[vebers]

Okay I have to cut a 17 X 10.5 slot 1" deep through 2 S-7 56-58 RC blocks 21.75 X 10.5 X 3. I am using an antique Cat 50 OKK MCV 500. Max spindle RPM 3000. The details require alteration after they were heat treated, and annealing them and reheat treating them will take more time than the company wants to be down. Any Ideas? I have never done this before and I am willing to buy good tooling. Speeds? Feeds? Depth of cut? step over? The cut will be interrupted due to bolt holes located in the slot area. Any information would helpful. I am not as interested in the High Speed aspect as not having to change inserts 500 times per block.

Thanks

[HuFlungDung]

That sounds like a lot of material removal, if I am picturing this correctly. I would check with Greenleaf ceramics:
http://www.greenleafglobalsupport.co...es_10001_10001

I have not used any of their products in a milling application, but have been impressed by some of their whisker reinforced ceramics, which are tough enough to endure some rough machining situations in lathe work. I do not know what grade would be suitable for working steels, so I'd suggest you contact their technical engineers for some advice.

[DareBee]

I would use AlTiN coated carbide.
I have found UltraTool works really well. If you want to PAY for the best get Mitsubishi cutters.

Sorry scratch that - 17 X 10.5? that is a crap-load of material.
I would use a short length, 1"dia, HiPos+ cutter from Ingersoll with 2030grade and .032CRad inserts.
You will have to play with F&S but, I would start at 1500RPM, 9IPM and .1DOC.

It may also be advisable to contact a local "tooling" salesman direct from a manufacturer.
I have had SandVik in before to recommend tools and they guarantee that what they recommend will work or they will take it back.

[HuFlungDung]

I'd be looking for negative rake tooling to get some edge strength to rough with.

[underthetire]

I would call your fav. tooling house and ask them to send a rep out and see if you could demo a cutter. My guy gives me stuff to try all the time.

[vebers]

Thanks guys that gives me something to chew on.

Vince

[DareBee]

I'd be looking for negative rake tooling to get some edge strength to rough with.

I agree wit the theory of using neg rake for stronger edge.
But have always been advised to (and do) use positive rake for hard milling.

58Rc is like butter on the hard milling scale.
I use all TiAln coated cutters in my VMC for general work and hard S7 cuts easy with them. 58Rc is the high end of typical hardness for S7 as well.

[mbi]

I am assuming the slot is blind? I would use a high feed cutter. I like the Mitsubishi 2.0 dia. high feed shell mill. That is a bit harder then I am use to however it is possible. I usually machine 45-48 Rockwell. I will run the cutter 860 rpms, 160 ipm .045 doc and a 1.4 step over. The Mitsubishi rep should be able to help you. He helped me alot. We machine much larger pockets then that daily.

[vebers]

If you mean blind like it is a pocket then no it will break out of the block in two directions. Basically it is a 1" deep slot through the block 17" wide. I like the recommendation but I couldn't get 160 IPM if my life depended on it. Maybe 30 IPM and it might have to slow down and think a little in the corners. lol

[tobyaxis]

I'll second Greenleaf. I have had some recent experience with Turning (though your application is Milling) with the WG300 CNMA Inserts in 60Rc 416SS. Cut like a HOT KNIFE Through BUTTER!!!

Surface Finishes were at least a 16.

DOC was light around .025
SFM was 150 to 200
IPR was .002

Machine was a new HAAS SL20.

I would say the Ingersol or Greenleaf would be your best bet for Hard Milling.

http://www.greenleafcorporation.com/

http://www.ingersollcuttingtools.com/en/index.htm

[tooldude328]

I don't see any posts on how you would program for that slot? I would cut it at full depth with a trochoidal tool path with about a .015 step over with a large diameter end mill. That should be able to cut it in one pass. I generally use just air blast rather than a flood coolant. You want to get the heat out with the chips. I cut S7 all the time with TIALN coated cutters with no problem. All though as stated before Rc56-58 is on the high end for S7. Usually 54 -56 for me.

[5axisguy]

I agree with tooldude, high feed type tools on hard S-7 has not worked very well for me, much better off with a full depth trochoidal path, if you have the cam to make the program for it.

[mactec54]

tobyaxis I think you have something wrong with your hardness tester if you were getting 60RC out of 416ss, it normally won't get to much over 40RC & you dont need to much in the way of special inserts to machine it , machines very easy heat treated or not.

vebers you say you have to mill through the plates, if you do, then get it done on a wire EDM machine, if it's not right through rough mill & finish with a Ram EDM you will most likly put to much stress in it by milling that much material out of them