I've built quite a few boards at OSH Park recently and I've generally been happy with the results. While they don't run a DRC for you, they do provide layer by layer and composite checkplots that make common errors obvious.
I did have a problem with too small annular rings when I got aggressive with my design rules. Dan Sheadel responded quickly confirming that I met their design rules and refunding my payment for the mis-drilled PCBs. While I agree with Etmax about the risks of using untested PCBs, I've been able to prototype complicated designs (ie. 0.8mm pitch BGAs) on PCBs costing me only ~$70 which is hard to ignore.
The do give great service at a very reasonable cost. There are very few companies that offer an a la carte method of creation of proto designs with these design allowables. As you can see, they have had great service.
I agree that there could be errors such as this that could be found via many methods, and that file conversions can lead to errors, in this case it was faster to encounter the error and learn from it. As you can see, the design is quite small and I was able to salvage all the expensive components. I may have felt differently about a larger board.
While I agree that there are pros and cons to every shop that you use, I did not go into this blindly. I understood that there was no check of the boards, I did not pay for that, but at the same time, I was able to get quality boards boards for a price much cheaper than it would have cost me for larger boards. Judging by the fact that there are few if any complaints about the processes that are used by OSHPark, I would suggest that their vendor has their process well under control and that if designed within the tolerances of their process you should have no yield problems. On the other hand, if you cut into the design allowable by 33% and not expect to have any issues, then you are fooling yourself. In that I do not blame them or their process.
Well my fist thought would be why the CAD SW designer had a separate switch for copper pours, clearance is clearance, and why you would not want to do a clearance check I don't know. I use OrCAD and Altium and I'm not sure about Altium, but OrCAD had a DRC button that checks everything. You can set the rules for pours differently (as you should) but DRC for clearances is DRC for all clearances. Sounds like designed by monkeys.
My second thought is why your PCB maker doesn't do a DRC check against their capabilities before they start the job, it seems totally silly unless they don't warrant their product and so don't care.
My final thought is why they didn't do a bare board test? My supplier does BBT on all boards at no extra cost, I might be loading $1000 worth of parts onto what is only a $5. bare board, why would I want to use an untested part? Would you build the whole board from untested parts from the manufacturer? I doubt they would sell untested parts because their reputation is important.
I don't know, maybe I'm an OCD sufferer, but for me the cost of repairing production boards would far outweigh the cost of a supplier that does DRC & BBT.
Had you checked the Gerber files with a Gerber viewer before sending the board to be manufactured?
On the other hand, a few years ago I used the Batch PCB service from SparkFun to make a board that had a filled outline (copper pour). I specified the RS-274X file format, with G36/G37 enabled. My Gerber viewer (ViewMate from Pentalogix) and the Batch PCB design checker both showed the copper pour was OK. But the board that came back only had the thin line around the outside edge of the copper pour. Luckily I had also used thick traces (this was the important GND net) to connect the pins, so the circuit worked. Maybe the board shop thought that the copper pour and the traces weren't both needed, so deleted the pour? Or they just accidentally deleted the copper pour? Who knows. When I sent an e-mail to Batch PCB, I never got a response. By the way, another copper pour on the other side of the same board was OK.
I am currently working on a board design that I plan to send to OSH Park. When I used ViewMate to view the Easy-PC v17 generated Gerber files, I was surprised (but shouldn't have been) to find that they did not totally match my design.
I had used 0 width lines to specify various filled outlines (yes, the Gerber specification explicitly says they are acceptable for creating G36 regions), but Easy-PC had changed them to 1 mil lines, without warning me. This caused all areas to grow by 1/2 mil on each side, which caused some clearances to be less than required.
Also, I had used some rounded rectangle pads. Easy-PC didn't use arcs for the corners, but instead generated 2 or 3 line segments to approximate the arc, which looks ugly. The Gerber specification has an example of how to write a macro to generate rounded rectangle pads -- it's actually easier than using line segments.
Not using enough resolution for the Gerber coordinates can also make the manufactured board vary from the design due to rounding errors. Ucamco (who produce the official Gerber file specification) actually suggest using 6 decimal places for inches, and 5 for millimetres.