Skip to content

Quoting guides

How to estimate machining time for a CNC quote

Why the time estimate carries the quote

Once material is priced, most of a CNC quote is time multiplied by a rate. An error in the minutes is multiplied twice: by the shop rate, and by every piece in the order. That is why estimating machining time is the part of quoting that experienced estimators watch most closely.

The most defensible number comes from a rough CAM program. One estimator who works that way says “I program ( roughly ) every RFQ and use the time the software generates”, and that it is “VERY time consuming and exhausting” [3]. The method below gets you a number you can defend without programming the part, and tells you when programming it is worth the time.

Setup time and run time are different kinds of time

Write the job up the way it will run, operation by operation: “I write it up as operations for the part. OP1, OP2, OP3” [5]. Then sort every minute into one of two buckets.

  • Setup, once per lot: CAM programming, fixtures or soft jaws, loading tools and setting offsets, proving out the first piece, and first-article inspection. It is the same for 1 piece or 100.
  • Run time, every piece: cutting time, the non-cutting time inside the cycle (tool changes, rapids, probing), loading and unloading, in-process checks and deburring.

Keep them apart all the way to the price. Setup is divided across each quantity break and run time is multiplied by it, which is why quantity break pricing only works if the two were never blended.

Roughing: volume divided by metal removal rate

Roughing time is mostly a volume problem. Work out how much material comes off (the stock volume minus the part volume; a 3D model gives you the part volume), then divide by how fast the tool removes it. Sandvik Coromant’s inch formulas for milling give the pieces [1]:

  • Spindle speed: n = vc × 12 / (π × D), with cutting speed vc in ft/min and tool diameter D in inches.
  • Table feed: vf = fz × n × zc, with feed per tooth fz and zc effective teeth, in in/min.
  • Metal removal rate: Q = ap × ae × vf, with axial depth ap and radial width ae in inches, in in³/min.

Take cutting speed and feed per tooth from your tool supplier’s data for the material, and the depths from how you actually run that tool. Then derate it. The formula gives the rate while the tool is fully in the cut; real roughing also spends time on ramps, corners, lighter stepdowns and air. An efficiency factor of 60 to 70% is a reasonable starting assumption until your own jobs tell you better.

Finishing passes, holes and turning

Finishing is a length problem, not a volume problem: time is toolpath length divided by feed. For a wall finished in one full-depth pass, the length is the wall’s perimeter. For a floor, it is the area divided by the stepover. Count spring passes and multiple depths if you run them.

For a drilled hole, the feed rate is feed per revolution times spindle speed, so the time is the depth (plus approach and breakthrough) divided by that rate. Pecking adds retract time on deep holes; tapping and reaming add their own passes.

On a lathe, Sandvik gives machining time directly as Tc = lm / (fn × n): machined length divided by feed per revolution times spindle speed [2]. A 2 in long pass on a 1 in diameter at 500 ft/min runs at about 1,910 rpm; at 0.008 in/rev that is 2 / (0.008 × 1,910) = 0.13 minutes per pass. Multiply by the number of passes, and remember that the spindle speed rises as the diameter gets smaller, up to the machine’s limit.

The minutes that aren’t cutting

On small aluminum parts, the time the tool isn’t cutting can match the time it is. Count it on purpose:

  • Tool changes: the number of tools times the chip-to-chip time. Time it on your own machine; the brochure figure is usually the best case.
  • Rapids, approach and retract: an allowance on top of cutting time, such as 10%, until you have programs to compare.
  • Load and unload: opening the vise, blowing off chips, seating the part, closing the door, for every operation. Time a few with a stopwatch.
  • In-process inspection: the minutes for a check times how often you check, spread over the parts. Three minutes every fifth part is 0.6 minutes a piece.
  • Deburring and bench work: usually at a lower rate than spindle time, so keep it on its own line.

A worked example: a 6061 housing

A 6061-T6 housing, finished 4.00 × 3.00 × 1.00 in, with a 2.50 × 1.75 × 0.75 in deep pocket and four 1/4 in through holes. It runs in two operations from a 4.25 × 3.25 × 1.25 in blank. Every cutting value below is an illustration; use your own tool data and your own timed handling.

