Why can't I manipulate parasolid geometry? 2

[Miyamoto12]

Probably a dumb question, but why can't I do simple things like trim/unite geometry from a parasolid? I can't even export it to .prt as it won't highlight when I try? Are they technically sheet bodies instead of a solid is that why?


Thanks,

-Xh

NX 10

 

[cowski]

You will be able to use good geometry from a parasolid file. I suspect that your parasolid geometry either has errors (you can check this with the 'examine geometry' command) or perhaps it is a facet body. Support for facet bodies is getting better in NX, but they are still among the worst geometry to work with.

www.nxjournaling.com

 

[Toost]

place the cursor on top of the object, pause the cursor until you get the three "..." next to the cursor, then click
The list will tell what type of objects you have. ( solids / sheets etc)

You should be able to export, no matter of the type.
Can you press "Ctrl+I" ( information - Object, hidden in NX10... ) and then select the object ?
can you snap a endpoint ? - Try Information - Point and snap an endpoint.

What NX version ?


Regards,
Tomas

 

[Miyamoto12]

Thanks for the replies. There were a few minor issues in the examine geometry process, but my understanding is that the tool lets you know of the locations, but doesn't have any autofix or anything. I suppose I could run optimize, but I don't think that will help me. I'd like to just split the model in half, but it won't actually let me select it! this is the info box, what part am I interested in? The quick pick menu doesn't help me much either. See att picture. It shows me both the yellow box AND the blue, how could it be both?

Name 1745-WFEEDERS_ID10_X_T
Owning part P:\................................................\-wfeeders_x_t.prt
Comp member in part P:\..................................................\wfeeders_id10_x_t.prt
Layer 1
Type Component

Color 134 (Medium Royal)
Font SOLID
Width 0.70 mm
Modified Version 1 04 Oct 2016 10:19 (by user kxh03)
Created Version 1 04 Oct 2016 10:19 (by user kxh03)
Actual Color 134 (Medium Royal)
Component Reference Set Name None

Component Translations:

Delta X = 0.000000000
Delta Y = 0.000000000
Delta Z = 0.000000000

Component Rotations:

X-axis Vector XC = 1.000000000 X = 1.000000000
YC = 0.000000000 Y = 0.000000000
ZC = 0.000000000 Z = 0.000000000

Y-axis Vector XC = 0.000000000 X = 0.000000000
YC = 1.000000000 Y = 1.000000000
ZC = 0.000000000 Z = 0.000000000

Z-axis Vector XC = 0.000000000 X = 0.000000000
YC = 0.000000000 Y = 0.000000000
ZC = 1.000000000 Z = 1.000000000

Component is Unconstrained

------------------------------------------------------------
Object dependency information is unavailable.

------------------------------------------------------------

INTEROP_FEATURE_LAST_UPDATE_GMT = 4-Oct-2016 17:12:49 (String)
INTEROP_FEATURE_PART_NAME = solid (String)
INTEROP_FEATURE_AUTHOR = Parasolid (String)
INTEROP_FEATURE_ID = solid (String)
NX_MaterialMissingAssignments = TRUE (String)
NX_MaterialMultipleAssigned = FALSE (String)



NX 10

 

[cowski]

It appears that you are working in the context of an assembly. The yellow box represents the component object and the blue box represents the body object in the component. To operate on the geometry, you will need to make the 1745-WFEEDERS_ID10_X_T component the work part (or make it the displayed part).

www.nxjournaling.com

 

[Miyamoto12]

Great, thanks. I need to spend a little more time in the help docs. btw you're site helped a bunch when I started here!

NX 10

 

[Toost]

When you have a parasolid file, there are two options in opening it.
1) File-Open- type= parasolid
and
2) File - import - parasolid

If the parasolid file has "structure", ( = is an assembly) method 1 will recreate the assembly, whilst method 2 will import everything into the work part.
- the structure will disappear. all bodies will be in the work part.


Regards,
Tomas