close and discard part changes in assembly.

[doug_anderson]

looking for some help

i was busy making some changes in a part with the assembly open in the background. i don't know what happen, maybe a caught a keystroke, but my model fell over and the undo button would not undo whatever had happened.

in creo how do you close a part and discard the changes from the assembly? effectively putting the assembly and part back to before the changes where even started.

thanks

[kdirth]

Assuming you are trying to keep the assembly open and preserve changes in the assembly:

• Suppress all instances of the part in the assembly (in suppress options Suspend everything)
• Go to part window and Erase Current to remove from session (File/Manage Session/Erase Current)
• In assembly Resume all instances of part.

Part should now be at the last saved state.

[doug_anderson]

hi kdirth

yes keep the assembly open but not preserve the changes in the part.

i used to use solidworks and if you'd changed something that caused big model issues you could close the part with the assembly open and you got an option to close and discard changes. really simple? anything like this in CREO?

[kdirth]

The steps above should get you what you want.  The key is to erase the part from memory.  Creo will not allow that if the part is active in an open assembly.  Suppressing it in the assembly will allow you to erase it from memory with the assembly open.  All relations to it will remain.

That is the simplest way I know of to do it in CREO.

[doug_anderson]

ok thanks. i'll give it a try when the need next arises.

probably better to try not break my models in the first place but these thing happen. especially as i'm still learning CREO.

cheers

[kdirth]

Could make a good CREO Idea to add a feature to Manage Session - Reload File.

[doug_anderson]

reload file would be a good idea. just trialed the suppressing method and it works but as the part was the 2nd in the tree lots of other parts below it also suppressed.

[kdirth]

When suppressing, if you see Options>> button, select options button to control how related parts are handled.

In the Children Handling window press Ctrl+A to select all, then RMB and select Suspend.  Select OK.

The parts will now fail placement, but that is fine.  When the part is unsupressed all of the failures should be repaired.

[doug_anderson]

thanks i'll give that a try and see how it goes. 

cheers

[dnordin]

Doug,

If you are using Windchill, simply activate the part in assembly mode, and then use FILE > OPEN > UPDATE CURRENT.  This will update the active model in session with the unmodified version in your Workspace.  If you happened to have saved the modified part file into your WS already, you will have to re-add the latest version from the Commonspace before doing the update current.

If you want to update everything in session with what is currently in your Workspace, you can use FILE > OPEN > UPDATE ALL.

Regards,

Dan N.

[doug_anderson]

hi Dan.

thanks for reply but not actually using windchill.

regards

doug