800.354.0806
765.456.6012

Machining

Recommended Tools and Machining Parameters Applicable to:
Corrosion-resistant Alloys
High-temperature Alloys

Be aware that the cobalt-base alloys in these categories (25 and 188) can require different feeds and speeds (as noted in the table) than the nickel- and iron-based alloys.

Operations Tool Types Tool Geometry
and Set-Up 		Speed Feed Depth of Cut Lubricant
- - - surface ft./min* in** in** -
Roughing with  severe interruptions;
Turning or Facing 		Carbide:
C-2 or C-3
grade 		Negative rake square or trigon insert,  45° SCEA 1, 1/16 in nose radius
Tool holder:
5° negative back rake,
5° negative side rake 		30-50 0.004-0.008
per revolution 		0.15 Dry2, oil3,
or water-based4,5
Normal roughing;
Turning or Facing 		As above As above

 

 90
(80 for cobalt alloys)6 		0.010
per revolution 		<0.15 Dry, oil,
or water-based
Finishing;
Turning or Facing 		As above

 

 Positive rake square or trigon insert,
if possible,
45° SCEA1, 1/32 in nose radius
Tool holder:
5° positive back rake,
5° positive side rake 		95-110
(90 for cobalt alloys) 		0.005-0.007
per revolution 		0.04 Dry
or water-based
Rough Boring As Above If insert-type boring bar,
use standard positive rake tools  with largest possible SCEA  and 1/16 in nose radius  
If brazed tool bar,
grind 0° back rake, 10° positive
side rake, 1/32 in nose radius
and largest possible SCEA 		70
(60 for cobalt alloys) 		0.005-0.008
per revolution 		0.125 Dry, oil,
or water-based
Finish Boring As Above Use standard positive rake
tools on insert-type bars
Grind brazed bars as for finish
turning, except back rake
may be best at 0° 		95-110
(90 for cobalt alloys) 		0.002-0.004
per revolution 		0.04 Water-based
High Speed Steel:
M-2, M-7, or M-40  series7 		Radial and axial rake
0° to 10° positive,
45° corner angle,
10° relief angle 		20-30
(20-25 for cobalt
alloys) 		0.003-0.005
per tooth 		- Oil or
water-based
Carbide:
C-2 grade
(marginal
performance) 		Use positive axial and radial
rake, 45° corner angle,
10° relief angle 		50-60
(35-40 for cobalt
alloys) 		0.005-0.008
per tooth
(0.005 per tooth
for cobalt alloys) 		- Oil or
water-based
End Milling High Speed Steel:
M-40 series
or T-15 		If possible, use short mills
with four or more flutes for rigidity 		20-25
(15-20 for cobalt
alloys) 		Feed per tooth:
¼ in dia. 0.002
½ in dia. 0.002
¾ in dia. 0.003
1 in dia. 0.004
(cobalt alloys:
¼ in dia. 0.001
½ in dia. 0.0015
¾ in dia. 0.002
1 in dia. 0.003) 		- Oil or
water-based
Carbide:
C-2 grade
  		Use sharp tools with 4 or more flutes and variable lead, if possible 50-60
(40-50 for cobalt
alloys) 		As above - Oil or
water-based
Drilling High Speed Steel:
M-33, M-40 series, or T-15 		Use short, heavy-web drills with 135° crank shaft point;
thinning of web at point may
reduce thrust and aid chip control 		10-15
(7-10 for cobalt
alloys)
Maximum of 200 rpm for
¼ in dia. drills
or smaller 		Feed per rev.:
⅛ in dia. 0.001
¼ in dia. 0.002
½ in dia. 0.003
¾ in dia. 0.005
1 in dia. 0.007
(same for
cobalt alloys)   		- Oil or
water-based Use coolant
feed drills
if possible
Carbide:
C-2 grade 		 Not recommended, but
tipped drills may be
successful on rigid set-ups if depth is not great.
The web must be thinned to
reduce thrust; use 135°
included angle on point Gun drill can be used 		50
(40 for cobalt
alloys) 		As above - Oil or
water-based Coolant-fed, carbide-tipped  drills may be
economical in some set-ups  
Reaming High Speed Steel:
M-33, M-40 series, or T-15 		Use 45° corner angle,
narrow primary land,
and 10° relief angle 		10-15
(8 for cobalt alloys) 		Feed per rev.:
½ in dia. 0.003
2 in dia. 0.008
(same for
cobalt alloys)   		- Oil or
water-based
Carbide: C-2 or C-3
grade   		Tipped reamers recommended;
solid reamers require very
good set-up
Tool geometry same as above 		40
(20 for cobalt
alloys) 		As above - Oil or
water-based
Tapping High Speed Steel:
M-1, M-7,
or M-10 		Use two flute, spiral point,
plug tap 0° to 10° hook angles
Nitrided surface may be helpful
by increasing wear resistance,
but may result in chipping or
breakage
Tap drill for 60-65% thread if
possible, to increase tool life 		7
(same for cobalt alloys) 		- - Use best
possible tapping
compound;
sulfo-chlorinated
oil-base
preferred
Carbide:
not
recommended 		- - - - -
Electrical
Discharge
Machining 		HAYNES® and HASTELLOY® alloys can be readily cut using any conventional
Electrical discharge machining (EDM) system, or by wire EDM

