Mail Archives: geda-user/2014/06/11/21:36:34
On Wed, Jun 11, 2014 at 07:56:16PM -0400, Dave McGuire wrote:
> On 06/11/2014 03:03 AM, Gabriel Paubert wrote:
> > On Tue, Jun 10, 2014 at 08:26:37PM -0400, DJ Delorie wrote:
> >>
> >> two options:
> >>
> >> 1. Turn the waveguide into an element, so you can edit the soldermask
> >> big enough.
> >>
> >> 2. Create a new layer called "extra top soldermask" that has the edits
> >> you want, and merge the gerbers in post-processing.
> >
> > Solution 2 is what I've been doing for years. Merging the photoplotter
> > files manually is relatively easy (even if having tools for this would
> > be nice).
>
> Got it...Thanks for the suggestions, guys.
>
> Gabriel, can you tell me how you do the gerber merge, and what tool(s)
> you use?
cat and emacs :-)
cat to concatenate the two files to a new one (always keep the originals!).
Then under a text editor (I use emacs since it keeps the DOS line breaks)):
- eliminate the M02 at the end of the first file,
- move the header which is just after this removed item to after
the header of the first file
- merge the headers by hand, this is easy since right now pcb allocates
non overlapping aperture ranges for each file. You must remove the
duplicate %MO and %FS parameter lines, which must be identical,
(same for %IP if it were present). The other parameters are less critical
but I prefer to keep the %LN from the first file.
- for the comment (G04) lines, do what you want, keeping in mind that
only printable ASCII characters are allowed with the exception of % and *.
That's about all, but I may have forgotten something.
Then I always check the results under gerbv.
> Can gerbv do this?
Not as far as I know, and last time I tried, saving under gerbv used
imperial units (even if you feed it exclusively metric files) and
lost precision in the process. With these caveats, I believe that the
only thing that gerbv allows is to delete items.
Gabriel
- Raw text -