As and after the PCB is designed, I check it using the native CAD tools. What do I need to check to make sure the generated Gerber files are ok?
The main point for me about looking at the Gerbers outside my primary CAD is to make sure everything looks OK. I put a lot of trust in my main CAD package, and use the Gerber viewer as a qualitative verification.
Things I look for:
- All layers are aligned
- All layers are present (file exists)
- All layers have data (not just vias)
- Board outlines have the correct dimensions
- Fill polygons have the right isolation, orphan settings
- Make sure your soldermask is correct near high-density parts (tented vias, etc.)
Making sure that Eagle merges the layers correctly is my biggest worry when I'm checking the Gerbers, because if you aren't using a 100% verified CAM flow, what you see on the page might not be what you get in the Gerbers. Other than that, everything should be the same. Think of it as looking at a printer's proof before ordering a lot of copies.
If you have the components on hand already, print the outer layers out at 1:1 and place all the parts on there. Ordering parts and boards at the same time is a little faster, but this would have saved me a couple board respins.
Your layout software should have checked the design rules. It's unlikely you'll find design rule errors on the gerbers that the PCB software missed. On the other hand, using gEDA-pcb's photorealistic rendering output, I've caught a few errors before fab, mostly soldermask.
Your fab will have a checklist of capabilities on their website. Go through this line-by-line.
EEVblog #127 discusses such things as panelization and fiducials. Worth watching, especially if you are designing for machine assembly.
A few gotcha's:
Make sure that the top and bottom layers are oriented the same way. An easy way to do this is to check that the soldermask for the top and bottom line up on a few through-hole vias and pads.
Gerber vs. Drill alignment:
Sometimes, the drill holes and the Gerbers will be grossly misaligned. Perhaps the gerbers are centered on the origin, and the drills have their bottom left corner at the origin.
Font not rendering correctly:
Unlike your PCB editor, Gerbers don't have a font library. Make sure to use a vector font, which can be defined as a series of vectors in the gerber, rather than a proportional font, which might be different (and may not) on the gerbers. This may only show up as a difference in character widths, which may or may not cause trouble.
These are easy to see in a Gerber viewer like GC-Prevue, but hard to detect in your export settings.
Check them with a Gerber viewer, I use GC-Prevue.
In addition to manually checking the gerbers as well described above, I also like to send the gerbers through an external checkers to ensure that my design rules were correct. There are many of them, mostly free. If you're really paranoid then send it through more than one service and compare results. A quick Google search for "dfm check" resulted in these three but there are others. I mainly use the first but I have used others. - freedfm.com - smartdfm.com - betterdfm.com When you get their results, go back into your gerber viewer program and see if you can spot the errors. That way you'll know what to look for when you view your gerbers the next time.
I use ViewPlot to view my gerber files generated by Eagle. Mainly, what I'm looking for is that my silk screen is all there, and that my drill holes line up with my solder mask. Specifically for the silkscreen, if you look at the assembly drawing only, that can be there but not present on the silkscreen layer
- Check that the layers are all present and numbered correctly. This can be a problem when adding, deleting, or reordering layers to a design.
- Check inner layers for missing pads.
- Check the notes.
- Check the stackup, including controlled impedance requirements.
- Check for thermal relief, if desired.
- Are the pin 1 indicators visible, even when the parts are installed?
- Does the CM need panelization? If so, does it meet their requirements, such as rails on the sides?
- Fiducials present for the PCB and BGAs (and panel) and they meet the CM's requirement.
- Make sure copper or silkscreen has the bare board part number and revision.
- Are the Gerbers in the zip files those for the board designed, for the latest revision? This can be an issue when the Gerbers were generated, an error in the design found, but the Gerbers weren't regenerated.
In addition to all the good answers, I would suggest doing a 1:1 scale print, double sided if possible, to check component dimensions, board dimensions, writing orientation, drill sizes, clearance for for container if any.
Few mistakes I have made in the past.
- Mirrored text
- Slightly wrong footprint for a specialized component
- Drill holes for resistors too small
If you can someone else to question your design it would also be a plus.