Simple Surfacing Woes
Simple Surfacing Woes
(OP)
OK. I know it's getting late, but what am I missing here? Why can't I knit these simple surfaces into a solid? It's got to be something silly, I know.
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RE: Simple Surfacing Woes
Chris
SolidWorks 09 SP4.1
ctopher's home
SolidWorks Legion
RE: Simple Surfacing Woes
Dan
www.eltronresearch.com
Dan's Blog
RE: Simple Surfacing Woes
I tried it and seem to work. Do you get an error?
Chris
SolidWorks 09 SP4.1
ctopher's home
SolidWorks Legion
RE: Simple Surfacing Woes
Chris
SolidWorks 09 SP4.1
ctopher's home
SolidWorks Legion
RE: Simple Surfacing Woes
Dan
www.eltronresearch.com
Dan's Blog
RE: Simple Surfacing Woes
I have had the same problem.
For your model I added an extrusion inside the surfaces.
I wish there were an easier way.
Chris
SolidWorks 09 SP4.1
ctopher's home
SolidWorks Legion
RE: Simple Surfacing Woes
Thanks for looking at it, Chris.
Dan
www.eltronresearch.com
Dan's Blog
RE: Simple Surfacing Woes
You're welcome.
I complained to my VAR a couple weeks ago and the 2010 roll-out about surfacing. They sort of shrugged it off.
It seemed that other areas are more important to them than surfacing. Ugh...
Chris
SolidWorks 09 SP4.1
ctopher's home
SolidWorks Legion
RE: Simple Surfacing Woes
My guess is that it is not solidifying because you have left the original surfaces of the solid, delete the back face of the solid first by using Insert -> Face -> Delete...
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Then build as usual, until you build the end cap faces.
Lofting a less than 4-sided surface like this is usually discouraged because it causes a degeneracy by collapsing an edge (surfaces like being 4 sided)
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You can see this by using Tools -> Sketch Tools -> Face Curves...
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You see the U-V flow lines coming to a point and bunching up there, potentially bad situation, although here I don't less than four sided faces with Fill Surface.
This is the default right?
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Check off "Optimize Surface" which might as well be called "Make surface awesome".
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Solidworks automatically overlays a 4-sided surface and trims back. I believe Solidworks is just about the only software that does this so well!! (not to sound to much like an infomercial here)
Then simply Knit them up "try to form solid" and you're done!
Then, just for kicks, take a look with View -> Display -> Curvature and you'll see it's a nice smooth tangent continuous solid, probably quite good for engineering.
http://i
Hope this helped!
Kevin
TDE Technologies
www.kevindesmet.com
CSWP-Surf
RE: Simple Surfacing Woes
RE: Simple Surfacing Woes
Regards,
Scott Baugh, CSWP![[pc2] pc2](https://www.tipmaster.com/images/pc2.gif)
FAQ731-376: Eng-Tips.com Forum Policieswww.scottjbaugh.com
RE: Simple Surfacing Woes
You might also try extending your suraces and re-trimming them to be sure they intersect properly.
Another trick is to use a face fillet to cover any funky edges, then use Delete Face to remove the fillet and force the edge to reconstruct.
RE: Simple Surfacing Woes
Dan
www.eltronresearch.com
Dan's Blog