Home / Manufacturing Processes / Cutting Speed, RPM & Feed Rate Calculator
Manufacturing Process Engineering
Cutting Speed, RPM & Feed Rate Calculator
In short: spindle speed is N = k·Vc/(πD), with k = 1000 in metric and 12 in imperial, and the feed rate is f·N in turning or fz·z·N in milling. Enter your cutting speed and diameter below, in metric or imperial, and this tool returns the spindle RPM and feed rate — or works in reverse to find the cutting speed from a known RPM, and checks the result against your machine limit.
Cutting speed, spindle RPM and feed rate
N = k·Vc / (πD) · Vc = πD·N / k · feed Vf = f·N (turning) or fz·z·N (milling)
Spindle speed
764 rpm
Starting values only — always confirm against your tool maker’s data.
What this calculator computes
This tool converts a recommended cutting speed into the two numbers a machine actually needs: the spindle speed in revolutions per minute and the feed rate the tool advances at. It is the first calculation of any machining setup, the step that turns a surface speed from a tool catalogue into a value you can dial into the control.
It works for turning, drilling, and milling, in metric or imperial units, and it runs in both directions, finding the RPM from a cutting speed or the cutting speed from a known RPM.
When you supply the feed, it also returns the table feed rate, and when you supply your machine’s maximum spindle speed, it tells you whether the tool can run at its recommended speed at all.
The reason this conversion matters so much is that cutting speed and spindle speed are different quantities that people often confuse. Cutting speed is a property of the tool and material, the speed at which the cutting edge should travel through the metal for good tool life and finish; it is fixed for a given pairing. Spindle speed depends on the diameter as well, because the same surface speed needs more revolutions on a small tool and fewer on a large one. Getting from one to the other correctly, through the actual diameter and the right unit constant, is the foundation of every downstream number, from feed rate to machining time to the cost of the part.
What sets this calculator apart is that it combines four things most free tools separate: a bidirectional RPM and cutting-speed conversion, a feed-rate calculation for both turning and milling, a live check against a machine speed limit, and a built-in material starting-speed and chip-load reference so you have a number to enter in the first place. Everything runs in your browser, with a chart of how the RPM changes across diameters and export to PDF or CSV, and nothing you type is stored.
How to use this calculator, step by step
Begin by choosing the operation, the unit system, and the direction. Pick turning or drilling for a rotating workpiece or drill and milling for a rotating multi-tooth cutter; choose metric, with millimetres and metres per minute, or imperial, with inches and surface feet per minute; and choose whether to solve for the RPM from a cutting speed, the usual case, or for the cutting speed from a known RPM, which is useful for checking an existing program. The input fields adapt to your choices: turning asks for a feed per revolution, milling asks for a tooth count and a feed per tooth, and an optional field lets you enter your machine’s maximum spindle speed.
Then enter the cutting parameters. The cutting speed comes from your tool maker’s recommendation for the material, and if you do not have one, the reference table further down gives typical starting values by material and tool type. The diameter is the workpiece diameter in turning or the cutter diameter in milling. The feed comes from the tool data too, as a feed per revolution for turning or a chip load per tooth for milling. The calculator opens on a worked turning example, 120 metres per minute on a 50 mm diameter at 0.2 mm per revolution, so you see a full result at once, and every field recomputes live as you type.
The result panel leads with the spindle speed, then lists the cutting speed in both unit systems, the feed rate in distance per minute, and the feed per revolution. If you entered a machine maximum and the required RPM exceeds it, a highlighted note tells you the speed has been capped and shows the reduced cutting speed you will actually achieve. The chart plots how the RPM must change across a range of diameters to hold your cutting speed constant, which makes the diameter dependence concrete, and you can download or share the setup locally.
Cutting speed and spindle speed: the core conversion
The heart of this calculator is the relation between cutting speed and spindle speed, and it is worth understanding rather than just applying. Cutting speed is defined as the linear speed of the cutting edge relative to the workpiece surface.
In one revolution, the edge travels the circumference of the cut, which is pi times the diameter; multiplied by the number of revolutions per minute, that gives the surface speed. Rearranging to solve for the revolutions gives spindle speed equal to cutting speed divided by pi times the diameter.
Because cutting speed is quoted in metres per minute against a diameter in millimetres, a factor of 1000 converts metres to millimetres, giving the metric working form, RPM equals 1000 times cutting speed divided by pi times diameter.
