Drilling Feed Rate Calculator
Solve spindle RPM, feed rate, and material removal rate from drill diameter, cutting speed (SFM), and feed per revolution (IPR). Imperial and metric. The math is the same for HSS, solid carbide, and modular insert drills — what changes is the SFM and IPR you start with for your specific tool.
Drilling feed rate is how fast the drill advances into the workpiece, in inches or millimeters per minute. It is the product of spindle speed and feed per revolution: vf = N × fn. Spindle speed is set from the recommended cutting speed (SFM) and the drill diameter via N = (12 × V) / (π × D). Machinists also call this a drilling speeds and feeds calculator, a drilling feed and speed calculator, or a CNC feeds and speeds calculator for drilling — same math, just different names for the same kinematic relationship. Both SFM and IPR come from the tool manufacturer’s catalog for the specific drill, material, and coolant strategy.
This calculator does the math — it does not recommend feeds and speeds.
Recommended cutting speed (SFM) and feed per revolution (IPR) depend on the specific drill grade and geometry, the workpiece material, the coolant strategy, and the rigidity of your machine. The same hole drilled with HSS-Co versus solid carbide versus a modular insert drill with through-spindle coolant runs at vastly different SFM and IPR. Pull starting values from your tool manufacturer’s catalog or feed/speed app, then drop them into this calculator to get spindle RPM and feed rate.
Reduce starting values when conditions are less favorable: low spindle horsepower, long tool stick-out, light fixturing, deep through-holes without TSC, or drilling stainless and exotic alloys at the high end of their hardness range. Listen to the cut — chatter, squeal or howl, and chips welding to the drill or packing in the flutes are reliable “too aggressive” or “losing chip evacuation” signals; bell-mouthed or oversized holes on inspection point to the same root cause. Chip color is more nuanced and tool-material dependent: on HSS, blue or purple chips mean the cutting edge is overheating and tool life will fall off fast — back the speed off. On carbide (especially with through-spindle coolant), blue or “steel-blue” chips are normal and often desirable, because the chip is carrying heat away from the tool rather than letting it accumulate in the cutting edge. Smoke is not a reliable indicator on its own — sulfurized cutting oils, common on manual lathes and drill presses, smoke during normal use.
Drilling Equations
Spindle Speed from Cutting Speed
N = (12 × V) / (π × D) (imperial: V in SFM, D in inches)
N = (1000 × V) / (π × D) (metric: V in m/min, D in mm)
N = spindle speed [revolutions / time] — e.g. RPM
V = cutting speed [length / time] — e.g. SFM (ft/min), m/min
D = drill diameter [length] — e.g. in, mm
π = 3.1416
Machinery’s Handbook 29th Ed., p. 1015 (Cutting Speed Formulas)
Feed Rate
vf = N × fn
vf = feed rate [length / time] — e.g. in/min, mm/min
N = spindle speed [revolutions / time] — e.g. RPM
fn = feed per revolution [length / revolution] — e.g. in/rev, mm/rev
Machinery’s Handbook 29th Ed., p. 1079 (variable definitions: f = feed in inches per revolution; fm = feed in inches per minute; fm = N × f)
Material Removal Rate
MRR = (π / 4) × D² × vf
MRR = material removal rate [volume / time] — e.g. in³/min, cm³/min, mm³/min
D = drill diameter [length]
vf = feed rate [length / time]
The hole cross-section is πD²/4 and the drill advances at vf, so volume removed per minute is the product. This is algebraically identical to the shorthand MRR = D · fn · vc · 3 published on Haas Tooling, Modular Drills Speeds and Feeds, Inch (page 2): substituting vf = N · fn and N = 12vc/(πD) into πD²/4 · vf, the π cancels and the constant simplifies to 12/4 = 3 (the 12 is in/ft converting SFM to in/min; the 4 is the denominator of πD²/4). Both forms produce the same in³/min result.
