Search function

kwsauter · ‎Sep 09, 2009

PDMLink is telling me it can't remove prt0001.prt from the workspace
because it's parent has to be removed from the workspace. When I look
at the parent assembly, and the parent drawing, I can't even find a
prt0001.prt in the model structure. The part is actually a pin from a
connector I imported, and I have already renamed the connector body and
pins so they have real names. I thought I could use the search function
to look through the assembly and drawing to find out where the part is,
but as usual with proe logic, 'part' is grayed out--the very thing I
want to use the search function for. How do I find this thing when It's
not in the model tree and PDMLink is pointing to the assembly as the
parent?

Ken Sauter
DRS Reconnaissance Surveillance and Target Acquisition
Infrared Technologies Division
PO Box 740188
Dallas, TX 75374
469-221-5430
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rapidoconsultin · ‎Sep 09, 2009

Check your drawing for notes or other items attached to the prt0001. Next save the drawing again, even if you have no changes other than an update the sheets. Many times the drawing still thinks it needs the model even though it has been removed from an assembly. Views can even hold on to model references until the next save. These are the things I look for first when dealing with PDMlink issues.

Eric Mills

Design and Project manager

http://www.rapidoconsulting.com

eric.mills@rapidoconsulting.com

kwsauter · ‎Sep 09, 2009

I checked the global reference viewer in the assembly, because it wasn't
available in the drawing (which PDMLink is referencing as the parent),
and there is nary a prt0001.prt to be found. It ain't there. When I
check the information link in PDMLink, it lists the part, shows it in
Productview, and just says it's a part without showing any parents. Yet
somehow PDMLink thinks it is attached to a drawing. There are no notes
that reference the part in the drawing, no '¶meter' notes anywhere,
or anything I can tell that references the part. The repeat region
calls out the connector assembly that used to have that part in it, but
that assembly has been modified to remove the part or rename it to
something else. The only thing I can figure is that Proe, in its unique
kind of logic, thinks the part is still part of the connector assembly
because it began as part of the connector assembly. This is the kind of
thing that makes me want to tear my hair out.

Ken Sauter
DRS Reconnaissance Surveillance and Target Acquisition
Infrared Technologies Division
PO Box 740188
Dallas, TX 75374
469-221-5430
- <">mailto:->

NOTICE: This e-mail transmission (and/or the attachments accompanying
it) may contain confidential or proprietary information belonging to DRS
Technologies or the sender. The information is only for the use of the
intended recipient. If you are not the intended recipient you are hereby
notified that any disclosure, copying, distribution or the taking of any
action in reliance on the contents of this information is strictly
prohibited. Any unauthorized interception of this transmission is
illegal under the law. If you have received this transmission in error,
please promptly notify the sender by reply e-mail, and then destroy all
copies of the transmission.

"This (document/presentation) may contain technical data as defined in
the International Traffic In Arms Regulations (ITAR) 22 CFR 120.10.
Export of this material is restricted by the Arms Export Control Act (22
U.S.C. 2751 et seq.) and may not be exported to foreign persons without
prior written approval from the U.S. Department of State."

gkemner · ‎Sep 09, 2009

We have been going through this quite a bit as we try to load legacy
data and experience phantom drawing references to parts and assemblies
that are no longer used in the drawing.

Here is how we have been fixing these issues, it is a pain but it has
been working.

1. Do a Pro/E File Backup of your drawing to a folder on your
computer hard drive outside of PDMlink. That should make a copy of the
drawing and all associated parts. Go to that folder and verify that has
occurred. If prt0001 is in that folder delete it since you want to get
rid of it.

2. Then in your workspace remove your drawing, the prt0001 file
and any other related items needed to get them removed from the
workspace.

3. Now go back to the folder where you "backed up" the drawing and
files. In Pro/E set this config option (you may have to type it in):
cleanup_drawing_dependencies yes

4. Restart Pro/E with that config option set, just to make sure it
takes effect.

5. Now in Pro/E open your drawing from that hard drive folder.

6. You should get a box that pops up listing missing drawing
references and it should list PRT0001.

7. Choose the REMOVE option from the box and say ok to any warning
it may present you with.

8. Save your drawing and the files should now be back in your
workspace once again but this time without prt0001.

I am using WF 3.0 M150 and Intralink 9.0 M030 but it should work
similarly on other builds or versions.

There needs to be a way to remove the references from a drawing other
than just when you open it. Something like a global reference viewer in
drawing mode.

Hope that helps, let me know if you have any questions.

lylebeidler · ‎Sep 09, 2009

Try replacing the drawing format on the drawing. Sometimes that eliminates
those relationships in Ilink, so it may work in PDMLink, too.

If possible, also remove & recreate your BOM tables on the drawing.

--

Lyle Beidler
MGS Inc
178 Muddy Creek Church Rd
Denver PA 17517
717-336-7528
Fax 717-336-0514
<">mailto:-> -
<">http://www.mgsincorporated.com>

KarenMoore · ‎Sep 10, 2009

In Reply to Greg Kemner:

ARE YOU ADDINGcleanup_drawing_dependencies yes TO EVERYONE'S CONFIG.PRO AS A DEFAULT? LOOKS LIKE IT IS A HIDDEN OPTION (WF4 M040)
Karen Moore
Honeywell, FM&T
We have been going through this quite a bit as we try to load legacy
data and experience phantom drawing references to parts and assemblies
that are no longer used in the drawing.

Here is how we have been fixing these issues, it is a pain but it has
been working.

1. Do a Pro/E File Backup of your drawing to a folder on your
computer hard drive outside of PDMlink. That should make a copy of the
drawing and all associated parts. Go to that folder and verify that has
occurred. If prt0001 is in that folder delete it since you want to get
rid of it.

2. Then in your workspace remove your drawing, the prt0001 file
and any other related items needed to get them removed from the
workspace.

3. Now go back to the folder where you "backed up" the drawing and
files. In Pro/E set this config option (you may have to type it in):
cleanup_drawing_dependencies yes

4. Restart Pro/E with that config option set, just to make sure it
takes effect.

5. Now in Pro/E open your drawing from that hard drive folder.

6. You should get a box that pops up listing missing drawing
references and it should list PRT0001.

7. Choose the REMOVE option from the box and say ok to any warning
it may present you with.

8. Save your drawing and the files should now be back in your
workspace once again but this time without prt0001.

I am using WF 3.0 M150 and Intralink 9.0 M030 but it should work
similarly on other builds or versions.

There needs to be a way to remove the references from a drawing other
than just when you open it. Something like a global reference viewer in
drawing mode.

Hope that helps, let me know if you have any questions.

RandyJones · ‎Sep 10, 2009

ARE YOU ADDINGcleanup_drawing_dependencies yes TO EVERYONE'S CONFIG.PRO AS A DEFAULT? LOOKS LIKE IT IS A HIDDEN OPTION (WF4 M040)
Karen Moore
Honeywell, FM&T

Permanently adding cleanup_drawing_dependencies (or cleanup_layout_dependencies) = yes is not a PTC recommended practice. See the following tpi's:

https://www.ptc.com/appserver/cs/view/solution.jsp?n=114763

https://www.ptc.com/appserver/cs/view/solution.jsp?n=134691

https://www.ptc.com/appserver/cs/view/solution.jsp?n=137198