A vertical mill shapes a block with a turning tool moved in X, Y and Z

On a vertical mill the cutting tool turns in a spindle above the work. The work is clamped on the table, the table moves it front to back and side to side, and the tool comes down into it. Every shape the mill makes is the space the turning tool swept through.

X and Y

The two directions across the table. In this lesson X runs left to right as you face the machine and Y runs away from you, toward the back.

Z

Up and down, along the tool. Z+ is up, away from the work, so negative Z is below the finished top face. The raw top is at Z +1, so facing can remove metal at zero or positive Z while taking off that allowance.

Readout

The display that shows where the tool is, in X, Y and Z. A readout on a manual mill is often called a DRO, for digital readout. Here it shows the position of the tool’s tip.

Work zero

The point the readout counts from. In this lesson X 0, Y 0 is the front left corner of the block and Z 0 is the finished top face. Every dimension on the drawings is measured from those same edges and that same face.

On a real knee mill the table carries the work under a spindle that stays put in X and Y. In the simulator you move the tool instead. The readout tells the same story either way: where the tool’s tip is, measured from work zero.

Each kind of tool cuts a shape of its own, and some cannot cut sideways

Face mill

A wide body with cutting inserts round its rim. It is fed across the work to leave a broad flat face. The one in the simulator takes at most 4 mm in one pass. The inserts sit at the rim, not across the middle, so it is brought down beside the work and then fed in, never pushed straight down into the metal.

End mill

Cuts on its sides and its end. The end mills here are centre-cutting: their end teeth reach the middle, so they can be fed straight down into the metal and then moved across to cut pockets, slots, steps and walls. An inside corner they leave is rounded to the cutter’s own radius.

Spot and chamfer tool

A pointed tool with a 90° point. Fed down, it cuts a cone: the start of a hole, or a countersink round the mouth of one. Run along an edge, it bevels the edge, which is a chamfer.

Drill

Cuts only at its point, as it feeds down along its own axis. It leaves a round hole its own size, with a cone at the bottom from its point. It must never be pushed sideways in the metal.

Tap

Cuts a screw thread into the wall of a hole that is already there. It only goes straight in and straight back out.

Boring head

An adjustable single cutting point on an offset bar. Set to a diameter and fed down a hole, it opens the hole to that size. Its bar has no cutting edge at the centre, so it needs a hole to start in.

The tool’s centre runs one radius away from the wall it cuts

The readout shows where the centre of the tool is. The metal is cut by its edge. To leave a wall at a given place, put the centre one radius away from it, on the side being cut away.

Worked example. A shoulder’s wall belongs at X 75, with the metal to the right of it cut away. A Ø12 end mill has a 6 mm radius, so its centre runs along X 75 + 6 = X 81. Run it along X 75 instead and the wall ends up at X 69, 6 mm too far into the part. That metal cannot be put back.

• Inside corners take the cutter’s radius. A round tool cannot reach into a sharp inside corner, so a pocket’s corners come out rounded to the radius of the cutter that made them. A drawing that allows R4 at most calls for a cutter no bigger than Ø8.
• Outside corners stay sharp. Going round the outside of a corner, the tool swings about it and never cuts into it.
• A slot is the width of the cutter that made it in one pass. A cutter moved in a straight line leaves a groove exactly its own width, with round ends of its own radius.

When a cutter cuts with its side, the metal is on one side of it or the other. With the cutter turning clockwise seen from above, metal on the cutter’s right as it moves is climb milling, and metal on its left is conventional milling. The simulator says which each side cut was. Climb and Conventional Milling explains the difference.

Holes: drilled to size, threaded by a tap, opened up by a boring head

A drill leaves a hole of its own diameter. A hole’s depth on a drawing is measured to where the hole stops being full size, not to the tip of the cone the drill point leaves below that.

A tapped hole starts as a smaller drilled hole

A tap cuts its thread into the wall of a hole, so the hole has to be drilled smaller than the thread first, to the tap drill size. For the common metric coarse threads that size is close to the thread’s outside diameter minus its pitch, the distance from one thread to the next:

Tap drill ≈ thread diameter − pitch. M6×1: 6 − 1 = Ø5.0. M8×1.25: 8 − 1.25 = Ø6.75, drilled Ø6.8.

Drilled too small, the tap has to cut too much metal and can break. Drilled too big, the thread is shallow. The simulator checks the hole against a simplified minor-diameter band and refuses a severely undersize pilot. This does not establish functional thread fit: pitch diameter, thread form and a real thread gauge are separate checks.

Drill deeper than the thread you need

The first few threads of a tap are ground away to a taper so that it can start in the hole. Those threads cut only part of a thread, so full thread stops short of the tap’s tip. In a hole with a bottom, the tap has to go deeper than the full thread you need, and the drilled hole deeper again, past the drill’s point. This simulated tap has a 4-pitch cutting chamfer; real taps vary. The job calls for full thread reaching Z −10 from the finished face. Its countersink removes the first part of the thread, so that is not 10 mm of surviving full-thread length.

Sizes no drill gives

Drills come in fixed sizes. A boring head is set to the size you need and fed down a hole already big enough for its bar, which makes it the tool for a hole of an exact, larger size.

What the simulator leaves out

The 3D target is a nominal guide sampled at 0.25 mm in X and Y. Its flat floors have the drawing’s depth; its small curved outlines are approximations. The cut surface is derived separately from the analytic tool paths. Neither picture is a dimensional gauge: inspection uses the drawing’s allowed limits, including smaller corners where the drawing says R4 max. Complex conical histories or very long cut histories switch to 2D sections to keep the controls responsive. The work is kept, and Undo or a fresh block can restore the 3D view.

The simulator is a model of where metal is and where tools can reach. It does not check speeds, feeds, forces or finish, and passing a job here says nothing about whether a real setup could take the same cuts. Feeds and Speeds is about those numbers.

• Only straight down and straight across. The tool axis is always vertical and nothing is undercut, so every shape is a height above each point of the table.
• Tools are exact and rigid. A hole is exactly the drill’s size, a cutter never bends or wears, and edges come out without burrs.
• Threads are recorded, not drawn. The simulator keeps the size of the hole a thread was cut in and how deep its full thread runs, and checks that later cuts have not taken the metal it is in. It does not model the thread’s form or fit.
• No chips, coolant or heat, and no limit on depth of cut except where a tool’s cutting edges run out.

Supporting detail: Addendum 1 — How the inspection decides, and what its numbers are.

What is G-code?