Feed per Tooth (Drills with Z > 1)
fz = fn / Z
fz = feed per tooth [length / tooth] — e.g. in/tooth, mm/tooth
Z = number of effective cutting edges (typically 2 for twist drills and most insert drills)
Drilling catalogs typically publish fn directly. Use this conversion only when your catalog gives per-tooth values.
How to Use This Calculator
Enter the drill diameter, the recommended cutting speed (SFM or m/min), and the recommended feed per revolution from your tool catalog. The calculator returns the spindle RPM you should program, the feed rate to use in your G94 cycle, the material removal rate, and the equivalent feed per tooth. To convert per-tooth (IPT) values from a milling-style catalog, enter the IPT directly in the feed-per-revolution field and update the flute count — or just multiply IPT by Z and use the IPR field.
For a deep hole — greater than three drill diameters — through-spindle coolant becomes the difference between a single-shot drill and a peck cycle. Haas Tooling’s Modular Drills speeds-and-feeds chart explicitly notes: “Through coolant is recommended for greater than 3XD applications.” If your machine has TSC, use the vendor’s TSC values; if not, derate to flood-coolant numbers and plan on pecking. To pair this with a chip-load check on the milling side, use our chip load calculator.
Drill Feed Rate Chart by Tool Material and Coolant Strategy
The math above is unit-agnostic and tool-agnostic. What changes across the common drilling setups is the cutting speed and feed per revolution you input. The values below are taken directly from Haas Tooling’s published speeds-and-feeds charts for low-carbon steel (ISO P1) wherever each chart covers it. Important: the four Haas charts cover different drill diameter ranges, so a same-diameter side-by-side isn’t possible from these PDFs alone — the diameter range each rung is calibrated for is shown beneath the SFM. Treat this as a tool-tier comparison, not a recommendation for your specific job.
(flood)
(flood)
(TSC)
(TSC)
Sources: Haas Cobalt Jobber Drill Sets Feeds and Speeds (P1 ~130 SFM, 0.05–0.24″); Haas Carbide Drills General Purpose (TSC) Speeds and Feeds, Inch (P2 non-alloy steel: 263 SFM at 0.04–0.08″, 362 SFM at 0.12–0.31″; chart caps at ~0.31″); Haas Modular Drills Speeds and Feeds, Inch (P1 low-carbon: 262/410/558 min/start/max SFM across 0.315–1.000″). The flood-only solid-carbide rung is qualitative because Haas Tooling doesn’t publish a flood-only carbide chart; 50–70% of TSC values is the conventional vendor derate (Sandvik Coromant CoroDrill, Kennametal B Series).
Cycle-time impact. Realistic apples-to-apples ratio: an HSS-Co jobber at 130 SFM and 0.005 in/rev versus a Modular insert at the 410-SFM start value and 0.009 in/rev (mid-range for ~0.47″ drills) is roughly a 5–6× feed-rate gain on top of the modular drill’s longer insert life and elimination of pecking on holes past 3×D. The exact ratio depends on diameter and depth; plug each row into the calculator above to see the difference for your part.
Where modular drills sit. A modular drill is a steel body with a carbide insert tip and integrated coolant channels for TSC. We run them at Pi Fabricators for production hole-making because they chatter less and produce truer holes with a better finish than carbide spade bits, and because we get many more holes out of an insert than out of a spade bit — a little more upfront cost, much better value over a production run.
Worked Example
Problem: Drill a 0.472″ (12 mm) hole in low-carbon steel using a Haas Modular insert drill with through-spindle coolant. From the Haas Modular Inch chart, ISO P1 (low-carbon, <125 HB) has a starting cutting speed of 410 SFM. The 0.472″ column lists a recommended feed range of 0.006–0.012 in/rev, so we’ll pick the mid-range 0.009 in/rev. Find the spindle RPM, feed rate, and MRR.
