I could use some help. The last 3 boards I have ordered have had the same issue. Something I have done has caused the solder mask to very slightly separate between the pad and the plane. This is causing an issue for me if the solder makes a bit outside of the pad, it will cause the pad to short to the ground or power plane. I asked OshPark about it and they were very helpful explaining to me what I had done wrong. In trying to decipher the explanation I am googling for “Stop Mask Expansion” in KiCAD and I cannot figure out how the advice applies to KiCAD.
I would really appreciate it if someone could help me understand which KiCAD settings I need to change and then I will re-order the PCBs. I was able to get 1 of each board working so far, but it has been pretty time consuming.
Here is the feedback I received:
"The issue on this is that the board itself is fabricated without shorts, as expected. However, the stop mask aperture is so large that it can expose the nearby ground plane. Here’s a image of what the design calls for, with the green circle being the exposed area.
Because of this, it’s very easy to inadvertently short the ground plane to other signals, even if you’re careful with soldering.
There’s two relatively quick and easy ways to prevent this on future designs:
Decrease the stop mask expansion. We recommend setting this to 2mils.
Increase the ground plane isolation so it’s (mask expansion + 3mil). This is generally not the ideal solution, but is sometimes needed for smaller footprints.
With a 2 mil mask expansion, combined with our 3 mil mask shift, the exposed area around each pad will never be more than 5 mil from the pad edge. When factoring in a 6 mil ground pour isolation, you’ll always have at least 1 mil of purple solder resist protecting your ground plane from shorts."
@hedrickbt I had noticed the same on a couple of new boards when using KiCad for Windows (4.0.0-rc1-stable.). Whereby on one board, I had the same problem. The ground plane was exposed. I have not upgraded this version of KiCad for a long time so I don’t know where this has crept in from. On the boards I have done since, I am careful to check Dimensions → Pads Mask Clearance. The solder mask clearance is defaulting to 0.2mm (0.007874015748"). Going back and checking other boards I had done, this value is usually zero.
I would be curious to know if this is the setting you are looking for and how it impacts your problem.
That sounds like that could be it to me… I just checked both boards I started in the last week with the same version (4.0.6) and one of them had 0.2mm and the other was 0mm, odd.
I concur with @Steve_Mayze. It looks like your ground plane clearance is set to 5 mil and your solder mask clearance is set to ~ 8 mil. Hence the solder mask will be retracted back so as to potentially expose 3 mil of ground plane, not including manufacturing tolerances on laying down the solder mask. I might suggest that the ground plane clearance should always be greater than the solder mask clearance, and probably should be greater than OSH Park’s minimum trace clearance (6 mil on 2 layer boards, 5 mil on 4 layer boards).
I believe OSH Park’s specs indicate a minimum solder mask web of 4 mil and a solder mask expansion, retraction, or shift of 3 mil (maximum). Thus, in the “Pads Mask Clearance” dialog I usually set the Solder mask min width to 4 mil and the Solder mask clearance to 2 mil (assuming the 3 mil max is an infrequent worst case). For really fine pitch pads I’ll set the solder mask clearance to 0 and cross my fingers.
Throwing in my vote as well. I would not normally recommend 0 mils clearance, as it can start to creep up over the edge of the copper. Like @alanford said, sometimes the pitch is fine enough you want to do that, but it can really mess with pad geometries and solderability.
@Steve_Mayze nailed it. The solder mask clearance value was .007…" on my new boards and 0 on my old boards. I am using KiCAD 4.0.6 on Windows. What I find very interesting is that 0.007874015748" = exactly 0.2mm… I don’t remember setting that value and it is really odd that Steve, @ALeggeUp, and I have the exact same value.
KiCAD issue?..
I have made the following changes, thanks to @AlanFord, on the 4 boards I had issues with. I will re-order one of them and see how things look.
I didn’t notice any visible changes in KiCAD when I redrew the pours/planes (keyboard b). Is that expected?
OLD Pads Mask Clearance
Solder Mask Clearance 0.007874015748" = 0.2mm
Solder Mask Min Width 0
NEW
Solder Mask Clearance 0.002" = 0.0508mm
Solder Mask Min Width 0.004" = 0.1016mm
All of my older boards that worked fine
Solder Mask Clearance 0
Solder Mask Min Width 0
Do I need to adjust my pours from .005" clearance and .01" min width?
I created a new project from scratch and see the same default. It looks like this may be the issue we have run into.
It may help to get the default changed if you click the link on that page to tell them the issue is affecting you. I added a comment and clicked the “it is affecting me” link
We suggest 4mil Solder mask clearance, 4mil Solder mask min width. This is considered to be a semi-premium offering as far as our PCB suppliers are concerned. IMHO, a supplier should simply state what they can do, and have you configure accordingly. Our specs say 4mil, you get 4mil. Simple
What I’ve learned from this business (we do assembled electronics, and blank PCBs) is that, for almost all suppliers, that if you go below their specs, they’re going to change it without informing you. It’s harder to manage multiple suppliers and demand the same minimum specs, but it’s better for the customer.
Since we posted this info, we’ve found KiCad output to be the most trouble free of any package that we get, and now we get more business from KiCad than any other package.
Folks are afraid of not having mask between their pads, but it isn’t an issue for fine pitch. We’ve done many thousands of such placements that way. Some were even successful
Yeah, well, we get pretty detailed on what to do, and maybe even heretical. For example:
But unless you’re doing something pretty funky, our strongest suggestion is to never use Pad or Footprint specific settings for setting mask and paste clearances unless you absolutely need to.
That’s probably what trips up most KiCad (and Altium) users - they have a local setting that overrides the global settings.
Compared to some other packages, say Eagle or Diptrace, it’s really a pleasure to get something from KiCad.
Again, that’s specific to us. The biggest issue we’ve seen in regards to zones/pours is the segments setting - if it’s set to 32, we get problems. 16, all is good. Seems to be related to how arcs are handled in other contexts.
I noticed that. I created a quick account. The pricing is comparable to OSH Park too. OSH Park at $5/sq in x 3 boards ( 2 layer ) and PCB:NG at 1$/sq in (2 layer) with a minimum order of 6 boards so 6$/sq inch for a typical hobbyist order, but you get 6 boards instead of three.
I can vouch for PCB:NG quality, I tried them out last year during the beta after @jonathan was a guest on The Amp Hour (episode #299). I just did blank PCB’s but I went through the interface to place parts and it was pretty slick.
@hedrickbt - totally correct on the pricing. Any other questions, feel free to hit me by direct message or email me at jonathan AT pcb.ng - don’t want to clutter up the forums with my commercial stuff.
With the clearance and min width changes, the boards look much better. I haven’t had a chance to solder them yet, but they look the way I would expect.
Left is new board, right is old. I have no idea why the silkscreen is partially missing on the old board.
@hedrickbt - it looks like you didn’t tent your vias. Was that intentional? I usually tent them, but on my current project (still working on CentralCommand from CE2) I am tempted not to tent and use them as test points.
