How to model a bent tapered spring in SolidWorks

Gavin Peters

30 May, 2014 01:29 PM

The taper on this solution is only a representation. If you know how I can change the appearance of the taper to the real word model please add to this thread. Thank you in advance.

1. Step 1:

   Part 1: Creating a helix along a path
   Draw the path of the centreline of the spring. Create a point at the midpoint of each bend as shown below.
   

   

2. Step 2:

   Part 1: Creating a helix along a path
   On a new sketch create a line perpendicular to the previous path. This line should just be longer than the maximum radius of the spring (from the centre of the spring wire to the centreline of the spring). If your spring is not tapered the line length should be the radius from the centre of the spring wire to the centreline of the spring.
   

   

3. Step 3:

   Part 1: Creating a helix along a path
   Use the surface sweep command. Sketch2 is the profile and sketch1 is the path. To make the helix we need to select “Twist Along Path” in the options. The number of coils can be selected by selecting define by “Turns”. It does not need to be a whole number of turns.
   

   

4. Step 4:

   Part 2: Taper the helix
   Temporarily suppress the surface body while we create the taper surface
   Show sketch1 for this step. Create planes on the middle of the curves and on each end of sketch1 (Note: I’m using the top plane for the bottom of the spring. Note: This is why we added the point on the initial sketch.
   

   

5. Step 5:

   Part 2: Taper the helix
   On each plane create a circle representing the diameter of the taper at that point. In this example I have an equal amount of spring either side of the arc which means that the diameter at plane 1 will be half way between the start and end.
   In this example the Top plane circle is drawn at 300mm
   

   

6. Step 6:

   Part 2: Taper the helix
   In this example the end circle is 200mm
   

   

7. Step 7:

   Part 2: Taper the helix
   In this example the middle circle is 250mm
   

   

8. Step 8:

   Part 2: Taper the helix
   On the same plane as sketch1 we are going to sketch a spline with one point at each taper circle. Use the pierce constraint at each point.
   While writing this tutorial I’ve noticed that this part is introducing some artistic license. The taper of the spring will not be 100% accurate as the spline should be linear along the straight sections of the path. – If you know how this can be improved please let me know.
   

   

9. Step 9:

   Part 2: Taper the helix
   Using a surface loft a tube is created. Use the circles from the previous steps as profiles (these will need to be in the correct order). The last sketch is the guide curve that stops the tube from ‘twisting’ and becoming narrower at certain spots.
   

   

10. Step 10:

    Part 2: Taper the helix
    Unsupress the surface sweep from Part 1. Use the Surface Trim command to taper the helical edge. The trim tool is the tubular surface and the 2nd selection is the original surface sweep. I have selected the external selection below and, therefore, the Remove selections option.
    

    

11. Step 11:

    Part 3: Taper the helix
    Select the Surface-Loft1 item from the surface bodies section of the featuremanager design tree and press the delete key. This will activate the Delete body command. You should have something similar to the image below. Accept this and the delete body command will be added to the featuremanager design tree.
    

    

12. Step 12:

    Part 4: Creating the spring
    Create a reference plane perpendicular to the helix on the end of the path.
    

    

13. Step 13:

    Part 4: Creating the spring
    Draw the wire cross section on to the new plane. I’ve used a hexagon shape here to show that it isn’t always round.
    

    

14. Step 14:

    Part 4: Creating the spring
    Use the Swept Boss/Base tool to generate the wire spring profile.
    

    

15. Step 15:

    Part 4: Creating the spring
    Select the Surface-Trim1 item from the surface bodies section of the featuremanager design tree and press the delete key. This will activate the Delete body command. You should have something similar to the image below. Accept this and the delete body command will be added to the featuremanager design tree.
    

    

16. Step 16:

    Final Design