Whatever you think of the fidget spinner craze and their usefulness (or lack thereof) in schools, there is no denying that they’re fun to play with. They’re quite fun (and simple) to design too. Before you start you’re going to need:
- some 608 Bearings (commonly used in skateboards),
- access to a 3D printer (try your local hackspace
- filament for printing.
If you don’t have a hackspace near you, or just want someone else to do the printing I recommend finding a local printer via 3D Hubs.
Import a bearing (not essential)
If you wish you can import a 608 Bearing into Fusion 360, which you may later use to animate your sketch:
- Insert > Insert McMaster-Carr Component
- search for 608 ball bearings
- Click on the part number then product detail.
- scroll down to the dropdown which says 3-D Solidworks, change the value to 3-D STEP and click save.
However you get the dimensions of the bearing (callipers work quite well) you will find that the part has a diameter of 22mm and a height of 7mm.
Design your spinner
Setup some variables
Before I start working on a sketch I like to set up the variables I’m going to need during the process. You can do this by clicking on Modify > Change Parameters and then hitting the plus button next to User Parameters.
As you can see here I’ve defined:
- bearing diameter (22.4mm - bearing diameter + 0.4mm this allows half a millimetre each side of the bearing for filament spread – as no extrusion printer is entirely accurate it’s worth building this flexibility into your design, obviously as you get to know the limits of your printer you can adjust the margins. I find that this works well with the printers I regularly use however.)
- arm length (32.4mm – 10mm between the outside edges of the bearings + 22.4mm so I can do the measurement from centre to centre)
- spinner height (7mm – same as the bearing height)
- offset (3mm – this is the distance between the bearing circle and
Now you can use these values instead of typing numbers into the diameter and other constraint boxes – this has the added advantage that if you need to change any of these values you can just go into the menu and change them globally, rather than having to go through your whole design adjusting each individual instance of the value (variables are good :).
Layout the spinner
Central bearing and first arm
- Create a centre diameter circle (keyboard shortcut: c) with a diameter of
- Now add a second centre diameter circle with a diameter of
bearing_diameterdirectly above the one you just made.
- Select both circles and use the sketch dimension tool to separate them by
Once you’ve done that select each circle and add an offset with the value
Construction lines for even attachments
In order to make connecting the outer bearings to the middle one easier we’re going to quickly create some construction lines. Using the line tool (keyboard shortcut: l) draw a line from the edge of the uppermost circle to the center point – as this is just a construction line accuracy on the outside edge doesn’t matter, however you do want it to be at 90 degrees. Select the line you’ve just created and go to Sketch > Circular Pattern. Select the center point of the circle as the center point for the rotation, and you want “full” as the rotation type. This allows you to divide the circles up evenly. I’ve chosen to divide them into 6 but you can do any fraction you want using this method.
Once you’ve got them in the place you want them, select all of the lines you just created and toggle normal/construction (keyboard shortcut: x).
Now you’re ready to rotate the outer bearing holder around the central one. Click and drag a square around the whole of the top bearing hole so that you’ve got everything that makes it up (you should have 22 objects) and go to Sketch > Circular Pattern again. This time select the centre of the lower circle as your centre point.
Join everything together
There are lots of ways you could join the ends of the arms to the central spinner, the simplest however is to use a 3 point arc (Sketch > arc > 3 point arc).
Use the construction lines you’ve just created to space the ends of the arc evenly on the outer circles and place the third point (the one that defines the angle of the arc) onto the outer of the two central circles when you get the handy intersection symbol:
Once you’ve done the first one you could use circular pattern to rotate the arc around, although I found it quicker just to draw three arcs.
Once you’re happy with the shape it’s time to extrude it. Select the bits you want to extrude:
Then use Create > Extrude (keyboard shortcut: e) to extrude your shape to
spinner height (for this it doesn’t much matter if you extrude symmetrically or not – unless you plan to make it spin, in which case you need to extrude it symmetrically by half
spinner_height. In general though I tend to extrude on one side only).
The fidget spinner will work like that, but it’s not terribly attractive so now you can start fiddling with the shape of the edges using the filet tool (or the chamfer if you prefer sharper edges). Go to Modify > Filet (keyboard shortcut: f) and select both the edges to create an even shape. Here I’ve created a Chord Length chamfer with a Chord Length of 4:
Design some end caps
Open a fresh design (File > New Design) and set up some more User Parameters:
This time you want:
- bearing_diameter 22mm, as you don’t need to allow for spread this time
- seating 11mm – same as the diameter of the inner, static section of the bearing
- hole 8mm (or 7.6mm if you want to be sure of easily putting it together) – the diameter of the hole through the bearings
- pin 4mm – you want this to be a tight fit
- cap_height 1mm (this is the bit on the outside of everything)
- seat_height 2mm (gives a slight offset from the body of the bearing)
- interlock 7mm (5mm each side plus 2mm to allow for the external bits of the cap)
Draw 4 concentric circles (keyboard shortcut: c) with the following diameters:
Duplicate them (cmd+c/cmd+v on a mac):
Extrude (keyboard shortcut: e) the caps to 1mm:
Go back into sketch mode and extrude the seating to 2mm.
Again, return to sketch mode and select the outer of the two remaining circles from one of the caps, and the inner from the other. Extrude these to 5mm:
Last return to sketch mode and extrude the final two circles to a depth of 1mm:
The caps are now complete and functional however to make them a little prettier on the outside and easier to clip together you may want to add a chamfer to the pin edges and the cap edges:
I used purple to pink thermochromatic filament: