Re: gEDA-user: Moving positioning diamond in PCB

[kai-martin knaak <kmk@xxxxxxxxxxxxxxx>]

blueeagle2@xxxxxxxxx wrote:

> I was wondering if someone could tell me how to move the 
> positioning diamond in PCB or how to move the the foot
> print itself so it is centered over the diamond. 

1) open a new layout

2) open the footprint chooser (accel key: [i])

3) select the footprint to be modifies

4) from the buffer menu do break_buffer_elements_to_pieces

5) click somewhere on the canvas to place the pieces

6) select all pieces by dragging with the mouse

7) position the mouse cursor where the diamond shall be

8) cut the pieces to buffer (accel key [ctrl-x])

9) from the buffer menu do convert_buffer_to_element

10) click somewhere on the canvas to place the footprint. It
should have the diamond on the right position.

11) regenerate the information of the footprint that got lost
during the process: 
   a) pin and pad numbers --> [n] on pins and pads
   b) square flag --> [q] on pins and pads
   c) proper solder mask clearance
      --> draw a rectangle in copper over the footprint
      --> activate solder mask
      --> go over every pad/pin and type [ctrl-k] twice. 
        This will decrement the size of the hole in the solder mask
      --> deactivate the solder mask
   d) position of the text associated with the footprint 
      --> [n] somewhere inside the footprint where no pins or pads are
      --> type an arbitrary string in the dialog --> click ok
      --> move the string to the desired posion

12) select the footprint (click on footprint)

13) cut the footprint to buffer ([ctrl-x]). It doesn't matter where
 you put the mouse cursor at this step.

14) from the buffer menu: save_buffer to_file

Yes, this is tedious. The reason for it is the lack of a real 
footprint editing mode in pcb.

--<)kaimartin(>---
-- 
Kai-Martin Knaak
Ãffentlicher PGP-SchlÃssel:
http://pgp.mit.edu:11371/pks/lookup?op=get&search=0x6C0B9F53



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