Guides · 24 October 2026
How to estimate CNC milling cycle time for a quote
You rarely have time to program a part in CAM before you quote it. You still need a cycle time you can defend. For most prismatic parts, three formulas and an honest allowance for the time the tool is not cutting get you close. Here is the method, with a worked example.
Spindle speed and feed rate
Tool makers give a cutting speed, Vc, in metres per minute, and a feed per tooth, fz, in millimetres. For a cutter of diameter D (mm) with z teeth:
n = 1000 × Vc ÷ (π × D)
vf = n × z × fz
n is the spindle speed in rpm and vf the feed rate in mm/min. In inches the first formula is n = 12 × SFM ÷ (π × D), with D in inches. As with turning, cap n at the machine's top speed: a small cutter in aluminium can ask for more rpm than an older machining centre has.
Roughing: think in volume, not in toolpaths
For roughing a pocket or a step you do not need the toolpath. Work out how much material comes out per minute, the material removal rate:
MRR = ae × ap × vf
ae is the width of cut (stepover) and ap the depth of cut, both in mm, so MRR comes out in mm³ per minute. Divide the volume to remove by it, then add 10 to 20% for ramping in, linking moves and corners, where the cutter is not taking a full cut.
Finishing, facing and holes: think in length
Finishing passes, facing passes and holes are better estimated by length: the distance the tool travels at feed, divided by the feed rate. For a facing pass, add the cutter diameter to the length so the cutter clears the part at both ends. For a drilled hole, add the drill point (about 0.3 × D) and a couple of millimetres of approach to the depth. A tap travels in and out at one pitch per revolution.
A worked example
A 6061 aluminium plate, 120 × 80 × 25 mm, on a vertical machining centre with a 10,000 rpm spindle. The top is faced 1 mm, a pocket 80 × 50 × 15 mm deep is roughed and finished, and four holes are drilled Ø6.8 mm, 20 mm deep, and tapped M8 × 1.25, 16 mm deep.
- Facing: Ø50 face mill, 5 inserts, 600 m/min (about 1,970 SFM), 0.10 mm per tooth: 3,820 rpm and 1,910 mm/min. Three passes of 170 mm.
- Roughing the pocket: Ø12 three-flute carbide end mill, 300 m/min, 0.05 mm per tooth: 7,958 rpm and 1,194 mm/min. With a 6 mm stepover and 5 mm depth of cut, MRR is 35.8 cm³ per minute; the pocket is 60 cm³.
- Finishing: one pass round the 260 mm of wall at 800 mm/min, and the floor in seven 80 mm passes at 1,194 mm/min.
- Drilling: Ø6.8 carbide drill, 100 m/min and 0.15 mm/rev: 4,681 rpm and 702 mm/min, 24 mm of travel per hole.
- Tapping: M8 × 1.25 at 25 m/min: 995 rpm, 36 mm in and out per hole.
| Operation | How it is worked out | Minutes |
|---|---|---|
| Face top | 510 mm ÷ 1,910 mm/min | 0.27 |
| Rough pocket | 60,000 mm³ ÷ 35,810 mm³/min, + 15% | 1.93 |
| Finish walls | 260 mm ÷ 800 mm/min | 0.33 |
| Finish floor | 560 mm ÷ 1,194 mm/min | 0.47 |
| Drill 4 holes | 4 × 24 mm ÷ 702 mm/min | 0.14 |
| Tap 4 holes | 4 × 36 mm ÷ 1,243 mm/min | 0.12 |
| Cutting time | 3.24 | |
| Rapids (10% of cutting) | 0.32 | |
| Tool changes | 5 tools × 10 s | 0.83 |
| Load, unload, deburr | timed on a similar part | 1.50 |
| Cycle time | 5.90 |
Two things stand out. Roughing the pocket is the biggest single item, which is where a better strategy (a deeper cut with a smaller stepover, or adaptive clearing) pays off. And the time spent not cutting, 2.66 minutes, is 45% of the cycle. On small parts that share is often higher.
At a machine rate of US$95 an hour, 5.90 minutes is US$9.34 of machine time per part, before material, labour, overhead and margin.
From cycle time to batch time
Add the setup once per batch. With a one-hour setup and 25 parts:
60 + 25 × 5.90 = 207.5 minutes, about 3.5 hours
At 5 parts the setup is two thirds of the machine time; at 100 parts it is a tenth. That is why the price per part has to fall with quantity, as the guide on pricing small batches shows.
Common mistakes
- Using catalogue maximums. Use the speeds and feeds you actually run on that material and machine, not the top of the tool maker's range.
- Pricing roughing from the toolpath length. Volume divided by MRR is quicker and usually closer for a quote.
- Forgetting the second operation. If the part has to be flipped, the second side is a second setup and a second load, even if it only has one feature.
- Leaving out tool changes and loading. They are machine time you pay for. Time them once on a typical part.
- Never checking. Log the real cycle time on the first batch and compare it with the estimate. After a few jobs you will know whether your estimates run fast or slow, and by how much.