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 Geometryand 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-3grade |
Negative rake square or trigon insert, 45° SCEA1, 1/16 in nose radius Tool holder: 5° negative back rake, 5° negative side rake |
30-50 | 0.004-0.008per revolution | 0.15 |
Dry2, oil3, or water-based4,5 |
| Normal roughing; Turning or Facing | As above | As above |
90 (80 for cobalt alloys)6 |
0.010per 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 rake0° 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) | 0.005-0.008per 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. 0.0031 in dia. 0.004(cobalt alloys: ¼ in dia. 0.001 ½ in dia. 0.0015 ¾ in dia. 0.0021 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 | Carbide: C-2 grade (marginal performance) | Use positive axial and radial rake, 45° corner angle, 10° relief angle | - | 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 for¼ 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. 0.0051 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. 0.0032 in dia. 0.008 (same for cobalt alloys) | - | Oil or water-based |
| Carbide: C-2 or C-3grade | 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 orbreakage 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).