Have you ever wanted or needed to create a square helix, or maybe even a triangular helix or any shape helix for that matter in SolidWorks but didn’t know where to start? It’s actually pretty easy to create any shape helix in SolidWorks. First you will need to create a “standard” circular helix by simply drawing a circle and using the helix command (Insert/Curve/Helix and Spiral). Then select your helix parameters and options that are required to define particular helix (height and revolution, etc…). Next hold down the Ctrl key and select the helix and the helix end point and create a new plane and draw a straight line from the orgin (or end point of the helix) outward. Use the surfacing toolbar and create a surface sweep using the “line” you just drew as your profile and the “helix” as your path.
You should now have something that looks similar to what’s above.
Next step is to create your “square”, “triangle”,”oval” or whatever shape helix you are after. Create a sketch on the same plane you created your circle sketch for your helix. Draw your shape, but make sure it fully intersects your sweeped surface you created. Now in the “Surface” tools use the Extruded Surface command and extrude your shape making sure it intersects beyond your sweeped helix. It should look similar to what I have below.
Next you will use a tool located in “Tools/Sketch Tools” called “Intersection Curve”. Select Intersection Curve and select both Surfaces that you created. I usually select the two surfaces under Surface Bodies toward the top of the Feature Tree.
This will ultimately create a 3D sketch that you will use to create a sweep. Now you just create a plane and a profile on the end of the 3D sketch and use the “Sweep” command to create your final helix.
That’s it! Hope this helps you create your next oddly shaped helix!