Skip to content
Academy

CNC machining glossary

Shop-floor terms explained with their formula, a worked example, typical values and a practical tip. Each term comes with its name in Spanish, English, German, Italian, Portuguese and French, so you can read any catalog. 250 terms

Do you know it? Test yourself with the machining quiz: a new challenge every day and a leaderboard.

#

5-axis machining

Machine

ES
Mecanizado en cinco ejes
DE
5-Achs-Bearbeitung
IT
Lavorazione a 5 assi
PT
Maquinagem em 5 eixos
FR
Usinage 5 axes

Machining with three linear axes and two rotary ones (tilting table or head) to reach five faces in one setup or to tilt the tool. It can be positional (3+2) or continuous (simultaneous).

Example

3+2 on Heidenhain: PLANE SPATIAL SPA+0 SPB+45 SPC+0 tilts the plane 45° about Y; on Siemens it is done with CYCLE800. In continuous mode, to keep the tip: M128 on Heidenhain and TRAORI on Siemens.

On the shop floor

The kinematics (rotation centers of the table or head) must be measured and up to date. On Heidenhain, the KinematicsOpt cycles measure and correct it by probing a calibration ball.

A

Abbe principle

Measurement

Calculator
ES
Principio de Abbe
DE
Abbesches Prinzip
IT
Principio di Abbe
PT
Princípio de Abbe
FR
Principe d'Abbe

To measure without tilt error, the instrument's scale must be in line with the dimension being measured. If they are apart, any play that tilts the probe is amplified.

Example

Caliper with the slider tilted 0.01 mm over 50 mm, measuring with the tip of 40 mm jaws: e = 40 × 0.01 / 50 = 0.008 mm of error without you noticing.

Typical values

The caliper does not satisfy the principle, because the scale sits to one side of the tips: that is why the measuring force and measuring with the jaw tips give large errors.

On the shop floor

With the caliper, measure as close as possible to the beam, at the base of the jaws, and without squeezing hard: the force is what tilts the slide.

Absolute and incremental coordinates

CNC programming

ES
Coordenadas absolutas e incrementales
DE
Absolut- und Inkrementalmaß
IT
Coordinate assolute e incrementali
PT
Coordenadas absolutas e incrementais
FR
Coordonnées absolues et incrémentales

Two ways of giving the program dimensions: in absolute (G90) each point is measured from the work origin; in incremental (G91), from the tool's previous position.

Example

Three holes every 20 mm from X10: in absolute, G90 X10 · X30 · X50; in incremental, after positioning at X10, G91 X20 · X20. On a Fanuc lathe incremental uses U and W; in Siemens, X=IC(20).

On the shop floor

A G91 left active is a classic: the next block or program takes the dimensions as jumps and the machine runs far away. Start every program with a safety block that includes G90.

Aluminium alloys

Materials

ES
Aleaciones de aluminio
DE
Aluminiumlegierungen
IT
Leghe di alluminio
PT
Ligas de alumínio
FR
Alliages d'aluminium

Shop aluminum is almost never pure: it is alloyed for strength. It is designated with four digits, such as EN AW-6082, and a temper, such as T6.

Example

EN AW-6082-T6: solution heat-treated and artificially aged. T651 is also stretched to relieve stresses before aging, so it distorts less when machined.

Typical values

6082 is the strongest of the 6000 series and the most widely used in plate for machining; it has replaced 6061 in many applications. In T6 it machines well.

On the shop floor

Sharp, polished positive inserts to avoid built-up edge, and high vc: it improves the cut without shortening edge life. In milling, always use coolant so the chips don't pack.

Annealing

Materials

ES
Recocido
DE
Glühen
IT
Ricottura
PT
Recozimento
FR
Recuit

Heating the metal and cooling it slowly to soften it, even out its structure or relieve stresses. Depending on the temperature and the goal there is softening anneal, stress-relief anneal and others.

Typical values

Stress relief in steel: 550-650 °C for 1-2 h and slow cooling. Softening: near A1, normally 700-900 °C depending on the alloy, for more than 4 h (Bodycote).

On the shop floor

If a part warps when released, do a stress-relief anneal after roughing and before finishing or grinding.

Austenitic stainless steel

Materials

ES
Inoxidable austenítico
DE
Austenitischer nichtrostender Stahl
IT
Acciaio inossidabile austenitico
PT
Aço inoxidável austenítico
FR
Acier inoxydable austénitique

Stainless steel with chromium and nickel of austenitic structure, such as 304 and 316. It is the typical ISO M group: soft when annealed, but it work-hardens a lot when machined, sticks and forms built-up edge.

Typical values

Relative machinability of about 60 % (duplex ones, 30 %). Adding sulfur improves machinability, but lowers corrosion resistance.

On the shop floor

Use sharp, positive edges, round inserts or a small lead angle against notch wear, the largest nose radius possible and always coolant.

Automatic tool changer

Machine

ES
Cambiador de herramientas
DE
Werkzeugwechsler
IT
Cambio utensile automatico
PT
Troca automática de ferramentas
FR
Changeur d'outils

Machining center system that stores the tools in a magazine and changes them in the spindle automatically when T and M06 are programmed. It can be carousel, double-arm or chain type.

Example

T12 M06 · T5: loads tool 12 and gets 5 ready while machining, so the next M06 takes less time. In Heidenhain, TOOL CALL 12 Z S3000 is enough; in Siemens, T12 M6.

Typical values

DN Solutions DNM vertical center: 1.2 s tool-to-tool and 3.2-4.1 s chip-to-chip; 30-tool magazine as standard, with a 40 or 60 option.

On the shop floor

Don't put tools in the magazine that are longer, heavier or wider than the machine manufacturer allows; check its magazine data before loading them.

B

Backlash

Machine

µm
ES
Holgura
DE
Umkehrspiel
IT
Gioco d'inversione
PT
Folga de inversão
FR
Jeu à l'inversion

Play an axis loses when changing direction: the motor turns but the table takes a few microns to move. It is typical of ball screw reversal and the feed drive transmission.

Example

With the dial indicator zeroed, you move X +0.100 mm and come back −0.100: if the indicator reads 0.006 mm instead of 0, there is 6 µm of backlash. The control compensates it with a value for each axis.

On the shop floor

In climb milling the cutting force pushes in the direction of feed: if the axis has backlash, the table advances in jerks and spoils the cut. Climb milling asks for a feed without play.

Ball nose end mill

Milling

Calculator
ES
Fresa de bola
DE
Kugelfräser
IT
Fresa sferica
PT
Fresa esférica
FR
Fraise hémisphérique

End mill with a half-sphere tip, used for 3D surfaces, molds and blend radii. Its real cutting diameter depends on how deep it cuts.

Example

Ø 10 mm ball (R = 5 mm) with ap = 0.5 mm: Deff = 2 × √(0.5 × 9.5) ≈ 4.36 mm. For 150 m/min: n ≈ 150 × 1000 / (π × 4.36) ≈ 10950 rpm, not ≈ 4775 rpm.

On the shop floor

At the center of the ball the cutting speed is zero and the edge drags. Sandvik recommends tilting the spindle or the part 10-15° so you don't cut with the tip.

Ball screw

Machine

Calculator
ES
Husillo de bolas
DE
Kugelgewindetrieb
IT
Vite a ricircolo di sfere
PT
Fuso de esferas
FR
Vis à billes

Screw with a nut in which balls roll, which converts the motor rotation into the feed of each axis with almost no friction. Its lead and preload set the speed and the play of the axis.

Example

With a 10 mm lead screw, each motor turn moves the axis 10 mm. For a 30 m/min rapid you need n = 30 × 1000 / 10 = 3000 rpm of motor (with direct coupling).

Typical values

Accuracy grades from C0 (the most precise) to C10, according to JIS B 1192 (ISO 3408). Preload, with a double nut or slightly larger balls, removes axial play and gives more rigidity.

On the shop floor

Don't just raise the preload: too much shortens life and generates heat. THK advises not exceeding 10 % of the dynamic axial load rating (Ca).

Bar feeder

Machine

ES
Alimentador de barra
DE
Stangenlader
IT
Caricatore di barre
PT
Alimentador de barras
FR
Embarreur

Equipment that pushes the bar through the lathe spindle and loads a new one when it runs out. It lets you turn parts in series without an operator, one after another, from long bar stock.

Example

3000 mm bar, 40 mm part plus 3 mm parting width and 150 mm remnant: (3000 − 150) / 43 ≈ 66.3, that is, 66 parts per bar.

Typical values

Long bar: the LNS Express 346 loads 3200 or 4020 mm bars. Short bar: the LNS Quick Load Servo 105 works with bars from 300 to 1600 mm, for small and medium runs.

On the shop floor

The remnant the bar feeder leaves counts in the part calculation: on the LNS Express 346 it can reach 400 mm. Check your bar feeder's data before calculating.

Bevel protractor

Measurement

°
ES
Goniómetro
DE
Winkelmesser
IT
Goniometro
PT
Goniómetro
FR
Rapporteur d'angle

Instrument with two arms and a circular scale that measures the angle between two faces, such as a chamfer or a taper. The universal type has a vernier to read minutes.

Example

The main scale reads 32° and the seventh line of the 5' vernier lines up: 7 × 5' = 35', that is, 32° 35'. In decimal, 35 / 60 ≈ 0.58, so 32.58°.

Typical values

Mitutoyo vernier ones (187 series) read 5'. The 187-501 digital displays in degrees and minutes, in 1' steps, or in hundredths of a degree (0.01°), with a maximum permissible error of 2'.

On the shop floor

Don't confuse resolution with accuracy: even though the digital shows minutes, its permissible error is 2'. For tolerances of a few minutes you need another measuring method.

Block skip

CNC programming

ES
Salto de bloque
DE
Satz ausblenden
IT
Salto blocco
PT
Salto de bloco
FR
Saut de bloc

Block that starts with a slash (/) and that the control skips when the operator turns on the block skip switch. It lets you keep parts in a program that are only done sometimes.

Example

/M00 after roughing: with block skip off, the machine stops and you measure the first part; in series you turn it on and it runs straight through. Fanuc, Siemens and Heidenhain use the same /.

Typical values

Fanuc: up to 9 levels (/1 to /9), depending on the machine. Siemens: up to 10 (/0 to /9). On Fanuc, an /M30 or /M99 with the skip active is not end of program.

On the shop floor

If the skipped block carries a modal (G41, F, G43), skipping it means that modal is not activated and what follows changes. And the control reads blocks ahead: change the switch before it arrives.

Bore gauge

Measurement

ES
Alexómetro
DE
Innenmessgerät
IT
Alesametro
PT
Comparador de interiores
FR
Alésomètre

Bore gauge: a movable plunger and a fixed anvil transmit the diameter to a dial. It is zeroed on a setting ring or with a micrometer and then measures the difference.

Example

Zeroed on a 40.000 mm ring, inside the bore the needle stays 0.012 mm toward the larger-diameter side: the diameter is 40.000 + 0.012 = 40.012 mm.

Typical values

Reading of 0.01 or 0.001 mm. One body covers, for example, 18 to 35 mm by changing anvils and washers.

On the shop floor

Rock the bore gauge inside the hole and read the needle's reversal point: it is the smallest diameter, when the gauge is perpendicular to the axis. Do the same when zeroing it on the ring.

Boring

Turning

ES
Mandrinado
DE
Ausdrehen
IT
Alesatura
PT
Mandrilagem
FR
Alésage

Turning the inside of an existing hole to bring it to size, center it or improve its finish. It is done with a boring bar, which works as a cantilever inside the hole.

Typical values

Maximum overhang in turning according to Sandvik: steel bar 4 × D, carbide 6 × D, anti-vibration steel up to 10 × D and carbide-reinforced anti-vibration up to 14 × D.

On the shop floor

Use the thickest and shortest bar that fits and a nose radius smaller than the depth of cut. Grooving and threading allow less overhang than turning because the radial force is greater.

Boring bar

Turning

Calculator
ES
Barra de mandrinar
DE
Bohrstange
IT
Barra di alesatura
PT
Barra de mandrilar
FR
Barre d'alésage

Cylindrical toolholder that works cantilevered inside the hole. Its diameter, material and overhang decide how much it deflects, and with it the size and finish of the bore.

Example

Steel bar (E ≈ 206000 N/mm²) Ø 16 mm, 64 mm overhang and 200 N: δ ≈ 0.026 mm. Carbide (E ≈ 600000 N/mm²), ≈ 0.009 mm. Going to Ø 20 mm divides the deflection by ≈ 2.4.

Typical values

Maximum overhang in turning (Sandvik): 4 × D in steel, 6 × D in carbide, 10 × D in anti-vibration steel and 14 × D in carbide-reinforced anti-vibration.

On the shop floor

Choose the thickest bar that leaves room for the chip between bar and hole, and with the smallest possible overhang. Bring the coolant to the cutting zone.

Boring head

Drilling and threading

ES
Cabezal de mandrinar
DE
Ausdrehkopf
IT
Testina per alesare
PT
Cabeça de mandrilar
FR
Tête d'alésage

Milling toolholder with a cutter that moves radially by turning a graduated screw. It lets you bore holes to exact size on the machining center, adjusting by hundredths.

Example

You measure Ø 39.96 and want Ø 40.00: 0.04 mm short on diameter. If each division is 0.01 mm on diameter, turn 4 divisions; if it is 0.01 mm on radius, only 2.

Typical values

Sandvik CoroBore 825: 50 graduations of 0.01 mm on diameter and a vernier of 0.002 mm; one turn moves 0.25 mm on radius. Check whether your head reads diameter or radius.

On the shop floor

Always adjust from smaller to larger diameter; if you overshoot, back off too far to remove the backlash and open up again. Lock the slide after each adjustment and check the size.

Brass

Materials

ES
Latón
DE
Messing
IT
Ottone
PT
Latão
FR
Laiton

Copper and zinc alloy. Free-machining brass contains lead, which does not dissolve in the metal and greatly improves cutting: it is one of the most grateful materials for turning and drilling.

Example

CuZn39Pb3 (CW614N): 57-59 % copper and 2.5-3.5 % lead, and the rest zinc. With 58 % copper and 3 % lead, the zinc is 100 − 58 − 3 = 39 %.

Typical values

CW614N has a machinability rating of 100 %: it is the reference against which the rest of the copper alloys are compared.

Built-up edge

Tools

ES
Filo recrecido
DE
Aufbauschneide
IT
Tagliente di riporto
PT
Aresta postiça
FR
Arête rapportée

Workpiece material that welds under pressure onto the cutting edge and changes its shape. It worsens the finish, changes the size and, when it breaks off, tears pieces from the edge.

Typical values

It occurs with low cutting temperature (low speed or feed) and materials that stick, such as stainless steels and low-carbon steels (Sandvik).

On the shop floor

Raise the cutting speed or feed and use a sharper edge. If it persists, Sandvik proposes cermet for materials that smear the edge.

Bull nose end mill

Milling

Calculator
ES
Fresa tórica
DE
Torusfräser
IT
Fresa torica
PT
Fresa tórica
FR
Fraise torique

Flat-bottom end mill with corners rounded by a radius. It withstands much more than a sharp-corner end mill and leaves less scallop than a flat one; widely used for mold roughing.

Example

Ø 12 mm end mill with a 2 mm radius and ap = 0.5 mm: Deff = 12 − 4 + 2 × √(0.5 × 3.5) ≈ 10.65 mm.

On the shop floor

Calculate rpm with the effective diameter, not the nominal one: with low ap the actual cutting speed is lower than it seems and the edge works below what was planned.

Burr

Milling

ES
Rebaba
DE
Grat
IT
Bava
PT
Rebarba
FR
Bavure

Deformed material left stuck to the edge where the tool exits. It cuts when handling the part, falsifies measurements and gets in the way in assemblies, so it has to be removed or avoided.

Typical values

ISO 13715 states on the drawing the condition of edges: + allows excess material (the burr is one case), − requires removing material and ± admits both, always with its maximum dimension.

On the shop floor

To reduce it, Sandvik proposes large-radius inserts that enter at a small angle and a depth of cut smaller than the radius; in stainless and superalloys it is worse. Add a chamfering pass to the program.

C

C axis

Machine

ES
Eje C
DE
C-Achse
IT
Asse C
PT
Eixo C
FR
Axe C

Control of the lathe spindle rotation as a positionable axis in degrees around Z. With live tooling it allows off-center drilling and milling of flats, keyways and slots.

Example

With the C axis activated (M14 on the standard Fanuc table, M52 on an EMCO lathe), G00 C0 · C90 · C180 · C270 positions the part for four holes on the face at 90°.

On the shop floor

To mill contours on the face or on the cylinder, positioning C is not enough: you need polar or cylindrical interpolation, G12.1 or G07.1 on Fanuc and TRANSMIT or TRACYL on Siemens.

Calibration

Measurement

ES
Calibración
DE
Kalibrierung
IT
Taratura
PT
Calibração
FR
Étalonnage

Comparing an instrument against a standard of known uncertainty to find out how much it is off. The standard, in turn, is calibrated against others up to the national standard: that is traceability.

Example

A micrometer reads 25.003 mm on a 25.000 mm gauge block: its error at that point is 25.003 − 25.000 = +0.003 mm, and it is compared with the maximum allowed.

Typical values

There is no fixed interval. The ILAC-G24 / OIML D 10 guide starts from the manufacturer's recommendation, the use, the environment and the uncertainty you need, and then adjusts the interval with the history.

On the shop floor

Calibrating is not adjusting: it only tells you how far off the instrument is. And don't leave fixed intervals unreviewed: the ILAC-G24 guide does not consider them reliable.

Canned cycle

CNC programming

ES
Ciclo fijo
DE
Bearbeitungszyklus
IT
Ciclo fisso
PT
Ciclo fixo
FR
Cycle fixe

Block that sums up a repetitive operation, such as drilling, tapping or roughing, in a single line. It is programmed once and repeated at every X Y position that follows, until canceled with G80.

Example

G00 X0 Y0 · G98 G83 Z-30 R2 Q5 F120 · X20 · X40 · G80. Drills three holes to Z-30 with 5 mm pecks. On Siemens it is CYCLE83 and on Heidenhain, cycle 200 or 205.

On the shop floor

Forgetting G80: the next positioning drills again where it shouldn't. Also watch G98 (returns to initial plane) and G99 (returns to R) if there are clamps between holes.

Case hardening

Materials

ES
Cementado
DE
Einsatzhärten
IT
Cementazione
PT
Cementação
FR
Cémentation

Treatment that enriches the surface of a low-carbon steel, such as 16MnCr5, with carbon and then hardens it. The surface ends up very hard and the core tough.

Example

You ask for 0.8 mm case depth and leave 0.2 mm per side for grinding after hardening: after grinding, 0.8 − 0.2 = 0.6 mm of useful case remains.

Typical values

16MnCr5: case-hardened at 880-980 °C and, tempered at 150-200 °C, it reaches about 60.5-62 HRC at the surface (Lucefin). The case is usually less than 2 mm deep (Bodycote).

On the shop floor

Machine it soft and leave stock for grinding after hardening. If you need to weld, do it in the annealed state and before case hardening.

Cemented carbide

Tools

ES
Metal duro
DE
Hartmetall
IT
Metallo duro
PT
Metal duro
FR
Carbure

Sintered material of tungsten carbide particles bonded with a cobalt-rich binder. The amount of cobalt sets the toughness of each grade and its resistance to deformation.

Typical values

ISO 513 groups grades by material (P, M, K, N, S, H) with a number: lower, more wear-resistant; higher, tougher. Only P grades reach 45 and 50.

On the shop floor

It is sensitive to thermal shock: in interrupted cuts Sandvik even recommends removing the coolant to avoid thermal cracks in the edge.

Centre height

Turning

ES
Altura de centro
DE
Mittenhöhe
IT
Altezza del centro
PT
Altura ao centro
FR
Hauteur de centre

Vertical position of the cutting edge relative to the rotation axis. The edge must sit exactly at axis height; otherwise the real cutting angles change and problems appear when reaching the center.

Typical values

Sandvik asks for ±0.1 mm, especially when parting off to the center. Below it the nib increases and the edge may break; at exact center, it breaks on pushing and the flank wears quickly.

On the shop floor

With long blade overhangs, Sandvik advises setting the edge at most 0.1 mm above center to compensate for the tool deflecting downward when cutting.

Ceramic cutting tool

Tools

ES
Cerámica de corte
DE
Schneidkeramik
IT
Ceramica da taglio
PT
Cerâmica de corte
FR
Céramique de coupe

Cutting material without metal binder: aluminum oxide, mixtures with carbides, whisker reinforcement, silicon nitride or SiAlON. It withstands very high temperatures and cuts much faster than carbide, but it is brittle.

Typical values

In superalloys, Sandvik gives up to about 300 m/min in turning and up to 1000 m/min in milling. In cast iron, Kyocera tests its silicon nitride at 600 m/min on a lathe, dry.

On the shop floor

It needs a rigid, vibration-free machine and an edge with a protective chamfer. In turning, plenty of coolant and no interrupted cuts; in milling, dry. In superalloys, round inserts and a light depth of cut prevent notch wear.

Cermet

Tools

ES
Cermet
DE
Cermet
IT
Cermet
PT
Cermet
FR
Cermet

Carbide with titanium carbonitride, Ti(C,N), particles bonded with cobalt; the first cermets contained nickel. It keeps its edge a long time and leaves bright surfaces with very stable sizes.

Typical values

Finishing of stainless steel, ductile iron, low-carbon steels and ferritics (Sandvik). It is chosen where built-up edge causes problems.

On the shop floor

It withstands thermal shock worse than carbide: to avoid cracks and breakage, Sandvik recommends running it without coolant.

