CNC Feeds and Speeds Calculator — RPM, Feed Rate, Chip Load, Cutting Speed and Machining Formulas

CNC Feeds and Speeds Calculator: RPM, Feed Rate, Chip Load and Cutting Speed

The Complete CNC Machining Formula Guide for Milling, Turning, Drilling and Tapping

Choosing the correct CNC feeds and speeds is one of the most important parts of successful machining.

Incorrect spindle speed can shorten tool life, generate excessive heat, or produce poor surface finish.

Incorrect feedrate can cause rubbing, chatter, tool breakage, excessive cutting forces, or unnecessary cycle time.

A reliable feeds and speeds calculation helps machinists understand the relationship between:

• Spindle speed (RPM)
• Cutting speed
• Feedrate
• Feed per tooth
• Feed per revolution
• Number of cutting edges
• Tool diameter
• Workpiece material
• Tool material
• Machining operation

This guide provides the essential formulas, step-by-step examples, CNC programming connections, troubleshooting advice, and reference tables needed to calculate machining parameters.

Important: Calculated values are starting points, not guaranteed safe machining settings. Actual cutting parameters depend on the tool manufacturer’s recommendations, material grade, tool geometry, coating, tool engagement, coolant, machine rigidity, workholding, and setup.

PART 1 — QUICK CNC FEEDS AND SPEEDS FORMULAS

1. CNC RPM Calculator Formula

For metric units:

RPM = (1000 × Vc) / (π × D)

Where:

• RPM = Spindle revolutions per minute
• Vc = Cutting speed in meters per minute
• D = Cutting diameter in millimeters
• π ≈ 3.14159

Example

Tool diameter: 10 mm

Cutting speed: 150 m/min

RPM = (1000 × 150) / (π × 10)

RPM ≈ 4,775

This is the theoretical spindle speed corresponding to the selected cutting speed.

It does not independently determine whether the tool or setup can safely operate at that RPM.

2. CNC Feed Rate Calculator Formula

For milling:

Feedrate (mm/min) = RPM × Number of teeth × Feed per tooth (mm/tooth)

Also written as:

Vf = n × z × fz

Where:

• Vf = Feedrate
• n = Spindle speed
• z = Number of effective cutting teeth
• fz = Feed per tooth

Example

Spindle speed: 4,000 RPM

Number of teeth: 4

Feed per tooth: 0.05 mm/tooth

Feedrate = 4000 × 4 × 0.05

Feedrate = 800 mm/min

3. Chip Load Calculator Formula

For a conventional milling feed calculation:

Feed per tooth = Feedrate / (RPM × Number of teeth)

Or:

fz = Vf / (n × z)

Example

Feedrate: 1,200 mm/min

Spindle speed: 6,000 RPM

Number of teeth: 4

fz = 1200 / (6000 × 4)

fz = 0.05 mm/tooth

This is the programmed feed per tooth.

Actual chip thickness also depends on cutter engagement and geometry.

4. Cutting Speed Calculator Formula

For metric units:

Vc = (π × D × RPM) / 1000

Example

Tool diameter: 12 mm

Spindle speed: 5,000 RPM

Vc = (π × 12 × 5000) / 1000

Vc ≈ 188.5 m/min

5. Feed Per Revolution Calculator

Feed per revolution = Feedrate / RPM

Or:

f = Vf / n

Example

Feedrate: 300 mm/min

Spindle speed: 1,000 RPM

f = 300 / 1000

f = 0.30 mm/rev

This relationship is especially useful in turning and drilling.

PART 2 — UNDERSTANDING CNC CUTTING SPEED

6. What Is Cutting Speed?

Cutting speed describes the relative tangential speed between the cutting edge and the workpiece surface at the relevant cutting diameter.

It is commonly expressed as:

• Meters per minute (m/min)
• Surface feet per minute (SFM)

Cutting speed is not the same as spindle RPM.

A large-diameter tool and a small-diameter tool running at the same RPM have different cutting speeds.

7. Why Tool Diameter Changes RPM

Consider two tools operating at the same target cutting speed.

