# How to Create a Movable Spring in SOLIDWORKS

Article by Jonathan Sorocki updated February 14, 2014

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Seeing is believing! What I am talking about is how to make a spring in SOLIDWORKS. While we can create motion with spring forces in SOLIDWORKS, the spring itself is not modeled and doesn’t move. To work around this obstacle, many users ask me how to model a spring that can be compressed or stretched in a SOLIDWORKS animation. The answer is not too complex, but is definitely not orthodox.

### Modeling a Movable Spring in SOLIDWORKS

First, let’s model the spring. To make this coil, we are NOT going to use a helix curve. Instead, we will use a single sweep function with two sketches. Sketch a line on the front plane. It should start at the origin and go straight up. DO NOT give it a dimension. Rename this Sketch LENGTH. Sketch a circle on the front plane located somewhere off of the origin. I like to place a construction line from the center of the circle out to the right. I then pierce the free endpoint of the line to the LENGTH segment. You can make this line horizontal to guarantee a smooth sweep. Dimension the circle (gauge) and the distance from the origin (diameter).

Exit the sketch and rename it GAUGE. Choose Swept Boss/Base feature.

The profile will be the sketch GAUGE. The path will be the sketch LENGTH. Under options,choose follow path > specify twist value > revolutions. Set the turns to however many coils you need. This will create our spring. After the spring is finished, cut off sections on the top and bottom to make mating it easier.

To get the spring to move, place the spring into an Assembly. Mate the bottom of the spring to a face from another part (PLATE) with a coincident mate. I suggest mating planes of the coil and the PLATE to keep the spring from rotating. For this example, I have inserted a second instance of the PLATE to use as the motion driver. Save the assembly.

Edit the sketch LENGTH. Choose the free endpoint and another edge (circular, linear; it will not matter) from the 2nd PLATE within the assembly. Choose coincident relationship. Exit the sketch and exit edit part mode.

Now, move the 2nd PLATE up. Press rebuild (ctrl+B). Move the face of the body down. Press rebuild. You should see your spring change in height.

With the relation is set up; let us get the animation going! Create a new animation through Motion Study.

Move the time bar to 2 seconds. Drag the PLATE up. A key should be placed for you on the timeline. Move the timebar to 4 seconds. Drag the PLATE down. Another key is placed for you. Press Play from Start. You should see the spring move dynamically!

And there you have it! You can check out our blog for more SOLIDWORKS tips.