A CNC mill moves its tool by reading a program from the top down, one line at a time. The language most mills read is called G-code. Each line holds a few words, and together they say where the tool goes next, how fast, and what the spindle and tool are doing.

Start with CNC Control Fundamentals for the control and machine types, CNC Axes and Offsets for coordinate references, and CNC Program Structure for common Fanuc-style milling codes. G- and M-code meanings vary by control. The simulator below uses its own documented subset; check the machine's manual for real programs.

Word

A letter and a number, such as X20, G1 or F300. The letter says what the number means: X, Y and Z are positions, F is the feed rate, S the spindle speed, T a tool number. G and M words are codes that choose what kind of move or machine action the line is.

Block

One line of the program. Machinists often call a line a block; in the simulator below, each block you snap into place is one line of G-code, with the same number.

Work zero

The point the program’s numbers count from. Here, as in Milling Operations, X 0, Y 0 is the front left corner of the block and Z 0 is its finished top face. The uncut stock starts at Z +1. Positions refer to the tip of the tool, on its centre line: Z −3 is 3 mm below work zero and 4 mm below that raw top. A pointed drill reaches its programmed Z at its tip; the full-diameter hole is shallower.

Modal

Most codes stay in force until another code from their group replaces them. After a G1, a line with only X80 is still a G1 move; a feed rate set with F remains available until changed. Not every word is modal. For ordinary G0/G1 moves, an omitted axis stays in place; it does not repeat the preceding incremental displacement.

Read the program above from the top. Line 2 sets millimetres, absolute positions and the XY plane. Line 3 puts tool 1, a Ø10 end mill, in the spindle, and line 4 starts the spindle at 2500 rpm. Lines 5 and 6 move the tool through the air to just above the start of the slot. Line 7 feeds it to Z −3, cutting 4 mm below the raw top at Z +1. Line 8 feeds it along the closed-ended slot, and line 9 lifts it clear. Line 10 stops the spindle and line 11 ends the program.

Rapid moves put the tool in place through the air; feed moves cut

• G0 is a rapid move. The control uses its rapid positioning rate, subject to machine limits and applicable overrides. It is for getting the tool to where a cut starts, through the air, never for cutting.
• G1 is a feed move. The tool moves in a straight line at the feed rate set by F, here in millimetres per minute. It can cut or feed through air.
• The spindle has to be turning first. S sets its speed in revolutions per minute, M3 starts it turning clockwise seen from above, and M5 stops it. T1 M6 changes to tool 1.
• A move goes in one straight line. G1 X80 Y40 Z-2 moves all three axes together and they all arrive at once. An axis left out of the line stays where it is: G1 X80 moves along X only.

A rapid into metal is a crash: the tool arrives at full traverse speed with nothing to say it should be cutting. The simulator stops a rapid at the point where it would touch the block and says so. It does the same if a feed move reaches the metal with the spindle stopped.

This simulator moves a rapid in one straight line, the way the LinuxCNC G-code reference describes G0. Controls differ in how they move during a rapid, so check how the one you use moves before you count on the path a rapid takes.

G90 and G91, G20 and G21: two modes that change what every number means

G90, absolute

A number is a position, measured from work zero. With the tool at X 10, G1 X30 moves it to X 30.

G91, incremental

A number is a distance from where the tool is now. With the tool at X 10, the same G1 X30 moves it 30 mm, to X 40.

G21, millimetres

X30 means 30 mm and F300 means 300 mm per minute with the simulator's G94 feed mode.

G20, inches

The same X30 means 30 inches, which is 762 mm, and, with G94, the feed rate is in inches per minute. A millimetre program read in inches asks for moves 25.4 times as long.

Because these modes change the meaning of every line after them, a program sets both near its start, before the first move. The simulator insists on it: a move before G20 or G21 and G90 or G91 have been set stops the program, and so does a change of units after the machine has started moving.

Work through a point list in Absolute and Incremental Positioning. Units and feed mode are separate settings; G95, where supported, uses feed per spindle revolution.

G2 turns clockwise and G3 counterclockwise, seen from above

An arc move cuts along part of a circle in the XY plane (G17) at the feed rate. Its direction is the way it turns as seen looking down on the work from above: G2 clockwise, G3 counterclockwise. The line gives the arc’s end point with X and Y, and its centre in one of two ways.

• I and J say where the centre is, measured in X and Y from the point where the arc starts. That is the usual mode, G91.1, and it holds even while G90 makes every X and Y a position. G90.1 makes I and J a position too in this simulator. Those decimal codes are not universal; check the control's centre-mode rules.
• R gives the radius instead, and the control works out the centre. A positive R selects an arc of up to half a turn, a negative R the longer way round in the convention used here. An R arc cannot be a full circle, because a circle through one point has no single centre; a full circle uses I and J with its end point the same as its start.

Worked example. The tool is at X 72, Y 15, moving right along the bottom of an outline. G3 X80 Y23 I0 J8 puts the centre 0 in X and 8 in Y from the start, at X 72, Y 23. Turning counterclockwise about it, the tool rounds a corner of radius 8 and ends heading up the right-hand side at X 80, Y 23. The end point has to lie on the circle: change J8 to J6 and the start radius is 6 mm while the end radius is √(8² + 2²) = √68, about 8.246 mm, so the simulator stops at that line instead of guessing.

In the diagram, absolute endpoints and start-relative centres give G03 X22 Y18 I0 J10 from A to B, then G02 X12 Y8 I-10 J0 back to A. Each start point needs its own centre offsets. Radius format can instead use G03 X22 Y18 R10 for the first arc under the stated convention.

G17 uses X/Y and I/J; G18 uses X/Z and I/K; G19 uses Y/Z and J/K. I, J and K correspond to centre components along X, Y and Z. Judge arc direction looking from the positive normal axis toward the plane: +Z for XY, +Y for XZ, +X for YZ. The simulator supports XY arcs only.

Practice quarter arcs

A drilling cycle packs a whole hole into one line

G81 X15 Y15 Z-8 R2 F120 drills a hole at X 15, Y 15. The tool moves there at rapid, comes down at rapid to R, the height just above the work where feeding begins, feeds down to Z, the drill-tip depth, and rises back up at rapid.

• How high it rises. In this simulator G99 rises to R between holes, and G98 rises to the height the tool was at when the cycles began, or to R if that is higher. The simulator needs one of the two before the first G81.
• The cycle is modal. After a G81, a line with only X or Y drills another hole with the same depth, R and feed. G80 ends the cycle; after it, a line with only X or Y is an error until a G0 or G1 says how to move.