General note: Use high pressure coolant systems and through the tool coolant, when possible.

*To convert to surface m/min, multiply by 0.305
**To convert from in to mm, multiply by 25.4

1SCEA = side cutting edge angle, or lead angle of the tool
2At any point where dry cutting is recommended, an air jet directed at the tool may provide a substantial increase in tool life
3Oil coolants should be premium quality, sulfo-chlorinated oils, with extreme pressure additives; a viscosity of 50 to 125 SSU at 100°F (38°C) is standard
4Water-based coolants should consist of a 15:1 mixture of water and either a premium quality, sulfo-chlorinated, water-soluble oil or a chemical emulsion, with extreme pressure additives
5Water-based coolants may cause chipping or rapid failure of carbide tools in interrupted cuts
6Depending upon the rigidity of the set-up
7M-40 series high speed steels include M-41 through M-46 at time of writing; others may be added and should be equally suitable

Applicable to:
Wear & Corrosion-resistant Alloy

ULTIMET® alloy can be successfully turned, drilled, and milled if appropriate tooling and parameters are employed. However, the alloy possesses high strength and work hardens rapidly. Machining guidelines specific to ULTIMET® alloy are as follows:

Turning (ULTIMET® alloy)

    Carbide (not high speed steel) tools are recommended.

    Surface speed: 60-70 surface ft./min (0.30-0.35 m/s).

    Feed rate: 0.005-0.010 in (0.13-0.25 mm).

    Depth of cut for roughing: 0.05-0.10 in (1.3-2.5 mm).

    Depth of cut for finishing: 0.010-0.015 in (0.25-0.38 mm).

Drilling (ULTIMET® alloy)

    Carbide tipped or high speed steel drills are recommended.

    Surface speed: 30-35 surface ft./min (0.15-0.18 m/s) for carbide tipped drills; 8-10 surface ft/min (0.04-0.05 m/s) for high speed steel drills.

    Feed rate: 0.004 in (0.1 mm) per revolution for 0.25 in (6.4 mm) diameter and greater.

    135° included angle on point.

Milling (ULTIMET® alloy)

    Carbide (not high speed steel) end mills are recommended.

    Surface speed: 25-30 surface ft/min (0.13-0.15 m/s).

    Feed per tooth: 0.002 in (0.05 mm) for cutter diameters below 0.75 in (19 mm); 0.003 in (0.08 mm) for cutter diameters above 0.75 in (19 mm). 

Print Page
Top