Tool A: 10 mm diameter

Tool B: 20 mm diameter

At 150 m/min:

10 mm tool:

RPM ≈ 4,775

20 mm tool:

RPM ≈ 2,387

Doubling the cutting diameter approximately halves the required RPM.

8. Cutting Speed vs Spindle Speed

Cutting speed describes surface velocity.

Spindle speed describes revolutions per minute.

The relationship depends on diameter.

This distinction is essential for:

• Milling
• Drilling
• Turning
• Boring
• Reaming
• Threading

9. How to Choose Cutting Speed

The most reliable starting point is the cutting-tool manufacturer’s recommended data for the exact:

• Tool grade
• Tool material
• Coating
• Workpiece material
• Machining operation
• Coolant condition
• Tool engagement

Published values may differ significantly between tools that appear similar.

A generic material chart should never override a tool-specific recommendation.

10. Why Higher RPM Is Not Always Better

Increasing RPM may increase productivity in some conditions.

However, excessive RPM can contribute to:

• Heat generation
• Accelerated tool wear
• Chatter
• Poor surface finish
• Tool failure
• Spindle limitations

The appropriate speed depends on the entire machining system.

PART 3 — CNC MILLING FEEDRATE CALCULATIONS

11. What Is Feed Per Tooth?

Feed per tooth is the programmed feed contribution associated with each cutting tooth during one spindle revolution.

It is commonly written as fz.

Example:

A four-flute end mill rotates at 5,000 RPM.

Each tooth has a programmed feed of 0.04 mm.

Feedrate = 5000 × 4 × 0.04

Feedrate = 800 mm/min

12. What Is Chip Load?

In common shop usage, chip load often refers to feed per tooth.

However, actual chip thickness can differ from programmed feed per tooth because of:

• Radial engagement
• Cutter entry angle
• Cutter geometry
• Tool runout
• Cutting conditions

This distinction matters particularly during low radial engagement milling.

13. Two-Flute End Mill Calculation

Example:

RPM: 8,000

Flutes: 2

Feed per tooth: 0.04 mm

Feedrate = 8000 × 2 × 0.04

Feedrate = 640 mm/min

14. Three-Flute End Mill Calculation

Example:

RPM: 10,000

Flutes: 3

Feed per tooth: 0.05 mm

Feedrate = 10000 × 3 × 0.05

Feedrate = 1,500 mm/min

15. Four-Flute End Mill Calculation

Example:

RPM: 6,000

Flutes: 4

Feed per tooth: 0.04 mm

Feedrate = 6000 × 4 × 0.04

Feedrate = 960 mm/min

16. Six-Flute End Mill Calculation

Example:

RPM: 4,000

Flutes: 6

Feed per tooth: 0.03 mm

Feedrate = 4000 × 6 × 0.03

Feedrate = 720 mm/min

17. Why Flute Count Matters

For a given spindle speed and programmed feed per tooth, increasing the number of effective teeth increases the calculated feedrate.

However, more flutes do not automatically mean better performance.

Important considerations include:

• Chip evacuation
• Tool geometry
• Material behavior
• Tool engagement
• Machine rigidity

18. Face Milling Feedrate

The same general feed formula applies to face milling when the appropriate effective tooth count and recommended feed per tooth are used.

Vf = RPM × Effective teeth × Feed per tooth

Insert geometry and cutter engagement may influence the recommended values.

19. High-Feed Milling

High-feed milling tools use specialized geometries and cutting strategies.

The programmed feed per tooth can be relatively large compared with conventional milling.

However, the actual chip thickness depends strongly on insert geometry and engagement.

Use the tool manufacturer’s specific recommendations.

20. Slot Milling vs Side Milling

A full-width slot generally creates different cutting conditions from a light side-milling pass.

Differences include:

• Radial engagement
• Chip evacuation
• Heat
• Cutting forces
• Tool deflection

A feedrate suitable for one operation may not be appropriate for the other.

PART 4 — RADIAL CHIP THINNING

21. What Is Radial Chip Thinning?

Radial chip thinning occurs when cutter engagement causes the maximum chip thickness to be smaller than the programmed feed per tooth.

This is especially relevant in low radial engagement milling.

The effect depends on cutter geometry and cutting conditions.

