View Full Version : How to turn an angle - NOT a taper

11-09-2015, 04:28 PM
Hello All,

Looking to make a fixture for making a part with a 1 degree angle in it.

Looking to make a .75" dia pocket/recess in the end of a shaft 1" shaft. Pocket needs to be 1 degree off relative to the shaft OD.

I'm not particular about if the pocket is offset/not centered. or if the pocket is at 0 degrees and part of the shaft is angled instead, that is to say if the shaft was no longer consistently 1" OD throughout due to an angle being machined into it, that's fine too.

I have a small lathe and a small mill with at least some of the normal tooling that goes along with them.

Any suggestions other than to make both normally and then drive over the bar with a precision calibrated truck? I'm thinking with the right packing in the jaws of a 4 jaw chuck this should be achievable, but getting it setup will be a real pain.


11-09-2015, 04:44 PM
Use a milling machine for the angled stub.
The work mounted on the lathe cross slide works also.

11-09-2015, 05:16 PM
You can put the part in v blocks in the mill vise on a 1 degree angle and drill the hole. It almost sounds like making a rotary broach.

11-09-2015, 05:56 PM
You might not have enough height for a drill bit and your part to do it on the mill,
depends on how long your part is.

Unless your rotate the mill head to horizontal.

Or you do the job on the lathe.
Mount a drill in the head stock and then mount your work piece to the compound slide.
If you have a quick change tool post, you could use a tool holder with no tool in it
and clamp your work piece to the slot in the holder, and adjust the holder to center height.
Then adjust the compound angle 1 degree off parallel to the long axis of the lathe and
feed in with the carriage.

11-09-2015, 06:43 PM
Thanks Guys. Without making a really short adaptor for the boring head in the mill or flipping the head horizontal this was a no go due to height. The cross slide idea I like quite a bit, that hadn't occured to me yet and it's seems like the perfect way to approach the job.

11-09-2015, 07:30 PM
Not sure I understand your project but one time I needed to taper a round shaft. The taper came to a point, but the point was tangent to the shaft diameter. Took some thinking. I made a fixture in a round piece of steel. Made an angled hole through the center of the round piece of steel. Insert the round shaft inside the hole. Setup in the lathe the round shaft had a terrible wabble. Turn down until the wabble was
gone and the round piece was pointed with the point even with the shaft diameter.
The piece was an arbor for a spring coiling machine. Jim

11-09-2015, 08:15 PM
You want to do something like this?
http://i1378.photobucket.com/albums/ah106/wrecktm1/anglefixture_zpsmvj7pf6q.jpg (http://s1378.photobucket.com/user/wrecktm1/media/anglefixture_zpsmvj7pf6q.jpg.html)

Depending on the required accuracy, pocket depth and shape of the bottom of the bore, flat or a deeper center hole is allowable, put it in a mill tilted at 1 then use a boring head after roughing with a drill or endmill, easy as that.

Paul Alciatore
11-09-2015, 11:41 PM
Depending on just how precise that one degree needs to be, I think your idea of shims in a four jaw is right on. I am sure with reasonable care you can get it +/- 0.1 degree.

The sine of one degree is 0.0175 so with two shims placed on opposite sides of the work piece, one at the front of the jaws and the other one one inch behind that, you should get that one degree with shims that are half that number thick, in inches. So use 0.0087" shims or 0.009" to round it off. They will probably crush a bit while tightening the jaws anyway. I would use steel shim stock as aluminum would probably crush too much. And they should be fairly narrow front to back, perhaps about 1/8": this is so they act more as single points to pivot on. Measure the spacing from the front edges of both so for 1" spacing the two together would be about 1 1/8" deep in the chuck.

Stick them on the work piece or the jaws with a bit of grease and tighten the four jaw in the normal way. Center the end of the work piece as you want and bore or drill away. If you are drilling, you may want to face it at that one degree angle first so the drill enters square.

Be sure to get it done in one go as it would be very difficult to register it again if it is removed and remounted.

If you don't have 0.009" shim stock you can vary the spacing to match some reasonably close stock that you have. Example, 0.010" shim: 0.020" / sin(1) = 1.146". So with two 0.010" shims you would place them 1.146" apart.

11-10-2015, 12:33 AM
Put the work on your cross slide and your cutter on your spindle. Technically this is a milling operation on a lathe machine, but it works.