SizingKitFree drilling feed rate calculator
Drilling feed, and the two depths that are not on the drawing
A drill is fed per revolution, so its feed rate is simply spindle speed times inches per revolution — and the two things that actually decide whether the hole works are how deep it is in drill diameters and how far the point stands ahead of the full diameter. This gives you the feed rate, the feed per lip, the peck increment with the feed reduction already applied, and the Z travel a through hole needs. Free, no account, and both reference tables print.
- 100% free
- No signup
- Peck depth in diameters
- 118° and 135° points
- Printable feed table
Letter and number drill sizes are decimals — look the diameter up rather than guessing it.
1/4 to 1/2 in: 0.004–0.007 in per revolution.
4.0 × diameter.
ANSI/ASME B94.11M: the standard included point angle of a general-purpose twist drill.
Two on a twist drill. This divides the feed for reporting; it never multiplies it.
FEED RATE
F5.9
5.94 in/min · 151 mm/min
Z TRAVEL
1.000 in
25.40 mm from touch-off
- Feed per revolution used
- 0.0050 in / 0.126 mm
- Feed per lip
- 0.0025 in / 0.063 mm
- Depth in diameters
- 4.00 × D
- Peck increment
- 0.2500 in / 6.35 mm
- Point stands ahead by
- 0.0751 in / 1.91 mm
- Tip reaches
- 1.0751 in deep
Chip evacuation set this feed, not the drill. At 4.0 diameters deep the hole is in the 3 to 5 × diameter band, where the guide takes the feed to 0.9 of the tabulated figure — so 0.0055 in per revolution becomes 0.0050, and that reduction is already in the feed rate above. Chip-break pecks of about one diameter, retracting only far enough to snap the chip. What ends a deep drill is not thrust: it is chips that can no longer get out of the flutes, and they pack, seize and snap the drill within a revolution of doing so.
Starting feed per revolution, by drill diameter
Five bands rather than a formula, because the limit changes across the range: on a small drill it is the web and the flute space, on a large one it is thrust and machine rigidity.
| Drill diameter | in per revolution | mm per revolution | in per lip, 2-flute |
|---|---|---|---|
| Under 1/8 in | 0.001–0.002 | 0.03–0.05 | 0.0005–0.0010 |
| 1/8 to 1/4 in | 0.002–0.004 | 0.05–0.10 | 0.0010–0.0020 |
| 1/4 to 1/2 in | 0.004–0.007 | 0.10–0.18 | 0.0020–0.0035 |
| 1/2 to 1 in | 0.007–0.015 | 0.18–0.38 | 0.0035–0.0075 |
| Over 1 in | 0.015–0.025 | 0.38–0.64 | 0.0075–0.0125 |
Conventional drilling feed-per-revolution bands by drill diameter, of the kind published in the drilling feed tables of Machinery's Handbook's Speeds and Feeds section.
None of these bands is a fixed value. Take the lower end in hard, tough or work-hardening material and in anything deeper than three diameters, the upper end in free-machining material through a short hole with a rigid setup. These assume a conventional 118° or 135° twist drill; a parabolic drill, a carbide drill and a spade drill each have their own feed regime, and a coolant-through carbide drill runs several times these feeds. Feed also has to fall away as depth grows past about three diameters, because the chips can no longer clear.
When to peck, how far, and how much feed to give back
Depth expressed as a multiple of drill diameter, which is the only unit chip evacuation responds to — a 1/8 in hole 1 in deep is a deep hole and a 1 in hole 1 in deep is not.
| Depth | Peck | Feed | What the cycle has to do |
|---|---|---|---|
| Up to 3 × diameter | none | 100% | Drill straight through at the tabulated feed. Chips clear on their own. |
| 3 to 5 × diameter | 1 × D | 90% | Chip-break pecks of about one diameter, retracting only far enough to snap the chip. |
| 5 to 8 × diameter | 0.7 × D | 80% | Full retract pecks. The drill has to come clear of the hole to shed the chips and take coolant back down. |
| Over 8 × diameter | 0.5 × D | 65% | Full retract, short pecks, and consider that a jobber drill is the wrong tool: a parabolic or coolant-through drill is designed for this depth and a standard one is not. |
Conventional deep-hole pecking practice for twist drills, expressed as multiples of drill diameter, of the kind published in the drilling sections of Machinery's Handbook and in drill manufacturers' application data.
None of these figures is a fixed value. Peck depth and feed reduction depend far more on the material's chip behavior than on depth alone: a stringing chip in soft steel or aluminum needs pecking well before three diameters, and gray cast iron's powder chips clear far deeper. A coolant-through carbide drill is a different regime entirely and these numbers do not apply to it.
