Spiral cone model issues

[rnl9t]

I am trying to create a 3D model of a spiral ramp ascending a conical shape.  My first thought was to draw a spiral in a 2D sketch and project it on to the surface, then sweep a sketch profile up that path.  This failed because I could not figure out how to draw a 2D spiral (so any tips would be appreciated).

I kludged a solution by using "coil" to create a spiral coil, and then projecting that onto the cone.  For some reason, I had to create a coil three times the size of the cone to get a spiral on the cone rather than just at the very top...not sure what is up with that (ideas?).  It also resulted in two conicident spirals on the surface going in opposite directions, one of which had to be deleted so I could stop getting the "one path is antiparallel to the other path" message (that's not exactly what it said but close).

Sweep still refused to cooperate, returning the usual-for-Fusion 360 cryptic "inconsistent edge-face relationships."  This despite using "align" to put a part of the profile on the point marking the start of the path.  I am not sure which edges and which faces are the problem.  One longer error message did suggest I use the "validate" function--which I have used before under Patch > Insepct, but for whatever reason does not appear there.

Then I had the bright idea to use "pipe," which drew a nice round pipe along the spiral just as I wanted.  But then when I switched to a square pipe (to make the ramp with a flat bottom), and for some reason the square pipe twisted around the path as it went up, resulting in a wonky ramp.

I gave up and just used the "trace" function in CAM to get the result I wanted.  But it would certainly be nice if there were a way to draw the actual model.

Thanks!

ETA: I meant to put this in the Sketching/sculping/modeling forum, could a moderator please move it?  Thanks.

[jeff_strater · Accepted solution]

Thanks for posting.  I'm glad you were ultimately able to get a decent result.  I think most of what you did in Fusion was correct.  I can help get the spiral curve on the cone a bit easier, but I ran into the same problem with sweep - currently Fusion does not have any "twist control" in sweep.  Would you be willing to post an idea for this on the Fusion 360 Idea Station?

Here is how to get the spiral curve onto the curve.  It's mostly the same process as you did, but with one additional step.

start with the cone, and add the coil as a separate body:

Then, create a new sketch.  It doesn't matter what plane is chosen, because the geometry will all be in 3D.  Use the "Include 3D Geometry" command:

And pick just one of the edges of the coil.  This creates a 3D curve:

Then, exit this sketch, and create a second sketch, again, the plane does not matter.  This time we will use the Project Curve to Surface command:

Select the cone as the surface, and the coil curve as the curve to project.  This will create a nice spiral curve on your cone:

That gets you the curve.  But, as you noticed, sweep will twist in ways that are not good.  I even tried Pattern on Path, and it has a similar problem.

So, there are really two ideas that are needed here:

1. Add a Helix curve to sketch - to create a coil curve, or a spiral curve

2. Add a "surface normal sweep" to allow you to control the twist of the sweep

Good luck with your Fusion work

Jeff Strater (Fusion development)

[rnl9t]

Thank you. I will try that next time (if I need this feature again...I have already cut the workpiece I wanted).

[Oceanconcepts · Accepted solution]

Actually, this led me to discover that the ability to make tapered coils is present in Fusion. That seems as if it could be a way to generate the shape, using a Boolean operation to get the ramp. 

[rnl9t]

I didn't see that until you prompted me to look--and it does work.  Thanks!

[innovatenate]

I made a screencast of an attempt below I thought may be a good add to this conversation.

http://autode.sk/1qFnEmN

Thanks,

[donsmac]

Here's a spiral ramp you can adjust the parameters of. Just fit this over a cone, adjust parameters if needed, and combine.

The screencast shows how I did this: