I sent out a new circuit board design to a PCB fab house last week, but was put on hold multiple times for the reason of “insufficient copper to copper spacing”. I have been using the same PCB fab for quite a long time, and I’m quire sure that the design was correct, at least my EDA software (Altium Design) didn’t report any error when running the DRC (design rule check). In order to triple check that my design meets the fab’s mini trace/space capability (6mil), I even increased the minimum clearance rule from 6mil to 6.1mil, which, of course, was a nightmare as I had to go through all the wiring again. It drove me nuts when I was put on hold again for the same reason, which really confused me.
The CAM engineer told me there were more than 50 instances of copper to copper spacing less than their requirement (6mil), most of which read something like 5.5 mil or 5.7mil. The single decimal place of those numbers seems very suspicious — was the gerber file accurate enough? After going over all the parameters regarding fabrication file export, I finally figured out why:
After your PCB design is finished, you choose “File” -> “Fabrication Outputs” -> “Gerber files” to launch the CAM conversion setup. The first tab of the diagram contains the accuracy setup “Format”. As is explained, “2:3″ gives 1mil resolution,”2:4” is 0.1mil and “2:5” is 0.01mil. Apparently, if you choose “2:3” for gerber export, the decimal part of all your coordinates will be trimmed to 1mil resolution. This also means all your design is virtually moved a little bit because of the trimming, and you have no idea how the trimming is calculated, whether intelligently or not. For sure this is going to break your restraint regarding trace spacing.
However, “Gerber Setup” is not actually generating your gerber files. Instead, it converts your design to CAMtastic (.cam) file. You can think of CAMtastic as some sort of filming process, in which all your trace/silkscreeen/drill holes are retained with netlist/relationship being removed. Now you need to output layers in your CAM file respectively, which usually contains the final format the fab house takes. Then, here comes another dialog, and this is exactly where I got screwed:
In your CAMtastic window, go to “Export” -> “Gerber”, the following windows pops up:
Pay attention to the “Format” again, this is very last setup that is really going to affect your output resolution. The one I mentioned before was the resolution for CAM, and this one is for the gerber file. Make sure you choose as high resolution as you want since the default seems to be “2:3”, which caused my design failing the PCB house’s sanity test.
This time, the higher resolution export went through all the PCB houses’ process smoothly without any problem. But I still didn’t quite get it — why all my previous designs worked well in spite of my unawareness of the resolution issue? Later on, I realized all my previous PCBs were designed on a 1mil or coarser grid. This time, however, the board was so dense and I still wanted to keep the cost low on a 6mil fab. So I lowered the grid to 0.05mil. And here comes all the trouble! As it is already warned me on the first dialog: “The 2:4 and 2:5 formats only need to be chosen if there are objects on a grid finer than 1 mil.”
One thought on “Tips for gerber export in Altium Designer”
Thank you, this was very helpful!