22. Why Chip Thinning Matters

If the actual chip thickness becomes too small, the cutting edge may rub rather than cut efficiently.

This can contribute to:

• Heat
• Premature wear
• Poor finish
• Reduced productivity

Increasing programmed feed may be appropriate in some low-engagement conditions, but the correction must be calculated for the specific tool and strategy.

23. Simplified Chip Thinning Relationship

For a conventional peripheral milling geometry with radial engagement less than half the cutter diameter, a simplified relationship is:

Maximum chip thickness ≈ fz × sin(θ)

Where:

cos(θ) = 1 − (2 × ae / D)

And:

• ae = Radial depth of cut
• D = Cutter diameter
• θ = Engagement angle
• fz = Programmed feed per tooth

This simplified model does not represent every cutter geometry.

24. Radial Chip Thinning Example

Tool diameter: 10 mm

Radial engagement: 1 mm

Programmed feed per tooth: 0.05 mm

cos(θ) = 1 − (2 × 1 / 10)

cos(θ) = 0.8

sin(θ) = 0.6

Maximum chip thickness ≈ 0.05 × 0.6

Maximum chip thickness ≈ 0.03 mm

The programmed feed per tooth is 0.05 mm, but the simplified maximum chip thickness is approximately 0.03 mm.

25. Chip Thinning Limitations

The simplified formula may not apply directly to:

• Ball nose tools
• High-feed cutters
• Complex insert geometries
• Strongly varying tool engagement
• Certain three-dimensional machining operations

Use specialized tool data or CAM calculations where appropriate.

PART 5 — CNC TURNING SPEED AND FEED

26. Turning Cutting Speed

In turning, the relevant cutting diameter is typically the workpiece diameter at the cutting location.

For metric units:

RPM = (1000 × Vc) / (π × D)

27. CNC Lathe RPM Example

Workpiece diameter: 50 mm

Target cutting speed: 180 m/min

RPM = (1000 × 180) / (π × 50)

RPM ≈ 1,146

28. Why RPM Changes During Turning

As the workpiece diameter decreases, maintaining the same surface speed requires higher RPM.

This is why constant surface speed control is useful in many turning operations.

29. G96 Constant Surface Speed

On many CNC lathes, G96 selects constant surface speed mode.

Illustrative syntax on a compatible metric FANUC-style lathe:

G96 S180

The meaning and units of S depend on the control and its active unit system.

Actual RPM varies with the effective cutting diameter.

30. G97 Constant RPM

G97 commonly selects constant spindle speed mode on many lathes.

Illustrative example:

G97 S1200

This requests a fixed spindle speed of 1,200 RPM on compatible controls.

31. G96 RPM Limits

Constant surface speed can demand increasingly high RPM as diameter approaches zero.

A suitable spindle-speed limit is therefore essential.

Some FANUC-style lathes use G50 for spindle speed clamping, while other controls use different methods.

Never assume one limit-setting command applies to every lathe.

32. Turning Feed Per Revolution

Turning feed is often specified in mm/rev.

Example:

Spindle speed: 1,200 RPM

Feed: 0.20 mm/rev

Equivalent feed per minute:

1200 × 0.20 = 240 mm/min

33. G94 and G95 Feed Modes

On many controls, G94 and G95 distinguish feed per minute and feed per revolution.

However, code meanings differ by controller and machine type.

For example, some FANUC-style turning controls use G98/G99 for feed modes.

Always verify the exact controller.

PART 6 — CNC DRILLING CALCULATIONS

34. Drilling RPM Formula

The same cutting speed relationship applies to drilling:

RPM = (1000 × Vc) / (π × Drill diameter)

Example:

Drill diameter: 8 mm

Cutting speed: 80 m/min

RPM ≈ 3,183

35. Drilling Feedrate Formula

Feedrate = RPM × Feed per revolution

Example:

RPM: 2,000

Feed per revolution: 0.12 mm/rev

Feedrate = 2000 × 0.12

Feedrate = 240 mm/min

36. Peck Drilling Considerations

Peck drilling may be useful when chip evacuation is difficult.

Relevant factors include:

• Hole depth
• Drill diameter
• Material
• Coolant
• Drill geometry
• Chip formation

Peck depth is not determined by RPM and feedrate alone.

