Specifically, based on my experience this is atypical. Most MFG will spec something called “soldermask swell” which is an expansion of the epoxy layer after curing, which is on the order of a few mils. And you take that into account in your clearances.
What this actually means in practice is that OSHPark is adjusting the Soldermask back a few mils to achieve the exact clearance specified in the gerber. Which is to @Rene_Poschl point that they are adjusting the pullback for you. Which may be desirable in some settings (like small run prototypes)
In some software soldermask clearance (used to define SMD/NSMD pad) is different parameter from soldermask pullback (used to account for soldermask swell).
P.S. a good mfg will try to do a cursory Design for Manufacturing review and identify problematic areas, I have been asked before if it was OK to add additional clearance to a pad they were concerned would get covered by soldermask. Because I know fabs do this regularly is why I suspect OSHPark is doing this as well
And, why would I not expect any Fab house to do this?
To your point, I did go down to the local hardware store and asked to have a 2x6 cut down several times. The adult idiot hired by the store never took into account the thickness of the blade; which is something I learned when I was 12 years old.
I also recently went to a company to have a template made by being laser cut out of acrylic. I specified the final hole size that I wanted, and they had no problem accounting for the small diameter of the laser beam to get the final cut the specified size.
The problem that I have is that I understand SMD/NSMD pads. Also, the fact that unless the normal/default clearance is set to zero, then how will the Fab house understand what you want if the design requires both?
I am going to continue to specify zero mask clearance until I find a Fab house that can do everything else right for the best price, and it is the only issue they can’t fix on their end.
The ultimate suggestion is to use an Engineering Drawing that calls out these features and explains your design convention. Putting the burden on the supplier to match what you are getting from OSHPark . For example, you can include a statement such as “All Soldermask Clearance for pads specified nominally, add sufficient clearance to guarantee NSMD Pad after expansion for SMT pads”, If you have a small number of SMD features you can literally point to them individually in the drawing, or you can include a small negative clearance to indicate your preference.
Having an engineering drawing, will at the very least, force the manufacturer to reach out to you with questions about your intent. But it also gives you an explicit place to state your design convention, using words to communicate that which is limited by the gerber format (More on that later)
Well , in principle I agree with you, but there is a “soft” industry standard/convention for soldermask dimensions, just like in machining there are certain conventions. Either way works, but mismatched conventions can cause confusion, so explicitly stating your need in a drawing is a good way to make sure everyone is on the same page (or you wait until prototypes and complain to the fab!)
Now part of this comes in some part due to the gerber format itself. Which is a plotting format that originally was directly used by the tooling, and does not carry any CAD data with it. So the burden was on EDA and the designer to take into account the process limitations. Now-a-days the fabs tweak and tune the gerbers more easily and do this for convenience of customer more often
Many manufactrurers are shifting from plotter assets to using the actual CAD data, the industry standard for this is ODB++ which includes real data for soldermask clearance and pullback, but some will also accept native formats like kicad or eagle files. Less common among PCB only mfg’s but certainly the new standard for PCBA.
A lesson learned hard way: always tell the manufacturer explicitly what you want unless you follow their predescribed rules. Because some summer holiday student worker (or some senior engineer) may think you have made a mistake and change SMD to NSMD. No matter what you believe is possible or whether the manufacturer is big and old or small and new company.
Good point, Which just reinforces my overall suggestion.
Instead of assuming, one should provide an engineering drawing where you can explain this stuff in words and sentences. Then you can expect exactly what you ask for. Creative use of the User and Documentation layers can let you create this directly from PCBNew but sometimes this is done in an external drafting program.
That goes against the currently fashionable practice of “user friendly” web pages where you simply clicky-clicky on a few menu choices and upload a pile of Gerber files.
Perhaps the problem will go away if there is ever an agreement on a replacement for the Gerber file format. (Except for incorporating the “aperture file” into the data files, it hasn’t changed much since the 1960’s when it was created to control mechanical photoplotters in the printing industry!) In the meantime, perhaps you could try telling the board vendor to build exactly as shown in the *.TSM and *.BSM files . . . . except that is essentially creating an Engineering Drawing!
Dale
P.S. - Almost half a century ago, the instructor in my university “Technical Communications” class (required of all Engineering students) said that we would be making, changing, or reviewing drawings as long as we were doing engineering. I didn’t believe him. I figured that, as an electrical engineer, I’d easily get along with nothing more than sketches of schematics. I wish I had paid closer attention in that class . . . .