won’t get that from the cheap chinese pooling service. (But likely it’s good enough for “simple” boards, especially if put some effort into getting the design right in the first place)
See also this remark from Naib:
(Oops, you are Naib 
)
but as I said, board fabricators modifying the GERBERS is quite standard. I am just in an industry that knows that and will always ask for artwork back. if they refuse we do not work with them.
One could say we broke their fabrication process,
what is important is a solution was found and that is only possible by engaging with the fabricator IF you need something non-standard AND you want to pay.
difference here is, I know when my fab’s change teh artwork (they all do). The vast majority of people won’t even know that it was done
And this is the key part. Basically you get what you pay for.
A cheap place will just take the routing bit and screw up your PCB’s.
Likewise every place is slightly different so what they do will be slightly different either due to some experienced CAM engineer or they have a different etching soup.
damn that person is smart, I agree with his statement
A couple of thoughts:
- Add an exclusion zone between the edge for the desired spacing. I’ve not tried this.
- Make a custom pad with the large OD and a smaller copper area.
- Possibly export the pad to Freecad and trim the copper to the desired size. Import back into Kicad.