How do you use delete face in place of simplify body?

[DesignIntent]

Hello,
I need to understand how to remove very complex interiors (containing thousands of faces) from solids using the delete face function.
I became very dependent on the older simplify body feature, with which I was blindingly fast, and now can't seem to find the corresponding methodology in the delete face dialog.
I've tried to use the cap face option but it only lets me select one cap face and then it is not clear to me how to indicate what interior faces I need to remove.
Do I do it by indicating a region to remove?
If so, even that is not intuitive to me.
Can any one help me understand how I can end up with a simplified (filled-in) solid body?
I am asked to work with many customer supplied cylinder head, engine block and turbine casting models which are always supplied to me in STEP or Parasolid formats and therefore have no features.

Thanks in advanced.
DI

 

[JohnRBaker]

What version of NX are you running?

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.

 

[KhimaniMohiki]

Use delete face, select the faces using Region Faces from the selection bar, select one of the interior faces as the seed face, then the cap faces as the region boundary, this will select and delet all the faces between the seed face and region boundary.

Khimani Mohiki
Design Engineer - Aston Martin
NX8.5

 

[DesignIntent]

Sorry John, I should have stated that I am using NX8.

 

[JohnRBaker]

What KhimaniMohiki described is the workflow which will basically duplicate the functionality of the old 'Simplify Body' function and it should work fine.

However, since you've using NX 8.0, you now have an alternative that you might want to look at if you're having problems doing it the 'conventional' way (as described previously). There is a new option in the 'Settings' section of the 'Delete Face' dialog called 'Heal'. Now by default this is toggled ON so as to retain the old Delete Face behavior, but thanks to our customers who migrated over from Ideas, they convinced us to add an option so that 'deleting' a face actually DELETED the face. That is it would leave a 'hole' in your model where the selected face were removed if this 'Heal' option was toggled OFF. Anyway, the alternate approach would be to literally DELETE all of those 'interior' faces and once they've all been removed, simply create the necessary sheet bodies using functions like 'Bounded Plane', 'N-Sided Surface', 'Through Curve Mesh' etc. to close-off the openings in your model and then sew it all together to make your final 'simplified' solid body.

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.