Gerber File Problems

I made two PCB’s (my first ones). I exported both boards independently, but when I go to upload them to my board house, I can see one board in their gerber viewer the other ones fails. I tried plotting the gerber files for both boards again, both with identical settings, and have the same problem. I also looked at the gerber files for both boards on my own gerber viewer and they look fine. I contacted the board house to see if they have any suggestions but haven’t heard back yet. Anyone have a suggestion? I attached the file here too. (51.5 KB)

Please explain how one board “fails”. The files won’t upload? The uploaded files don’t display? The files display, but the board house’s DRC software finds some kind of error?

Your attached file “” includes Gerbers for only one board. I presume this is the one that is causing problems for you. My WAG suggestions:

  1. Are the filename extensions acceptable to your board house? There are no real standards for the extensions on Gerber files, although some board houses impose their own requirements.

  2. Your back silkscreen layer seems to be blank. Is the empty layer confusing the fabricator’s DRC?

  3. Your board is offset quite a ways from the (0, 0) coordinate origin. Is it outside the field-of-view of the board house’s DRC?

  4. On a quick, cursory, review I see you have used a few non-standard (to me, at least) design practices but I don’t think they should trigger any DRC squawks.


Thanks for the reply and for taking a look Dale. I’m new to designing PCB’s, so my practices are definitely not standard. What stuck out with you that I should do differently? Definitely open to as much advice/criticism as you want to give :slight_smile:

The thing is, I made a board with the exact same plot parameters so I don’t understand what would be different. Once I upload the file (I’m using JLC for a board house), I should be able to see the gerber view but I cannot for the board that is giving me problems. I posted a picture showing the correct boards on top and the problem board on the bottom. When I try to look at the board in their online gerber viewer it tries to load but never loads but keeps trying. When I look at the working board, I can see everything in their online gerber viewer. I will check out the offset and back silkscreen as you suggested. Thanks!

Make a screenshot of both your designs (if you are allowed to. Otherwise just of the board outline layer)
And of your plot settings. Maybe we can already see something that way.

Does this board pass DRC in PcbNew?
The Via under RV2 looks to close to the trace between RV3 and C7.

You have a floating stray bit of copper trace on the front layer that is to the left of the board (and it is kinda small). Recommend setting the copper to white if using a black background to help find the trace.

It also has silk off to the right of the board.
Pressing “Home” will put both of these artifacts on the screen to assist you in finding them.

Ok thanks for the advice I will give it a try. The board does pass the DRC.

i opened your gerber, everything is fine, but for PIR_Sensor-F.Cu.gtl。 i found a extra line at top left corner(out of pcb outline)。 pls try to remove it.

(I think it’s the wiper terminal of RV2.) Clearance looks like 8 mils (0.2mm). Most quick-turn fabs will produce that as a “standard” job, but you may be right against the limits of their capabilities. Why force them to perform at that level, when you have space to move traces and increase the clearance?

A greater concern is the annular ring on your pads - only 5 mils (0.125mm). That will NOT pass the manufacturability test at many fabs.

(I think these two comments refer to the same thing.) Look near coordinate location (2800, -2325) mils ( (71, -59) mm).

Look near coordinate location (8025, -3530) mils ( (204, -90) mm).

The via under RV1 seems unnecessary, since it is so close to a component pin. Same is true for the via at U1.

There is neither a silkscreen “dot” nor a square pad to identify Pin 1 of any IC package.

The thermal reliefs are a bit stingy. Decreasing the spoke width and increasing the antipad clearance will make them more effective.

Does this board need any mounting holes?

Some of the back-side traces can probably be eliminated if you put some effort into it.

Good use of “Fill Zones”!


1 Like

I practice the philosophy, “If it’s not needed, don’t send it.” The presence of a blank layer may not confuse the CAM software, but why take the risk? And if somebody sees a file for back-side silkscreen they may assume there is something in it, and bill you for silkscreen on the second side. (Until recently, back-side silkscreen was an option that added both cost and manufacturing time to your order.)


1 Like

I just did a board out to the “Purple Board People” and I did NOT want bright white silkscreen on neither of the Front or Back sides of the board; I never sent those layers in the Gerbers.

The Web Site gave me a non-critical warning, and the boards delivered to my mail box were just fine.

This topic was automatically closed 90 days after the last reply. New replies are no longer allowed.