Given: D = 0.472″, V = 410 SFM, fn = 0.009 in/rev
Spindle speed: N = (12 × 410) / (π × 0.472) = 4920 / 1.4828 = 3318 RPM
Feed rate: vf = 3318 × 0.009 = 29.9 in/min (759 mm/min)
MRR: (π / 4) × 0.472² × 29.9 = 0.1750 × 29.9 = 5.23 in³/min (85.7 cm³/min)
An HSS-Co jobber would attack the same 12 mm hole at roughly 130 SFM and 0.005 in/rev: N = 12 × 130 / (π × 0.472) = 1052 RPM, vf = 1052 × 0.005 = 5.26 in/min — the modular drill is roughly 5.7× faster in cut. On production work with many holes, that compounds into hours of saved cycle time per shift, and the carbide insert lasts dramatically longer than the HSS drill bit.
Frequently Asked Questions
How do you calculate drilling feed rate?
Drilling feed rate is spindle speed times feed per revolution: vf = N × fn. Spindle speed comes from cutting speed and drill diameter: N = (12 × V) / (π × D) for V in SFM and D in inches, or N = (1000 × V) / (π × D) for V in m/min and D in mm. For example, a 1/2″ drill running 300 SFM at 0.010 in/rev needs N = 12 × 300 / (π × 0.5) = 2,292 RPM, giving a feed rate of 2,292 × 0.010 = 22.9 in/min. (Machinery’s Handbook 29th Ed., pp. 1015 and 1079.)
Why doesn’t this calculator recommend a feed rate or cutting speed?
Recommended cutting speed (SFM) and feed per revolution (IPR) depend on the specific tool you are running, the workpiece material, the coolant strategy, and the rigidity of your machine. An HSS-Co jobber drill in mild steel runs around 130 SFM at 0.005 in/rev (Haas Cobalt jobber chart); a Haas Modular insert drill with through-spindle coolant in low-carbon steel has a published min/start/max range of 262/410/558 SFM, with feeds of roughly 0.006–0.012 in/rev for ~0.47″ drills. That’s a roughly 5.7× faster cut rate from HSS to modular insert at comparable diameters (3× from higher SFM, another 1.8× from higher feed per revolution). The math is the same; only the inputs change. Pull SFM and IPR from your tool manufacturer’s catalog or feed/speed app, then drop them into this calculator to get spindle RPM and feed rate.
Can I run carbide drills faster than HSS?
Yes — roughly 2 to 3 times faster in steel at comparable conditions. Cobalt HSS drills (Haas’s HSS-Co jobber sets, for example) are tabulated at conservative speeds appropriate for the heat tolerance of high-speed steel. Solid carbide drills with through-spindle coolant tolerate much higher cutting temperatures and clear chips actively, so vendors publish much higher SFM. Concrete numbers from Haas Tooling’s own published charts: in low-carbon steel (ISO P1), Haas’s Cobalt jobber set is tabulated at roughly 130 SFM (range 0.05–0.24″ diameter); their solid-carbide GP-TSC chart covers small/medium drills (up to ~0.31″) at 263–362 SFM in non-alloy steel; and their Modular insert drill chart covers 0.315–1.000″ drills with a min/start/max range of 262/410/558 SFM. The cost-per-hole drops sharply because cycle time falls and tool life climbs — but only with the rigidity, coolant pressure, and machine power to back it up.
How much faster can I drill with through-spindle coolant?
Through-spindle coolant (TSC) does two things: it floods the cutting zone with high-pressure coolant for heat removal, and it actively flushes chips up the flutes so they don’t recut. Both effects raise the safe SFM and let you drill deep holes (greater than 3 times the diameter) without pecking. Haas’s Modular Drills speeds-and-feeds chart explicitly notes: “Through coolant is recommended for greater than 3XD applications.” For a Haas Modular drill in low-carbon steel, the published min/start/max range is 262/410/558 SFM — start at 410 and adjust within that range based on rigidity, hole depth, and target tool life. With flood coolant only, expect to back that off; typical practice is 50–70% of TSC values for similar-grade carbide drills depending on hole depth and chip evacuation. The exact derate depends on your tool and your part; vendor catalogs usually list separate flood and TSC columns.
Why does my TSC low-flow alarm trip when running small drills?