37. G81 Drilling Cycle

G81 is commonly used for basic drilling on compatible milling controls.

Feedrate calculations remain important when selecting cycle parameters.

However, the exact canned-cycle syntax and return behavior are controller-specific.

38. G83 Peck Drilling Cycle

G83 commonly represents peck drilling on compatible milling controls.

A correct feedrate does not automatically guarantee that peck depth, retract behavior, or chip evacuation is suitable.

PART 7 — CNC TAPPING CALCULATIONS

39. Tapping Feed Formula

For a single-start thread:

Feedrate (mm/min) = RPM × Thread pitch (mm/rev)

Example:

RPM: 500

Pitch: 1.25 mm

Feedrate = 500 × 1.25

Feedrate = 625 mm/min

40. M8 × 1.25 Tapping Example

For an M8 × 1.25 thread:

Pitch = 1.25 mm

At 400 RPM:

Feedrate = 400 × 1.25

Feedrate = 500 mm/min

This is the theoretical feedrate corresponding to the thread lead.

The actual tapping program must use the feed mode and synchronization method required by the controller.

41. M10 × 1.5 Tapping Example

Pitch = 1.5 mm

RPM = 300

Feedrate = 300 × 1.5

Feedrate = 450 mm/min

42. Multi-Start Thread Considerations

For multi-start threads, the axial advance per revolution is the thread lead, not simply the pitch.

Lead = Pitch × Number of starts

Use lead when calculating the required axial advance per revolution.

43. Why Tapping Is Different

Tapping requires synchronization between spindle rotation and axial feed.

A mathematically correct feedrate does not prove that the machine’s rigid-tapping cycle is configured correctly.

Check controller requirements and tool manufacturer guidance.

PART 8 — IMPERIAL CNC MACHINING FORMULAS

44. Surface Feet per Minute

In imperial machining, cutting speed is commonly expressed as SFM.

The RPM formula is:

RPM = (12 × SFM) / (π × Diameter in inches)

A common approximation is:

RPM ≈ (3.82 × SFM) / Diameter

45. Imperial RPM Example

Cutting speed: 300 SFM

Tool diameter: 0.5 inches

RPM ≈ (3.82 × 300) / 0.5

RPM ≈ 2,292

46. Inches per Minute Feedrate

IPM = RPM × Number of teeth × IPT

Where IPT means inches per tooth.

Example:

RPM: 5,000

Teeth: 4

IPT: 0.002

IPM = 5000 × 4 × 0.002

IPM = 40

47. Inches per Revolution

IPR = IPM / RPM

Example:

IPM = 24

RPM = 1,200

IPR = 24 / 1200

IPR = 0.020

48. Metric and Imperial Conversion

Useful conversions:

• 1 inch = 25.4 mm
• 1 foot = 0.3048 m
• 1 mm = approximately 0.03937 inches
• 1 m/min = approximately 3.28084 SFM

Always confirm unit modes before transferring calculated values into a CNC program.

PART 9 — CNC MACHINING PARAMETER TABLES

49. Formula Reference Table

Calculation	Metric formula
RPM	1000 × Vc / (π × D)
Cutting speed	π × D × RPM / 1000
Milling feedrate	RPM × Teeth × fz
Feed per tooth	Feedrate / (RPM × Teeth)
Feed per revolution	Feedrate / RPM
Drilling feedrate	RPM × Feed per revolution
Tapping feedrate	RPM × Thread lead
Machining time for constant feed	Cutting travel / Feedrate

50. Example RPM Reference Table

The following table is a mathematical comparison using a hypothetical target cutting speed of 100 m/min. It is not a recommended cutting-speed chart.

Diameter	Calculated RPM
3 mm	10,610
5 mm	6,366
6 mm	5,305
8 mm	3,979
10 mm	3,183
12 mm	2,653
16 mm	1,989
20 mm	1,592
25 mm	1,273
50 mm	637

51. Example Milling Feedrate Table

Assumptions:

RPM = 5,000

Feed per tooth = 0.05 mm

Effective teeth	Feedrate
2	500 mm/min
3	750 mm/min
4	1,000 mm/min
5	1,250 mm/min
6	1,500 mm/min

These values demonstrate the formula only.

