This week I was sent an email from a member of my user group with a modeling challenge. They needed to model a helix cut that had different widths at the start point and end point. I first thought that this could get pretty involved with different sketches and profiles but after playing with it for a few minutes I realized that it is actually quite simple to accomplish this. Here are the steps I took to get this variable profile helix cut.
I started the model by creating a simple shaft with a chamfer on the top. I then offset a new plane off of the top plane that I want to use as the beginning (or ending depending on which way you think) of the helix cut. You can see these first couple steps in the above screenshot.
Next I created the 2 sketches that I want to use for my beginning profile (shown in red above) and my ending profile (shown in yellow above).
Then I created the helix that I want to follow by starting it on my helix start plane and telling it to do 1 revolution in the distance to the bottom of the shaft. The helix I created is shown in blue in the above screen shot.
The next step is where I actually create the cut. I used the “Lofted Cut” command. For my 2 profiles I used the 2 sketches that I created earlier. Now 1 thing to keep in mind when doing this is that we you select the sketches SolidWorks puts a green point at the closest end point of the sketch. You will want to make sure that those end points are at the corresponding points on both sketches. You can simply drag and drop the points to to the correct location if SolidWorks misinterprets where to put them. Next, I used the helix that I created as the Centerline Parameters of my loft. This allowed my loft to rotate around the part like I wanted.
Voila, it worked and I achieved the desired variable profile helix cut that I wanted. If you have another way to accomplish this same profile please feel free to share.