On our Doosan DNM 5700, a small TSC drill — for example, a 7/32″ (5.6 mm) solid carbide through-spindle drill — doesn’t move enough coolant volume to satisfy the through-spindle coolant flow meter, so the machine alarms out even when coolant is flowing fine. The fix is to bracket the small-drill cycle with two M-codes: M313 before the cycle to disable the TSC flow meter for that operation, and M314 immediately after to re-enable it. In Autodesk Fusion we add these as Manual NC blocks in the operations tree so the post-processor inserts them at the exact right point in the program — we just post the file and don’t need to go back and edit raw G-code by hand. Always pair the codes: leaving the flow meter disabled through the rest of the program means a real coolant failure (clogged line, pump issue, broken tool plugging the channel) won’t trigger an alarm and you can lose a part or a tool before noticing. M313/M314 are what our DNM5700 uses; other controls may use different M-codes for the same purpose, so check your operator’s manual.
How do I convert SFM to RPM for drilling?
Use N = (12 × V) / (π × D) for V in SFM and D in inches, or N = (1000 × V) / (π × D) for V in m/min and D in mm. Going the other way: V (SFM) = (π × D × N) / 12, or V (m/min) = (π × D × N) / 1000. Example: a 1/2″ drill at 300 SFM needs 12 × 300 / (π × 0.5) = 2,292 RPM. Reversing — a 1/2″ drill spinning at 2,292 RPM has surface speed of (π × 0.5 × 2292) / 12 = 300 SFM. The same kinematic formula applies to milling cutters and lathe work; drilling is just one application of the cutting-speed-from-surface-speed relationship. (Machinery’s Handbook 29th Ed., p. 1015.)
How do I convert IPT to IPR for drilling?
Multiply by the number of cutting edges: IPR = IPT × Z. Standard twist drills, jobber drills, and most insert drills are 2-flute, so IPR = 2 × IPT. Multi-flute drills (some step drills, some indexable drills with 3 effective edges) use the corresponding count. Most drilling catalogs publish feed in IPR directly because the geometry concentrates cutting on the centerline; per-tooth rates are more common in milling, where chip-load-per-tooth is the critical parameter.
What is the difference between drilling feed and milling feed?
Drilling feed is normally specified per revolution (in/rev or mm/rev) and applies to the whole tool, because every flute is cutting at the centerline at all times. Milling feed is normally specified per tooth (in/tooth or mm/tooth) and gets multiplied by the number of flutes to get the table feed: vf = N × fz × Z. The kinematic relationship vf = N × fn is identical in both; the only difference is whether catalogs publish the feed as fn (per rev, drilling) or fz (per tooth, milling).
What is a drilling speeds and feeds calculator?
A drilling speeds and feeds calculator (also called a CNC feeds and speeds calculator for drilling, or a drilling feed and speed calculator) is the same kinematic tool as this one: it converts a tool catalog’s cutting speed (SFM or m/min) and feed per revolution (IPR or mm/rev) into the spindle RPM and feed rate (in/min or mm/min) you program in CAM. The two halves people search for separately — speeds and feeds — are linked by N = (12 × V) / (π × D) and vf = N × fn. This calculator does both in one shot, plus material removal rate.
How should I derate cutting speed for stainless steel and exotic alloys?
Use the vendor’s tabulated SFM for your specific material — but as a calibration, the Haas Modular insert drill chart shows ferritic/martensitic/PH stainless (ISO P5–P6) at 160/210/260 SFM (min/start/max), austenitic stainless (M1) at 130/260/360, and duplex stainless (M3) at just 70/110/160 SFM — about a quarter of the 262/410/558 SFM range published for low-carbon steel (P1). Inconel and other nickel-based superalloys typically run even lower. Feed per revolution drops similarly. Don’t try to extrapolate from a P-group SFM by eye; pull the M-group or S-group row from the catalog directly.
Should I reduce SFM for very small drills?
Often yes — but it’s an RPM-ceiling problem, not an SFM problem in principle. A 1/16″ drill at 300 SFM needs 18,335 RPM. Most production VMC spindles top out at 8,000–15,000 RPM, so on small drills you become RPM-limited and end up running at lower effective SFM than the catalog allows.
