Key Points of CNC Milling of Steel

• 1
  What makes CNC milling of steel different from aluminium
• 2
  Tool grade and geometry choices that hold up
• 3
  Speeds, feeds and depth of cut in practice
• 4
  Workholding and heat control for tight tolerances
• 5
  Surface finish, tolerance and what gets measured
• 6
  Steel grade to cutting approach

Aluminium cuts at 3 to 5 times the surface speed of mild steel on the same spindle. That single fact drives everything else: higher cutting forces, faster tool wear and far more heat concentrated at the tip of the cutter. A 12 mm carbide end mill in 6061 might run at 5,000 rpm. In 1018 steel it runs nearer 1,200 rpm, and the feed per tooth drops from roughly 0.10 mm to 0.05 mm.

Hardness is the second variable, and it is not a single number. Low-carbon steels such as 1018 and A36 sit around 120–180 HB and machine cleanly. Medium-carbon 1045 and alloy steels like 4140 and 4340 arrive anywhere from 180 HB to 320 HB depending on heat treatment. Pre-hardened 4140 at 28–32 HRC still cuts well with coated carbide. Above roughly 45 HRC the tool life curve turns sharply.

Thermal expansion matters more than most drawings admit. Steel grows about 11–13 μm per metre per °C. A 300 mm bore machined at 30 °C and measured at 20 °C is not the same hole. For work held to ±0.005 mm, we let the part stabilise before final inspection rather than measuring hot off the machine.

Chip control is the last difference. Steel produces continuous chips that carry heat away from the cut when they break correctly. Stringy chips wrap around the tool, raise the temperature and leave a poor finish. Feed per tooth that is too low is the usual cause, not spindle speed.

For most steel milling we use solid carbide with a TiAlN or AlTiN coating. The coating is what lets the edge survive 800–1,000 °C at the contact zone. Uncoated carbide works in 1018 at low speed but loses its edge quickly in 4140.

Substrate grade matters as much as coating. A tougher grade handles interrupted cuts and hard materials without chipping; a harder grade holds a sharp edge longer in continuous finishing passes. For 17-4PH in the H1150 condition or tool steel near 50 HRC, we move to a harder substrate and accept lower feed rates rather than risk a broken tool in the middle of a finishing operation.

Geometry follows the operation. Roughing uses a 4-flute cutter with a strong core and a small corner radius, often 0.4–0.8 mm, to spread load and resist chipping. Finishing uses more flutes, 5 to 7, so feed per revolution rises without overloading any single edge. Aluminium-style high-helix cutters are the wrong choice in steel because the thin edge cannot take the load.

Corner radius is not cosmetic. A sharp internal corner in a steel pocket concentrates stress in the part and load at the tool tip. Adding R0.5 mm or more reduces both. If the drawing calls for a true sharp corner, that is a sinker EDM job, not a milling one.

Starting points for coated carbide in 1018 at 12 mm diameter: 120–160 m/min surface speed, 0.05–0.08 mm feed per tooth, 1.0–1.5 mm radial depth, up to 1× diameter axial depth on a rigid setup. In 4140 pre-hard, drop surface speed to 80–120 m/min. In 17-4PH H1150, expect 40–60 m/min.

These are starting points, not a recipe. The correct check is chip colour and sound. Silver or light straw chips with a steady note mean the cut is healthy. Blue chips mean the surface speed is too high for the coating. A high-pitched squeal usually means the tool is rubbing rather than cutting, which is a feed problem, not a speed problem.

Radial depth of cut and tool life trade off directly. Going from 10 percent to 30 percent radial engagement can cut cycle time by half, but only if the setup can absorb the side load and the machine has the spindle torque to keep the feed per tooth constant. On our 3-axis machines with 500 × 500 × 450 mm travels, deep radial cuts in 4140 are routine. On thin-walled parts they are not.

Coolant is a real decision. Flood coolant removes heat and flushes chips but can cause thermal shock on carbide during interrupted cuts. High-pressure through-spindle coolant, 30–70 bar, is better for deep pockets and for drilling. In finishing passes on hard steel, some shops run air blast to avoid thermal cycling of the edge.

Steel cutting forces are roughly double those in aluminium for the same removal rate. A vise that holds a part in aluminium will shift under a heavy steel roughing pass. We use a rigid machine vise on a ground bed, plus toe clamps or a fixture plate for parts that need more than one setup.

Thin parts are the hard case. A 3 mm steel plate will deflect under clamping pressure long before the cutter touches it. Vacuum chucks and low-pressure clamping with support underneath keep the part flat. If the finished wall is under 2 mm, we plan the machining sequence so the wall is cut last.

Heat goes into the part, not just the chip. Roughing generates most of it, so we rough, let the part cool, then finish. Skipping that pause shows up as a bow in a long part, often 0.05–0.15 mm over 300 mm, which no amount of finishing will remove.

Roughing before finishing also gives the material a chance to move. Residual stress in rolled or forged steel is released as material is removed. For a part with a tight flatness call, we take an even amount off both sides rather than machining one face to size in a single pass.

As-machined steel typically lands at Ra 1.6–3.2 μm. Careful finishing with a sharp tool and a light depth of cut reaches Ra 0.8–1.6 μm. Below Ra 0.2 μm requires grinding or polishing, not milling, and should be specified as a separate operation.

Tolerance is a function of machine, setup and material stability, not just the control. Our standard working tolerance is ±0.005 mm. That figure assumes a rigid setup, stable part geometry and a controlled temperature. It is not achievable on a 3 mm wall with no support, and quoting it would be dishonest.

Inspection is where steel parts often fail late. We check raw material certificates before cutting, monitor critical dimensions in process, and inspect 100 percent before shipment. Reports are available on request. For bores and hole positions, CMM data beats calipers because it shows form error, not just size.

Threads deserve their own note. Tapping 4140 by hand at 30 HRC is slow and breaks taps. Thread milling gives better thread form, works in blind holes and lets one tool cover several thread sizes. For small tapped holes in hard steel, we often thread mill rather than tap.