How to set a drilling cycle, feed and depth together
One multiplication for the feed, then the two corrections that decide the Z numbers.
Enter the drill and the speed, and check the feed the band filled in
Feed per revolution is banded by diameter rather than given by a formula, because the limiting thing changes across the range: a small drill is limited by its web and the space in the flutes, a large one by thrust and by how rigid the setup is. The panel reads the band your diameter falls in and takes the middle of it. Type over it if the drill maker published a figure for that specific drill, which supersedes any class table.
Say whether the hole is blind or goes through, and give the depth
For a blind hole the depth is to full diameter, which is not where the tip ends up — the point adds a cone below the shoulder and the panel reports where the tip actually lands. For a through hole the input is the plate thickness and the answer is the travel: thickness plus point length plus a clearance so the cycle does not finish part-way through the breakout. Both accept fractions and millimeters.
Let the depth-in-diameters decide the cycle, not the depth in inches
Chip evacuation responds to the ratio, not the absolute figure: a 1/8 in drill an inch deep is eight diameters and needs full-retract pecking, while a 1 in drill an inch deep is one diameter and needs none. The panel works the ratio out, picks the band, prints the peck increment as a real distance in inches and millimeters, and — this is the part usually left out — applies the band's feed reduction to the feed rate it gives you rather than mentioning it in a footnote.
Technical specifications
| Feed bands | 5 by diameter: 0.001–0.002 in/rev under 1/8 in, rising to 0.015–0.025 in/rev over 1 in — a twelve-fold span across the range |
|---|---|
| Peck guide | 4 bands by depth in diameters: none under 3 × D, 1 × D chip-break pecks to 5, 0.7 × D full retracts to 8, 0.5 × D beyond that |
| Feed reduction | Applied to the answer rather than noted: 90% of the tabulated feed from 3 to 5 diameters, 80% from 5 to 8, 65% past 8 |
| Point length | L = (D / 2) ÷ tan(θ / 2) — 0.300 × D at 118° and 0.207 × D at 135°, computed rather than approximated |
| Point angles | 118° general purpose and 135° heavy duty, both the standard included angles of ANSI/ASME B94.11M |
| Through-hole travel | Thickness plus point length plus breakthrough clearance, the clearance pre-filled at 0.030 in and editable because it is a programming allowance rather than a standard |
| Feed per lip | Reported beside feed per revolution, half of it on a two-flute drill, so the two numbers can never be confused for one another |
| No upload | Both tables and the point geometry compile into the page, so the cycle you are working out is never sent anywhere and the charts print with the network off |
Frequently asked questions
Why is a drill fed per revolution rather than per tooth?
Because both lips of a drill are cutting the same hole at the same time, and what the material sees is one advance per revolution shared between them. That is also the convention every drill feed table in existence is written in, so a figure of 0.006 in/rev means the drill descends six thousandths in one turn and each of the two lips removes three. Hand that same 0.006 to a milling feed calculator as a two-flute cutter and it will multiply rather than divide, giving 0.012 in/rev — twice the intended load on a tool with no side support at all. This is the single most common way a drill gets destroyed by a calculator.
How deep can I drill before I have to start pecking?
About three diameters with a standard twist drill, and the number is a ratio rather than a length. Up to 3 × D the chips climb the flutes and leave on their own, so drill straight through at the tabulated feed. From 3 to 5 diameters short chip-breaking pecks are enough — retract just far enough to snap the chip — and the feed comes back about 10%. From 5 to 8 the drill has to come fully clear of the hole each time to shed chips and let coolant back down. Past 8 diameters a jobber drill is the wrong tool: parabolic and coolant-through drills are designed for that depth and a standard one is being asked to do something it was not made for.
How much deeper than the plate do I program a through hole?
The plate thickness, plus the point length, plus a clearance — and the point length is the term people forget. A 118° drill stands 0.300 times its diameter ahead of the full diameter and a 135° one 0.207 times, so a 1/2 in 118° drill through a 3/4 in plate needs 0.750 + 0.150 + a clearance, call it 0.930 in of travel rather than 0.750. Stop at the thickness and the hole is at full size for only part of its depth and leaves a ragged partial breakout on the far face. This is also why a drilled hole in a stack of two plates needs the point cleared through both.
Does a 135° split point drill faster than a 118°?
