Copper traces looks fine in F360, but they are not in the exported gerber!

[Anonymous]

Hi there,

My PCB looks perfect in the CAM preview, good copper, good holes, everything in place. I export the gerbers files, and on the copper layers, I have the result you can see in the picture (no traces).

I thought that was a problem with my viewer (gerbv), so I proceeded to production and the manufacturer said that my copper traces were inexistants so he couldn't produce it.

Am I doing something wrong?

[everettac]

From your screenshot, it looks like they are there, but ridiculously thin. You might want to check your trace widths in the board editor. I believe default width should be 6 mil. Also, I’m not sure what process your manufacturer is using, but if it is an acid-based one, the acute angle in the intersection could prove to be problematic.

[Anonymous]

Thanks for your answer.

simple signals are 6mils (default), some are 10, and the main power is 12mils (the one showing in the screenshot should be 12).

and all looks perfect in the 3D PCB, also the CAM preview, and also the CAM processor where you can export the gerbers. The problem seems to appear during the export...

[Anonymous]

Here a screen of what it looks in F360 with the poly unpoor

[jorge_garcia · Accepted solution]

Hi Benn2525,

Are you in a location where commas are used in numbers? Looking at gerbv the traces are super thin, I'm concerned that maybe some regionalization setting has been affected.

Could you open your gerbers in a text editor and see if there's anything noteworthy? Or if you could post a sample gerber file that would be helpful.

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

Best Regards,

[Anonymous]

OK some news, hang on it becomes ever weirder (+solution!!) : 

so I yesterday I quit after being unsuccessful, trying to reset all the traces to the default 6mils, rip everything, and reroute everything... nothing worked, so I closed F360 and went to sleep.

Next day morning, I restart F360, try to export one more time and.... IT WORKED !! (yay!!)

So I set one trace to 12mils, and 4 other to 10mils, reexport and.... the problem was back! every traces being just virtual lines! I saved everything, quit F360, and restart it. Reexport without changing anything and.... SUCCESS !!

Now the juicy stuff, and sir, you were 100% right as far as I can analyse in the gerber:

the buggy output:

%ADD10C,1,524000*%
%ADD11C,1,879600*%
%ADD12C,1,524000*%
%ADD13C,1,308000*%
%ADD14R,1,100000X1,000000*%
%ADD15C,0,304800*%
%ADD16C,0,152400*%
%ADD17C,0,756400*%

the good one:

%ADD10C,1.524000*%
%ADD11C,1.879600*%
%ADD12C,1.524000*%
%ADD13C,1.308000*%
%ADD14R,1.100000X1.000000*%
%ADD15C,0.254000*%
%ADD16C,0.152400*%
%ADD17C,0.756400*%

see that? dots and commas!

I am in Japan, but I set everything in english in F360, and right now my windows is...in french (and yes in france we use commas! :'( ).

Can I do something to force dots during output?

[jorge_garcia]

Hi @Anonymous,

I've pinged the developers on this. For now the best suggestion I can give is to set your Windows to be in English and see if that fixes it. Our devs will be looking into this because this is serious.

Best Regards,
Jorge Garcia

[Anonymous]

Thanks a lot!

for the records, I changed the units in the windows control panel : asked for the decimal sign to be a dot instead of a freackin' comma.

that should do the trick from now.

Thanks a lot for your help.

[christopher2KLSVU]

I had a same problem, thanks for this solution, I set a windows region as US.