I want to twist the object below a certain number of degrees. I need the degrees to be a parameter so that I could specifiy 180 degrees of twist or 720 degrees twist or greatter. I've read the posts on how to make twisted pairs and tried using that add-in, but it does not do what I need. I have spent several hours trying to work out a way to do this. I went into this with the notion that there must be a way to twist an object or a sketch but I can not find it.
Hi @JohnSays,
Fusion, today, does not support any kind of "global deformation" on a solid body.
Here are a couple of related Idea Station entries that you should vote for if you are interested:
There are ways to design in the twist. Some forum threads that might help:
Jeff
Hey John,
After doing a little creative modeling, I think I’ve found a solution for you! It takes a bit of work arounds in order to get there, but once you create it you can control the twist parametrically (as you wanted to be able to control). Here’s the final geometry I created:
To begin, I created the “plus sign” sketch profile using two rectangles.
The method I used for creating the geometry was to sweep this “plus sign” sketch profile along a linear path, and use a helical guide curve to get it to twist as its swept. This means I need to get creative on how to make a helical guide curve. Here’s how I created the helix.
I created a cylinder that’s the same diameter as the height of the plus sign sketch. In this case the diameter of the cylinder will be 150 mm for my example.
The helix will run along the outer face of the cylinder. To do this, I’ll create a coil that intersects the outer face. I enabled the “coil” command, drew the circle on the same plane as the “plus sign” sketch, and used the following parameters:
The goal here is to get the coil to intersect the cylinder at a single point along the face. I used a triangular profile, and since the diameter is set to 150 mm, the endpoint of the triangle is all that intersects the cylinder. If you use a triangular section for the coil, be sure the diameter is the same as the cylinder, the section is set to “triangular (internal)”, and the section position is set to “outside”.
From here, you want to split the face on the cylinder. Enable the “split face” command, then select the cylinder as the “faces to split”, and use the coil as the “splitting tool”.
Now that there’s a helical guide curve we can use, which runs along the edge of the cylinder, the sweep geometry can be created.
First, add a sketch line extending outward directly from the “plus sign” sketch.
Next, enable the Sweep command. Change the type from “single path” to “path + guide rail”. Select the plus sign sketch profiles as the sweep profile (you may need to hide the cylindrical body), then select the linear sketch line as the path. Next, make sure the cylinder body is showing, and select the helical edge as the guide curve. Most importantly, make sure that the operation is set to “New Body”, and click OK.
Now, hide the cylindrical body, and the sketches, and the geometry now twists along the linear path! From here, you can adjust the parameters for the coil to change how tight the twist is on the body. Hope this gets you what you need!
