Modeling twist for rectangular section

[SyncroTec]

I need suggestions on modeling a twist in a rectangular cross section.

The aluminum casting cross section is 160mm x 96mm x 10mm wall and the twist length is about 60mm. The twist angle is 12 degrees.

 

[SBaugh]

Look at SW05 Flex feature or if you make a sweep you can twist the sweep at certain degrees. Also there is a deform feature you might look at.

Regards,

Scott Baugh, CSWP
3DVision Technologies

http://www.3dvisiontech.com

http://www.scottjbaugh.com

faq731-376
faq559-716 - SW Fora Users

 

[TheTick]

If you use a sweep, try using a guide curve to orient your section along the sweep path. Use pierce constraints in your section sketch to constrain your sketch to the path and guide curves.

I could be the world's greatest underachiever, if I could just learn to apply myself.

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[Theophilus]

If you use a sweep, it sounds like your path will be a straight line while your guide curve will be a helix. Check help for details.


Jeff Mowry

http://www.industrialdesignhaus.com

Reality is no respecter of good intentions.

 

[ShaggyPE]

Sounds to me like a great usage for a loft. When opposite points are selected on both of the sketch profiles, the loft will do some twisting.

 

[Jabberwocky]

I agree with Shaggy, a loft should work here. Just set up your second section, then dimension your second section to 12 degrees on a new datum plane 60mm down the path. That way you will have control over both of your end sections. The middle should fill itself in.

A helical guide curve couldn't hurt either.

 

[SyncroTec]

Thanks for everyone's input.

But this what finally worked for me.

I created the 160x96 rectangular sketch and rotated the sketch in 3 degree increments with 15mm increments spacing up to 60 mm that resulted with the final 12 degrees. Than added "curve through reference points" on each corner of the incremental rotated sketch. Than swept the rectangle profile and a 60mm path with 4 guide curves.

The only inconvenience was that I now needed to array the feature 3 times at 120 degrees, but SW would not array the feature with guide curves.

The resulting part is a 3 bladed wind turbine rotor hub.

 

[Ataloss]

To get the circular pattern to work with a "sweep with guide curve" don't you just have to turn on the "geometry pattern" option in the sweep function, or am I getting this confused with something else?

What about not merging the original blade to the base part (so you have two bodies) and doing a pattern of bodies instead of a pattern of features?

Bob