Assembly EXPORT to customer

[GPowers2]

Magic button time
or a slick process required
I have an assembly of NX parts and have a requirement to export the external detail ONLY to a customer using a altenate CAD package [non parasolid based] (I am happy to consider STEP). I would also like to not show the internal detail. and to add more of a challenge solids would be nice, rather than a shell. I am sure this is not a crazy request and that someone out there has passed this way before. I am using NX7.5.3.3 MP1 but am a little new to some functionality and maybe missing a trick.

help would be appreciated

Gary
aerospace

 

[looslib]

Copy your assembly, promote the bodies and unite them. Then do your STEP export of a single body that will in theory only be the space envelope.



"Wildfires are dangerous, hard to control, and economically catastrophic."

Ben Loosli

 

[GPowers2]

? - question : will that actually suppress the internal detail of the parts ....

 

[looslib]

No, but depending on how complex the internal shapes are that you want to hide, you may need to add some blocks at the assembly level inside your assembly to unite and mask the details.
The STEP file will only have the shape, no construction details.


"Wildfires are dangerous, hard to control, and economically catastrophic."

Ben Loosli

 

[GPowers2]

Hello Ben ... I am looking for something a little smarter and less labour intensive and need to make sure that there is absolutely no other option before i embark on that process .... let me know if you have any other ideas ..

thanks for your thoughts

gary

 

[cowski]

Search NX help for "wrap assembly" and "linked exterior". One of these commands might get you close enough.

http://www.nxjournaling.com

 

[JohnRBaker]

If you need to preserve the external shape and size, then try using...

Assemblies -> Advanced -> Simplify Assembly...

However, if yor're only looking for a conservative 'armature' to be used for space planning or 'packaging' then...

Assemblies -> Advanced -> Wrap Assembly...

...may be something you may wish to look at since it's very quick and easy to use.

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA

http://www.siemens.com/plm

UG/NX Museum:

http://www.plmworld.org/p/cm/ld/fid=209

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

 

[looslib]

Don't the Wrap and Simplify produce sheet solids when exported and not solid bodies? I was aware of those commands, but the OP asked for solid bodies in his export.


"Wildfires are dangerous, hard to control, and economically catastrophic."

Ben Loosli

 

[JohnRBaker]

NO, both Wrap and Simplify produce a Solid Body as a final result.

It's the 'Linked Exterior' which produces a series of sheet bodies which may or may not be easily 'sewen' into a final solid.

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA

http://www.siemens.com/plm

UG/NX Museum:

http://www.plmworld.org/p/cm/ld/fid=209

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

 

[GPowers2]

people,

thanks for the inputs ... i have taken a look at
Assemblies -> Advanced -> Simplify Assembly...
and that is exactly what i need . sufficient automation on the complex parts with some level of control on extactly what i ship.
thanks to all for your help.
I am all set for now

best regards ... gary

 

[vball85jb]

Simplify Assembly does not appear to be functioning in NX 8.0.2 has anyone tried it with NX 8?

 

[JohnRBaker]

For what it's worth, 'Simplify Assembly' appears to be working fine in NX 8.0.3.3, which is a development phase of what will be the next NX 8.0 MR.

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.

 

[vball85jb]

John,

Any idea when 8.0.3.3 will be released?

 

[JohnRBaker]

Actually NX 8.0.3.3 will NEVER be released.

The MR will be NX 8.0.3.4

As for when it will be released, it should out by the end of summer.

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.