Chamfer mill

Milling

Calculator
ES
Fresa de chaflanar
DE
Fasenfräser
IT
Fresa per smussi
PT
Fresa de chanfrar
FR
Fraise à chanfreiner

Cutter with conical edges, normally 90° included (45° per side), for chamfering, deburring edges and countersinking. Its real cutting diameter depends on the depth at which it works.

Example

90° point cutter, at ap = 2 mm: Deff = 2 × 2 × tan 45° = 4 mm. For 100 m/min: n ≈ 7958 rpm; with the nominal Ø 12 it would come out ≈ 2653 rpm, three times less.

On the shop floor

Don't cut with the tip, where the speed is almost zero: go a little deeper and let the middle zone of the cone cut. Calculate rpm with the actual diameter at that height, not the nominal one.

Chatter

Cutting parameters

ES
Vibraciones o chatter
DE
Rattern
IT
Vibrazioni (chatter)
PT
Vibrações (chatter)
FR
Broutage

Vibration of the tool or the part during cutting that leaves regular marks on the surface and shortens edge life. It appears with long overhangs, non-rigid clamping or cutting data that fall in an unstable zone.

Example

4-flute cutter at 3000 rpm: the teeth hit 4 × 3000 / 60 = 200 times per second (200 Hz). If that frequency falls close to the tool's natural frequency, it vibrates.

Typical values

Usual causes: long overhang (in milling, more than 4 times the diameter), clamping far from the table, large nose radius, excessive ap or ae and a chip so thin that the edge rubs.

On the shop floor

First change the rpm: sometimes raising it by about 50 rpm is enough to reach stable cutting. Then shorten the overhang or use a differential-pitch cutter. Lowering the feed usually makes it worse, because the edge rubs.

Chip conveyor

Machine

ES
Transportador de viruta
DE
Späneförderer
IT
Trasportatore di trucioli
PT
Transportador de aparas
FR
Convoyeur à copeaux

Belt or auger that carries the chips out of the machine into a bin while the coolant returns to the tank. Without it, chips pile up on the bed and you have to stop to clean.

Example

On Haas, M31 starts the conveyor and M33 stops it. On other machines the codes are set by the manufacturer: look them up in the manual or in the M-code list.

Typical values

Hinged belt for large, long chips; with coolant filtration, down to 50 µm, if there are fine chips (LNS). On Haas lathes it is an auger.

On the shop floor

Haas warns that continuous use heats the motor: with settings 114 and 115 the conveyor starts at set intervals and runs only for a while.

Chip thickness

Cutting parameters

Calculator
h · mm
ES
Espesor de viruta
DE
Spandicke
IT
Spessore del truciolo
PT
Espessura da apara
FR
Épaisseur de copeau

Real thickness of the chip before it deforms, measured perpendicular to the cutting edge. It is what actually loads the edge and does not always match the programmed feed.

Example

With f = 0.3 mm/rev: with κr 95° the chip is h = 0.3 × sin 95° ≈ 0.3 mm; with κr 45°, h = 0.3 × sin 45° ≈ 0.21 mm.

On the shop floor

According to Sandvik, a chip that is too thin is the most common cause of poor performance and shortens tool life; one that is too thick overloads the edge and can break it. Adjust the feed to the thickness the manufacturer asks for.

Chip thinning

Cutting parameters

Calculator
ES
Adelgazamiento de viruta
DE
Spanausdünnung
IT
Assottigliamento del truciolo
PT
Afinamento da apara
FR
Amincissement du copeau

Effect by which the chip comes out thinner than the programmed feed, due to a lead angle below 90° or a width of cut below half the diameter. It forces you to raise the feed.

Example

End mill Ø 10 mm with ae = 1 mm: factor = 2 × √(0.1 − 0.01) = 0.6. For hex = 0.05 mm you need fz = 0.05 / 0.6 ≈ 0.083 mm. With κr 45°: fz ≈ 1.4 × hex.

On the shop floor

If you program the catalog fz with a small ae or 45° inserts, the tool works below its rated load: it rubs and wears out sooner. Compensate the feed.

Chip types

Cutting parameters

ES
Tipos de viruta
DE
Spanformen
IT
Tipi di truciolo
PT
Tipos de apara
FR
Types de copeaux

Shapes the chip takes depending on the material, feed, depth and chip breaker: from long unbroken ribbons to very short pieces. Its appearance is a good indicator of whether the cutting data are right.

Typical values

Bad: long ribbons that wrap around the part or the tool (low feed or low ap) or very short, stuck-together pieces, a sign of an excessively hard break that loads the edge.

On the shop floor

Long, tangled chip: raise the feed or ap, or use a tighter chip breaker. Very short, hard chip: lower the feed or use a geometry for higher feeds, or the insert will break sooner.

Chipbreaker

Tools

ES
Rompevirutas
DE
Spanformer
IT
Rompitruciolo
PT
Quebra-aparas
FR
Brise-copeaux

Shape of the insert face that bends the chip until it breaks into short pieces. It avoids long strings that wrap around the part and the tool.

Typical values

Each geometry has a working zone of feed and depth: finishing (small passes and feeds), medium and roughing (Sandvik). Outside its zone the chip does not break well.

On the shop floor

With feed too low you get stringy chips, flank wear and built-up edge. With feed too high you lose chip control and crater wear appears (Sandvik).

Circular interpolation

CNC programming

Calculator
ES
Interpolación circular
DE
Kreisinterpolation
IT
Interpolazione circolare
PT
Interpolação circular
FR
Interpolation circulaire

Arc motion at feed rate F: G02 clockwise and G03 counterclockwise, depending on the active plane (G17, G18 or G19). The arc is defined with its radius R or with the center I, J, K.

Example

From X0 Y0: G02 X20 Y0 I10 J0 F200 makes a half circle of radius R = √(10² + 0²) = 10 mm. G02 X20 Y0 R10 F200 gives the same arc.

On the shop floor

With R, an arc of more than 180° takes a negative R and a full circle is not possible: use I and J. In Heidenhain the center is given separately (CC X Y) and the arc with C X Y DR-.

Clearance and interference

Tolerances and surface finish

Calculator
µm
ES
Juego y apriete
DE
Spiel und Übermaß
IT
Gioco e interferenza
PT
Folga e aperto
FR
Jeu et serrage

Difference between the hole diameter and the shaft diameter. If the hole is larger there is clearance; if the shaft is larger there is interference, and the part is assembled by press fit or by heating.

Example

Ø 25 H7/p6: hole 25.000-25.021 and shaft 25.022-25.035 mm. Jmin = 25.000 − 25.035 = −35 µm and Jmax = 25.021 − 25.022 = −1 µm: interference of 1 to 35 µm.

On the shop floor

For shrink fitting, calculate how much the hole expands with temperature: you need more than the maximum interference, with some margin to go in without seizing.

Clearance angle

Tools

α · °
ES
Ángulo de incidencia
DE
Freiwinkel
IT
Angolo di spoglia inferiore
PT
Ângulo de folga
FR
Angle de dépouille

Angle between the flank face of the edge and the surface already cut. It prevents the tool from rubbing the workpiece below the edge.

Typical values

Second letter of the ISO code: N 0°, B 5°, C 7°, P 11°. Negative inserts (N) have 0°; once mounted in the tool holder, the actual clearance may differ from the nominal one.

On the shop floor

On a lathe, if the edge sits above center the clearance decreases and the flank wears quickly. Sandvik asks for center height within ±0.1 mm.

Climb milling

Milling

Drawing
ES
Fresado en concordancia
DE
Gleichlauffräsen
IT
Fresatura concorde
PT
Fresagem concordante
FR
Fraisage en avalant

Way of milling in which the tooth enters the material with a thick chip and leaves with a thin one, because the cutter rotation goes with the feed. It is the normal choice on CNC.

Typical values

With a normal right-hand cutter, contouring with compensation to the left of the material (G41) gives climb milling, according to the Haas programming manual.

On the shop floor

It gives a better finish and longer edge life, but pulls the cutter toward the part: if the table has backlash, the feed can jump and break the edge. In that case, conventional milling.

Coating

Tools

ES
Recubrimiento
DE
Beschichtung
IT
Rivestimento
PT
Revestimento
FR
Revêtement

Thin layer of hard material, such as TiN, TiAlN, TiCN or alumina, deposited on the edge by CVD or PVD. It increases wear resistance and protects the edge from heat and oxidation.

Typical values

CVD (TiCN and alumina): thick coating, steel turning with crater resistance. PVD (TiN, TiAlN): sharp, tough edges; solid end mills and drills and almost all threading (Sandvik).

On the shop floor

In low-silicon aluminum, Sandvik proposes uncoated carbide or with a thin coating and a sharp edge; with high silicon, PCD.

Coaxiality

Tolerances and surface finish

ES
Coaxialidad
DE
Koaxialität
IT
Coassialità
PT
Coaxialidade
FR
Coaxialité

Position tolerance that requires the axis of a diameter to lie within a cylinder of the stated diameter, centered on the datum axis.

Example

Coaxiality Ø 0.02 relative to A: the axis may deviate at most 0.01 mm from the axis of A, because the zone is a cylinder of Ø 0.02 mm.

On the shop floor

With a dial indicator, rotate the part on the datum: the difference between the maximum and minimum reading is the coaxiality value. If it swings 0.02 mm, the axis is offset 0.01 mm.

Collet

Turning

ES
Pinza de torno
DE
Spannzange
IT
Pinza
PT
Pinça
FR
Pince de serrage

Slotted sleeve that closes evenly around the bar when pulled or pushed. It grips the whole circumference, centers very well and opens quickly, ideal for bar work.

Typical values

Röhm gives a concentricity and repeatability of less than 0.01 mm on its CAPTIS-M collet chuck. The clamping range of each collet is a few tenths of a millimeter.

On the shop floor

Always use the collet for the bar diameter and work with calibrated bar: outside its clamping range, the collet loses force and centering.

Collet chuck

Tools

ES
Portapinzas
DE
Spannzangenfutter
IT
Mandrino portapinze
PT
Porta-pinças
FR
Mandrin à pinces

Tool holder that clamps cylindrical shanks with a slotted collet that closes when the nut is tightened. In the ER system (DIN 6499 / ISO 15488) each collet covers a small range of diameters.

Typical values

REGO-FIX ranges: ER11 0.5-7 mm, ER16 0.5-10 mm, ER20 1-13 mm, ER25 1-16 mm, ER32 2-20 mm, ER40 3-26 mm. Each collet spans 1 mm (0.5 mm on the small ones).

On the shop floor

First snap the collet into the nut until you hear the click and insert the shank more than 2/3 of the collet length. Tighten with its wrench, preferably a torque wrench, without extensions or a hammer (REGO-FIX).

Computer-aided manufacturing (CAM)

CNC programming

ES
CAM
DE
Rechnergestützte Fertigung (CAM)
IT
Fabbricazione assistita (CAM)
PT
Fabrico assistido por computador (CAM)
FR
Fabrication assistée par ordinateur (FAO)

Computer program that calculates toolpaths from the 3D model or the drawing and, with the post-processor, converts them into the code the machine understands, almost always G-code.

Example

For a pocket, the CAM stores in an intermediate file the tool, the operation type and the path of the cutter center; your machine's post-processor translates it into G-code.

On the shop floor

CAM doesn't know how the part is clamped or what is on your machine: simulate with the real workholding, check the first blocks and test the first cycle with the override low.

Constant surface speed

Cutting parameters

Calculator
ES
Velocidad de corte constante
DE
Konstante Schnittgeschwindigkeit
IT
Velocità di taglio costante
PT
Velocidade de corte constante
FR
Vitesse de coupe constante

Lathe mode (G96) in which the control changes the rpm according to the diameter to keep the same vc. It improves finish and tool life in facing and profiles.

Example

Facing with G96 S200 from Ø 80 to Ø 10 mm: starts at 200 × 1000 / (π × 80) ≈ 796 rpm and would end at ≈ 6366 rpm. That is why it is limited, for example G50 S3000.

On the shop floor

Always program the rpm limit before G96: G50 S… on Haas, LIMS=… on Siemens. To drill and tap at the center, switch to G97 with fixed rpm.

Contour milling

Milling

ES
Contorneado
DE
Konturfräsen
IT
Contornatura
PT
Fresagem de contorno
FR
Contournage

Milling the outer or inner profile of a part with the side of the cutter, following the drawing. It is programmed on the part contour with cutter radius compensation.

Typical values

Sandvik: in deep walls, ae ≈ 0.5 × D; in thin walls, leave 0.2-1 mm of stock per side for finishing. Climb milling as the first choice.

On the shop floor

Make the cutter roll into the cut, with a lead-in arc, so the chip always exits with zero thickness. If you enter head-on, the cutter leaves a mark on the wall.

Conventional milling

Milling

ES
Fresado en oposición
DE
Gegenlauffräsen
IT
Fresatura discorde
PT
Fresagem discordante
FR
Fraisage en opposition

Way of milling in which the tooth enters with almost zero chip thickness and leaves with a thick chip, because the rotation opposes the feed. The edge rubs on entry before it starts to cut.

Typical values

With a normal right-hand cutter, contouring with compensation to the right of the material (G42) gives conventional milling, according to the Haas programming manual.

On the shop floor

That rubbing burnishes and the next edge meets work-hardened material. Sandvik reserves it for machines with backlash, very uneven stock or ceramic inserts in superalloys.

Conversational programming

CNC programming

ES
Programación conversacional
DE
Dialogprogrammierung
IT
Programmazione conversazionale
PT
Programação conversacional
FR
Programmation conversationnelle

Way of programming at the control itself by filling in screens with drawings and data (diameter, depth, material) instead of writing G-code. The control generates the toolpath and often suggests the cutting data.

Example

Instead of G83 X20 Y0 Z-30 R2 Q5 F120, you choose 'deep drilling' and fill in Ø 8, depth 30, peck 5 and position X20 Y0. Examples of systems: Mazatrol on Mazak, ShopMill and ShopTurn on Siemens.

Typical values

Mazak introduced MAZATROL in 1981 as the first control with conversational programming; today it can generate the program from a 3D model made in CAD.

On the shop floor

ShopMill and ShopTurn programs carry the contour description added at the end of the file: if you copy or edit them as text, don't cut off that part.

Coordinate measuring machine

Measurement

ES
Máquina de medir por coordenadas
DE
Koordinatenmessgerät
IT
Macchina di misura a coordinate
PT
Máquina de medição por coordenadas
FR
Machine à mesurer tridimensionnelle

Machine that touches the part with a probe at many points and uses software to calculate diameters, distances, positions and geometric tolerances relative to the drawing datums.

Example

With a maximum error of 1.8 + L/300 µm, when measuring a length of 300 mm the permissible error is 1.8 + 300 / 300 = 2.8 µm.

Typical values

Maximum error according to ISO 10360-2, given as A + L/K µm: for example 1.8 + L/300 or 2.2 + L/300 µm depending on the probe, guaranteed between 18 and 22 °C.

On the shop floor

Let the part equalize to room temperature before measuring: a part fresh off the machine gives false measurements.

Coordinate rotation

CNC programming

ES
Giro de coordenadas
DE
Koordinatendrehung
IT
Rotazione delle coordinate
PT
Rotação de coordenadas
FR
Rotation de coordonnées

Function that rotates the coordinate system by an angle around a point. Used to machine a shape programmed straight on a part clamped at an angle or to repeat a contour at several angles.

Example

G68 X0 Y0 R30 · (contour) · G69. The point X50 Y0 lands at X = 50 × cos 30° ≈ 43.30 and Y = 50 × sin 30° = 25. On Siemens: ROT RPL=30; on Heidenhain: CYCL DEF 10 ROTATION with ROT+30.

Typical values

Positive angle, counterclockwise rotation. Fanuc rotates about the center you specify (or the current position) and Heidenhain about the active origin. Useful when the part is clamped slightly rotated.

On the shop floor

With G68 active, Fanuc does not allow G28 or origin changes (G54-G59, G92): cancel first with G69 and give the first move after G69 in absolute. On Heidenhain, cycle 10 cancels radius compensation.

Copper

Materials

ES
Cobre
DE
Kupfer
IT
Rame
PT
Cobre
FR
Cuivre

Very soft, ductile metal and a good conductor of heat and electricity. It is used in EDM electrodes, busbars and heat exchangers, and is the base of brass and bronze.

Example

Alloyed with zinc it gives brass (60-85 % copper and 40-15 % zinc); with tin (10-14 %) or aluminum (3-10 %), bronze.

Typical values

Sandvik includes it in ISO group N, the soft metals under 130 HB. Electrolytic copper is 99.95 % Cu.

Countersinking

Drilling and threading

Calculator
ES
Avellanado
DE
Kegelsenken
IT
Svasatura
PT
Escareamento
FR
Fraisurage

Cone made at the mouth of a hole to seat the head of a countersunk screw or to remove the sharp edge. It is made with a countersink or a spotting drill.

Example

Ø 20 mm countersink with a 90° tool: Z = 10 / tan(45°) = 10 mm measured from the theoretical tool tip.

Typical values

90° for metric countersunk head screws (ISO 10642); 82° for inch flat-head screws; 60° for center holes for the tailstock (DIN 333 drills).

On the shop floor

If the countersink has no real tip, the depth measured from the workpiece face is less than Z. Test first and adjust with the offset before running the batch.

Crater wear

Tools

KT · mm
ES
Desgaste en cráter
DE
Kolkverschleiß
IT
Usura a cratere
PT
Desgaste em cratera
FR
Usure en cratère

Hollow formed on the rake face by the rubbing of the hot chip. It appears mainly with high cutting speed or feed and is measured by its depth, KT.

Typical values

Criterion recommended by ISO: KT = 0.06 + 0.3 × f mm (with f = 0.3 mm/rev, about 0.15 mm). The Université de Lille notes give 0.10-0.20 mm as acceptable values.

On the shop floor

Lower the cutting speed or feed, choose a more positive geometry or a more wear-resistant grade. CVD alumina coatings resist cratering well (Sandvik).

Cubic boron nitride (CBN)

Tools

ES
CBN (nitruro de boro cúbico)
DE
Kubisches Bornitrid (CBN)
IT
Nitruro di boro cubico (CBN)
PT
Nitreto de boro cúbico (CBN)
FR
Nitrure de bore cubique (CBN)

Polycrystalline cubic boron nitride, with great hot hardness for cutting at very high speeds. It is brazed onto a carbide base for turning and milling hardened steels and gray cast iron.

Typical values

Finish turning of steels over 45 HRC; above 55 HRC, Sandvik gives it as the only tool able to replace grinding. Also fast roughing of gray cast iron.

On the shop floor

Use an edge with a chamfer: a wide one gives more security and allows more feed; a small one improves finish and size with less force and vibration (Sandvik).

Cutting force

Cutting parameters

Calculator
Fc · N
ES
Fuerza de corte
DE
Schnittkraft
IT
Forza di taglio
PT
Força de corte
FR
Effort de coupe

Component of the force that acts in the direction of the cutting speed, tangent to the workpiece in turning. It is the one used to calculate cutting power and torque.

Example

590 MPa steel, f = 0.2 mm/rev: manufacturer tables, kc ≈ 2940 N/mm². With ap = 3 mm, Fc = 2940 × 3 × 0.2 ≈ 1764 N. At vc = 200 m/min, Pc = 1764 × 200 / 60000 ≈ 5.9 kW.

Typical values

kc rises as feed drops: in 590 MPa steel it goes from about 2500 N/mm² with f = 0.4 mm/rev to about 3490 with f = 0.1 mm/rev.

On the shop floor

With Fc you know how hard the cut pushes against the insert and the workholding: if the part slips in the chuck or the jaw leaves marks, check the clamping pressure before lowering the depth of cut.

Cutting speed

Cutting parameters

Calculator
vc · m/min
ES
Velocidad de corte
DE
Schnittgeschwindigkeit
IT
Velocità di taglio
PT
Velocidade de corte
FR
Vitesse de coupe

Speed at which the cutting edge travels over the material surface. It is the starting data the tool manufacturer gives for each material; the revolutions are calculated from it.

Example

Turning Ø 50 mm at 1000 rpm: vc = π × 50 × 1000 / 1000 ≈ 157 m/min. To run at 200 m/min you would need n = 200 × 1000 / (π × 50) ≈ 1273 rpm.

Typical values

Haas starting values in turning with carbide inserts, by grade: steel 120-395 m/min, austenitic stainless 120-215, gray cast iron 180-450, wrought aluminum 490, titanium 45-100.

On the shop floor

If the edge wears quickly, lower vc first: according to Sandvik it weighs the most on edge life; feed weighs less and depth of cut, little.

Cutting temperature

Cutting parameters

°C
ES
Temperatura de corte
DE
Schnitttemperatur
IT
Temperatura di taglio
PT
Temperatura de corte
FR
Température de coupe

Temperature reached in the contact zone between chip and tool. It depends on cutting speed, feed and material, and it sets wear, edge life and which tool material is suitable.

Typical values

In titanium, which conducts heat very poorly, the heat stays in the cutting zone and punishes the edge; that is why it is machined with low vc (about 60 m/min in roughing) and plenty of coolant.

On the shop floor

Raising the feed makes the chip carry away more heat and extends edge life, especially in titanium. When milling with ceramic inserts, no coolant: thermal shock breaks them.

Cutting time

Cutting parameters

Calculator
tc · min
ES
Tiempo de corte
DE
Hauptzeit
IT
Tempo di taglio
PT
Tempo de corte
FR
Temps de coupe

Time the tool spends cutting. Added to rapids, tool changes and part loading, it gives the cycle time, which is what gets quoted.

Example

Turning 120 mm at f = 0.2 mm/rev and 1500 rpm: vf = 0.2 × 1500 = 300 mm/min and tc = 120 / 300 = 0.4 min (24 s).

On the shop floor

Don't forget to add the approach and the exit to L, and the repeated passes: on short parts they make up a good share of the time.

