Newbie -- How to properly associate DNI or Do Not Populate to component

[bbruce888]

I have searched for quite awhile and I cannot seem to find the answer to this
seemingly easy question:

How should I correctly associate a DNI or DNP (Do Not Populate) attribute to
a component so that the Pick & Place file will know not to include that
component in the final output BOM?

Thanks in advance.

[Peter Clifton]

Post by bbruce888
I have searched for quite awhile and I cannot seem to find the answer to this
How should I correctly associate a DNI or DNP (Do Not Populate) attribute to
a component so that the Pick & Place file will know not to include that
component in the final output BOM?

I'm not sure where you're looking here. You can make a component
invisible to gEDA's netlisting by marking with the "graphical=1"
attribute. This means no trace of it ends up in your PCB board either.

OTOH, if you're just looking for a "NO FIT" type instruction, where I
_do_ want the footprint on the PCB board - just empty, I typically just
add the attribute "value=NO FIT" to that component. The assembly house I
use seem to understand what I mean, and didn't complain that it appeared
in the XY file used for programing the pick'n'place machine.

Best regards,
--
Peter Clifton

Electrical Engineering Division,
Engineering Department,
University of Cambridge,
9, JJ Thomson Avenue,
Cambridge
CB3 0FA

Tel: [phone] - (No signal in the lab!)

[Duncan Drennan]

Post by Peter Clifton
OTOH, if you're just looking for a "NO FIT" type instruction, where I
_do_ want the footprint on the PCB board - just empty, I typically just
add the attribute "value=NO FIT" to that component. The assembly house I
use seem to understand what I mean, and didn't complain that it appeared
in the XY file used for programing the pick'n'place machine.

Or you can just set "value=NO FIT" (or DNP, DNI, etc.) and delete the
relevant lines from the XY file by searching for that term....or write
a script which post-processes the XY file and removes the DNP lines.

[joe tarantino]

I took a different approach which is a little more work. I added a field to
my symbols called "loadstatus" which I mark for "no load", "through hole",
or blank. Blank is the default, and means a SMT part that is loaded. It's
not hard to use gnetlist -g bom2 (if I remember correctly) to slice out this
field on your report to the board stuffer. Sort the resulting list to put
the no-load parts at the bottom so that they're easy to ignore. I don't
like the idea of stepping on the value field since then the schematic loses
it's knowledge of what you might want to load at a later date.

Be sure to include this field in your "attib" file so gnetlist grabs it as
desired.

Joe T

On Mon, Oct 20, 2008 at 10:26 PM, Duncan Drennan

Post by Duncan Drennan

Post by Peter Clifton
OTOH, if you're just looking for a "NO FIT" type instruction, where I
_do_ want the footprint on the PCB board - just empty, I typically just
add the attribute "value=NO FIT" to that component. The assembly house I
use seem to understand what I mean, and didn't complain that it appeared
in the XY file used for programing the pick'n'place machine.

Or you can just set "value=NO FIT" (or DNP, DNI, etc.) and delete the
relevant lines from the XY file by searching for that term....or write
a script which post-processes the XY file and removes the DNP lines.
_______________________________________________
geda-user mailing list
http://www.seul.org/cgi-bin/mailman/listinfo/geda-user

[Duncan Drennan]

Post by joe tarantino
I took a different approach which is a little more work. I added a
field to my symbols called "loadstatus" which I mark for "no load",
"through hole", or blank. Blank is the default, and means a SMT part
that is loaded. It's not hard to use gnetlist -g bom2 (if I remember
correctly) to slice out this field on your report to the board
stuffer. Sort the resulting list to put the no-load parts at the
bottom so that they're easy to ignore. I don't like the idea of
stepping on the value field since then the schematic loses it's
knowledge of what you might want to load at a later date.
Be sure to include this field in your "attib" file so gnetlist grabs
it as desired.
Joe T

That is fine for generating BOMs, but the Pick & Place files are
generated from PCB, which only has the RefDes, Description (footprint
name), and Value available. Placing a DNP in the value field will at
least propagate through to the PCB layout.

One the point of info available in PCB, is it possible to pass any
other attributes across when using gsch2pcb, or substitute other
attributes for the Description or Value? If you could pass a different
value for the description, like DNP or a stock code that could be
useful.