Adding weitgh to a table (drafting) in UG 5 1

[BEAEROHEAD]

I need to add the weight of a part to a unigraphics NX5 dwg table. I can extract expressions and attributes, but I can't find a way to link the weight field from the properties.Got it to work in NX2 but not 5.

 

[JohnRBaker]

If you wish to do weight only, open the part model and select...

Tools -> Expressions...

...and and then go to the bottom of the dialog and select the Measurement option and select Measure Bodies and select the model and hit OK (you will probably want to edit the name of 'weight' measurement to something like 'Weight' so that it will be easier to find later on.

Now open your drawing and if you already have your Tabular Note created, just select the desired 'cell', press MB3 and select 'Style' and under the 'Cells' tab you can decide what sort of format that you wish (for numerical data you can use either Text or Number, the difference being where and how you control the number of decimal places) and if you wish any prefixes or suffixes be added to the value in the cell. Now hit OK and once more select the 'cell' and press MB3 and this time select 'Edit Text' and then select the 'Relationships' tab and then select the 'Expression' option. Now if you working with a Master Model drawing, you will need to select the 'Link to Part' button and select the component to get the list of available Expressions. Anyway, select the desired expression, which I had suggest that you name 'Weight' (if you had selected the 'Text' type for the cell, then you will need to set the 'Format' in this dialog to control the number of decimal places, but if you selected the 'Number' option than you will control the decimal places back in the Cell 'Style' dialog) and hit OK. Now you can also add any additional text here in the Annotation editor if you wish or just hot OK once more and you're done.

Anyway, that should do you.

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

http://www.siemens.com/plm

http://www.plmworld.org/museum/

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

 

[BEAEROHEAD]

I don't get the Measure Bodies option. Maybe a preference thing. I keep looking

 

[JohnRBaker]

It's the second icon from left at the bottom of the Expression Dialog. It's drop-down with 5 options, the 4th one down being the 'Measure Body' option.

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

http://www.siemens.com/plm

http://www.plmworld.org/museum/

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

 

[BEAEROHEAD]

I found it and it works! I bow to your superior UG knowledge. Thanks

 

[hudson888]

Just be carefull of doing that too much as when things go out of date then the expression may fail. It works fine when it works but it has proven occasionally troublesome to maintain in the past.

Why not use a parts list and have the component masses show there? It may be what you want or maybe not. I wish that NX would also provide masses in the part list for assemblies.

Best Regards

Hudson

www.jamb.com.au

Nil Desperandum illegitimi non carborundum

 

[JohnRBaker]

Note that the Measure Bodies function returns both Weight and Mass.

As far as the updating, if you link directly to the Measurement Expressions, you shouldn't have any problems. Now if you've passed those values to an Attribute and then reference the Attribute, there could be some delay getting the last link in the 'chain' to update in a timely fashion (it will update upon saving and reopening the part, but might not update if something is changed during your current session). These update issues will be fully cleared up when we implement the new Attribute architecture in a future release of NX.

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

http://www.siemens.com/plm

http://www.plmworld.org/museum/

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

 

[potrero]

Which future release will that be?

 

[JohnRBaker]

One that will be released, in the future.

I'm sorry, but that is all that I'm allowed to say at the moment. When we get to the point where we have a better idea of both the content and the schedule of that release, we will be more forthcoming, but until then...

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

http://www.siemens.com/plm

http://www.plmworld.org/museum/

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