Re: gEDA-user: pine size

[Peter Clifton <pcjc2@xxxxxxxxx>]

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 window
is 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 multiple
times. 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 the
element into the buffer, then use "Buffer" menu -> "Save buffer elements
to file".

> If yes, can I get more information ?

It depends on your distribution and exactly how you installed PCB, but
there is a .pdf with some documentation, perhaps
in /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 for
production (sending to a fabricator).

"File" menu -> "Export layout..."

Then choose what you want:

"ps" for postscript (printing of the layers which you could turn into
a .pdf (with "ps2pdf"), for use in documentation, a UV exposure or
toner 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,
Cambridge
CB3 0FA

Tel: +44 (0)7729 980173 - (No signal in the lab!)



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