Cycle time

Cutting parameters

Calculator
min
ES
Tiempo de ciclo
DE
Zykluszeit
IT
Tempo ciclo
PT
Tempo de ciclo
FR
Temps de cycle

Total time to make a part, from one cycle start to the next: cutting, rapids, tool changes, stops and loading and unloading. It is the basis of the price and of planning.

Example

Cutting 150 s + rapids 12 s + 6 changes of 4 s (24 s) + loading 30 s = 216 s = 3.6 min. That gives 60 / 3.6 ≈ 16.7 parts per hour.

On the shop floor

In quotes, add setup separately (clamping, zeros, first part) spread over the batch: on short runs it weighs more than the cycle itself.

Cylindricity

Tolerances and surface finish

ES
Cilindricidad
DE
Zylinderform
IT
Cilindricità
PT
Cilindricidade
FR
Cylindricité

Form tolerance that requires the surface of a cylinder to lie between two coaxial cylinders radially separated by the stated value. It controls roundness and straightness at the same time.

Example

Cylindricity 0.01 on a bearing seat: the whole surface fits between two cylinders whose radius difference is 0.01 mm.

On the shop floor

It is measured with a roundness tester, rotating the part on its table, or with a measuring machine touching four or more points at several heights. A micrometer only gives a clue.

D

Damped boring bar

Tools

ES
Barra antivibratoria
DE
Schwingungsgedämpfte Bohrstange
IT
Bareno antivibrante
PT
Barra antivibratória
FR
Barre anti-vibratoire

Boring bar with a damper inside the body that absorbs vibration. It allows boring with much more overhang than a solid bar without scratching the part.

Example

Bar Ø 32 mm turning: solid steel, up to 4 × D = 128 mm overhang; anti-vibration steel, up to 10 × D = 320 mm.

Typical values

Maximum overhang when turning (Sandvik): steel 4 × D, carbide 6 × D, anti-vibration steel 10 × D and carbide-reinforced 14 × D. Recommended from 3 × D.

On the shop floor

Clamp it in a split sleeve with at least 4 × D of clamping length (6 × D on bars over 200 mm). Never press screws directly on the shank: they damage the bar.

Datum

Tolerances and surface finish

ES
Referencia o datum
DE
Bezug
IT
Riferimento
PT
Referência
FR
Référence

Face, axis or point on the part, marked with a letter in a triangle, from which geometric tolerances are measured. They are taken in order: primary, secondary and tertiary.

Example

Frame | ⌖ | Ø 0.1 | A | B | C |: the part rests first on A, then on B and finally on C, and the holes are measured from that system.

On the shop floor

Clamp and set the zero on the same datum faces as the drawing. If you machine from another face, you add up errors that the metrologist will see.

Deep hole drilling

Drilling and threading

Calculator
ES
Taladrado profundo
DE
Tieflochbohren
IT
Foratura profonda
PT
Furação profunda
FR
Perçage profond

Drilling holes that are very long relative to their diameter. It calls for long drills, pressurized internal coolant that flushes out the chip and, on the deepest ones, a pilot hole to guide the entry.

Example

Hole Ø 6 mm and 90 mm deep: L / D = 90 / 6 = 15. From 15 × D, Sandvik recommends first making a pilot with a short drill of the same diameter.

Typical values

Sandvik's deep-hole carbide drills reach 12-30 × D, with at least 10 bar of internal coolant and 40 bar recommended above 20 × D.

On the shop floor

Pilot of 3-5 × D, or at least 1.5 × D, with a short drill of the same diameter. When breaking out of the hole, lower the feed to 30 % of the recommended one (Sandvik).

Depth of cut

Cutting parameters

Calculator
ap · mm
ES
Profundidad de pasada
DE
Schnitttiefe
IT
Profondità di taglio
PT
Profundidade de corte
FR
Profondeur de coupe

How much the cutting edge enters the material, measured perpendicular to the feed. On a lathe it is the radius removed in a pass; in milling, the axial depth along the cutter.

Example

Going from Ø 50 to Ø 44 mm in a single lathe pass: ap = (50 − 44) / 2 = 3 mm.

On the shop floor

Sandvik advises working with a depth of cut larger than the nose radius: choose a radius equal to or smaller than ap and, if there is a tendency to vibrate, a smaller one.

Dial indicator

Measurement

Calculator
ES
Reloj comparador
DE
Messuhr
IT
Comparatore
PT
Comparador
FR
Comparateur

Instrument that amplifies on a dial the displacement of a probe. It doesn't measure absolute dimensions, but differences: centering parts, aligning vise jaws, checking runout or comparing against a standard.

Example

Centering in a 4-jaw chuck, the dial reads 0.08 mm total indicator reading in one revolution: the eccentricity is 0.08 / 2 = 0.04 mm, and it is corrected by moving the jaw 0.04 mm.

Typical values

0.01 mm per division with 10 mm of travel on plunger types. On lever types, 0.01 mm with 0.8 mm of travel, or 0.002 mm with less travel.

On the shop floor

Put the plunger in the measuring direction, or the lever parallel to the surface: tilted 20°, a reading of 0.50 mm is actually 0.50 × cos 20° ≈ 0.47 mm (cosine error).

Dial test indicator

Measurement

ES
Comparador de palanca
DE
Fühlhebelmessgerät
IT
Comparatore a leva
PT
Comparador de alavanca
FR
Comparateur à levier

Dial indicator with a pivoting tip instead of a spindle that moves up and down. It is small and fits in holes and slots, which is why it is used for centering on mills and lathes.

Example

With the lever tilted 30° to the surface, a reading of 0.10 mm is actually 0.10 × 0.87 = 0.087 mm: 13 % less than it shows.

Typical values

Short travel: on the Mitutoyo 513 series it goes from 0.14 mm (0.001 mm graduations) to 1 mm (0.01 mm graduations); the usual one is 0.8 mm with 0.01 mm graduations.

On the shop floor

Set the lever almost parallel to the surface to avoid cosine error. If you can't, multiply the reading by the cosine of the angle: 0.98 at 10°, 0.94 at 20°, 0.87 at 30°.

Diameter programming

CNC programming

ES
Programación en diámetro
DE
Durchmesserprogrammierung
IT
Programmazione in diametro
PT
Programação em diâmetro
FR
Programmation en diamètre

On a lathe, the X dimension is written as the part diameter and not as the distance to the axis. It is the usual practice because it matches what the drawing says and what you measure with the micrometer.

Example

To turn to Ø 40 mm: G01 X40 Z-50 F0.2, with the tip 20 mm from the axis. On Siemens with DIAMON, G91 X-2 is also in diameter: it removes 2 mm of diameter, 1 mm per side.

On the shop floor

On Siemens, DIAMON puts X in diameter in absolute and incremental; DIAM90, only in absolute (in G91, in radius), and DIAMOF goes back to radius. Check which one is active before giving dimensions in G91.

Dimensional tolerance

Tolerances and surface finish

Calculator
mm
ES
Tolerancia dimensional
DE
Maßtoleranz
IT
Tolleranza dimensionale
PT
Tolerância dimensional
FR
Tolérance dimensionnelle

Difference between the maximum and minimum sizes allowed on a dimension. It is indicated with deviations (+0.1 / −0.05) or with an ISO class (H7, g6).

Example

Ø 25 +0.1 / −0.05: the part is good between 24.95 and 25.1 mm, tolerance T = 25.1 − 24.95 = 0.15 mm. A Ø 25 H7 runs from 25.000 to 25.021 mm.

Typical values

Dimensions without tolerance, per ISO 2768 medium class: ±0.2 mm from 6 to 30 mm and ±0.3 mm from 30 to 120 mm.

On the shop floor

Work to the middle of the tolerance, not to the limit: edge wear and temperature move the size over the course of the batch.

Driven tool

Turning

Calculator
ES
Herramienta motorizada
DE
Angetriebenes Werkzeug
IT
Utensile motorizzato
PT
Ferramenta motorizada
FR
Outil motorisé

Turret toolholder that rotates its own milling cutter or drill. Together with the C axis it allows drilling, tapping and milling on the lathe without moving the part to another machine.

Example

Ø 6 mm cutter at vc = 100 m/min: n ≈ 5305 rpm. If the live tool only reaches 4000 rpm, the real vc stays at π × 6 × 4000 / 1000 ≈ 75 m/min.

On the shop floor

Check whether the tool is axial or radial and its maximum rpm. To drill or mill off-center with the spindle stopped, lock it (on Haas, M14 locks it and M15 releases it).

Dry machining

Cutting parameters

ES
Mecanizado en seco
DE
Trockenbearbeitung
IT
Lavorazione a secco
PT
Maquinagem a seco
FR
Usinage à sec

Machining without coolant, only with air or nothing. It saves coolant and cleaning and avoids thermal shock in interrupted cuts, but all the heat goes into the chip, the part and the edge.

Typical values

It works well in milling steel, especially roughing, gray cast iron and hardened steel. Aluminum needs coolant so it doesn't stick to the edge, and so do titanium and superalloys.

On the shop floor

In milling steel, stainless in roughing or gray cast iron, dry is better than coolant: each entry and exit heats and cools the edge, and coolant increases thermal cracks.

Ductile iron

Materials

ES
Fundición nodular
DE
Gusseisen mit Kugelgraphit
IT
Ghisa sferoidale
PT
Ferro fundido nodular
FR
Fonte à graphite sphéroïdal

Cast iron with the graphite in the form of nodules instead of flakes. It is stronger and much more ductile than gray cast iron, which has little impact resistance.

Example

EN-GJS-500-7: minimum tensile strength of 500 MPa, yield strength of 320 MPa and 7 % elongation. EN-GJS-400-15 withstands 400 MPa, but elongates 15 %.

Typical values

ISO K group, but it machines worse than gray iron and tends to form built-up edge. The ferritic grade behaves almost like a low-alloy steel; the pearlitic one is more abrasive.

On the shop floor

All cast irons contain silicon carbide, very abrasive to the edge. With sand on the part, a high vc sends wear through the roof: use PVD-coated grades and coolant.

Duplex stainless steel

Materials

ES
Inoxidable dúplex
DE
Duplexstahl
IT
Acciaio inossidabile duplex
PT
Aço inoxidável duplex
FR
Acier inoxydable duplex

Stainless with a half ferrite, half austenite structure, such as 1.4462 (21-23 % Cr, 4.5-6.5 % Ni, 2.5-3.5 % Mo). It resists corrosion like 316L or better and withstands much more load, but it machines worse.

Example

Minimum yield strength in solution-annealed condition: 1.4462, 450 MPa; 1.4404 (316L), 200 MPa. That is 450 / 200 = 2.25 times more, and it shows in the cutting forces.

Typical values

ISO group M, with a relative machinability of 30 % (Sandvik). Outokumpu gives for carbide turning vc ≈ 100 m/min in finishing, 85 in semi-finishing and 55 in roughing.

On the shop floor

Rigid setup, sharp edges to generate less heat and not work-harden the surface, always coolant and the smallest possible nose radius to avoid vibration. Unlike 316L, it is magnetic.

Dwell

CNC programming

Calculator
s
ES
Tiempo de espera
DE
Verweilzeit
IT
Tempo di sosta
PT
Tempo de espera
FR
Temporisation

Programmed pause in which the axes stay still while the spindle keeps turning. Used to clean the bottom of a slot, a counterbore or a blind hole and leave a clean size.

Example

To make 2 turns at the bottom at 400 rpm: t = 2 × 60 / 400 = 0.3 s. Fanuc: G04 P300 (milliseconds) or G04 X0.3 (s). Siemens: G4 F0.3 or G4 S2 (revolutions). Heidenhain: FUNCTION DWELL TIME0.3 or REV2.

Typical values

Uses cited by the manuals: relief grooves (Siemens), chip breaking (Heidenhain) and exact stop at the end of a block (Fanuc). During the dwell, the F and S programmed earlier are maintained.

On the shop floor

P changes by control: on Fanuc it is in milliseconds and without a decimal point (G04 P1000 = 1 s). On Haas, P with a decimal point is seconds and without, milliseconds: P10. is 10 s; P10, 10 ms.

E

Eccentric turning

Turning

e · mm
ES
Torneado excéntrico
DE
Exzenterdrehen
IT
Tornitura eccentrica
PT
Torneamento excêntrico
FR
Tournage excentrique

Turning of a diameter whose axis is offset by a distance e from the main axis of the part, as in cams, eccentrics and crankshafts.

Example

Eccentricity e = 3 mm: when rotating the part on its main axis, the indicator resting on the eccentric diameter shows a total runout of 2 × 3 = 6 mm.

Typical values

Four-jaw independent chuck, adjusted one jaw at a time to offset the part. If it ends up unbalanced, Kitagawa says to lower rpm or add counterweights to a balance quality of G6.3 or better.

On the shop floor

Center with a dial indicator until the runout is twice the eccentricity. Before machining, rotate at low rpm and check that the part and chuck do not touch the turret.

Edge chipping

Tools

ES
Astillado del filo
DE
Schneidkantenausbruch
IT
Scheggiatura del tagliente
PT
Lascamento da aresta
FR
Écaillage de l'arête

Small pieces that break off the cutting edge and leave it nicked. The finish gets worse suddenly and, if not corrected, it ends in insert breakage.

Typical values

Causes: grade too hard, weak geometry, thick coating, vibration, chip hammering, excessive feed or depth of cut, sand inclusions and built-up edge that tears off pieces when it breaks away.

On the shop floor

Move to a tougher grade (higher ISO number), a more robust geometry or one with more edge rounding, and a thin PVD coating. Lower the feed in interrupted cuts and shorten the overhang.

Edge preparation

Tools

ES
Preparación del filo
DE
Kantenpräparation
IT
Preparazione del tagliente
PT
Preparação da aresta
FR
Préparation d'arête

Microscopic shape given to the edge after grinding it: hone, negative land or a combination. It removes the micro-cracks of the sharp edge and makes it stronger, at the cost of cutting with a bit more force.

Example

Turning with a small feed, below 0.1 mm/rev, a pressed insert with a rounded edge leaves a burr because the feed is too low for that rounding. With a ground sharp-edge one it cuts clean.

Typical values

Ground inserts: small rounding or sharp edge; pressed: more rounding. In ceramic, chamfers of 0.05 to 0.2 mm at 20-25°.

On the shop floor

The chip thickness must exceed the edge rounding. If a burr or vibration appears with a robust edge and small feed, switch to a ground insert or one with a thin PVD coating.

End mill

Milling

ES
Fresa plana o de mango
DE
Schaftfräser
IT
Fresa a candela
PT
Fresa de topo
FR
Fraise deux tailles

Solid cutter with edges on the side and at the tip, flat-bottomed with a sharp corner. It is the basic tool of the machining center for contours, pockets, slots and shoulders.

Example

Ø 10 mm carbide at vc = 120 m/min: n ≈ 3820 rpm. With 4 flutes and fz = 0.05 mm, vf ≈ 0.05 × 4 × 3820 ≈ 764 mm/min.

Typical values

Shank with h6 tolerance for precision tool holders. For aluminum there are high-helix cutters, 45° with 2 or 3 flutes, which evacuate the chip faster and leave a better finish.

On the shop floor

Before plunging straight down, check in the catalog whether it cuts at center: not all of them do. Calculate rpm with the actual diameter it cuts, not the shank diameter.

Engagement angle

Milling

DrawingCalculator
φ · °
ES
Ángulo de contacto
DE
Eingriffswinkel
IT
Angolo di impegno
PT
Ângulo de contacto
FR
Angle d'engagement

Rotation angle during which each tooth is cutting. It depends on the width of cut relative to the diameter and determines the load, the heat and the real chip thickness.

Example

Ø 10 mm end mill with ae = 1 mm: φ = acos(0.8) ≈ 37° and the maximum chip is sin 37° ≈ 0.6 × fz. For a 0.05 mm chip, fz ≈ 0.05 / 0.6 ≈ 0.083 mm.

Typical values

Full slot (ae = D), 180°; ae = D / 2, 90°. Centered face mill with ae = 0.7 × D: φ = 2 × asin(0.7) ≈ 89°.

On the shop floor

Below 90° (ae less than D / 2) the chip gets thinner: if you don't raise fz, the edge rubs. Sandvik gives a factor of 1.66 with ae of 10 % and 2.3 with 5 %.

Engineering plastics

Materials

ES
Plásticos técnicos
DE
Technische Kunststoffe
IT
Tecnopolimeri
PT
Plásticos técnicos
FR
Plastiques techniques

Engineering plastics with good strength and stability, such as POM (acetal), PA (nylon) and PEEK. They cut easily, but expand a lot and distort with heat and clamping.

Example

A 100 mm POM part measured at 25 °C instead of 20 °C grows 100 × 130 × 10⁻⁶ × 5 ≈ 0.065 mm. The same in steel, about 0.005 mm.

Typical values

Expansion (Ensinger, 23-60 °C) in 10⁻⁶ /K: POM-C ≈ 130, PA 6 ≈ 120, PEEK ≈ 50; steel, about 10. PA 6 absorbs water (0.6 % in 96 h).

On the shop floor

Use very sharp edges: a dull one heats and distorts the part. Clamp without stress and do the finishing when the material has cooled completely.

Entering angle

Turning

DrawingCalculator
κr · °
ES
Ángulo de posición
DE
Einstellwinkel
IT
Angolo di registrazione
PT
Ângulo de posição
FR
Angle de direction d'arête

Angle between the main cutting edge and the feed direction. It determines the chip thickness, where the cutting force pushes and which shapes the toolholder can machine.

Example

With f = 0.3 mm/rev: at κr = 95° the chip is ≈ 0.30 mm thick; at κr = 45° it drops to 0.3 × sin 45° ≈ 0.21 mm, spread over a longer edge.

Typical values

Sandvik: 91-95° for turning against a shoulder; 95° for facing and turning with the same tool; 93° for copying; 45-75° to raise the feed with the same chip.

On the shop floor

On slender or thin-wall parts use κr close to 90°: even going from 91° to 95° changes the direction of the cutting force and can make the part vibrate.

Envelope requirement

Tolerances and surface finish

Ⓔ
ES
Requisito de envolvente
DE
Hüllbedingung
IT
Requisito dell'inviluppo
PT
Requisito de envolvente
FR
Exigence de l'enveloppe

Requirement, marked with Ⓔ after the dimension, that the feature must not go outside a perfect form at its maximum material size. So the size also limits the form: a shaft within tolerance cannot be bent.

Example

Shaft Ø 20 0/−0.02 Ⓔ (19.98 to 20.00 mm) that measures 19.99 everywhere: it may bow by at most 20.00 − 19.99 = 0.01 mm. If it measured 20.00, it would have to be perfectly straight.

Typical values

In ISO, without Ⓔ the independency principle applies (ISO 8015): size and form are checked separately. In the ASME standard the envelope applies by default.

On the shop floor

To check it: the GO side passes with a ring or plug of the full length, which captures the form; the NO GO side, measuring with two-point contact at several sections.

F

Face mill

Milling

ES
Fresa de planear
DE
Planfräser
IT
Fresa per spianare
PT
Fresa de facear
FR
Fraise à surfacer

Large-diameter cutter with inserts on the periphery that cuts with its front face. It is chosen by its lead angle, its tooth pitch and its diameter relative to the width of the part.

Example

60 mm wide face: Sandvik asks for a diameter 20-50 % larger, D ≈ 72-90 mm, so an Ø 80 mm cutter, which works with 60 / 80 = 0.75 of its diameter inside the part.

Typical values

45°, first choice for general use; 90° for thin walls, weak clamping and squares; round inserts for demanding face milling. With low power or long overhang, coarse pitch and differential pitch.

On the shop floor

Place the cutter off-center relative to the part, so the chip is as thin as possible at the tooth exit.

Face milling

Milling

ES
Planeado
DE
Planfräsen
IT
Spianatura
PT
Fresagem frontal
FR
Surfaçage

Milling a flat surface with the front face of the cutter, normally an insert face mill. Used to clean up and size the part's reference face.

Example

Ø 63 mm face mill, 5 teeth, fz = 0.15 mm and 1000 rpm: vf = 0.15 × 5 × 1000 = 750 mm/min. For a 300 mm part plus 63 for approach and overtravel, t ≈ 363 / 750 ≈ 0.48 min.

Typical values

Sandvik: cutter 20-50 % wider than the pass, with ae ≈ 70 % of the diameter; 45° cutters are the first choice for general use.

On the shop floor

Don't center the cutter right over the part: shift it to one side so the chip enters thick and exits as thin as possible, as in climb milling.

Facing

Turning

ES
Refrentado
DE
Plandrehen
IT
Sfacciatura
PT
Facejamento
FR
Dressage

Lathe operation in which the tool feeds perpendicular to the axis to leave the front face of the part flat. It is usually the first pass, because that face serves as the Z origin.

Example

With constant vc = 200 m/min, at Ø 80 mm the spindle turns at ≈ 796 rpm, but at Ø 10 mm it would ask for ≈ 6366 rpm. That is why the maximum rpm is limited before facing.

Typical values

To face and turn with the same tool, Sandvik proposes κr of 95° with an 80° rhombic or trigonal insert. A chamfer or radius at the end of the cut avoids the exit burr.

On the shop floor

With constant surface speed (G96), always set an rpm limit (G50 S… on Haas). If the edge is below center, it leaves a nib in the center of the face.

Feed force

Cutting parameters

Ff · N
ES
Fuerza de avance
DE
Vorschubkraft
IT
Forza di avanzamento
PT
Força de avanço
FR
Effort d'avance

Component of the cutting force that acts in the feed direction and opposes it. It is carried by the ball screw and the axis motor; in drilling it is the axial thrust of the drill.

Typical values

It depends mainly on the lead angle: with large κr (90-95°) the thrust goes axial, toward the chuck, and Ff is high; with small κr (45° or round insert) it shifts to radial.