They are not universal recommended cutting parameters.

PART 10 — MACHINING TIME CALCULATIONS

52. Basic Machining Time Formula

For constant linear feed:

Time (minutes) = Cutting travel (mm) / Feedrate (mm/min)

Example:

Cutting travel: 200 mm

Feedrate: 500 mm/min

Time = 200 / 500

Time = 0.4 minutes = 24 seconds

53. Why Actual Cycle Time Is Longer

Real cycle time may include:

• Rapid movements
• Tool changes
• Spindle acceleration
• Dwell
• Peck retracts
• Coolant delays
• Machine acceleration
• Programmed stops

A simple cutting-time formula does not include these additional operations.

54. Material Removal Rate for Milling

For a simple rectangular milling engagement:

MRR = ap × ae × Vf

Where:

• ap = Axial depth of cut in mm
• ae = Radial width of cut in mm
• Vf = Feedrate in mm/min

Result:

MRR in mm³/min

55. Material Removal Rate Example

Axial depth: 2 mm

Radial width: 5 mm

Feedrate: 800 mm/min

MRR = 2 × 5 × 800

MRR = 8,000 mm³/min

Equivalent:

8 cm³/min

This simplified formula assumes the stated engagement is maintained.

PART 11 — CNC FEEDS AND SPEEDS TROUBLESHOOTING

56. Tool Rubbing Instead of Cutting

Possible causes:

• Feed per tooth too low
• Incorrect tool geometry
• Tool wear
• Excessive runout
• Unsuitable engagement
• Poor cutting conditions

Rubbing can generate heat and accelerate wear.

57. Excessive Tool Wear

Potential causes include:

• Excessive cutting speed
• Incorrect feed
• Poor coolant application
• Abrasive material
• Unsuitable tool grade
• Excessive cutting forces

Tool wear should be evaluated together with the machining conditions.

58. CNC Chatter

Chatter can be influenced by:

• Spindle speed
• Feedrate
• Tool overhang
• Machine rigidity
• Workholding
• Cutting depth
• Tool geometry

Changing RPM alone may not resolve the problem.

59. Poor Surface Finish

Possible contributors:

• Incorrect feed per tooth
• Tool runout
• Tool deflection
• Chatter
• Tool wear
• Incorrect tool geometry
• Unstable workholding

A surface finish problem should be diagnosed systematically.

60. Broken End Mill

Potential causes:

• Excessive engagement
• Poor chip evacuation
• Incorrect toolpath
• Incorrect feedrate
• Incorrect spindle speed
• Tool deflection
• Collision
• Tool damage

Do not automatically reduce feedrate without determining the actual failure mechanism.

61. Burning or Excessive Heat

Possible causes:

• Rubbing
• Poor chip evacuation
• Excessive cutting speed
• Incorrect coolant strategy
• Unsuitable tool material
• Excessive contact time

Different materials require different approaches to heat management.

62. Aluminum Machining Problems

Aluminum machining may be affected by:

• Built-up edge
• Chip evacuation
• Tool coating
• Cutting speed
• Tool geometry
• Coolant or lubrication strategy

Use recommendations appropriate to the exact aluminum alloy and cutting tool.

63. Stainless Steel Machining Problems

Stainless steels vary widely in machinability.

Some grades are susceptible to work hardening.

Important factors include:

• Appropriate cutting speed
• Sufficient effective chip thickness
• Tool grade
• Stable engagement
• Coolant delivery
• Machine rigidity

Avoid relying on a single universal stainless-steel cutting-speed value.

64. Titanium Machining Problems

Titanium machining can involve:

• Concentrated cutting heat
• Tool wear
• High cutting forces
• Tool deflection
• Limited thermal conductivity

Tool-specific cutting data and stable machining conditions are essential.

PART 12 — CNC G-CODE CONNECTIONS

65. Spindle Speed S Command

On many CNC controls, S specifies a spindle speed or cutting-speed value depending on the active spindle mode.

Example:

S2500 M03

On a compatible fixed-RPM milling configuration, this requests 2,500 RPM and clockwise spindle rotation.

Machine-specific behavior must be verified.

