Here’s a little tip based upon a recent request from one of our customers. They asked if there was any way that SOLIDWORKS could help them to create a square spring.
Firstly, you will need some circular sketch geometry to base a Helix curve on.
For this example, I created a 100mm circle on the top plane.
With the circular geometry in place a Helix can be specified easily from the Command Manager under Features – Curves – Helix and Spiral.
The Helix that you specify should have the same values as the required end result spring. In this case, 10 revolutions at a pitch of 10mm.
The next step in the process for creating the spring is to create a new 3D sketch and use the Convert Entities tool from the Sketch tab of the Command Manager to convert the Helix. This then allows you to hide your original Helix and also gain all of the benefits of using a 3D sketch.
The next piece of sketch geometry that you will need is a single line that is larger than your intended design of spring and sketched on the same plane as the circle used to define the Helix. The line should be Coincident with the centre of your Helix, and I have made this line intentionally unrelated in any orientation (i.e. vertical). I can then make the line Coincident with the endpoint of my converted 3D sketch.
The next bit of sketch geometry that you will need is the profile that you would like your spring to be. In this example I have used a square that has filleted corners, but the shapes that you can use are as varied as your imagination.
Now, let’s start construction of the spring. Firstly, use a Swept Surface using the single sketch line as the profile and the converted Helix on the 3D sketch as the path.
Secondly, we need an extruded surface based upon the final profile that we want the spring shape to be. This Extruded Surface needs to be the same height or larger than the original helix. You can use the Up to Vertex option to match the height of the existing geometry for this.
Now that we have the two surfaces, we can use SOLIDWORKS sketch tool ‘Intersection Curve’ to do all of the hard work for us.
Within the tool, select all of the faces or you can select the surface bodies from the feature manager. When you accept the selections, SOLIDWORKS will generate a 3D sketch exactly where the faces intersect. In this case, giving a helical incline around the square profile.
At this point, you can hide the surface bodies leaving only the 3D sketch of the square spring visible.
The last step in creating the square spring is to give it a material thickness. The most common way of doing this is to use a Swept Boss, but first we will need a profile sketch for the material thickness.
The ideal location for a profile sketch for a Swept Boss is at one end of the sweep path and in an orientation perpendicular to the angle of the start of that path. SOLIDWORKS has a function for generating a reference plane that exactly satisfies this need.
We can create a reference plane using the line at the start of our square helix as the first reference, and by selecting the end point of the same line, SOLIDWORKS will automatically position the new plane perpendicular to the line and coincident with the end point.
Now that the correct sketch plane is in place, a simple profile is added for the spring material profile.
The Spring can now be finalised by creating a Swept Boss Base selecting the spring profile and the profile sketch and our square spring path as the path sketch.
The spring doesn’t have to be square though, the limit is your imagination.