Keyseat Cutters

[M_CODE1]

You guys have always been helpful in the past so I thought I'd come here for some advice on a part we are having issues with. We have a part that we are having trouble putting the woodruff key seats in. The part is 4140 and heat treated to 42-47Rc. We decided to heat treat the stock first then have 2 lathe operations, then a mill operation. We did not think we would be able to hold the keyseat tolerance and position if we did them soft and had a grind operation after heat treat. We are using a Fullerton .875" X .1875" Keyseat Cutter (#607 ). We made a fixture that locates the part on the 1.7722 diameter on both end and is clamped cross the top. The Fullerton book recommends 60-140 SFM for hardened steel for speed of 257-600, then a feed of around .004 IPR, so 1.0 - 2.4 IMP. We have has no luck in that range. The cutters have broke at different times, some at the start of cut and others at the bottom. I tried to program it and roll the cutter into the part to have a thick to thin chip, but that did not seem to help either.

 

Any advice on a different too to use? Or any other way to better cut this part? Does anyone have an experience cutting key seats in 4140 at 42-47Rc?

 

A few of the things we have tried

-Part was in V block vice jaws, made fixture to make it more rigid.

-Made sure tool was as short as possible

-Tried rolling cutter in

-With and without coolant (part was cool after a couple cuts, but then cutter broke)

-Tried to peel mill .005" step over with a 3/4" keyseat tool to rough out (S7500, F30), Broke cutter after 3 keyseats.

 

Thanks

 

Mike

[JOHNAKA]

i would rough it out an leave .01 and heat treated and comes again and finish it. it is too hard to mill at the hardness. well for now u need some special tools

[RaiderX]

let me throw this in since you seam to be committed in your project at this point.

try a smaller diameter and generate your .875 dia. (.4375 rad) cuts. this will be less tool rad. contact thus less heat. Carbide would be good too if you can get something ground stagger tooth usually doesnt hurt either but you are looking at pretty small dia cutter for that so am not sure if that is practical.

 

Doug

[crazy^millman]

Got a 4th axis? Do what you can with a ball endmill at vertical rotate 90 deg and then take out the left over with the key seat cutter. If not then just do that in 2 operations. Carbide would be my only choice would not attempt with HSS or Cobalt. Harvey makes some very nice carbide head ones.

[Machineguy]

M code,

 

4140 is tough material. In the hardened state its hard all the way thru. That part won't move much in heat treat for its size.

As per John, I would rough turn, leaving .005-.007 per side for grind. That depends how good your heat treater is.

Rough in the slots, leave .02 for later.

heat treat

Re dress the 2 centers.

Finish grind, or hard turn.

Finish the slots with a carbide keyseat cutter. M42 tool steel is not going to last long at 47RC.

I would run coolant on the finish.

 

Machineguy

[M_CODE1]

Thanks for some of the ideas. The cuter that we are using is solid carbide straight tooth.

[Newbeeee™]

I would do as Doug (RaiderX) says - smaller tool and Get the revs up a little and generate. Also definately go for thinner tool - say .080" max thickness.

Do PH Horn have anything near - they do replaceable carbide ends which locate/screw onto a carbide shank. Work like a charm in ally

In all seriousness you're pushing the limits I would have thought. Safest way is do what the others say and machine then heat treat, but you may loose your shirt depending how it's been quoted...

[reidmachine]

7500 might be a little too hot for the 3/4tool (1472 sfm)

I threw this together, I have used this method in 4340 at 45Rc with success.

350-400 sfm is about all your going to get away with, that is, with an altin or equivalent coating.

TRY THIS.MCX-7

[reidmachine]

I didn't mean to kill this thread!

 

To the OP, What did you end up getting the part done with?

Tool?

Toolpath?