Without cutter compensation, program the tool centre path

With cutter compensation off, as in this simulator, X and Y describe where the centre of the tool goes. The metal is cut by its edge, one radius further out. A Ø10 end mill fed along Y 30 cuts a slot from Y 25 to Y 35. To leave a wall at X 80 with the metal beyond it cut away, the centre runs along X 85. Milling Operations works through the same rule for a shoulder and a pocket.

Controls can do that offset for you with cutter radius compensation, G41 and G42. The simulator does not model it, so every program here is written as the path of the centre, and a line with G41 or G42 stops with a message. CNC Axes and Offsets explains left/right compensation and tool-length offsets.

What the simulator reads, and what it leaves out

The simulator reads a small part of G-code, modelled on the way the LinuxCNC control reads it. Any other code, or a line that is not G-code at all, stops the program at that line with a message saying what is wrong. Nothing is skipped.

Motion

G0 rapid, G1 feed, G2 and G3 arcs in the XY plane, G81 drilling cycle and G80 to end it.

Modes

G17 XY plane, G20 inches, G21 millimetres, G90 absolute, G91 incremental, G90.1 and G91.1 for I and J, G94 feed per minute, G98 and G99 for the drilling cycle. G40, G49 and G54 are read as the settings the simulator always has: no cutter compensation, no tool length offset, and its one work offset.

Machine

M3 spindle on, M5 off, M6 tool change, M8 and M9 coolant on and off (shown, with no effect on the cut), M2 or M30 program end: stops spindle and coolant, restores G90 and G1, and leaves the tool at its last position.

Words

X Y Z positions, I J arc centre, R arc radius or drilling R plane, F feed rate, S spindle speed, T tool, N line number, and comments in brackets or after a semicolon.

Tools

T1 Ø10 end mill, T2 Ø6 end mill, T3 Ø6 drill, T4 Ø12 spot and chamfer tool, T5 Ø50 face mill: the tools of Milling Operations, with the same rules about what each can cut.

• Some rules are the simulator’s own. It needs units and distance mode set before the first move, a speed before M3, G98 or G99 before a drilling cycle, and, for a tool change, the spindle stopped and the tool at Z +20 or higher. A real control may be less strict, or strict about different things.
• Only straight down and straight across, through metal. The block is modelled as a height above each point, so the tool can cut moving along Z alone, or in X and Y at one height. A move in X or Y and Z at once is followed exactly through the air, but stops if it would reach the metal: ramping and helical moves are not modelled.
• Arcs are cut as short straight chords, each within 0.01 mm of the true arc. They are drawn as true arcs.
• Simple timing. Feed moves run at their F and rapids at 5000 mm per minute, with no acceleration, no blending of one move into the next, and no time for tool changes.
• Not a check of a real program. The speeds and feeds in the examples are round teaching numbers, not cutting recommendations; Feeds and Speeds is about choosing them. A program that runs here has met only this simulator’s rules. Controls differ in the codes they accept, in their starting modes and in how they change tools, so a program for a real machine is checked against the manual for its control. See CNC Programming and Prove-Out for graphics, dry run, single block and overrides; follow Equipment Operating Procedure for machine use.

Supporting detail: Addendum 2 — How the simulator reads and runs a program.

Climb versus Conventional Milling

A milling cutter turns while the work and cutter move past each other. At the part of the cutter that is making the cut, climb milling means the cutting edge moves in the same direction as that relative feed; conventional milling means it moves against the feed. Those two relationships are the whole distinction—not a universal left or right direction on the machine.

Climb milling

Also called down milling. Where a tooth is cutting, it moves the same way the work is fed. Each chip starts thick and ends thin.

Conventional milling

Also called up milling. Where a tooth is cutting, it moves against the feed. Each chip starts thin and ends thick.

Feed per tooth, width of cut (radial engagement) and axial depth of cut are defined together on Feeds and Speeds. This page uses them only to show what changes when the direction changes.

Chip Forming Characteristics

A chip does not stay where the slice was. The cutting edge shears it off the work, it slides along the face in front of the edge and curls into the flute, and the flute carries it round until it is thrown clear. The drawings compare chip paths in the cross-section of this horizontal-cutter setup; they do not predict a universal chip-flight direction.

Swipe the four moments sideways on a narrow screen, or focus the drawing and use the arrow keys to scroll.

Reading the cutter

• Cutting edge: the tip of each tooth, the only part that touches the finished surface. The tooth that is cutting is outlined in blue.
• Rake face: the face just in front of the edge. The chip slides along it as it forms.
• Flute: the curved valley in front of each tooth. The chip curls in it and is carried out of the cut in it, so a flute packed with chips cannot take the next one.
• Core: the solid centre, hatched because the drawing cuts through it. In this illustrated family, more flutes leave a thicker core and less room for chips. Actual proportions depend on the tool design.

The chip is drawn shorter and thinner than the slice so it fits the flute at a feed drawn many times too large. A continuous metal chip usually becomes shorter and thicker through deformation; IIT Kharagpur’s chip-formation lesson explains the change. The path it takes is illustrative. Actual chip motion depends on the rotation/feed relationship, engagement, flute helix and chip space, material and chip-breaking geometry, and coolant or air delivery. Helical flutes can also move chips along the cutter axis; this in-plane drawing does not show that axial evacuation. The cutter’s flutes and chip space follow Harvey Performance’s end mill anatomy.

Starting thin means rubbing; starting thick means a bite

A real cutting edge has a rounded tip. When the uncut layer is extremely thin, the edge can push and rub the metal before a chip forms. The peripheral cuts shown here make that difference visible.

• Conventional milling starts every chip at zero, so every tooth rubs before it bites. Rubbing makes heat and wears the edge. Look at where the tooth enters, too: on the finished surface, the one you are keeping.
• Climb milling starts the chips shown here at their thickest, so the tooth bites at once, with a knock each time a tooth enters.

That is the main reason climb milling is often the preferred direction when the machine can hold the work steady against it. Whether it can is the next card.

Supporting detail: Addendum 3 — When a rough or hard exterior can change the choice.

Which way the cut pulls on the work

• Climb: the teeth drag the work along the way it is already being fed, and tend to push it down onto the table in the peripheral arrangement shown.
• Conventional: the teeth push back against the feed and tend to lift the work in this arrangement, so whatever holds the work has to resist that lift.

The dial counts screw rotation; the indicator finds the carriage

A handwheel dial does not measure the carriage. It counts how far the screw has turned and multiplies by the lead. That is the carriage's travel only while the screw keeps pushing the nut in one direction.