On the shop floor

As ap rises, the thrust that pushes the insert away from the part becomes more axial, and that is good: the force directed toward the chuck gives less vibration than the radial one.

Feed per minute and per revolution

CNC programming

ES
Avance por minuto y por vuelta
DE
Vorschub pro Minute und pro Umdrehung
IT
Avanzamento al minuto e al giro
PT
Avanço por minuto e por rotação
FR
Avance par minute et par tour

Way the control interprets the F letter: in millimeters per minute or in millimeters per spindle revolution. Per revolution, the feed follows the rpm; per minute, it does not.

Example

Drill at 2000 rpm: with G95 F0.15 it feeds 0.15 × 2000 = 300 mm/min; with G94 you would write F300. On the Haas lathe they are G98 per minute and G99 per revolution; on Siemens, G94 and G95.

Typical values

Siemens gives as an example G94 F250 (mm/min) in milling and G95 F0.2 (mm/rev) on the lathe. On the Haas lathe, G99 (per revolution) is the default mode.

On the shop floor

The costly mistake: an F300 meant as mm/min with per-revolution mode active asks for 300 mm per revolution. Always declare the feed mode at the start of each tool.

Feed per revolution

Cutting parameters

Calculator
f · mm/v
ES
Avance por vuelta
DE
Vorschub pro Umdrehung
IT
Avanzamento per giro
PT
Avanço por rotação
FR
Avance par tour

Distance the tool advances per spindle revolution. It is the usual feed on lathes (G95) and in drilling, and together with the nose radius it determines the surface finish.

Example

Turning at f = 0.25 mm/rev with the part at 1200 rpm: vf = 0.25 × 1200 = 300 mm/min.

On the shop floor

In finishing, feed rules the roughness: the theoretical value is h = f² / (8 × rε), so with half the feed it drops to a quarter.

Feed per tooth

Cutting parameters

Calculator
fz · mm/diente
ES
Avance por diente
DE
Vorschub pro Zahn
IT
Avanzamento per dente
PT
Avanço por dente
FR
Avance à la dent

Distance the cutter advances between one tooth's cut and the next. It is the milling data the manufacturer gives, because it sets the load each cutting edge withstands.

Example

4-flute end mill at 3000 rpm with fz = 0.05 mm: vf = 0.05 × 4 × 3000 = 600 mm/min.

On the shop floor

An fz that is too low does not protect the cutter: according to Sandvik, a chip that is too thin is the most common cause of poor performance and shortens edge life. If you lower the lead angle, raise fz.

Feeler gauge

Measurement

ES
Galga de espesores
DE
Fühlerlehre
IT
Spessimetro
PT
Apalpa-folgas
FR
Jauge d'épaisseur

Set of steel blades of exact thickness that you slide into a gap to find out how wide it is. Used for clearances, guideway play, flatness against a surface plate and shimming.

Example

The 0.05 mm blade goes in with slight drag and the 0.06 mm one does not: the gap is between 0.05 and 0.06 mm.

Typical values

The Mitutoyo 184-303S set has 28 leaves from 0.05 to 1 mm: in 0.01 mm steps up to 0.15 mm and then in 0.05 mm steps. Some sets start at 0.03 mm.

On the shop floor

Each leaf has its own tolerance (on the 184-303S, ±0.005 mm up to 0.15 mm and ±0.02 mm from 0.55 to 1 mm). If you stack two leaves, you also add their errors.

Fit

Tolerances and surface finish

ES
Ajuste
DE
Passung
IT
Accoppiamento
PT
Ajustamento
FR
Ajustement

Relationship between a hole and a shaft of the same nominal diameter according to their tolerances. It can be clearance, transition or interference, and is written as H7/g6.

Example

Ø 25 H7/g6: hole 25.000-25.021 and shaft 24.980-24.993 mm. Minimum clearance 0 − (−0.007) = 7 µm and maximum 0.021 − (−0.020) = 41 µm: it turns or slides precisely.

Typical values

H7 in Ø 25: g6 gives a clearance of 7 to 41 µm; h6, 0 to 34 µm; k6, transition (clearance up to 19 µm or interference up to 15 µm); p6, press fit.

On the shop floor

The fit is decided on the drawing by function; you only meet the two tolerances. Measure both at the same temperature before assembly.

Flank wear

Tools

VB · mm
ES
Desgaste de flanco
DE
Freiflächenverschleiß
IT
Usura sul fianco
PT
Desgaste de flanco
FR
Usure en dépouille

Worn band that appears on the flank, just below the cutting edge, from rubbing against the workpiece. It is the normal wear and the one used to decide when to change the edge.

Typical values

ISO 3685 end-of-life criterion: VB = 0.3 mm if the wear band is uniform and 0.6 mm if the wear is localized. Sandvik considers it the preferred wear: it gives a predictable tool life.

On the shop floor

If it grows very fast, Sandvik says to lower the cutting speed, move to a more wear-resistant grade or improve the coolant.

Flatness

Tolerances and surface finish

ES
Planitud
DE
Ebenheit
IT
Planarità
PT
Planeza
FR
Planéité

Form tolerance that requires all points of a surface to lie between two parallel planes separated by the stated value. It has no datum.

Example

Flatness 0.02 on a seating face: the whole surface fits between two planes 0.02 mm apart, even if the face is tilted relative to others.

On the shop floor

With a measuring machine, touch four or more points spread over the whole face. With a dial indicator, the reading changes depending on the points chosen and who measures: repeat the measurement before rejecting.

Free-cutting steel

Materials

ES
Acero de corte fácil
DE
Automatenstahl
IT
Acciaio automatico
PT
Aço de corte fácil
FR
Acier de décolletage

Steel with added sulfur, and sometimes lead, to improve machinability: they break the chip and extend tool life. It is the typical automatic-lathe material for small parts.

Example

11SMnPb30 (1.0718) contains 0.27-0.33 % sulfur and 0.20-0.35 % lead, with a maximum of 0.14 % carbon; 11SMn30 is the lead-free version.

Typical values

As rolled, it has a tensile strength of 380-570 N/mm² up to 40 mm diameter, with 169 HB maximum (ISO 683-4).

On the shop floor

11SMnPb30 is not suitable for hardening and welding is not recommended. If the part needs heat treatment, choose a case-hardening grade (10S20) or a direct-hardening grade (44SMn28).

G

G-code

CNC programming

ES
Código G
DE
G-Code
IT
Codice G
PT
Código G
FR
Code G

CNC program instruction that tells the machine how to move or what mode to work in: rapid, straight, arc, plane, units or cycles. It is written with the letter G and a number; the reference standard is DIN 66025.

Example

N10 G90 G54 G17 G21 · N20 G00 X0 Y0 · N30 G01 Z-2 F150. One block can hold several G-codes from different groups: absolute, work offset, XY plane and millimeters go on the same line.

Typical values

Most-used groups: G00-G03 motion, G17-G19 plane, G20/G21 inch or mm, G40-G42 cutter compensation, G43/G49 tool length, G54-G59 work offsets, G80-G89 canned cycles, G90/G91 positioning mode, G94/G95 feed.

On the shop floor

The same number does not mean the same thing on all machines: on a Fanuc lathe with code system A, feed per minute is G98 and not G94, and G90 is not «absolute». Always check the manual.

Gauge blocks

Measurement

ES
Bloques patrón
DE
Parallelendmaße
IT
Blocchetti di riscontro
PT
Blocos-padrão
FR
Cales étalons

Blocks of steel or ceramic with two parallel faces at a very exact distance. They wring together by sliding and make up any size to calibrate and zero instruments.

Example

For 45.6785 mm with a base-1 mm set: 1.0005 + 1.008 + 1.17 + 17.5 + 25 = 45.6785 mm. Start with the last decimal and use the fewest blocks possible, and the thickest ones.

Typical values

ISO 3650 grades: K or 0 for calibrating other blocks, 0 or 1 as reference, 1 or 2 for inspection and for checking instruments, and 2 in the shop.

On the shop floor

Clean them before wringing and touch them as little as possible: the heat of your hand lengthens a steel block. When taking the stack apart, separate them by sliding, not pulling.

General tolerance

Tolerances and surface finish

ES
Tolerancia general
DE
Allgemeintoleranz
IT
Tolleranza generale
PT
Tolerância geral
FR
Tolérance générale

Tolerance that applies to all the dimensions on the drawing that do not carry their own. It is stated in the title block, normally with ISO 2768-1 and a class: f (fine), m (medium), c (coarse) or v (very coarse).

Example

Drawing with 'ISO 2768-m' and a 50 mm dimension without tolerance: it falls in the 30 to 120 mm range, which is ±0.3 mm, so it is good from 49.7 to 50.3 mm.

Typical values

ISO 2768-1, 30-120 mm range: f ±0.15, m ±0.3, c ±0.8, v ±1.5 mm. 6-30 mm range: f ±0.1, m ±0.2, c ±0.5, v ±1 mm.

On the shop floor

If the title block gives no general tolerance, ask before manufacturing. The letter that follows (H, K or L, as in mK) sets the general geometrical tolerances of ISO 2768-2, not the dimensional ones.

Geometric tolerance

Tolerances and surface finish

ES
Tolerancia geométrica
DE
Geometrische Toleranz
IT
Tolleranza geometrica
PT
Tolerância geométrica
FR
Tolérance géométrique

Zone within which the form, orientation or position of a feature must lie, according to ISO 1101. It is shown in a frame with the symbol, the value and the datums.

Typical values

Four families: form (flatness, straightness, roundness, cylindricity), orientation (parallelism, perpendicularity, angularity), location (position, coaxiality, symmetry) and runout.

On the shop floor

Read the frame from left to right: symbol, zone size (with Ø if cylindrical) and datums in order of importance. Clamp the part by those datums.

Go/no-go gauge

Measurement

ES
Galga pasa / no pasa
DE
Grenzlehre
IT
Calibro passa-non passa
PT
Calibre passa-não passa
FR
Calibre entre/n'entre pas

Fixed gauge with one side made to the limit that must enter and another to the limit that must not. It doesn't give the size, it only says whether the part is within tolerance, quickly and without interpretation.

Example

Hole Ø 20 H7 (0 / +0.021 mm): the go side is made at 20.000 mm and must enter; the no-go, at 20.021 mm, and must not enter.

Typical values

Plug gauges for holes and rings or snap gauges for shafts (ISO 1938-1). On working gauges, the go side carries a wear allowance according to DIN 7164.

On the shop floor

Put it in without forcing or twisting hard: if you need to push, the hole fails. With the part still hot from the machine, the result is misleading.

Grey cast iron

Materials

ES
Fundición gris
DE
Grauguss
IT
Ghisa grigia
PT
Ferro fundido cinzento
FR
Fonte grise

Iron with more than 2 % carbon, with the graphite in flake form. It is the typical ISO K group: it gives short chips and carbon and iron dust.

Typical values

Average hardness of about 200-250 HB. At high cutting speeds you move from carbide to ceramic or CBN inserts.

On the shop floor

It runs very well dry or with minimum quantity lubrication, because graphite lubricates. Control the carbon and iron dust it gives off.

Grooving

Turning

ES
Ranurado en torno
DE
Einstechen
IT
Scanalatura
PT
Ranhuragem
FR
Gorgeage

Operation in which a narrow insert plunges radially or axially to make grooves, seal seats or thread reliefs. The groove width usually comes from the insert width.

Typical values

Sandvik: multiple grooving for slots deeper than wide and plunge turning for those wider than deep. When turning sideways with a grooving insert, maximum ap of 75 % of the width.

On the shop floor

In wide and deep grooves, first make separate cuts leaving ribs thinner than the insert and remove them afterward. When turning sideways, use an ap larger than the insert radius.

Gun drill

Drilling and threading

Calculator
ES
Broca cañón
DE
Einlippenbohrer
IT
Punta a cannone
PT
Broca canhão
FR
Foret à canon

Single-edge drill with a straight V groove along the tube. Coolant enters under pressure through the inside, flushes the chip out through the groove, and guide pads bear on the wall and keep the drill straight.

Example

Hole Ø 8 mm and 800 mm long: L / D = 800 / 8 = 100. It is a gun drill job: Botek makes these drills in lengths of up to 5000 mm.

Typical values

Indicative (Botek): from about 10 to over 100 × D, with tolerances down to IT7. Coolant pressure depends on diameter and depth; in their examples, 70-140 bar.

On the shop floor

It does not center itself: it needs a guide bushing or a pilot hole almost exactly to size, for example +0.01 to +0.02 mm for Ø 4-12 mm. The quality of that pilot decides how the drilling turns out.

H

Hard turning

Turning

ES
Torneado duro
DE
Hartdrehen
IT
Tornitura dura
PT
Torneamento duro
FR
Tournage dur

Turning of hardened steel, typically 55 to 65 HRC, mainly with CBN inserts. On many parts it replaces grinding with more flexibility and shorter lead times.

Typical values

According to Sandvik: CBN for case-hardened or induction-hardened steels; below ≈ 55 HRC, ceramic or carbide. Dry whenever possible; with overhang, length up to ≈ 2 × diameter.

On the shop floor

Use a rigid machine and clamping, the smallest possible depth of cut and the correct edge preparation. Make chamfers and radii before hardening and enter and leave the cut rolling, never abruptly.

Hardening

Materials

ES
Templado
DE
Härten
IT
Tempra
PT
Têmpera
FR
Trempe

Treatment that heats steel until it becomes austenitic and cools it very quickly in water, oil or gas so that it forms martensite. The steel becomes very hard, but brittle and with internal stresses.

Example

A 42CrMo4 is hardened from 820-880 °C in oil or water and then tempered between 540 and 680 °C; right after quenching it is hard and brittle.

Typical values

A tool steel oil-hardened from about 825 °C comes out at about 65 HRC before tempering, and it is used tempered to about 62 HRC.

On the shop floor

Watch out for the false friend: English «tempering» is revenido, not templado, which is «hardening». Leave stock: hardening and tempering change the size (one manufacturer recommends 0.25 %).

Hardness

Materials

ES
Dureza
DE
Härte
IT
Durezza
PT
Dureza
FR
Dureté

Resistance of a material to being penetrated. It is measured with standardized tests (Rockwell HRC, Brinell HB, Vickers HV) and is the data point that says the most about how a steel will machine.

Example

According to table A.1 of ISO 18265 for unalloyed and low-alloy steels, 450 HV is equivalent to about 428 HB and a tensile strength of about 1455 MPa.

Typical values

42CrMo4 annealed: max. 241 HB. Above 45 HRC and up to 68 HRC it is treated as group H; typical hard turning runs from 55 to 65 HRC.

On the shop floor

Conversions between scales are approximate and only valid for the table's material: don't convert hardness of aluminum or austenitic stainless with the steel table.

Height gauge

Measurement

ES
Gramil o calibre de altura
DE
Höhenmessgerät
IT
Truschino
PT
Graminho
FR
Trusquin

Instrument with a base that rests on the surface plate and a scriber that moves up and down a column. It measures heights from the surface plate and its tip can also be used for marking out.

Example

You zero the height gauge on the surface plate. It reads 62.40 mm on the top face and 37.15 mm on the step: the step height is 62.40 − 37.15 = 25.25 mm.

Typical values

Shop digital ones (Mitutoyo 570 series) resolve 0.01 mm with travels of 300 or 600 mm; high-precision ones, like the Linear Height LH-600, reach 0.0001 mm.

On the shop floor

Clean dust and burrs from the surface plate and the base. Lower the probe slowly and without pressing: with too much force the base lifts off the plate and the measurement comes out wrong.

Helical interpolation

Milling

Calculator
ES
Interpolación helicoidal
DE
Helixinterpolation
IT
Interpolazione elicoidale
PT
Interpolação helicoidal
FR
Interpolation hélicoïdale

Circular motion in the plane combined with linear feed in the perpendicular axis, drawing a helix. Used to open holes with an end mill, ramp into pockets and mill threads.

Example

Ø 30 mm hole with a Ø 20 mm cutter and 600 mm/min at the cutting edge: the center must go at 600 × 10 / 30 = 200 mm/min. Programming 600 would triple the load on the edge.

On the shop floor

Sandvik: in a single continuous helix you open a hole of at most twice the cutter diameter; if the cutter is too small, a core is left in the center.

High-feed milling

Milling

Calculator
ES
Fresado de alto avance
DE
Hochvorschubfräsen
IT
Fresatura ad alto avanzamento
PT
Fresagem de alto avanço
FR
Fraisage à grande avance

Roughing with very small lead angle cutters and a light depth of cut. The chip comes out thin even if the feed per tooth is very high, which gives a lot of removal per minute.

Example

With κr = 15° and fz = 1 mm: hex = 1 × sin 15° ≈ 0.26 mm. A 45° cutter would give that chip with only fz = 0.26 / sin 45° ≈ 0.37 mm.

Typical values

Sandvik: 10° cutters with depth of cut limited to less than 2.8 mm; at 10° the chip thins almost six times (factor 5.8), and at 45°, 1.4 times.

On the shop floor

If you program the fz of a 90° cutter, the chip ends up so thin that the edge rubs. Multiply fz by the thinning factor of its angle to recover the thickness.

High-speed machining

Cutting parameters

ES
Mecanizado de alta velocidad
DE
Hochgeschwindigkeitsbearbeitung
IT
Lavorazione ad alta velocità
PT
Maquinagem a alta velocidade
FR
Usinage à grande vitesse

Milling with very high cutting speeds and feeds and light passes, mostly in width. It removes material fast with little force and little heat in the part; used in molds, aluminum and thin-walled parts.

Example

Cutter Ø 6 mm at vc = 300 m/min: n = 300 × 1000 / (π × 6) ≈ 15915 rpm. With 3 flutes and fz = 0.05 mm, vf = 0.05 × 3 × 15915 ≈ 2390 mm/min.

Typical values

It is applied mainly to 3D and 4- or 5-axis programs with many short segments, such as molds and dynamic milling, where the control has to link hundreds of blocks per second.

On the shop floor

The machine must be able to keep up with the feed: the control reads blocks ahead (look-ahead) to link segments without stopping. Without that function, on short segments it slows down and the actual feed falls far below the programmed one.

High-speed steel

Tools

ES
Acero rápido
DE
Schnellarbeitsstahl
IT
Acciaio rapido
PT
Aço rápido
FR
Acier rapide

Alloy steel with carbon, tungsten, molybdenum, vanadium, chromium and sometimes cobalt, which can exceed 30 % of the total. Hardening and several temperings give it the hot hardness it needs to cut.

Example

HSS drill Ø 8 mm in structural steel at 30 m/min: n = 30 × 1000 / (π × 8) ≈ 1194 rpm.

Typical values

HSS and HSS-E drills in structural steel: about 27-35 m/min according to Hartner. Cobalt improves resistance at high temperature (Böhler).

Hole-basis system

Tolerances and surface finish

ES
Sistema de agujero base
DE
Einheitsbohrung
IT
Sistema foro base
PT
Sistema de furo base
FR
Système de l'alésage normal

Fit system in which all holes take position H (lower deviation zero) and the fit is achieved by varying the shaft tolerance.

Example

Ø 25 H7 is always 25.000-25.021 mm. With a g6 shaft it has clearance, with k6 transition and with p6 interference, without touching the hole.

On the shop floor

It is the most widely used system: the hole is always made with the same tool and you play with the shaft, which is easier to machine. The basic-shaft system (h) is used, for example, in transmissions with long shafts.

I

Inch or metric units

CNC programming

ES
Pulgadas o milímetros
DE
Zoll oder Millimeter
IT
Pollici o millimetri
PT
Polegadas ou milímetros
FR
Pouces ou millimètres

Unit in which the control reads the program's dimensions and feed: inches or millimeters. On Fanuc it is chosen with G20 (inches) and G21 (mm); on Siemens, with G70 and G71.

Example

With G20, X2.5 is 2.5 × 25.4 = 63.5 mm and F10. is 10 × 25.4 = 254 mm/min. On Siemens, G70/G71 change only the dimensions; G700/G710 also change the feed. On Heidenhain it goes in the header: BEGIN PGM PART MM or INCH.

Typical values

1 in = 25.4 mm exactly, so 0.001 in = 25.4 µm. On Fanuc, at power-up, the machine stays in G20 or G21 as it was when it was switched off.

On the shop floor

Fanuc requires G20 or G21 in its own block at the start, before setting the origin, and does not allow changing it mid-program. Without G20, a machine in G21 reads X2.5 as 2.5 mm.

Inclination angle

Tools

λs · °
ES
Ángulo de inclinación
DE
Neigungswinkel
IT
Angolo di inclinazione
PT
Ângulo de inclinação
FR
Angle d'inclinaison d'arête

Angle the cutting edge makes with the horizontal reference plane, seen looking at the edge from the front. It decides where the chip flows and which part of the edge touches the workpiece first.

Typical values

Sandvik example: a tool holder for DNMG 15 04 08 has λs = −7° and rake of −6°. Positive: the chip flows away from the part. Negative: it goes toward the part, but the edge is stronger.

On the shop floor

If the chip scratches the already machined surface, try a more positive inclination. For impacts on entering the cut, negative is better, although the force toward the part increases and it vibrates more easily.

Indexable insert drill

Drilling and threading

ES
Broca de plaquitas
DE
Wendeplattenbohrer
IT
Punta a inserti
PT
Broca de pastilhas intercambiáveis
FR
Foret à plaquettes

Steel-body drill with two screwed-on inserts, a central one and a peripheral one, that drills into solid without a spot hole. It is the cheap, fast option for medium and large diameter holes.

Example

Ø 30 mm with the vc the catalog gives, for example 180 m/min: n = 180 × 1000 / (π × 30) ≈ 1910 rpm. With f = 0.1 mm/rev: vf = 1910 × 0.1 ≈ 191 mm/min.

Typical values

Sandvik CoroDrill 880: Ø 12-84 mm and from 2 to 5 × D, with tolerance 0/+0.25 mm at 2-3 × D. Sandvik recommends internal coolant and, if possible, at about 70 bar.