In imperial units the logic is identical but the unit factor changes. Cutting speed is quoted in surface feet per minute against a diameter in inches, so a factor of 12 converts feet to inches, giving RPM equals 12 times surface feet per minute divided by pi times diameter. Machinists often use the simplified constant form, RPM equals 3.82 times surface feet per minute divided by the diameter in inches, where 3.82 is simply 12 divided by pi. The two forms give the same answer; the simplified one is convenient for mental arithmetic on the shop floor, and the calculator uses the exact form internally so there is no rounding loss.
The practical consequence of the diameter in the denominator is the single most important intuition in speeds and feeds: for a fixed cutting speed, RPM is inversely proportional to diameter. Halve the diameter and you must double the RPM to keep the same surface speed. This is why a small drill or a slot-drilling end mill spins so fast, why a large face mill turns slowly, and why the same recommended cutting speed produces wildly different spindle speeds across a job. The chart on this page draws exactly this inverse curve, and the machine-limit check exists because on small diameters the required RPM can climb past what the spindle can deliver.
Calculating the feed rate
Once the spindle speed is known, the feed rate follows, and this is where turning and milling diverge. Feed rate is the distance the tool advances per minute, the value the machine control is actually programmed with, sometimes called the table feed in milling. In turning and drilling, the feed is specified per revolution of the workpiece or drill, so the feed rate is simply the feed per revolution multiplied by the spindle speed. A cut at 0.2 mm per revolution turning at 764 rpm advances at about 153 mm per minute. The feed per revolution is a direct, intuitive parameter in turning, and it is what the calculator asks for.
In milling the feed is specified per tooth, because a milling cutter has several cutting edges and each takes a chip once per revolution. The fundamental parameter is the chip load, the feed per tooth, and to get the feed per revolution you multiply by the number of teeth; to get the feed per minute you multiply again by the spindle speed.
So the milling feed rate is the feed per tooth times the number of teeth times the RPM. This is why a cutter with more flutes, at the same chip load and speed, feeds faster: an eight-flute cutter feeds twice as fast as a four-flute one at the same chip load.
The calculator asks for the tooth count and the chip load in milling and carries them through to the table feed.
The chip load itself is worth care, because both extremes cause trouble. Too small a chip load makes the edge rub and burnish rather than cut, generating heat, work-hardening the surface of alloys like stainless steel, and wearing the tool quickly. Too large a chip load overloads the edge and risks chipping or breaking it. The tool maker’s recommended chip load, typically a few thousandths of an inch or a few hundredths of a millimetre depending on the tool size and material, is the value to enter, and the reference table below lists typical starting ranges. The feed rate the calculator returns is the number you program; the chip load is the parameter you tune.
Recommended cutting speed and chip load by material
Cutting speed depends on the tool and material pairing and is published by the tool maker, but a starting-value table is invaluable when you are setting up quickly or sanity-checking a recommendation. The values below are typical carbide starting points for general machining; high-speed-steel tools run at roughly 40 to 50 percent of these speeds, and modern coated carbide can run 20 to 50 percent faster. Treat them as a first estimate to enter into the calculator, then refine against the specific tool data and your machine.
| Material | Cutting speed (m/min) | Cutting speed (SFM) | Chip load, ~6 mm (1/4″) tool |
|---|---|---|---|
| Aluminium 6061 / 7075 | 240–450 | 800–1500 | 0.05–0.10 mm (0.002–0.004″) |
| Brass / bronze | 150–300 | 500–1000 | 0.05–0.10 mm (0.002–0.004″) |
| Mild steel 1018 | 90–120 | 300–400 | 0.05–0.08 mm (0.002–0.003″) |
| Alloy steel 4140 | 75–110 | 250–360 | 0.04–0.08 mm (0.0015–0.003″) |
| Stainless 304 / 316 | 60–90 | 200–300 | 0.04–0.06 mm (0.0015–0.0025″) |
| Cast iron | 60–120 | 200–400 | 0.05–0.10 mm (0.002–0.004″) |
| Titanium alloy | 30–60 | 100–200 | 0.03–0.05 mm (0.001–0.002″) |
Two adjustments matter when reading the table. First, tool material and coating scale the whole row: an uncoated HSS end mill in mild steel runs near the bottom of the range or below, while a coated carbide insert can run above the top. Second, the operation matters: a light finishing pass tolerates a higher speed than a heavy roughing cut, and an interrupted cut or a deep pocket calls for a more conservative value. The table gets you a defensible starting number; the calculator turns it into RPM and feed; and a test cut, watching chip colour, sound, and finish, confirms it.
