Create a "Dummy" Part

[LAWilson]

I have a large sheet metal assembly model that I have spent many hours on and it contains proprietary engineering information. My customer is requiring a model to use for fit up. I do not want to send him a model that he can “easily” reverse engineer. Is there a way I can package this assembly so my customer can not separate out all of the sheet metal parts and obtain their properties? I want to send them a dummy model that acts as one large conglomerated part. They want this file in x_t format which can easily be done with solid edge, but I know when I open a parasolid assembly it creates parts that I can easily convert to sheet metal and unfolded.

Any help would be greatly appreciated.

 

[CorBlimeyLimey]

SolidWorks can save an assy as a part with exterior surfaces only; does SE have a similar function?

 

[beachcomber]

Hi,
Depending on the complexity of your assembly you may be able to do a "Insert Part Copy" into a part file then export the result as x_t.
You may get problems if the assembly has complex interfaces such as edge-to-edge contacts.

bc

 

[jlbmech]

Try this.

Do a save as "parasolid doc. x_b* x_t*"

It will do one of two things...
a) save model assemb. as a solid body feature.
b) save part copies of parts but still maintain secrecy.

hope that helps.

SE v18 SP7 WinXP SP2

 

[KENAT]

For simple geometry what beachcomber says works very well.

However, SE do not recomend it, I guess because it only works with 'simple geometry'.

Look at simplified assemblies. As I recall you can turn a simplified assembly into a part, though with pretty much the same limitations as Beachcombers idea.

KENAT, probably the least qualified checker you'll ever meet...

 

[beachcomber]

LAWilson,
Can you give some idea of what the assembly is and what info you want to remove.
As far as I know, creating a parasolid or step file will remove intelligence, but will still give individual part definitions within the assembly. When you open a step or x_t file in edge you get the option of creating a single part file or creating an assembly with all the parts in it.
However, the destination cad system might not have the second option.
I'd forgotten about Simplified Assembly.
That is definitely worth a try as it makes a single body that you may be able to export.

bc

 

[LAWilson]

beachcomber,

Thanks. It took over 1.5 hours to process, but inserting a part copy worked....Only, if I might add, if you uncheck the link to file option during the insert copy dialog. If you leave the copy linked for some reason the parasolid will explode all of the piece parts.

Sincerely,
LAWilson