A screw and its nut need some clearance between their thread flanks (a flank is the sloping side of a thread). After the screw changes direction, it must turn through that clearance before its other flank meets the nut and the carriage moves again. That clearance is backlash, the same idea defined for threads in Screw Threads and for gear teeth in Gear Drives and Tooth Geometry. The turn spent crossing it is lost motion: input that produces no output.

• Dial reading: travel predicted from screw rotation, turns × lead. See Lead Screws.
• Carriage position: where the carriage really is, as an indicator touching it would show.
• The difference is zero after a forward approach (the direction the dial was zeroed in) and one full clearance after a reverse approach.

Supporting detail: Addendum 5 — Where the definition comes from.

Predict the dead band: clearance divided by lead, as a fraction of a turn

Once the screw reverses, the carriage stays still until the screw's helix has moved one full clearance B. One turn moves the helix one lead L, so the dead band is B ÷ L of a turn.

The carriage error after a reverse approach is the same 0.20 mm in both rows. A finer lead only spreads that same clearance over more of the handwheel turn.

Land on a dimension: finish every approach in the direction the dial was set

If you overshoot a target, turning straight back to the number leaves the carriage one clearance away from it, because the screw is now pushing on the other flank. Instead:

1. Back the handwheel past the target by more than the backlash.
2. Turn in the original direction again and stop on the number.

The same reasoning applies when setting a dial. MIT's 2.670 milling notes say to “be certain that the backlash in the mechanism driving the table is taken up prior to setting the dial indicator”. A dial set with the clearance taken up in one direction reads true for approaches in that direction. For edge finding, Mill Indicators and Part Zero repeats the touch from the same direction for the same reason.

Supporting detail: Addendum 6 — A readout that measures the slide, and when the clearance still matters.

What the lab model includes and leaves out

• Included: a rigid screw that turns but never slides along its axis, a nut fixed to the carriage, and a total axial clearance B. The carriage position c stays within B/2 of the screw's helical phase s = −Lφ/360° (right-hand thread, φ the screw rotation); inside that band it does not move.
• Assumed: friction holds the carriage still inside the clearance, and no outside force pushes it along the axis.
• Left out: forces, friction values, stiffness and elastic wind-up, preload, stick-slip and wear. Drives designed to remove the clearance, such as preloaded ball nuts or adjustable split nuts, are beyond this model.
• Illustrative: the leads, clearances and the 3D screw (5 mm lead, 1.0 mm clearance, 30° flanks) are chosen to be seen, not taken from a standard thread or a measured machine.

For drive design in depth, Alexander Slocum's Precision Machine Design (1992) covers actuators and transmissions in Chapter 10, including section 10.8, Linear Power Transmission Elements.

Six quantities connect the cutting data, machine and cut

Start by separating six quantities. Cutting speed and feed per tooth describe what the cutting edges should experience. Spindle speed and table feed are the corresponding machine settings. Width of cut and axial depth describe how much of the cutter is engaged. The exact starting values come from cutting data for the tool, material and operation.

Cutting speed

How fast the cutting edge moves through the material: the speed at the outside of the cutter. Written in surface feet per minute (SFM) or metres per minute (m/min). Also called surface speed. Comes from cutting data.

Feed per tooth

How far the work moves while the cutter turns from one tooth to the next, in inches or millimetres per tooth. Also called chip load, because it sets the size of the bite each tooth takes. Comes from cutting data.

Spindle speed

How many turns the cutter makes each minute, in revolutions per minute (rev/min, usually said RPM). Set on the machine.

Table feed

How fast the work moves past the cutter, in inches or millimetres per minute. Also called the feed rate. On a machine that moves the cutter instead, it is how fast the cutter travels. Set on the machine.

Width of cut, a_e

The cutter’s radial engagement in the work, measured across the cutter in inches or millimetres. It is also called radial depth of cut; those names describe the same quantity, not two separate settings.

Axial depth of cut, a_p

The distance engaged along the cutter’s axis, in inches or millimetres: the difference between the uncut and cut surfaces in that axial direction.

Spindle speed: the turns it takes to reach the cutting speed

Cutting speed is a distance per minute, measured at the edge of the cutter. In one turn, a point on that edge travels once around the cutter: its circumference, π × D. So the spindle speed is the cutting speed divided by the distance one turn covers, once the two are in the same units.

Spindle speed (rev/min) = 12 × cutting speed (SFM) ÷ (π × cutter diameter in inches)

The 12 is there because cutting speed is in feet and the diameter is in inches: 12 inches to the foot. In metric units the same idea needs a 1000, millimetres to the metre:

Spindle speed (rev/min) = 1000 × cutting speed (m/min) ÷ (π × cutter diameter in mm)

Worked example, with illustrative numbers. A 0.5 in cutter, with cutting data that calls for 300 SFM: 12 × 300 ÷ (π × 0.5) = 2,292 rev/min. The 300 SFM is there to make the arithmetic concrete. It is not a recommendation for any tool or any material. The feed value below is illustrative too; use the later material guide for the carbide starting bands.

Look at where the diameter sits: underneath. Halve the diameter and the spindle speed doubles. A small cutter has to turn faster to give its edge the same cutting speed, which is why small cutters so often ask for more speed than a machine has. That case has its own card below.

Table feed: each tooth takes one chip load as it passes

Each time a tooth passes, the work should have moved one feed per tooth. The number of teeth passing each minute is the spindle speed times the number of flutes, so:

Table feed = spindle speed × flutes × feed per tooth

Worked example, continued. A 4-flute cutter at 2,292 rev/min, with a feed per tooth of 0.002 in: 2,292 × 4 × 0.002 = 18.3 in/min. The units work out on their own: turns per minute, times teeth per turn, times inches per tooth, leaves inches per minute.

Turned around, the same relation tells you what chip load a feed gives. That is the way to check a feed someone else has set:

Feed per tooth = table feed ÷ (spindle speed × flutes)

Flutes here means the teeth that actually take a chip in each turn. For an ordinary end mill that is simply the number of flutes.

Removal rate: width × depth × table feed

Two more numbers describe the cut itself. The width of cut is how far the cutter reaches sideways into the work, across the direction of feed. The depth of cut is how far down its side the cutter is buried, along its axis. A side cut can be no wider than the cutter; a wider path takes more than one pass.

While the table feeds, the cutter sweeps through the work and leaves a channel behind it. In a stretch of time the cutter travels table feed × time, and the solid metal it takes out in that stretch is a slab as wide as the cut, as deep as the cut, and as long as that travel. Per minute, that is the material removal rate:

Removal rate (in³/min) = width of cut (in) × depth of cut (in) × table feed (in/min)

The front of the cut is curved, because it is the cutter’s own shape. The slab’s two ends are the same curve, one travel apart, so whatever the curve, the slab holds exactly width × depth × travel.