Checking against the machine speed limit
A recommended cutting speed is only useful if the machine can actually deliver the RPM it implies, and on small diameters it often cannot. Because RPM is inversely proportional to diameter, a small end mill or drill at a normal cutting speed can demand tens of thousands of revolutions per minute, well beyond a general-purpose machine’s spindle. A 6 mm cutter in aluminium at 300 metres per minute, for instance, needs nearly 16,000 rpm, which many mills cannot reach. When that happens, you cannot run the recommended surface speed; you run the machine flat out and accept a lower cutting speed.
The optional machine-maximum field makes this explicit. Enter your spindle’s top speed and the calculator compares it with the RPM your cutting speed requires. If the requirement is within the limit, nothing changes and the RPM is reported normally. If the requirement exceeds the limit, the calculator caps the RPM at the machine maximum and recomputes the cutting speed you will actually achieve at that ceiling, showing it in a highlighted note. This tells you at a glance whether the tool is being run at its intended speed and, if not, how much you are giving up, which affects tool life and finish and may argue for a smaller step-over, a different tool, or a higher-speed spindle.
Five worked examples you can follow
Example 1: the default turning conversion
The calculator opens on a turning cut at 120 metres per minute on a 50 mm diameter, feeding at 0.2 mm per revolution. The spindle speed is about 764 rpm, the cutting speed reads 120 m/min (about 394 SFM), and the feed rate is about 153 mm per minute. This is the complete first step of the setup, surface speed turned into machine settings.
Example 2: a small milling cutter
Switch to milling and enter 200 metres per minute on a 20 mm four-flute cutter at 0.05 mm per tooth. The spindle speed is about 3183 rpm and the feed rate is about 637 mm per minute (0.05 times 4 times 3183). Note that the feed rate would double with an eight-flute cutter at the same chip load and speed.
Example 3: working in imperial
Change the units to imperial and enter 300 surface feet per minute on a 0.5 inch diameter turning at 0.005 inch per revolution. The spindle speed is about 2292 rpm and the feed rate is about 11.5 inches per minute. The result strip also shows the cutting speed as about 91 metres per minute, so you can cross-check a metric catalogue.
Example 4: hitting the machine limit
Enter a turning cut at 300 metres per minute on a 10 mm diameter and set the machine maximum to 4000 rpm. The required RPM is about 9549, well over the limit, so the calculator caps it at 4000 and reports the achievable cutting speed as about 126 metres per minute. You now know the tool cannot run at its recommended speed on this machine.
Example 5: reverse solving for cutting speed
Switch the direction to solve for cutting speed and enter an existing program’s 764 rpm on a 50 mm diameter. The calculator returns a cutting speed of about 120 metres per minute, letting you check whether an inherited program is running the tool at a sensible surface speed for the material.
Three expert tips for reliable results
Convert through the real diameter
Never enter cutting speed as if it were RPM. Always convert through the actual tool or part diameter; the same surface speed gives very different RPM on a small drill and a large mill.
Match the feed to the operation
Turning feed is per revolution; milling feed is per tooth and must be multiplied by the tooth count. Entering a per-revolution value in milling badly understates the feed rate.
Check the spindle limit on small tools
Small diameters demand high RPM. Enter your machine maximum to see whether you can reach the recommended cutting speed, or how much surface speed you lose at the ceiling.
The mathematics behind the results
The spindle-speed formula comes straight from the definition of cutting speed. The surface speed at the cutting edge is the distance the edge travels per minute, which is the circumference of the cut, pi times the diameter, times the rotational speed in revolutions per minute.
Setting that equal to the cutting speed and solving for the rotational speed gives RPM equals cutting speed divided by pi times diameter. The unit constant then reconciles the mixed units in which the quantities are conventionally quoted: 1000 to convert metres to millimetres in metric, or 12 to convert feet to inches in imperial.
The reverse form, cutting speed equals pi times diameter times RPM divided by the same constant, simply inverts the relation and is what the calculator uses when you solve for cutting speed.
The feed-rate formulas follow from the definition of feed. In turning, feed per revolution is the advance in one revolution, so the advance per minute is that value times the revolutions per minute.
In milling, the chip load is the advance per tooth, and since each of the several teeth cuts once per revolution, the advance per revolution is the chip load times the tooth count, and the advance per minute is that times the RPM.
The feed per revolution the calculator reports for milling is the chip load times the tooth count, which lets you compare a milling setup directly with a turning one. The surface-speed conversion between metric and imperial in the result strip is the exact factor, one foot equal to 0.3048 metres.
