Display tolerance as column in part navigator? 1

[CNSZU]

Hello all,

Sometimes I tighten the tolerance for specific features to increase the accuracy of surfaces, other times I loosen them to enable features to work. However, recently I ended up with a solid body with strange jagged edges which failed to export as a solid in a STEP file. This indicates some tolerances are too loose. The details pane at the bottom of the part navigator does not display tolerances, so to solve the problem I had to open every feature to see which tolerance was too high (because I couldn't remember which features I had changed the tolerances).

To make this easier, is there a way to display the tolerance of each feature in a column in the part navigator? Or a command to give a listing of all features with tolerances?

NX8.5 Win7SP1 64bit i7-3770K@4.3Ghz 16GB Quadro2000

 

[JohnRBaker]

You understand of course that some features have no tolerances set for them and even some that do, in many cases the set values have no impact on the results, it's only when an approximation has to be made that the Modeling tolerance ever comes into play. But in any case, while the tolerance values are captured as part of the definition of a feature (if it's relevant) they are not storted as parameters (expressions) like the other parameters used to numerically define a feature and therefore are not accessible by any of the interactive tools other then when editing the feature using the normal edit dialog. It might be possible to create an NX Open program which could go into a part model and extract the tolerance values used by each relevant feature, but that's about the only approach that I can think of to get the information that you're looking for in an accessible format, such as an Object Attribute assigned to the feature which could then be displayed in the Part Navigator.

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.

 

[cowski]

Check your solids with the "examine geometry" tools before you attempt to export them.

www.nxjournaling.com

 

[CNSZU]

Thank you John, I've already created a journal that creates a listing window of all the features and any tolerance values. However, I've encountered a problem. I do a Select Case for every feature according to the FeatureType. But Swept and Ruled Surface both are of the feature type "SKIN". What should I do to tell these two features apart? Also, you mentioned a method to create object attributes which can be accessed in part navigator. How does this work?

NX8.5 Win7SP1 64bit i7-3770K@4.3Ghz 16GB Quadro2000

 

[CNSZU]

Thanks cowski, I'll remember that next time.

NX8.5 Win7SP1 64bit i7-3770K@4.3Ghz 16GB Quadro2000

 

[JohnRBaker]

When you select a feature, press MB3, select the 'Properties' option and then the 'Attribute' tab. Now you can assign an Attribute to the selected feature. Note that you MUST name all of the 'tolerance' attributes that you assign to each feature the exact same name. Then open the part Navigator, press MB3 over some 'white space', select the 'Properties' option and then the 'Columns' tab. At the bottom of the dialog enter the name of the 'tolerance' attribute that you assigned to the features. Now you will have a column in the Part Navigator which will show the value of that Attribute for each feature.

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.

 

[CNSZU]

Thanks John, I got it.

NX8.5 Win7SP1 64bit i7-3770K@4.3Ghz 16GB Quadro2000