Bug: Eagle 9.7.0 exporting invalid gerbers using comma digit seperators

[tekdemo]

A customer just sent over these files exported from Eagle 9.7.0 . They appear to have configured comma digit separators somewhere in their system configuration, which generates invalid output. Effectively, Eagle honors this value when it shouldn't, converting the integer and mantissa parts of the aperture decleration into parameters. If viewers even open the file, many parts of the image are missing or corrupted.

I can't include the whole file (customer data), but I can  provide the header which contains the errors. I can confirm that replacing the incorrect commas with periods resolves the issue, and the files then reads correctly. 

G04 EAGLE Gerber RS-274X export*
G75*
%MOMM*%
%FSLAX34Y34*%
%LPD*%
%INTop Solder Mask*%
%IPPOS*%
%AMOC8*
5,1,8,0,0,1.08239X$1,22.5*%
G01*
%ADD10C,5,503200*%
%ADD11R,1,703200X1,503200*%
%ADD12R,1,503200X1,703200*%
%ADD13R,2,003200X1,903200*%
%ADD14R,1,903200X2,003200*%
%ADD15R,1,403200X1,403200*%
%ADD16R,2,403200X0,803200*%
%ADD17R,0,863600X2,235200*%
%ADD18R,1,203200X1,603200*%
%ADD19R,1,633200X0,663200*%
%ADD20R,2,065200X2,065200*%
%ADD21C,2,065200*%
%ADD22C,1,981200*%
%ADD23R,1,828800X1,092200*%
%ADD24R,1,828800X3,378200*%
%ADD25R,1,092200X1,828800*%
%ADD26R,3,378200X1,828800*%
%ADD27P,2,144431X8X22,500000*%
%ADD28P,1,694157X8X22,500000*%
%ADD29C,1,565200*%

[jorge_garcia]

Hi @tekdemo,

I hope you're doing well. We've received a few reports of this issue but have so far been unable to reproduce, even when changing the regionalization settings.

If you can get us more info about what regionalization settings this user is using that would help.

Best Regards,

[jakesama]

We have a customer that submit us similar gerber files. Customer is either using Finnish or Swedish regional settings.

Our CAM processor (Downstream CAM350) will interpret the sizes of the Dcodes in a way that it will throw away the decimals. So below 0mm will become 0 width, above 1mm will become 1mm exactly etc.

This is a duplicate issue as the one fixed with an enviromental parameter FORCE_DECIMAL_GERBER_OUTPUT = true over in the bugs of Fusion 360 in this issue.

Regional number settings shouldn't be consulted when formatting these numbers, the numbers should be formatted as ###.###### always, otherwise these gerbers will lead into very serious breaking issues. If the manufacturers of PCBs will not check the apertures agains't the gerbers and wires might be completely left out from the PCBs.