The Turner's Cube we are going to make is an interesting little project that originally came from beginners learning to work in the metal shop. The seasoned old veteran or shop owner would hand one of these to a new apprentice and tell him to figure out how to make it and reproduce it.
For me it was a fantastic first project on the Tormach CNC Mill at the TechShop: http://www.TechShop.ws
In this instructable you will learn how to make a Turner's Cube and in the process practice your skills and precision needed to tackle much more difficult projects and open the doors of all the incredible things you can make using a metal mill.
Metal Bandsaw (horizontal and/or vertical)
Square or Center Finder (ruler works fine too)
CNC Mill (Such as the Tormach 1100 at the TechShop)
1/2" End Mill bit
2"x2" cube of aluminum
For my tutorial on designing the cube in AutoDesk Inventor 2012 go here: https://www.instructables.com/id/Turners-Cube-Designing-in-AutoDesk-Inventor-Pro/
Step 1: Step 1 - Creating a Perfect Cube
The most important and often most challenging step of this process is milling a perfect cube.
The tolerance for the cube must be within .01 inches or it will be visibly off.
Cutting the blank
First get yourself a chunk of aluminum. It can be just about any shape but you will need to get it roughly to 2"x2". This can be done with a horizontal and or vertical bandsaw. I started with a 4"x8"x2" blank and made one cut on the horizontal band saw and then again in half on the vertical band saw.
The more care you take in getting it cut at straight right angles the better for later on.
Measure the blank with calipers and get a rough idea of how long each side is.
Facing the cube
This was the trickiest part for me; measure twice cut once!
I started off spending a lot of time learning how to zero all the axis of the Tormach. This should be included in the introductory class from the TechShop and you should already be somewhat familiar with this process. Be sure to check both ends of the vise for being at Y0.00 I try to get within .003 inches to be sure my precision is good enough. Don't forget to account for the width of the edge finder when finding zero (0,0).
Find the two surfaces that are the most parallel and put them against the faces of the vice. Below the piece I used a set of 1/2" parallels. At this point it wont make much difference and just about none of your faces are square yet.
Find your Z zero by starting the spindle and lowering it close then jump stepping till the bit cuts in. I used .002 steps here. Zero out your Z axis. Remember EVERY time you reset your piece in the vise you need to find your Z axis zero again. If your face is closer to finished you can lower the bit without the spindle moving till a piece of paper no longer slides between your piece and the bit, then set it at .003 (the thickness of a piece of paper)
Using the jump step settings on your CNC Mill bring your spindle about .05 below z0 and start to face the top of the cube. I would usually bring the bit left and away from my piece, use the Gcode g0z0x-1y0 to bring the bit to z0 then I would set the jump step to about .05 and jump down one step so you are at z-0.05 then set the jump step to .25 and the spindle speed to 7. Start slow and use the override at 50% and work up from there as you get comfortable. I would manually move the bit back and forth across the face with my stepover never exceeding .25
Once my top is machined flat, measure the top to bottom and using the same faces that were against the vice, orient the piece bottom up.
Calculate how much you need to take off to get to 1.875 inches (the final thickness of the cube), find zero again and face the surface down at about .05-.1 thickness max depth at a time. Measure twice and be sure you have your math right. Better to face it in a few paths than screw it up now. There is no shame in leaving the cube roughly at 1.925 inches and doing the final dimensions when you are sure you have your cube faces all perpendicular and clean.
Repeat this process until you have a perfectly square cube at 1.875 in choosing the most square sides to put against the vice sides and bottom you can with each face.
Congrats, one of the most challenging parts is over!
-Use some compressed air each time you reorient the cube to be sure there are no metal chips between the vise and parallels and your cube. Once chip can screw up the entire precision.
-Remember to wack the top of the piece with a mallet after you tighten the vice to be sure the parallels below are held firmly and snug the vise one more time. Several of my mistakes came from the piece moving slightly in the vice when machining.
Step 2: Step 2 - Drilling Center
Use a center finder or a square like the one pictured above and scribe an x in the very center of the piece.
Use a 1/4" drill bit and the drill press to drill a hole through the three axis.
Be sure to use liquid coolant and move the bit up and down throughout to not damage the bit or your piece.
Pretty simple step but take your time.
Step 3: Step 3 - Milling the Piece
Upload the stl file i included into the CAM program (I used Cut 3D)
The settings I used in Cut 3D were:
.5in End Mill
Speed 5000 rpm
Feed 7 inches/min
Plunge depth .1in (to ensure three passes)
Plunge rate 2 in/min
Origin to xyz at top left corner
I only used a roughing pass and set the machining tolerance to .0001 The fine tool-pathing is unsuitable for this project.
Start off slow, find your z0 using the paper method and begin with an airpass. Go to z+4.0 (Gcode is g0z4) and set z to zero. Then run your program once all the way through to be sure you have everything correct. This will run your program 4 inches above your piece.
Bring it back to z0 and set it to the proper z value as z4 again.
You are ready to run your first toolpath. Start it off slow at 50% override and as things look good you can slowly raise it back up to 100%.
If you have managed to make it through all 6 faces and did not mess up congrats! You have achieved the basic machining skills to be very successful in future projects!
Step 4: TroubleShooting
Well if you screwed up join the crowd. This was a very challenging first project for me.
My first mistakes include:
Not starting with a perfect cube.
Having to make my cube smaller than planned because I went too deep on the manual facing several times.
A couple divots in my piece when it moved in the vise.
Forgetting to change the machine tolerance to 0 or .001 so the cube needed another pass on each face.
Tips for avoiding and fixing errors
GO SLOW and measure everything twice!!
If you end up with a smaller cube than expected you can figure out based on the current dimensions where x,y,z should be and set zeros in space to there.
For example. If your cube ended up being 1.85in on each face instead of 1.875in, find your actual x,y,z zero and add .0125 to each (gcode g0x-.0125y.0125z.0125 and then zeroing all axis assuming you are starting at the top left corner for zeros, the x axis is minus in that case). This is because the difference is .025 and the cube is half that thickness less on each side. (1.875-1.85=.025, .025/2=.0125)
If you get done and the cubes are not distinct enough with the corners being attached with too much material you can add additional thickness to the z axis and run your program again on each face. For example I wanted to make mine a bit more defined so I needed to take off an additional .05 thickness of each face. I found my z zero and then set it so it was actually z0.053 (my added thickness and the thickness of the paper i was using to set it to zero). I ran the program again on all the surfaces, scribing marks on the surfaces I hadn't done to keep track.
If your piece jumped out of place in the vice don't fret. Just finish the piece as you should and then reface the entire cube again afterwards below the ding in it.