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23-Emerald III
StephenW23-Emerald III
23-Emerald III
July 2, 2014
Question

show only selected components in new simplified rep

  • July 2, 2014
  • 9 replies
  • 11428 views
I've searched and searched and can't find the answer.
I have an assembly with several thousand parts/assys. I want to temporarily show 8 or 10 components I have selected and nothing else.
I've done this and seen this described before on the user group but can't for the life of me find it or remember how I did it. It must have been PRE-CREO.

Sort of like isolating using layers but I don't want to mess with the layers on this model, it's a nightmare.


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9 replies

N
nrollins1-Visitor
1-Visitor
July 2, 2014
Steve,



Select the components to isolate, RMB>set rep to> master



Killing it I believe requires going to view manager and resetting the master
rep (don't save it)



-Nate


S
23-Emerald III
StephenW23-Emerald IIIAuthor
23-Emerald III
July 2, 2014
Thanks Nate and Tom.
In the master rep, Select the components, right-click, set rep, Master.

That is exactly what I was doing BUT I was already in a user defined simplified rep, so it was setting the components in that rep to Master, not isolating as I was expecting. You have to be in the master rep for this to work.

I don't like working in the master rep on these models simply because they are large and unwieldy.

D
dgschaefer21-Topaz II
21-Topaz II
July 2, 2014
I've been on WF4 for the past several projects, so I'm not sure the exact steps in Creo. If you create a new rep, it defaults to picking components to exclude. If you pick the top level assy in the tree it sets the rep to be a default exclude rep, then you're picking components to set to include.

--
B
BillRyan16-Pearl
16-Pearl
July 2, 2014
In Creo Parametric 2, you can do the following steps:

1) Copy simp Rep in View Manager and then edit the new rep

2) Use the preview window in the view manager to box select the items you want to keep or use other methods to select them. (first picture)

a. The additional selection tools built into the preview window are very impressive.

3) Then use the "isolate" icon. (second picture)


Note Make sure your config setting for searching server with preview is set to "no" if embedded with Windchill when you are in an environment where not all objects of the assembly reside in your workspace.

Also, Creo View has this functionality available using box selection and RMB functions directly in the graphics window...


[cid:image002.jpg@01CF95E7.E8DC00F0]


[cid:image007.jpg@01CF95E7.E8DC00F0]


S
23-Emerald III
StephenW23-Emerald IIIAuthor
23-Emerald III
July 2, 2014
Thanks Bill, that's interesting. I'll give that one a shot.
It's a little more step intensive but if I have to select several items, it might be easier in the long run.

J
jelpedes11-Visitor
1-Visitor
July 2, 2014
If you liked the way simplified reps used to work and you prefer it that way, you will need this line in your config.pro: new_wf5_simp_rep_ui no

Call me old school but I like to be able to just pick the models in the window or the model tree. I also find it very convenient to toggle the default between Include or Exclude. Sooo much easier (at least for me).

[cid:image003.png@01CF9618.5A2BDFC0]






Jerry Elpedes

Senior Engineer



Trijicon, Inc.

248-960-7700 Ext.1130

49385 Shafer Avenue | P.O. Box 930059

Wixom, Michigan 48393 US

- | www.trijicon.com
B
BillRyan16-Pearl
16-Pearl
July 3, 2014
Jerry, we have some old school users here too. Note: one of the reasons users disliked the new UI was that they had to manually save the simplified rep when making changes using the model tree column functionality or RMB functions(ref picture). Sometime after build M070 build of Creo Parametric 2, the PTC programmers changed the functionality of the old UI to perform the same as the new UI in this regard. I’ve got a couple users that lost work on their definition of the simplified rep using the old UI and have convinced them to come to the other side!

95% of the time I’m using the model tree or simp rep column to manipulate the simplified rep so I’m not going to the UI.

[cid:image001.png@01CF96A1.2B7B0FA0]
J
jlippeth1-Visitor
1-Visitor
July 21, 2014
Just to chime in

I use the Pre Creo 2 setting (new_wf5_simp_rep_ui no)

Reason, I found using the new UI, the display window that pops up for selection shows surface/quilt layers on.

If you have library parts with cut quilts, layer default off, the new UI turns them on in the selection window.

Hard to pick the comps in the selection window with a massive blob of surfaces.

This is not the case with the old UI.

Is there a setting for this in the new UI?



Note: CREO View Express will also display surface/quilts on

But if you have your cut quilts on a custom layer IE. Cut_Srfs they will not be displayed if originally set to off.



JSCOTT



Jeff Lippeth ▪ Mold Design Engineer

NyproMold, Inc.

▪ P 847.855.2226


S
23-Emerald III
StephenW23-Emerald IIIAuthor
23-Emerald III
July 21, 2014
Not sure about the quilts blob or the settings for it. I know that the 3 or 4 times I have worked with large surface models, I was not a happy user.

And an update on the solution to isolate:
I did try the isolate function in the new user interface (haha, not so new anymore) and it’s awesome. I was able to box select an area that narrowed down the items show to just a few. Then I used the box selection again on the narrowed down selection again with a different spin on the model to narrow it down even further. I took an assembly of several thousand components and isolated 8-10 components I wanted to see in just a few seconds. I never had to activate the master rep which is the downside to the first method that was suggested which sometimes can be an issue on large assemblies.

I can use this functionality in my day to day usage when working on large assemblies to quickly created temporary simplified reps so I can add hardware to a component or check clearance in a specific spot.

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