Speed and feed question for a side mill cut

[hercules]

I am a college student trying to learn to cut some gears on a Haas VMC. I am cutting teeth in a blank using a form cutter held in a side milling arbor on the spindle. The work piece is mounted on and indexed by the 4th axis. I am having trouble getting the speeds and feeds right.

I have a 3" diameter carbide side mill/form cutter (involute, 20 degree pressure angle) and the gear blank I am cutting is a piece of untreated 4140 steel (5/8" thick round), I am using full coolant flow during the cut etc. I can get 50 rpm with 1.3 inches per minute feed to work OK but it takes 7 hours just to cut a 28 tooth gear that way. I have 12 gears to cut and some are much larger. I must have something wrong. I know industry would use a gear hobber. We don't have a gear hobber but the gears aren't really the point, learning to use the VMC is.

Have I done the speeds and feeds wrong? Can anyone help me with some advice on speed, feed and depth of cut that should work as a starting point for this work? I would appreciate some advice, it just seems to me that the work is taking way too long given that this is a full sized production machine.

Pat

[jackson]

can you get a pic of the cutter and post it

[CarbideBob]

50 rpm with 1.3 inches per minute ?
Ok I give, why is it spinning so slow? A 3 inch carbide cutter in alloy steel (4140 thru 6150) should be spinning at least 150 RPM with about 400 being tops for an uncoated tool (150 to 350 SFM). You didn't say how many teeth in the cutter so I can't judge your feedrates but be sure to feed faster when you speed up the spindle. How deep is the gear tooth and how many passes are you taking? You're probably going to want to turn the coolant off but this is a matter or trial and error and depends on the grade of the carbide. Generally speaking the chips should come off the part silver or straw colored and turn blue while setting on the bed.

[hercules]

Here is a pic of the cutter. Carbide is a typo, it is HSS. The depth of cut per pass was set at 0.025 for starters. Pat

[One of Many]

I think your setup is inherently weak. I doubt you will be able to achieve a decent chip load with that operation. The blanks could be mounted flat against that spud in the chuck with a center bolt to hold it in place, preferably with the blanks keyed to the spud(just incase you had to recut them for some odd reason and so they do not slip during cutting). The tailstock is pretty useless IMHO. The rotation for the cutter could be set so that the major cutting forces are toward and supported by the spud keeping it as short and rigid as possible. The stub arbor nut tightening direction could be important here if there is no key on that cutter.

Using HSS, 4140 in raw form should cut in the range 35-100SFM.

So, to get a spindle RPM suitable with flood coolant, maybe 50-75SFM, but you could push this up later since you are using flood coolant.

RPM = SFM*12/(p*D)
Something like 60-100RPM spindle speed.

To get a decent feed rate. Conservatively at .001/tooth full depth, early passes could go in at .002/tooth. At full depth, there is a lot of tool pressure in that profile. Can we presume there are 12 teeth on that cutter?

IPM = FPT*N*RPM

Roughly .72-2.4 IPM feed rate and maybe 3 passes to total tooth depth.

I might plan it this way if the setup were rigid enough to handle it. With 2 roughing passes per tooth all the way around. 1st pass at 50% depth and second at 80-90% depth. Final pass on all teeth at full depth and possibly a slower feed rate to improve finish.

Just keep your hand on the feed rate over ride, listen and feel the machine loads.

DC

[hercules]

Thanks a million for the help! You are right about the tail stock, I have removed it after some trial and error seemed to show that it was not adding any rigidity to the set up. Yes the cutter has a dozen teeth and yes it is keyed to the arbor. The gear blanks are a press fit on the stub and then secured tight with a nut (ie the end of the stub is threaded).

I will try your three pass suggestion with the final pass slowed to see if I get a good finish. The set up may not be rigid enough for that deep of a cut per pass but I'll give it a try on a spare blank and see what happens. You are right in that with the very small depth of cut and speed/feed that I was using the spindle load indicator hardly shows any change as the tool begins it's pass.

Thanks again for your help and advice. I appreciate you taking the time to help me out. I want to learn to do this stuff right. Pat