How to Make a CNC Turner's Cube - [ Creative CNC Project ]

How to Make a CNC Turner's Cube:
[ Creative CNC Project ]

The Magic of the Turner's Cube

The Turner's Cube is a fascinating object. In the old days, novice machinist's were handed one and told to work out how to make one of their own. It was considered a good test to give a budding machinist to see whether they could first understand how to go about making one and second to see whether they could operate the machinery to the level of precision needed to produce a nice cube.

It isn't just machinists who love Turner's Cubes. After seeing my first example, my wife immediately appropriated it for display in the kitchen. She later asked me to make her a small one for a pendant. Color me surprised as most of her input on my machine so far had been to hold down the costs and quit dragging chips into the house!

Here are some spectacular examples of the art:

In perspex and displayed on an edge by Mark Thomas...

Even under construction Mark's work is beautiful. Kind of like a flux capacitor for the De Lorean!

Lots of embedded shapes are possible with CNC. They'd make pretty Christmas tree ornaments!

This cube was made by Marcel Beaudry. Sticklers will tell you it isn't truly a Turner's cube unless the interior shapes are free to float. You can make that happen with an undercut using a cutter with flutes larger than the shank. For example, use a dovetail cutter...

A Jack in a Cube...

Turner's Cube Dimensions

After seeing enough different examples go by on the web, I got the bug and decided to try to make one. Working out the dimensions is the first problem. For a given cube, one needs to understand the diameter and depth of bore needed to produce the desired effect. This sounds like a job for the G-Wizard calculator!

So, I added a quick and easy calculator that takes your face width and cranks out the hole diameters and their depths:

Here is the calculator set up for a 4" face width...

To figure out the proportions the calculator uses, I went through through a few quick iterations looking at Rhino 3D models to create a pleasing result:

Squaring Up the Block

The first place to start making a Turner's Cube is to square up a block of material. My project calls for a 2 1/2" square block of material, but you could scale it to any size or you could use the spreadsheet or you CAD software to figure out your own dimensions. If you're going to be making the cube through manual machining, I recommend squaring the block to exactly the desired dimensions of the cube. Then you can either bore out the holes on the lathe or the mill. However, if you plan to use CNC, just get the block square and either exactly the correct size (realizing that "exactly" means to you tolerances, as decorative art a few thou will be fine) or just a little larger. The main thing is that you be able to set it in the vise squarely, which means the stock needs to be square.

Here is an example of how I go about squaring up a block of aluminum:

That's my DeWalt Multicutter, a killer carbide saw for chopping metal. Works way better than an abrasive chop saw or the slow 4x6 metal cutting bandsaw I used to use!

It took about 30 seconds to chop that block of aluminum off...

Next, I locked that block down in the softjaws of my 6" Kurt vise on my Industrial Hobbies mill. The face mill is a 7 insert 3" diameter Lovejoy 225 that I got off eBay for a steal brand new from Lovejoy. Really a nice cutter and is much faster than a fly cutter for this sort of thing. The finish left behind is not bad, but a well tuned up fly cutter will still leave a nicer finish. This cutter is running at max spindle rpm (1500) and the fastest my power feed will feed. Depth of cut is about 0.020". It just sings right through the material.

Once you've got the first face square, flip the block upside down and do the second face. Those two faces should now be parallel to one another. Be sure to either use parallels or the soft jaws to sit the block up high in the vise. The sides of the block have not been machined and you want to minimize their effect on the procedure.

Now that you've got 2 sides parallel, bury the cube down in the vise with the jaws bearing on those 2 sides and do the 3rd face. When that's done, flip it over and catch the 4th face. That just leaves the top and bottom of the cube. There's a trick to these that I learned reading Machine Shop Trade Secrets. Cut the 5th face, with the cube buried in the jaws. Now flip the cube upside down, but turn it 90 degrees as you flip it. Mill the 6th face. All sides are now square except for the 5th. Flip the cube again and mill that 5th face. Your workpiece is now square, meaning the sides are all parallel and at right angles, but the width of each edge may not be identical.

Let's recap the milling steps to square the block:

- Put the rough stock on parallels or on a softjaw step in your milling vise and surface the top.

- Flip the block so the freshly machined face is down and surface the top. Now we have 2 faces parallel to one another.

- Bury the block in the vise with the jaws bearing on the 2 parallel sides and surface again.

- Flip the block upside down and surface the 4th face.

- Now there are just 2 faces left, and there are 4 faces square to one another. Bury the block with 2 of the 4 faces against the jaws and an unsurfaced face up (the other unsurfaced face is at the bottom. Surface the 5th face.

- Now flip the cube upside down, and rotate it 90 degrees. Surface the 6th face.

- Your 5th face (on the bottom right now) is not yet square. Flip the cube again and surface that face.

