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" Hide Other " function is what i need for Christmas


" Hide Other " function is what i need for Christmas

I am working with Creo Parametric 2.0 and often working with assemblies. Sometimes i use the Hide function to hide parts and subassemblies.

What i really need and a much better missing function is Hide Other. I want to select a few parts or sub-assemblies and then hide all non selected parts and subassemblies. If there are a way to do this today please let me know.

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Accepted Solutions

An "inverse selection" option would be way cool! I don't know of one.

Welcome to the forum, Geir.

View solution in original post


Hi Geir Ove,

you can use functionality of Layers and Find command.

  1. create a layer (eq. DISPCOMPS) and put components that remain displayed in it
  2. use Find command - activate Status tab, select Layer options, define Criteria with Comparison Not included and Value DISPCOMPS, click Find Now button
  3. click into items found area and press CTRL+A to select all components
  4. click arrow button to display selected components in items selected area, then click Close button
  5. components are selected in Model Tree, you can click RMB and use Hide command

Currently I do not have an idea, how to make the above procedure "on-click" action.

You can try to use mapkey functionality to execute steps 2-4.

Maybe you can try to develop AutoIt script.

Martin Hanak

Martin Hanák

1. Pick the components you want to see.

2. Right click and select Representation/Master.

This creates a simplified rep showing only the selected parts, whcih you can save if desired.

An "inverse selection" option would be way cool! I don't know of one.

Welcome to the forum, Geir.

I think its easy for PTC to implement such an option for Creo users.

I think it's cool enough to put on the "wish list"

As a realative new Creo user this forum is very usefull for me.

Instead of hiding them directly, create a layer and put the items you want to see on that layer and change the layer visibility mode to Isolate.

"In Assembly mode, if you set a specific layer or layers to Isolate, PTC Creo Parametric hides all components. In addition, PTC Creo Parametric hides all other items that are assigned to any non-Isolate layer."


You can also create a layer that is driven by a rule that includes all items not on the layer created, making it so that all items are covered. Normally Isolate will show those items on the Isolated layer and all items not on any layer. The rule forces all items to be on some layer, so they don't show up unexpectedly.

Try this:

1. Copy my attached mapkey to your

2. Create a simplified rep called "3" in your assembly (You can make this in your start parts)

3. Call mapkey pressing F9

4. Select components to isolate and press resume.

Tell me if it has worked.


Listen to Nate!

What he describes does pretty much that, except you are not working with hide but a temporary simp rep.
Select components you wantto see, right mouse button 'Represenation' -> 'Master'
This will excluse all other components in a temp. Simp Rep. If you want to switch back you simply go the view magager, Simp rep tab and hit Master again to display everything.
Quick and easy, no layers, no rules no new selection mechanism...


But that only works if the you haven´t changed the simp rep.

If you exclude one component that method doesn´t work anymore. With the mapkey I shared before, you can still isolate the components you want.



1. With my method, if you want to save a new simplified Rep of the visible parts, you can do that by simply right clicking on the Master Rep in the simp rep menu and saving under a new name.

2. You can add visible parts to the modified master rep by selecting them from the model tree and right click and choosing master rep.

3. You can reset the visibility of the assembly by double clicking the master rep.


There is of course merit in using simplified reps and combination states.

However, I rarely find myself using them on the fly.

A simple selection reversal would be something useful in assemblies.

However, selected features limit the RMB menu choices.

In the case of this discussion, if your reverse selection includes an already

hidden object, the "Hide" option is not available with the RMB.

Another consideration is handling patterns. Are you selecting the pattern feature,

or the features or parts being patterned?

After several years in Creo, I still haven't found efficient mass selection techniques.


Antonius, to select multiple components at once, you can change the filter to parts and then select by window. Selecting from right to left is not the same that selecting from left to right. One selects just components that are totally inside of the window, other selects all components "touched" by the window. Autocad style.

Another option is the 3d box, but I rarely use this one.

Video Link : 5524

true, I knew the windowing works with in and cross depending on direction.

The problem is that it is hard to quickly realize when a window option is available for selection.