Milling — basic modes
How to use the milling data calculator
The calculator operates in two modes. In the “Recommendation” mode, select the cutter diameter, number of teeth, ISO material and tool type - the calculator will offer starting Vc and fz through the preset (LOW / MID / HIGH). In Calculator mode, enter RPM directly. Specify ae (width) and ap (depth) - get RPM, table feed Vf, cutting speed Vc, MRR and chip thickness hex. When ae is low, chip thinning compensation is automatically activated. Optionally specify the machine limits - the calculator will warn you if it is exceeded.
Why Starting Modes Are Not a Guessing Game
Milling conditions are determined by three parameters: cutting speed Vc (depending on material and tool), feed per tooth fz (depending on diameter and geometry) and depth/width of cut ae × ap. Everything else is derivative: RPM is calculated from Vc and diameter, table feed Vf is calculated from RPM, number of teeth and fz.
Tool manufacturers provide Vc and fz ranges for each material + cutter type combination. The calculator contains these ranges and offers three starting points: conservative (LOW), moderate (MID) and aggressive (HIGH). These are not final values - they are a starting point that needs to be adjusted based on the results on the machine.
What influences the choice of modes
Workpiece material (ISO).Determines the Vc range. Aluminum (N) allows 250-500 m/min, steel (P) - 120-220, stainless steel (M) - 70-140, heat-resistant (S) - only 40-90. Going above the range = overheating and wear. Down = built-up (BUE) and poor surface.
The diameter of the cutter and the number of teeth. RPM is inversely proportional to the diameter: a cutter Ø 6 mm at Vc = 150 m/min = 7960 RPM, and Ø 20 mm at the same Vc = 2390 RPM. The number of teeth determines the table feed: Vf = RPM × Z × fz. More teeth = higher Vf for the same fz.
Tool type: Solid carbide cutters allow a slightly lower Vc, but operate at a higher fz with small diameters. Cases with plates (indexable) - higher than Vc, but fz depends on the geometry of the plate.
Width and depth of cut (ae, ap). Determine load and MRR. At low ae (< 50% D), the chip thinning effect is activated: the actual thickness hex drops below fz. The calculator automatically compensates for this by increasing fz to maintain the desired hex. Without compensation, the tool rubs instead of cutting.
Machine Limits: Older machines are often limited by RPM (e.g. 6000 rpm) or table feed Vf (2000–3000 mm/min). The calculator warns if the calculated values exceed the specified limits - this is a signal to reduce Vc or select a cutter of a larger diameter.
Frequently Asked Questions
Where do the starting values of Vc and fz come from? From the tool manufacturers' tables. The calculator contains average ranges for each ISO material group × cutter type × diameter combination. This is not a replacement for a specific manufacturer’s catalog - it’s a quick start when the catalog is not at hand or you need to evaluate the mode “by eye”.
What is MRR and why is it needed? MRR (Material Removal Rate) is the volume of metal removed per minute: MRR = ae × ap × Vf. Measured in cm³/min. MRR shows real productivity: you can reduce ae by half and increase Vf by half - MRR will remain the same, but the processing strategy will be completely different (HSM vs conventional milling).
When to turn on chip thinning? Automatically turns on when ae < 50% of D. If you are milling with small overlap (trochoidal milling, HSM, wall finishing) - chip thinning is required. Without it, the tool does not cut, but rubs, and you get overheating and BUE instead of chips.
Why does the calculator show fz (CT) higher than the catalog value? Because with a small ae, the tooth removes a thin sickle, and not a full-fledged chip. In order for hex (real thickness) to remain at the level of the catalog fz, the software fz needs to be increased. This is normal and correct - this is how trochoidal milling works.
What to do if the RPM is above the machine limit? Two options: 1) Reduce Vc - switch from MID to LOW preset. 2) Use a larger diameter cutter - RPM is inversely proportional to Ø. For example, going from Ø 8 mm to Ø 12 mm reduces RPM by 33% for the same Vc.
Do you need help selecting a cutter and modes for a specific material or machine? Contact our specialists - we will select a tool and strategy.