How to Create a Spring That Will Expand and Compress in a SOLIDWORKS Assembly

This tutorial demonstrates a simple example of how to create a spring part that can be inserted into a SOLIDWORKS assembly that will expand and compress with the movement of other parts.

Creating the Spring Part

The Sweep

The key to allowing a spring to compress and expand at the assembly level is to leave the spring component underdefined. For this reason, we won't use the Helix and Spiral feature. Instead, we'll create an underdefined Sweep. The sweep path sketch will be underdefined with only a relation on one end. The profile sketch can be fully defined as usual.

1. Start a new part.
2. Create the path sketch on the Front Plane (Sketch1):
   
   • Start a line and make the first end coincident to the origin and place the second end directly above it, allowing a vertical relation. This will leave the top endpoint free and make it appear blue, indicating the sketch is underdefined - which is exactly what we want.
     
     
     
     
3. Create the profile sketch on the Front Plane (Sketch2):
   • • Add a circle, with the centerpoint aligned to the fixed endpoint of the path sketch (or the origin) with a horizontal relation. Define the circle diameter and distance to the line to fully define the sketch.
       
       
       
       
4. Create the Swept Boss, with a twist:
   • Select each sketch in its corresponding section; Sketch2 is the Profile, and Sketch1 is the Path.
   • • Expand the Options section and change the Profile Twist option to Specify Twist Value. Set the Twist Control to be based on Revolutions, and specify how many revolutions/coils you want for your spring.
       
       
       
       
5. Once finished, we should now have the general spring shape.
   
   

Flattening the Ends

To make this part more realistic and easier to mate at the assembly level, reference planes and surfacing tools are used to make the spring planar on each end.

1. Show the path sketch (Sketch1) by right-clicking it in the FeatureManager Design Tree and selecting the show icon (eyeball). This will allow you to use the endpoints of the sketch to create the needed reference planes. If the sketch doesn’t appear in the graphics area, go to View > Hide/Show, and make sure Sketches is selected.
   
   
   
   
2. Create a reference plane. In the Features tab, under Reference Geometry, choose Plane.
   
   
   
   
3. Define the references. One reference will be coincident with the sketch endpoint, and the other perpendicular to the line.
   
   
   
   
4. Repeat steps 2-3 for the other end of the part.
   • Looking at the part from the side, notice that the reference planes are intersecting part of the spring. This is intentional, as we will use these planes to cut each end of the spring so they are planar.
     
     
     
     
5. To flatten the ends, use Cut With Surface (located in the CommandManager's Surfaces tab, which may not be visible by default). Note: You can always locate features via the Command Searchbar too.
   
   
   
   
6. Once the tool is open, select one of the reference planes you created and choose which direction you want to cut. In the graphics area, an arrow indicates the direction from the plane where material will be removed. If needed, change the direction by clicking the flip cut icon.
   
   
   
   
7. Follow steps 5-6 for the bottom of the part.
8. Now we have nice planar surfaces on each end to easily mate at the assembly level.
   
   
   
   
9. Save the file.

Adding the Spring Into an Assembly

Now we will work on the assembly. The trick with this is keeping the fixed ends together and the free ends together. When creating the spring part, we fixed the bottom of the spring in the path sketch and left the top underdefined. For this example, a simple assembly was created with two discs and a center pin. The base disc is fixed, and the top disc will move to expand or compress the spring.

1. Create or open the needed assembly.
   
   
   
   
2. Insert the spring into the assembly.
3. Add a coincident mate from the bottom planar face of the spring (the one with the fixed endpoint in the path sketch) to the top of the fixed base disc.
   
   
   
   
4. Add a concentric mate between the spring and the pin. The easiest way to do this is to show and select the path sketch and the pin.
   
   
   
   
   • The spring will still rotate, so if you want to lock the rotation, right-click on the concentric mate and select Lock Rotation.
     
     
     
     
5. Edit Sketch1 from the spring part in-context (this is where the underdefined path sketch from the spring part comes in handy!). Right-click the sketch from the FeatureManager Design Tree or in the graphics area, and select Edit Sketch.
   
   
   
   
6. Now add a relation from the blue endpoint in the sketch to the bottom edge of the top free-moving disc.
   
   
   
   
7. Once the relation is accepted and we exit the sketch, the spring part will expand to meet the top disc.
   
   
   
   
8. Now, whenever the top disc is moved along the pin, and the assembly is rebuilt (Ctrl + Q or Ctrl + B), the spring will compress with the assembly.
   
   

Conclusion

Creating a dynamic spring in SOLIDWORKS that expands and compresses with the motion of an assembly adds a level of realism and polish to drawing views, screenshots, and animations.

Want to learn more about SOLIDWORKS? Check out additional tutorials and tips below. Additionally, join the GoEngineer Community, where you can create forum posts, enter design contests, and answer questions from other SOLIDWORKS users.

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