These relations are exact for the idealised geometry, and their assumptions are worth stating.
The diameter used is the effective cutting diameter: the full tool diameter for a slot or a turned bar, but for some milling geometries, such as a ball nose cutting at shallow depth or a chamfer, the effective diameter is smaller than the nominal one, and using the nominal diameter overstates the cutting speed.
The calculator computes with the diameter you enter, so for those cases you enter the effective diameter. The feed rate is likewise the nominal programmed feed; chip thinning at low radial engagement means the actual chip is thinner than the nominal chip load, which is a refinement layered on top of the basic calculation rather than a change to it.
Where cutting speed calculations fit in the workflow
This conversion is the entry point to the whole speeds-and-feeds workflow, and it connects directly to the other tools in this silo.
The RPM and feed rate it produces are the inputs the machining time and MRR calculator needs to work out how long a cut takes and how fast metal comes off; in fact that tool performs the same surface-speed-to-RPM step internally before computing time and removal rate.
The cutting speed you set here is also the variable the tool life calculation trades against wear: a higher cutting speed shortens the machining time but shortens tool life faster, and the economic cutting speed balances the two. Seen this way, the cutting speed is the master parameter of a machining operation, and this calculator is where you choose it and translate it into machine settings.
In day-to-day work the calculation is used at the setup sheet and the CNC program. A process planner writing a setup sheet lists the RPM and feed for each tool, derived from the catalogue cutting speed and the diameter exactly as this tool derives them.
A programmer entering speeds and feeds into a CAM system or typing them at the control does the same conversion, and checking it against the machine’s spindle limit avoids programming a speed the machine cannot reach.
An apprentice or a machinist verifying an inherited program uses the reverse direction to see whether the RPM in the program corresponds to a sensible cutting speed for the material. In every case the calculation is small but foundational, and getting it wrong propagates into scrapped parts, broken tools, and poor finish.
Beyond the individual operation, cutting speed sits at the centre of manufacturing process engineering. It links to tooling selection, since the achievable speed is what justifies a more expensive coated or ceramic tool; to machine selection, since high-speed work needs a spindle that can turn fast enough on small diameters; and to cost estimating, since the speed drives the cycle time that a quote is built on. Return to the Manufacturing Processes hub for the companion calculators that take these speeds and feeds forward into machining time, tool life, and the forming and molding calculations that complete the silo.
Turning, drilling and milling: one conversion, different diameters
The three common cutting operations share the surface-speed-to-RPM conversion but differ in which diameter and which feed to use, and keeping them straight avoids the commonest setup errors. In turning, the workpiece rotates and the diameter in the formula is the diameter of the workpiece at the cut, which shrinks as material is removed; strictly the cutting speed rises slightly as the diameter falls at constant RPM, though for a single pass the change is small. The feed is per revolution of the workpiece. Drilling follows the same pattern: the diameter is the drill diameter and the feed is per revolution of the drill, so a drill is entered exactly like a turning cut.
In milling the tool rotates and the diameter in the formula is the cutter diameter, which is fixed for the operation, and the feed is per tooth, requiring the tooth count to reach the table feed.
The distinction that trips people up is the feed: a milling program needs a table feed in distance per minute, but the tool catalogue gives a chip load per tooth, and the multiplication by teeth and RPM is where errors creep in. The calculator removes that risk by asking for the chip load and tooth count and returning the table feed directly.
Whichever operation you choose, the RPM comes from the same relation, and only the diameter you enter and the feed form change, which is why one calculator serves all three.
Constant surface speed on CNC lathes
On a lathe the workpiece diameter changes across a facing cut or between features, and because RPM at a fixed setting would then give a changing surface speed, CNC lathes offer a constant-surface-speed mode. In this mode you program the cutting speed directly, in metres per minute or surface feet per minute, and the control continuously adjusts the spindle RPM as the diameter changes so the surface speed at the cutting edge stays constant. As the tool moves toward the centre on a facing cut, the diameter falls and the control raises the RPM, which is why a facing cut speeds up as it approaches the axis and why the control needs an RPM clamp to avoid runaway speed at the very centre.
This calculator computes the RPM for a single, definite diameter, which is exactly what you need for a turning pass at a fixed diameter, for setting the RPM clamp in constant-surface-speed mode, or for a milling or drilling operation where the diameter is fixed. To see how the RPM must vary across a range of diameters at your chosen cutting speed, read the chart on this page: it is the same inverse relationship the constant-surface-speed control applies automatically, drawn out so you can see how steeply the required RPM climbs as the diameter shrinks. The clamp you set on the machine is simply the point on that curve where the spindle reaches its limit.