On the shop floor

In through holes a disc forms that can fly off at high speed: close the chuck guard or the machine door. On a lathe, offsetting it radially enlarges the diameter without changing drills.

Indexable milling cutter

Milling

ES
Fresa de plaquitas
DE
Wendeschneidplattenfräser
IT
Fresa a inserti
PT
Fresa de pastilhas
FR
Fraise à plaquettes

Cutter with a steel body and screwed-on carbide inserts that are indexed or replaced when worn. It pays off mainly in roughing and in medium and large diameters.

Example

Face mill Ø 80 mm with 6 inserts at vc = 200 m/min: n ≈ 796 rpm. With fz = 0.15 mm, vf ≈ 0.15 × 6 × 796 ≈ 716 mm/min.

On the shop floor

Clean the seat before mounting the insert and tighten with a torque wrench to the manufacturer's torque: with more torque the insert, shim or screw breaks; with less, the insert moves and vibrates.

Insert

Tools

ES
Plaquita
DE
Wendeschneidplatte
IT
Inserto
PT
Pastilha
FR
Plaquette

Small piece of carbide, cermet, ceramic, CBN or PCD with one or several cutting edges that is screwed or clamped into a toolholder. When an edge wears out, it is indexed or replaced.

Example

CNMG 120408: C 80° rhombic, N 0° clearance, M tolerance class; 04 is the thickness (4.76 mm) and 08 the nose radius (0.8 mm).

Typical values

Indicative maximum feed according to nose radius (Sandvik): 0.25-0.35 mm/rev with 0.4 mm; 0.4-0.7 mm/rev with 0.8 mm; 0.5-1.0 mm/rev with 1.2 mm.

On the shop floor

Choose the largest radius possible for a strong edge and a smaller one if there is vibration. Use a depth of cut of at least 2/3 of the radius to avoid vibration and poor chip formation.

Insert grade

Tools

ES
Calidad de plaquita
DE
Schneidstoffsorte
IT
Qualità dell'inserto
PT
Classe da pastilha
FR
Nuance de plaquette

Combination of cutting material and coating of an insert. The ISO 513 standard places it with a letter for the material group and a number: low for finishing and wear, high for roughing and impacts.

Example

HC-P10: coated carbide for finishing steel at high vc. HC-P25: general use in steel. HC-M30: roughing stainless. HW-K20: uncoated carbide for cast iron.

Typical values

ISO colors: P blue (steel), M yellow (stainless), K red (cast iron), N green (non-ferrous), S brown (superalloys and titanium), H gray (hard materials). Range from 01 to 50 depending on the group.

On the shop floor

ISO 513 classifies by application, not by composition: one brand's P25 is not another's P25. If the edge breaks, go up a number (tougher); if it wears, go down (more wear-resistant).

Inside micrometer

Measurement

ES
Micrómetro de interiores
DE
Innenmessschraube
IT
Micrometro per interni
PT
Micrómetro de interiores
FR
Micromètre d'intérieur

Micrometer that measures inside diameters directly. The three-contact type centers itself in the hole; the rod type is for large diameters with extensions.

Example

Hole Ø 25 with tolerance 0 / +0.021 mm. You set the micrometer zero on a 25.000 mm setting ring and on the part it reads 25.012 mm: it is within tolerance.

Typical values

Each three-contact head covers a short range: the Mitutoyo 368-166 measures from 20 to 25 mm, with 0.005 mm graduations and a maximum error of ±3 µm.

On the shop floor

Set the zero on the ring the same way you will measure: Mitutoyo warns that it does not read the same resting on the whole contact as on just the tip. Always use the ratchet.

Interrupted cut

Cutting parameters

ES
Corte interrumpido
DE
Unterbrochener Schnitt
IT
Taglio interrotto
PT
Corte interrompido
FR
Coupe interrompue

Cut in which the edge enters and leaves the material one or several times per revolution: shafts with keyways, parts with cross holes, castings with scale, or any milling. Each entry is an impact.

Example

Turning a shaft with a keyway at 1000 rpm, the edge takes 1000 impacts per minute, more than 16 per second, besides heating and cooling on every revolution.

Typical values

Ask for tough grades and strong geometries: negative insert, the largest nose radius the part allows and a large point angle. In stainless with impacts, PVD grades.

On the shop floor

With heavy interruptions, lower the starting cutting data. If the edge chips, try a tougher grade before a weaker geometry: toughness makes up for the lack of edge strength.

ISO material groups

Materials

ES
Grupos ISO de materiales
DE
ISO-Werkstoffgruppen
IT
Gruppi di materiali ISO
PT
Grupos de materiais ISO
FR
Groupes de matières ISO

ISO 513 classification that groups materials by how they machine, with a letter and a color. Manufacturers use it to indicate which materials each insert grade suits.

Example

A quenched and tempered 42CrMo4 is group P (blue); a 316L, M (yellow); a GG25, K (red); a 6082, N (green); an Inconel 718, S (brown); and a steel hardened to 58 HRC, H (gray).

Typical values

P steels (blue), M austenitic stainless steels (yellow), K cast irons (red), N non-ferrous (green), S heat-resistant alloys and titanium (brown), H hard materials (gray).

On the shop floor

In a grade like P25, the number runs from 01 (more wear-resistant, for higher speed) to 50 (tougher, for more feed and interrupted cuts).

IT tolerance grade

Tolerances and surface finish

Calculator
IT · µm
ES
Grado IT
DE
Toleranzgrad
IT
Grado di tolleranza IT
PT
Grau de tolerância IT
FR
Degré de tolérance IT

Number from ISO 286 that sets the tolerance size according to the diameter: the lower, the tighter. The 7 in H7 is the IT grade.

Example

Range from 18 to 30 mm: D = √(18 × 30) ≈ 23.2 mm, i ≈ 1.31 µm and IT7 = 16 × 1.31 ≈ 21 µm. At Ø 25: IT6 = 13, IT7 = 21, IT8 = 33 µm.

On the shop floor

The standard rounds the values in its table: use the table, not the formula, to accept a part.

J

Jaw chuck

Turning

ES
Plato de garras
DE
Backenfutter
IT
Mandrino a griffe
PT
Bucha de castanhas
FR
Mandrin à mors

Lathe workholding system in which several jaws close at the same time on the part. The three-jaw self-centering chuck is the most common; the four-jaw independent chuck lets you center by hand.

Typical values

Three-jaw self-centering chuck for round parts; four independent jaws, adjusted one by one with their screw, for irregular parts.

On the shop floor

Centrifugal force reduces clamping in proportion to the square of rpm, and more so with heavy or wide-open jaws. Respect the chuck's maximum rpm and clamp within the useful stroke of the jaws.

K

Knurling

Turning

ES
Moleteado
DE
Rändeln
IT
Zigrinatura
PT
Recartilhamento
FR
Moletage

Operation that marks a pattern of straight, diagonal or crossed ridges on a surface to grip it by hand or for a press fit. It is done by deformation, with rollers that press, or by cutting.

Example

Straight knurl by deformation with 1 mm pitch and final Ø 20 mm: turn beforehand to ≈ 20 − 0.5 × 1 = 19.5 mm, because the displaced material makes the diameter grow.

Typical values

Standardized pitches in DIN 403: 0.5, 0.6, 0.8, 1, 1.2 and 1.6 mm. Forms on the part according to DIN 82: straight (RAA), left or right-hand (RBL, RBR) and cross (RGE, RKE…).

On the shop floor

The pre-turn diameter factor changes with the form: 0.5 × pitch on straight and angled ones, 0.67 on cross with a protruding point and 0.33 with a recessed point. It is approximate: test it first. Use cutting oil on steel.

L

Left-hand thread

Drilling and threading

ES
Rosca a izquierdas
DE
Linksgewinde
IT
Filettatura sinistra
PT
Rosca esquerda
FR
Filetage à gauche

Thread that tightens by turning counterclockwise. Used where the working rotation would loosen a normal thread and where a connection must not be mixed up, as with fuel gases.

Example

M12 × 1.5 LH. On a lathe, the spindle can turn in either direction and the tool can feed toward the chuck or away from it; with a right-hand tool, the left-hand thread is made feeding outward.

Typical values

Examples: bicycle left pedal, rotating parts that a normal thread would loosen, and gas cylinder fittings.

On the shop floor

If you make the left-hand thread with a right-hand tool (or the other way around), mount a negative-inclination shim. On a milling machine, the left-hand tap uses its reverse cycle (G74 on Haas), with the spindle on M04.

Linear guides

Machine

ES
Guías lineales
DE
Linearführungen
IT
Guide lineari
PT
Guias lineares
FR
Guidages linéaires

Rails with ball or roller blocks on which the carriages of each axis move. Because they roll instead of sliding, there is hardly any difference between static and dynamic friction, and the axis moves without jerking.

Typical values

Balls with cage: low noise and high speeds. Rollers: much more rigidity. THK makes them from miniature sizes up to large sizes for machine tools.

On the shop floor

THK includes lubrication and dirt protection in choosing the guide: don't ignore the lubrication alarm and check that the wipers don't let chips through.

Linear interpolation

CNC programming

Calculator
ES
Interpolación lineal
DE
Linearinterpolation
IT
Interpolazione lineare
PT
Interpolação linear
FR
Interpolation linéaire

Straight-line motion at the programmed feed rate F, with all axes coordinated to arrive at the same time. It is the basic cutting motion: turning, facing, chamfers and straight contours.

Example

Lathe in G95 at 1500 rpm: G01 Z-40 F0.2 feeds F = 0.2 × 1500 = 300 mm/min. On a mill, with G94, the feed per minute is programmed directly: G01 X80 F300.

On the shop floor

G01 is modal, and so is G00: if after a G00 you forget to write G01 before entering material, the tool enters at rapid.

Linear scale

Machine

ES
Regla óptica
DE
Längenmessgerät
IT
Riga ottica
PT
Régua óptica
FR
Règle de mesure

Measuring system that reads the real position of the carriage on a fixed scale. With it the axis works in closed loop; without it, the control only knows how much the motor has turned (encoder) and assumes the rest.

Example

The screw heats up and grows 0.02 mm. With only the motor encoder, the dimension comes out 0.02 mm off and the control does not see it; with a scale, it measures where the table is and corrects it.

Typical values

Accuracy grades of Heidenhain scales for machine tools: ±5 and ±3 µm (some, ±2 µm). The closed loop corrects spindle heat, reversal backlash and pitch error.

On the shop floor

With a lot of coolant or mist, sealed scales are protected with compressed air, but clean: Heidenhain asks for it filtered according to ISO 8573-1. Dirty or oily air fouls them inside.

Longitudinal turning

Turning

Calculator
ES
Cilindrado
DE
Längsdrehen
IT
Tornitura longitudinale
PT
Torneamento longitudinal
FR
Chariotage

Lathe operation in which the tool feeds parallel to the part axis to reduce its outside diameter. It is the most common pass, in both roughing and finishing.

Example

Ø 40 mm at vc = 200 m/min: n = 200 × 1000 / (π × 40) ≈ 1592 rpm. With f = 0.25 mm/rev, vf ≈ 398 mm/min and 80 mm are turned in about 12 s.

Typical values

Sandvik example for medium machining of steel: f 0.2-0.4 mm/rev with ap 2 mm. On the CNMG 120408, -PM is the first choice; -PF for low ap and feed, -PR for high.

On the shop floor

Don't use a depth of cut smaller than about 2/3 of the nose radius: the edge rubs, vibrates and the chip forms badly. That is why the nose radius should be equal to or smaller than ap.

Look-ahead

CNC programming

ES
Look-ahead
DE
Vorausschau
IT
Look-ahead
PT
Look-ahead
FR
Anticipation de blocs

Ability of the control to read many blocks ahead to calculate where to brake and accelerate. With it, CAM programs with very short segments run smoothly without losing the shape at corners.

Example

Fanuc: G05.1 Q1 at the start of the CAM finishing and G05.1 Q0 at the end, each in its own block. On Siemens it is activated with CYCLE832 and the tolerance; on Heidenhain, with CYCL DEF 32 TOLERANCE (T0.01).

Typical values

Fanuc 16i/18i reads 40 blocks ahead in AI contour control and 180 in AI nano contour control; Haas, 80 blocks.

On the shop floor

On Haas, look-ahead also calculates macros 80 blocks before the motion. In programs with macros and short moves, limit it with G103 P1, as Haas indicates.

M

M-code

CNC programming

ES
Código M
DE
M-Funktion
IT
Codice M
PT
Código M
FR
Code M

Miscellaneous function that turns on or stops something on the machine that is not a motion: spindle, coolant, tool change, stops and program end. Many are defined by each machine builder.

Example

T5 M06 · S2000 M03 · M08 … M09 · M05 · M30. Loads tool 5, starts the spindle clockwise at 2000 rpm, turns on the coolant, at the end turns it off, stops the spindle and ends the program.

Typical values

Almost universal: M00 stop, M01 optional stop, M03/M04/M05 spindle, M06 tool change, M08/M09 coolant, M30 end of program and M98/M99 subprogram (Fanuc).

On the shop floor

Each control limits how many M-codes fit in a block: Siemens allows up to five. And free M-codes are defined by the manufacturer: the same M may do something else on another machine.

Machinability

Materials

%
ES
Maquinabilidad
DE
Zerspanbarkeit
IT
Lavorabilità
PT
Maquinabilidade
FR
Usinabilité

Ease with which a material is machined: tool life, forces, finish and chip form. It is usually given as a percentage against a reference free-cutting steel.

Example

If you work at 250 m/min on the reference steel, a material with a 50 % rating will call for about 250 × 0.5 = 125 m/min as a starting point to last as long.

Typical values

With AISI B1112 free-machining steel as 100 %: Ti6Al4V ≈ 21 % and Inconel 718 ≈ 18 %. On another scale, from one manufacturer: austenitic ≈ 60 %, duplex ≈ 30 %.

On the shop floor

The index is indicative and changes a lot with the condition of the material: the same steel annealed or quenched and tempered, or with or without added sulfur, machines very differently.

Machine vise

Machine

ES
Mordaza
DE
Maschinenschraubstock
IT
Morsa
PT
Torno de máquina
FR
Étau

Mill workholding with a fixed jaw and a movable one that clamps the part. It is the most used workholding for prismatic parts; the part rests on parallels to bring it to the right height.

Example

You run the indicator along the fixed jaw over 100 mm in X and it reads 0.02 mm: the vise is rotated by atan(0.02 / 100) ≈ 0.011°. You loosen, tap gently and repeat until the needle does not move.

Typical values

Jaw openings from 46 to 125 mm in the LANG Makro•Grip range for 5 axes. On centering ones, both jaws move at the same time and center the part.

On the shop floor

On a centering vise, take the origin of the clamping axis at the center of the vise, not on one jaw. And check the alignment again with the indicator every time you remove it.

Machine zero

CNC programming

ES
Cero máquina
DE
Maschinennullpunkt
IT
Zero macchina
PT
Zero máquina
FR
Origine machine

Fixed point that the manufacturer defines as the origin of the machine coordinates; everything else is measured from it. With incremental encoders you must reference the axes at power-up; with absolute ones, you don't.

Example

G91 G28 Z0 · G28 X0 Y0: raises Z straight to the reference and then moves X and Y. With G53 G00 Z0 you go to Z0 in machine coordinates. On Siemens: G0 SUPA Z0, or G75 FP=1 Z0 to a fixed point.

On the shop floor

G28 Z0 in absolute (G90) first passes through the part's Z0, which is usually its surface: the tool goes down before going up. Write it with G91 G28 Z0.

Machining centre

Machine

ES
Centro de mecanizado
DE
Bearbeitungszentrum
IT
Centro di lavoro
PT
Centro de maquinagem
FR
Centre d'usinage

CNC milling machine with an automatic tool changer, able to mill, drill, tap and bore in a single setup. They come vertical and horizontal, the latter often with pallet changing.

Typical values

Medium vertical: DN Solutions DNM 5700, X 1050, Y 570 and Z 510 mm, 8000 rpm as standard and 30 tools; DMG MORI CMX V, X 600-1100, Y 560 and Z 510 mm, 12000 rpm.

On the shop floor

Compare the travels with your largest part plus the clamping: with 1050 mm in X a 1050 mm plate with vises on the sides won't fit, nor can you reach its edges with the cutter.

Maximum material condition

Tolerances and surface finish

Calculator
Ⓜ
ES
Condición de máximo material
DE
Maximum-Material-Bedingung
IT
Condizione di massimo materiale
PT
Condição de máximo material
FR
Condition du maximum de matière

Size at which the part has the most material: the smallest hole or the thickest shaft. With the Ⓜ symbol, the geometric tolerance grows the further the part moves from that size.

Example

Hole Ø 10 +0.1/0 with position Ø 0.2 Ⓜ: MMC = 10.0 mm. If it comes out at Ø 10.08, the position tolerance becomes 0.2 + 0.08 = Ø 0.28 mm. A gauge with a Ø 9.8 pin (10.0 − 0.2) checks the assembly.

On the shop floor

Ⓜ is used on screw and pin holes: what matters is that it assembles. If a hole comes out shifted, enlarging it within tolerance can save the part. Check with a functional gauge.

Measurement uncertainty

Measurement

U · µm
ES
Incertidumbre de medida
DE
Messunsicherheit
IT
Incertezza di misura
PT
Incerteza de medição
FR
Incertitude de mesure

Range around the measured value within which the real value lies, with a given probability. It adds up the instrument, the standard, the temperature, the operator and the part itself.

Example

Hole 25 H7 (25.000-25.021 mm) measured with U = 0.003 mm: to prove it is good, it is only accepted between 25.003 and 25.018 mm (ISO 14253-1).

Typical values

It is normally given with k = 2, that is, with about 95 % probability. It should not exceed 1/10 of the tolerance (1/5 if there is no other option).

On the shop floor

A measurement without uncertainty is incomplete: two people who measure differently can both be right. Measure several times and under the same conditions before rejecting a part at the limit.

Metal removal rate

Cutting parameters

Calculator
Q · cm³/min
ES
Caudal de viruta
DE
Zeitspanvolumen
IT
Volume di truciolo asportato
PT
Taxa de remoção de metal
FR
Débit de copeaux

Volume of material removed per minute. It is used to compare roughing strategies and to estimate the power that will be needed.

Example

Milling with ap = 10 mm, ae = 4 mm and vf = 800 mm/min: Q = 10 × 4 × 800 / 1000 = 32 cm³/min. On a lathe: Q = vc × ap × f.

On the shop floor

In slots, trochoidal milling swaps ae for ap: Sandvik proposes it with ae up to 20 % of D and ap up to 2 × D, with heat and wear spread along the whole edge.

Micrometer

Measurement

Calculator
ES
Micrómetro
DE
Bügelmessschraube
IT
Micrometro
PT
Micrómetro
FR
Micromètre

Instrument that measures with a threaded spindle of very precise pitch: each turn of the thimble advances one pitch, and the divided thimble gives the fractions. It is the usual hundredth-of-a-millimeter measurement in the shop.

Example

0.5 mm spindle and a 50-division thimble: 0.5 / 50 = 0.01 mm. You see 12 mm and the half-millimeter line (12.5) and the thimble reads 28: 12.5 + 0.28 = 12.78 mm.

Typical values

Ranges in 25 mm steps (0-25, 25-50…). Resolution of 0.01 mm, or 0.001 mm with vernier or digital. A catalog 0-25 mm mechanical micrometer allows ±2 µm error.

On the shop floor

Always close with the ratchet or the friction thimble, not the thimble itself: that way everyone applies the same force. Set zero with the standard for the range and don't hold it in your bare hand: the heat lengthens it.

Minimum quantity lubrication

Materials

ES
Mínima cantidad de lubricante
DE
Minimalmengenschmierung
IT
Lubrificazione minimale
PT
Lubrificação em quantidade mínima
FR
Microlubrification

System that delivers to the edge an air mist with very little oil, instead of flooding the area with coolant. The lubricant is consumed in the process: the chips come out almost dry and there is no emulsion to maintain.

Typical values

About 5-50 ml of lubricant per hour of cutting, with synthetic esters or fatty alcohols.

On the shop floor

It works especially well in gray cast iron, low-silicon aluminum and steels up to about 800 N/mm². In demanding processes, deliver it through the tool.

Mirror image

CNC programming

ES
Imagen espejo
DE
Spiegeln
IT
Immagine speculare
PT
Imagem espelho
FR
Image miroir

Function that reverses the sign of one or several axes about a line, to machine the symmetrical part (left and right) with the same program or subprogram.

Example

G51.1 X0 · M98 P1000 · G50.1 X0: repeats the subprogram contour mirrored about X0; a point at X30 comes out at X-30 and each G02 is made as G03. On Siemens: MIRROR X0; on Heidenhain: CYCL DEF 8 MIRROR IMAGE.

Typical values

When mirroring a single axis, arcs are reversed (G02 ↔ G03) and so is compensation (G41 ↔ G42). Mirroring two axes at once, the machining direction returns to the original.

On the shop floor

With a single axis mirrored, climb milling becomes conventional milling: the finish and size may change between the original part and the mirrored one. And always cancel the mirror before continuing.

Modal code

CNC programming

ES
Código modal
DE
Selbsthaltende Funktion
IT
Codice modale
PT
Código modal
FR
Fonction modale

Code that stays active in the following blocks until another from the same group changes it, such as G01, G90, F or S. Non-modal ones, such as G04 (dwell), only apply in their own block.

Example

G01 X50 F200 · Y30 · X0: all three lines cut in a straight line at 200 mm/min, even though only the first has G01 and F. To return to rapid you must write G00.

On the shop floor

When starting mid-program, the control may not have the earlier modal codes active (G41, G43, F, plane). Start at a block that repeats them all or use block search with calculation.

