I got an Error
Error: Front solder mask aperture bridges items with different nets
The connector where this is occurring has pads with 2 mm of space between the pads.
The soldermask expansion is 0. In the Board Setup and in the Clearance Overrides and Settings.
What am I missing?
Posting a screenshot may help.
I am not sure how the screen shots will help, but here they are.
It must be some configuration setting I cannot find.
Kip
Looks to me like the pads on that device were drawn with a huge soldermask expansion.
Edit the footprint and see if there is a soldermask clearance override being set. If so, remove it, or modify it to be smaller.
I think I found it. But I do not understand it.
The part was from SAMTEC QTH-030-02-L-D-A
In the part, for each pad, under pad properties they had under Clearance Override and Settings a solder mask expansion of 0.102 mm. I changed it to 0.1 mm and it did not fix the problem.
I changed it to 0.05 mm and that fixed the problem.
I am not sure why they had an override at all. The pins are on 0.5 mm centers. With pins that close I would have wanted solder mask between pins to help prevent solder bridging.
I am still thinking about this.
Have you checked the data sheet for the footprint recommendations?
Solder mask is one of those area’s that is not well defined. PCB manufacturers always have some manufacturing tolerance for the placement of the solder mask relative to the copper of the pads. As a result, when the solder mask has the same size as the copper, then the actual exposed copper area will vary on production tolerances, and that is a bad thing for manufacturability.
None the less. I think it’s still the most common to use no solder mask expansion at all. In this case, the PCB manufacturer will often add a little bit of solder mask expansion to accommodate for the tolerances in their own production process. The goal is that all copper of the pads will be exposed, even if the solder mask shifts a bit in production. (These tolerances are in the order of 100um or so).
But there is no guarantee that your PCB manufacturer will do it this way. We’re all living on a big round mud ball here and people seem more inclined to argue then to seek consensus.
And with SMT pads of a relatively fine pitch (0.5mm or so) there is yet another problem. The remaining solder mask between the pad becomes a very thin sliver. And these thin sections can (and do) break off, and the loose hair like bits and pieces cause problems elsewhere. I am guessing that this was the reason for the solder mask expansion in your SAMTEC footprint. The intention proabably was to remove the solder mask in between the pads.
If it’s not complicated enough, then I dare you to a search for:
https://html.duckduckgo.com/html?q=solder+mask+defined+pads
Ooh, SMD (solder mask defined) pads vs NSMD (non-solder mask defined) pads is an interesting topic. I came upon it in this document for LEDs. They have great pictures and drawings and describe it on page 7.
Working with NSMD pads is what caused me to first see the error that OP is discussing, and I eventually just ignored the error. It’s not an error if it’s intentional. My PCBs all turned out fine.
If you’re interested or even just curious, I recommend giving it a little read:
Fixed ? 
0.05mm could be not acceptable as because of manufacturing tolerances it can lead to soldermask being partially on pads what probably negatively affects automatic assembly. When reflow soldering, the component may be pushed off the pads instead of being automatically centered on them.
Since always I was using solder mas expansion of 3 mils (0.075mm) and minimum solder mask width also being 3 mils. This defines the distance between pads to be 0.225mm or more. So for example for 0.5mm pitch with 0.3mm pads you can’t have soldermask between pads.
When a dozen or so years ago I came to this problem I discussed it with our contract manufacturer and found that they were surprised I am using here 3 mils as they, for both this parameters use 4 mils.
Sorry, but what you want is less important than what technology accepts.
Now, for 0.4mm pitch footprints with 0.2mm pads I have reduced my 3 mils a little and have soldermask between pads but it is after consultation with contract manufacturer, who agreed it with PCB manufacturer and he have to know which PCBs use it to order them from PCB manufacturer who confirmed it.
For 0.4mm pitch footprints with 0.22mm pads I use big soldermask openings covering whole pad rows.
This may sound too confident because of language barrier. It’s possible that the manufacturer doesn’t like so small value, at least for their cheapest price, but it’s also possible they accept 0.025 mm. And remember they may also want zero, doing their own modification fitting their processes.
So, you must ask them, not us.
Thanks everyone. You have given me a bunch to read.
Kip
