Surface blend 4

[ctopher]

I have been fighting with these surfaces.

The bottom section are surfaces, the top is an extrusion. I have tried both surface and solid extrusions.
The extrusions are from a sketch with lines 'on edge' of the edge shown.
I can not get the edge to blend properly. It is very close on the part model, but when I send it as a parasolid to the vendor for machining, the step shows. It shows for me also when I open the parasolid.
It is not only on my PC.
How do I make an extrusion from the top surface of the bottom feature to make it blend? Tangent to surface during the extrusion feature does no help.

Chris
SolidWorks 09, CATIA V5
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[ctopher]

Also, Import Diagnostics will not fix it.

Chris
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[CorBlimeyLimey]

Can you post the actual part to play with?

 

[ctopher]

Parts of it are offset surfaces from another part. The other part I can not send.
Here is the part though so you can see what is happening.
Version 2009.

Chris
SolidWorks 09, CATIA V5
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[CorBlimeyLimey]

Take a close look at BoundarySurface1. It has an anomaly which may be at least partly to blame for the mismatch.

 

[ctopher]

Thanks CBL.
I had an inkling that surface was a problem, but could not figure out a work around.

Chris
SolidWorks 09, CATIA V5
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[KevinDeSmet]

True, don't try to boundary that without making a physical edge (i.e. Split Line) to ensure contact. I used a fill with "optimize surface" checked off to have a relaxed surface.

I got it into a solid, but had some trouble with the split lines, seeing this, I guess it might be a good idea to do split lines all the way at the end of a model to avoid small misalignment issues (don't feel bad, I didn't know that either until now!!)

I also noticed non-tangency in a that very top sketch and that very top surface (with all the extend surfaces) was brutality mutilated and beaten so I tried converting edges in a 3DSketch and used Fill surface with an influence sketch, check it out.

CSWP-Surf

 

[ctopher]

Thanks Kevin.
I will change my model per your suggestion also.

I never really worked with surfaces much until two months ago.

Chris
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[KevinDeSmet]

Surfaces are definitely hard to grasp at first, the hardest thing is that they are abstract. Most solid features are analogous to real-life machining, or grinding, or lathing.

But surfacing is an abstract method of modeling, it's 'talking' to SolidWorks on a lower level. But sometimes, it's handy to do that, and surely handle to be able to do that!

I sure haven't learned everything about surfacing either, just take little chunks at a time and keep trying out a new feature every now and then, or looking something up online - I can recommend looking up how NURBS and BREP work, they're fundamentally what surfacing is all about

CSWP-Surf

 

[ajack1]

Firstly I would say we do not use solidworks as we found the surfacing option, or at least the ability of the VAR we spoke to very limited, so all the “terms” may not be correct.

However I would say it would be well worth your while to get some training in surfacing. To simply “bodge” everything with poor trimming, non tangent extensions and the like will cause you much bigger problems down the road when you try to offset, thicken a surface, produce offset cavities etc.

Surfacing is an art all on its own and the time and effort involved in learning it will pay dividends over time especially if you have to work with the dreaded iges imports from other CAD systems.

 

[ctopher]

ajack1,
I agree. I will look into training. There are some on YouTube as well.

Chris
SolidWorks 09, CATIA V5
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[ctopher]

I guess the only way to make the surfaces a solid is save as a parasolid? Knitting does not seem to create a solid for these surface, they are closed.

Chris
SolidWorks 09, CATIA V5
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[ajack1]

For the reason mentioned above the terminology may not be correct but just because they are knitted does not mean they will be a solid. A solid needs to be watertight, knitted surfaces do not.

Especially on imported data you may find the closer tolerance causes havoc, especially if the surface tolerance and the wireframe tolerance are different, you can end up with slithers and small gaps everywhere and non tangent surfaces will not off set and close.

It really is worth getting some training.

 

[KrisCADD]

Yes, surfaces can be difficult at times. I usually have to come up with some work-around. It's good to know other approaches to a surfacing problem, and better knowledge of the software definitely helps in these cases. Its seems like the higher capabilities of Solidworks, such as splines and surfacing etc., you start to see more bugs in the software, therefore require more work-arounds.

-------------
Rancho Cucamonga, CA
Solidworks 2009-2010
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[dgowans]

ctopher,

A fully knitted surface does not necessarily make a solid body in Solidworks. When performing the knit operation, there is an option to try to form a solid at the same time. If you already have a single closed surface body you can try to form a solid via Insert, Boss/Base, Thicken and checking the option to form a solid from a closed surface (or something similar). If you have a closed surface and can't form a solid body with either of the above options you may have geometry errors/issues preventing the solid body from being formed. That will undoubtedly prove to be a huge pain if you truly need a solid...

 

[ctopher]

dgowans,
The "Insert Boss/Base, Thicken" worked great!
The step is gone.
Thank you!

Chris
SolidWorks 09, CATIA V5
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[kellnerp]

It is helpful to review the curvy stuff tutorials by Ed Eaton. This problem is explained, I think, in the 2005 SWW presentations.

Curvy Stuff

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[ctopher]

Thanks kellnerp.

Chris
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[Theophilus]

Chris, let me know how you're doing on this part (email if you like). There are a couple of things I'd do differently in building this with surfaces by rolling back and trying some other methods. Some of the surfaces seem a bit stressed the way they are, but we can use lofts/fills to re-create them in a more robust way if you like.

Fixing this would likely take about 20-30 minutes, depending on what is critical (vs. what isn't critical). One thing I'd recommend is building half of this along the axis of symmetry, and then mirroring the knitted solid body (when the half is complete). Knit the two halves with the option to create solid, and you're finished.



Jeff Mowry

http://www.industrialdesignhaus.com

A people governed by fear cannot value freedom.

 

[kellnerp]

You are welcome.

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