surface loft partner profiles?

[anchange]

I want to create a surface loft using the two identical profiles in sketch 1 as my starting and ending profiles. Sketch 2 is the centerline. I get an error saying that I need more then one profile. How can I recognize more then one profile in the same sketch or how can I move one of the profiles in the sketch into a different sketch but have it automatically duplicate changes made to its partner profile?

SCREEN GRAB -

http://tinyurl.com/q8lqgj

Thanks for the help!

 

[anchange]

So I realized swept might be better for what I need but it didn't work either... why? Seems to not like turning the corner on sketch 2?

http://tinyurl.com/pqs9q2

 

[ArtemTat]

Make sure you have a single segment in the Profile Sketch when creating the Swept-Surface.

I was able to create similar surface from my end.

If you still have a problems it would be the best you attach this model.

Artem Taturevich
CSWP

 

[Updraft]

You can make a second sketch that is tied to another by using "Convert Entities". When the parent sketch changes the child sketch will follow. These sketches can be on different planes, but they should be parallel for your stated situation.

- - -Updraft

 

[Theophilus]

anchange, if you're using straight segments for your sweep path, you'd probably find creating this surface is simpler with basic Extrusions. Extrude past each edge of each surface and then Trim the surfaces.

With sweeps, having a sharp change in the path (no radius) like you've shown will always cause self-intersection of a concave profile like you've shown--so it cannot form properly. I think Help will detail some of this in better detail. (It's a logical limit, not a software limit.) If you put a generous radius on your path, this surface will sweep just fine.



Jeff Mowry

http://www.industrialdesignhaus.com

A people governed by fear cannot value freedom.

 

[ArtemTat]

I'm not sure that using the profile with sharp changes in path is impossible. SolidWorks allows to do this. Please refer the attached picture. As you can see the Swept feature created succesfully.

It fails in case of intersection of the profile only but not streight segments.

Artem Taturevich
CSWP

 

[bvanhiel]

If your were using the same two sketches your sweep failed because sketch #1 had two entities.

 

[Theophilus]

Artem, in a case like that, why not just extrude the zig-zag shape? Much faster, simple to edit.

The problem I mentioned with SolidWorks having a limit in sweeps is when your profile will self-intersect on such harsh bends. If you're using a convex profile (external to your bends) this isn't an issue, but concave profiles, such as were shown by anchange are a problem because of self-intersections along the path.

At least on this level of simple geometry, there are many ways to get the form you're looking for (extrude, loft, sweep, whatever), so if it works, do it.



Jeff Mowry

http://www.industrialdesignhaus.com

A people governed by fear cannot value freedom.