Re: gEDA-user: Question about PCB

[sdb@xxxxxxxxxx (Stuart Brorson)]

Hi --

> The other question belongs to producing new Footprints - in SMD - in the 
> case when I have to define pads with strange withs and  distances.
> If I want to generate a footprint - the old way should not be used - and 
> the new way is bounded to the grid of the PCB tool.
> So was the question: Is it possible to place elements directliy as x/y 
> coordinates -parhaps als manual change in text-file?

If I understand you correctly, you want total control over all aspects
of your footprint and PCB prevents you because you are locked to
drawing along the grind points.  Right? 

If so, then your best method is to first draw the footprint
approximately, and then save it out as an "element".  The edit the
footprint using a text editor.  Here is a step-by-step method:

1.  Draw your footprint in PCB.  On the component layer use lines to
create SMT pads, and vias for through-hole pins.  Then change to the
silk layer and draw a coponent boundary.

2.  Select all your components using the select tool.

3.  In the top menu, do "buffer -> copy selection to buffer"  You will
be prompted for the element's location.  The point you select will
later become the reference point for the part (mark).  Just click on
the point you want to make the mark.  I usually select the center of
pin 1, or a point of maximum symmetry depending upon the footprint's
geometry.  

4.  Next do "buffer -> convert buffer to element".   Don't worry that
a ghost of your selected component will follow the cursor around.

5.  Do "buffer -> save buffer elements to file".  Browse around and
save the footprint into your project directory under the footprint name
you wish to use.

6.  Leave PCB and edit the new footprint using Emacs or vi.  At this
stage, you have a rough draft of the footprint and your goal is to
make it perfect by changing the widths, heights and other sizes to
your desired values.  You can change all footprint parameters using
the text editor if you know what the parameters are.  A doc describing
the format of newlib footprints is here:  

http://www.brorson.com/gEDA/

It's the last item in the first list.

Finally, if you are just looking for a standard footprint, why not
just download one of John Luciani's?  He has a large collection at:

http://www.luciani.org/geda/pcb-footprint-list.html

Stuart