I would like to export a parasolid, which contains names of surfaces and parts. How should this be done? At this moment, when I export solids as parasolid, the names don't appear when opening the parasolid in 3rd party software.
Currently using NX 9.0 and NX 10.0.
Solved! Go to Solution.
I mean feature names from the part navigator. I.e. if I sew together 6 surfaces to become a solid cube, I want to name these surfaces ‘front face’, ‘ back face’. ‘right face’, etc. and export these names to the parasolid.
Name the faces in the component part, ie set the selection filter to "face", select them, and then right click properties. On the General tab, enter the name. Ok, and save the part.
This is how we get named faces from NX into Star CCM+ via parasolid.
A couple of hints that you probably already know, but just in case...
To see the names assigned to the faces, select "Menu > Preferences > Visualization" and select the Names/Borders tab. Change the "Show Object Names" from "Off" to one of the remaining options ("View of Definition", "Work View" or All Views").
If you don't want to set the Selection Filter to face each time, learn to use the top selection priorities. In this case, hit 'Shift + G' to make top selection priority "Face". Select "Menu > Edit > Selection" to see the list of available options.
Thank you Dave for providing the answer to my question, and thank you Ben for the extra hints! In reaction to your hints: Is there a way to obtain a full list of all faces? This allows me to check if I named all faces properly.
(I expected these to show up in the part navigator, but I assume only the features are shown here, not the faces themselves; I'm still getting used to the solids way of modelling, as opposed to the Rhino method that I'm familiar with. )
Select "Menu > Information > Object", change your Selection Filter to "Face" and rectangle select the geometry you are interested in to obtain a list of faces and their names. Unfortunately there's *a lot* of information returned regarding each face. I suspect what you need is a program to highlight faces that have not been named. @cowski1 might be able to help you with that, or at least tell you if it's possible.
One easy thing to try is to (temporarily) turn on object names: menu -> preferences -> visualization -> names/borders -> show object names (try the "work view" option). If the display object itself (body, face, edge, etc) has been named as outlined by @DaveK, the name will appear in the graphics window somewhere close to the object.
edit: whoops! I quickly scanned through the thread and didn't notice that @BenBroad had already suggested this.
Note that changing the feature name in the part navigator does not automatically transfer that name to the faces/objects the feature creates. If you want to transfer names via a parasolid file, the object itself must be named (as features are not included in a parasolid file).
It wouldn't be too difficult to create a small program that highlights or colors faces that do not have a name and/or generates a report of faces and their names. It should even be possible to name face objects according to the feature name that creates them (if needed). Let me know if any of this sounds useful and I can get something going when I have time.
I think I may have a non-program solution...
Selection Filter: Face
Menu > Information > Object
Other Selection Methods > Select By Name: * <-- enter an asterisk
Invert Selection (all unnamed faces are highlighted)
You could similarly use the same method with Edit Object Display to temporarily color faces that have not had names assigned.