Re: gEDA-user: Increment drill size on 344 vias
John Coppens wrote:
The pcb commands will take only vias from the selected set and change
them.
That said, it _would_ be very helpful to have something else available
except the +/- 10 mils fixed step (not only for holes, also for track
widths etc)
I'm not too experienced a programmer, but I'm willing to help out...
John
[jg]
We don't have easy to user program dialogs yet, but you should do the lesstif
pcb compilation, so you can assign your own bindings to keys.
You can still put commands in the command window as is, and copy and paste them
from a list you keep ready while doing layout.
The key binding code for what you ask looks like this for the ctrlv key as an
example:
{decrease line 4 mils a={Ctrl-l 4 CtrlKeysl4}
ChangeSize(SelectedLines, -4,mil) }
{decrease line 6 mils a={Ctrl-l 6 CtrlKeysl4}
ChangeSize(SelectedLines, -6,mil) }
{decrease line 3 mils a={Ctrl-l 3 CtrlKeysl3}
ChangeSize(SelectedLines, -3,mil) }
Once you have these in your local pcb-menu.res file, (and are using the lesstif
compilation of pcb), you can press ctrlv followed by the second key press to
get the amount. (The second key doesn't have to be integer amounts, I just set
it up this way)
An example for increasing Vias:
{incr via/drill 4 mils a={Ctrl-V 4 CtrlKeysv4} Atomic(Save)
ChangeSize(SelectedVias,+4,mil) Atomic(Restore) ChangeDrillSize(SelectedVias,
+4, mil) Atomic(Block)}
Increasing and decreasing need separate first key press binding for this scheme
of doing things.
It would be nice to have some general guile/scheme/LISP/Skill way to hook into
the core functions of pcb code, and work toward all of that being able to act on
any hierarchical piece of layout. That's how Cadence chip design tools work.
Glad Dan is thinking along those lines.
If we made it work that way, maybe someone would eventually write in the gnetman
database engine so the size of layout that could be handled would be huge enough
for chips as well as boards. That would make sense once we made the file-based
functioning of pcb modeled after Cadence layout.
John Griessen
___
geda-user mailing list
geda-user@moria.seul.org
http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Increment drill size on 344 vias
The easiest way is with a perl/python script. ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Increment drill size on 344 vias
David Carr wrote: Quick question: I have a board with 344 vias that I'd like to increase in size from 20 mils to 24 mils. Is there a way to do this semi-automatically in PCB? There are other vias of different sizes on the board. Maybe 'find and replace' over the section of your pcb with the vias. I've done this before and it's pretty painless. You could paste that section into another file and 'replace all'. or something. Phil ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Increment drill size on 344 vias
David Carr wrote: Quick question: I have a board with 344 vias that I'd like to increase in size from 20 mils to 24 mils. Select them and any other non-via objects, but not the other size vias somehow. Maybe multiple area selects or one big one or select all...depending... In the pcb command window give the command ChangeDrillSize(SelectedVias, 24, mil) and if you want to make the annulus bigger too... ChangeSize(SelectedVias,44,mil) The pcb commands will take only vias from the selected set and change them. John Griessen ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Increment drill size on 344 vias
On Wed, 15 Nov 2006 19:03:57 -0600 John Griessen [EMAIL PROTECTED] wrote: David Carr wrote: Quick question: I have a board with 344 vias that I'd like to increase in size from 20 mils to 24 mils. Select them and any other non-via objects, but not the other size vias somehow. Maybe multiple area selects or one big one or select all...depending... In the pcb command window give the command ChangeDrillSize (SelectedVias, 24, mil) and if you want to make the annulus bigger too... ChangeSize(SelectedVias,44,mil) The pcb commands will take only vias from the selected set and change them. That said, it _would_ be very helpful to have something else available except the +/- 10 mils fixed step (not only for holes, also for track widths etc). I would gladly sacrifice the +/- 10 options for a simple dialog which asks for a new size. It doesn't make much sense to decrease a 12 mil track by 10 mils anyway. I'm not too experienced a programmer, but I'm willing to help out... John ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Increment drill size on 344 vias
John Griessen wrote: David Carr wrote: Quick question: I have a board with 344 vias that I'd like to increase in size from 20 mils to 24 mils. Select them and any other non-via objects, but not the other size vias somehow. Maybe multiple area selects or one big one or select all...depending... In the pcb command window give the command ChangeDrillSize(SelectedVias, 24, mil) and if you want to make the annulus bigger too... ChangeSize(SelectedVias,44,mil) The pcb commands will take only vias from the selected set and change them. This all makes me wish more and more for a more powerful user programming capability in pcb and also gschem. Despite the pain which skill programming can be, this sort of thing would be trivial in cadence. It is fairly easy to iterate over a design and find instances of a certain type (a via in layout, an instance of a particular cell, whatever) and filter based on some property and then change things. Granted, I'm more likely to want this programming capability when dealing with hundreds of pages of schematics. Then again, 344 vias is not a small number. -Dan ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