Worked example, continued. The same cutter, 0.1 in wide (20% of its diameter) and 0.5 in deep, at 18.3 in/min: 0.1 × 0.5 × 18.3 ≈ 0.917 in³/min, or 15.0 cm³/min. In 5 seconds the cutter travels 1.53 in and removes 0.0764 in³.

That is the volume of solid metal. Once it is chips, the same metal lies loose and takes up far more space, so the removal rate is not the size of the chip pile.

Cutting power: removal rate times the energy each cubic inch takes

Cutting a cubic inch of a given material takes roughly a given amount of energy. That is its specific cutting energy, and it is why the same cut needs more power in steel than in aluminum. Written as power per unit of removal rate, it turns a removal rate straight into power:

Cutting power (hp) = removal rate (in³/min) × unit power (hp per in³/min)

Cutting power (W) = removal rate (mm³/min) × specific energy (J/mm³) ÷ 60

The 60 turns minutes into seconds, because a watt is a joule per second. One mechanical horsepower is 745.7 W.

Worked example, continued. For 6061-T6 aluminum the guide in the calculator gives a band of 0.16 to 0.30 hp per in³/min. At 0.917 in³/min that is about 0.15 to 0.28 hp, or 110 to 210 W. The same cut in 304 stainless steel, whose band is 0.65 to 1.3 hp per in³/min, needs about 0.60 to 1.2 hp.

The answer is usually a band. Some table rows give one factor; that still produces an estimate, not a measured certainty. Published bands cover a family of materials over a range of hardness, and the energy a real cut takes also depends on chip thickness and cutting-edge geometry. Treat the band as the size of the job, not a prediction to the watt.

Three different powers get called “the power”, and they are not the same:

• Cutting power is what the cutting edge spends. That is the estimate above.
• Motor shaft power is more, because the belts, gears and bearings between the motor and the cutter lose some on the way. If the drivetrain passes on 80% of what the motor delivers, the motor must deliver the cutting power ÷ 0.8.
• Electrical power drawn from the supply is more again, because the motor and its drive lose some too.

None of these tells you whether a machine can take the cut. A spindle motor’s rating is not necessarily available at every speed, and power is only one limit: the tool, the holding and the machine’s stiffness are others. Use the estimate to compare cuts and to see why a cut is heavy, not to approve one.

When the machine cannot turn as fast as the formula asks

Because small cutters ask for high spindle speeds, the formula can easily give more than a machine’s top speed. A 0.125 in cutter at 300 SFM asks for 9,167 rev/min. On a machine that stops at 4,000, it runs at 4,000.

• Work the feed from the speed the spindle really turns. At 4,000 rev/min, with 2 flutes and 0.0008 in per tooth, that is 4,000 × 2 × 0.0008 = 6.4 in/min. Each tooth then takes the chip load you meant it to.
• The cutting speed is what you give up. At 4,000 rev/min the edge of a 0.125 in cutter moves at π × 0.125 × 4,000 ÷ 12 = 131 SFM, not the 300 the data asked for.

Working the feed from the speed that was asked for, rather than the one the spindle is turning, gets the chip load wrong by the same ratio. A feed worked from 9,167 rev/min would give each tooth 9,167 ÷ 4,000 = 2.3 times the chip load intended.

The same applies to a machine that offers only certain speeds, through belts or gears: set the nearest speed it has, and work the feed from that one. The calculator’s machine top speed box does this for a top speed.

The length that matters starts at the clamp

Stickout is unsupported length. Here it is the distance from the rigid clamp face to the point where the sideways force acts. It is not the total tool length, and it is not automatically the flute length.

A force bends the tool and moves its cutting edge away from its unloaded position. The clamp end stays in place and keeps its direction; the bend grows along the unsupported length. In a real cut, force acts over the engaged cutting edges rather than at one perfect point.

Length is cubed; diameter is raised to the fourth power

For the ideal solid round tool in this lab, tip bending is proportional to F × L³ ÷ (E × d⁴). Change one input at a time to see which factor is responsible.

Try a combined change: start at L = 40 mm and d = 10 mm, save that baseline, then set L = 80 mm and d = 20 mm. The length contributes 8× and the diameter contributes 1/16×, leaving half the bending at the same load and modulus. The two changes compete.

Supporting detail: Addendum 9 — The calculation and its units.

Use the trend; know what this model leaves out

This is a static, linear-elastic, slender-beam model: a uniform solid round tool, a perfectly rigid clamp, a steady sideways point load at the free end and deflections small compared with the length. Elastic modulus E measures stiffness, not hardness or breaking strength.

The lab starts at E = 600 GPa, a chosen teaching value within Hyperion's published 430–690 GPa range for cemented-carbide wear grades. It is not a universal value for carbide cutters. The force is an assumed input, not calculated from a milling operation.

Flutes and necks change stiffness. The holder, spindle and workpiece can move too, and a milling force changes as teeth engage. Static bending alone does not predict chatter thresholds, surface roughness, fracture, safe loads or guaranteed finished-part error.

The lab flags L/d below 4 and bending above 1% of L as prompts to question this simplification. Those are teaching checks, not certification or safety limits.

Supporting detail: Addendum 10 — Primary references.

Connect the setup to feeds, speeds and removal rate, and explore the path and tool access in Milling Operations.

Identify the parts that rotate, guide and feed

Headstock and spindle

The headstock supports the rotating spindle and its drive. The spindle carries the chuck, faceplate or other workholding. Its axis is the reference for turning.

Bed and ways

The bed supports the assemblies. Its guide surfaces, called ways, guide carriage travel and locate the tailstock.

Tailstock

Supports the far end of work with a center, or holds axial tools such as drills and machine reamers. Its quill extends along the spindle axis when aligned.

Carriage, cross slide and compound rest

The carriage moves along the bed. The cross slide moves across the axis. The compound sits above it and swivels to guide short angled movements. The tool post holds the cutting tool on the compound.

Apron

The assembly on the front of the carriage contains feed mechanisms and controls.

Feed rod and leadscrew

On machines with separate drives, the feed rod powers ordinary turning or facing feeds; the leadscrew synchronizes threading. Some lathes combine functions, so identify the actual drive arrangement before selecting a feed.

Half-nuts and quick-change gearbox

The half-nuts close around the leadscrew to drive the carriage during threading. The gearbox selects ratios for feeds or thread pitches; its chart tells you which control combinations produce each ratio.

