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Enhance hide/unhide !

Enhance hide/unhide !

Add the posibility to hide all parts except the ones selected and after doing an action on the selected parts (for instance creating a feature in one of the parts), return to the previous shown parts.

This improves working speed and working ease.

18 Comments
cpreßinger
2-Guest

I dont see a benefit from that. You are already able to view the simplified representation options in the model tree. Just suspend the master-assembly and include everything you want - job done. You even can save this state to get it back quickly.
As a bonus, your performance will increase.

The only limitation i see - all excluded models wont regenerate by the changes done in the included parts, as long as they are excluded...

mwa
14-Alexandrite
14-Alexandrite

Of course you can do this by making simplified reps and for things you want to keep this is the preferred method. But often when you work  on large assemblies and you want to add detail features to some parts, you want to activate that part and have only the parts surrounding this effected parts in the sketch for the new feature, so that the others do not mash up your sight.

Of course you can also do this by making a simplified rep, but this will be a lot of extra work (creating and deleting afterwards). When creating the new features you want to go straight forward to speed up productivity.

cpreßinger
2-Guest

You dont have to create saved simreps, you can build them temporarily.

We use "user-assemblies".

Thats nothing more than an assembly, where the top assembly is placed by standard conditions.

It allows you to modify simreps as you want without affecting the simrep-states of the subassemblies.

In your case, you could handle it like this:

Create a "user-assembly"

Place the assembly you like to work in just by standard-conditions.

Select all parts/assemblies you like to see, then rightclick and change the simrep to "master" -> this will overwrite any simrep-state that is defined by the assemblies above. You can do that in the model tree as well as in the 3d-view - just as you like.

Now, creo should already have excluded the user-assembly (and according to that all parts/assemblies, that werent marked as dedicated "master" before).

You now can do your changes as you like, you can even save everything without modifying any of the simrep-states except in your user-assembly.

If you want to get back to the original master simrep, open the view manager and doubleclick the master simrep. (pay attention, that there is a "+" next to the master-simrep - this means it is modified). The doubleclick will eliminate all temorary simrep-modifications for the master-simrep and load the original state.

Working like that, let you show/hide the needed geometry within seconds (for sure - it depends on how much parts you have to select).

I hope all translations were correct, I am using creo with the german language pack...

mwa
14-Alexandrite
14-Alexandrite

The above working method is the method we are using nowadays also ! But the enhancement is about improving productivity, not about getting the job done !

StephenW
23-Emerald II

In any assembly, if you select components you want to show, then RMB, set representation, master, it will temporarily "isolate" the selected components (in other words, temporarily modify the master rep as shown in the simplified rep tab of the view manager) and only show the selected components. If you double click on master rep in the view manager, it resets back (or if you want to save the rep for later use, you can)

mwa
14-Alexandrite
14-Alexandrite

In Creo 2.0: This is working for the Master Rep, but unfortunately not working for another simplified rep. If this is also going to work for other simplified reps, than this issue is solved

dgschaefer
21-Topaz II

Creo already has an "isolate" command, but it only applies to layers.  So, if you create a temporary layer, add your components and isolate it (under the drop down menu in the layer tree).  That shows only what's on that layer.  With components on a layer, it effectively hides everything else.

StephenW
23-Emerald II

You are correct, unfortunately it only works when you are in the master rep.

mwa
14-Alexandrite
14-Alexandrite

This is not a very productive way and probably more work than making a new simplified rep. The behavior which is shown by Stephan here above is what we want, but then also for the other simplified reps.

cpreßinger
2-Guest

it kinda does. The limitation is: If you are creating your own simplified reps, you have to give the parts you want to see (or you dont want to see) dedicated status. These are already isolated.

And thats where it starts to get complicated.

If you want to exclude a subassembly, while its components already got a dedicated master status, it wont affect them, because the dedicated status overrules the relationship between the subassembly and the component.

I guess it would help a lot if you upload a model and show us your requirements.

Pieface
6-Contributor

Put everything on Layers allows you to quickly turn off/on visibility of parts.

svillafuerte
6-Contributor

Everything people are saying will work ACCEPT all of these REP options everyone is talking about DO NOT work with all Creo licenses. I have a bunch of Foundation licenses and they will not do any REP options because those licenses do not have the features needed to perform them. So that alone leads me to vote on this enhancement so that all my users have the same chance at highlighting just what they want to see/work on for a short time and then have a quick option to turn them all back on. I think this makes sense.

jquiring
6-Contributor

I agree with Marco this would be a productive enhancement.  All the techniques suggested will work but they arrest my creative moment and force me to stop working on my problem and start working on the tool (Creo) when I finish I go back to working on my problem.  Not very efficient.  The technique Stephen mentions is the closet to being what I would like maybe a little tweaking by PTC and we would be there.

svillafuerte
6-Contributor

Sorry, my ACCEPT should have been EXCEPT. I even capitalized it to emphasize it and still got it wrong.

creis
1-Newbie

Did you consider using "Style" you can use it to blank out parts and allows you to save it, and it's available in Foundation.

mwa
14-Alexandrite
14-Alexandrite

Also  invert the selection would be a ver helpfull enhancement additional to the above item 

auijttewaal
7-Bedrock

I think you're request has been answered!
'Show Only' has been added in Creo 5 🙂

olivierlp
Community Manager
Status changed to: Archived

Hello,

We are archiving your idea as part of a general review. This action is based on the age of your idea and the total number of votes received, as per this announcement.

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