Wave link revising parent body 1

[Lars1978]

Hi All,

I've made an assembly of a gutter. The gutter eventually will consist of all sheet metal parts.
I created a master part witch consists of all sheet boby features.
I've made parts wave linked to the master part and waved the relevant sheets body for creating a sheet metal part. (works nice with part to sheet metal function )

Problem is when revising the master model (make unique) all wave links are pointing to the old parent ?

I'd like all children part to point to the new parent. I can imagine there will be a simple solution for this ?

Kind regards,

Lars




Lars
Solid Edge
Inventor
NX10.0.3.5 native

 

[adkad]

Hi Lars,

Before opening part, change assembly load option to "Latest working".

It may work.

Thanks,
adkad

 

[cowski]

The "latest working" option is only available in teamcenter, and I don't think it would help here anyway...

I'm not clear on why you are using the "make unique" command. If you are creating a new revision of the master, a "save-as" would be more appropriate. If all the parts are fully loaded before doing the "save-as", all of the existing links should be properly updated.

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[Lars1978]

Cowski,

So when revising a parent part the save as function will cause the wave links of it's children to be redirected to the new (saved)parent file ?

Is this the main difference between save as and make unique ?




Lars
Solid Edge
Inventor
NX10.0.3.5 native

 

[cowski]

So when revising a parent part the save as function will cause the wave links of it's children to be redirected to the new (saved)parent file?

Yes, when done correctly. There are various load options for interpart data, but the easiest way is just to fully load all the components that take part in the wave link operations.

Save-as and make unique are different tools for different purposes. If you have a component that is used multiple times in an assembly and you later want to make some changes to one of the instances, the "make unique" command is the way to go. I would not recommend using it to create revisions. To create a revision, open the part, its drawing (if using master model method), and fully load any assemblies that make use of it. With the model file as the display part, perform a "save-as" and give the file a new name (usually just a revision increment in the file name). Save-as will also prompt you to give new names to the drawing and assemblies; give the drawing a new name, but hit cancel for the assemblies (unless you also want a new copy of the assembly file). If you hit cancel for the assemblies, they will not be renamed, but they will reference the newly saved component. You will need to save the assemblies to keep the change.

www.nxjournaling.com

 

[Lars1978]

Cowski,

This is very useful info. Thank you.


Lars


Lars
Solid Edge
Inventor
NX10.0.3.5 native