Hi :
   The functoin called surface_based feature , you can find it in the Part Design workbench. In it, you can get four icon , Split , Close , thickness and sew , that the function you need.

Hello,

I was looking more in terms of if you create a box(cube) using surface function under wireframe and surface module and then want to covert those 4 surfaces that create an enclosed volume into a solid part.  Thanks in advance.

qpublic,

As 13910634301 advised, you want to use the CLOSE feature to convert your 4-sided surfaced box into a solid.  CLOSE will automatically close up both open ends and give you the six-sided solid.  Another way to do it is in the Part Design workbench, using the top menu INSERT + SURFACE-BASED FEATURES + CLOSESURFACE.

By the way, CLOSESURFACE will also convert a fully surfaced (6-sided) box into a solid, as long as you JOIN all the surfaces together to create the enclosed volume. Although I'm not sure why you would want to go through the extra effort if your part is a simple box.

Jack

Hi qpublic:
   We can close the surfaces into solid in the part design , but remember first you should join all the surfaces you created together , and then close the joined surface . Maybe it's why you can't close it.
    Good luck

    Chen   

...also, all the 'ends' of the open surface(s) will need to be co-planar...
...(which, if it's a box, they will be, but then, why would you do it that way... :^ )
...(ie, the 'solidising' function ['close feature'] won't smooth a 'free-form patch' thro non-coplanar ends of [joined] surfaces,  - that's my experience so far!)

steve

Hello All,

Thanks for your valuble input... and just to put the mystery to rest:) the box example was just so I can get started with something, the actual geometry is a lot more complicated.  Thanks once again.

Need help with this issue please.  I have a sweep that is just a tube.  I used "FILL" to close both ends of the tube.  Then I joined them all (SWEEP, and 2 FILLS).  Then used "CLOSE".  Then I started to make cutouts to the solid tube.  Problem is, whenI shade it the "open body" surfaces are not trimmed.  It is like I have two of the same surfaces.  Please help.  Thanks Much!!!

Mike

HP UNIX V5 R8

hide the open body, so the surfaces are not displayed and you only see the solid

Thanks Jackk, that worked!  Is that how you deal with the surfaces you used to create the solid? When I export this part via igs to send to a tool shop that does not have catia, all the surfaces are sent.  How would I hide them in this case?

Thanks Mike

Mike... that would depend on which CAD system (or viewer) the tool shop is using. Most have capabilities to hide by geometry type, layer, color, etc. But the real problem is that IGES typically doesn't handle solids very well. I know that CATIA V4 converts solids to surfaces for IGES transfers. (I'm not sure what V5 does) I'd suggest you run a couple test transfers with your tool shop and try putting stuff in different layers before you send it. I'd also suggest you try STEP because it does handle solids   ....Jack

PS: from your description of the tube you designed, I'm curious why you are using surfaces to begin with. I think you can model it directly with solids.

Thanks again Jack.  The part is a headrest rod for a seat headrest. I used the surface sweep pick.  Is there there a solid sweep pick?  Thanks agian for you help, have a great weekend!!

Mike

Hi Mike
I understand you want to export only the parts which are shown and not the parts which are hidden. here is a option
go to tools>Options>Compatibility>IGES>and switch on Save only shown entities. this will save only the parts which are shown. so u may hide all the unwanted entities and save the file as IGES.
Hope this helps

Cheers
Ganesh.N
ganesh.n@engg.tjc.co.in