Common mistakes to avoid
A handful of errors account for most bad speeds-and-feeds calculations. Watch for them.
- Entering cutting speed as spindle speed. They are different quantities; RPM depends on the diameter. Always convert through the actual diameter rather than typing a surface speed into an RPM field.
- Mixing units. A metric cutting speed with an imperial diameter, or feet with millimetres, corrupts the RPM. Set the unit switch and keep every input in one system; use the dual-unit result strip to cross-check catalogues.
- Using per-revolution feed in milling. Milling feed is per tooth; multiply by the tooth count and RPM for the table feed. A per-revolution value understates the feed by the number of teeth.
- Ignoring the machine speed limit. Small tools demand high RPM that many machines cannot reach; running below the recommended cutting speed changes tool life and finish. Check the requirement against your spindle maximum.
- Using the nominal diameter for shallow ball-nose or chamfer cuts. The effective cutting diameter is smaller, so the true cutting speed is lower than the nominal figure; enter the effective diameter for those geometries.
- Running too light a chip load. Below the tool’s minimum, the edge rubs instead of cutting, generating heat and work-hardening; a chip load that is too small is as damaging as one that is too large.
Input format and quick reference
Choose the operation, unit system, and direction, then enter the cutting speed (or RPM), the diameter, and the feed; milling also needs the tooth count. The reference below explains each output.
| Output | What it means |
|---|---|
| Spindle speed (rpm) | How fast the machine turns, from cutting speed and diameter: k·Vc/(πD) |
| Cutting speed | The surface speed at the edge, shown in both m/min and SFM for cross-checking |
| Feed rate | Distance the tool advances per minute; f·N in turning, fz·z·N in milling — the value you program |
| Feed per revolution | Advance per revolution; the chip load times the tooth count in milling |
Frequently asked questions
How do I calculate RPM from cutting speed?
Spindle speed in revolutions per minute is the cutting speed divided by the circumference of the tool or part, which is pi times the diameter.
Because cutting speed is quoted as a surface speed, a unit factor converts it to revolutions: in metric the formula is RPM = 1000 times the cutting speed in metres per minute divided by pi times the diameter in millimetres, and in imperial it is RPM = 12 times the surface feet per minute divided by pi times the diameter in inches, which is often simplified to RPM = 3.82 times SFM divided by the diameter in inches.
For example, a cutting speed of 120 metres per minute on a 50 mm diameter gives about 764 rpm. This calculator does the conversion for both unit systems and for both turning and milling, and it also runs the calculation in reverse to find the cutting speed from a known RPM.
What is the difference between cutting speed and spindle speed?
Cutting speed is the speed of the cutting edge relative to the workpiece surface, measured in metres per minute or surface feet per minute, and it is the value you look up in a tool catalogue for a given tool and material.
Spindle speed, in revolutions per minute, is how fast the machine actually turns, and it is not the same number, because a given surface speed needs a high rotational speed on a small diameter and a low one on a large diameter. The two are joined by the diameter: RPM equals a constant times the cutting speed divided by pi times the diameter.
This is why the same recommended cutting speed calls for very different RPM on a small drill and a large face mill, and why you must always convert through the actual diameter rather than entering one value for the other.
How do I calculate feed rate?
Feed rate is the distance the tool advances per minute, and it is what the machine control is programmed with. In turning, the feed is specified per revolution, so the feed rate is the feed per revolution times the spindle speed in revolutions per minute.
In milling, the feed is specified per tooth, the chip load each cutting edge should take, so the feed rate is the feed per tooth times the number of teeth times the spindle speed. A four-flute end mill at 0.05 mm per tooth turning at 3183 rpm feeds at 0.05 times 4 times 3183, about 637 mm per minute.
This calculator computes the feed rate from your feed setting, tooth count, and the spindle speed it has just derived from your cutting speed, so the whole chain from surface speed to programmed feed is done in one step.
What is chip load or feed per tooth?
Chip load, also called feed per tooth, is the thickness of material each cutting edge of a milling cutter removes as it passes through the work, and it is the fundamental feed parameter the tool maker recommends for a material.
It matters because too small a chip load makes the tool rub instead of cut, which generates heat, work-hardens the surface, and wears the edge, while too large a chip load overloads the edge and can break it.
