Hi Jean-Paul,
I used millimeters. Did not try using inches, so may be that's the cause.
If I look to the drill files in a text editor, then the difference is that the
decimal format has the dot devider in the number, where options with the
supressed zeros do not.
There must be some problem with interpreting millimeters correctly in these
cases
The layout of the drills are fine, but only 10 times larger then the real board
size.
So far using the millimeter with decimal format goes fine, but may be I have to
switch to inches when starting with Gerbmerge for the multipanel
Best regards,
Ellio
PS. I prefer to use millimeters, it's about time to finally get rid of inches
and such.
The metric system is just calculating much easier, especially between
different units.
--- In [email protected], "Jean-Paul Gendner" <jean-paul.gend...@...>
wrote:
>
> I am surprised, because I use GC-Prevue with the default values to show the
> drill and Gerber files without any problem. More exactly, the first time, I
> tried to use Millimeters, and there I had a difference between drill and
> Gerber files. So I switched back to Inches and there all was OK. However I
> only worked on single board, not multiboard.
>
> Regards,
>
> Jean-Paul
>
>
>
> ****************
>
> Jean-Paul Gendner
>
> 03.88.27.03.44
>
> _____
>
> De : [email protected] [mailto:[email protected]] De la
> part de elliomartina
> Envoyé : lundi 25 janvier 2010 02:06
> À : [email protected]
> Objet : [kicad-users] Viewing KiCad drill files in GC-Preview or Gerbv- Got
> some strange results
>
>
>
>
>
> I am using KiCad for a few weeks and have designed a few boards ready for
> production.
> Following the advise to check the Gerber files, I installed GC-Preview on my
> Win box and Gerbv on my linux box.
>
> Found some tips for the settings to be used when creating the drill files
> and discovered that most of the settings do not work for viewing them in
> both viewers.
>
> So I started analyzing about what happened when creating the drill files
> using different options of the settings panel and viewing them
>
> As Gerbv did not show anything properly when starting I first tried with
> GC-preview using the some suggested working settings I found with searching
> for solutions.
>
> I started off with Driil Origin = Auxiliary axis and then trying several
> Zero formats.
>
> All of the comined options except Decimal Format did not work at all to get
> a good result
> Mirror X axis should be OFF by default or you never get the drill holes into
> the board layout, at least I did not get it
>
> Here are some messages GC-View showed when importing the dril files:
>
> File format: Seen by GC-Preview as:
> Result:
> Supress Trailing + 2.4 Aux origin = 3.2/Abs/mm/Trailing Supp/Quad ->
> size=x10
> Supress Leading + 3.2 Aux origin = 4.1/Abs/mm/Leading Supp/Quad-> size=x10
>
> !!!! x10 means that you see the drill holes, but sized 10 times that of the
> board!
>
> I noticed that the format changed not consistently when selecting trailing
> or leading.
> Depending on saving the settings in the plot panel, the format displayed
> either 3.2 and 3.3 or 2.3 and 2.4 when opening the Drill export panel. This
> is somewhat confusing.
>
> So I selected also some settings in this "confusing" modes
>
> Supress Leading + 2.3 Aux origin = 3.2/Abs/mm/Leading Supp/Quad-> size=x10
> Supress Leading 2.4 Aux origin = 3.3/Abs/mm/Leading Supp/Quad-> size=x10
> Absolute origin selection did not work either with these supress options
>
> Finally I tried to use the Decimal format option.
> File format: Seen by GC-Preview as:
> Result:
> Decimal Aux origin = 4.1/Abs/mm/Trailing Supp/Quad -> Screen size= OK
> perfect result
>
> Decimal Absolute = 4.3 /Abs/mm/Leading Supp/Quad- size= OK but the drills
> are placed on negative Y-axis Not mirrored however.
> So this is not usable with GC-Preview since the absolute Gerber files are
> placed as the auxiliary ones.
>
> With Gerbv the Decimal Auxiliary+Absolute origin options are both working
> properly for viewing the Gerber files.
> So far I must conclude that if the drill file's X Y numbers do not have a
> decimal dot sign
> viewing in GC-Preview or Gerbv does not work for the Kicads drill files
>
> Next to check is what GerbMerge is doing when making a multiboard panel
>
> Best regards from Holland,
>
> Ellio
>
