Exclude parts from sectioning in assembly drawing 1

[lgnx]

Hi,

Please find the attached assembly file of Machine vice. I tried to exclude washer, and two nuts (first image) from sectioning by adding attributes in part files, but i couldnt get it. can somebody see where am failing?


i follwed this link to create new attributes. As JohnRBaker says i should have added attributes before inserting into assembly. i think i failed somewhere there. i dont know how to apply attributes in context of drawing assembly as he says.

https://www.eng-tips.com/viewthread.cfm?qid=296740

appreciate your help.

 

[JohnRBaker]

My original approach should still be valid. Unfortunately, I can't help you much further than that since I no longer have access to NX.

John R. Baker, P.E. (ret)
EX-Product 'Evangelist'
Irvine, CA
Siemens PLM:
UG/NX Museum:

The secret of life is not finding someone to live with
It's finding someone you can't live without

 

[NutAce]

You can use the "Section in View" option to set a component to Non-Sectioned (or not)
This is however in context of that drawing.


Ronald van den Broek
Senior Application Engineer
Winterthur Gas & Diesel Ltd
NX9 / TC10.1.2

Building new PLM environment from Scratch using NX12 / TC11

 

[niedzviedz]

Hello,

You have to create new attrbute in part, not in assemblly called:

SECTION-COMPONENT

and in value put

NO

There is also option i drawing (like @NutAce mention) - "Section in View". In tjis case You must work in assemblly drawing. First You select section view in which You want to make parts non sectioned, then You choose which parts. It's safer to choose parts from assemblly navigator. And finally in "Action" choose "Make non sectioned".

With best regards
Michael

 

[Xwheelguy]

Another option is if they are components, just use Hide Component in Drafting. Invoke the command, pick the view(s) in which you wish to not show the component(s) and then select the components to hide in the view(s). Component selection can be made in the view or from the Asm Navigator. Show Component brings them back. No messing around with attributes. Update the view if necessary and components are gone.

In Drafting, Menu -> Assemblies -> Context Control -> Hide Components in View or Show Components in View.

Pretty under-utilized command, IMO.

Tim Flater
NX Designer
NX 11.0.2.7 MP11 Rev. A
GM GPDL 11-A.3.5
Win7 Enterprise x64 SP1
Intel Core i7 2.5GHz 16GB RAM
4GB NVIDIA Quadro K3100M

 

[lgnx]

Thank you all for your inputs. small inputs led to much broader understanding. also i found this youtube video very helpful. sharing so that it may help others.

blob:

https://www.youtube.com/4950502d-a1ee-48d7-bc96-eb3c7c7694a4

Thanks.

 

[NutAce]

Another option is if they are components, just use Hide Component in Drafting.

Why would he want to do that? He wants to section the components, not remove them.

Ronald van den Broek
Senior Application Engineer
Winterthur Gas & Diesel Ltd
NX9 / TC10.1.2

Building new PLM environment from Scratch using NX12 / TC11

 

[Xwheelguy]

@NutAce,

You're right - I misunderstood. Actually, he doesn't want to section certain components.

When we run into that where I work, we just don't show the components - hence why I responded the way I did.

Tim Flater
NX Designer
NX 11.0.2.7 MP11 Rev. A
GM GPDL 11-A.3.5
Win7 Enterprise x64 SP1
Intel Core i7 2.5GHz 16GB RAM
4GB NVIDIA Quadro K3100M