You have to set a couple of DRC items to do this, under manufacturing,
'testpoint style'  fill out the size and what side of the board the
testpoints are on, I would set the testpoint grid size to 1mil or else it
won't find many of them (possible bug?)
Then under the same manufacturing tab go to 'testpoint usage' and make sure
testpoint required is checked,  also  the 'allow multiple tespoints on same
net' should be checked if you are using more then 1 testpoint on say power
nets.

After setting up these rules you can now run the 'find and set testpoints'
under the tools menu in the PCB editor, it should highlight all the ones it
finds. (you'll find that the ones it identifies will now have the tespoint
attribute checked when double clicking on the pad)
Once you've done this you can go under cam manager and run a testpoint
report which will list the just found testpoints in an ASCII format file.

Hope this helps, it's a bit of a pain but it does work, I've used it
successfully many times.

Best regards,
Casey Vanderweide.


----- Original Message -----
From: "Tim Fifield" <[EMAIL PROTECTED]>
To: "Protel EDA Forum" <[EMAIL PROTECTED]>
Sent: Thursday, December 13, 2001 12:43 PM
Subject: Re: [PEDA] .TXT File generation


> Thanks Tony, but I'm too busy to test the Pad X&Y theory right now.
>
> (To Group) However, my next problem is that I have a 170 test points on
the
> bottom of my pcb that don't have the "testpoint" box checked and I can't
> seem to globally edit to change them all so I can generate a testpoint
> report. Any thoughts???
>
> Tim
>
> -----Original Message-----
> From: Tony Karavidas [mailto:[EMAIL PROTECTED]]
> Sent: Thursday, December 13, 2001 3:50 PM
> To: Protel EDA Forum
> Subject: Re: [PEDA] .TXT File generation
>
>
> Mid is the "geometric" center of the object. Who knows exactly how they
> compute it and what they take into account???? IIRC, this is what I've
used
> in the past.
>
> I believe the Ref if the "Reference" point assigned when the component was
> built in the library editor.
>
> Pad? Dunno. Maybe this uses "Pad1" as a default.
>
> You could try placing a part or two and telling us. :)
>
> I any case, the assembly house when programming their P&P machines will
> verify and correct for offsets or inaccuracies in these numbers. I've seen
> them do tria runs to figure out if all these numbers are correct.
>
> Tony
>
> > -----Original Message-----
> > From: Tim Fifield [mailto:[EMAIL PROTECTED]]
> > Sent: Thursday, December 13, 2001 10:50 AM
> > To: Protel EDA Forum
> > Subject: Re: [PEDA] .TXT File generation
> >
> >
> > Lloyd,
> >
> > That works great! What's the difference between Mid X&Y, Ref X&Y, and
Pad
> > X&Y?
> >
> > Tim
> >
> > -----Original Message-----
> > From: [EMAIL PROTECTED] [mailto:[EMAIL PROTECTED]]
> > Sent: Thursday, December 13, 2001 1:51 PM
> > To: Protel EDA Forum
> > Subject: Re: [PEDA] .TXT File generation
> >
> >
> > Tim,
> > Under the CAM outputs, you have choices to generate gerbers, NC Drill,
Pik
> > and Place etc. This the the section that you wish to use. Just choose to
> > generate Pick and Place which gives you two files a *.txt and a *.csv
file
> > of the X/Y co-ordinates for the components. Also choose to generate a
> > Testpoint report, which will output the X/Y co-ordinates of all your
> > testpoints, provided that you have set all the testpoints as such.
Meaning
> > checked the testpoint box under the pad attributes menu.
> >
> > Regards,
> > Lloyd
> >
> > -----Original Message-----
> > From: Tim Fifield [mailto:[EMAIL PROTECTED]]
> > Sent: Thursday, December 13, 2001 9:41 AM
> > To: Protel EDA Form
> > Subject: [PEDA] .TXT File generation
> >
> >
> > My production facility (not pcb house) is asking for the following:
> >
> > X/Y coordinates of components .TXT file
> > X/Y coordinates of test points/pads in .TXT file
> >
> > Is it possible to generate those files in P99SE? If so, how?
> >
> > Tim
> >
>

* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
* To post a message: mailto:[EMAIL PROTECTED]
*
* To leave this list visit:
* http://www.techservinc.com/protelusers/leave.html
*
* Contact the list manager:
* mailto:[EMAIL PROTECTED]
*
* Forum Guidelines Rules:
* http://www.techservinc.com/protelusers/forumrules.html
*
* Browse or Search previous postings:
* http://www.mail-archive.com/proteledaforum@techservinc.com
* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *

Reply via email to