On Tue, 2008-05-06 at 11:05 +0100, Patrick Dupre wrote:> Hello,> > How can I change the pine size with pcb ?
The diameter of a through hole component or via's drill size?
Two ways:
Mouse over it, then:
Alt+S (Hole bigger) Alt+Shift+S (Hole smaller) S (Pad bigger) Shift + S (Pad smaller)
Or, if you have lots to do at once, select them, then:
"Window" Menu -> "Command Entry" (The keyboard shortcut for this windowis just ":"
Then type in the command window, something like:
changedrillsize(selectedpins, 90, mil)changedrillsize(selectedpins, 1, mm)changedrillsize(selectedvias, 1, mil)
Full syntax:
changedrillsize(target, size, units) target = {selectedpins | selectedvias | selectedobjects | selected}
For changing the pad size:
changesize(target, size, units) target = {selectedlines | selectedpins | selectedvias | selectedpads | selectedtexts | selectednames |selectedelements | selected}
You might also be interested in:
changeclearsize(target, size, units) target = {selectedpins | selectedpads | selectedvias | selectedlines | selectedarcs | selectedobjects | selected} Changes the clearance of objects.
If you set "File" menu -> "Preferences" -> Enables: "Use separate window for command entry",there will be a drop down box with some syntax hints like these. If the option is un-ticked,command entry will appear in the status bar underneath the schematic.
If I cannot change from pcb, do I need to change the footprint ?
You could do it that way, assuming you wanted to place it multipletimes. For footprints you generate yourself, this is a good idea.
If yes Do I have to edit the .fp file ?
Yes, or you could open the .fp file in PCB. You'll need to cut theelement into the buffer, then use "Buffer" menu -> "Save buffer elementsto file".
If yes, can I get more information ?
It depends on your distribution and exactly how you installed PCB, butthere is a .pdf with some documentation, perhapsin /usr/share/pcb, /usr/share/doc/pcb, /usr/share/doc/pcb-common
Then, do I need to generate a png file ? if yes how ?
You can generate a png, but its probably not what you want forproduction (sending to a fabricator).
"File" menu -> "Export layout..."
Then choose what you want:
"ps" for postscript (printing of the layers which you could turn intoa .pdf (with "ps2pdf"), for use in documentation, a UV exposure ortoner transfer process.
"gerber" for sending to a board fabricator
"png" for a graphics export for embedding in a document (for example).
Hope that helps,
(PS. Nice to see another UK gEDA user join our ranks).
Best wishes,
-- Peter Clifton
Electrical Engineering Division,Engineering Department,University of Cambridge,9, JJ Thomson Avenue,CambridgeCB3 0FA
Tel: +44 (0)7729 980173 - (No signal in the lab!)
_______________________________________________geda-user mailing listgeda-user@xxxxxxxxxxxxxxxxxx://www.seul.org/cgi-bin/mailman/listinfo/geda-user