topic Re: Hiding Parts in ISO Section View in Inventor Forum

Hiding Parts in ISO Section View

Anonymous — Fri, 15 May 2015 18:50:01 GMT

I've an assembly, and want to hide some parts to show more internal details...typically, find the part in the browseer, rt. click and turn on/off visability...yet it is "grayed"out and unable to be selected...

I tried to post a screenshot with it, but it won't allow me to shoot the rt. click drop box...sorry!

Cheers all!!

Jess

Re: Hiding Parts in ISO Section View

mdavis22569 — Fri, 15 May 2015 18:55:33 GMT

Do it with a View representation

Make a new View Rep with only what you want to see ...

Double click the view and pick that View Rep

Re: Hiding Parts in ISO Section View

Anonymous — Fri, 15 May 2015 19:01:39 GMT

Thanks for the info...Im not clear on how to do that within that view...the ISO Section that is....

Secondly, is hiding the part within the ISO Section not allowed...I'm sure Ive seen it somewhere (YouTube I think).

Re: Hiding Parts in ISO Section View

mdavis22569 — Fri, 15 May 2015 19:20:57 GMT

Go to your IAM .... then to your browser.

Expand your Representation Folder. Should have Master (locked) and Default, Right mouse button and make a New view... Call it View 1, or Iso your choice.

While in that View Rep, turn off all the items you want turned of in the ISO view.

Once you're done turning off everything you don't want .... SAVE the IAM

Click back on Default making it active. Everything you turned off should be back on.

Go to your IDW. Double click on the View.

In the pop up ... You'll see Views like I post earlier. Click on your new one that you made and close the pop up. You should see an updated view with all the items you wanted turned off .... Off now ...

Re: Hiding Parts in ISO Section View

mdavis22569 — Fri, 15 May 2015 19:23:49 GMT

As for is it allowed ..Yes it is ...

are you now able update any of the views? Is Defered update on?

Re: Hiding Parts in ISO Section View

SBix26 — Sun, 17 May 2015 01:36:15 GMT

In the Edit View dialog box, uncheck the Associative check box just above the View Representations list (you can see it in Michael's posting, has a link icon next to it). Inventor gives you the ability to control component visibility either in the drawing (non-associative) or in the assembly via View Reps (associative). Looks as if you wish to work non-associative and your view was placed associative, so all you need to do is change that condition.

Sam B

Inventor Professional 2015 SP2
Windows 7 Enterprise 64-bit, SP1
HP EliteBook 8770w; 8 GB RAM; Core™ i7-3720QM 2.60 GHz; Quadro K4000M

Re: Hiding Parts in ISO Section View

Anonymous — Mon, 18 May 2015 15:36:51 GMT

Thanks, guys!! It was the "Associative" relationship...all good now!!

Have a great week!!!

Cheers,

Jess