Some time ago I posted This Thread asking how to use cutter comp for threadmilling in conversational. As it turns out I was able to find a better way, thanks to the help of the forum here - just use a location block (seems so obvious now).
Well, the threadmilled holes are in these parts, and I thought I'd post up how they came out. The pictures are clickable thumbnails.
First, the setup. I used a cheap 3-jaw lathe chuck to hold these round parts. This is my test setup, just a leftover slice of CPVC that I used for testing out the threadmilling programming.
You can see that I made a set of soft jaws to hold the part, and my test piece is much smaller than the softjaws which is why it's up on the parallels. Notice how nice and clean the machine is?
When I got the threadmilling programing squared away it was time to make the parts.
Not a Hurco! That's my helper Mark turning out the blanks. He faced one end and turned the taper on that Colchester lathe. He's running about 700 RPM and 0.020 feed with a shallow DOC. There's a bunch of parts stacked up on that board on the ways. We ended up making a few hundred of these. Did you know that 4.5" diameter CPVC rod is about $10 per inch?
This is a blank in the lathe chuck. The outside sleeve with the 2 arrows on it is because the OD of the part is tapered to make a press fit inside the 4" pipe. The sleeve has an opposite taper. It also protects the tapered surface. The machining operations are to hollow out the part, leaving various internal bosses for mounting a set of circuit boards. Then blind holes are drilled for #6 self tapping screws. One unthreaded hole, and two holes to be threadmilled, are then helically interpolated. The final op is to threadmill the two 3/4-NPS threads.
To do the stock removal I used a 1/2" 3 flute rougher from Niagara. I used 1/2" depth of cut, either full width slotting or half width stepovers, running 1200 RPM and 60 IPM. I had to open up the allowed tolerances in the control to be able to contour at 60 IPM. I believe I could have used more DOC and feed. The endmill worked absolutely wonderfully. The rougher chipped the CPVC into nice little pieces, unlike CPVC's usual desire to make long strings (the long strings on the table are from the finishing endmill used to helical the holes). That black nozzle with blue tape on it is my chip blower. To get the chips out of the 1.1" deep cavity that I was creating I used a shop vac hooked up in reverse as a blower, and wired it to the flood coolant contactor. This worked great but was a little messy. It looked like a snowstorm inside the enclosure.
Loading a blank. This is about 1/3 through the parts. Remember how high the lathe chuck was? At points it was totally buried in CPVC snow. I emptied at least 5 30 gallon trash barrels full of CPVC chips, not counting the chips Mark made with the lathe. These parts would be suited to injection molding, which was my first plan. The customer delayed so long that there was no chance of getting a mold made, qualified, in production and the parts made in time - so we made them from barstock.
A finished part. The few chips that stuck to the tools are pretty obvious, and were simple to clean off while changing parts. The chip blower piled most of the chips up on the right side of the machine. You can see how much of the original CPVC bar is gone. The part went from about 18 ounces weight to about 6 ounces weight. You can see the shop made threadmill on the far left of the picture. Spindly looking, isn't it? It's a shop-made "single point" threadmill - I just turned a 1/2" diameter hardware store piece of cold rolled steel to a 60 degree "v", turned the shank down, milled four teeth in it, and hand-filed top and side relief. It is a 0 degree lead angle cutter, and it worked far better than I had ever hoped. I was only cutting plastic, after all.
Looking into the part. The mounting bosses for the circuit boards are 1/2" high, and their locations drove the selection of the 1/2" rougher for the major stock removal. The rough texture is desired, as this gets filled up with urethane for water resistance when it's complete. The two holes at the top are the ones that are threadmilled. The threadmilling ran at 1000 RPM, 50 IPM and made acceptable threads, though there was some "faceting" because I needed to increase the control's allowed error to get 50 IPM. The total part time, including 3 toolchanges, was about 4 1/2 minutes. I think I could have reduced that perhaps 30% more by improving the toolpaths (which were done in conversational) and taking more DOC with the rougher. I did learn a few points to improve cycle times, most importantly load your first tool at the end of the program, which means you don't need a spindle orient cycle starting from 0 speed - the spindle can orient while stopping for the tool change.
Another look at the CPVC snow inside the machine. The drifts on the table were 6" high at times - this may be one of those times as the lathe chuck is about buried.
I did take some videos of the steps with my camera, including the threadmilling, and I'd load them onto photobucket if there's interest.