Choose workholding for the shape and the surface that must run true

Running true means the reference surface is centered on the spindle axis, with little measured runout. Gripping a part does not automatically establish that alignment.

Read the role before choosing the device. A setup can combine location, grip, drive and support. Support is not the same as drive, and gripping a surface does not by itself establish that it runs true.

Three-jaw scroll chuck

Moves its jaws together for quick gripping of round or suitable hexagonal stock. Self-centering is convenient, but does not promise zero runout, especially after removing and replacing a part.

Four-jaw independent chuck

Moves each jaw separately. Useful for square or irregular work, intentional offsets, or indicating an existing surface true. Adjustment takes more time.

Collet

Grips around a matching stock shape over a limited size range. Useful for repeated work and small diameters; choose the correct collet and its permitted clamping range.

Centers and drive dog

Centers locate work through prepared center holes. A dog clamped to the work transmits torque from a drive plate; the centers provide support. Useful when several surfaces must share the center-hole axis or the work must be removed and returned.

Faceplate

Provides slots or mounting features for clamping work that does not suit chuck jaws. The fixture must locate the intended axis and account for the off-center mass.

Steady rest

Mounts on the bed and supports a long workpiece at a fixed position. It can support work when the end must remain accessible for drilling or boring.

Follow rest

Mounts to the carriage and travels with the tool. It supports slender work near the cut to reduce bending under cutting force. Its support contacts must suit the diameter being supported.

Supporting detail: Addendum 11 — Reference examples for these mechanisms.

For why a chuck key must never remain in the chuck, and for rotating-work precautions, see Machine Hazards and Housekeeping. See Personal Protective Equipment and Metal Chips and Swarf for protection and chip handling.

Match tool travel to the feature, and set the edge on center

Facing feeds across an end to establish a plane perpendicular to the axis. Straight turning feeds parallel to the axis to make a cylinder. Shoulder turning joins a cylindrical diameter to a step face; the tool needs clearance to reach both surfaces without its holder or unused edge contacting the work.

Center drilling prepares the seat for a supporting center. It is not automatically the best starting method for every drill. Tailstock drilling makes an axial hole; reaming removes a controlled small allowance to improve hole size and finish. Select that allowance from the reamer maker. A reamer generally follows the existing hole, so it is not a reliable way to correct a misplaced hole. Boring uses a single-point tool to enlarge an existing hole and establish its surface relative to the spindle axis.

Grooving makes a recess; parting continues a similar radial cut until the part separates. Chamfering makes a bevel at an edge. Form knurling presses a pattern into the surface and increases the diameter over the raised points; cut knurling is a different process.

Use spindle center height as the starting reference for ordinary turning and threading tools, then follow any tool-specific instruction. An off-center edge changes the effective rake and clearance. In facing, a tool that cannot reach the axis leaves a small central nub. Boring also needs clearance between the tool and the curved hole wall.

Supporting detail: Addendum 12 — Rake and chipbreakers depend on the whole cutting setup.

Continue with Turning Tapers and Single-Point Threading. Cutting speed and feed belong on Feeds and Speeds; dimensional acceptance and finish belong on Tolerances and Fits and Surface Texture and Finish.

A lathe spins the work and moves the tool on two slides

In ordinary turning the work rotates while the tool feeds along it or toward its center. This simulator models parts that are round about the spindle’s axis. The shape comes from where the tool is put against the turning work, and in what order.

Chuck

Grips the bar and turns with the spindle. The jaws hold one end; the tool works on the part of the bar that sticks out.

Carriage (Z)

Carries the tool along the bed, parallel to the axis. On this page Z minus is toward the chuck and Z plus toward the tailstock.

Cross slide (X)

Moves the tool straight toward or away from the axis. The simulator’s X readout is the diameter the tool would cut. On a real lathe, find out whether a dial or readout shows diameter or radius before you trust it.

Tailstock

At the far end of the bed, on the centerline. It holds the center drill, the drills and the countersink, which feed straight along the axis.

Z0

Where the drawing’s finished front face belongs. Every length on the drawings is measured from the front face.

Before using a real lathe, read Machine Hazards and Housekeeping. The chuck key stays in your hand until it is out of the chuck.

Each simulator tool has a defined job; its form knurl displaces metal

Facing, turning, drilling, threading and knurling are not the same action with a different shape of tool. Each tool reaches different places and moves in different ways.

Turning tool

The roughing tool supplied here has a 10° lead and a 0.008 in nose radius. Its angled edge reaches ahead of its readout point. Stopping an axial pass leaves an angled shoulder; leave allowance instead of running the nose to the finished shoulder plane.

Facing tool

A square, 1/16 in wide finishing blade set for radial feed. Put its left corner at the finished Z and feed X across the end or shoulder. Its actual sweep removes the allowance and leaves the face flat. Retract clear before moving Z. These are the simulator’s selected tools; other turning tools and settings can both turn and face.

Chamfer tool

A 90° point. Plunged at an edge, each side cuts a 45° chamfer.

Grooving and parting blade

Cuts only on its front edge. Plunged part of the way it makes a groove; plunged to the center, or into the hole, it parts the work off.

Center drill, drill, countersink

Fed from the tailstock along the axis. A center drill makes a small pilot and a 60° seat for a lathe center; a spotting drill has different starting geometry. The twist drill makes the hole and the countersink chamfers its mouth. Choose a real drill’s starting method and spot angle from its maker’s guidance.

Boring bar

Turns the inside of a hole that is already there, the way the turning tool works on the outside. Its bar has to fit in the hole.

Threading tools

Form tools with a 60° point, one for outside threads and one on a bar for inside threads. For a threading pass the carriage is driven by the leadscrew, so the tool moves one thread lead for every turn of the work; for the single-start threads here, lead equals pitch.

Knurling tool

A straddle head with two opposed forming wheels, with left-hand and right-hand diagonal teeth. Their axles lie parallel to Z; together they roll a diamond pattern. Gap Ø is a simulated gap/contact-diameter control. A real tool’s arm adjustment and locking are separate from cross-slide infeed. The picture shows the barrels and axles in side projection; the highlighted rims are the forming contact.

Tool shape and setting matter: Sherline’s tool-grinding guide describes cutting edges, clearance and form tools. The particular blade widths, nose radius and operating limits used here are declared teaching choices, not specifications for every lathe tool.

Most parts start with a facing cut and end with parting

More than one order can make the same part, and the simulator accepts any order that gets there. Some orders are still better than others, for reasons you can see in the work.

