Regeration Failue and after renaming part 2

[Speedy]

I renamed the file name of parts (using File/Rename) but now I can't regenerate the assembly.

I used 'quick Fix / Find Component' but it won't open the renamed parts.

From what I understand I should have had the assembly open in session at the time of renaming the part. Then regerate the assembly and then save. I did this with the drawing at the time and no problems. Is this correct?

How can I get the assembly to open the renamed parts?

I'll have no hair left by the time I learn this package. It ain't user friendly, that's for sure!

 

[looslib]

Replace the components with the new ones and save your assembly.

"Wildfires are dangerous, hard to control, and economically catastrophic."
"Fixed in the next release" should replace "Product First" as the PTC slogan.

Ben Loosli
CAD/CAM System Analyst
Ingersoll-Rand

 

[3dlogix]

If you are using Intralink, renaming is almost fail-safe. If you are not using Intralink, then rename parts and assemblies with all their associated drawings and higher-level assemblies in session.

In your particular case, you can rename the parts to their orginal names, then open the original assembly, and then rename the parts back to the new names. Keep the assembly in session as well as any drawings that are associated with it.

Steve

http://www.sprdesign.com

http://www.3dlogix.com

 

[mjcole]

Good Tip Steve,

I went through a similar problem with renaming files yesterday because I had the second to top level assembly open.

If you have your top level .asm open open all your drawings with the components that are changing and rename from part level up. Make sure you check rename objects on disk and in session. Then when you rename your part and regen your drawings the drawing model will update with the new name and you can rename your drawing and save.

If you've already changed the model name and the drawings won't open saying that the old_name.prt cant be found you can rename the part to the name referenced by the drawing and open it in Pro/E by typing the exact file name even if it doesn't show in the open file dialog. then open the drawing and rename your part again.

Michael

 

[Heckler]

Steve,

Great post and the makings of a FAQ. a lot of beginners don't understand the relationships between the part, assembly and drawings which results in a lot of frustration. You have earned a

Best Regards,

Heckler
Sr. Mechanical Engineer
SW2005 SP 5.0 & Pro/E 2001
Dell Precision 370
P4 3.6 GHz, 1GB RAM
XP Pro SP2.0
NIVIDA Quadro FX 1400
o
_`\(,_
(_)/ (_)

Just because I'm paranoid doesn't mean that they aren't out to get me.

- Woody Allen

 

[3dlogix]

Cool, a 2 star day.

Another option, although more elaborate is this.

Part renamed, and drawing now fails because it was not in seesion.
Take renamed part and make an instance with the same name as the original.
Open the instance, and now open the drawing, and in drawing mode use REPLACE, and replace the instance with the generic model. Save your drawing.
In the part, delete the instance or Family Table. And save.

Long, but may be of use for some cases.

Steve

http://www.sprdesign.com

http://www.3dlogix.com

 

[Tofflemire]

Hi Steve,

You can just rename the part in Windows, and reopen the drawing once the name is changed back, then rename the part with the drawing open in session.

Tofflemire

 

[3dlogix]

That will work too.

Steve

http://www.sprdesign.com

http://www.3dlogix.com

 

[Guest0527211403]

(For the FAQ) It's a good idea to back up your drawing and assembly to another directory before you do any renaming without Intralink.
I've landed myself in similar hot water and (very) luckily had a backup of the assembly to get me out.

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