66. Feedrate F Command

Example:

G94

G01 X50. F500.

On a compatible metric milling control, this illustrates a programmed feed of 500 mm/min in feed-per-minute mode.

The command does not establish safe tooling, workholding, or clearance.

67. Feed Per Revolution Programming

On compatible controls, feed-per-revolution mode allows the programmed F value to represent distance per spindle revolution.

The actual G-code used to select that mode depends on the controller.

68. G96 and G97 in Turning

G96 is commonly used for constant surface speed.

G97 is commonly used for constant RPM.

A correct turning program must account for spindle limits, diameter, tool location, and controller conventions.

69. G84 Tapping and Feed Calculations

G84 commonly represents a tapping cycle on supported controls.

The feed parameter must match the controller’s required feed mode and thread lead.

A formula alone cannot verify spindle-feed synchronization.

PART 13 — FREQUENTLY ASKED QUESTIONS

70. How Do You Calculate CNC RPM?

Use:

RPM = 1000 × Cutting speed / (π × Diameter)

For metric units, cutting speed is in m/min and diameter is in mm.

71. How Do You Calculate CNC Feedrate?

For conventional milling:

Feedrate = RPM × Effective teeth × Feed per tooth

72. What Is Chip Load in CNC?

Chip load commonly refers to feed per tooth.

Actual chip thickness may differ depending on cutter engagement and geometry.

73. What Is the Difference Between Feedrate and Cutting Speed?

Feedrate describes how quickly the tool advances along the programmed path.

Cutting speed describes the relative surface velocity at the cutting diameter.

74. What Is the Difference Between RPM and SFM?

RPM measures spindle revolutions per minute.

SFM measures cutting speed in surface feet per minute.

75. How Do I Calculate Feed Per Tooth?

Use:

Feed per tooth = Feedrate / (RPM × Effective teeth)

76. How Do I Calculate Drilling Feedrate?

Use:

Feedrate = RPM × Feed per revolution

77. How Do I Calculate Tapping Feedrate?

For a synchronized tapping operation:

Feedrate = RPM × Thread lead

When programming in feed-per-revolution mode, the programmed feed convention must match the controller.

78. Does Increasing RPM Improve Surface Finish?

Not necessarily.

Surface finish depends on tool geometry, feed, stability, wear, and other machining conditions.

79. Does Increasing Feedrate Always Increase Productivity?

Not always.

Excessive feedrate can increase cutting forces, cause tool failure, or produce unacceptable parts.

80. Is There One Correct Cutting Speed for Steel?

No.

The appropriate cutting speed depends on the steel grade, cutting tool, operation, and machining conditions.

81. Can I Use the Same Feeds and Speeds for Every End Mill?

No.

Different tool geometries, grades, coatings, and manufacturers can require different parameters.

82. What Is a Good Starting Point for CNC Feeds and Speeds?

Use the cutting-tool manufacturer’s recommendations for the exact tool and material.

Then verify machine limits, workholding, tool engagement, and process requirements.

PART 14 — PROFESSIONAL MACHINING WORKFLOW

83. Step 1 — Identify the Material

Determine the exact workpiece material and grade.

84. Step 2 — Identify the Cutting Tool

Record:

• Tool diameter
• Tool material
• Tool grade
• Coating
• Number of effective teeth
• Geometry
• Tool overhang

85. Step 3 — Select Cutting Speed

Use verified manufacturer recommendations.

86. Step 4 — Calculate RPM

Apply the correct formula for the unit system.

Check machine and tool speed limits.

87. Step 5 — Select Feed Per Tooth or Revolution

Use the appropriate recommended feed data for the operation.

88. Step 6 — Calculate Feedrate

For milling:

Vf = RPM × Teeth × fz

For turning or drilling:

Vf = RPM × Feed per revolution

89. Step 7 — Check Tool Engagement

Review:

• Axial depth
• Radial width
• Toolpath
• Chip evacuation
• Tool deflection
• Cutting forces

90. Step 8 — Verify the NC Program

Confirm:

• Correct spindle mode
• Correct feed mode
• Correct units
• Correct tool
• Correct offsets
• Correct machining strategy

91. Step 9 — Monitor Machining Results

Evaluate:

• Tool wear
• Surface finish
• Chip formation
• Machine load
• Chatter
• Dimensional accuracy

Adjust parameters using qualified machining judgment and manufacturer guidance.