• Face first. The faced end is the datum: every length on the drawing is measured from it. A sawn end is neither flat nor square to the axis.
• Rough, then finish. A large step comes off in several passes, and only the last one goes to the size on the drawing. On the stepped pin, stop the roughing passes 0.040 in short of each shoulder, retract clear and change to the facing tool. With its left corner at the final shoulder Z, feed X to the smaller diameter. A deeper shoulder needs more clearance for the angled edge; the facing blade can remove its allowance in slices up to 0.0625 in wide.
• Drill, then bore to size. The boring bar needs a hole its bar fits in. A center drill is available here to explore its pilot and center-seat shape, but it is not a universal prerequisite for drilling. On a real machine, use the starting method recommended for the following drill.
• Heavy work before thin sections. Knurling pushes hard on the work. Knurling before the thin sections next to it are turned keeps the work stiff while it happens.
• Make room for the threading tool. A thread needs somewhere for the tool to stop: a relief groove, or a stop short of the shoulder. Chamfer the end first so the thread starts on a clean edge.
• Chamfer the back edge before parting. Once the part is cut off, its back edge is out of reach without a second setup.
• Part off last. The part falls free, and anything not done to it by then needs another setup.

The small Chuck end circle is a separate axial view, looking from the tailstock toward the chuck. Its forward-rotation arrow and animation run counterclockwise in that view. The main picture is longitudinal, not a view along the spindle. See the viewpoint diagram in Haas’s spindle-direction training, page 16.

A thread is cut in several passes along one helix

For a threading pass the carriage is coupled to the leadscrew, so the tool advances exactly one lead for every turn of the work. For the single-start threads here, that is one pitch: 1/16 in for 16 threads per inch. Every pass follows the same helix, so every pass deepens the same groove.

The section uses a schematic thread envelope. Its unhatched bands lie between the surviving crests and dashed roots; they are not solid annular thread teeth. A real single-start helix intersects opposite sides half a pitch apart. The model samples a thread profile for depth checks and preserves its material envelope for later cuts and parting. The carriage still stops at the requested Z, even between full turns. Sandvik explains the lead/pitch relation for single- and multi-start threads.

• A little deeper each pass. The simulator allows 0.015 in of infeed per pass outside and 0.012 in inside. The thread is done when its roots reach the root diameter on the drawing.
• Back out before you come back. At the end of a pass the tool is still in the groove. Bringing the carriage back without backing the tool out would cut the crests off.
• Keep the pitch. A pass at another pitch cuts a second helix across the first: a crossed thread.
• Leave somewhere to stop. The tool runs into a shoulder unless a relief groove gives it room, which is why the thumb screw has one.

Supporting detail: Addendum 13 — How a manual lathe keeps every pass on one helix.

A form knurl moves metal instead of cutting it

The knurling tool makes no chips. Its wheels press a pattern into the turning work, and the metal they push aside has to go somewhere: it rises between their teeth. The diameter over the points ends up larger than the blank was.

Blank

The diameter turned before knurling. On these drawings it is not given: the knurled size is, and you work back to the blank.

Full points

The wheels pressed deep enough that the diamond points are fully formed. Too shallow leaves flat tops; pressing past full depth crushes and flakes the points.

Over the points

The knurled diameter, measured across the crests.

In the simulator the roots sink exactly as far as the crests rise, 0.010 in each at full depth, so a full knurl adds 0.020 in to the diameter. A real knurl’s growth depends on its pitch, the material and how hard it is pressed.

This paired-wheel forming arrangement supports feeding along Z after engagement. Dorian’s straddle setup instructions (H-19) and paired diagonal-wheel example (H-48) describe that combination. The drawing is a generic teaching head, not a dimensioned catalog tool or a setup instruction for a particular machine.

Count the teeth to find the speed

The driver supplies motion; the driven gear receives it. For one external gear mesh, each tooth passing on the driver advances the driven gear by one tooth space. A gear with twice as many teeth needs twice as many passing teeth to complete a turn.

This lesson uses reduction ratio i = input speed ÷ output speed, with speed magnitudes. A 2:1 reduction means two input turns for one output turn. Ratios above 1 reduce speed; ratios below 1 increase it. At zero speed, use tooth counts to find the ratio; do not divide 0 by 0.

Notation map: this page's original equations use N for teeth and n for speed. The course uses n for teeth, ω for angular velocity and τ for torque. Thus page N = course n; page speed n is written ω in the additions below. GR and i name the same reduction ratio.

In course notation, using magnitudes: GR = nout/nin = dout/din = ωin/ωout = τout/τin for an ideal single pair. Here d is pitch diameter; the torque equality assumes no losses. For a compound train, multiply the stage ratios; the first and last tooth counts alone do not give the overall ratio.

Supporting detail: Addendum 14 — Why tooth counts work, and what the dashed circles mean.

An idler and a compound shaft do different jobs

Same shaft means the same angular speed. A large B and a small C fixed to one shaft make the same number of turns in the same direction. Their rim speeds differ because their radii differ. They do not mesh with each other.

In the compound example, 20 → 40 teeth halves the speed. A second 20 → 40 stage halves it again: 120 → 60 → 30 rpm. The two external meshes make the final output turn in the same direction as the input.

An idler is not another reduction stage. Drop its tooth count when finding the end-to-end ratio, but count every external mesh for direction: odd means opposite; even means the same, viewed from the same end of the parallel shafts. Do not drop a gear that shares a shaft with a different gear in a compound train.

More torque costs speed; it does not create power

Torque is turning effort. In this ideal, lossless train at steady load, output torque magnitude = input torque magnitude × reduction ratio. A 2:1 reduction changes 120 rpm and 2 N·m into 60 rpm and 4 N·m. The 4:1 compound example gives 30 rpm and 8 N·m.

Rotational power is torque × angular speed: P = T × 2πn/60 when T is in N·m and n is in rpm. Both sides of either example carry 25.13 W ideally. Real friction and other losses leave less output power. Tooth strength, bearings, shafts, lubrication and the motor all limit usable torque.

At zero speed, mechanical power is zero. A loaded, stationary gear train can still carry torque. The lab shows ideal static torque balance in that case; it does not model motor stall behavior or promise a safe load.

Supporting detail: Addendum 15 — Primary references and model boundaries.

Connect the gears to Angular Motion, Rotation and Linear Speed and Torque.

Stage efficiencies multiply; losses accumulate

Each stage receives only the power that survived the stage before it. Use decimal efficiencies and multiply: η_total = η₁ × η₂ × η₃. Never add or average them. See Power and Efficiency for the general meaning of efficiency.

