gEDA-dev: PCB - XY values of centrioid in BOM/DXF exproter (wasgEDA-user: PCB Element for a Molex 71661-2068?)

[Timmerman, Bert]

Hi Dan,

Reading your reply I can see that my dyslexical typing habbit is not yet
under control  ;-)


On second thought: only double symmetrical packages are _probably_ in
the clear.

One could argue that a single symmetrical package, for instance a
TO-220, which has symmetry across the (local) Y-axis and not across the
(local) X-axis, is definitely not in the clear.

The X-value of the calculated centroid of pins/pads will be correct with
respect to the X-value of the center of gravity, while the Y-value of
the center of gravity may differ from the Y-value of the calculated
centroid of pins/pads.


I see two options for the DXF exporter I'm writing:

1)

Use the mark X,Y-value pair to insert 3D models of packages in an
assembly 3D model, as the mark X,Y-value is _probably_ willingly chosen
by the creator of the footprint, and _maybe_ checked and correct (a lot
of assumptions here).

This would require some code changes in a not yet released HID, and
would not break any footprints in the real world.

Or

2)

Stay with the calculated centroid X,Y values following the calculation
method in the BOM exporter.

I know and you know, there is a _possible_ problem in actually using the
centroid X,Y-values in a real life "pick-and-place" situation.


My preference is with option 1.

To get this right for the BOM exporter is another matter, for I have my
focus on the DXF exporter.

About a checkbox in the BOM exporter, I guess I can allways not send in
a patch, and let the user decide for himself/herself wether or not to
delete the file, I can live with the situation as it is.

Kind regards,

Bert Timmerman.

BTW: For now I use 0.0 as the Z-value of the insertion point of the 3D
model of the packages.


-----Original Message-----
From: geda-dev-bounces at moria.seul.org
[mailto:geda-dev-bounces at moria.seul.org] On Behalf Of Dan McMahill
Sent: Thursday, March 08, 2007 2:03 PM
To: gEDA developer mailing list
Subject: Re: gEDA-dev: PCB - XY values of centrioid in BOM/DXF exproter
(wasgEDA-user: PCB Element for a Molex 71661-2068?)

Bert Timmerman wrote:
> Hi Dan and all,
> 
> For the DXF exporter I'm currently coding, I use the centroid
X,Y-value (as
> in the BOM exporter) as the insertion point for the 3D model of the
package
> involved, in a mechanical CAD package (for example AutoCAD).
> 
> For symmetrical and double symmetrical packages (> 99% of all
packages) this
> should be no issue as it coincides with the center of gravity.
> 
> The problem lies in assymetrical [PGA, BGA, SIL, TO, connectors, ...]
> packages where the centroid (a calculated average X,Y-values of the
actual
> existing pins/pads on the package) does not coincide with the center
of
> gravity of the package (basically for X and Y values, since pcb has no
> notion of Z values).
> 
> This asymmetricallity arises from pins/pads missing in the pattern, or
shape
> of the connector (pin/pad pattern).
> 
> IMO it would be a good practice to use the center of gravity as a
> mark/insertion point for pcb footprints/3D models.

yes.

> Now, there are a lot of footprints out there, and we do not want to
break
> _everything_.
> 
> So, this [should, could] be solved by using the mark X,Y-values in the
DXF
> exporter and _not_ use the calculated centroid X,Y-value.

assuming that all the footprints are fixed up.  When I made the 
decision, it wasn't clear how many footprints actually put the mark in 
the right place.

> However, a question that comes to mind is whether anyone is actually
using
> the XY file for "pick and place" of components ?
> Positive feedback ? (from list members who actually use this feature).

good question!  I asked for feedback when I added (since it had been 
asked for) but didn't really get any.  I will note that gerbv (in cvs 
head) can read PCB XY files.

> 
> If not, it's not lean to _allways_ provide a centroid file, that is,
there
> probably should be a checkbox to be ticked in the BOM exporter if
someone
> _really_ needs this file (default set to unticked).
> 
> I think I can send a patch if needed.

I guess I'd rather see the default be checked just to avoid breaking any

scripts or makefiles that users may have aleady.  I'm not sure what the 
harm is though of always generating the file.  I'm sure many users don't

use some of the layers which come out of the gerber export either.  For 
example solder paste stencil is probably not used by most hobby or very 
low volume users.

-Dan




_______________________________________________
geda-dev mailing list
geda-dev at moria.seul.org
http://www.seul.org/cgi-bin/mailman/listinfo/geda-dev