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Isolate selected components in assembly

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Re: Isolate selected components in assembly

The solution!

Go to 6:25.

 

This Creo Parametric tutorial shows you how to use Layers in assemblies. The most common use for Layers is to manage the visibility of entities and reduce sc...
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Re: Isolate selected components in assembly

Very good... Thank you!

It's more steps than other CAD software... but I'll give this a try.

 

Thanks again!!!

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Re: Isolate selected components in assembly

Hi @creuz and @doneill 

Creo command search can translate solidworks commands to Creo.  So just type in "Isolate" and the Creo command is shown.  Layers and simplified reps are useful but not as simple as "show-only" which is a "one-click" just like many other software.

command_search_isolate.png

Show OnlyShow Only

I think everyone overlooked this simple answer because these show/hide "eyeball" icons are universal to many software.  Just in case... another basic function is to activate the part you want to work on. 

 

ActivateActivate

 

ActivatedActivated

 

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Re: Isolate selected components in assembly

Oh cool! The command is not working for me though. Clicking on the search result doesn't do anything, and after adding it to my shortcut menu, it is greyed out. What am I missing?

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Re: Isolate selected components in assembly

What version of Creo do you use? 

Also, possibly you need creo helpcenter installed.  Clicking the search should open a text box to the left.

Make sure you are in an assembly and picking parts from the model tree.  The show-only should pop up for both left and right clicks.

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Re: Isolate selected components in assembly

4.0

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Re: Isolate selected components in assembly

Aha, I think it might be newer than Creo 4.

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Re: Isolate selected components in assembly

Also see this thread

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Re: Isolate selected components in assembly

Here is a good work around I came up with.

Creo 4 does not seem to have a "hide all parts"  so instead use a "hideall" mapkey that will make it pretty quick to do isolate.  I used the F8 key for the mapkey.  So the process is hit F8, then select the parts to unhide, then select unhide.  

It works by searching for all *.prt in the model tree (binoculars), adding to the current selection (+) then hide, then delete/clear the *.prt from the model tree search. (you can record this yourself or use the "code" below.)

 

Unfortunately Creo does not remember what was selected before hitting the mapkey (F8) so it has to be 2 steps instead of 1. 

 

You could just add this to your config.pro file.

mapkey $F8 @MAPKEY_LABELhideall;\
mapkey(continued) ~ Update `main_dlg_cur` `PHTLeft.simple_search_ph.ss_key_input_panel` \
mapkey(continued) `*.PRT`;~ Command `ProCmdSimpleSearch` ;~ Command `ProCmdSSApplyResult` ;\
mapkey(continued) ~ Command `ProCmdViewHide` ;~ Command `ProCmdSSClear`;

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Re: Isolate selected components in assembly

Thank you...

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