At 98% per stage, three stages give 0.98³ = 0.941192: about 5.88% total loss, not 6%. Fewer, higher-quality stages often beat many cheap stages for efficiency, provided they can meet the ratio and load requirements.

Supporting detail: Addendum 16 — Why adding losses is only an approximation.

Positive drives keep the speed ratio; losses reduce torque

A positive drive keeps input and output linked in a fixed ratio without slipping. Gears, chains and timing belts are positive drives. A slipping flat belt or V-belt is not. Follow Rotation and Linear Speed for the connection from rotation to belt travel.

The teeth still set the speed exactly in this model. Efficiency reduces output torque from its ideal value. It does not reduce output rpm as well. Use matching torque units on both sides: lbf·ft or N·m. The course conversion is 1 rpm ≈ 0.1047 rad/s when angular speed in rad/s is needed.

Supporting detail: Addendum 17 — Follow both stages of one loaded train.

Count stages for ratio, meshes for direction and stated losses

For a simple train A → I → B, the idler cancels from (NI/NA) × (NB/NI) = NB/NA. The two external meshes still reverse direction twice.

Follow the loss assumption in the problem. Real meshes lose some power, but a problem may explicitly ignore it. If every actual mesh is 96% efficient, A → I → B has ηtotal = 0.96². If a whole stage including its idler is assigned 96%, use that stage value once. If η = 1.00 is stated, ignore losses. Do not infer the loss count from the reduction-stage count when an idler is present.

A size tolerance gives two limits

Manufacturing produces variation. For each diameter in this lab, the drawing gives a size between two limits. A measured diameter inside that interval passes this size check.

Nominal size

The size a feature is named by, such as Ø0.7500 in. Ø means diameter. Every limit is measured from this number.

Deviation

How far a limit sits above (+) or below (−) nominal. +0.0010 puts a limit 0.0010 in above it.

Limits

Nominal plus each deviation: the largest and smallest sizes that pass inspection. Ø0.7500 +0.0010 / 0.0000 means anything from 0.7500 in to 0.7510 in.

Tolerance

The width of that range: largest limit minus smallest limit. Here, 0.0010 in.

Clearance is the hole size minus the shaft size

Put a shaft in a hole and the number that decides the fit is the difference between their two diameters.

clearance = hole size − shaft size

• Positive: the hole is bigger. There is a gap, and the shaft slides in.
• Negative: the shaft is bigger. That is interference: on paper the parts overlap, so the shaft has to be pressed in, or it does not go at all.
• Zero: exactly the same size, called line-to-line. No gap and no overlap.

Clearance is measured across the whole diameter. With the shaft centred in the hole, the gap you would see on each side is half of it:

gap on each side = clearance ÷ 2

Three kinds of fit, decided by the two worst cases

You do not have to check every pair of parts a drawing allows. Two pairs settle it: the tightest and the loosest.

Tightest legal pair

The smallest hole with the largest shaft. Its clearance is the least any good pair can have:
hole minimum − shaft maximum

Loosest legal pair

The largest hole with the smallest shaft. Its clearance is the most any good pair can have:
hole maximum − shaft minimum

The zero cases are deliberate. When the tightest pair comes out at exactly zero, every good pair either has a gap or just meets, so this page counts it as a clearance fit and the lab marks it zero at the limit. The same goes the other way for interference.

A surface has lay, waviness and roughness

Every manufactured surface carries marks from the process that made it. Surface texture describes those marks: which way they run, how far apart they are, and how tall they stand.

Roughness

The finest, closely spaced marks, such as the feed marks a cutting tool leaves at each pass or the scratches of abrasive grit.

Waviness

A longer, gentler undulation that the roughness sits on, for example from vibration or deflection while the part was made.

Lay

The direction of the main surface pattern, set by how the tool or the part moved.

Form

The overall shape, such as a face that is slightly curved. Size and geometric tolerances control form; surface texture is what is left on top of it.

Ra, Rz and Rt read the roughness differently

All three come from the same roughness profile. They answer different questions about it. This lab uses the older ISO 4287 convention with five sections for Rz; the drawing-symbol comparison separately shows older and current graphics.

Ra

The average distance of the roughness profile from its mean line over the evaluation length. Peaks and valleys count alike.

Rz

The average of the sections’ peak-to-valley heights. Each section counts once, whatever is in it.

Rt

The largest peak-to-valley height over the whole evaluation length: the single highest peak to the single deepest valley.

Ra = average of |roughness| over the evaluation length

Rz = (Z1 + Z2 + Z3 + Z4 + Z5) ÷ 5

For the trace above: Ra 1.55 µm; Rz = (6.55 + 6.56 + 6.70 + 6.57 + 6.87) ÷ 5 = 6.65 µm; Rt 7.10 µm.

The values are in micrometres (µm). They can also be given in microinches (µin): one inch is exactly 25.4 mm, so 1 µin is exactly 0.0254 µm, and Ra 1.6 µm is 63.0 µin.

Same Ra, different surfaces

These three roughness profiles all have Ra 1.6 µm. They are not the same surface. All three plots use the same height scale.

• Ra alone cannot tell these apart.
• Rz separates the rounded marks from the other two, but not flat tops from narrow peaks.
• Where the extremes sit, above or below the mean line, separates those two.

One number does not describe a surface. That is why a drawing names the parameter, not just a value.

Reading a surface texture symbol

The symbol’s point touches the line that represents the surface in a drawing view. Its shape says how the surface may be made; the text beside it says what texture is required.

Current or older

An ISO 21920-1 symbol carries a short separate dash above the short leg, touching neither leg. The older ISO 1302 graphic has none, so the familiar older marks are not the current symbols unchanged.

The requirement

The parameter and its limit, such as Ra 3.2, sit below the long line, to the right of the long leg, in both.

The lay

In an ISO 21920-1 callout the process and the lay sit above the long line. In the older symbols the lay symbol sits beside the long leg, below the line.

A complete specification can state more than this page draws, such as the measuring direction. The process mark is a requirement about how the surface is made; a profile measurement checks the texture, not whether material was removed.

Lay symbols belong to the drawing view

A lay symbol says which way the marks run. = and ⊥ are judged against the plane of projection of the view the symbol is drawn in, not against the page or the screen.

The first two figures are the same surface. Its marks run front to back: parallel to the right side view’s plane of projection, so = there, and perpendicular to the front view’s, so ⊥ there. The arrow shows which way each view looks.

Lay and trace direction are different things. The lay says how the marks run. The trace direction says how they were measured; it is usually across the lay unless the drawing specifies one.

The lay symbols and meanings here are those of ISO 1302:2002.