Typical starting values are around 0.002 to 0.004 inch per tooth on a quarter-inch cutter and 0.003 to 0.006 inch on a half-inch cutter, larger for aluminium and smaller for hard alloys. Multiplying the chip load by the number of teeth and the spindle speed gives the table feed rate the machine uses, which is exactly what this calculator does.
How do I convert SFM to metres per minute?
Surface feet per minute and surface metres per minute measure the same thing, the linear speed of the cutting edge, in different units, and the conversion is a straight factor: one foot is 0.3048 metres, so metres per minute equals surface feet per minute times 0.3048, and surface feet per minute equals metres per minute divided by 0.3048, or roughly times 3.28.
For instance, 300 surface feet per minute is about 91 metres per minute, and 100 metres per minute is about 328 surface feet per minute. This matters because tool catalogues from different regions quote cutting speed in different units, and mixing them corrupts the RPM.
This calculator shows the cutting speed in both units in its result strip so you can cross-check a recommendation regardless of which system the catalogue uses.
What cutting speed should I use for my material?
Cutting speed is a property of the tool and material pairing, and the tool maker publishes the recommended value; there is no single right number, because it depends on the tool material and coating, the workpiece alloy and hardness, the coolant, and the operation.
As a rough guide with carbide tooling, aluminium alloys such as 6061 run very fast, in the region of 240 to 450 metres per minute, mild steels such as 1018 run around 90 to 120 metres per minute, and stainless steels such as 304 run slower still, around 60 to 90 metres per minute; high-speed-steel tools run at roughly 40 to 50 percent of the carbide speeds, and coated carbide can go 20 to 50 percent faster.
Use the reference table on this page as a starting point, then confirm against the specific tool data, and enter the value into the calculator to get the RPM and feed.
Can this calculator check my machine speed limit?
Yes. Every machine has a maximum spindle speed, and on small diameters the RPM needed to reach a recommended cutting speed can exceed it. If you enter your machine maximum spindle speed, the calculator checks the required RPM against it: when the requirement is within the limit it reports the RPM as usual, and when the requirement exceeds the limit it caps the RPM at the machine maximum and reports the reduced cutting speed you will actually achieve at that ceiling. This tells you immediately whether your machine can run the tool at its recommended speed and, if not, how much surface speed you are giving up, which is a common constraint with small tools on general-purpose machines.
Does the calculator work for both turning and milling?
Yes. The RPM conversion is identical for both, since both depend on the cutting speed and the diameter, but the diameter and the feed differ. In turning the diameter is the workpiece diameter and the feed is per revolution; in milling the diameter is the cutter diameter and the feed is per tooth, multiplied by the number of teeth.
The calculator switches its feed inputs when you change the operation, asking for feed per revolution in turning and feed per tooth with a tooth count in milling, so each operation is entered in its natural terms while the underlying surface-speed-to-RPM conversion stays the same.
It also handles drilling, which follows the turning form with the drill diameter and a feed per revolution.
Does this calculator store the numbers I enter?
No. The calculator runs entirely in your browser. The cutting parameters and any other values you enter are never sent to our servers, stored, or shared. You can download a PDF or CSV of your results locally, and nothing leaves your device. See our Privacy Policy for details.
Is the cutting speed calculator free?
Yes. The cutting speed, RPM, and feed rate calculator is completely free, with no account, sign-up, or usage limit. It converts cutting speed to spindle RPM and back, computes the feed rate for turning and milling in metric or imperial units, checks the result against a machine speed limit, plots how RPM changes with diameter, and exports to PDF and CSV, all at no cost.
Related manufacturing process calculators
More tools in this silo. Return to the Manufacturing Processes hub for the full set.
Sources, disclaimer and editorial transparency
This calculator uses the standard machining relations: spindle speed N = k·Vc/(πD) with k = 1000 (metric) or 12 (imperial); the inverse Vc = πD·N/k; and feed rate Vf = f·N (turning) or fz·z·N (milling), consistent with standard machining-handbook practice. The material starting speeds and chip loads are typical published carbide ranges for general machining and are guidance only. This calculator and guide are created and reviewed by the OpsCalculators team; see our Editorial Policy for how each tool is researched, built, and tested.
Results are accurate estimates for planning, programming, and education, not a substitute for verified tool-maker data or a machine’s own limits. Achievable speeds and feeds depend on the machine, tool, coating, coolant, and material. See our full Disclaimer. OpsCalculators.com is operated by MAFHH INTERNATIONAL LTD. Your data is processed in your browser and never stored; see our Privacy Policy.