• 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!