Fidget spinner beginning

(William Adams) #1

Just wrote up how to draw one up on the support e-mail.

Here’s a file to get folks started if they wish to make one:

Easy download link:

(William Adams) #2

That said, a basic fidget spinner is straight-forward enough that one can make on in Carbide Create:

Job Setup

  • Stock Size
  • Width (X) 100mm
  • Height (Y) 100mm
  • Units
  • MM
  • Document Background
  • edit to have 5mm spacing

Metric is used since typical bearings (and the one used for this example) are measured in metric.

Carbide Motion does not show cutter position
(William Adams) #3

Start by going into design and drawing a circle at the center of the page. Change the radius to make a circle the diameter of a 608 bearing (11mm):

Copy the circles, and selecting the top or the bottom drag them into position so that they are placed along the vertical centerline and equidistant from the center:

Select the bottom-most circle, clone it (control/command c) and re-position the clone so as to be stacked on the original. Then rotate it 60 degrees about the center of the page:

repeat, but rotate -60 degrees around the center of the page.

(William Adams) #4

Duplicate each circle, numerically position the duplicate over the original, and change the radius to 20mm:

(William Adams) #5

Select two or three of the larger circles and Boolean union them to begin to make the outer profile of the fidget spinner:

Continue until one has:

(William Adams) #6

With the design done, one turns to CAM. First considerations:

  • material
  • endmill

To make this simple, we select HDPE, and a 1/4" #201, so that we may use the numbers from the official Carbide 3D feeds and speeds chart:

  • Depth per Pass: 0.125"
  • RPM: 21500 (4 or so on either a Makita or Dewalt dial)
  • Feed: 80" / min.
  • Plunge rate: 40" / min.

Go into Job Setup and change to Imperial measure (and set the material thickness to match the material you will be machining), then select an inner circle for a bearing and go into Toolpaths and set the feeds and speeds:

  • Toolpath | Contour | Edit

  • clear the “Set speeds automatically” checkbox

  • Cutting Parameters

  • Depth per Pass: 0.25

  • Stepover won’t matter since we’re going to cut slots, not pockets

  • Speeds and Feeds (per minute)

  • Spindle Speed — this is more of a note on a Shapeoko (it would be nice if the software would mention the speed and note an appropriate dial setting when sending the file)

  • Feed Rate: 40

  • Plunge Rate: 40


Then set the Toolpath options:

  • Cutting Depth — click “Use Stock Bottom”
  • Offset Direction — select the radio checkbox for “Inside / Left” for the bearings
  • Name — always enter an appropriate name for the Toolpath, if feasible, only select one region of geometry at a time to cut (otherwise the machine will lift out and move to the next with each pass, potentially greatly increasing the machining time).

Repeat for the balance of the inner bearing holes:

(William Adams) #7

Enter appropriate settings for the outer profile:

  • Offset Direction — select the radio checkbox for “Outside / Right” for the outer profile

Preview the toolpaths:

Be certain to test the feeds and speeds on a scrap piece before cutting.

Clamp the stock in place, home the machine relative to the desired origin, and cut.

(Carl Hilinski) #8

How would you have done the spinner using your original drawing instead of the one for which you gave the step-by-step? Would you have used another set of circles to get the concave connections between the three outside circles and then joined them in the same manner?

(William Adams) #9

The original image would have had pretty much the same toolpaths, center, top, right, and left for inner profiles, then an outer profile along the perimeter — should be the same, just skip the drawing/creation steps.

Please let me know if there are any difficulties with the files or instructions — the young man who asked about this on the support e-mails said:

… I made some time and (have) been making fidget spinners like crazy the shapeoko 3 is the best machine ever

(which I was very relieved at — hopefully his parents will grant him permission to share some photos)

(William Adams) #10

Oh. Now I see what you mean. You mean how would I have drawn the original image.

Yes, rotating a couple of properly sized elipses around after drawing them would have worked — I did it in Freehand though, using circles, rectangles, unioning and then the pen tool, since it was faster to draw there than to describe. I’ll try to find time to work up a similar tutorial in Inkscape.


(Carl Hilinski) #11

I’m not sure a tutorial about how to do it in Inkscape is necessary. I was wondering how you would do it in CC because I think you’d have to add three additional circles to get that concave “web” (it reminds me of the webbing on a duck’s foot). If I were doing the spinner, I’d do it in F360 and use a three-point arc to do the “web” but I don’t remember if there’s an arc tool in CC.

(William Adams) #12

There is a Bezier curve tool, but it’s extremely limited for some reason. I’ll see if I can puzzle out a way to do this in CC. Thanks!

(Jesus Martinez) #13

the link is not allow for download - it open a page with the image that is all ??? Thanks

(mark robinson) #14

Right click the image and save as

(Jesus Martinez) #15

Awesome - Thank You - pls help me
I try to export my file as a DXF file and I got an error, I post on the forums, but no one reply, could you help me? pls see attach of error message

(William Adams) #16

Here’s a zip archive which ought to work: (1.3 KB)

(William Adams) #17

For DXF import issues:

Import DXF

  • it may help to use the OVERKILL command to eliminate any overlapping or intersecting paths before exporting from AUTOCAD
  • AutoCAD 2000 DXF format (model geometry only, base model scaling) export from the desired face (not isometric view)
    2004 Lines

If that doesn’t work, post the file or send it to