Re: [Kicad-developers] Should gerber files in protel format use same name? (PATCH?)
Hi, Thanks for answer, well, I think that's stupid things they do, Just if we stay on that format we have, that's a point, I will use the python scripts. You see, that's very common PCB manufacturer in Russia. And if it's decided to use scripts, and their company will change nothing, I will write them instructions how to deal with their production with KiCad. Just I want to be sure, that's I know the proper way to do it. On Wed, 16 Oct 2019 at 11:08, jp charras wrote: > > 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 Protel extensions is outdated (and inconsistent) since a long time.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 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@lists.launchpad.net > >> Unsubscribe : https://launchpad.net/~kicad-developers > >> More help : https://help.launchpad.net/ListHelp > > > > ___ > > Mailing list: https://launchpad.net/~kicad-developers > > Post to : kicad-developers@lists.launchpad.net > > Unsubscribe : https://launchpad.net/~kicad-developers > > More help : https://help.launchpad.net/ListHelp > > > > > -- > Jean-Pierre CHARRAS > > ___ > Mailing list: https://launchpad.net/~kicad-developers > Post to : kicad-developers@lists.launchpad.net > Unsubscribe : https://launchpad.net/~kicad-developers > More help : https://help.launchpad.net/ListHelp ___ Mailing list: https://launchpad.net/~kicad-developers Post to : kicad-developers@lists.launchpad.net Unsubscribe : https://launchpad.net/~kicad-developers More help : https://help.launchpad.net/ListHelp
Re: [Kicad-developers] Should gerber files in protel format use same name? (PATCH?)
Alexander Shuklin schrieb: >>"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" jp charras schrieb: >Excellon files have no way to specify the format actually used >in files. As I have access to commercial Gerber Tool at work, I recently did some tests for importing diffrent Excellon format precision into GerbView: 7+8 digit formats (seems possible but no standard (???) and) are not detected automatically by GerbView. 6 digit formats 3.3 or 2.4 or 4.2 always import correct with or without leading zero supression or step Another thing I found, that the (old header) G81 FMT1 instruction generates error message while G05 FMT2 equivalent does not (but both behave well). If anybody is interested in test file data I can dig for them or generate new test files ___ Mailing list: https://launchpad.net/~kicad-developers Post to : kicad-developers@lists.launchpad.net Unsubscribe : https://launchpad.net/~kicad-developers More help : https://help.launchpad.net/ListHelp
Re: [Kicad-developers] Should gerber files in protel format use same name? (PATCH?)
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 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@lists.launchpad.net >> Unsubscribe : https://launchpad.net/~kicad-developers >> More help : https://help.launchpad.net/ListHelp > > ___ > Mailing list: https://launchpad.net/~kicad-developers > Post to : kicad-developers@lists.launchpad.net > Unsubscribe : https://launchpad.net/~kicad-developers > More help : https://help.launchpad.net/ListHelp > -- Jean-Pierre CHARRAS ___ Mailing list: https://launchpad.net/~kicad-developers Post to : kicad-developers@lists.launchpad.net Unsubscribe : https://launchpad.net/~kicad-developers More help : https://help.launchpad.net/ListHelp
Re: [Kicad-developers] Should gerber files in protel format use same name? (PATCH?)
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? On Wed, 16 Oct 2019 at 09:16, Alexander Shuklin 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@lists.launchpad.net > Unsubscribe : https://launchpad.net/~kicad-developers > More help : https://help.launchpad.net/ListHelp ___ Mailing list: https://launchpad.net/~kicad-developers Post to : kicad-developers@lists.launchpad.net Unsubscribe : https://launchpad.net/~kicad-developers More help : https://help.launchpad.net/ListHelp
[Kicad-developers] Should gerber files in protel format use same name? (PATCH?)
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. From 1357e1f191043809e0dfc7b00ec2ac7af4a3ec08 Mon Sep 17 00:00:00 2001 From: Alexander Date: Wed, 16 Oct 2019 08:04:02 +0300 Subject: [PATCH] Use same file name when plot with protel extensions MIME-Version: 1.0 Content-Type: multipart/mixed; boundary="2.23.0" This is a multi-part message in MIME format. --2.23.0 Content-Type: text/plain; charset=UTF-8; format=fixed Content-Transfer-Encoding: 8bit --- pcbnew/dialogs/dialog_plot.cpp | 6 +- 1 file changed, 5 insertions(+), 1 deletion(-) --2.23.0 Content-Type: text/x-patch; name="0001-Use-same-file-name-when-plot-with-protel-extensions.patch" Content-Transfer-Encoding: 8bit Content-Disposition: attachment; filename="0001-Use-same-file-name-when-plot-with-protel-extensions.patch" diff --git a/pcbnew/dialogs/dialog_plot.cpp b/pcbnew/dialogs/dialog_plot.cpp index 5f1c97fa7..ecedf61f1 100644 --- a/pcbnew/dialogs/dialog_plot.cpp +++ b/pcbnew/dialogs/dialog_plot.cpp @@ -834,7 +834,11 @@ void DIALOG_PLOT::Plot( wxCommandEvent& event ) if( m_plotOpts.GetFormat() == PLOT_FORMAT_GERBER && m_useGerberExtensions->GetValue() ) file_ext = GetGerberProtelExtension( layer ); -BuildPlotFileName( , outputDir.GetPath(), board->GetLayerName( layer ), file_ext ); +// Do not use suffix for protel extensions +wxString suffix = ""; +if( !m_plotOpts.GetUseGerberProtelExtensions() ) +suffix = board->GetLayerName( layer ); +BuildPlotFileName( , outputDir.GetPath(), suffix, file_ext ); wxString fullname = fn.GetFullName(); jobfile_writer.AddGbrFile( layer, fullname ); --2.23.0-- ___ Mailing list: https://launchpad.net/~kicad-developers Post to : kicad-developers@lists.launchpad.net Unsubscribe : https://launchpad.net/~kicad-developers More help : https://help.launchpad.net/ListHelp
