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Part attributes not updating with dimensional change

Part attributes not updating with dimensional change

Part attributes not updating with dimensional change

(OP)
I am using nx8.0.0.25

I have a drafting sheet that refrences a part in a different file. I have some attributes in my drafting sheet refrencing this other part. I made a change to these attributes in the part. I then opened the drafting sheet and they update correctly.

The problem now is that when I make a dimensional and an attribute change, the attributes for this part do not update in the drafting sheet. The dimensional changes are correct, but not the attributes. I played around with it for a while and found that if I right click part in the assembly navigator and click properties, they update correctly if I hit the override attribute green checkmark

I am wondering if I might be doing something incorrectly or if I can do anthing to have my attributes update correctly.

RE: Part attributes not updating with dimensional change

Try toggling OFF 'Partial Loading' in your 'Load Options'.

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
Siemens PLM:
UG/NX Museum:

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

RE: Part attributes not updating with dimensional change

(OP)
Partial Loading is toggled off

RE: Part attributes not updating with dimensional change

Are you using the old, pre-NX 8.0, KF based routines to link Attributes to Expressions or the new built functions which were added to NX 8.0 as part of the Attribute enhancement project? If it was done using the older routines, may I suggest that you replace them using the new approach.

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
Siemens PLM:
UG/NX Museum:

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

RE: Part attributes not updating with dimensional change

Hi,
Try using Tools/Update/Update for external changes.
Best Regards
Kapil

RE: Part attributes not updating with dimensional change

(OP)
I did Try using Tools/ interpart Update/Update all .

Right now I insert an attribute from another part file by inserting a note. From there I choose relationships> insert object attribute, pick the component in the assembly navigator, then choose the attribute I want. Is there a new way of doing it?

RE: Part attributes not updating with dimensional change

For linking Attributes and Notes, while there are some dialog changes, that mechanism is basically the same as pre-NX 8.0. However, for linking Attributes and Expressions that workflow has completely changed for NX 8.0 and while the older pre-NX 8.0 scheme is still supported (at least with respect to legacy part files continuing to behave as they did prior to opening them in NX 8.0) going forward the only tools which will be accessible to the user to create new relationships will be the new ones. And the reason I suggest that you may wish to rework any Attribute/Expression links is that while we continue to support the old KF routine-based scheme for linking Attributes and Expressions, these part files will continue to exhibit the same limitations and less-than-ideal behavior that they exhibited before. Part of the rational for the enhancement effort was to remove both these limitations as well as to provide an easier to use, dialog based (as opposed to using KF routines which required strict formatting rules) interface.

That being said, since you mention that you're linking Attributes between multiple part files, when selecting a Component's Attributes, if you're actually going down to the original Master Model part file to reach the Part Attributes you may have to use interpart Expressions to link these parts with the Drawings where the Notes are. However, if you are actually linking to the Object Attributes of the Components in the Master Model Drawing, this should not be necessary, however in that case it will now depend on making sure that if you're making changes at the detail (Master Model) part file, that these changes are propagating up to the Master Model Drawing as well.

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
Siemens PLM:
UG/NX Museum:

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

RE: Part attributes not updating with dimensional change

Hi,
Please try Update for External changes too.In case the association somehow follows the same route as K.F then this should do.I experienced the same while updating expressions driven through external source (let us assume an excel sheet).
In case possible could you please attach a snapshot too.
Best Regards
Kapil Sharma

RE: Part attributes not updating with dimensional change

(OP)
just tried Update for External changes, but still doesn't work.

I am creating these refrences in nx8 and they are in the format <WRef1*0@pn>. in earlier version they had a series of digits before the @ symbol. The odd thing is that these attributes update fine without a problem, but if I make any sort of dimensional change to the model somehow they don't update. If I go to override attribute, then delete it then they start updating like they should. Could this be a bug in version I am running?

RE: Part attributes not updating with dimensional change

Could you provide a simeple set of parts where this problem is manifesting itself?

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
Siemens PLM:
UG/NX Museum:

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

RE: Part attributes not updating with dimensional change

First a disclaimer: I tested these parts in NX 8.0.3.4, which will be ready for download very soon.

That being said, everything appears to working as expected. Now I suspect that I might see what has happened.

With NX 8.0, when you select a Component from the Assembly Navigator and you select the 'Properties' option and select the 'Attribute' tab, please note that there is a list of options at the top of the dialog titled 'Object Selection'. This allows you to assign/edit attributes to the various manifestations of a Component in an Assembly, in this case a Master Model Drawing. Note that there are 4 options including the ability, if you have Write ownership, to edit/create attributes on the Component's Master Part Model, something that prior to NX 8.0 you could only do from within the Master Part Model itself. One of the other options is to edit/create attributes on the 'Occurrence' of the Component in the assembly. Now under normal conditions, when you select a Component while in an assembly, you are selecting the 'Occurrence' of that component and therefore when you create a note on your Drawing which is using value of an Attribute, it's the Attribute which was assigned to the 'Occurrence'.

Now in your example, there are 4 notes on your Drawing. The one near the 'top' of the Drawing is linked to the Attribute assigned to the Component's Master Part File, while the other 3 notes are linked to the Attribute assigned to the 'Occurrence' in this particular Assembly (Master Model Drawing). What has happened is that Attribute edited on the 'Occurrence' is actually overriding the Attribute inherited from the Master Part Model. Now you can see that that has occurred by looking at the 'Inherited' column in the Properties 'Attribute' tab dialog when the 'Object Selection' is set to any option OTHER than the 'Apply to components as part attribute' option.

Anyway, if you edit the Part attribute of the component, the note near the top of the Drawing sheet will update. If you edit the Attribute assigned to the 'Occurrence' of the Component, then the other 3 notes will update.

So take a look and see what I'm talking about.

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
Siemens PLM:
UG/NX Museum:

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

RE: Part attributes not updating with dimensional change

(OP)
Right now that top note is linked to an expression, and it is a bit more complicated and time consuming to use IMHO.

I am seeing what you mean by occurence. Is there a way to link an attribute from a part loaded in the file so that it updates using an object attribute? If so then how. What would be the best way to get the attribute information from the master part so that the note in the drawing changes with any update.

RE: Part attributes not updating with dimensional change

You've already found the solution.

This is one of the reasons for the NX 8.0 attribute project, to more closely link Attributes and Expressions since we already have ways of linking expressions up and down an assembly tree. Once you make it easier to link attributes expressions, you can now leverage the tools already in place that supports expressions. It's better to leverage what's already there than to reinvent the wheel (by adding a second scheme just for linking attributes up and down the assembly tree.

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
Siemens PLM:
UG/NX Museum:

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

RE: Part attributes not updating with dimensional change

(OP)
Thanks for taking the time to explain it all to me. Definately learned a lot more about attributes. I just wish there was a different result.

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