Multi-start thread

Drilling and threading

Calculator
Ph · mm
ES
Rosca de varias entradas
DE
Mehrgängiges Gewinde
IT
Filettatura a più principi
PT
Rosca de várias entradas
FR
Filetage à plusieurs filets

Thread with two or more starts that wind in parallel. With the same pitch it advances more per revolution, so it moves quickly without making the thread deeper or weakening the core.

Example

Tr 20 × 8 P4: two starts with 4 pitch, lead 8 mm. The first start is cut with F8 and then the second with the start shifted one pitch, 4 mm in Z. At 300 rpm, the carriage runs at 2400 mm/min.

Typical values

The helix is steeper: on Tr 20 × 8 P4 about 8° at the pitch diameter, compared to 4° with one start. The shim is chosen from the lead, not the pitch.

On the shop floor

Make one complete start with all its passes and then the next. Instead of offsetting in Z, some controls offset the spindle starting angle (360° / z), such as the Q address of G32 on Haas.

N

Net power

Cutting parameters

Calculator
Pc · kW
ES
Potencia de corte
DE
Nutzleistung
IT
Potenza netta
PT
Potência líquida
FR
Puissance nette

Power consumed by the cut at the cutting edge. It is compared with the spindle motor's to know whether the machine can handle the pass you want to take.

Example

Turning with ap = 3 mm, f = 0.3 mm/rev, vc = 200 m/min and kc = 2000 N/mm²: Pc = 3 × 0.3 × 200 × 2000 / 60000 = 6 kW.

On the shop floor

It is the power at the edge: divide by the machine efficiency (Keyence calculates with 0.8) to get the motor's. In milling: Pc = ap × ae × vf × kc / (60 × 10⁶).

Nitriding

Materials

ES
Nitrurado
DE
Nitrieren
IT
Nitrurazione
PT
Nitruração
FR
Nitruration

Treatment that diffuses nitrogen into the steel surface at about 500 °C. It forms a thin, very hard layer without quenching, so the part hardly distorts.

Typical values

Gas: 470-530 °C (Bodycote); gas and plasma, 500-540 °C (Gerster). Standard depth of 0.3-0.6 mm depending on process and steel. Steels with chromium and aluminum exceed 1000 HV.

On the shop floor

The compound layer (5-20 µm) makes the part grow slightly: compensate for that change in the prior machining. If it is quenched and tempered, nitride at least 30 °C below its tempering temperature.

Nose radius

Turning

DrawingCalculator
rε · mm
ES
Radio de punta
DE
Eckenradius
IT
Raggio di punta
PT
Raio de ponta
FR
Rayon de bec

Radius that rounds the insert tip. Together with the feed it sets the theoretical roughness, and it also gives the edge strength: a larger radius withstands more, but pushes harder and vibrates sooner.

Example

f = 0.2 mm/rev and rε = 0.8 mm: Rt ≈ 0.04 × 1000 / 6.4 ≈ 6.3 µm. With double the radius (1.6 mm) the theoretical roughness halves, ≈ 3.1 µm.

Typical values

Indicative maximum feed according to Sandvik: 0.25-0.35 mm/rev with rε 0.4 mm; 0.4-0.7 with 0.8; 0.5-1.0 with 1.2; 0.7-1.3 with 1.6. It is the last pair of digits of the code (08 = 0.8 mm).

On the shop floor

Set a depth of cut of at least 2/3 of the nose radius. If you cut less, the insert rubs on the curve, vibrates and the chip forms badly.

Notch wear

Tools

ES
Desgaste en entalla
DE
Kerbverschleiß
IT
Usura a intaglio
PT
Desgaste em entalhe
FR
Usure en entaille

Notch that forms on the cutting edge right at the depth of cut line. It weakens the edge at that point and leaves the surface with burr or a poor finish.

Typical values

It appears mostly in stainless and superalloys, which work-harden, and when cutting forging or casting scale. Also with edge oxidation at high temperature.

On the shop floor

Vary the depth of cut between passes to spread the wear, use a smaller lead angle (45° or round insert) and a sharper edge. Lowering vc a little also helps.

Number of teeth

Milling

Calculator
z
ES
Número de dientes
DE
Zähnezahl
IT
Numero di denti
PT
Número de dentes
FR
Nombre de dents

Number of cutting edges on the cutter. It multiplies the feed per tooth to give the feed rate, and determines how much room is left for the chip between one edge and the next.

Example

4-flute end mill at 8000 rpm with fz = 0.05 mm: vf = 0.05 × 4 × 8000 = 1600 mm/min. With 2 flutes and the same fz, only 800 mm/min.

Typical values

Sandvik: coarse pitch (few teeth) for unstable setups and aluminum; normal pitch for roughing in steel, stainless and superalloys; close pitch for cast iron and small ae.

On the shop floor

More teeth give more feed, but less room for the chip. In long-chipping materials and setups that vibrate, few teeth; with small ae, more so that more than one always cuts.

O

On-machine measurement

Measurement

ES
Medición en máquina
DE
Messen in der Maschine
IT
Misura in macchina
PT
Medição na máquina
FR
Mesure sur machine

Measuring the part with the machine's own probe, without unclamping it. Used to correct the tool offsets and rework before releasing the part.

Example

A diameter programmed at 40.000 mm measures 40.018 mm with the probe: 0.018 mm too much on diameter, that is, (40.018 − 40.000) / 2 = 0.009 mm per side, which you correct in the wear offset before the finish pass.

Typical values

Standard Renishaw probes, such as the OMP40-2 for machining centers or the OLP40 for lathes, have a unidirectional repeatability of 1 µm (2σ).

On the shop floor

The machine measures itself: its geometric and thermal errors are not seen. Validate with parts measured outside and let the part cool after heavy roughing.

Optional stop

CNC programming

ES
Parada opcional
DE
Wahlweiser Halt
IT
Arresto opzionale
PT
Paragem opcional
FR
Arrêt optionnel

Program stop with M01 that only happens if the operator has the optional stop button on. Unlike M00, which always stops, M01 lets you prove out with pauses and produce without them.

Example

… M09 · M05 · G91 G28 Z0 · M01 · T2 M06 · S1800 M03 · M08. With optional stop on, the machine stops at the end of each tool so you can check; when off, it keeps going. On Siemens it is M01 and on Heidenhain, M1.

Typical values

It goes at the end of each tool, before the change: on the first part you turn it on to check chips and sizes; in production you turn it off.

On the shop floor

What the machine does at the stop (whether it stops the spindle and coolant or not) depends on the manufacturer, Fanuc warns. Just in case, repeat S, M03 and M08 after M01, as in the example.

Override

CNC programming

ES
Override
DE
Override
IT
Override
PT
Override
FR
Override

Panel selector that instantly changes the programmed feed, rapids or spindle speed, as a percentage and without touching the program. Used to test cautiously and to adjust the cut by watching the chip.

Example

Program with F300 and feed override at 80 %: the machine feeds at 300 × 0.8 = 240 mm/min. Returning to 100 % restores the programmed 300 mm/min.

Typical values

EMCO panel with Fanuc 31i: feed and spindle from 0 to 120 %; in rapid it does not go above 100 % and it has no effect when threading. On Siemens, the programmed override (OVR) goes up to 200 %.

On the shop floor

When testing a new program, lower the rapids and leave the feed at 0 near the part; compare the distance to go on the screen with what you expect before letting it run.

P

Parallelism

Tolerances and surface finish

ES
Paralelismo
DE
Parallelität
IT
Parallelismo
PT
Paralelismo
FR
Parallélisme

Orientation tolerance that requires a face or an axis to lie between two planes, or inside a cylinder, parallel to the datum and separated by the stated value.

Example

Plate resting on its face A on the surface plate; you run the indicator over the top face and it reads from 0.000 to 0.015 mm: parallelism 0.015 mm. With a 0.02 tolerance, it passes.

On the shop floor

Without a datum there is no parallelism: rest face A, well cleaned, directly on the surface plate and run the indicator over several lines of the top face, not just one.

Parametric programming

CNC programming

ES
Programación paramétrica
DE
Parameterprogrammierung
IT
Programmazione parametrica
PT
Programação paramétrica
FR
Programmation paramétrée

Programming with variables instead of fixed numbers, with calculations, conditions and loops. A single program serves a family of parts or repeats passes changing only one value.

Example

Fanuc: #100=20 · #101=#100/2 · G01 X#101 F200. Siemens: R1=20 · R2=R1/2 · G1 X=R2 F200. Heidenhain: FN 0: Q1 = +20 · FN 4: Q2 = +Q1 DIV +2 · L X+Q2 F200. All three take the tool to X10.

Typical values

Fanuc: #1-#33 local, #100-#149 are cleared at power-off and #500-#531 are retained (more with an option). Siemens: R parameters from R0, as many as machine data MD28050 sets. Heidenhain: Q0-Q1999.

On the shop floor

On Fanuc, a calculation inside an address goes in square brackets: G01 X[#1+#2]. And an empty variable is not zero: with #2 empty, G00 X#1 Y#2 executes without the Y.

Parting off

Turning

ES
Tronzado
DE
Abstechen
IT
Troncatura
PT
Sangramento
FR
Tronçonnage

Radial cut to the center that separates the finished part from the bar. It is one of the most delicate lathe operations because the tool is narrow and long.

Example

3000 mm bar, 40 mm part and 3 mm parting blade: each part uses 43 mm. Not counting the final remnant, 3000 / 43 ≈ 69.8, that is, 69 parts.

Typical values

Sandvik: center height ±0.1 mm; reduce the feed by up to 75 % from about 2 mm before center and stop the feed about 0.5 mm before: breakages occur at the center.

On the shop floor

Stick the blade out just enough and part off close to the chuck. If the overhang exceeds 1.5 times the blade height, lower the feed to the lower end of the recommended range for the geometry.

Passive force

Cutting parameters

Fp · N
ES
Fuerza radial o pasiva
DE
Passivkraft
IT
Forza passiva
PT
Força passiva
FR
Effort passif

Component of the cutting force perpendicular to the machined surface: on a lathe, the one that pushes the tool away from the part radially. It does not consume power, but it deflects the part and the tool.

Typical values

It grows with small κr (45°, round inserts), with large nose radii and when ap is smaller than the nose radius. As ap increases, part of it becomes axial.

On the shop floor

On slender parts or in boring, use κr near 90° (never below 75° on internal work), a nose radius equal to or smaller than ap and, if it vibrates, a smaller radius.

Peck drilling

Drilling and threading

ES
Taladrado con picoteo
DE
Bohren mit Entspanen
IT
Foratura con scarico truciolo
PT
Furação com descarga de apara
FR
Perçage avec débourrage

Peck drilling: the drill plunges a depth Q, retracts to break or clear the chip and goes back in. It prevents the chip from clogging the flutes and breaking the drill.

Example

Hole 40 mm deep with Q = 8 mm: the cycle makes 40 / 8 = 5 pecks. With G83 the drill returns to the R plane after each one; with G73 it only retracts a little to break the chip.

Typical values

On Haas, G73 retracts after each peck by the amount set in setting 22 (0.5 mm by default). Sandvik requires internal coolant on its carbide drills from 3 × D.

On the shop floor

Use G73 when the chip only needs to be broken and G83 when it jams. On Haas you can give I, J and K (first peck, reduction and minimum peck) instead of Q.

Perpendicularity

Tolerances and surface finish

ES
Perpendicularidad
DE
Rechtwinkligkeit
IT
Perpendicolarità
PT
Perpendicularidade
FR
Perpendicularité

Orientation tolerance that requires a face or an axis to lie between two planes, or within a cylinder, at exactly 90° to the datum and of the stated width.

Example

Perpendicularity 0.05 relative to A on a face 100 mm high: equivalent to deviating at most about 0.029° (0.05 / 100 as a tangent).

On the shop floor

Square and feeler gauge are fine for a quick check, but they are not very accurate. With a measuring machine, first take the datum with several points and then measure the face.

Pitch diameter

Drilling and threading

Calculator
d2 · mm
ES
Diámetro de flancos
DE
Flankendurchmesser
IT
Diametro medio
PT
Diâmetro de flancos
FR
Diamètre sur flancs

Diameter of an imaginary cylinder that cuts the thread flanks where the solid and the space are equal in width. It is the diameter that decides whether a thread fits and the one checked in quality control.

Example

M10 × 1.5: d2 = 10 − 0.6495 × 1.5 ≈ 9.026 mm (nominal value; the 6g or 6H tolerance puts it slightly below or above).

On the shop floor

It is not measured with a caliper: use a thread micrometer, the three-wire method (optimum wire ≈ 0.577 × P on 60° threads) or a go / no-go gauge.

Plastic deformation

Tools

ES
Deformación plástica
DE
Plastische Verformung
IT
Deformazione plastica
PT
Deformação plástica
FR
Déformation plastique

The edge softens from temperature and pressure and sinks or bulges, especially at the tip. The geometry changes, the size drifts and in the end the edge breaks.

Typical values

Causes: cutting temperature and pressure too high for the grade, grade too soft, materials that conduct heat poorly and insufficient coolant.

On the shop floor

If the edge sinks, lower the feed first; if the flank bulges, lower vc first. Use a harder grade (lower ISO number), a larger nose radius and improve the coolant.

Plunge milling

Milling

ES
Fresado por penetración
DE
Tauchfräsen
IT
Fresatura a tuffo
PT
Fresagem por mergulho
FR
Fraisage en plongée

Roughing in which the cutter goes down in Z as if drilling and moves sideways between one plunge and the next. The force goes along the spindle, so it tolerates long overhangs without chatter.

Example

120 mm stretch with 8 mm between plunges: 120 / 8 = 15 plunges. At 40 mm depth and vf = 400 mm/min, each plunge takes 6 s: ≈ 1.5 min of cutting plus the retracts.

Typical values

Sandvik: overhang greater than 4 × D, low stability or power, deep slots and 90° corners. Stepover 0.75 × D with overhang under 3 × D; otherwise 0.5 × D.

On the shop floor

At the end of each plunge, move 1 mm away from the wall before retracting, and don't use a drilling cycle, because it cuts again on retract. Leave constant stock for finishing.

Pocket milling

Milling

ES
Cajeado
DE
Taschenfräsen
IT
Fresatura di tasche
PT
Fresagem de caixas
FR
Usinage de poches

Removal of a closed area of the part down to a depth, leaving walls and a floor. The cutter has to plunge into the material, clear the chip and finish the corners.

Typical values

Sandvik: cutter diameter at most 1.5 times the corner radius (cutter radius ≈ 75 % of the corner radius); use the largest cutter possible and clean up the corners separately.

On the shop floor

To enter, a linear ramp on two axes is better than plunging. With cutters that don't cut at center, use one with a small lead angle or round inserts, or drill first.

Point angle

Drilling and threading

DrawingCalculator
σ · °
ES
Ángulo de punta de broca
DE
Spitzenwinkel
IT
Angolo di punta
PT
Ângulo de ponta
FR
Angle de pointe

Angle formed by the two main cutting edges at the drill point. It determines how well it centers on entry and how much point length must be added to the programmed depth.

Example

Ø 10 mm drill at 118°: L = 5 / tan(59°) ≈ 3.0 mm. With a 140° one: L = 5 / tan(70°) ≈ 1.8 mm. For 20 mm of full-diameter depth program Z−23 or Z−21.8.

Typical values

118° on general-purpose high-speed steel drills (Mitsubishi Materials); 135-140° on carbide drills (Hartner).

On the shop floor

If the drawing dimensions the cylindrical part of the blind hole and you program the depth to the tip, the hole ends up short by exactly the length of the tip.

Polycrystalline diamond (PCD)

Tools

ES
PCD (diamante policristalino)
DE
Polykristalliner Diamant (PKD)
IT
Diamante policristallino (PCD)
PT
Diamante policristalino (PCD)
FR
Diamant polycristallin (PCD)

Composite of diamond particles sintered with a metallic binder. It is the right edge for non-ferrous and abrasive materials, such as high-silicon aluminum and composites.

Typical values

High-silicon aluminum, metal matrix composites and carbon-fiber plastics. For turning aluminum with more than 13 % silicon, Sandvik indicates PCD because carbide lasts very little.

On the shop floor

Don't use it on steel or cast iron: at high temperature diamond loses chemical stability and dissolves into the iron.

Position tolerance

Tolerances and surface finish

Calculator
ES
Tolerancia de posición
DE
Positionstoleranz
IT
Tolleranza di posizione
PT
Tolerância de posição
FR
Tolérance de localisation

Zone, normally a cylinder of diameter t, centered on the exact theoretical position of a feature, such as the axis of a hole, measured from the datums.

Example

Hole displaced Δx = 0.02 and Δy = 0.03 mm: real Ø = 2 × √(0.02² + 0.03²) ≈ 0.072 mm. With a Ø 0.1 tolerance it is fine.

On the shop floor

A ±0.05 in X and Y is a square; the circular zone around it (Ø 0.14) has 57 % more area. Don't convert position to ± without thinking. With Ⓜ there is extra tolerance.

Post-processor

CNC programming

ES
Postprocesador
DE
Postprozessor
IT
Postprocessore
PT
Pós-processador
FR
Post-processeur

Part of the CAM that translates toolpaths into the exact dialect of a machine and its control: G and M codes, number format, tool changes, rotary axes and safety header.

Example

The same arc comes out as G02 X20 Y0 R10 F200 with a Fanuc post and as CC X+10 Y+0 · C X+20 Y+0 DR- F200 with a Heidenhain one.

On the shop floor

Each machine accepts or interprets some codes in its own way: one makes arcs and another asks for them in straight segments. Use a post-processor adjusted to your machine and dry-run the first program.

Process capability index Cpk

Tolerances and surface finish

Calculator
Cpk
ES
Índice Cpk
DE
Prozessfähigkeitsindex Cpk
IT
Indice di capacità Cpk
PT
Índice de capacidade Cpk
FR
Indice de capabilité Cpk

Index that tells whether a process produces within tolerance with margin, taking into account the spread and how well centered it is. The higher, the fewer bad parts.

Example

Ø 25 ± 0.02 mm with mean 25.005 and σ = 0.004 mm: Cpk = min(0.015; 0.025) / 0.012 = 1.25. Centered, Cp would be 0.04 / 0.024 ≈ 1.67.

Typical values

With the process centered, Cp = 1 leaves 0.27 % outside and Cp = 1.33 about 64 ppm. Minimum Cp according to Montgomery: 1.33 for existing processes and 1.67 for new ones with a critical characteristic.

On the shop floor

If Cp is good and Cpk is not, the process is off-center: correcting the wear offset is enough. If Cp is also poor, the spread must be reduced.

Profile turning

Turning

ES
Copiado o perfilado
DE
Kopierdrehen
IT
Tornitura di profilo
PT
Torneamento de perfis
FR
Copiage

Turning in which the tool follows a contour with straight, tapered and curved sections in a single pass. It requires that the insert and the toolholder do not rub on the descending sections.

Typical values

Sandvik: first choice κr of 93° with a 55° rhombic insert (D); the 35° (V) for steeper plunges. Leave at least 7° of clearance on the plunge for finishing.

On the shop floor

Turn on cutter (nose) radius compensation (G41/G42): it is only needed on tapers and radii, which is exactly where a profile would come out off size without it.

Q

Quenching and tempering

Materials

ES
Bonificado
DE
Vergüten
IT
Bonifica
PT
Têmpera e revenido
FR
Trempe et revenu

Hardening followed by a high-temperature temper. It gives steel much higher strength than the annealed state without losing toughness, and it can still be machined with standard carbide.

Example

A 42CrMo4+QT from 16 to 100 mm in diameter comes in at 900-1200 MPa; according to the ISO 18265 table, that is about 265 to 355 HB.

Typical values

42CrMo4+QT: 1100-1300 MPa up to 16 mm, 1000-1200 MPa from 16 to 40 mm and 900-1100 MPa from 40 to 100 mm. Annealed (+A), max. 241 HB.

On the shop floor

The thicker the bar, the less strength the quenched and tempered condition reaches: check the diameter on the certificate and adjust vc to the actual condition, not to the annealed one.

R

Radial depth of cut

Cutting parameters

Drawing
ae · mm
ES
Ancho de corte
DE
Radiale Schnitttiefe
IT
Profondità di taglio radiale
PT
Profundidade radial de corte
FR
Profondeur de coupe radiale

Part of the cutter diameter that is inside the material, measured perpendicular to the tool axis. Together with ap it defines how hard the cutter works and how much the chip thins.

Example

Contouring with a Ø 16 mm end mill at 25 % of the diameter: ae = 0.25 × 16 = 4 mm. In slotting, ae = 16 mm (the whole cutter).

Typical values

Slotting: ae = D. Trochoidal (Sandvik): ae up to 20 % of D and ap up to 2 × D. Face milling (Sandvik): cutter 20-50 % larger than the workpiece width.

On the shop floor

With ae less than half the diameter, the chip comes out thinner than the programmed fz: increase the feed to recover the thickness, as explained by chip thinning.

Rake angle

Tools

γ · °
ES
Ángulo de desprendimiento
DE
Spanwinkel
IT
Angolo di spoglia superiore
PT
Ângulo de saída
FR
Angle de coupe

Inclination of the face the chip flows over. If positive, the edge cuts more smoothly and with less force; if negative, the edge is sturdier and withstands impacts.

Typical values

Positive geometry: less cutting force, the one Sandvik proposes for internal turning and slender parts. Negative inserts: stronger edge, first choice for heavy cuts.

On the shop floor

If the machine runs short of power or the part is thin and vibrates, move to a more positive geometry and a sharper edge: cutting forces drop.

Ramping

Milling

Calculator
ES
Entrada en rampa
DE
Rampeneintauchen
IT
Entrata in rampa
PT
Entrada em rampa
FR
Plongée en rampe

Way of lowering the cutter into the material by moving diagonally, instead of plunging straight down. It spreads the load and allows entry with cutters that don't cut well at center.

