• Curved pressure springs in SolidWorks
• Bend your springs in SolidWorks

Create a Surface Loft with two profiles.

Notice the Start/End Constraints.

Create the second surface.

Now it’s time to create the Intersection curve, start an profile for the Sweep and here we are!

First of all you’ll need to create a sketch with the curve on the front plane. This is the centreline of the spring. This can be an arc of a poly line. In this case I’ve chosen a polyline with construction lines on both ends. To add more control I’ve added the relation ‘Equal Curvature’ to the constructionlines and the polyline.

Now create another sketch on the front plane. This is the profile for the Swept Surface we create on the following step.

Now add the Swept Surface and add the preffered options. Specify the amount of turns.

If you have a large number of turns specified the final Solid Sweep can cause problemens!

This is the result of the Swept Surface:

Now create a new Swept Surface with a circular profile with the diameter of the spring and the centreline of the spring as a path (use the sketch tool Convert Entities to pick the centreline you’ve already used in the first Swept Surface and project the curve on the front plane).

Now you’ve got two surfaces, it should look something like this:

And here comes the magic! Select both surfaces and go to Tools -> Sketch Tools -> Intersection Curve

An intersection curve is created after you’ve clicked the menu button. Hide the two surfaces to create a better overview.

Now we create the profile of the spring on the front plane. This is the material diameter…

And add an ordinary Sweep to these two sketches and here we are!

Create the contour

First you’ll need to sketch something like this on the front plane. Please note that all the dimension lines are centre lines and the poly line is not. The vertical line is our axis in the next step.

You can also add this sketch is a part that you have inserted like I described in the previous article about springs Pressure springs in SolidWorks.

For the next step you’ll need the surfaces toolbar. If you don’t see this toolbar in your interface you can add this by right clicking on a empty space in the upper command bar and select the surfaces tool bar.

Add a Revolved Surface to the sketch.

Line 1 is the centre line we’ve defined in the sketch.

This is what we have now

Create the path

Add another sketch on the front plane (or the same plane you’ve created the first sketch).

Draw a simple line in this sketch from top do bottom.

Add another sketch on the front plane an this one contains a horizontal line. The length of this line is not important, as long as it intersects the cup we’ve already made with the revolved surface.

Now we need a surface sweep. Select this feature in the surface toolbar. Sketch 2 is the rotation axis, Sketch 3 is the profile that needs to be swept. Choose in the options ‘Twist Along Path’ and specify the turns.

This is what we have at the moment. Two surfaces that are totally a mess, but there is a logic behind these two surfaces. The first one is the contour of the spring and the second one is the path of the spring.

Project path on contour

We’re almost done and we’re up to the point were the magic happens. Now we need to project the path of the spring on the contour. Select the two surfaces.

And choose ‘Intersection Curve’ and select the contour (cup) and the inner line of the path.

You’ll get a curved 3D sketch that looks like this. Select the two surfaces and hide them for a better overview.

Create the profile

Create a sketch on the front plane and draw the profile of the spring.

Make sure that the centre of the circle is pierced by the 3D sketch.

At last we’ve got to add a swept boss/base to these two sketches.

Define the profile and the path and you’ll have a tapered or curved pressure spring!

The result

We’ll start with a shock absorber assembly without a spring. We’re going to add this part to the assembly.

Add a new part to the Assembly with the top down method in SolidWorks. Read more about this in the article 10. Top down modelling in SolidWorks.

Select the Assembly front plane to define your first sketch plane.

A new part is added to the feature tree and the rest of the parts are displayed as outlines. This means that the assembly is in the ‘edit part’ mode.

Draw a centre line trough the centre of the assembly. This is the rotation axis of the spring.

Add some dimensions to it. In this case I’ve added some extra length to the spring to flatten the outer ends of the spring. Make sure the smart dimensions points to the contact points of the spring.

Create a new sketch on the front plane.

Draw a circle on the sketch. This will be the contour of the material the spring is made of. Add a horizontal relation to the end of the centre line and the centre of the circle.

Now just add a Swept Boss/Base to these two sketches.

And put some attention to the options of this feature. Define the turns and the apply the modifications.

Here you are, a top down pressure spring. Drag the piston to change the stroke of the shock absorber and hit the rebuild button. You’ll see that the spring is changing in length.

Just use the Cut Extrude feature to modify the outer ends of the spring!

The result

This is how it looks like when you’re creating a animation of the assembly!