Sweeping a semi-complex sketch around a central circular path (EG: twist around axis)

[crlaozwyn]

I'm designing a paddle and want to introduce a mild sweep so it naturally pushes things down as it turns. For the life of me, I can't figure out how to make this work. Basically, I'm trying to make the blades rotate slightly around the central shaft. I tried making a coil with the same diameter/length of the shaft and sweeping the sketch around it (tried circular and internal/external triangles) but I get an "illegal surface" warning, which makes sense because the object would impossibly overlap. I also tried sweeping it along the circular shaft which worked but created a solid semicircular block, whereas I want the top of my extrusion to start on one side of said block and the bottom to end on the other side (if that makes sense).

I realize I may have to redraw my sketch or move it to another plane to do this, but I'm stuck and would greatly appreciate any help. 

Here are top/side views of my paddle to give an idea what I'm working with

Here's the result of sweeping around central shaft sketch. Rather than having it get wider the farther out you go, I want to keep the blade with consistent throughout, so it would look like the above-left picture at any given Z point, but have the top of the paddle start on higher up on Y axis (farther away in the picture) and the bottom lower on the Y axis (close to our perspective).

Apologies if I haven't articulated clearly. Happy to put it in different words if needed. TIA!

[davebYYPCU]

Sweep a twisted surface, 

Revolve cut to profile shape,

thicken and Pattern.

Might help....

[crlaozwyn]

Thanks, that sounds like what I'm trying to accomplish and your shape does have the twist I'm looking for. Unfortunately I'm not quite sure how to follow your instructions. If I put even 1 degree of twist on my sweep, it says "there was a problem combining geometry together." At 15 degrees, "the body would intersect itself." It does this even if I select the entire paddle, not cutting out the diagonal slices.

[davebYYPCU]

Would need to see your file to see why that happens.

Might help....

[crlaozwyn]

Attached, thanks

[davebYYPCU · Accepted solution]

For some reason your file will not allow the surface Sweep without error, and I had my file to work with ....

I suspect that it's because there are 5 almost overlapping lines on the centreline of that sketch.

I copied your sketch to my file, (without your centrelines) you will have to edit the Sweep for the correct twist angle.

When you add the hub, the 3 blades will get joined to the hub.

Blue lines and white dots are not recommended.  I fixed the ones I needed.

Sweep the widest line in the sketch, along the depth. (fix the twist angle)

Select the silhouette of the blade from the sketch and use Revolve > Intersect to cut the white space off the blade.

This allows the blade surface to be thickened symmetrically, (fix the thickness)

Pattern before the hub, will save you a Combine command.

Surface Body can be Removed now.

Might help.....

[crlaozwyn]

Thank you so much for your help. I'll study the difference between your sketch and mine to figure out what changes you made (not familiar the alternatives to blue lines/white dots). From there, reimplementing your steps should be straightforward.

Again - thank you, kind internet stranger.

[davebYYPCU]

Happy to help where I can, 

Blue, orange lines and white dots are not recommended, they should be black, purple or worst case green.  Is a polite way to say your sketch is unstable, and prone to unexpected errors, especially when you develope onto variable parameters, so good practise now, will be a huge benefit later.  White dots will disappear when Fusion is told to make the end point coincident to the line you want to connect to.  Black and purple dots will be ok

I could not see how you made the rib width.

I don’t like repeating, stuff that exists, so I copied your sketch, all except the centre lines and points.  It was only later, I found you have drawn the Long centre line over the short legs of the rectangle, and then two more for the (logical?) dimensions at the bottom, one long line will do the job the other four are doing, and I can’t confirm, but believe it is why I could not get a Sweep to happen in your file, and gave up.

Might help....

[crlaozwyn]

Great info and a reminder of the perils of "I'll learn by doing." I'll take some time to circle back on some of the basics before embarking on another project of this scope (the paddle is one part of many).

Thanks again for the help and useful info.