How to Calculate CNC Cutting Parameters

CAM232 Team | April 18, 2026 | 9 min read

Getting the right cutting parameters is the difference between a perfect part and a broken tool. Spindle speed (RPM), feed rate, step over, and step down all work together to determine cut quality, tool life, and machining time. This guide covers the essential formulas and provides ready-to-use values for common materials.

The RPM Formula

Spindle speed is calculated from the recommended cutting speed (Vc) for the material and the tool diameter (D):

RPM = (Vc x 1000) / (PI x D)

Where:

Vc = Cutting speed (m/min) - depends on material

D = Tool diameter (mm)

PI = 3.14159

Example: Aluminum, 10mm end mill

RPM = (200 x 1000) / (3.14159 x 10)

RPM = 200000 / 31.4159

RPM = 6,366 RPM

Feed Rate Calculation

Feed rate (F) determines how fast the tool moves through the material, measured in mm/min:

F = RPM x fz x Z

Where:

fz = Feed per tooth (mm/tooth)

Z = Number of flutes (cutting edges)

Example: 6366 RPM, 0.05 mm/tooth, 3-flute end mill

F = 6366 x 0.05 x 3

F = 955 mm/min

Step Over and Step Down

Step Over (Radial Depth of Cut - ae)

The amount the tool moves sideways between passes. Expressed as a percentage of the tool diameter:

Roughing: 40-60% of tool diameter
Finishing: 5-15% of tool diameter
Slotting: 100% (full width cut)

Step Down (Axial Depth of Cut - ap)

How deep the tool cuts in each pass:

Roughing: 0.5-1.0x tool diameter
Finishing: 0.1-0.3x tool diameter
Hard materials: Reduce by 50%

Material Cutting Speed Table

Recommended cutting speeds (Vc) and feed per tooth (fz) for carbide end mills:

Material	Vc (m/min)	fz (mm/tooth)	Notes
Aluminum 6061	200-400	0.05-0.15	High speed, use flood coolant
Aluminum 7075	150-300	0.04-0.12	Harder alloy, slightly slower
Mild Steel (1018)	80-120	0.03-0.08	Flood coolant recommended
Carbon Steel (1045)	60-100	0.03-0.07	Reduce speed for deeper cuts
Stainless Steel 304	40-80	0.02-0.06	Work hardening - keep tool moving
Stainless Steel 316	35-70	0.02-0.05	Lower speed, rigid setup needed
Titanium Grade 5	30-60	0.02-0.05	High pressure coolant, low ae
Brass	150-300	0.05-0.12	Easy to machine, watch for grabbing
Copper	100-200	0.04-0.10	Soft, use sharp tools
Cast Iron	60-120	0.04-0.08	Dry cutting or air blast
Acetal / Delrin	200-500	0.05-0.15	No coolant needed, high speed
Acrylic (PMMA)	100-300	0.03-0.10	Single flute preferred, air blast
Wood / MDF	300-600	0.10-0.30	Dust extraction, single/double flute

Coolant Selection Guide

Choosing the right coolant strategy significantly impacts tool life and surface finish:

Coolant Type	Best For	Notes
Flood Coolant	Steel, stainless, aluminum	Best chip evacuation and cooling
Mist Coolant	Light cuts, aluminum	Less messy, adequate for moderate loads
Through-Spindle	Deep holes, titanium	Best for chip evacuation in deep cuts
Air Blast	Plastics, cast iron, dry machining	Chip clearing only, no cooling
MQL (Minimum Quantity)	Steel, aluminum	Eco-friendly, fine mist with lubricant
Dry	Cast iron, hardened steel with CBN	Some materials cut better dry

Practical Example: Aluminum Pocket

Machining a pocket in 6061 aluminum with a 10mm 3-flute carbide end mill:

Given:

Material: Aluminum 6061

Tool: 10mm 3-flute carbide

Vc = 250 m/min

fz = 0.08 mm/tooth

Calculations:

RPM = (250 x 1000) / (3.14159 x 10) = 7,958 RPM

Feed = 7958 x 0.08 x 3 = 1,910 mm/min

Step Over = 10 x 0.50 = 5.0 mm (50%)

Step Down = 10 x 0.75 = 7.5 mm

G-Code:

S7958 M3

G1 F1910

Common Mistakes to Avoid

Too slow RPM with high feed: Causes excessive chip load and tool breakage
Too fast RPM with low feed: Generates heat, causes rubbing instead of cutting
Ignoring step over in pocketing: Full-width cuts generate 2-3x more cutting forces
No coolant on stainless steel: Work hardening makes re-cutting impossible
Same parameters for roughing and finishing: Finishing needs lower step over and higher RPM

Let CAM232 Calculate Your Parameters

CAM232 automatically calculates optimal cutting parameters for your material and tool. Just select the operation, enter your tool size, and get production-ready G-Code.

Try It Free

Conclusion

Correct cutting parameters are essential for efficient CNC machining. Start with the recommended values from the material table, adjust based on your specific setup (machine rigidity, tool quality, workholding), and always listen to the cut. A smooth, consistent sound means good parameters. CAM232 can handle these calculations automatically, letting you focus on the design rather than the math.

CAM232 Blog