NX5 parts list text 2

Go into Insert -> Text... and open the full Text Edit dialog. Enter the Text String (without the quotes): "Grease ID of Item " and at that point select the 'Relationships' tab at the bottom of the dialog and select the 'Object Attribute' item and then select the the COMPONENT (make sure it's the component and not a face/edge/body) which is item 25 and when the list of available attributes comes up, select 'CALLOUT' and then OK and then finish you note. When you get done the text string in the editor should look something like:

"Grease ID of item <W!24976@CALLOUT> before assembly"

where the number '24976' is the internal NX object id for the Component.

John R. Baker, P.E.
Product 'Evangelist'
NX Design
Siemens PLM Software Inc.
Cypress, CA

To an Engineer, the glass is twice as big as it needs to be.

Jerry,

We have had similar requests before so I know that what John refers to will work perfectly well. Many of the people making these requests in the past expected to use them in an automated sense and that is where will struggle. That object number will refer only to that object as used on that drawing, so that if you have several that you want to do that way then you have to repeat the selection process for each. I think this is all fine and good as I don't know how you'd expect it to work pretty much any other way, but I thought I'd add the explanation anyhow.

The good news is that if you do use this in the notes or wherever it should correspond with the ID callouts for the life of the drawing. It gets rid of the requirement that you manage to keep the same callouts from one drawing release to the next despite parts being add or removed, so that you have to try and manually manage parts lists by locking rows to make each part number associated with a fixed callout ID, or keep manually checking that references in the notes are correct. This way you can keep the parts list columns sorted as you wish and the ID numbers are free to change without introducing errors.
Some people still don't like this. Some people are a pain in the neck

Of course the other place you can use it is in a leaderless balloon ID as well.

Cheers

Hudson

Thanks guys for some very good but obscure info!

Believe it if you need it or leave it if you dare. - [small]Robert Hunter[/small]

Hi Guys,

I tried out the steps as told by John.. works good.. but in a scenario where I will reorder the way i have assembled the components of the assembly and then come back to drafting and see that obviously all the balloons will have got un associated.. I associate the balloons again and if I look at that note, its not updated.. I have to redo the assigning the callout in the obj attrib for that note.. Am I doing anything wrong.. Let me know

Iam using NX4.. Do no whether this topic is specific to NX5 or it should work fine with NX4 also..

Thanks...

It's a delayed update problem which we're working on but which won't be fixed 100% until the next release (NX 7). However, if you save your part and reopen they are correct. Also if to plot or create a PDF file, they are correct. The actual data structure is correct it's just that the notes linked to attributes don't update in real-time, but they will be right when you 'publish' (plot or export PDF) so it's low priority fix (but expense to do so we're lumping it into the NX 7 new Attribute project).

John R. Baker, P.E.
Product 'Evangelist'
NX Design
Siemens PLM Software Inc.
Cypress, CA

To an Engineer, the glass is twice as big as it needs to be.