1. Cutting fluid/coolant: for slow operations like drilling, boring, & tapping, use heavy lubricants, like sulfurized oil. Water-based fluids are preferred for high-speed turning, milling and grinding because of the greater cooling effect.
2. Drilling: use steady feed rates-- don't allow the tool to dwell, which causes work hardening at the bottom of the hole, and makes cutting more difficult once it resumes. Set-up should be as rigid as possible, using stub drills and jigs where possible.
Heavy-duty high speed steel drills with a heavy web can be used. Grades T15, M41, M42, & M43 are recommended. Carbide tools are also used. TiN coated tools will have lower friction, hence reducing tool temperature and wear.
To minimize work hardening, use positive rake angles with adequate relief. Cutting pressures are reduced and a positive effective rake maintained if the web is thinned at the chisel point. Increasing the point angle to 135 degrees can be helpful.
Feeds and speeds: For unaged condition, speed should be 3-4 m/min, or 10-12 sfm. Aged condition is 2-3 m/min, or 8-10 sfm. Feeds depend on diameter:
3. Tapping: Drill size should be 50-55% of thread depth. Speeds should be ~ 1.5-3 m/min or 5-10 sfm. Inconel alloys are best tapped using serial taps, which are standard taps modified in diameter so that each successive tap increases the thread diameter proportionately. Tap in the unaged condition if possible. Ample cutting fluid is necessary for either hand or machine tapping; chlorinated waxes being the preferred type.