Example

Going down 3 mm with a 3° ramp: L = 3 / tan 3° ≈ 57 mm. If the pocket is shorter, make back-and-forth ramps or a helix.

Typical values

With insert cutters, the maximum ramping angle depends on the cutter diameter and the insert radius: Sandvik gives it in charts for each insert size.

On the shop floor

To open holes, Sandvik always prefers a linear ramp on two axes to plunging. With cutters that don't cut at center, choose one with a small lead angle or round inserts.

Rapid traverse

CNC programming

ES
Movimiento rápido
DE
Eilgang
IT
Movimento in rapido
PT
Movimento rápido
FR
Avance rapide

Movement at the machine's maximum speed to bring the tool in or out without cutting. It is programmed with G00 and does not use feed F: the speed is set by the machine manufacturer.

Example

G00 X50 Y20 · G00 Z2 · G01 Z-5 F120. You position in XY at a safe height, go down at rapid to 2 mm above the part and enter cutting with G01.

Typical values

A current vertical center (DN Solutions DNM 5700) rapids at 42 m/min in X and Y and 36 m/min in Z. In G00, the feed override does not go above 100 %.

On the shop floor

In G00 the axes may not move in a straight line: on Siemens, with RTLIOF each axis moves on its own and the path makes an elbow. Raise Z first and then move in XY.

Reaming

Drilling and threading

ES
Escariado
DE
Reiben
IT
Alesatura
PT
Alargamento
FR
Alésage à l'alésoir

Finishing an already drilled hole with a multi-flute reamer, removing very little material. It leaves the hole on size, round and with a good finish, for tight tolerances such as H7.

Example

Hole Ø 10 H7 in steel: Sandvik's table gives 0.2 mm of stock between 5.1 and 10 mm, so you drill at 10 − 0.2 = 9.8 mm and ream.

Typical values

Stock in steel according to Sandvik: 0.1-0.2 mm up to Ø 5 mm; 0.2 mm from 5.1 to 10; 0.2-0.3 mm from 10.1 to 20; 0.3-0.4 mm from 20.1 to 30; 0.3-0.5 mm above that.

On the shop floor

With little stock the reamer rubs, wears quickly and the hole loses size. And it does not correct the position or straightness of the previous hole: if it is crooked, it will stay crooked.

Reference temperature

Measurement

Calculator
°C
ES
Temperatura de referencia
DE
Bezugstemperatur
IT
Temperatura di riferimento
PT
Temperatura de referência
FR
Température de référence

Drawing dimensions are valid at 20 °C, according to ISO 1. If the part or the instrument is at another temperature, they expand and the measurement changes even if the part is good.

Example

42CrMo4 part of 200 mm at 28 °C, with α ≈ 12.1 µm/(m·°C): ΔL = 12.1 × 0.2 × 8 ≈ 19 µm. In 6082 aluminum, with α ≈ 23.4, it would be about 37 µm.

Typical values

Averages between 20 and 100 °C: 42CrMo4 ≈ 12.1 µm/(m·°C), 1.4301 stainless ≈ 16, 6082 aluminum ≈ 23.4. Steel gauge blocks ≈ 10.8.

On the shop floor

If part and instrument are both steel and equally warm, the error almost cancels out. The problem is measuring warm aluminum with a steel micrometer, or a part fresh off the machine.

Repeatability and gauge R&R

Measurement

Calculator
%R&R · %
ES
Repetibilidad y R&R
DE
Wiederholbarkeit und R&R
IT
Ripetibilità e R&R
PT
Repetibilidade e R&R
FR
Répétabilité et R&R

Repeatability is how much the reading varies when measuring the same thing several times with the same instrument and operator; reproducibility, how much it varies between operators. The R&R study compares both with the tolerance.

Example

Tolerance of 0.05 mm and σR&R = 0.002 mm: %R&R = 6 × 0.002 / 0.05 × 100 = 24 %. Acceptable depending on the use, but it eats almost a quarter of the tolerance.

Typical values

AIAG criterion: below 10 % the system is adequate; from 10 to 30 %, acceptable depending on the application and cost; above 30 %, not acceptable.

On the shop floor

Minitab asks for at least 10 parts, 3 operators and 2 measurements of each part per operator, in random order. With more parts the estimate improves.

Resolution

Measurement

ES
Resolución
DE
Auflösung
IT
Risoluzione
PT
Resolução
FR
Résolution

The smallest variation the instrument can display, for example 0.01 mm. It is not the same as its accuracy: a 0.01 mm digital caliper can be wrong by 0.02 mm.

Example

Ø 20 h7 has 0.021 mm of tolerance. With the 1/10 rule: 0.021 / 10 ≈ 0.002 mm of uncertainty at most, so a 0.01 mm micrometer is not enough.

Typical values

Golden rule of metrology: measurement uncertainty at most 1/10 of the tolerance; today 1/5 is often accepted.

On the shop floor

A display with three decimals doesn't mean the measurement has them: trust the instrument error and how you measure, not the digits.

Rigid tapping

Drilling and threading

Calculator
ES
Roscado rígido
DE
Synchrongewindebohren
IT
Maschiatura rigida
PT
Roscagem rígida
FR
Taraudage rigide

Tapping in which the control synchronizes the spindle rotation with the Z feed. It needs no compensating tap holder and allows tapping faster and more accurately.

Example

M10 × 1.5 at 500 rpm in G94: F = 500 × 1.5 = 750 mm/min. In G95, F1.5 is enough.

On the shop floor

On Fanuc, rigid mode is activated with M29 S… before G84 when parameter 5200#0 is zero; the number of that M is set by parameters 5210 or 5212. Check your control's manual.

Rotary table

Machine

ES
Mesa giratoria o cuarto eje
DE
Rundtisch
IT
Tavola rotante
PT
Mesa rotativa
FR
Plateau rotatif

Rotary axis mounted on the mill table (or built in) to rotate the part. It lets you machine several faces in a single setup and mill around a cylinder.

Example

Groove around a Ø 60 mm cylinder: 1° of rotation travels π × 60 / 360 ≈ 0.524 mm. A G01 A90 F300 rotates at 300 °/min, which at the surface is about 157 mm/min, not 300.

Typical values

To position (index) and then cut with the axis braked; or continuously, rotating while X, Y and Z move, with feed in degrees or inverse time (G93).

On the shop floor

If you machine with the axis stationary, brake it (manufacturer's M-code): without the brake, the cutting force makes it yield. And take the origin from the center of rotation, not from the edge of the chuck.

Roughness Ra

Tolerances and surface finish

Ra · µm
ES
Rugosidad Ra
DE
Mittenrauwert Ra
IT
Rugosità Ra
PT
Rugosidade Ra
FR
Rugosité Ra

Average of the unsigned heights of the surface profile relative to its mean line. It is the most used finish parameter on drawings and is measured by the surface roughness tester.

Example

Sandvik theoretical Ra in turning with f = 0.25 mm/rev: insert with rε = 0.8 mm, 2.25 µm; rε = 1.2 mm, 1.5 µm; wiper with rε = 0.8 mm, 0.45 µm.

Typical values

Roughness classes: N6 = 0.8 µm, N7 = 1.6 µm, N8 = 3.2 µm and N9 = 6.3 µm Ra. Each class doubles the previous one.

On the shop floor

The calculated values are theoretical: on the part it comes out somewhat worse. To improve it, lower the feed, raise the nose radius or use a wiper insert: at the same feed, half the roughness.

Roughness Rz

Tolerances and surface finish

Calculator
Rz · µm
ES
Rugosidad Rz
DE
Gemittelte Rautiefe Rz
IT
Rugosità Rz
PT
Rugosidade Rz
FR
Rugosité Rz

Height between the highest peak and the lowest valley of the profile, normally averaged over five sampling lengths. It captures isolated scratches and peaks better than Ra.

Example

With f = 0.15 mm/rev and rε = 0.8 mm: Rz ≈ 0.15² / (8 × 0.8) × 1000 ≈ 3.5 µm. With f = 0.2 mm/rev it rises to 6.25 µm: feed counts squared.

Typical values

There is no exact conversion to Ra. In Ceratizit's class table, Rz runs from about 5 to 8 times Ra: N7 is Ra 1.6 µm and Rz 10 µm.

On the shop floor

If the drawing asks for Rz, set the roughness tester to Rz instead of converting from Ra. On sealing surfaces Rz1max is used, the largest of the five individual Rz values.

Roundness

Tolerances and surface finish

ES
Redondez
DE
Rundheit
IT
Rotondità
PT
Circularidade
FR
Circularité

Form tolerance that requires every cross section of a round feature to lie between two concentric circles separated radially by the stated value. It has no datum.

Example

Oval shaft with max Ø 20.012 and min Ø 19.992 mm: with the micrometer, roundness is estimated as (20.012 − 19.992) / 2 = 0.01 mm. With tolerance 0.01 it is at the limit.

On the shop floor

The micrometer does not see a 3- or 5-lobe shape: each lobe has a flat zone opposite it and the diameter measures the same. Use a V-block or a roundness machine. The 3-jaw chuck causes it.

Runout

Tools

mm
ES
Excentricidad
DE
Rundlauffehler
IT
Eccentricità
PT
Excentricidade
FR
Faux-rond

How far the cutting edge or the shank of a tool deviates from the rotation axis as it turns. It makes some teeth cut more than others: worse finish, oversize and shorter tool life.

Example

2-flute end mill with fz 0.05 mm and 0.02 mm of runout on the dial: one tooth cuts up to 0.05 + 0.02 = 0.07 mm and the other only 0.03 mm. The first works 40 % harder.

Typical values

Maximum runout of REGO-FIX collets: standard ER 0.01-0.025 mm depending on diameter and length; ER-UP 0.005 mm. Haimer gives less than 0.003 mm on some of its shrink-fit chucks.

On the shop floor

Measure with a dial indicator near the edge, turning by hand. If holes come out off size, Sandvik says to check the radial runout before touching parameters.

Runout

Tolerances and surface finish

Drawing
ES
Salto radial y axial
DE
Lauf (Rundlauf und Planlauf)
IT
Oscillazione radiale e assiale
PT
Batimento radial e axial
FR
Battement radial et axial

Maximum variation shown by the dial indicator when the part is turned one revolution about its datum axis. Radial is measured on a diameter and includes roundness and eccentricity; axial, on a face.

Example

Part between centers, indicator on Ø 40: when turned it reads from −0.004 to +0.008 mm, radial runout 0.012 mm. If it were only eccentricity, the axis would be offset 0.006 mm, half.

Typical values

Circular runout is checked section by section; total runout, moving the indicator along the whole surface while it turns, and it also captures taper and straightness.

On the shop floor

Rotate the part on its datum (between centers or in V-blocks), not in the chuck: in the chuck you also measure the machine.

S

Scallop height

Milling

DrawingCalculator
h · mm
ES
Altura de cresta
DE
Kammhöhe
IT
Altezza della cresta
PT
Altura da crista
FR
Hauteur de crête

Height of the material left uncut between two passes of a ball-nose or bull-nose end mill. It defines the theoretical finish of 3D surfaces and how much polishing will be needed.

Example

Ø 10 mm ball (R = 5 mm) with a 0.5 mm stepover: h = 5 − √(25 − 0.0625) ≈ 0.0063 mm, about 6 µm.

On the shop floor

The formula holds on flat surfaces; on sloped walls the real stepover changes. That is why CAM systems offer constant-scallop strategies instead of a fixed stepover.

Shrink-fit chuck

Tools

ES
Mandril térmico
DE
Schrumpffutter
IT
Mandrino a calettamento termico
PT
Mandril de aperto térmico
FR
Mandrin de frettage

Tool holder whose bore expands when heated in a shrink-fit machine; the shank is inserted and, as it cools, it is clamped with very little runout.

Typical values

Cylindrical shanks of h6 tolerance, carbide or high-speed steel (Haimer). Haimer gives a runout below 0.003 mm on some of its models.

On the shop floor

A standard chuck works with any shrink-fit machine on the market: Haimer makes them in hot-work steel hardened to 54 ± 2 HRC.

Side and face cutter

Milling

ES
Fresa de disco
DE
Scheibenfräser
IT
Fresa a disco
PT
Fresa de disco
FR
Fraise trois tailles

Disc-shaped cutter, with teeth on the periphery and often on the faces, mounted on an arbor or on a shank. Used for narrow, deep slots, T-slots, keyseats and cut-offs.

Example

Disc Ø 100 mm, 10 teeth, vc = 120 m/min: n ≈ 382 rpm. With fz = 0.1 mm, vf ≈ 0.1 × 10 × 382 ≈ 382 mm/min.

On the shop floor

The maximum depth is limited by the shaft hub diameter, the strength of the driving keys and the room for the chip. In deep slots lower fz and, if the chip jams, try conventional milling.

Slenderness ratio

Turning

Calculator
L/D
ES
Esbeltez de la pieza
DE
Schlankheitsgrad
IT
Snellezza
PT
Esbelteza
FR
Élancement

Ratio between the free length of the part and its diameter. It indicates how much it will deflect and vibrate when cutting, and decides whether the chuck is enough or a tailstock or steady rest is needed.

Example

Shaft Ø 20 mm with 120 mm sticking out of the chuck: λ = 120 / 20 = 6. That is triple the 2:1 that Sandvik considers acceptable without support, so a tailstock is advisable.

Typical values

Sandvik: up to ≈ 2:1 with the part held at one end only is normally acceptable; with a tailstock, the ratio can be longer.

On the shop floor

On slender parts use κr close to 90°, a sharp edge and a small nose radius, and a depth of cut larger than that radius: this lowers the radial force that makes it vibrate.

Slot milling

Milling

ES
Ranurado con fresa
DE
Nutfräsen
IT
Fresatura di cave
PT
Fresagem de ranhuras
FR
Rainurage

Milling a slot with the cutter working at its full diameter (ae = D). It is the most demanding case: it engages 180°, the chip has trouble escaping and the cutter works in climb and conventional milling at the same time.

Typical values

Sandvik: axial depth around 70 % of the cutting edge length; in trochoidal slotting, cutter at most 70 % of the slot width.

On the shop floor

For a keyway with a width tolerance, use a cutter smaller than the slot and do it in two passes. Clear the chip from the slot with air so it doesn't jam.

Soft jaws

Turning

ES
Garras blandas
DE
Weiche Aufsatzbacken
IT
Griffe tenere
PT
Castanhas macias
FR
Mors doux

Jaws of unhardened steel or aluminum that are turned in the machine itself to the size of the part. They grip with more surface, center better and do not mark finished faces.

Typical values

According to Kitagawa: turn them to the part diameter, clamping a disc near the middle of the jaw stroke and with a pressure equal to or slightly higher than the working pressure.

On the shop floor

Use a thick disc that does not deform when clamped; if it deforms, lower the pressure or change the disc. Then take a test pass to check accuracy and that the part does not slip.

Specific cutting force

Cutting parameters

Calculator
kc · N/mm²
ES
Fuerza específica de corte
DE
Spezifische Schnittkraft
IT
Forza di taglio specifica
PT
Força de corte específica
FR
Force de coupe spécifique

Force needed to cut a chip cross-section of 1 mm². It depends on the material and the chip thickness, and is the base data for calculating force, power and torque.

Example

Steel with 0.55 % C or more, annealed (ISCAR: kc1 = 1700 N/mm², mc = 0.24), cutting with h = 0.2 mm: kc = 1700 × 0.2^(−0.24) ≈ 2500 N/mm².

Typical values

kc1 according to ISCAR: unalloyed steel 1350-1900 N/mm², austenitic stainless 2150, gray cast iron 1150-1350, aluminum 700-800, titanium 1700-2110.

On the shop floor

With thinner chips kc rises: cutting at very low feeds is not as cheap in power as it seems. The table kc1 is valid for 0° rake angle; a positive one lowers it.

Spindle

Machine

Calculator
ES
Husillo
DE
Arbeitsspindel
IT
Mandrino
PT
Árvore
FR
Broche

Rotating axis of the machine that turns the part (lathe) or the tool (milling machine and machining center). Its power, torque and maximum speed determine which cuts can be made.

Example

15 kW spindle at 1000 rpm: M = 15 × 30000 / (π × 1000) ≈ 143 N·m. At 8000 rpm, with the same power, only ≈ 18 N·m: that is why large cutters call for low rpm and high-torque spindles.

Typical values

DN Solutions DNM vertical centers: taper 40 and 8000 rpm as standard, with a 12000 or 15000 rpm option. A DMG MORI CLX 450 universal lathe: 4000 rpm on the main spindle.

Spindle speed

Cutting parameters

Calculator
n · rpm
ES
Velocidad de giro
DE
Spindeldrehzahl
IT
Velocità del mandrino
PT
Velocidade do fuso
FR
Vitesse de broche

Revolutions per minute the spindle makes: the part on the lathe or the tool on the milling machine. It is programmed with the letter S and comes from the cutting speed and the diameter.

Example

Ø 12 mm end mill in steel at vc = 120 m/min: n = 120 × 1000 / (π × 12) ≈ 3183 rpm. Program S3180 or S3200.

On the shop floor

On small cutters the calculated rpm often exceeds the spindle maximum. If you fall short on rpm, lower the feed in the same proportion so as not to load each tooth more.

Spot drilling

Drilling and threading

ES
Punto de centro
DE
Anbohren
IT
Centratura
PT
Centragem
FR
Pointage

Small cone made before drilling so the drill enters centered and doesn't wander. On a lathe it is also the conical hole where the tailstock center rests.

Example

90° spot drill leaving a 0.5 mm chamfer on a Ø 8 hole: the cone must measure 9 mm at the surface, so the depth is 9 / 2 = 4.5 mm.

Typical values

60° DIN 333 center drills for DIN 332 center holes for the tailstock. For 135-140° carbide drills, Hartner proposes 142° spotting drills.

On the shop floor

Spot with a slightly larger angle than the drill so its tip enters first. If the pre-cone has a smaller angle, Sandvik warns that the drill runs unstable and damages the corners.

Steady rest

Turning

ES
Luneta
DE
Lünette
IT
Lunetta
PT
Luneta
FR
Lunette

Support with three contact points (pads or rollers) that embraces the part between the chuck and the tailstock. The fixed one sits on the bed; the traveling one follows the carriage next to the tool.

Typical values

Röhm self-centering steady rests, designed to support slender parts, cover for example Ø 8 to 350 mm (SLZN) or Ø 40 to 800 mm (SLZ, for heavy parts).

On the shop floor

Bring the supports in until they touch the part without forcing it, so it turns freely, and grease the tips of the pads during the job.

Step drill

Drilling and threading

ES
Broca escalonada
DE
Stufenbohrer
IT
Punta a gradino
PT
Broca escalonada
FR
Foret étagé

Drill with two or more diameters on the same tool. It makes the hole and its step or chamfer in a single pass, for example the clearance for a screw and the seat for its head.

Example

Stepped 6.6 / 11 mm. If you set vc 80 m/min on the larger diameter: n = 80 × 1000 / (π × 11) ≈ 2315 rpm. On the 6.6 mm step the actual vc drops to about 48 m/min.

Typical values

DIN 912 / ISO 4762 M6 screw (10 mm head): clearance hole of 6.6 mm and counterbore of 11 mm. Conical multi-step drills are for sheet metal up to about 4 mm.

On the shop floor

On thick parts don't use the sheet-metal conical drill: choose a two-diameter stepped drill or drill and then counterbore with a pilot counterbore (DIN 373, 11 × 6.6 mm for M6).

Stepover

Milling

Calculator
ae · mm
ES
Paso lateral
DE
Seitliche Zustellung
IT
Passo laterale
PT
Passo lateral
FR
Pas latéral

Lateral distance between two consecutive cutter passes. In roughing it sets the edge load; in finishing with a ball-nose end mill it sets the height of the scallops left between passes.

Example

Ø 10 mm ball-nose (R = 5 mm) and a maximum scallop of 0.01 mm: ae = 2 × √(0.01 × 9.99) ≈ 0.63 mm between passes.

Typical values

Sandvik: below ae = 50 % of the diameter the chip thins (fz × 1.66 with ae of 10 %); in trochoidal, ae ≤ 20 %. With ball nose, the scallop sets it.

On the shop floor

Halving the stepover divides the scallop by about four, but doubles the time. Look for the scallop the drawing asks for, not the smallest possible.

Stock allowance

Milling

ES
Sobremetal
DE
Aufmaß
IT
Sovrametallo
PT
Sobreespessura
FR
Surépaisseur

Material left on purpose after an operation to be removed in the next: from roughing to finishing or from turning to grinding. In CAM and in cycles it is specified separately on walls and floors.

Example

Lathe G71 with U0.4 W0.1: U is the stock in X, on diameter (0.2 mm per side), and W the stock in Z (0.1 mm on the faces). Then G70 finishes the same profile and removes it.

On the shop floor

Leave constant stock for finishing: a finish that sometimes cuts 0.05 mm and other times 0.6 mm changes force and the size wanders.

Straightness

Tolerances and surface finish

ES
Rectitud
DE
Geradheit
IT
Rettilineità
PT
Retitude
FR
Rectitude

Form tolerance of a line: a line element must lie between two parallel straight lines separated by the stated value. If the dimension carries Ø, it applies to the axis, which must fit inside a cylinder of that diameter.

Example

You run the indicator along a 200 mm line element on a reference straightedge and, with the tilt removed, it reads from −0.006 to +0.008 mm: straightness 0.008 + 0.006 = 0.014 mm. With 0.02, it passes.

On the shop floor

If the frame says 0.02/100, straightness is required over any 100 mm section of the generatrix, not over the whole length. With no length stated, it applies to the whole part.

