鑽孔速度與進給計算機
Calculate spindle speed (RPM), linear feed rate, actual drilling time (with optional drill-point breakthrough allowance), and metal removal rate (MRR) for CNC drilling. Every parameter is explained in plain shop-floor language.
Calculator Inputs
Auto-calculating liveSelect your unit system and workpiece material to load typical starting parameters, or enter your own tooling catalog values directly.
計算結果
Use RPM and Feed Rate directly for CNC programming (S and F codes), and Time / MRR for cycle quoting.
Understanding the Parameters Visually
These diagrams connect every symbol in the calculator to the physical motion of the twist drill on your CNC machine.
Diagram 1: Diameter (D), Cutting Speed (vc), and RPM (n)
Because cutting speed vc is measured at the outer margin of diameter D, smaller drills require much higher spindle RPM (n) to reach the same surface speed.
Diagram 2: Feed Rate (vf), Hole Depth (L), and Point Length
The linear feed rate vf equals feed per revolution fn multiplied by RPM (n). For through holes, include the drill tip cone (approx. 0.3 × D for 118° drills) so the full diameter breaks through.
Drilling Formulas With Full Parameter Explanations
Every formula below updates automatically to match your selected unit system (Metric or Imperial) and explains each symbol in detail.
1) Spindle Speed (RPM)
- n = spindle speed in revolutions per minute (rpm).
- vc = cutting speed at the outside diameter of the drill (m/min).
- D = drill diameter (mm).
- 1000 = converts meters to millimeters; π ≈ 3.1416.
2) Linear Feed Rate (vf)
- vf = linear feed speed of the Z-axis per minute (mm/min).
- fn = feed per revolution, distance advanced in 1 spindle turn (mm/rev).
- n = calculated spindle speed (rpm).
3) Drilling Cycle Time (Tc)
- Tc = net cutting time in minutes (multiply by 60 for seconds).
- Leff = effective drilling travel (hole depth L + point allowance if through-hole).
- vf = linear feed rate (mm/min).
4) Metal Removal Rate (MRR)
- Q = volume of metal removed per minute (cm³/min).
- D = drill diameter (mm); (π × D² ÷ 4) is the hole cross-sectional area.
- vf = linear feed rate (mm/min).
- ÷ 1000 = converts mm³/min into standard cm³/min.
How to Use This Calculator
Select units and material
Pick Metric or Imperial first. Choosing a workpiece material loads conservative starting values for cutting speed and feed per revolution without overwriting your hole dimensions.
Set drill size and hole type
Enter your drill diameter (or click a quick-size button) and hole depth. Choose whether it is a blind hole or a through hole requiring 118° / 140° point breakthrough.
Apply or copy setup values
Read your spindle RPM, feed rate, and cycle time in seconds immediately. Click Copy Setup Summary to paste the complete parameter sheet into your CAM notes or quote.
Worked Example
Example condition: Drilling a Ø10 mm hole in alloy steel, 25 mm deep (blind hole), using a solid carbide drill at vc = 80 m/min 和 fn = 0.18 mm/rev.
- Spindle speed (n): (1000 × 80) ÷ (3.1416 × 10) ≈ 2,546 rpm
- Linear feed rate (vf): 0.18 × 2,546 ≈ 458 mm/min (18.04 in/min)
- Drilling time (Tc): 25 ÷ 458 ≈ 0.055 min (3.3 seconds; or 3.7 seconds if adding 3 mm point allowance for a through hole)
- Metal removal rate (Q): (3.1416 × 10² ÷ 4) × 458 ÷ 1000 ≈ 36.0 cm³/min
常見問題
What is the difference between cutting speed (vc) and feed rate (vf)?
Cutting speed (vc, measured in m/min or SFM) is the peripheral speed of the drill's outer corners as it spins. Feed rate (vf, measured in mm/min or in/min) is how fast the drill advances downward into the workpiece along the Z-axis.
How much extra depth should I add for a through hole?
標準 118° twist drill has a conical point length of approximately 0.30 × D, while a 140° carbide drill has a point length of about 0.18 × D. You can select either option in the "Hole type & drill point allowance" dropdown above to include this distance automatically.
Why does the calculated drilling time look shorter than my actual machine cycle?
The calculator outputs pure cutting time (Tc) while the drill is feeding at vf. Total machine floor-to-floor time also includes rapid approach/retract, spindle acceleration, tool change time, and peck-drilling (G83) dwell or chip-clearing retracts.
When should I reduce speed and feed for deep holes?
Once hole depth exceeds 5 × D, chip evacuation and heat dissipation become more demanding. Look at the L/D Ratio indicator under the results: for holes deeper than 5×D, verify internal coolant pressure or reduce feed rate by 10–25% and use a peck cycle if using HSS drills.
