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creating solid part geometry from a surfaced part in V5
- Thread starter qpublic
- Start date
13910634301
Aerospace
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.
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.
- Thread starter
- #3
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
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
13910634301
Aerospace
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
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
...(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
- Thread starter
- #7
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
Mike
HP UNIX V5 R8
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
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.
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.
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
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
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