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gsteinsvåg4-Participant
4-Participant
December 12, 2014
Solved

" Hide Other " function is what i need for Christmas

  • December 12, 2014
  • 6 replies
  • 7658 views

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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Best answer by TomD.inPDX

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

Welcome to the forum, Geir.

6 replies

M
MartinHanak24-Ruby III
24-Ruby III
December 12, 2014

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

N
N8_011-Visitor
1-Visitor
December 12, 2014

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.

    T
    TomD.inPDX17-PeridotAnswer
    17-Peridot
    December 12, 2014

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

    Welcome to the forum, Geir.

    G
    gsteinsvåg4-ParticipantAuthor
    4-Participant
    December 15, 2014

    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.

    D
    dschenken1-Visitor
    1-Visitor
    December 12, 2014

    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."

    ref http://help.ptc.com/creo_hc/creo30_pma_hc/usascii/index.html#page/pma/fundamentals/fund_six_sub/About_Layer_Display_1.html

    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.

      J
      Jose_Costa12-Amethyst
      12-Amethyst
      December 13, 2014

      Try this:

      1. Copy my attached mapkey to your config.pro

      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.

      Jose

      C
      Constantin15-Moonstone
      15-Moonstone
      December 15, 2014

      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...

        J
        Jose_Costa12-Amethyst
        12-Amethyst
        December 15, 2014

        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.

        Jose

        N
        N8_011-Visitor
        1-Visitor
        December 15, 2014

        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.

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