Machining strategies and parameters are very much dependent on:
- Available CAM Software strategies
- Machine and fixture rigidity,
- Spindle torque
- Tool shank diameter
CoCr is extremely tough, if you expect to get any sort of tool life your smallest DoC (Depth of Cut) should be at least .1mm.
Generally speaking, ideally you want:
- Coated carbide tooling (TiSiN or TiAlN)
- Very rigid fixturting
- Tooling as short as possible
- Flood coolant
Not sure what tooling you have (6.0mm shank is best) but here are some guidelines/starting points (if abiding by above conditions):
Roughing/Semi-finishing
3mm ball nose DOC 0.18mm / step over 0.75mm @ 20,000 RPM/ 2,000 mm/m
2mm Ball nose DOC 0.1mm / step over 0.5mm @ 22,0000 RPM / 2,000 mm/m
Finishing
1.0 mm Ball Nose DOC 0mm / Step over 0.05mm @ 32,000 RPM / 1300 mm/m
Above may be too fast or agressive for your set-up (machine & fixture rigidity, tool shank size, tool coating, etc.) so slow it down (spindle, feedbrate). You will know if you need to.
Also,
- Make sure you are getting the chips/slurry out of from the machining area
- Always be climb cutting
- Machining from bottom, up is typically preferred
- Avoid plunging into material, arcing, ramping, helixing into and out of a cut instead.
- Use strategies that produces smooth tool path that produces uninterrupted paths that avoid sudden changes in direction (reference attached image.)
- Avoid intermittent cutting by running enough semi-finishing and/or semi-roughing operations with appropriate DoC, Step-over and stock allowance to assure a consistent amount of stock.is on the part (consistent stock thickness/scallop heights). Reference attached image.
Not sure if this is what you are looking for but maybe it will help....