I am often in need of special tools that are not available in the marketplace, or when they are, come from unreliable sources and have very poor specs. Recently I have been tooling up our CNC milling machine with quick change tool holders based on the neat Tormach system that utilizes a R8 precision ¾ inch collet in the spindle and tool holders with ¾” shafts and a locating ring for precise and repeatable tool lengths. We have a good collection of holders here at Kraus Motor Co, but I am always in need of more for specialized applications. So I decided to make my own. I started by choosing the right material for the tools.
I wanted a 100Kpsi minimum strength without having to harden the part by heat and risking distortion, and I wanted a metal that I could turn with a great finish. My choice was 1144 alloy steel also known as stress-proof. I procured a bar of 1-½” round stock and started by slicing 2-½ and 3 inch lengths on our horizontal band saw, cutting at slow speed and with coolant. Next I chucked up one of the pieces lightly in a 3 jaw on our manual lathe, rubber hammered the round until it had the least amount of run-out wobble and tightened. Then I lightly faced and drilled a 60 degree pilot countersink to support the round with a live center. Next I cut the round down to ¾ for about 1-3/8 inches in length.
Although I am using a DRO equipped rigid Colchester-Clausing lathe that cuts smooth and true with flood coolant, I take diameter measurements with a digital micrometer and correct my DRO as I approach my final cuts. Using a triangular carbide indexable insert with a generous nose radius, I make sure I’m perfectly centered on axis to get the best cut and finish and the least measurement distortion. My speed starts at about 300 RPM at 1-½ diameter and is up at around 500 RPM at ¾ diameter. Yes the lathe has continuous variable speed. My feed is 0.016 per rev and I reduce it to 0.010 for my final cut . I try to keep depth of cut around 0.035 . The final finish is ground shaft quality. Next I cut a ¼” chamfer at the end to facilitate placing the tool in a collet and drilled a 3/8 hole the length of the ¾ shaft using the tailstock. This gives access to the bore of the tool holder.
In order for the tool holder’s locating ring to be able to contact the spindle nose of the mill and provide a repeatable height offset when the drawbar pulls the collet tight, I need to give the collet nose a bit of space. I do that by creating a .090 inch deep relief with a diameter a bit larger then the collet nose protruding from the spindle. About 1.270 inch diameter will do. This can be done in the lathe with an appropriately shaped grooving tool, but I did it in the CNC mill after writing a quick program for a 2 flute carbide ¼ carbide mill to cut the pocket. The nice thing is that I located my x and y zero by just tightening the newly created tool holder’s ¾ inch shaft in the spindle and then lowering it into a 3 jaw chuck and tightening it around the body of the tool holder before clamping the chuck firmly to the mill table. Then released the drawbar and raised the spindle to receive the milling cutter.
After this it’s back to the lathe and this time I used a ¾ inch 5C collet to hold the finished part of the tool holder . Since my setup is perfectly concentric I can now cut the body of the tool holder down to an outside diameter that will correspond well with the intended hole for the cutter I want to place in it. Keep in mind that there will be a setscrew to secure the cutter’s Weldon shank. For one of my tool holders all I needed is a 0.157 inch hole with a 8-32 setscrew to hold the shaft of a dial indicator that I use to set up my work with. So I turned the tool holder outside diameter to about 1 inch.
Next I cut a 30 degree taper using the cross slide. I like doing this with the spindle turning clockwise so I can cut the backside of the taper and feed the cross slide away from me. The taper is cut by eye until the nose is about 0.825 inches in diameter.
Now I spot drill the tool holder’s nose using the tailstock and proceed to a small drill bit, peck drilling and retracting out every ¼ inch so chips don’t pack up and deviate the bit from a true centered hole. Then I enlarge it by 8ths gradually to a bit 1/64th smaller then my final bore. Finally I use a reamer with plenty of flood lubricant/coolant for my exact bore size. I hold the reamer with the drill chuck, just like the drill bits, but I only hold it by its last ¼ inch, so its free to flex and find the center. Ideally I would use a floating reamer holder, but I am quite confident in my tailstock being centered. To double check it turn a test round bar about 12 inches long held between a spindle center and a live center with a light cut and then run an indicator along the side and top edge.
The final operations consist in drilling and tapping a hole for the setscrew that will hold the cutter or measuring device. For this I use the Bridgeport as a drill press and I use a edge finder to locate the center. If the tool holder is going to be used in a high speed spindle, then I remove a bit of metal from the opposite side of the setscrew hole, to account for the rotational imbalance created by the setscrew hole minus the setscrew. I use a powder loading scale to carefully weigh the chips created by drilling and tapping the setscrew hole, subtract the weight of the setscrew giving me the amount I have to remove. It borders on being obsessive, but that’s what it takes if you want precision.