Removing the parent part reference for a broken link 2

[CADMANSOUTH]

When I delete a component in an assembly it breaks the link. But there is still a reference to the parent part.

How to I remove the reference to the parent part?

I am using NX 8.5 :-(

 

[cowski]

If you don't need the model parameters, you can convert it to a "dumb" object with edit -> feature -> remove parameters.

www.nxjournaling.com

 

[CADMANSOUTH]

Thanks, cowski!
As so often you are a great help.

I can verify that edit -> feature -> remove parameters will work.
But I am hoping for another solution. I hate to use "remove parameters". It is a last resort. I never know when I will need to rebuild something.

Maybe someone else has another solution?

 

[multicaduser]

If the feature is edited and the associative button is unchecked before the component is deleted it essentially becomes a "dumb" feature that can later be re-linked to another parent in the future, but doesn't complain about a missing parent when edited.

NX10.0.0.24 MP1/Windows 7 Service Pack 1

 

[CADMANSOUTH]

Regarding unchecking the associative button.

The issue I'm having is: I need to import files into SAP's ECRT (Engineering Control Center) This is SAP's Teamcenter like a product.

If you have an assembly file and go Information > Part > Loaded Parts At the bottom there maybe a list of parts that are "Not Loaded"
You can also view the unloaded parent parts with
Assembly > Wave > Interpart Link Browser

In my case, these are components that have been deleted. Some Linked bodies that have broken links are still referencing the parent parts.


At import, ECRT will look for look for these not loaded parent parts and stop.
So far the only solution I have is edit -> feature -> remove parameters

Sometimes the parent part does not exist anymore. Or the file was exported out of Teamcenter and the file name is some very odd name in the "Windows file".

So I need to remove this reference to the parent parts.

 

[cowski]

After you remove the parameters and are left with a dumb body, you can "convert to linked body" and re-parent it to a live file if so desired (or leave it as a linked body with no parent). If you go this route, I'd suggest adding a name or attribute to the body to note where it originally came from.

www.nxjournaling.com

 

[CADMANSOUTH]

Hi cowski,
How can I convert a dumb body, to a linked body?

 

[Recon1775]

Go to the part navigator where the unparameterized body is and right click the body.
You will see "convert to linked body" select that, then right click on the broken link to redefine it (edit with rollback or edit parameters) to a new reference body.

 

[CADMANSOUTH]

Hi Reconbomber,
That is it!!

Yes if I Remove parameters on the Link and then I "convert to linked body" it does exactly what I was asking for. NX now loses the reference to the parent part.
23 years of working with NX/UG at ver. 8 and I'm still learning. Thanks! I like this "convert to linked body"!

Now what is the workflow for linked curves??

 

[Recon1775]

Well the only way I know of keeping the curve broken and no indication of where it was linked to is the copy the exact same curve into the work part the link is apart of. Redefine the linked curve to use the copied curve. Then edit the link curve again and turn off the associativity. Then just delete the copy one from the model. Since the curve was referencing within the work part the link won't show any association to any other curve but can still be edited to reference anything within or outside the work part.