Need Help!- Question about hard milling

[AMCTony]

I have 16 holes that need to be milled in A2 that has been hardened to 57-59HRc. Each hole is a precision countersink that is 0.375" diameter +0.0000-0.0005 and is 0.402" deep. There will be a 0.250 thru hole pre drilled before hardening. I am looking for recomendations on endmills to do this. I am thinking of using a 1/4" 3flute TiAlN carbide endmill with a small corner radius to rough with a helical bore tool path to depth leaving 0.005 for finish. Then using a 1/4" 5 flute TiAlN carbide endmill to finish the hole to size. I am assuming that a high feed rate, high RPM and very low depth of cut will be the way to go. Any help on this would be appreciated.

Thanks,

Tony

[Geof]

My hard material experience is limited but what you describe sounds suitable. I suggest rigging up a very powerful air blast right close to the tool.

[littlerob]

I dont know what you consider to be high feeds and speeds but in that hard a material (personally) I would slow the spindle down, maybe 150 SFM. But Geof is certainly more experienced than I am, By a long shot. Just me, Robert

[Geof]

Originally Posted by littlerob I dont know what you consider to be high feeds and speeds but in that hard a material (personally) I would slow the spindle down, maybe 150 SFM. But Geof is certainly more experienced than I am, By a long shot. Just me, Robert

Maybe not more experienced in this particular area. I have machined hard stuff but only a little and only for in-house stuff.

Probably someone with more experience will come on later; Hu where are you?

[JIMMY]

You have the right idea, your thinking is the right approach. When I cut something just like that I would find out how much material is left on the floor before you start. If there is .01 inch on the floor I would helical bore staying .012 away from the floor. I would then do another helical bore from .014 from depth with a lighter helical staying away from the wall and leaving .002 to .005 on the floor. I would come back in with your finish cutter(which I use osg's 6 fluted cutters) and helical bore the walls staying away from the bottom .001 from where your roughing cutter left. Then I would finish the floor with a program that would start from center and go out staying away from the wall about .001. The key thing about hard milling is to think about the cutting edge of the cutters.

I run my cutters at 800 sfm with .001 chipload, but that is because I have the machines to handle that. You have to make a judgment on what you machine can handle.

[littlerob]

No, seriously Hu, where are you? I am in Utah, what use can I be. But I have had pretty serious chatter issues with a particular part,(Welded components then edges cut out on a burn table, pretty hard maybe 65 HRC), and have had better luck with a composite endmill at lower SFM. (YG-1 TANK POWER) you pay for it, but for my application it is working well. Hope that helps at all.

[dertsap]

you'd be better off using a 4 flute stubby endmill , i'd try dialing and plunging a 3/8 endmill far sooner than than attempting to interpolate with a 1/4" em , carbides are generally a few tenths undersized , if you used something like a hanita varimill which has 45 deg corners rather than sharp corners , the tool will most likely self align itself and run fairly smoothly through the hole
thats not soft material and .0005 isnt much room to play in as far as interpolating , you will need to dial the tool in dead nuts , meaning you would need to dial in the dia and the length to be sure your endmill isnt naturally going to taper the hole adding to the tool deflection that you are most likely going to face ,

if you are going to interpolate the hole get it right the first time , one thing to keep in mind is the concerns to spring passes , DonT trusted them , lets say the hole is undersized by .0006 , should be simple to dcomp it , lets say you dcomp it and run it , no change , d comp it again , still nothing ,d comp again , .003 oversize , it easily can happen like that , not always but often enough , sometimes it is better to polish the one hole later and make the appropriate adjustment for the next hole


run it slowww speed and feed , too high of a feed you could be dealing with either fracturing the tool or fractures in the part

[Andre' B]

Since there is a 1/4 starting hole I would be tempted to drop a 3/16 4FL down a few thou short of full depth and spiral out, switch to a finish endmill or maybe run a semi finish and a finish tool.
Figure I paid for all that cutting edge on the sides may as well use it.
If the heat treat was not under inert gas may want to clean out the scale with a die grinder first.

Would likely start at around 350SFM, spiral out per time around of about 3 or 4 percent of the end mill diameter, and a feed per cutting edge of around 0.25 to 0.3 percent of end mill diameter.

I have side cut 60Rc S7 and A2 with a 3/8 end mill at 1.25 DOC, 0.010" step over, 350SFM, and 0.0015" feed per flute. Have had good luck with flood coolant as long as the coolant is clean, well filtered and lots of it, otherwise dry with an air blast.


Or if the part will go in a good solid lathe or you have a horizontal mill you may be surprised how well just plunging a 23/64 end mill will work, use a G73 canned cycle or macro to keep the chips from getting to long, roughly 0.015" pecks. Then to a semi finish and finish pass with CBN inserts and good solid boring heads if on a mill. I don't see if you said how flat the bottom needs to be finished to.

The TIALN coated carbide end mills available today are awesome compared to not so long ago. And cheap, $13.00 for a 3/8 1'DOC Sq. end 4FL, not saying where.

[AMCTony]

Thanks for the help all. I have a pretty good idea about how I am going to attack this job.

[HuFlungDung]

I'm not a real experienced hard miller, but I think what Jimmy outlined is the way I'd try it. The end of the flutes on the endmill tend to have the stronger edge because of the way the relatively slow helix meets the end. This creates closer to a 75 or 80 degree included angle supporting the cutting end edges. The side flutes, by comparison, are weak, with perhaps 30 to 40 degree included angle supporting the cutting edge. So a helical path down in a boring type fashion would be my choice, with the tip radius doing most of the cleanup of the wall. I would not be expecting the side flutes to do much (for long) in a spiralling outward routine, except for the light bottom facing cut Jimmy described.

If the holes turn out tapered (almost expected), I might try taking a tool and relieving the side flutes (grind clearance) except for the last 1/16" near the tip. Then, attempt a helical up routine beginning at the bottom. Yes, you would have to spiral outwards to begin, but hopefully by this time, there would only be a matter of .001 to .002 to remove. Starting with the sharp tool at the bottom of the hole may be your best chance to cut the taper out.