Is there a way to make a sweep around a helix without the profile twisting as it sweeps along the path curve. Here's an example of what I'd like, done in Rhino.
And what I get from Fusion.
Thanks Mark.
Mark Hughes
Owner, Hughes Tooling
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Hi Mark,
The sweep body should not be twisting while travelling along the helical path. We are aware of this twisting issue with sweep if the curve used as the path is an approximation of a true helix. Where did you get the sketch used for sweep in Fusion from? Can you post that file? Fusion currently does not have a Helical Curve command in Sketch. You can create a helical sweep in Fusion through the Coil feature, but I am sure you are aware of that.
Thanks
Gautham
The problem with coil is the profile is not kept perpendicular to the helix, if you have a steep helix the square becomes very deformed.
Mark
Mark Hughes
Owner, Hughes Tooling
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@gautham_kattethota wrote:
Hi Mark,
The sweep body should not be twisting while travelling along the helical path. We are aware of this twisting issue with sweep if the curve used as the path is an approximation of a true helix. Where did you get the sketch used for sweep in Fusion from? Can you post that file? Fusion currently does not have a Helical Curve command in Sketch. You can create a helical sweep in Fusion through the Coil feature, but I am sure you are aware of that.
Thanks
Gautham
I used project to extract the edge of a coil. File attached.
Mark
Mark Hughes
Owner, Hughes Tooling
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You can try using a loft instead of a sweep. It's a little bit more work, but it may get you where you need to go. Check out the below screencast for more.
Does this look better?
I made two triangle (round probably works) coils with 5 mm difference in diameters everything else the same
then I made a sketch "plane along path" of the larger coil. I projected the end points of the two paths. constrained the sketch to them. then did a sweep with guide rail and keeped section the same.
The coil tool does not have a square section or circular section Rather it is rectangular or eliptical. It looks circular or square at the end because the end is cut at an angle to the center line of the material. For some reason the coil tool uses a square or circle that is not perpendicular to the path that runs up the center of the coil material, rather the square or circle is in the same plane as the main centeral axis of the coil. The screen shot below shows the difference, comparing the coil to a sweep. I think the coil tool needs to be redone. The sweep shown in the screen shot is the only object that has a circular section.
~Don
Hi Mark,
Projecting an edge of a coil into a sketch results in an approximated curve. When you then use that projected curve as a path for a sweep, it results in a twisted result. We are aware of this issue and should fix it sometime in the future.
Regards
Gautham
This can be done with Sweep set to Path + Guide Rail. Just draw a line along the centre axis of the coil that's at least as long as the coil and select it as the path then select the edge of the coil as the guide rail. I've attached a sample file.
Mark
Mark Hughes
Owner, Hughes Tooling
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Just for orthers who maystill be stuck at trying to get a "parralel", or "non twisted" sweep of your surface and failed to do so (because of geometry errors or else) using the method offered above (as I did), in my last fusion 360 version, I tryed using "path + guide surface".
I started with a coil, simplified it to a triangle so that I have "planar" surfaces, and used one of them as the guide. The vertical axe is not required.
Nevertheless, thanks anyway because the previous answer pointed me in the right direction 🙂
@laurent.chenet The problem with your method is you don't get clean surfaces, your's are very segmented. Here's what I get using sweep with guide curve. The sweep profile does need to be parallel with the helix though.
Mark
Mark Hughes
Owner, Hughes Tooling
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