topic Re: Difference between BRD and Gerbers in EAGLE Forum

Difference between BRD and Gerbers

Anonymous — Wed, 27 Jun 2018 08:04:15 GMT

Hi,

I made a board with Eagle, which was sent to an EMS for manufacturing prototypes.

when I received the PCBs, I found a short-circuit, because of a difference between my brd and the generated Gerbers.

Did you ever have this problem ? Is in a problem with the package, with Eagle, ... ?

Thank you for your help,

Thib.

Re: Difference between BRD and Gerbers

havlicek6TH3H — Wed, 27 Jun 2018 08:38:26 GMT

Hi,

It´s strange. DRC check is ok? Did you try to generate GRB files again? Is it shorted in the manufacture preview? L4 part is created by you? Try to check the part. Try to show all layers in board, maybe you will see more.

Re: Difference between BRD and Gerbers

Anonymous — Wed, 27 Jun 2018 08:53:51 GMT

Thank you for your response.

- DRC check is ok for this zone.

- Yes, I tried several times to generate Gerbers : X2, RS274X with and without comments ... It's the same each time.

- I don't know for the manufacturer preview, as it's not an online manufacturer, and I didn't ask him for his preview

- L4 part is created by me, yes, but reviewed by one of my collegue, and there are others parts I created, without this problem.

- I tried to display all layers, but nothing weird.

Re: Difference between BRD and Gerbers

huayuliang — Wed, 27 Jun 2018 09:16:01 GMT

Did you checked your Gerber files? such as ViewMate?

Re: Difference between BRD and Gerbers

Anonymous — Wed, 27 Jun 2018 09:17:55 GMT

I checked my Gerber files with Gerbview. The screenshot is the view of the bottom layer in Gerbview, where we can see the problem.

Re: Difference between BRD and Gerbers

one-of-the-robs — Wed, 27 Jun 2018 09:18:47 GMT

That looks like one of the polygon flood fills is not respecting the presence of L4 when the Gerbers are generated. I don't know what would cause that but it may be worth experimenting with the polygon's settings - particularly the "rank" and "isolate".
And always check your Gerbers in something like gerbv or GCPreview before sending them anywhere.

Re: Difference between BRD and Gerbers

Anonymous — Wed, 27 Jun 2018 09:24:01 GMT

The polygon settings are something to look at, you're right.

It's a 6-layers PCB, I control my BRD file, but not the Gerbers. I don't think I should have to check Gerber files, it's a pain and I want to trust the BRD -> Gerber conversion. But obviously, I will for this kind of problem.

Re: Difference between BRD and Gerbers

Anonymous — Wed, 27 Jun 2018 12:58:13 GMT

Looks like the same problem I have, see my other post

Would really like to know what the problem is and how to prevent it. I've sent some other boards for manufacturing that were produced with Eagle v9. Now I'm worried they will also have errors so I'm having to go back through, render with v7, and look for differences. Crazy!

Re: Difference between BRD and Gerbers

Anonymous — Wed, 27 Jun 2018 13:02:20 GMT

Indeed, it looks like the same problem. I'm using Eagle 9, I'll take a try with an Eagle 8 version to see if it's ok.

Re: Difference between BRD and Gerbers

Anonymous — Wed, 27 Jun 2018 13:19:29 GMT

Very good help marsFUHFQ.

I've generated Gerbers with Eagle 8, and there's no problem. Attached is a screenshot of the good Gerber.

So, the problem is Eagle 9, and we can't afford to use it while the problem is there, as we don't have time to control Eagle outputs.

Re: Difference between BRD and Gerbers

havlicek6TH3H — Thu, 28 Jun 2018 10:10:35 GMT

I hope that this behavior will be repaired as soon as possible. I can´t imagine, that I chck all my gerber files. It would take too much time for proper check.

Re: Difference between BRD and Gerbers

edwin.robledo — Thu, 28 Jun 2018 23:13:51 GMT

Hi thibaudZ7MQK,

Thank you for participating on the Autodesk EAGLE forum. Apparently a legacy CAM job was used to create the Gerber files. This did create some issues with the polygons on the board. This has been repaired for our next release. For now, in the easiest way to solve this in EAGLE v9.0.1 is to load the CAM Job in the CAM Processor, then double click the legacy sections to convert them into the new format. Processing the Gerber file using the new format will be able to handle the polygons the correct way.

FYI: We tested a few legacy CAM jobs in the next release of EAGLE, they worked just fine.