Removing part of a body

[ArmoredSpecialtyCars]

I recently had the door of a car scanned and auto surfaced. The file came in as one body (actually 7 bodies, but 6 of them are so small they are negligible) and I would like to remove part of the body. I have highlighted the area I would like to delete but do not know if it is possible on a solid body. In case it is difficult to be able to clearly see, I want to delete the inner skin of the door. Thank you!

 

[JohnRBaker]

If it's a surface model you could create a solid body by extruding a profile just deep enough to pass through the inner face and then do a Boolean subtract picking the 'door' as the Target Body and the extruded solid as the Tool Body

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.

 

[TaylorAnderson]

So are the triangulated facets here actually BREP surfaces, then?

One option might be to just use Delete Face (Home tab, Synchronous Modeling palette in the ribbon UI, Insert --> Synchronous Modeling in the older pull-down menus).

If you want to create a clean edge near your red boundary, you might project a boundary curve and Divide Face (Home tab, Feature palette, More button, Trim group, in the ribbon UI, Insert --> Trim in the older pull-down menus) first, before deleting.

And if your inner panel is a solid with thickness, then you may want to project a boundary to both the inside and outside, divide both, delete unwanted faces from both (at which point you'll have an open sheet body), create a ruled surface between the new boundaries, and re-sew the solid closed.

Does that help?

Taylor Anderson
NX Product Manager, Knowledge Reuse and NX Design
Product Engineering Software
Siemens Product Lifecycle Management Software Inc.
(Phoenix, Arizona)