CustomPartNet
·
August 21, 2026
·
Updated August 21, 2026
Every machining operation starts with two numbers that determine whether a job goes smoothly or ends in a snapped tool: spindle speed and feed rate. Get them wrong and you either burn through cutters chasing an unrealistic surface speed or leave money on the table running too conservatively. CustomPartNet's Speed and Feed Calculators solve this for three of the most common machining operations, milling, turning, and drilling, by converting the cutting speed a material and tool combination can handle into the actual RPM and feed rate a machinist or CAM programmer needs to set.
These widgets are meant for engineers sourcing parts who want to sanity check a supplier's quoted cycle time, students learning the relationship between cutting speed and rotational speed, and shop-floor programmers who need a fast second opinion before committing a program to the machine. Each calculator lives at CustomPartNet's Widgets section and takes the guesswork out of a calculation that is simple in theory but easy to get wrong in practice.
Milling, turning, and drilling are different operations, but they share the same underlying physics. A cutting edge has to move across the workpiece at a speed appropriate for the material being cut, expressed as surface feet per minute (SFM). Because the cutting edge is mounted on something that rotates, either the tool in milling and drilling or the workpiece in turning, that surface speed has to be translated into a rotational speed based on the diameter involved. Once RPM is known, feed rate follows from how far the cutting edge advances with each revolution or each tooth engagement.
That relationship is expressed as:
RPM = (12 × SFM) ÷ (π × D)
where D is the diameter in inches, either the tool diameter for milling and drilling or the workpiece diameter for turning. From there, feed rate depends on the operation. Milling multiplies RPM by the number of teeth on the cutter and the feed per tooth. Turning and drilling multiply RPM by the feed per revolution. Once feed rate (IPM) is known, cutting time for a given pass length is simply length divided by IPM.
It is important to note that these are simplified models meant to be a rule of thumb when setting cutting parameters. They do not take into account factors like tool wear, chatter, or tool/workpiece rigidity, which can all have a significant impact on the outcome. The results here should be used as a starting point or sanity check.
This widget determines spindle speed and feed rate for milling operations, where a rotating multi-tooth cutter, such as an end mill or face mill, is fed into a stationary workpiece.
Inputs:
Tool diameter
Number of teeth on the cutter
Cutting speed (SFM), based on the workpiece and tool material combination
Feed per tooth
Outputs:
Spindle speed (RPM)
Feed rate (IPM)
Cut time for a specified cut length
Turning reverses the setup: the workpiece rotates in a lathe chuck while a single-point tool feeds along its length or face. Because turned parts often step down in diameter, the calculator is typically run once per diameter along the part, since RPM has to change to hold a constant surface speed as diameter changes.
Inputs:
Cut diameter (the workpiece diameter at the point of the cut)
Cutting speed (SFM)
Feed per revolution
Outputs:
Spindle speed (RPM)
Feed rate (IPM)
Cut time for a specified cut length
Drilling shares its math with milling but applies it to a single axial cutting operation. A twist drill or similar tool rotates and feeds straight into the workpiece to produce a hole equal in diameter to the tool.
Inputs:
Tool (drill) diameter
Cutting speed (SFM)
Feed per revolution
Outputs:
Spindle speed (RPM)
Feed rate (IPM)
Cut time for a specified hole depth
Milling example. Consider a 0.5 inch diameter, 4-flute carbide end mill cutting 6061 aluminum at a cutting speed of 800 SFM with a feed of 0.005 inches per tooth.
RPM = (12 × 800) ÷ (π × 0.5) ≈ 6,112 RPM
Feed rate = 6,112 × 4 × 0.005 ≈ 122 IPM
For a 6 inch pass, cut time works out to roughly 3 seconds, which is why aluminum roughing passes look almost instantaneous compared to steel.
Turning example. Now take a 2 inch diameter 1018 steel bar turned with a carbide insert at 350 SFM and a feed of 0.008 inches per revolution.
RPM = (12 × 350) ÷ (π × 2) ≈ 668 RPM
Feed rate = 668 × 0.008 ≈ 5.3 IPM
A 4 inch facing or turning pass at that feed rate takes about 45 seconds, a useful number for estimating cycle time on a quoted part.
Drilling example. Finally, a 0.375 inch drill boring aluminum at 300 SFM with a feed of 0.006 inches per revolution.
RPM = (12 × 300) ÷ (π × 0.375) ≈ 3,056 RPM
Feed rate = 3,056 × 0.006 ≈ 18.3 IPM
A 1 inch deep hole at that feed rate takes only a few seconds, though real-world cycle time should also account for peck cycles and retraction on deeper holes.
Job shops quoting new work who need a quick check on realistic cycle times before committing to a price
CAM programmers validating that a post-processed program's feeds and speeds match the tool and material on the job traveler
Engineering students and new machinists learning why SFM stays constant while RPM changes with tool or workpiece diameter
Buyers evaluating a supplier's quoted machining time against an independent estimate for the same operation
Toolmakers troubleshooting excessive tool wear or poor surface finish by checking whether the running parameters match the material's recommended cutting speed
Why does RPM change when the tool diameter changes but SFM stays the same?
Surface speed depends on how fast a point on the tool's circumference is moving, which is a function of both rotational speed and diameter. A larger diameter tool covers more distance per revolution, so it needs a lower RPM to hit the same SFM as a smaller tool.
How do I know what cutting speed to use for my material?
Recommended SFM values are typically published by tooling manufacturers and vary based on the workpiece material, tool material (HSS versus carbide), and whether the operation is roughing or finishing. Softer materials like aluminum tolerate much higher SFM than harder alloys like titanium or hardened steel.
Why does turning require recalculating RPM at different diameters?
Because the workpiece itself is rotating, cutting speed depends on whatever diameter is currently being cut. As a part steps down in a facing or turning operation, the diameter shrinks, so RPM has to increase to hold the same surface speed, unless the machine is running in constant surface speed (CSS) mode.
What happens if feed rate is set too low?
A feed that is too light in relation to cutting speed causes the tool to rub rather than cut cleanly, generating excess heat and accelerating wear. This is a common cause of premature tool failure that looks like a speed problem but is actually a feed problem.
Do these calculators account for tool deflection or machine rigidity?
No. They calculate the theoretical RPM and feed rate based on cutting speed and tool geometry. Actual achievable parameters may need to be adjusted downward for long tool overhangs, thin-walled workpieces, or less rigid machine setups.
Can these calculators be used for CNC swiss-type or multi-axis machines?
The underlying speed and feed math applies to any rotating cutting operation, but complex multi-axis toolpaths may involve simultaneous moves that change effective engagement, so these results should be treated as a starting reference rather than a final program value.
Whether you are validating cycle time on a quote or scoping a new machining program, CustomPartNet can help you take the next step. Get a fast machining cost estimate or connect directly with qualified CNC suppliers.
Get a Machining Cost Estimate → or Register for a Free Account → to build supplier shortlists and manage RFQs.