[Author Prev][Author Next][Thread Prev][Thread Next][Author Index][Thread Index]
Re: gEDA-user: How to make vias have a solder stop mask?
On Tue, 24 Jul 2007 21:27:14 +0200, lynx.abraxas-KuiJ5kEpwI6ELgA04lAiVw
wrote:
> stop mask was on the copper that the vias weren't in the stop mask How
> can I make them clear the mask?
For individual vias:
1) Position the mouse above the via (mouse cursor will
change in recent versions of pcb)
2) Type "k" several times until soldermask clearance exceeds the
diameter of the via pad. Every strike of the key will increase
the clearance by 2 mil.
For groups of vias:
1) select the all the vias you want to clear from soldermask.
You may switch off all the other layers to conveniently collect
exclusively the vias.
2) Type "Ctrl-k" several times.
The command interface provides more control over the actual size of the
clearance. Type ":" to get the command line window, then type:
ChangeClearSize(SelectedVias, <delta>)
where <delta> is given in 1/100 of a mil. Thus 3000 corresponds to 30 mil.
Simple integers for <delta> will set the clearance to this value. If the
value is preceded by a minus "-" or a plus "+" clearance be decreased or
increased. This also works with SelectedPins, SelectedPads, SelectedLines,
SelectedArcs or even SelectedObjects.
See the pcb reference for definitive information on commands. e.g:
http://pcb.sourceforge.net/pcb-cvs/pcb.html#ChangeClearSize%20Action
---<(kaimartin)>---
PS: I just added the details above to the wiki:
http://geda.seul.org/wiki/geda:pcb_tips#how_do_i_change_the_soldermask_clearance_around_a_hole_via
--
Kai-Martin Knaak tel: +49-511-762-2895
Universität Hannover, Inst. für Quantenoptik fax: +49-511-762-2211
Welfengarten 1, 30167 Hannover http://www.iqo.uni-hannover.de
GPG key: http://pgp.mit.edu:11371/pks/lookup?search=Knaak+kmk&op=get
_______________________________________________
geda-user mailing list
geda-user@xxxxxxxxxxxxxx
http://www.seul.org/cgi-bin/mailman/listinfo/geda-user