All sides are now square to one another, although the dimensions of the workpiece may not be square. Measure the different dimensions and see what to do next:

I used my surface plate and height gage to measure the cube, and just wrote the dimensions onto the cube faces. The two faces you can see are on sides measuring 2.503" and 2.436". As I'm striving to get to 2.350", I have marked how much material I want to remove from each face. This is another job for the face mill, although you may want to try something finer for the last finishing cuts. I didn't bother as this is my first cube and I had no idea how it might turn out. I got it within +/- 0.001" in thickness, and the sides measured to 0.001" in squareness as well with my tenths indicator. More than satisfactory for this project!

For a tip or two about precision face milling, check the milling techniques page under "Accurate Z-Axis Adjustment". Also, check our page of tips to make sure you're getting the best possible surface finish from your milling. There are a few tricks to try!

Manual Machining: Things Are About to Get Very Boring Now

I started out trying to make Turner's cubes on my mill and lathe with manually machining and botched up 2 tries. I got closer with the mill, but I think that was dumb luck. The mill attempt was first, and failed when I flipped the cube but made a mistake in lining it up. The lathe attempt failed because my first spreadsheet had an error. I made what they called out, but it wasn't a Turner's Cube because the bores were too large. Doh!

Important tip: Do your bores on two adjacent faces (faces at right angles to one another) first and you'll see the error of your ways before wasting too much time.

As you must have surmised, the Turner's Cube is an ideal 4-jaw chuck exercise. Many HSM's dread the 4-jaw, but I find it is my second most commonly used chuck, next to my 6-jaw. Maybe you'll like my trick for squaring up rectangular workpieces that I've show here. I use a bubble level to get the face level, then I drop my height gage onto the cross slide platform (mine is flat) and measure the height of the face. This is compared to the height of the opposite face. If you are measure like this, it pays to record how much movement can be had by a full twist of one of the jaw screws. On my 4-jaw, it's 0.140" per turn. Once you know how far off you are numerically and how much a turn gives you, the process goes much faster. As you can see, I got it lined up within a thousandth!

Once we have a face lined up, we're going to go through the whole series of bores before removing the cube to work on another face.

I did not complete a Turner's cube via manual machining, because about that time I got serious about converting my mill to CNC. So this story ends with the manual version incomplete (sorry, you'll have to work through that one for yourself), as I move on to CNC.

CNC Machining: Circular Interpolation is Your Friend!

Let's assume you've got a piece of squared stock ready to go. By squared, I mean the faces are appropriately flat and parallel or perpendicular to one another. The dimensions may not be square, but each one is at least as long as the finished cube's dimension. Making the Turner's Cube from that stock on a CNC mill is pretty easy. To do so, we need to be able to drop the workpiece in the vise with predictable alignment, let's say predictable to the lower left corner of the cube. The Y and Z predicatability will come from step jaws or parallels on a properly trammed in vise. The X may come from a workstop. I like to use a Kant-Twist clamp on the jaw.

So now we can drop the piece on the vise, and because of symmetry, we can run one CNC program on each of the 6 faces, and we will be done. That CNC program does the following:

1. Surfaces the face until we get to the desired z-height. Let's say we zero Z at the top of the parallels (or step on the jaw). Then Z = 0.000" is the bottom of the workpiece. If we want a 2.500" cube as is called out on the drawing above, we surface until we get to Z = 2.500".

2. Next we cut a series of concentric circular pockets, the diameters and depths of each pocket as called out on the dimensioned drawing. That drawing uses a minimum of 0.250", so we can use a 3/16" endmill to avoid a tool change. Based on that drawing, we want the following circular pockets:

- 1.856" diameter to a depth of 0.500". In other words, cutting from z = 2.500" to z = 2.000".

- 1.237" diameter to a depth of 0.750". In other words, cutting from z = 2.500" to z = 1.750". I give the full cut range so I don't have to worry about rapids hitting the edge of the pocket for some crazy reason. We can optimize it better, but it may not be worth worrying about.

- 0.619" diameter to a depth of 1.000". So cutting from z = 2.500" to z = 1.500".

- 0.250" diameter to a depth of 1.500". Cutting from z = 2.500" to z = 1.000". In theory, I could cut this to a depth of 1.250", and the other side meets in the middle. I am cutting all the way through just to make a nice clean hole.

Note that you won't need a CAM program for this--surfacing and cutting circular pockets are both operations the Mach3 wizards support very nicely right out of the box.

I'll structure this as 2 CNC programs, since I need to surface and then I need to interpolate some holes. To save on tool changes, I could surface all 6 sides with the same tool, and then start in on the holes after a tool change. I've got some new tooling I want to play with as well, so I'll do some of the work with different cutters.

Let's get started!