Published Geometry

[mpeterson]

Hello group,

I have a question in regard to using published geometry and the "master model" techinque. I typically use a master model to generate all main part surfaces for an assembly and then publish that and other referencesI will need in the parts like datum planes, datum axis, etc. My question is pertaining to making new versions of the design and retaining the original. How can a new master model be created that also includes copying all the downstream parts to reference it? What I currently do is save a copy of the master and also save a copy of the downstream parts that still are dependent on the original master. Then I redefine the published geometry to reference the new master part and Pub Geom, but then all feature and surface associationsare lostand the new part file must be rerouted or redefined feature by feature for all failed features. Is there a better way to do this? Please advise if you have any better methods or techniques.

Mark A, Peterson

Senior Product Engineer

Igloo

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[mpeterson]

Thanks to Dorian F. for reminding me of the method below.

For now I am opening up the assembly, master part file and drawing and then backing them up into a total seperate directory. After clearing memory and changing to that new directory I am renaming all files. Once that is done I am moving the all the parts back to the original design directory.Currently we are not running any PDM software, so doing this old school is my better method so far. If anyone has other better, more efficient solutions please advise.

Thanks,
Mark A. Peterson
Sr Product Engineer
Igloo

[ptc-1932745]

One 'shortcut' that may work, is at the top-level assembly, do a save-as
and rename the assembly. Pro-E will bring up a list of all of the
components used in the assembly and allow you to rename, or reuse the
existing part(s) in the new assembly. Rename the parts as needed, and
(if the parts have the same file name as the drawings) the new structure
and the new drawings will be created by Pro-E.



Another useful thing I have found today is the following:



1 Copy an existing part to your local working directory.

2 Make changes as needed.

3 When ready, do a 'save-as' back to the 'public' directory

Pro-E will copy the file and update the file version number as needed.



This works without using a PDM system.



Christopher Gosnell

TRIGON INC.
FPD Company
124 Hidden Valley Road
McMurray, PA 15317
PH: 724.941.5540
FX: 724.941.8322
www.fpdinc.com

[mpeterson]

I tried the Save As method of the assembly, but there was no line prompting me to reuse or rename the master part file in the renaming dialog box, so thus I did a backup of both. I don't know if there could be a config setting that influences this or not.

Mark P

[ptc-1932745]

I just rechecked this morning with the following:



WF4 M110



1) Open Assembly

2) Choose File | Save a Copy…

3) File dialog opens, give assembly a new name in the ‘New Name’ dialog

4) Assembly Save As Copy dialog opens, listing all of the referenced components in the assembly, with the option to reuse or rename

5) Rename new parts as needed (again, any drawings with the same file name as the parts / assemblies will be copied and renamed also)



Also check the Assembly help topics, page 215



This has saved a lot of work on similar designs…



Christopher Gosnell

TRIGON INC.
FPD Company
124 Hidden Valley Road
McMurray, PA 15317
PH: 724.941.5540
FX: 724.941.8322
www.fpdinc.com

[dgschaefer]

"I tried the Save As method of the assembly, but there was no line
prompting me to reuse or rename the master part file in the renaming
dialog box, so thus I did a backup of both. I don't know if there could
be a config setting that influences this or not."

If your master part file is not part of your assembly, this will happen.

Doug Schaefer