Making Small Turner's Cubes

Squaring the Cube with a Face Mill

Before an accurate cube can be made, the stock must be squared. The proper procedure to square stock is as follows:

1. Place material in vise that is approximately to size. Set it up high on parallels because the sides the vise will clamp to are not yet square. Face mill top side, leaving a little margin for milling the face opposite this one.

2. Flip part upside down. face mill this side to a depth that results in the correct square dimension for these two sides.

3. Bury the part deeper with the jaws on the two freshly faced sides. Make a face mill pass over the top.

4. Flip freshly milled side #3 down and face mill the side opposite. Depth of cut should result in the correct square dimension for these two sides.

5. Position the material to reveal the 5th side, not yet milled. The jaws are bearing only on squared sides, and the workpiece should be buried well down in the vise. Face the 5th side.

6. Flip upside down to expose the last face. Rotate the cube 90 degrees. Face mill that last surface. Leave a little extra versus the square dimension.

7. Flip upside down again and surface a last time. Depth of cut here should ensure the correct square dimension.

Okay, now let's work that procedure out for a CNC.

Let's say we want to do this for a cube that is 1" on a side. Let's further assume that we will be using parallels that sit the workpiece 0.22" below the top (we'll use this one when be bury it "deep") of the vise jaw and 0.12" below the top (we'll use this one when we sit the workpiece "high"). Any parallels will do so long as the result holds the workpiece securely and high enough that our face mill won't cut into the vise jaws.

Let's further leave an allowance of 0.100" when we are not trying to cut to dimension.

So, now our steps look like this:

We can choose to vary the stock height, the different parallel allowances, and the slop allowances (based on how accurately the rough stock is sawn to size and squareness).

Squaring the Cube with an Endmill

Okay, we can use the Face Mill approach, but it requires a lot of manual effort. Let's try another tack and see if we can use an Endmill. Let's say we have some 3" wide by 3/4" thick 6061 aluminum. We want to get some cubes out of it that are exactly 0.600" on a side. Further, let's say we plan to do this with a 1/4" endmill, so we need a minimum of 0.6 + 0.5 + 0.6 + 0.55 + 0.6 = 2.8". So, each 3" section can be something over 0.7" long and still include 3 cubes. Let's go on to say we're going to do 9 cubes in a 3 x 3 array at a time. Lastly, we are going to machine the cubes as an array in the vise on parallels that end 0.12" below the jaw tops, and leave a pad that is 0.1" thick on the bottom (that's a little below the jaw top so we had better be careful!) to hold them together and be gripped by the vise. We will finish the block of 9 except for the bottom face that is embedded in the pad. We will then saw the 9 apart, and individual mill off the 0.1" pad to get a cube. In fact, we can mill them off 3 at a time in the vise.

For our CNC program, we will have Z=0 be the top of the parallels, which are 0.120" below the vise jaw top, so we are working in positive coordinates. Normally we work negative (top of workpiece is Z=0), but positive will make things a little easier for us. So, to set the zero, we touch off the top of the jaw in Z and set our Z to 0.12" (the parallel is 0.12" below the jaw).

Here are the steps:

1. Insert the rough sawn workpiece, which will be approximately 3" x 3" x 0.75" in the vise. Take a shallow face milling pass to true the face. Our work is sitting circa 0.75" above the parallel, which sits 0.12" below the vise jaw top. If the top of parallel is 0, we want to face until Z = 0.600" + 0.12".

2. Run a CNC program that profiles nine 0.6" x 0.6" cubes to a depth of 0.72 - 0.610" = 0.100". We're cutting a little deeper to make sure we will be free and clear of the pad.

3. Saw the workpiece into 3 pieces, each with 3 cubes.

4. Place a 3 cube piece in the vise and face mill to a depth of the finished square height, or 0.6".

Let's plan to use a 3/8" endmill. For roughing in the full slots, we will run it at 1600 rpm and 0.25" depth of cut, which gives a feedrate of 10 IPM. We'll run a finish pass 0.010" at half that feedrate.

I'll use my Glacern 45 degree 3" facemill for the initial and final facing passes. We'll take cuts of 0.030" at 1600 rpm and 30 IPM.

Here is the G-Code:

First Facing Pass: Assumes Z=0 top of parallel, workpiece XY=0 left corner of fixed (rear) vise jaw. Material height is 0.750 and we will face it down to 0.720". The CAM program will make 2 30 thou passes starting at 0.720 + (2 * 0.030") = 0.780"

Profile Pass

Finish Facing