Reliable titanium milling depends on a rigid climb-milling setup, strong cutter teeth, ample chip space, appropriate rake and clearance angles, and conservative engagement. This guide summarizes geometry and cutting data for face mills, end mills, ball mills, fast-feed cutters, high-speed milling, and plunge milling.
Climb milling is generally preferred for titanium because the chip is thin as each tooth exits, reducing adhesion at the cutting edge. In conventional milling, adhered chips can break when the tooth re-enters and cause edge flaking. Because titanium has a low elastic modulus, climb milling also demands a rigid machine, tool, and setup. Short tool-chip contact requires strong teeth and ample chip space; chip packing can cause severe wear.
| Cutter | Rake/axial-radial rake | Clearance | Other geometry |
|---|---|---|---|
| Indexable carbide face mill | Axial 5–8°; radial −13 to −17° | Application dependent | Entering angle 12–60° for roughing |
| Inserted-carbide end mill | Rake 0° | 12° primary; 5–8° secondary | 30° helix; 0.5–1.0 mm corner radius |
| HSS side-and-face mill | Rake 5–10° | 15° | Entering angle 30–50° roughing or 75–90° finishing; 0.5–1.5 mm radius |
| Solid-carbide end mill | Rake 9–13° | 12–16° | 40° helix |
| Solid-carbide ball mill | Rake 3° | 10° primary; 25° secondary | 40° helix |
Use a smaller clearance angle when climb milling hard scale; use a larger value on small-diameter end mills.
| Operation | Material/strength | Speed | Feed per tooth | Depth/width guidance |
|---|---|---|---|---|
| Carbide face milling, roughing | Rm ≤1,000 MPa | 24–37 m/min | 0.10–0.15 mm | ap 1.5–5 mm; ae ≤0.6D |
| Carbide face milling, finishing | Rm ≤1,000 MPa | 30–45 m/min | 0.04–0.08 mm | ap 0.2–0.5 mm |
| Carbide face milling, Rm >1,000 MPa | Rough/finish | 20–24 / 24–30 m/min | 0.08–0.12 / 0.04–0.06 mm | ap 1.5–5 / 0.2–0.5 mm |
| HSS end milling | Rm ≤1,000 MPa | 12–19 m/min | 0.08–0.10 rough; 0.04–0.08 finish | ap 0.5D–2D; ae 1.5–3 mm |
| Carbide ball milling, finishing | Rm >1,000 MPa | 20–60 m/min | 0.15–0.20 mm | ap 0.1–0.3 mm; ae 0.3–0.5 mm |
For 50–100 mm PVD-coated fast-feed cutters, representative speeds are 30–60 m/min, depths 0.1–1.0 mm, and feeds 0.1–1.5 mm/tooth depending on insert geometry. High-speed shoulder mills use 40–180 m/min, 0.02–0.25 mm/tooth, and 0.1–0.2 mm depth; solid end mills use 40–400 m/min, 0.01–0.25 mm/tooth, and 0.05–0.2 mm depth; ball mills use 60–160 m/min, 0.02–0.10 mm/tooth, and 0.02–0.10 mm depth.
For plunge milling with 6–20 mm flat-bottom carbide tools, both axial depth and stepover are about one-quarter of diameter. Representative spindle speed rises from 450 to 700 r/min and feed from 60 to 80 mm/min across that diameter range. Reduce parameters for the first row and first plunge of each row as conditions require.
Share your drawing, material, tolerance target, or application question. Our engineering team can help review the machining route and suggest a practical next step.
Machining Technology
Titanium turning requires controlled temperature, sharp tool geometry, alloy-specific speed correction, and high-flow cooling. This guide preserves recommended HSS, carbide, and boring-tool...
Read ArticleMachining Technology
This article explains key programming considerations for turn-mill CNC machining, focusing on machining plane setup, cutting parameter selection, and chip evacuation. It...
Read ArticleMachining Technology
Titanium alloys combine high specific strength, corrosion resistance, and hot strength, but low thermal conductivity, chemical reactivity, springback, and concentrated contact pressure...
Read ArticleMachining Technology
CNC machining is a computer-controlled subtractive manufacturing process that removes material from blocks or sheet stock to create finished parts. This article...
Read Article
