Astrolloy?

[littlerob]

Hey anybody ever milled "Astrolloy"? When I saw the print I thought typo they meant Hastelloy. Wrong. I googled it but couldn't find anything on machinability. There will be two turn op's that will be on the Okuma so I'm not worried about that ,, but there will be one mill operation on a 2000 VF-3 with 30 horse, is this too much for this machine? There are a couple of tight ones but to redeem myself from my previous remark I like the Haas. Is it going to be too hard on the machine?

Robert




(edit) this will be ongoing for about a year

[shawnc74361]

Milling

Total cutting rate equals the feed rate times the number of inserts in cutter times rpm. Uniform distribution of feed rate per insert requires the use of precision inserts. This precision is necessary to assure that each edge is working beyond the zone work hardened by the preceding insert. For optimum metal removal in interrupted machining (i.e. milling), best results are also accomplished using negative rake, mechanically clamped, tungsten carbide inserts. The machining practice depends on the hardness of the steel and the rigidity of the part and the machine, among other variables. The generally recommended feed rate is 0.003" per tooth. Fully annealed plate, (240-300 BHN) can be cut with a cobalt end mill at 15 sfm or with a carbide end mill at 150 sfm, depending on the rigidity of the machine and the part. Fully hardened material requires carbide inserts and 50 sfm. Flame cut edges may have a shallow layer over 500 BHN, requiring suitable reduction in feed rate.

For cutting keyways in material less than 350 BHN hardness, use a two fluted high-speed end mill at a speed of 12 sfm. Use a good coolant to keep the cutter and steel cool. The great majority of fatigue failures in shafting made from any steel can be traced back to sharp corners and notches like those found at the base of a square cornered keyway. To greatly increase your shafting life, put a small radius at the corners of the keyway and put a corresponding radius on the matching corners of the key. Suggested minimum radius is 1/16".


Drilling

Apply positive power feed to produce continuous chip and avoid work hardening.
Use a full flow of heavy duty coolant to dissipate heat and lubricate cutting edges.
Use high speed steel drills modified with cobalt. AWT has had good experience with Cleveland Twist Drill Premium Steel Cobalt (List No. 2440 for taper shank bits and List No. 2013 for chuck mounted bits). Drill bits should be ground so that the included point angle is 140-150 degree, taking care to ensure that the point angle has exact centering. The flute lip should be ground to a 5 degree positive rake with an approximate land width of 1/32 inch. The web should be thinned to approximately 3/32 inch to reduce drill pressure and to minimize work hardening at the drill center.
For material 444 BHN and harder, cutting speed should be in the range of 6-8 surface feet per minute with a feed rate of 0.004" per revolution. For material 320 to 370 BHN, used 12 to 15 sfm with a feed rate of 0.004" per revolution.
Drill rigidity is important to successful drilling. Drill rigidity can be enhanced by using secure set-up and shortened drill bits

[littlerob]

Thanks for the response. The Haas did fine, with chip load at about .005 per tooth and 150 sfm. Funny thing, I was worried about the Haas, and the turn operations turned out to be the hardest, what ended up working was about 200 sfm, and roughing feeds of .03 tpr, .2 doc with 433 cnmg. It is hard on the tool but this crap can not get hard in front of the cutter, obviously.

Robert

[Ben Olson]

I have messed around a little bit with EN30b (basically astroloy without the trade name ) and yeah , don't let it work harden , and the stringy chips will cut you really bad ( found this out the hard way )

[littlerob]

and the stringy chips will cut you really bad

Me too 14 stitches across three fingers, what commitment I have.