Download the tutorial file

First draw a circle on the top plane.

Add a Centerpoint arc and start at the top of the circle. Add two guide lines to control the gab (to weld the to cilinder for example)

Create the Base Flange, you can find this feature under the Sheet Metal tab.

You can see how the result looks like when you Unsuppress the Flat Pattern in the feature tree.

But when you add a sketch to cut a part away, these cut will not be shown when you Unsuppress the Flat Pattern.

Look at the example, first the unsuppressed flat pattern with a extruded cut:

And now I’ll suppress the Flat Pattern…

No holes in the cylinder any-more and look at the Feature Tree, the Cut Extrude is Suppressed. How to solve this? Well, go on with this tutorial!

Remove the Cut extrude and Suppress the Flat Pattern. Now add an Unfold feature to the model. This can be found under the Sheet Metal tab.

Select an outer edge of the gab of the cylinder and press the button Collect All Bends.

Press the OK button and here we are, a flat sheet metal!

Start a new sketch for a Cut Extrude on the flat surface.

I’ll make four of them with the Linear Pattern feature. The space between is the total length of the sheet metal divided with four.

The last step is to fold the sheet metal back to it’s original shape. Use the Fold feature in the Sheet Metal tab.

And here we are:

Now I’ll expand the sheet thickness to 10mm (and change the distance between the cut extrude) to show the edges of the circular cuts in the sheet. Only with this method you’ll get such a result.

I hope this was a useful tutorial for you!

Enjoy!

Right click on the upper tool bar and click on the bottom on Customize.

Go to Annotation and look foor the Cosmetic Thread icon.

Drag the icon to the preferred tool bar. I’ve got mine in the sketch tool bar.

3D

I’ll start with a simple axle.

Click the Cosmetic Thread button and specify the thread type

Press OK or Apply

To edit the thread, just look beneath the feature where the outer thread is applied. In this case it’s really obvious because I have only one feature for the axle but you have to search sometimes when you’ve got a large feature tree.

And here we are:

2D

When we insert a model view from a part where we already have added a Cosmetic Thread SolidWorks indicates it immediately.

But when you start with a clean axle you can also add a thread. Add the button to your sketch toolbar via the method I described at the begin of this topic.

Click Cosmetic Thread button and select the outer diameter of the axle surface you’d like to add a thread.

Here we are!

Do you have troubles to make the threaded surface visible? Read more about this problem.

Insert a threaded hole

I’ll start with a simple block.

Select the Hole Wizard…

… and select the parameters for the hole.

Select the tab Positions and click on a define place on the part. In this case I’d like to have a threaded hole in the centre of my part. This is not as simple as it should be. Click on a random point on the top surface…

… press Escape and drag the hole to the centre point (origin).

Press OK and everything should be fine now.

Do you have troubles to make the threaded surface visible? Read more about this problem.

When you add a Smart Dimension in a drawing the thread type will be shown in the dimension.

3D Part

I see only the Dmin in the part but I’d like to see a threaded surface.

Right click on the Annotations folder in your feature tree and select Details…

Enable the ‘Shaded cosmetic threads’ on the upper right corner.

Press OK or Apply and this should to the trick.

2D Drawing

When I create a drawing from this part I’d like to see the thread in the Shaded Isometric view as well.

Go to Tools, Options and select the Document Properties tab. Select Detailing and here we’ve got the same Display Filter section. Enable the Shaded Cosmetic Thread checkbox and finish with the OK button.

Press OK or Apply and this should to the trick.

Even anno 2010 SolidWorks hides some features and visibility options on strange places.

I’ll use a SolidWorks file that I used for rendering the logo of Young Dutch Design.

Add a camera by right clicking on the Lights, Camera and Scene folder in the Feature Tree.

Set up the view you prefer and set the target point. This is the point the lens will focus on so I’ll manually select the first grey sphere. In the image below you’ll see a top view of the sphere’s.

Scroll to the bottom of all the options and turn on ‘Depth of Field’.

This is the most important part. Set the d value so that the solid blue rectangular surface is on the part that need the focus. Set the f value such that the surrounding components are quickly faded/off focus.

Hit the apply button on top and start rendering after you’ve set the scene and the appearances. If you need some info about this part read Rendering realistic chrome with SolidWorks.

This is my result! Be careful, don’t make the f value too small because it will look very unnatural.

• 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!

This is my sketch with a spline on it.

Go to reference geometry on the feature command bar.

Select the spline and one of the points on the end of the spline.

Apply the plane and here you are! A plane at the end of a spline with a perpendicular relation!

Example

Just create a new sketch on the plane you’ve created and draw a circle on it with the centerpoint related to the spline.

Add the feature ‘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!