strategies to excluded developmental geometry from automated ( batch) step files 2

[RonnyC]

Hi All,

We are using batch conversion prt -> step to create step files for internal and supplier needs.

We sometimes encounter issues where developmental geometry is converted together with the actual part geometry, which can be confusing.
So I'm looking for possible strategies to streamline the batch step creating functionality.

- obviously, having a dedicated layer for developmental geometry, and excluding that layer would work
Unfortunatly, because of historical reasons and conflicting layer rules for different customers this is not the case.

- For assemblies, when component developmental geometry is not included in the ref-set, this data is not in the assembly step file
Unfortunatly, step files created at singlepart level include all geometry regardless of ref-set status.
is there a way to tell NX to exclude non-ref-set data ??

- any other strategies are welcome..

thanks,
Ronny

 

[JohnRBaker]

If the so-called "developmental geometry" consists of either Solid or Sheet Bodies, there is a step that you could start doing as part of your regular modeling workflow. Just before you consider you design models complete, simply use the 'Delete Body' function to 'remove' these referenced bodies from the history of the model. In this way they will no longer be seen by the system when exporting your models as IGES or STEP files.

Note that this is NOT the same as actually deleting the Bodies from the data record of the model, however by using this relatively new (introduced in NX 8.5) 'Delete Body' function it's as if the Bodies no longer exist yet it has NO effect whatsoever on your final design model even if those bodies had been used during some previous modeling operation, like a Trim or an Extrude To, further back in the 'Timestamp Order' or history of your model. And later on, if you ever need to have these 'deleted' bodies made available again, all you have to do is simply Suppress the 'Delete Body' feature(s) and they will be 'resurrected' and available once more for whatever use that you need them for.

Anyway, give it a try and see if this addresses your issues for you.

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

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

 

[RonnyC]

Hi John,

great tip, that can indeed be usefull to "correct" historical models

thanks

Ronny

 

[PrintScaffold]

You may take a leaf out of the book of Top-Down strategy. One of the features of this strategy is to keep development and resulting geometry in different prt files. In a nutshell, you build a part in 1.prt, and then WAVE-link the resulitng body into 2.prt.

http://www.cadroad.com

 

[jerry1423]

You can specify what layers to include (or not include) in your STEP translation.
So therefore not include certain geometry if in a certain layer.

 

[RonnyC]

Thanks for your reply everyone.

Just wondering, Is there a way to convert only the visible items in a prt file ( in batch mode ofcourse )
Maybe as a script which first extracts the visible layers of the prt file and restricting the conversion-layers to those?

I 'm a complete novice at marco's/journal/grip/NX-open so don't know if it is possible at all.

thanks

Ronny

 

[RonnyC]

by the way : a " convert-only visible "-option in the translator menu would be a good add-on for future NX-releases.
I understand it is an available option in Catia

regards