CNC machining time calculation: estimating by splitting cutting distance, feed, rapids and non-cutting time
Uses a two-pass lathe OD example to explain the calculation cutting time = distance ÷ feed per minute, conversion from feed per revolution, non-cutting time such as rapids and tool changes, and why simulated time differs from the actual cycle time.
The basic estimating formula
The starting point for machining time calculation is simple: cutting time (min) = cutting distance (mm) ÷ feed per minute (mm/min). If the program is written in feed per revolution, first convert it with feed per minute = F (mm/rev) × S (rpm). Adding the time for rapids, tool changes, spindle acceleration and auxiliary actions such as coolant and doors gives the cycle time.
What makes estimates wrong is mostly not the formula but the items left out. An estimate based on cutting time alone usually comes out shorter than reality, and the smaller the part, the larger the share of non-cutting time.
Example program
Two turning passes of 62 mm each at Ø50 and Ø46, S1000, F0.25
O3008
T0101
G21 G90 G18 G40 G99
G97 S1000 M03
G00 X52. Z2.
G01 X50. F0.25
Z-60.
G00 X54. Z2.
X46.
G01 Z-60. F0.25
G00 X100. Z100.
M30The figure above is the CNC Path Analyzer result for this program (linear cutting 3 segments, rapid 3 segments).
Calculating the example's cutting time by hand
Note that the X travel on a lathe is half the diameter difference. The infeed from X52 to X50 is 2 mm in the program, but the tool moves only 1 mm. Also, since the cut starts at Z2, the 2 mm of air cutting in front of the face is included in the cutting time. The approach clearance is needed for safety, but in production runs of hundreds of parts these few millimeters add up to meaningful time.
| Section | Distance | Feed per minute | Time |
|---|---|---|---|
G01 X50. infeed | 2 mm in diameter → 1 mm in radius | 0.25 × 1000 = 250 | About 0.24 s |
Z-60. pass 1 | 62 mm (Z2 → Z-60) | 250 | About 14.9 s |
G01 Z-60. pass 2 | 62 mm | 250 | About 14.9 s |
| Total | About 125 mm | - | About 30 s |
Rapid traverse time
Rapids move at the machine's maximum speed, but they do not take zero seconds. On a lathe with a rapid rate of 20 m/min, the rapid moves in the example add up to a little over 200 mm, so the pure travel time is under one second. Each axis, however, has acceleration and deceleration phases, so many short rapids take much longer in reality than the calculation suggests. The difference is especially large in drilling patterns and peck cycles with many short moves.
Time often left out of estimates
- Tool changes: one turret index or ATC cycle usually takes a few seconds. In a program that changes tools ten times, that alone is tens of seconds.
- Spindle acceleration: time is spent whenever the spindle speed changes a lot, from standstill to 3,000 rpm, or from forward to reverse as in a tapping cycle.
- G96 spindle speed changes: with constant surface speed control, the spindle speed follows changes in diameter, and the per-minute speed of feed per revolution changes with it. Facing time can come out shorter or longer than under a fixed-speed assumption.
- Corner deceleration: contours made of many short blocks, or CAM output, slow down at every corner and do not reach the programmed F.
- Part loading and measurement: this time lies outside the program, but it determines the actual output per hour.
How to use simulated time
CNC Path Analyzer calculates a reference machining time from the distance, feed and spindle speed of supported blocks. Acceleration and tool change time differ from machine to machine and are not included. This value is therefore best regarded as close to the lower bound of the actual cycle time.
A practical approach is to determine once the ratio between the cycle time actually measured on a machine and the calculated value. For example, if a similar part calculated 3 minutes and measured 3 minutes 40 seconds, you can try multiplying the next estimate by a correction factor of about 1.22. The more similar the type of part (many short moves or long cuts), the better this factor fits.
What to check first when reducing machining time
Doing the calculation shows where the time goes. If cutting time dominates, look first at cutting conditions and the number of passes (such as choosing between G71 and G72); if non-cutting time is large, look first at the tool order, approach clearances and rapid paths. Removing unnecessary moves is often both safer and more effective than feeding faster.