Creating wires and ropes in SOLIDWORKS is commonly done with a Swept Boss/Base feature. By using a single circular profile and a path, the Swept Boss/Base feature can create a simple wire. But if you need a more complex illustration, such as that of a pair of twisted wires or a rope with multiple strands, then this article will help you. So, let’s get started.
In this article, we will discuss how to make a twisted pair of wires.
1. Create a 2D sketch or 3D sketch according to your requirements. Use a 2D sketch if the wire is placed on a plane surface. But most of the time this is not the case. So for this tutorial, we’ll use a 3D sketch. Start a 3D sketch by clicking on the down arrow below the Sketch tool and selecting 3D sketch.
2. Create the path of the wire with the help of lines, curves, or splines. Here, we are going to use a spline to create the path.
3. Next, we need to create the profile of the wires. There are several methods to do so but we’ll show two methods in this tutorial.
Method 1: By creating a Reference Plane
Create the plane from Features Tab -> Reference Geometry ->Plane with the following options:
- In the First reference, select the plane which is parallel to one of the endpoints’ normal of the 3D sketch that we created.
- In the Second reference, select that endpoint.
Now let’s create the profile on this plane. You can create 2, 3, or more circles depending on how many wires you want twisted. The diameter of these circles will represent the wire diameters.
Tip: Make sure that the circles don’t intersect or touch each other. To make a solid sweep, all contours must be closed and non-intersecting. If they touch each other, either the Sweep will fail or you may encounter a “Zero thickness Error”.
Method 2: By creating a reference Swept Boss/Base.
This method is recommended because most of the time, creating a plane that is perpendicular to the path’s endpoints can’t easily be done. And this method also provides an overview of what the end result will look like allowing you to fine-tune the path in this step.
Create a Sweep by invoking Swept Boss/Base command present in the Features Tab.
- Under the “Profile and Path” menu, choose Circular Profile and then select the 3D sketch as the “Path” and then input the outer diameter of your wire (this diameter is only for reference).
Click on the Green Checkmark and you’ll have a simple wire. Now right or left-click on any of the end faces of the sweep and click on the Sketch icon to start the sketch. Then draw your profile sketch on it.
Now, if you know how to work with Feature Scope, you can delete this solid body we just created whenever you deem fit but if you’re a beginner, we would highly suggest you delete this body right after you’re done with your sketch. To do so, go to Insert-> Features-> Delete/Keep Bodies and select the Sweep body to delete it.
6. Now that we have both the path and profile of the wires, let’s create the sweep by selecting Swept Boss/Base from the Features tab.
- Under the “Profile and Path” menu, select the sketch we made on the plane as “Profile” and the 3D sketch as the “Path“.
- In the “Options” menu, select Keep Follow Path in “Profile orientation“.
- In “Profile Twist“, select Specify Twist value, and in the “Twist Control” drop-down, you can select any of the provided options and then enter the amount of twist you want in your wires. You can change the direction of revolution by clicking on the reverse direction icon present alongside the input box.
7. Next, click on the Green Checkmark to make the sweep and you’ll have multiple wires twisted into each other depending on how many circles you made in the profile sketch. These will be individual solid bodies to which you can apply appearances or materials according to your needs.
In this quick tutorial, we learned how to use the Sweep feature to create a pair of twisted wires. By increasing the number of circles in the profile sketch and increasing the twist value, this method can be used to create a complex rope too.
