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Isolate selected components in assembly

Newbie

Isolate selected components in assembly

Hi,

 

I am a beginner in creo.  In previous cad software which i used (inventor and solidworks), I can easily isolate the components in assy environment, but in creo I cant find a proper way to do it. I search around the web, which I find a poor way which is: select the components you want to isolate --> representation--> master. But this method cant longer be used once you are in another simp representation mode. So please advice the fastest way or at least the efficient way to perform the 'isolate' function since me and my colleague use "isolate" function quite frequent when need to modify part feature in assembly environment.

20 REPLIES 20

Re: Isolate selected components in assembly

1. kindly stop thinking Solidworks and Inventor way..to work better in Creo.

2.yes you are right, the master option works only once, after using it ones you can further use the exclude option to remove the component/components which you do not want.

3. Solidworks and Inventor were made with ease of use in mind, the would always be better in ease of use.

Re: Isolate selected components in assembly

Sadly, this is not possible at the moment with Creo, using GUI only.

You can tell Creo to search for all parts, and exclude them all from rep using find tool within a mapkey. But how to store selected parts as a selection set upfront to set them to master representation afterwards? Propably only with an API.

Has anyone ever bothered coding anything like that?

Re: Isolate selected components in assembly

Since there is no way to perform components isolation, is there any ways to perform certain action similar like this? I am wandering how you all doing a top down design on assy environment (insert a new part (blank component) within assembly and then isolate certain components around blank component to get a better view around the new blank component --> model the blank component --> un isolate to get view of full assy.

Another question I would like to ask: Suppose I am in sketch mode on new part, the I open another part (part b) on new tab, somehow the new part dimension which is on sketch mode need to refer part b, so that I switch to part b window so that I can measure the length or diameter of holes. Creo didn't allow me to perform any action on part b, unless I need to exit or complete the sketch on new part. Is it got any trick to play around?

Thanks for help~

Re: Isolate selected components in assembly

In SW (I can't comment on Inventor), one accepted method of top down design (TDD) is "in context edits" where you build a component in the assy, referencing the related other parts as needed.  This method is possible in Creo, but not desirable because it easily creates an unstable mess of external references. (I find that to be the case in SW as well, but it at least works better there.)

Creo has a very robust TDD tool called "skeleton modeling" which is part of the Advanced Assy Extension (AXX). If you want to do TDD, you should acquire AXX if you do not already have it and then search the help files and knowledge base for skeleton modeling, copy geometry features adn publish geometry features.  it's a very different concept than SW TDD, but far more robust, powerful and flexible.

If you do not have AAX and cannot acquire it, search for the "master model technique" or "merge features" or "inheritance features".  These are possible without AAX and provide much f the functionality of skeleton modeling.

Spend some time learning Creo methodologies, it will pay off. Creo is not SW, if you try to use it like SW you will be frustrated. If you learn its strengths, however, you will be rewarded with more robust models and better control over your design intent than SW can provide.

--
Doug Schaefer | Experienced Mechanical Design Engineer
LinkedIn

Re: Isolate selected components in assembly

In regards to isolating components, if you simply want to control the display of components, you can use layers or simplified reps. 

You can place components on a layer and hide them and you can define any number of layers to hide various groups of components.The components are still open, just hidden from view.  You can also define various "layer states" in the view manager to save your assy with different components visible.

There is a not well known "Isolate" command with layers.  If you create a layer and place a single component and isolate that layer, Creo will show you only the contents of that layer.  In assy mode, with components on the layer, it will hide all components that are not on that layer.  Isolate woks differently in part mode and when features or feature entities are on the layer.  The isolate command is in the layer tree (view tab > layers) and under the icon that looks like a stack of papers.

You can also define simplified reps and remove certain components.  This is also done through the view manager and multiple states can be defines as well.  With a simplified rep, however, the component can also be removed from memory, so it is valuable for managing large assys.

--
Doug Schaefer | Experienced Mechanical Design Engineer
LinkedIn

Re: Isolate selected components in assembly

Have you tried to make use of SimpReps (Simplified Rep’s or Representations)?  Using SimpReps, you can make as many representations as you wish, save them and retrieve them any time you want.  This functionality has been around for VERY long time and works excellent.  I use it ALL the time.

Bob Schwerdlin

Design Engineer

Dukane Corp.

2900 Dukane Dr.

Charles, IL 60174 USA

630-679-1941 direct

-<mailto:->

www.dukane.com/us

Re: Isolate selected components in assembly

Thanks   

Re: Isolate selected components in assembly

Still a good question 4 years later...

Re: Isolate selected components in assembly

Makes absolutely no sense that ISOLATE is not a 1 button command.   Someone must have IP that PTC can't violate?!?

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