Quick Change Tool Post
Click for larger view
I have always wanted to have a quick change tool post for the lathe. Currently there are a few companies offering these for small lathes such as the Taig or Sherline models. I was thinking of buying one, but then one rainy weekend I decided to tackle it myself as it looked like a small project which in its own right offered some good machining challenges. I'll outline the general procedures here for anyone else wanting to try making one.
Since it was the weekend my metal supplier was closed so I had to scrounge around the shop to see what I could use. I came up with a 6" piece of 2" rod of 12L14 steel I had forgotten about. It had been laying outside and was completely rusted, but it was the perfect size. Before selecting the rest of the material I drew a quick sketch in Autocad just to give me an idea of the general shape of the post and to make sure I could machine it out of the stock I had found. Fig 1 shows the drawing.
At this point I still didn't have the full design in my head yet, but the only real challenge was figuring out how the pistons and cam would work. I took a look on the web at the many tool posts offered and decided that I wanted a single handle which would operate both pistons together. This is in comparison for example to the Sherline version which uses a separate cam for each piston.
I also wanted to eliminate the need for any allen keys so planned on making the center bolt myself (I kept the hole size standard however just in case I decided to use a cap screw instead). With a built-in handle.
For the rest of the material I used a bit of scrap brass, and for the holders some aluminum 6061 bar stock.
The most important part is the main body of the post. I cut off a 2" length from the scrap rod with the abrasive cutoff saw, and cleaned off the surface rust. The first step was to machine the two outer edges, making sure they were 90 degrees to each other. These edges would be used to register the remaining sides. I used a 3/8 four fluted milling bit and multiple passes, This I did with on-the-fly g-code primarily making use of the G77 auto incremental command.
Once I had these side finished I then milled the other side flat and parallel to the by making sure that the previous sides were registered to the base and front jaw of the vise. Again this was done with some simple g-codes. When this was finished I milled the remaining ends square to the sides. The next operation was to cut the dove tails. I use dovetails a lot in my woodworking so I am fairly aware of some of the pitfalls. I also knew that both dovetails had to be exactly the same size or I would end up with a post that needed separate sized holders for each of the two sides, which would defeat the much of purpose of the post.
The tails of a dovetail are always the easiest to machine and the only real concern was that they turn out equal size. Once again I used one line g-codes, but this time used the ability of Turbocnc to log all my commands to file. This meant that although the first dovetail was a bit tedious, the second was automatic as I just re-ran the code saved in the log file. This is a great feature within Turbocnc and greatly aids in prototyping. I ran multiple passes of the dovetail cutter using very light cuts of 0.02 per pass.
In fig 1 above you can see that my initial plan was to use 45 degree dovetails however I decided at the last minute to go with 60 degree instead. No real reason other than Taig uses 60 degree for most of their dovetail and I thought I would continue along with the same. My feeling now is that the 45 degree dovetails would have given a more esthetic feel to the post.
Once the dovetails were milled it was time to drill the center hole for the anchor bolt. The center isn't exactly in the center as I wanted to make sure that the pistons had enough room to move freely without worrying about jamming. After I had marked and punched the center hole I set up a four jaw independent chuck on the lathe and indicated the point in. Once properly centered around the punch mark I drilled out and reamed a .250 hole.
Once the hole was finished, I took the chuck off the lathe without removing the post and mounted it on the rotary table on the mill. One note here, you don't need a rotary table to build this, it just makes things easier. Once mounted on the mill I centered the mill on the hole in the middle, now by offsetting the milling bit I could cut the channel I needed for the cam.
Milling the tool post body.
The milling procedures was to mill the channel with two passes at each depth, the inner with the rotary table turning clockwise, and the outer .05 offset CCW. Since the channel is quite deep 1.25" it is important to use the offset in steps else there is a good chance the bit will dig into one of the sides. I used a 0.25 milling bit so the finished channel is 0.3" wide.
Once the milling was complete I put the chuck back on the lathe and to a final finishing pass with a boring bit on the lathe. Unfortunately I was a bit careless and went in just a bit too deep and you can see the resulting chatter marks at the bottom of the channel in the photo below. This will not affect the operation of the post, but...
Tool post body and cam.
Following this step I drilled and reamed the holes for the pistons at 0.375".
The next part to make was the main cam. This starts off as a cylinder slightly large than the diameter of the channel in the post body. The body is then turned down to fit the channel leaving a shoulder of about 0.200". A hole needs to be bored in the center too match the center post core. What I did to insure a good fit was to first turn the outside diameter down slightly oversize, then bored out the center, slightly undersize. I then bored the first .25" of the center slightly oversize so that I could test the outer diameter with the actual tool post body. Once the outside diameter was turned to a perfect fit I went back and finished boring out the inner hole, again using the tool post body to test the final size. The result was a very good fit, if I put the pistons in place and insert the cam the pistons a forced out of the post. If I were to put the pistons in place, then seat the cam into place over the final .250" distance with a sharp hand blow the pistons would fly out and dive for hidden recesses in the shop over 10 feet away. Don't ask me how I know this.
Once again the chuck is transferred to the rotary table. if you haven't used the mill since milling the body there is no need to re-center the rotary table. Align the mill bit so that it is just touching the outside edge of the cam. rotate the rotary table until the bit is also lined up just slightly to the edge of the piston hole. You now need to take a serious of cuts, moving the x-axis towards the center of the cam while the cam rotates 90 degrees. The typical G-Code will look something like this:
G1 X5.95 A90 F6
G1 X6 F6
G1 X5.95 A180 F6
G1 X6 F6
This is repeated until the correct Z depth is reached, then X is repositioned and the next serious of cuts are made. I took a total of .200 measured at 0 and 90 degrees. You can see the finished shape of the cam in the photo above. If you don't have a rotary table then you can get the same result cutting an arc with x and t axis defining a center of the arc to be off-center.
(to be continued...)
General view of the Tool Post
A birds eye view of the tool post
A sample of some of the tool holders made so far
Parting tool holder