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.
Dan
Dan's Blog
Dan
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Simple Surfacing Woes 2
- Thread starter Eltron
- Start date
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1
- #2
Pick only the 3 surface lofts, then select surface-knit, and check the "try to form solid" box. The other features are already solids.
Chris
SolidWorks 09 SP4.1
ctopher's home
SolidWorks Legion
Chris
SolidWorks 09 SP4.1
ctopher's home
SolidWorks Legion
- Thread starter
- #3
Dan,
I tried it and seem to work. Do you get an error?
Chris
SolidWorks 09 SP4.1
ctopher's home
SolidWorks Legion
I tried it and seem to work. Do you get an error?
Chris
SolidWorks 09 SP4.1
ctopher's home
SolidWorks Legion
- Thread starter
- #6
The knit works just fine, but no solid is created. Take a section through your model, and you'll see what I'm talking about. Plus there is a surface body listed. I'm trying to get this guy into a single solid piece so I can print it up. Why are the simplest things the hardest, anyway?
Dan
Dan's Blog
Dan
Dan's Blog
I see it now.
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
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
- Thread starter
- #8
That's what I ended up doing, too. I think there's something wonky at the edges where the surfaces meet the solid on the ends. If you zoom in on the edge after you do the up-to-surface extrude it's not a smooth curve. It'll do for now, but I would like to know why it isn't exact.
Thanks for looking at it, Chris.
Dan
Dan's Blog
Thanks for looking at it, Chris.
Dan
Dan's Blog
Dan,
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
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
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1
- #10
KevinDeSmet
Computer
What a great model, it's simple models that seem to fail like these, that are great to learn from.
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...
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)
You can see this by using Tools -> Sketch Tools -> Face Curves...
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?
Check off "Optimize Surface" which might as well be called "Make surface awesome".
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.
Hope this helped!
Kevin
TDE Technologies
CSWP-Surf
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...
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)
You can see this by using Tools -> Sketch Tools -> Face Curves...
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?
Check off "Optimize Surface" which might as well be called "Make surface awesome".
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.
Hope this helped!
Kevin
TDE Technologies
CSWP-Surf
One thing I have done to see where the problem is at is to export the file to Parasolid and bring it back in. Sometimes that will tell you what and where the problem is. Its fool proof, but it works about 90% of the time.
Regards,
Scott Baugh, CSWP![[pc2]](/data/assets/smilies/pc2.gif "[pc2] [pc2]")
Regards,
Scott Baugh, CSWP
faq731-376
If the resulting knitted surface is completely enclosed, you can use Thicken to create a solid body. If the surface is enclosed, there will be an option to "Create solid from enclosed volume" (instead of just a shell).
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.
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.
- Thread starter
- #14
The solution Kevin posted above worked well. However, I didn't use the Delete Face option. I just included that face as part of the Knit, and she worked fine. This forced me to do a Combine of the two resulting bodies, but that's no big deal in this case.
Dan
Dan's Blog
Dan
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