kicad-developers team mailing list archive

[jp charras <jp.charras@xxxxxxxxxx>]

Le 16/10/2019 à 09:36, Nick Østergaard a écrit :
> A related issue was brought up on
> https://forum.kicad.info/t/gerber-filenames-with-protel-extensions/14177
> 
> I think the manufacturer should only make it a warning not an error. I
> assume their reasoning is that they want to make sure only one project
> is embedded in the gerber package they have, but I don't think that is
> a fair way to determine if it is the same project.
> 
> I think having the layer names in the file name helps to verify that
> the layer is correct when viewed in a gerber viewer.
> 
> I don't think the patch is good as is, as it changes the behaviour of
> the protel file name extensions unconditionally. I think it should be
> added as a option, but we already do have a lot of options. I think
> you are better of using a python script for plotting and packing it up
> as you like it. See for example
> https://github.com/KiCad/kicad-source-mirror/blob/master/demos/python_scripts_examples/gen_gerber_and_drill_files_board.py
> 
> Don't your fab support X2 and gerber job files?
> 
I agree with Nick:

Protel extensions is outdated (and inconsistent) since a long time.

Please use X2 support and Gerber job files.

"they demand drill files to be same precision as gerbers (for example
4:5). Can you confirm that proper Excellon format should be 3:3 precision"

I confirm the best format is the decimal format, not x:y format.
Excellon files have no way to specify the format actually used in files.

The only one doc on Excellon format (this is a user manual of a CNC
machine) says the metric format is 3:3 (units = micrometer) or 3:4 (or
of course decimal format that avoid this issue.

The Excellon format is not related to Gerber format (they are 2
different formats, although based on G commands)

For recent doc on drill files see:
https://www.ucamco.com/files/downloads/file/305/the_xnc_file_format_specification.pdf

Looks to me your manufacturer want files just like Altium does.
But Kicad is not Altium.


> On Wed, 16 Oct 2019 at 09:16, Alexander Shuklin <jasuramme@xxxxxxxxx> wrote:
>>
>> Hi,
>> sorry, I'm not quite sure with that topic, as I never worked with
>> protel gerber format before. My PCB manufacturer started to use some
>> online tool to check gerbers
>> (https://www.frontline-pcb.com/products/sales/insight-pcb-overview.html)
>> and now they demand to send them files with protel extensions. But
>> that tool expect all files with same name. But now if you switch "use
>> protel extensions" in KiCad, it generate something like :
>> project_name-F_Cu.gtl
>> project_name-B_Cu.gbl
>> If "project_name.gtl" is the proper way, can you please apply my patch?
>> btw, Altium creates similar to "project_name.gtl"
>>
>> And another question:
>> For some reason they demand drill files to be same precision as
>> gerbers (for example 4:5). Can you confirm that proper Excellon format
>> should be 3:3 precision? In that case, I would send bug report to
>> them.
>> _______________________________________________
>> Mailing list: https://launchpad.net/~kicad-developers
>> Post to     : kicad-developers@xxxxxxxxxxxxxxxxxxx
>> Unsubscribe : https://launchpad.net/~kicad-developers
>> More help   : https://help.launchpad.net/ListHelp
> 
> _______________________________________________
> Mailing list: https://launchpad.net/~kicad-developers
> Post to     : kicad-developers@xxxxxxxxxxxxxxxxxxx
> Unsubscribe : https://launchpad.net/~kicad-developers
> More help   : https://help.launchpad.net/ListHelp
> 


-- 
Jean-Pierre CHARRAS