Popular Topics

# How to Make a Helix in SOLIDWORKS

Welcome back to my “how-to” blog series. In this blog, I demonstrate how to make a helix in SOLIDWORKS. One of the most common applications for making a helix is in order to cut threads onto a model – and that’s exactly what I’m going to cover today. In my last blog, I demonstrated how to make a screw in SOLIDWORKS, and to continue with this blog series, I’m going to be working with that same model. Let’s get started.

I’m going to begin by taking my hex cap screw that I modeled in my previous blog and I’m going to create a shaft coming off of it. If I look back at the specifications sheet, the shaft diameter should be .250 for ¼ 20 hex cap screw. I’m going to then extrude that out to a height of 1.5 inches.

Next, I am going to begin a new sketch, and I’m going to sketch a circle because every time you make a helix in SOLIDWORKS, the way you begin is by creating a new sketch, and then sketching a circle. After you create that circle you can go to the command Features > Curves > Helix and Spiral. From within the helix command, we can designate what we want the height and pitch to be, the pitch and revolution, or the height and revolution.

Let’s say we do pitch and revolution and we make the pitch .125 and we make the number of revolutions 5. You can see some of the other controls we have are “what is the start angle”, “what direction is the helix going in?”, “is it going clockwise or counter-clockwise”, we can even make something that is called a variable pitch helix.

With a variable pitch helix, what we do, is we say we want the pitch to be at .125 as we go from 0 revolutions to 2 revolutions. Then, as we go from 2 revolutions to 4 revolutions, we’re going to say that we want the pitch to increase to .250. You can see here that it’s no longer holding a constant pitch. Then we can say from 4 revolutions to 6 revolutions, we want it to remain at .250.

So now you can see that we end up with a spring that’s compressing on one end or there could be a number of applications for creating a variable pitch helix.

In today’s example, I’m going to make a constant pitch helix so I can cut some threads on to the hex cap screw. So I’m going to select a face and begin a sketch because every time you make a helix in SOLIDWORKS, you always start out by sketching a circle.

Now, we want our circle to be an exact duplicate of the top edge of the model, so I’m going to click on the top edge of the model and I’m going to choose Convert Entities – that will give us an exact duplicate of the top edge of the model in the form of a sketched circle. Now you can go to the command Features > Curves > Helix and Spiral.

In this case, I don’t want to use Variable Pitch, I want to use Constant Pitch. If it’s not going in the correct direction, you can select Reverse Direction and insert the pitch amount (in my case 1/20 because I’m making ¼ 20 hex cap screw). As for the number of revolutions, I want mine to go to 1 inch, so under Defined By, instead of Pitch and Revolution, I’m going to select Height and Pitch and select the height to 1 inch. So now I have an inch and a half long shaft with 1 inch of threading.

You can also control your start angle here (I’m going to leave mine at zero). My threading is going to be clockwise since it’s a standard thread and you don’t want to taper at all while you’re creating your helix. Once it looks good, go ahead and hit the green check mark and that’s it! That’s how to make a helix in SOLIDWORKS.

You can watch a video demonstration of this by checking out the video below.

In my next blog, I’m going to demonstrate how to make threads in SOLIDWORKS and how to cut threads along this helix using a cut sweep.

Related Articles

How to Make a Screw in SOLIDWORKS

How to Create Manual Configurations and Design Tables in SOLIDWORKS

Edit an STL File in SOLIDWORKS – It’s Easier Than You Think