PART 15 — ADVANCED CNC CALCULATIONS

92. Constant Surface Speed Across Different Diameters

Suppose target cutting speed is 180 m/min.

At 60 mm diameter:

RPM ≈ 955

At 40 mm diameter:

RPM ≈ 1,432

At 20 mm diameter:

RPM ≈ 2,865

This demonstrates why spindle RPM increases as turning diameter decreases under constant surface speed control.

93. Feedrate When RPM Changes

Suppose feed per tooth remains 0.04 mm and the tool has four effective teeth.

At 4,000 RPM:

Feedrate = 640 mm/min

At 6,000 RPM:

Feedrate = 960 mm/min

At 8,000 RPM:

Feedrate = 1,280 mm/min

The programmed feedrate must change proportionally to maintain the same feed per tooth.

94. Feed Per Tooth When Feedrate Changes

Suppose RPM is 5,000 and the tool has four effective teeth.

At 500 mm/min:

fz = 0.025 mm/tooth

At 1,000 mm/min:

fz = 0.05 mm/tooth

At 1,500 mm/min:

fz = 0.075 mm/tooth

This demonstrates how feedrate affects programmed feed per tooth.

95. Tool Diameter and Cutting Speed Comparison

At 5,000 RPM:

5 mm diameter:

Vc ≈ 78.5 m/min

10 mm diameter:

Vc ≈ 157.1 m/min

20 mm diameter:

Vc ≈ 314.2 m/min

The same spindle RPM produces very different cutting speeds at different diameters.

96. Why Calculators Cannot Replace Tool Data

A calculator performs mathematical operations.

It does not automatically know:

• Tool grade
• Coating
• Material hardness
• Workholding quality
• Machine rigidity
• Tool wear
• Coolant effectiveness
• Process stability

A calculated result is only as useful as its input assumptions.

FINAL CNC FEEDS AND SPEEDS CHEAT SHEET

Parameter	Symbol	Typical unit
Spindle speed	n	RPM
Cutting speed	Vc	m/min
Tool diameter	D	mm
Feedrate	Vf	mm/min
Feed per tooth	fz	mm/tooth
Feed per revolution	f	mm/rev
Number of effective teeth	z	Count
Axial depth of cut	ap	mm
Radial width of cut	ae	mm
Material removal rate	MRR	mm³/min

Essential Equations

RPM

n = 1000 × Vc / (π × D)

Cutting speed

Vc = π × D × n / 1000

Milling feedrate

Vf = n × z × fz

Feed per tooth

fz = Vf / (n × z)

Feed per revolution

f = Vf / n

Drilling feedrate

Vf = n × f

Tapping feedrate

Vf = n × Thread lead

Milling material removal rate

MRR = ap × ae × Vf

Constant-feed machining time

Time = Travel distance / Feedrate

CONCLUSION

Correct CNC feeds and speeds begin with understanding the relationship between cutting speed, spindle RPM, feed per tooth, feed per revolution, and tool engagement.

The essential calculation process is:

IDENTIFY THE MATERIAL

↓

SELECT THE CUTTING TOOL

↓

CHECK MANUFACTURER CUTTING DATA

↓

CALCULATE RPM

↓

CALCULATE FEEDRATE

↓

VERIFY TOOL ENGAGEMENT

↓

CHECK MACHINE LIMITS

↓

VERIFY THE CNC PROGRAM

↓

MONITOR MACHINING PERFORMANCE

A feeds and speeds calculator can save time, reduce arithmetic errors, and help programmers understand machining parameters.

However, safe and productive machining always depends on verified cutting data, correct setup, suitable tooling, and informed process decisions.

THE GOLDEN RULE OF CNC MACHINING:

CALCULATE THE NUMBERS. VERIFY THE CONDITIONS. MACHINE WITH CONTROL.

Complete CNC Milling, Turning, Drilling and Tapping Formula Reference — RPM, Feedrate, Chip Load, Cutting Speed and Machining Calculations.