topic Re: Manufacture gerber output files are not correct in Fusion Electronics Forum

Manufacture gerber output files are not correct

berkelaarmrt — Wed, 29 Jul 2020 15:31:55 GMT

When I create a electronics project and draw a board, the manufacture output will return incorrect gerber data. All traces with a width <1mm are set to zero.

An user on reddit already reported a similar (same?) issue in which case the language settings was the problem. Using a ',' in a decimal number instead of a '.'

I am from the Netherlands where we also us the ',' (very annoying) but I think I have setup everything in English.

https://www.reddit.com/r/Fusion360/comments/ga96hz/problem_with_gerber_export_in_f360_everything/

How can I work around this issue in the short term so I can order my pcb's?

I have create a minimal design which shows the problem. It consists of 3 traces. The first (highest) is 0.2mm width, the second is 0.8128mm width and the last (lowest) is 1.016mm width.

I have shared my design: https://a360.co/2X7UIa0

Fusion screenshot showing the 3 different width traces.

Screenshot from a gerber viewer (gerv) and it only show the lowest trace.

I have also attached the generated manufacture output

Re: Manufacture gerber output files are not correct

jorge_garcia — Wed, 29 Jul 2020 18:41:52 GMT

Hi @berkelaarmrt,

I hope this message finds you well, the workaround in the mean time is to change your regionalization settings to be US that way the commas in the files get replaced with periods.

We are working to figure out where the error is specifically on our end, since the CAM processor shouldn't care at all what the regionalization settings are.

Let me know if there's anything else I can do for you.

Best Regards,

Re: Manufacture gerber output files are not correct

berkelaarmrt — Thu, 30 Jul 2020 10:51:37 GMT

Thanks! This works. I changed the regional format to Eglish (united states) in windows settings -> "region settings"

Re: Manufacture gerber output files are not correct

sn2010 — Tue, 04 Aug 2020 07:27:47 GMT

I got the same problem, an order at Elecrow was rejected because this. My region settings are german, temporarily setting to English created correct gerber files. Ugly workaround.

Re: Manufacture gerber output files are not correct

RichardHammerl — Tue, 04 Aug 2020 09:25:58 GMT

Hi @sn2010 @berkelaarmrt

just wanted to give a bit more information on the Gerber localisation problem. If it goes wrong, the aperture size definition in the Gerber files uses a comma instead of a period as delimiter in the values. It would be possible to correct this in a text editor, as a quick workaround.

Regards,

Re: Manufacture gerber output files are not correct

Anonymous — Wed, 09 Dec 2020 16:41:02 GMT

Hello,

same problem here - despite Fusion is configured to English language setting since first day using it. Only switching Windows to English UI language seems to help. Pretty nasty workaround, as the keyboard layout changes as well. Hopefully this bug will be fixed soon.

BTW, the CAM preview as well as the integrated Gerber viewer show correct results, but any 3rd party viewer reveals the problem instantly. So never trust a viewer integrated in the generating software!

Regards,

Holger

Re: Manufacture gerber output files are not correct

AutomaticRock — Tue, 13 Apr 2021 12:45:26 GMT

Is this problem still not fixed?
I've just send my last design to our pcba supplier, and on their end my design looks like this:

I have set the environment variable:

But that didn't seem to help?

Re: Manufacture gerber output files are not correct

RichardHammerl — Tue, 13 Apr 2021 13:47:51 GMT

Hi @AutomaticRock,

I hope you are well and all is okay. Thank you for your post.

Actually the Gerber fix for polygons has been deployed with the March update of Fusion. At the moment I am not aware of other problems with gerber output. How have the gerber files been created? Did you use the CAM Processor in Fusion electronics or did you send the PCB data to the board manufacturer?
Would it be possible to share the board / Gerber data ? So I could look into it.

Best regards,

Re: Manufacture gerber output files are not correct

AutomaticRock — Tue, 13 Apr 2021 14:10:14 GMT

Hi @RichardHammerl ,

The Gerber files have been made by Fusion with these settings:

And the weird thing is, I've 4 boards of which I've made the CAM files, all on the same day. But only one set has the meshed up copper layers and 0 width traces for tracks of <1mm width.

I've have now changed my Windows 10 settings to use the dot as decimal separator and let Fusion redo the Gerber files. Our PCBA supplier has just checked this lasted file, and now it's fine.

I don't mind sending you the board and Gerber files, but can this be done private?
Earlier today I've also files a support ticket for this; case number 17690566.

Best regards,
Benno

Re: Manufacture gerber output files are not correct

RichardHammerl — Tue, 13 Apr 2021 14:38:43 GMT

Hi @AutomaticRock

that's interesting... What are the regional settings you are working with on your Windows 10 system?

This might be interesting for our support guys as well. Maybe you could add this info to the ticket?

I'm on a German windows, but just to show you the screen how it looks on my side.

I hope this helps.

Best regards,

Re: Manufacture gerber output files are not correct

AutomaticRock — Tue, 13 Apr 2021 14:57:58 GMT

Hi @RichardHammerl ,

Besides the short date and country I have the same settings as you:

As you can see I'm from the Netherlands.

Re: Manufacture gerber output files are not correct

RichardHammerl — Thu, 15 Apr 2021 14:17:37 GMT

Hi @AutomaticRock ,

could you please send me the files (board and Gerbers), if possible. You could it send to me as private message. I would like to have a look into it and investigate with the dev team.

Thank you and best regards,

Re: Manufacture gerber output files are not correct

RichardHammerl — Thu, 15 Apr 2021 15:50:53 GMT

Hi @AutomaticRock ,

just one idea: Did you restart Fusion after you set FORCE_DECIMAL_GERBER_OUTPUT = true ?

Thanks and regards,