Re: gEDA-user: home made pcb final check

[DJ Delorie <dj@xxxxxxxxxxx>]

> I have a layout for a one layer pcb.  I have Pulsar's toner transfer
> paper and white trf foil.  I found a shop in town that has a laser
> printer.  I exported the pcb layout to gerber files.  I then used
> gerbv to print post script files for each gerber file.
> 
> Do I need to print mirrors or inverses of the top and/or the silk
> screen layers?

Ah, the mirroring dilemma.  I suggest you put some text on your layers
that should read correctly when you look at the physical board
(i.e. NOT correctly on the screen, for the "back" layers).

For toner transfer, the print is a mirror of what you want the toner
to be when transferred.  I.e. for your top silk, everything should
read backwards, so that the transferred toner reads forwards.

For solder-side copper (through hole, not smt), the print you see on
the paper should match what you see on the screen when looking at the
top of the board (i.e. through the fr4).  This is the mirror of what
the copper will look like when you flip the board over to look at the
copper side.

For component-side copper (smt, no vias), the print should be mirrored
from the screen, just like the silkscreen.

If you have a new-ish pcb, selecting "auto-mirror" AND "mirror" should
give you the right prints (export via ps, not gerber); that's what I
always used for toner transfer, and still use for photofilm (you
expose ink-down to get crisper edges).  The PS exporter can also
compensate for the laser printer - most shrink/grow the image a
percent or so, and some (like mine) make the dark sections too big by
half a pixel (~0.83 mil).

For toner transfer, don't use "invert".  That's for negative photofilm
like I use.


_______________________________________________
geda-user mailing list
geda-user@xxxxxxxxxxxxxx
http://www.seul.org/cgi-bin/mailman/listinfo/geda-user