It starts better and it drills a shorter hole, which are two separate advantages. The split point removes most of the chisel edge, so the drill self-centers instead of wandering and the thrust needed to start it drops sharply — that is why 135° split points are standard for hard, tough and work-hardening material and why they can often be started without a spot drill. The shorter point also means less travel: 0.207 × D of cone instead of 0.300 × D. What it does not do is raise the feed per revolution, which is set by the material and the flute space, not by how the tip is ground.
Why does a drill wander when it first touches the work?
Because the very center of a twist drill has no cutting speed and no cutting geometry. The chisel edge across the web is not a cutting edge at all — it extrudes metal sideways under enormous pressure — and until the outer lips engage there is nothing holding the drill on center. A spot drill with a point angle equal to or wider than the drill's fixes it by producing a chamfered start the drill's corners contact first; a center drill does not, because its small pilot tip is fragile and it leaves a radius the drill point does not match. A split point avoids most of the problem by removing the chisel edge, which is the same fix from the other direction.
The hole is oversize and the drill squealed. What went wrong?
Almost always the drill was fed too lightly or is unevenly ground, and both produce the same oversize hole. A drill only cuts on size if both lips are the same length and at the same angle; if one lip is longer it takes the whole cut and swings the drill, cutting a hole larger than the drill by twice the error. Too little feed makes it worse by letting the drill ride and rub rather than bite. A drilled hole is not a precision feature in any case — a hole that has to hold a tolerance is drilled undersize and reamed or bored — but a well-ground drill fed properly will hold a few thousandths over, and a badly ground one will be tens of thousandths over and out of round.
Do these feeds apply to a coolant-through carbide drill?
No, and not by a small margin — a coolant-through carbide drill often runs at several times these feeds and drills to ten diameters or more without pecking at all. The bands here describe a conventional high-speed steel twist drill with a 118° or 135° point, which is what is in most drill indexes and most tool cribs. Parabolic drills, spade drills, indexable drills and coolant-through carbide each have their own feed regime, and in every case the manufacturer publishes it for the specific drill. Using a class table where a product table exists is leaving most of the tool's capability unused.
About feed per revolution, chip evacuation and drill point geometry
The arithmetic of a drilling feed is one line — inches per minute is rev/min times inches per revolution — and everything difficult about drilling is in the two numbers that line does not contain. The first is depth measured in diameters. A drill is a tool with a conveyor built into it: the flutes have to carry every chip the lips make all the way back out of the hole, and past about three diameters they stop managing it. The chips pack, the packed chips grip the flutes, the drill seizes and the next revolution twists it off. Nothing about thrust or power warns you first. That is why the pecking guide is expressed as multiples of diameter rather than as inches, and why the feed itself has to come down as the hole gets deeper — a smaller chip is a chip with a better chance of getting out.
The second is the point. A twist drill does not end in a flat face; it ends in a cone whose included angle is 118° for general work or 135° for hard and work-hardening material, and the cone stands (D/2) ÷ tan(θ/2) ahead of the full diameter — 0.300 times the diameter at 118°, 0.207 at 135°. Every depth decision has to account for it. A through hole is not through until the full diameter has cleared the far face, so the travel is the thickness plus the point plus a clearance. A blind hole reaches its nominal depth at the shoulder and the tip is already deeper, which matters when there is a cooling passage or an opposite face below. And the center of that same point is the reason drills wander: the chisel edge across the web is turning at zero surface speed however fast the spindle goes, so it extrudes material rather than cutting it until the outer lips take hold. The drill size chart has the decimal diameter for the fractional, number, letter or metric drill you are about to put in the chuck, which is the figure this panel wants.
Everything here describes a conventional twist drill, and it is worth saying what that excludes. A coolant-through carbide drill runs at several times these feeds and goes to ten diameters or more without a peck; parabolic drills, spade drills and indexable drills each have their own regime; and in all of those cases the manufacturer publishes data for the specific tool that supersedes any class table, including this one. What the panel can do is give you a defensible starting point with the reasoning printed beside it. If the plate you are drilling is going to be bent afterwards, note that hole positions belong to the flat blank rather than to the finished part, and the flat comes from the bend allowance or the bend deduction, both of which need the K factor for the material and the radius. A hole drilled at the wrong distance from a bend line is a scrapped part, and it is scrapped before the drill ever touches it.
Nothing about this cycle leaves the tab
Every number on this page is worked out by JavaScript running in the tab you are reading it in. Nothing you type — loads, lengths, nameplate ratings, the rates your utility charges you — is uploaded, logged or kept, which is also why the calculators carry on working in a mechanical room with no signal.
The drill, the depth and the plate you described are used to fill in the panel and are gone when the page closes. The peck and feed tables are part of the page rather than something it fetches, which is why the charts still print on a machine with no network.