kicad-developers team mailing list archive

[Marco Hess <marco.hess@xxxxxxxxxxxxxx>]

One of the reasons I did this patch was in an attempt to deal with some 
of the PCB manufacturers I am using. If I send them the default named 
KiCad files they did not understand the Gerbers at all. They basically 
complained that the ZIP I send them only contained a drill file.

I found that many of them use a package called CAM350, I had a bit of a 
play with a trial version of that package and found that on importing a 
design it mainly looks at the file extensions used on the gerbers to 
assign the right gerber to the right layer. It uses a number of 
'profiles' that matched extensions used with the typical more popular 
packages and even has some auto-scan feature to look for the best match. 
Unfortunately the default KiCad naming was not one of the profiles they 
had. If the extensions could not be matched to anything, CAM350 was 
unable to assign the gerber to the right layer and assigned the gerber 
to a default 'Graphical' layer and the manufacturing check bailed out 
with an error.

When I renamed the gerbers with either the Protel extensions or with the 
default extensions used for Orcad, I had more success with these PCB 
manufacturers accepting my ZIP package :-).

Not sure what others experiences are in this area. I am not on KiCad 
that long, I previously mainly used Protel 99 and some Altium and for 
that I could just send the PCB file without having to worry about 
individual Gerbers (although I found it annoying that often I had holes 
in my board as they interpreted the KeepOut layers as board outline in 
addition to the normal board outline.

I personally hate dialog boxes with too many options. I like when things 
can be locked down and scripted where possible so that I can generate 
gerbers the same way each and every time I produce a board.

A such I feel that KiCad could do with an extension in the manufacturing 
output where you can select a a predefined 'Profile' that sets the DRC 
rules for a particular manufacturer (or personal defaults) but also 
configure the gerber file naming rules. Over time there could be a 
collection of such manufacturer profiles files that can be included to 
help newer users to generate the right manufacturing pack straight of 
the bat.

I might have a look into that at some time when things settled down a 
bit and I got my other changes submitted :-)

Marco



On 25/06/2015 9:54 PM, Lorenzo Marcantonio wrote:
> On Thu, Jun 25, 2015 at 10:03:31PM +1000, Mitch Davis wrote:
> > I think the name Protel is there to indicate the historical origin,
> > rather than be the name of a current package.  (Do factories still use
> Exactly. In the past the dialog said 'proper' but I assumed it was
> a typo since they were the extension protel used; remember those days
> where 8+3 filename times, so you had to be creative :P
>
> AFAIK Altium has a configurable CAM processor so it wouldn't be correct
> to call them 'altium extension' (unless it still use these by default:D)
>
> > Gerber plotters?  Do factories still use Excellon dill machines?)
> It was something like Gerber->Barco->Ucamco (at least that's what
> wikipedia says...), so you could say that gerber plotter are *still* in
> use. Well, a little different since they are raster machine these
> days...
>
> No idea if there are many other photoplotter manufacturer arounds;
> however it seems that everyone eventually standardized on RS274X (i.e.
> gerber). At least, it seems that *everyone* uses the same preprocessor, at
> least here in italy (genesis)
>
> As for the drill tapes, excellon is still in business so I'd say that
> even for these, yes, they still use them :D there are other format in
> use however (Sieb&Mayer, for example).
>
> Pick and place and AOI however are a whole hell of custom file formats,
> don't worry :D