Make part "invisible" to parts list attribute?

[3dr]

It seems like it's something we should have.
When fastening together a large assembly we sometimes have to mate into position up to 4 parts
EX: 1 Bolt, 1 nut & 2 washers.

We should be able to make an assembly of them 1 time and position that assembly where ever we want in the assembly hierarchy .
With the parent part invisible to the parts list, but the children reporting.

What are other people doing to handle this problem?
It's tedious and time consuming placing all these fasteners!



Dave
Automotive Tooling / Aircraft Tooling / Ground Support Structures

NX11, Win 10 Pro

 

[NutAce]

Did you have a look at the "Fastener assemblies"? Also available in NX11


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

Building new PLM environment from Scratch using NX12 / TC11

 

[3dr]

Not recently... should I?

I've looked / read up on them a couple of times over years.
Never perused them tho... it seamed like a complicated solution to a simple problem.


Dave
Automotive Tooling / Aircraft Tooling / Ground Support Structures

NX11, Win 10 Pro

 

[Toost]

Fastener Assemblies has some unique features, it will "mate" the fastener assy to both sides of the object-s
The screw/washer-s will be "mated" to one side and the nut/washer-s will be "mated" to the opposite side.
If you create a "homemade fastener assy" ( Without the tool mentioned), the position of the nut/washers-on-the-backside will have the position saved/stored in the "homemade fastener assy"
And therefore the distance screw head to bottom washer/nut is "almost always wrong".
You will then need to go "Override position" on the washer/nut to move these into position. ( If this is required ?)

The true benefit of "NX Fastener assemblies" is speed when you need to add many fasteners.
You select the hole close to the screw top face, NX will then identify the two faces to place the top washer and screw, NX will attempt to find the bottom face for the washer/nut, if that fails you pick that . - Done.

In case you like to do the "homemade fastener assy" and hide the assy from the BOM,
Add the Attribute "PLIST_IGNORE_MEMBER = yes" in that file. this will make that part "non-reported" in any parts list.( If you run Teamcenter you can select the "Reference Component" button.)

Regards,
Tomas

 

[3dr]

Thanks Toost
You just schooled me on the PLIST_IGNORE_MEMBER attribute.
It does what I was looking for.

But I swear I've tried using it for that a few different times in the last 5 to 6 years.
Each time it didn't do what I needed but or I was doing something wrong.
It did this morning so I'm happy to have options.

I'll look into the fastener assembly thing... is there any solid documentation on it?





Dave
Automotive Tooling / Aircraft Tooling / Ground Support Structures

NX11, Win 10 Pro

 

[multicaduser]

I wrote first grip then a journal to set this attribute for assemblies so they didn't show up in the bill of materials. However, with NX12, if this was accidentally set in a component I found it impossible to manually "unset" it and had to write a journal for this purpose. Should have added that it was sometime impossible to unset, but not usually.

NX 12.0.1.7 Windows 10

 

[Toost]

i have neither found out how to "unset" this variable, -anybody ?

 

[multicaduser]

Go into File->Properties->Attributes, locate "PLIST_IGNORE_MEMBER" and delete it. It's easier for me to find using "Traditional" display rather than "Bulk Edit".

NX 12.0.1.7 Windows 10