How do I calculate drilling feed rate in metric?
Use N = (1000 × V) / (π × D) where V is the cutting speed in m/min and D is drill diameter in mm. Then vf (mm/min) = N × fn, where fn is feed per revolution in mm/rev. Example: a 10 mm drill at 100 m/min and 0.20 mm/rev needs N = 1000 × 100 / (π × 10) = 3,183 RPM, giving 3,183 × 0.20 = 637 mm/min feed rate. To convert imperial inputs to metric, multiply SFM by 0.3048 to get m/min and inches by 25.4 to get mm. The unit toggle on this calculator handles the conversion automatically.
When does drilling need a peck cycle?
Pecking is needed whenever chips can’t evacuate the hole on their own. Two situations drive that: drilling deeper than 3–5 drill diameters with flood coolant only (no TSC), or drilling soft and gummy materials that produce long stringy chips (low-carbon steel, soft aluminum, copper alloys) regardless of depth. With TSC and a proper drill geometry (parabolic flutes, polished flute surfaces), holes to 8–10 diameters can often be drilled in a single shot. Per the Haas Modular drilling chart, through coolant is the recommended path for any hole greater than 3 times the diameter. Pecking adds cycle time roughly proportional to the number of pecks, so the economic case for TSC is strong on production work.
What is material removal rate (MRR) for drilling?
MRR for drilling is the cross-sectional area of the hole times the feed rate: MRR = (π/4) × D² × vf. For a 1/2″ drill at 22.9 in/min feed rate, MRR = (π/4) × 0.25 × 22.9 = 4.5 in³/min. MRR is useful for estimating spindle horsepower draw and comparing different tooling strategies — a higher MRR means more material removed per minute, but requires the spindle power and rigidity to handle the cut. For machining horsepower, MRR multiplied by the material’s unit horsepower constant gives the cutting horsepower estimate.
Related Calculators
- Chip Load Calculator — Convert between chip load and feed rate for milling, with chip-thinning compensation
- Tap Drill Size Chart — Look up the correct drill size for any thread before tapping
- Thread Milling Calculator — RPM and feed for thread mills
References
- Oberg, E. et al. Machinery’s Handbook, 29th Edition, Industrial Press, 2012, p. 1015 (“Cutting Speed Formulas”): N = 12V / (πD) imperial and N = 1000V / (πD) metric.
- Oberg, E. et al. Machinery’s Handbook, 29th Edition, p. 1079 (Spade Drilling power formulas): variable definitions f = feed in inches per revolution, fm = feed in inches per minute, fm = N × f.
- Haas Automation. Modular Drills, Speeds and Feeds, Inch. Haas Tooling published speed/feed chart for the Modular Drill body + insert system. Source for ISO P/M/K material-group SFM and IPR ranges and the “Through coolant is recommended for greater than 3XD applications” note. Retrieved May 2026 from haascnc.com.
- Haas Automation. Carbide Drills, General Purpose (TSC), Speeds and Feeds, Inch. Haas Tooling published speed/feed chart for solid carbide TSC drills. Source for solid-carbide-with-TSC SFM rung in the comparison table. Retrieved May 2026 from haascnc.com.
- Haas Automation. Cobalt Jobber Drill Sets Feeds and Speeds. Haas Tooling published speed/feed chart for HSS-Co jobber drill sets. Source for HSS-Co rung in the comparison table. Retrieved May 2026 from haascnc.com.
Data last verified: May 2026
Request a Quote
Pi Fabricators is a CNC and fabrication shop in Salem, Oregon. We deliver precision-machined and fabricated parts and assemblies to your specifications.
Request a QuoteThis calculator is provided for reference only and is offered “as is” without warranty of any kind. Pi Fabricators LLC is not liable for any damages or losses arising from the use of this tool. Verify all critical calculations independently with a qualified professional.
Spot an error on this page? Let us know at Contact@pifabricators.com