This tutorial is about how to make a cylinder pressure spring in SolidWorks. This spring is not static but dynamic. In this case I mean that the length of the coil is variable, but the amount of revolutions is not. A very realistic pressure spring which can be used for animations or other purposes.
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!
Comments (9)
Leandro Filipe Sousa Pereira says:
Only Fantastic
Rob Yorke says:
I am having difficulty with this,
Once the new part has been added, and the centre line is drawn, how does it allow you to relate dimensions to an external part?
When I try to add dimensions to the other parts in the assembly therefore allowing for the external models to alter the length of the centre line it flags up a problem and doesn’t allow the smart dimension to work.
Please help!
Crispijn says:
Well, this isn’t easy to explain in text but I’ll try…
After you’ve inserted the new part select the face that is the bottom of the spring in your assembly. Draw and dimension the circle and exit the sketch mode. Add a new sketch in the current part and sketch it on the base plane that is perpendicular on the first one.
Draw a line from the center of the circle you’ve created (this has to be no problem because it’s the same part. To add relations between two parts just select the face of the existing/defined parts and select the endpoint of the line. Now add a relation Coincident and that should be fine…
What version of SolidWorks are you using? I’ve tested this method from SW 2008 up to 2010 and everything should be fine…
Morten Falnes says:
Great tutorial! I’ve used this in an assembly of my own and it works, but I am now struggling a bit with the animation part. I can only get it to move/compress when I do it manually.
Have you made a tutorial for this or do you have any hints?
Cheers!
Lou says:
Thank you Crispijn for the lesson. That’s very cool way to build a spring on the assembly. I followed your instruction and everything came together.The only one part I couldn’t figure out is when I tried in motion study the spring comes out of the shock, nothing holds it in to get compressed. Could you tell me what is it that I am doing wrong? I’d highly appreciate that.
Thank you
Lou
Crispijn says:
Hi Lou,
Are you sure you have related borg ends to a surface? Did you already tried to render the simulation because SolidWorks needs to rebuild every frame – so every little displacement.
Good luck!
Lou says:
Thank you Crispijn again that worked well, pretty cool stuff.
Lou says:
Thanks again Crispijn, that worked well, pretty cool.
lou says:
Hi Crispijn,
I am trying to build a website for assemblies that are made with various parts. The problem that I am having is that when I save the parts, I don’t really have a distance between the virtual camera and the part, so the parts don’t have a relation between each other as far as the scale goes. So same of the parts are saved closer and they look bigger than some other ones that are saved further out. I don’t know if you could help showing me how to set that distance and resolve my problem. That would be greatly appreciated.
Thank you
Lou