Drawing attributes NX6 1

[jerry1423]

I am working in master model in NX6.
When I am in the drawing file ANT, and click on the model file, and do properties > attributes
I get the picture that is attached. Some of the attributes have an icon to the left of them, and others don't.

Why is there a "sheet" icon next to some of the attributes, and not the others?

I reason that I am asking is because one of my attributes is not updating, in the drawing, after it is changed in the model file.

 

[jerry1423]

oops, I the attachment didn't work the first time

 

[JohnRBaker]

First thing that you need to understand is that when you're in an Assembly and you select a Component and check it 'properties' that the Attributes that you see, irrespective of any special symbols or icons, are THE attributes that ALL NX functions will assume have been assigned to THAT COMPONENT 'object' which resides inside of THAT Assembly. Please don't confuse this with what you might see if you were to open just that 'component' as a detailed (master) part file.

OK, now that this is understood, lets look at what the symbols mean. First the 'sheet' icon, which actually is the symbol for 'file' (which may help in this next part of my reply), is indicating that the 'value' of this Attribute, as seen by the Assembly, is inherited or 'Comes from' the original master model part file (that's what the little up-pointing 'arrowhead' at the upper-left corner of the 'sheet icon means, it's 'coming UP FROM the original Part file'). That is if you were to open the detailed part file and go to Part -> Properties... that you would see these same exact attributes and their values would be identical.

Now if you don't see the 'sheet' icon (it's plain) it could mean one of two things. Either that Attribute was ADDED to the COMPONENT 'object', at the Assembly level, as an Object Attribute, OR it was edited at the Assembly level and the value has been changed from what it originally was. Now there's no easy way to tell if the Attribute was edited or added, except that if you 'delete' an edited Attribute it will revert back to the inherited values and the 'sheet' icon will reappear.

Now there is one other type of icon and that's one that shows a small 'box' (instead of a 'sheet') icon with an up-point arrowhead. What this means is that this Attribute is being inherited from the Reference Set and not actually from the orignal detailed (master) Part file properties. Again these can be edited at the Assembly level and they too will 'lose' their icon.

Now how these Attributes can be used it for example, I might have an Attribute 'Material' assigned at the detailed part level as a Part Attribute, but then have two different Reference Sets, each with an Attribute 'Finish' assigned, one set to 'Nickel-Plated' and the other to 'Zinc-Plated'.

Now as for your 'problem' of someone editing an Attribute in the detailed Part file and it does NOT change in the assembly, this could be due to one of two situations. Either, there is a Reference Set specific Attribute which is OVERRIDING (because this is what they do and why we implemented this stuff the way we did) the original Part Attribute (but then you should have seen the 'box' icon), or, which is more likely, someone manually edited one of the Attributes with the 'sheet' icon and therefore it has also OVERRIDDEN the original Part Attribute. Now if that is what happened, then it's working exactly as it was designed to work since this is the scheme we provided to ALLOW you to OVERRIDE Attributes at the Assembly level for special situations.

Anyway, with this new understanding of what's actually happening, take a second a look at your Assembly and see if you can see why you're seeing what you are, OK?

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

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