Can this be turned on a lathe?

[Matt Adams]

The short answer is: there's a whole lot more you need to know about cutting speeds and feed rate. It really depends on the material the gear is made out of. If it's a hardened spur gear, you can have quite a bit of trouble cutting the material itself.

As for the lathe hitting the drilled out edges, it's a dynamic forces sort of thing since the metal will continually be engaging metal as it spins. I could honestly see this as a, "it's no big deal" or "don't you dare try to lathe that!" situation. You might be better off to just 2nd day ship out the gear(s) and lathe it down.

If you're just looking to reduce weight, it's just a matter of ounces you're looking at since you already have a fairly nice bolt patern in there... is it really worth it?

(I know, it's always worth it when you're 3 ounces over weight. It's also worth it if the hub is interfering with another component)

Anyway, hopefully you'll be able to post a little more information about the gear so that a machinst can throw out some speed and feeds for you, especially in this situation.

Matt

[sanddrag]

Well, the gear is a steel Martin gear. As for it being hardened, I have no idea. All I know is that it was not too hard to drill. It needs to be turned down to fit in our gearbox. If we don't turn it down, we would have to face the hub off to like .125 (which would make it fit in our gearbox) but we'd rather leave the width of the hub since we were concerned about it wobbling on the shaft. It is a 60T 20P gear and having it only .625 wide total might make it want to wobble up near the teeth. We are having a pretty tight fit on the shaft but still the more width you have the more guarantee that it is straight.

Can someone provide a little more specific answer as to whether or not we can turn this?

Also, if we cannot lathe it, how hard would it be to have it go around a mill bit in the CNC mill in a "circular spiral" pattern until the correct diameter is reached?

[indieFan]

Yes, this can be done. Contact a local community college or occupational school and ask to talk to the machining teachers. They should be able to give you all of the information you need.

indieFan

[sanddrag]

Originally Posted by indieFan

Yes, this can be done. Contact a local community college or occupational school and ask to talk to the machining teachers. They should be able to give you all of the information you need.

We have the full machine shop of our local community college available to us. I am probably the most experienced student machinest on our team (having done it for over two years now) but I just have never turned anything like this. I've done hex and square bar just fine but that is not so jagged really. We'll be going in tomorrow and I'll give it a try.

[dlavery]

Yes, you can do it, but you are probably going to want to do it in two steps.

The first part of the cut will be an interrupted cutting operation. This is rather hard on carbide tool bit, so I would recommend using a "standard" tool steel cutting bit, with very light rake (you want all the support for the cutting edge that you can get). If this is one of the standard Martin gears made of 303 Steel, then you will want a surface cutting speed of about 50 ft/min. For a 2.25 inch diameter gear hub this works out to about 85 rpm. Since it is an interrupted cut, you would be safe to slow it down by another 20%. In other words, cut slowly and cut shallow (about 0.010" - 0.015" per pass if you are using a small lathe [1-1/2HP or less]). The tool steel bit should stand up under the shock loads and last long enough to get past the bolt holes.

Once you are down to a smooth cut, switch to a carbide bit. Crank up the surface cutting speed to about 150 ft/min. You should be able to increase the cut depth to 0.030" per pass. You will get through the rest of the cut a lot faster.

Since you are doing this as a "one-off" these numbers are close enough to do the job. If you were going to do 10,000 of these as a production run and were concerned about the very best optimum cutting speeds and maximizing tool life and overall productivity rates, then there would be a lot more we would have to talk about. But for this type of work you should be all set. Good luck!

-dave

[Andrew]

Another option would be to do this on a rotary table on a mill. You might want to check with the shop if they have one.

[ChrisH]

Originally Posted by sanddrag

Well, the gear is a steel Martin gear. As for it being hardened, I have no idea. All I know is that it was not too hard to drill.

If the gear is hardened, it will probably only be locally flame hardened in the area of the teeth. Since you appear not to be messing with the teeth it shouldn't be a problem.

ChrisH

[157#1Driver]

Yes its easy to machine in a lathe, use a collet to hold the part by the gear side. No the collet wont hurt the gear teeth. you should be able to machine it, doens't look like it has been harden. As for the cutting tool hitting the gaps, dont worry about it, just go slow with your feed, the speed the cutting tool moves at. You could probably get away with an rpm of 100 or a little more. Thats what i would do. Any questions or complication just ask.