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Create a NX Drafting note using Assembly Component Attribute "CALLOUT" from another drawing

Experimenter
Experimenter

Hello all- Please forgive if this topic has been covered elsewhere.  I searched but didn't find anything.  I have an issue that would be nice to resolve.  I am using NX 10.0.3 mp4.

 

I have an assembly documented in Drafting, including a "Parts List" and auto-ballooning.  Of course, one of the columns in the parts list is the callout, which is basically the balloon number.  If I right-click on the component (not the part) in the assembly navigator and go to Properties and then the Attributes tab, I can see the Attribute named "CALLOUT".  This is a fluid number that is assigned by the system and can potentially change based on sort, number of components and such.

 

Now here is my issue.  I have a separate drawing file that documents the part (of the component in question).  On that drawing, I have a note that tells what the CALLOUT number from above it.  Unfortunately, if the CALLOUT changes, I have to manually go update my note.

 

Is there a way to make the note point to the other drawing/sheet and read that attribute?  I've played around with it and can't find any way to do this.  I have a call with GTAC and it stumped him as well.  He's asking a developer, but I thought maybe someone in the user community has a way to do this.  I don't consider what I am trying to do anything too out of the ordinary.  How do people in the real NX world handle this sort of thing?

 

==

As an alternate idea, I would also be okay with freezing the CALLOUT number of the Component in the assembly drawing.  That way I could just put a note on the part drawing and know it's always going to be the same.  But GTAC and I could not figure out how to freeze the attribute either.  Either way would work for me.  (On a side note here, it has to be a COMPONENT attribute that freezes and not a PART attribute, because the part could be used in a different assembly and have a different callout.)

 

Let me know if you have any suggestions.  Thanks!

6 REPLIES

Re: Create a NX Drafting note using Assembly Component Attribute "CALLOUT" from another dr

Gears Honored Contributor Gears Honored Contributor
Gears Honored Contributor

When you lock the row in the parts list, it will effectively freeze the value of the callout.

 

https://docs.plm.automation.siemens.com/tdoc/nx/10/nx_help/#uid:index_drafting:id702253:id702255Smiley Tongueartl...

 

It's generally considered bad practice to include the assembly callout number on the part drawing for the very reason that you list in your post.

 

...because the part could be used in a different assembly and have a different callout.

Re: Create a NX Drafting note using Assembly Component Attribute "CALLOUT" from another dr

Experimenter
Experimenter

Thank you.  I wasn't aware you could lock the row.  This is helpful.

 

While I agree that it's not a good idea to call the CALLOUT in a different drawing, it is my customer who is driving this requirement and not my call.  Even if I have to do it manually, I have to do it.  I'm just trying to find the best way to accomplish this while eliminating the possibility of errors.  Thanks for your reply.

Re: Create a NX Drafting note using Assembly Component Attribute "CALLOUT" from another dr

Gears Honored Contributor Gears Honored Contributor
Gears Honored Contributor

If the part drawing is in a separate file from the assembly drawing, I don't know of a good way to associatively use the callout number from the other file.

 

You might want to take a look at drawing booklets. I've not personally used them, but it looks like it may help to organize and relate various drawings.

Re: Create a NX Drafting note using Assembly Component Attribute "CALLOUT" from another dr

Phenom
Phenom

 

A very kludgey way.
Use spreadsheet and linked expressions.
In the drawing file of assembly.
Create an expression "PartXCallout" for each component.
Open spreadsheet.
Extract attributes (this gives access to object attributes).
Extract expressions.
Link expression value link to callout attribute value (eg cell PartXCallout = E2 where E2 is cell of Callout attribute).
Push expressions back to part (Update NX part).
In each component part part link to callout expression(Callout=Asy_drg:Smiley TongueartXCallout).
or push expression with link from drg asy (PartXCallout::Callout=PartXCallout).

 

Re: Create a NX Drafting note using Assembly Component Attribute "CALLOUT" from another dr

Siemens Creator Siemens Creator
Siemens Creator
but the link is only for these assembly?
the reference is only with them or can a new reference of other assembly?

Re: Create a NX Drafting note using Assembly Component Attribute "CALLOUT" from another dr

Pioneer
Pioneer

Another way is to create a new attribute called detail (or whatever) in each part. when you add your part list change the callout column to detail instead. They will always be the same. When you balloon use the detail as the callout as well.

The only drawback is that you have to manually add the attribute to each part, but it won't change unless you change it.

Then sort your parts list to the detail column and your good to go

 

You can then add the detail attribute to your part prints as well

Brian
NX 11.0.2
Win 7 pro 64 bit
quadro k4000