  • Roughing: 1/2 in 3-flute carbide end mill at 800 ft/min: n = 800 × 12 / (π × 0.5) = 6,112 rpm, about 6,100. At 0.004 in per tooth, vf = 0.004 × 6,100 × 3 = 73.2 in/min. At 0.5 in deep and 0.2 in wide, Q = 0.5 × 0.2 × 73.2 = 7.32 in³/min.
  • Volume to remove: the blank is 17.27 in³ and the envelope 12.00 in³, so 5.27 in³ comes off the outside; the pocket is 3.28 in³. Together, about 8.55 in³.
  • Drilling: 1/4 in drill at 300 ft/min is about 4,580 rpm; at 0.005 in/rev that is 22.9 in/min, and each hole is 1.15 in of travel with approach and breakthrough.
Run time per piece, 6061-T6 housing (illustrative)
ElementHow it’s worked outMinutes
Roughing8.55 / 7.32 in³/min, at 65% efficiency1.80
Finish walls22.5 in of wall at 60 in/min0.38
Finish pocket floor and topArea divided by stepover, at 60 in/min0.49
Drill four holes4 × 1.15 / 22.90.20
Spot drill and chamferFrom path length0.30
Tool changes8 changes × 6 seconds0.80
Rapids and approach10% of 3.17 minutes of cutting0.32
Load and unload2 operations × 0.75 minutes1.50
Machine time per piece5.79
DeburrAt the bench1.50
In-process inspection3 minutes every 5th part0.60
Total per piece7.89
Setup per lot: programming 1.5 h, operation 1 setup 0.75 h, operation 2 setup 0.5 h, first-article inspection 0.5 h; 3.25 hours in all.

Now put the lot together. Setup is 195 minutes whatever the quantity:

Time per piece at three quantities (illustrative)
QuantitySetup + run timeTotal hoursMinutes per piece
1195 + 7.893.38202.9
10195 + 78.94.5727.4
50195 + 394.59.8311.8
Price machine time and bench time at their own rates; they are added together here only to show the shape.

The table shows where to spend your estimating effort. At 1 or 10 pieces, setup is most of the time, so a careful setup estimate matters more than a careful roughing estimate. At 50 pieces, a roughing estimate that is 50% optimistic adds 0.9 minutes a piece, or 45 minutes across the order: that is the point where programming the part to get a real cycle time pays for itself.

Calibrate against your own jobs

The efficiency factor, the handling minutes and the tool-change time are all assumptions until your own jobs confirm them. Estimates also tend to miss in one direction on one kind of work. One shop owner put it well: “I’m hitting really good numbers on lathe work … It’s mill work that I’m missing on” [4].

The fix is to record actual time against quoted time on finished jobs. Asked whether they compare the two, one experienced machinist answered “Always track and compare” [6]. After a dozen jobs you will know your real roughing efficiency, and your next estimate will start from your shop’s numbers instead of a rule of thumb.

From minutes to a price

Once you have setup hours and run minutes per piece, the quantity break calculator turns them into a price for each break, with the setup spread across each one. If you don’t have a rate to multiply by yet, start with the shop rate calculator. The rest of the quote, from reading the print to the final review, is in how to quote CNC machining jobs.

Machining time in QuoteSooner

In QuoteSooner’s worksheet you enter each operation with its setup and run time, and they are priced at the rates you set, with setup spread across every quantity break. When a 3D model comes with the request, an optional starting price works from the part’s geometry and your rates; its run time is refitted each week to the prices you actually sent, and by default it only fills in once it has come within 30% of five of your sent quotes. You can set it to always or never. The estimator approves every price. See how it works.

The free plan covers 5 RFQs a month for one user, with no card: start free.

Questions

How do you estimate CNC machining time?
Separate setup (once per lot) from run time (every piece). Estimate roughing as material volume divided by a derated metal removal rate, finishing as toolpath length divided by feed, and holes as depth divided by feed per revolution times rpm. Then add tool changes, rapids, load and unload, inspection and deburring.
What is the formula for metal removal rate in milling?
In inch units, Q = ap × ae × vf: axial depth times radial width times table feed, in in³/min. Table feed is vf = fz × n × zc, and spindle speed is n = vc × 12 / (π × D) [1].
How do you calculate turning time?
Machining time is Tc = lm / (fn × n): the machined length divided by feed per revolution times spindle speed, for each pass [2]. Multiply by the number of passes and add the non-cutting time.
How much should I add for non-cutting time?
Measure it rather than guess. Time tool changes chip to chip and time loading and unloading on your own machines. Until you have programs to compare, an allowance of about 10% of cutting time for rapids and approach is a reasonable start.
When is it worth programming the part in CAM to quote it?
When run time decides the price: higher quantities, long cycle times, or complex 3D surfaces. At low quantities setup dominates, and a formula-based estimate with a careful setup estimate is usually enough [3].

Sources

Facts about other products come from their own websites, read on the dates shown. If something has changed, tell us at hello@quotesooner.com and we will correct it.

  1. Sandvik Coromant: Formulas and definitions for milling, inch read October 30, 2026
  2. Sandvik Coromant: Formulas and definitions for turning, inch read October 30, 2026
  3. Practical Machinist: Quoting issues (2019) read October 3, 2026
  4. Practical Machinist: Quoting work, how do you do it? (2011) read October 3, 2026
  5. Practical Machinist: Methods to expedite quoting (2020) read October 3, 2026
  6. Practical Machinist: How many shops track actual hours vs. the bid price? (2026) read October 3, 2026

Put it into practice on your next RFQ.