I came across this a few years ago when looking to flatten a screw conveyor flight.
I believed it couldn’t be done but here’s how….
Create a sketch on the front plane and place a 100 mm diameter circle on it.
Use this to create your first Helix/Spiral using the Pitch and Revolution option. Select Constant Pitch of say 600mm and 1 clockwise revolution starting at 0 degrees.
Repeat this with the same settings but use a larger diameter circle say 500mm.
Now comes the tip – Create two 3D sketches one for each helix. In the first 3D sketch select the helix and use the convert entities command. This will place a spline in the 3DSketch with an On edge relation to the helix. Repeat converting the second helix in the second 3D Sketch to make a second spline.
The rest is easy
Go to the Insert>Sheet metal>Lofted bends and select the two 3DSketches as the profiles using a thickness of say 6mm.
You flight is now finished and ready to be flattened
Mark Duggan
Intercad Technical Support Mgr
