In reference to this question, do you actually perform DRC on Gerbers? Or do you do it for the PCB (post-design or interactive) and trust that the generated Gerbers will be OK?


One thing should be clear: you can't just do a DRC on the Gerbers alone. Your PCB design may have several design rules which the Gerbers don't have information about, like clearance between nets (like mains voltage and SELV) or trace width for high current nets.

I have interactive DRC, so I get warned when I'm violating a design rule during layout. Before I create my Gerbers I run DRC again over the complete design. That's it.

The PCB shop may/will run a DRC on the Gerbers it receives, mainly to check minimum trace widths and clearance between traces/pads. If you talked these through with your shop you should have the same design rules in your EDA software, and you shouldn't get any surprises.


I always run the "DRC" in my PCB software before generating Gerbers. The netlist and most of the other information that is helpful for finding the kinds of common errors that DRC is supposed to catch is simply unavailable in any of the Gerber files.

I don't run any sort of check on the Gerbers, other than printing out the Gerbers at 1:1 and briefly glancing at it while dropping a few physical components on it.

Advanced Circuits and a few of the other PCB manufacturers have software that somehow performs DRC checks using the limited information available in the Gerber files.

In theory any possible problem they could find should have already been caught by my PCB software DRC check. In practice they have caught a problem on more than one board of mine that the DRC in my PCB layout software somehow missed.

  • 1
    \$\begingroup\$ Graphicode's GC-PrevuePlus Gerber viewer/editor has support for DRC although I believe the rules are stored in a separate project file. The free version doesn't have this feature although there is a "DFM" (Design For Manufacturing" menu item which doesn't seem to do anything. \$\endgroup\$ – MikeJ-UK Apr 12 '12 at 15:08

The only sensible path is to check both within the CAD software ("is the design correct") and also check the Gerber, drill, etc. files ("will it be correctly fabricated").

Your CAD system will have high-level information about what you're trying to accomplish. In the world of CAD software people this is called your "design intent". Starting with the schematic's logical connections, the layout can be confirmed. But, just because the CAD system thinks things are going to be connected, the fabricated reality may be quite different.

The people that build the board are very, very likely do so from Gerbers. They may get the gerbers from you, or they may generate them (many shops have a "native design conversion" option of some kind). Either way, the machines they have need gerbers and the outcome of fabrication will depend on how well they are crafted. It's not just about "trace and space". There are a myriad of problems that come into play when copper is removed from fiberglass with acid, holes are drilled, etc.

Review your gerbers after you confirm your design in CAD. Use a free gerber viewer to grab pictures to include with the order so the board shop knows what you saw when you thought to yourself "yeah, that's what I want".


Your Answer

By clicking “Post Your Answer”, you agree to our terms of service, privacy policy and cookie policy

Not the answer you're looking for? Browse other questions tagged or ask your own question.