How to create a toroidal coil/ helix?

[Anonymous]

I found some information on how to do this in inventor, but I do not presently have access to inventor, so I was wondering if there is a way in Fusion 360 to create what at least one person dubbed a toroidal helix.  Specifically, is there a way that I can take a coil/ helix and bend it 360 deg and attach end to end to create a spiral that wraps around a torus? Or even a way to make a straight pipe into a torus that I could use the same process on a coil? Is there a bend feature in Fusion 360? Sorry I am brand new to this and may be missing something obvious, but it is driving me nuts!

Thank you for any insight!

[donsmac · Accepted solution]

Here's a way to do it. Here I made six hexagons and connected the corner points (3D sketch on). Then do a loft. I added the pipe to each edge afterwards.

You can add more sections if you want more turns on the coils.

[Anonymous · Accepted solution]

That's insanely cool! 

I went with the quasi-cheating approach, creating a spreadsheet from the helical toroid parametric equations (http://math.stackexchange.com/questions/324527/do-these-equations-create-a-helix-wrapped-into-a-toru... and then just importing that as a 3d spline that can be used as a path.

The process to do something like this is described here:

http://forums.autodesk.com/t5/post-your-tips-and-tutorials/creating-equation-spreadsheet-and-importi...

I used the .05 value for k as in the example, so the total number of degrees needed to complete the shape is 360/.05=7200. 

Also found this free online service is great for plotting 3d scatter and line graphs (I had to find an error I made in the spreadsheet data):

http://help.plot.ly/make-a-3d-line-chart/

There was a little bit of imperfection where I did a loft between the starting and ending faces of the coil to complete the shape.  I would probably redo that by having one less spline point in my table, and connect the gap between the starting and ending of the helical spline with an additional spline, insuring both ends are tangent to the imported spline. 

If you try this method let me know if you need any help.

Cool challenge!

Jesse

[Anonymous]

Wow! Super intuitive, thank you!! I will definitely experiment with this method, looks like it will fit my current needs perfectly.

[Anonymous]

Wow, well thought out! And useful resources to know about.  I will definitely experiment with this method as well. As for the k just to be sure I am reading this right, if I wanted 4 revolutions rather than 20, I would use a value of .25? And if I wanted it to be a double helix, just copy and rotate by 180 deg? Or is there a way to produce multiple 3d splines from one spreadsheet/ import? Thank you!  

[Anonymous]

That's right about the k value.  And for creating a second coil for double helix, you're right about advancing the second coil phase by 180 degrees, which in terms of the overall shape rotation using Move command, well to get a complete 360 degree phase cycle would be 360/4=90 degrees, so to offset second coil phase by 180 degrees, actual rotation would be 45 degrees. 

You could instead create a second table with the offset phase and import second spline, but that seems like needless work.

Good luck!

Jesse

[Anonymous]

I just wanted to point out that to do this in Inventor you can use a 3D sketch equation curve as shown below. Then use the resulting curve as a sweep path.

[HughesTooling]

Fusion can do this quite easily now using sweep with a twist to create a path.

File's attached.

Mark

[craig_smith72]

Thganks for a great tip !! I was really struggling with this until I found your post. I know it's 4 years on, but it fixed up my issue for me.

Thanks again !!