Milling D2 Tool Steel

I am a fairly new CNC machinist running a Haas VF-3 mill. I have to machine D2 tool steel and am having a hard time finding a good speed and feed rate. Im using 3/4" Accupro TiCN coated, solid carbide, fine tooth roughing end mills. They are about $200 a piece and I have already destroyed several of them. I have tried to take take .125 and .250 deep cuts, the full width of the end mill at 1200 rpm 10in/min, 1000rpm 10in/min, and 750rpm 6in/min. So far I have had the best luck with the 750 and 6, .125 deep but it still isnt right. Anyone have any speeds and feeds that would work good? Thank you

i think your problem is not the spindle speed, its the feed and depth..
try this option since i am doing tool steel as well on my current job..and it works good, i dont have the same cutter as you, but i think should be close enuf..
try:
2mil depth of cut (inch 0.078 i think)
spindle speed 1273 rpm
feed 4 to max 5 inches per min...

and dont use coolant what so ever..not even a drop or mist..
you can blast dry air would be heaps better...

hope this helps

I think peace and calm is close, your depth of cut was way to deep, I've run a face mill, with carbide inserts machining tool steel, It worked it was hard on the inserts, but did the job. So more passes less depth.. Good luck

yes,depth of cut is the name of the game.i work with soft tool steele and hard cut it.carbide and air is the way to go,hard or soft..030 d.o.c. feed 50-60 in.per min. on soft.on a 50 taper viper.

This thread is old but man what terrible advice, I machine d2 tool steel all day long everyday, usually I use indexibles or high feed indexible end mills but when I run roughers I can take a 5/8" rougher 5/8" deep in an end mill holder at 12ipm and I believe 1528 rpm, all day long, that's unhardened d2, for hard d2 I wouldnt recommend a rougher at all, standard 4 flute will work. Coated and flood coolant, light passes, I hard mill at 75-100 sfm , the info above everybody recommends like .030 or .040 depth of cut, why would you use a rougher for a .030 depth of cut???? I can run a high feed end mill at 200ipm .040 depth of cut and .047 chip load on a vf3.....

up your rpm to 18,000 for hardened tool steel.

For roughing D2 you can't go wrong with negative rake ceramics as long as it's not an interrupted cut. No coolant or you'll get thermal shock that will shatter the inserts very rapidly~

I ran my 2" facemill at 2,200 rpm, 50-100IPM at around .030"-.045" DOC. I've run it as deep as .250 deep at around a 10-20IPM but if the inserts go out you wreck the hole cutter instead of $20 in ceramic discs.

I've literally machined several tons of D2 at 61-63 Rockwell with this setup and the only problem I've ever had was catching my VMC on fire twice~

Ceramics like smooth interrupted cuts but even when I've had to machine down recycling blades that had interrupted cuts along the perimeters, I'd just watch for the chips to start turning brighter orange and then rotate the inserts.

I'd get on average 20 cutting edges per insert x4 inserts. I would average roughly 24 cubic inches of material removal per set of cutting edges. Inserts were $10 a piece, so for $40 I could remove around 480 cubic inches of material. I had a little over $1,500 into my CAT40 holder, retention stud, Ingersol Rand facemill and inserts.

The finish with new inserts is good enough to see your reflection pretty decent.

This cutter works so good in D2 that I was able to charge over 4 times my regular hourly rate.

Be careful though, it will burn the wipers off of your way covers and catch anything around it on fire!!!