Sub-spindle

Turning

ES
Contrahusillo
DE
Gegenspindel
IT
Contromandrino
PT
Contrafuso
FR
Contre-broche

Second spindle facing the main one that picks up the part and lets you machine its back side. The part comes out finished in a single cycle, without flipping it by hand.

Typical values

Siemens sequence: bring the counter-spindle to the pick-up position, synchronize the spindles, part off, cancel synchronization and move it to its working position. Behind, it is programmed the same, with Z inverted.

On the shop floor

To pick up the part, synchronize both spindles before closing the chuck and part off with the part held on both sides. If the pick-up is with the spindle turning, confirm with the manufacturer that it is safe.

Subprogram

CNC programming

ES
Subprograma
DE
Unterprogramm
IT
Sottoprogramma
PT
Subprograma
FR
Sous-programme

Separate program with a repeating sequence, such as a contour or a hole pattern, which the main program calls as many times as needed. It saves lines and avoids copy errors.

Example

M98 P30100 runs O0100 3 times, which ends with M99: the last four digits are the program and the leading ones, the repetitions. On Siemens it is called by name (CONTOUR1); on Heidenhain, with CALL LBL or CALL PGM.

On the shop floor

To repeat across several parts, move inside the subprogram in incremental (G91) and return to G90 before M99. Otherwise the main program stays in G91 and the machine goes where it shouldn't.

Superalloys

Materials

ES
Superaleaciones
DE
Superlegierungen
IT
Superleghe
PT
Superligas
FR
Superalliages

Nickel, cobalt or iron alloys that keep their strength at very high temperature, such as Inconel 718. ISO group S: among the hardest to machine.

Typical values

With dedicated carbide, indicative: 40-80 m/min in turning; with ceramic, 150-400 m/min. Inconel 718: machinability rating of 18 %.

On the shop floor

Use a lead angle smaller than 45°, sharp edges and more than 0.25 mm depth in ramps or several passes, so you don't cut in the work-hardened layer. Always coolant.

Surface plate

Measurement

ES
Mármol de medición
DE
Messplatte
IT
Piano di riscontro
PT
Mesa de desempeno
FR
Marbre

Very flat plate of granite or cast iron that serves as a reference plane for measuring. The part, the height gauge and the dial indicators rest on it to measure heights, parallelism or flatness.

Typical values

DIN 876: grade 00 laboratory, 0 inspection, 1 toolroom and 2-3 shop. Local flatness over 250 × 250 mm: 3 µm (00), 3.5 (0), 7 (1) and 15 (2).

On the shop floor

Clean it before each measurement, together with the base of the instrument: dust and burrs cause error. Granite does not rust and, if hit, it may chip but it does not raise a burr.

Surface roughness tester

Measurement

ES
Rugosímetro
DE
Rauheitsmessgerät
IT
Rugosimetro
PT
Rugosímetro
FR
Rugosimètre

Instrument that drags a diamond tip across the surface, records the profile and calculates roughness parameters, such as Ra and Rz, with the filters the standard specifies.

Example

For a turned surface of Ra 1.6 µm, a cutoff λc of 0.8 mm and an evaluation length of 5 × 0.8 = 4 mm are used.

Typical values

ISO 4288 (now ISO 21920-3): λc = 0.8 mm for Ra from 0.1 to 2 µm, and 2.5 mm for Ra from 2 to 10 µm. Stylus tip of 2 or 5 µm radius.

On the shop floor

Choose λc according to the Ra you expect and check the result: if the measured Ra falls in another band of the table, repeat the measurement with the λc that applies.

Surface texture symbol

Tolerances and surface finish

ES
Símbolo de acabado superficial
DE
Oberflächensymbol
IT
Simbolo di finitura superficiale
PT
Símbolo de acabamento superficial
FR
Symbole d'état de surface

V-shaped symbol with a longer stroke that indicates on the drawing the finish of a surface, according to ISO 1302. It carries the parameter, such as Ra 1.6, and can indicate the process, the direction of the lay and the stock allowance.

Example

V closed into a triangle with 'Ra 1.6': material must be removed and not exceed 1.6 µm. V with a circle inside: removing material is prohibited. Open V: any process is acceptable.

On the shop floor

Without «max» the 16 % rule applies: 16 % of the measurements may exceed it. With «Ra max 1.6» none may exceed it. If the first measurement is below 70 % of the limit, it already complies.

Swiss-type lathe

Turning

ES
Torno de cabezal móvil
DE
Langdrehautomat
IT
Tornio a fantina mobile
PT
Torno de cabeçote móvel
FR
Tour à poupée mobile

Lathe in which the headstock moves the bar in Z through a guide bushing, and the tool always cuts right next to that support. It allows long, slender parts with high precision.

Typical values

Small-bar machines: at Star, for example, the SB-16R machines up to Ø 16 mm, the SB-20R up to Ø 20 mm and the SR-38 up to Ø 38 mm, with 320 mm of headstock stroke.

On the shop floor

Before choosing a machine, look at the maximum diameter, the headstock stroke and how many live tools there are at the front and on the back unit: on the SR-38 there are up to 8 behind.

Symmetry

Tolerances and surface finish

ES
Simetría
DE
Symmetrie
IT
Simmetria
PT
Simetria
FR
Symétrie

Position tolerance that requires the median plane of a slot or a tab to lie between two parallel planes, separated by the stated value and centered on the datum plane or axis.

Example

Keyway with symmetry 0.04 relative to axis A: its median plane must lie between two planes 0.04 mm apart and centered on the axis, that is, offset ±0.02 mm at most. If it is offset 0.015 mm, it passes.

On the shop floor

ASME Y14.5-2018 eliminated this symbol; in ISO 1101 it is still in force, so you will see it on ISO drawings and on older ASME drawings.

T

Table feed

Cutting parameters

Calculator
vf · mm/min
ES
Velocidad de avance
DE
Tischvorschub
IT
Avanzamento tavola
PT
Avanço da mesa
FR
Avance de table

Distance the tool travels relative to the part in one minute. It is the F value programmed in milling (G94) and the one used to calculate times.

Example

5-flute end mill, fz = 0.1 mm and 2000 rpm: vf = 0.1 × 5 × 2000 = 1000 mm/min. On a lathe it would be vf = f × n.

On the shop floor

If you change the rpm with the spindle override and not the feed override, you change the load per tooth without realizing. Recalculate vf whenever you touch n.

Tailstock

Turning

ES
Contrapunto
DE
Reitstock
IT
Contropunta
PT
Contraponto
FR
Contre-pointe

Assembly at the end opposite the chuck that supports the part by a center hole with a point, usually a rotating one. It prevents long parts from deflecting or coming loose.

Typical values

Sandvik: with the part held at one end only, up to L/D ≈ 2:1 is usually acceptable; with a tailstock it can be longer. 60° center holes (DIN 332-1, types R, A, B and C).

On the shop floor

On Haas lathes, M21 advances the tailstock to its support point and M22 retracts it; the positions are set in the machine parameters.

Tap

Drilling and threading

Calculator
ES
Macho de roscar
DE
Gewindebohrer
IT
Maschio
PT
Macho de roscar
FR
Taraud

Tool that cuts or forms an internal thread in an already drilled hole. It advances exactly one pitch per turn, so the feed is not chosen: the thread imposes it.

Example

M8 × 1.25 at 600 rpm: vf = 600 × 1.25 = 750 mm/min. In feed per revolution (G95), program F1.25.

Typical values

According to Sandvik, the long chamfer is typical of the spiral-point tap and the medium one, standard for blind holes, of the spiral-flute tap. The forming tap makes no chips.

On the shop floor

If there is little room at the bottom of a blind hole, Sandvik recommends a short-chamfer tap (form E): thread almost to the end of the point.

Tap drill size

Drilling and threading

Calculator
ES
Agujero previo de rosca
DE
Kernlochdurchmesser
IT
Preforo per filettatura
PT
Furo para roscar
FR
Avant-trou de taraudage

Hole drilled before tapping. Its diameter sets how much thread is formed: if it is too small the tap breaks; if too large the thread is loose.

Example

M10 × 1.5: Dp ≈ 10 − 1.5 = 8.5 mm. M8 × 1.25: 8 − 1.25 = 6.75, and a 6.8 mm drill is used.

Typical values

Valid for metric cutting taps (OSG table according to DIN 13 and ISO 965-1). Forming taps need more: D − P / 2 according to Sandvik (M10 × 1.5 → 9.25 mm).

On the shop floor

The forming tap needs a ductile material: Sandvik gives 1200 N/mm² tensile strength as the recommended limit. Never use the cutting-tap drill for a forming tap.

Taper

Turning

DrawingCalculator
C
ES
Conicidad
DE
Kegelverjüngung
IT
Conicità
PT
Conicidade
FR
Conicité

Ratio between the diameter difference of a cone and its length. It is expressed as 1:x or as an angle, and defines tool tapers, shafts and seats.

Example

D = 30 mm, d = 20 mm and L = 50 mm: C = 10 / 50 = 1:5. The half-angle is α/2 = atan(10 / 100) ≈ 5.71°.

Typical values

According to ISO 1119, Morse tapers range from 1:19.002 (no. 5) to 1:20.047 (no. 1) and 7:24 (16.59°) is the one for machine spindles and SK shanks (ISO 7388-1).

On the shop floor

On CNC, program the two points of the taper with cutter radius compensation active. Otherwise the nose radius leaves the taper at a different angle and diameter.

Tapered thread

Drilling and threading

Calculator
ES
Rosca cónica
DE
Kegeliges Gewinde
IT
Filettatura conica
PT
Rosca cónica
FR
Filetage conique

Thread cut on a taper, so that it tightens and seals as it is screwed in further. The most common are NPT (American, 60°) and BSPT or R/Rc (ISO 7-1, 55°), both with a 1:16 taper on the diameter.

Example

1/2" NPT (14 threads, P = 25.4 / 14 ≈ 1.814 mm) over 20 mm of length: the diameter changes 20 / 16 = 1.25 mm: 0.625 mm on radius, the taper that is programmed in the cycle (I in Haas G92).

Typical values

NPT (ASME B1.20.1) uses sealant. In ISO 7-1, R is the tapered external, Rc the tapered internal and Rp the parallel internal; G (ISO 228-1) is parallel and does not seal on the thread.

On the shop floor

Don't mix NPT and BSPT: in 1/2" both have 14 threads and 1:16 taper, but one is 60° and the other 55°, and they are not interchangeable. Check with the standard's gauges, not by measuring the diameter.

Tempering

Materials

ES
Revenido
DE
Anlassen
IT
Rinvenimento
PT
Revenido
FR
Revenu

Heating to a lower temperature done after hardening to remove brittleness and stresses. The higher the tempering temperature, the less hardness and the more toughness.

Typical values

Low, from 180 °C on an oil-hardening tool steel: it keeps almost all the hardness (about 62 HRC). High, 540-680 °C on 42CrMo4: quenched and tempered, tougher and machinable.

On the shop floor

Temper as soon as the part drops to 50-70 °C after quenching, twice and at least 2 h each time on that tool steel. The final hardness is set by the tempering temperature.

Thermal cracks

Tools

ES
Fisuras térmicas
DE
Kammrisse
IT
Cricche termiche
PT
Fissuras térmicas
FR
Fissures thermiques

Small cracks perpendicular to the cutting edge, like the teeth of a comb, caused by heating and cooling the edge over and over. When they join up, they pull pieces off the edge.

Typical values

Typical in milling and interrupted cuts, where each tooth heats up while cutting and cools in the air. Coolant makes them worse, especially if it arrives intermittently.

On the shop floor

Cut dry or with plentiful, constant coolant, so the temperature does not fluctuate. Use a thermal-shock-resistant grade with a thin PVD coating, and lower vc a little.

Thermal drift

Machine

ES
Deriva térmica
DE
Thermische Drift
IT
Deriva termica
PT
Deriva térmica
FR
Dérive thermique

Change in the dimensions the machine produces while the spindle, ball screws and structure warm up. The same dimension comes out different cold than with the machine hot.

Example

A steel ball screw (α ≈ 10 µm/(m·°C)) with 500 mm of travel that heats up 4 °C grows 10 × 0.5 × 4 = 20 µm. Without a linear scale, that difference shows up on the part.

Typical values

Heidenhain cites ball screw heat as a source of position error, and the increasingly hot working space in enclosed, fast machines. Linear scales correct it.

On the shop floor

Without scales, the dimension changes while the ball screw warms up: measure and adjust with the machine already at working temperature, not with the first cold part.

Thermal expansion

Tolerances and surface finish

Calculator
ΔL · mm
ES
Dilatación térmica
DE
Wärmeausdehnung
IT
Dilatazione termica
PT
Dilatação térmica
FR
Dilatation thermique

Change in a part's size when its temperature changes. Drawing dimensions are valid at 20 °C, so a hot, freshly machined part measures oversize.

Example

200 mm shaft with α = 11.5 × 10⁻⁶/°C measured at 30 °C: ΔL = 11.5 × 10⁻⁶ × 200 × 10 = 0.023 mm. With double α, it would be 0.046 mm.

On the shop floor

Let the part cool or measure part and standard at the same temperature. For hundredth-of-a-millimeter tolerances, even the hand on the micrometer heats it.

Thread depth

Drilling and threading

Calculator
h3 · mm
ES
Profundidad de rosca
DE
Gewindetiefe
IT
Profondità del filetto
PT
Profundidade de rosca
FR
Profondeur de filet

Height of the thread form, from crest to root, measured on the radius. On a lathe it is the total depth to be given in the threading passes.

Example

M10 × 1.5 external: h3 = 0.6134 × 1.5 ≈ 0.92 mm on radius. Internal: H1 = 0.5413 × 1.5 ≈ 0.81 mm, counted from the nut's minor diameter D1.

Typical values

Sandvik gives as an example a thread of 1.5 mm pitch with 0.94 mm profile depth made in 6 passes, with infeeds from 0.23 to 0.10 mm.

On the shop floor

The actual depth depends on the insert: the Sandvik example uses 0.94 mm, not the theoretical 0.92 mm. Fine-tune the size with small final passes and test with the gauge or the nut.

Thread gauge

Measurement

ES
Galga de roscas
DE
Gewindelehre
IT
Calibro per filettature
PT
Calibre de roscas
FR
Calibre de filetage

Name given to the thread pitch gauge, which tells the pitch by comparing teeth, and to the go / no-go thread plug and ring gauges, which check whether the thread is within tolerance.

Example

Internal thread M10 × 1.5 6H: the go plug must enter by threading in by hand, without forcing, and the no-go must not enter more than two turns (ISO 1502).

Typical values

Plugs in 6H tolerance for metric internal threads and 6g rings for external ones. On double-ended plugs, the no-go side is marked in red.

On the shop floor

With the comb, rest several teeth and look at it against the light: close pitches, such as 1.5 mm and 16 threads per inch (25.4 / 16 ≈ 1.59 mm), are confused over one or two teeth.

Thread insert

Drilling and threading

Calculator
ES
Inserto roscado
DE
Gewindeeinsatz
IT
Inserto filettato
PT
Inserto roscado
FR
Filet rapporté

Wire coil spring in the shape of a thread that goes into a larger threaded hole to repair a damaged thread or reinforce it in soft materials. The hole is tapped with a special STI tap.

Example

Repairing an M8 × 1.25: the HELICOIL M8 tap leaves a thread of at least 9.6 mm diameter (8 + 1.299 × 1.25 ≈ 9.62), on a hole of 8.4 mm. The screw is still M8 × 1.25.

Typical values

Usual insert lengths in kits: 1, 1.5 and 2 × D. Before tapping, the hole is countersunk at 90° to the STI thread diameter plus 0.1 mm.

On the shop floor

Use the drill the kit asks for (8.4 mm for M8), not the one for the next metric size: the STI tap is not a standard thread. If you don't remove the driving tang, the screw goes in less.

Thread milling

Drilling and threading

Calculator
ES
Fresado de roscas
DE
Gewindefräsen
IT
Fresatura di filetti
PT
Fresagem de roscas
FR
Fraisage de filets

Threading with a thread-profile cutter that follows a helix: one turn in XY while it descends one pitch in Z. The same cutter serves several diameters and right-hand or left-hand threads.

Example

Internal thread Ø 20 mm with a Ø 12 mm cutter and 300 mm/min at the cutting edge: at the cutter center you must program 300 × (20 − 12) / 20 = 120 mm/min.

Typical values

According to Sandvik, the cutter can always be pulled out of the part, the same tool makes several diameters of the same pitch and the thread reaches closer to the bottom of a blind hole.

On the shop floor

In internal threads the programmed feed applies to the center of the cutter: if you don't correct it, the edge moves faster than you think. In hard materials, Sandvik splits the thread into two or more passes.

Thread pitch

Drilling and threading

Calculator
P · mm
ES
Paso de rosca
DE
Gewindesteigung
IT
Passo della filettatura
PT
Passo de rosca
FR
Pas de filetage

Distance between two consecutive thread crests, measured parallel to the axis. On a single-start thread it is how far the screw advances in one turn; in inches it is given as threads per inch.

Example

1/4-20 UNC thread: P = 25.4 / 20 = 1.27 mm. On a two-start thread with a 1.5 mm pitch, the lead per revolution is 2 × 1.5 = 3 mm.

Typical values

Coarse metric (OSG table according to DIN 13): M6 1 mm, M8 1.25 mm, M10 1.5 mm, M12 1.75 mm, M16 2 mm, M20 2.5 mm. Fine metric uses smaller pitches.

On the shop floor

Check the pitch with a thread pitch gauge before doing a rework. An M10 × 1.25 and an M10 × 1.5 look very much alike to the eye and won't thread together.

Thread turning

Turning

Calculator
ES
Roscado en torno
DE
Gewindedrehen
IT
Filettatura al tornio
PT
Roscagem no torno
FR
Filetage au tour

Operation in which an insert with the thread profile makes several passes synchronized with the rotation, advancing one pitch per revolution. Used for external and internal threads of any pitch.

Example

M20 × 2.5: h ≈ 0.6134 × 2.5 ≈ 1.53 mm depth. At 800 rpm the carriage feeds 2.5 × 800 = 2000 mm/min, so it needs a run-up distance to accelerate.

Typical values

Sandvik: modified flank infeed (1-5°) as first choice, first pass the deepest and the last about 0.07 mm. It advises against spring passes with no infeed.

On the shop floor

Thread with fixed rpm (G97), as in the Haas G76 examples, and start a few millimeters before the part: the feed per revolution must equal the pitch.

Threading die

Drilling and threading

ES
Terraja
DE
Schneideisen
IT
Filiera
PT
Cossinete
FR
Filière

Ring-shaped tool with internal cutting edges that cuts an external thread on a round bar or tube. Used by hand with a die stock or on the lathe, and it is the opposite of the tap.

Example

M10 × 1.5: blank of about 9.85 mm (between 9.73 and 9.97 mm for class 6g) and chamfered tip down to about 8.3 mm so the die starts well.

Typical values

There are solid dies and dies split on one side (adjustable); the split ones allow you to adjust the cutting size a little.

On the shop floor

Turn the blank below the nominal size, as the manufacturer's table indicates, and start with a die holder or guide to enter aligned. If the thread is left-hand, the die is turned the other way.

Three-wire method

Measurement

Calculator
ES
Medición con tres alambres
DE
Dreidrahtmethode
IT
Metodo dei tre fili
PT
Método dos três arames
FR
Méthode des trois fils

Way of measuring the pitch diameter of an external thread: three calibrated wires are placed in the thread grooves, you measure over them with a micrometer and calculate d2.

Example

M10 × 1.5 with d2 = 9.026 mm: optimum wire d = 0.577 × 1.5 ≈ 0.866 mm. Over the wires you should read M = 9.026 + 3 × 0.866 − 0.866 × 1.5 ≈ 10.325 mm.

Typical values

Formula for metric and unified 60° threads. For Whitworth (55°), Mitutoyo gives d2 = M − 3.16568 × d + 0.960491 × P and optimum wire of 0.564 × P.

On the shop floor

The formula uses the actual wire diameter, so you can enter your own even if it is not the optimum one. Put two wires on one side and one on the other, and measure with the ratchet.

Through-spindle coolant

Machine

ES
Refrigeración interna
DE
Innenkühlung
IT
Refrigerazione interna
PT
Refrigeração interna
FR
Arrosage par le centre

Coolant that reaches the cutting zone through the spindle and the tool and exits through holes next to the cutting edge. It clears the chip from the bottom of the hole and cools right where the cutting happens.

Example

Carbide drill Ø 8 mm for a 40 mm hole: 40 / 8 = 5 × D. Above 3 × D, Sandvik Coromant recommends internal coolant so the chip does not jam.

Typical values

Options on a DN Solutions DNM vertical center: 20, 30 or 70 bar through the spindle. For titanium and superalloys, Sandvik Coromant indicates high pressure of up to 70 bar.

On the shop floor

If you only have external coolant, use it on shallow holes with good chip formation, and aim the nozzles close to the tool axis.

Titanium

Materials

ES
Titanio
DE
Titan
IT
Titanio
PT
Titânio
FR
Titane

Light and very strong metal, from ISO group S. It conducts heat poorly, so the cutting heat stays at the edge; with excessive speed it reacts with the tool, and it has low rigidity.

Typical values

With dedicated carbide, indicative: 40-80 m/min in turning. Ti6Al4V has a machinability rating of 21 % compared with free-machining steel.

On the shop floor

Use uncoated or PVD inserts, sharp edges and always coolant, plentiful and well aimed. On slender parts, be careful: titanium flexes and vibrates.

Tolerance stack-up

Tolerances and surface finish

Calculator
ES
Cadena de cotas
DE
Maßkette
IT
Catena di quote
PT
Cadeia de cotas
FR
Chaîne de cotes

Sum of consecutive dimensions that determines a final measurement, such as the length of an assembly or a clearance. Their tolerances stack up: in the worst case they add, and with a statistical approach, they add in quadrature.

Example

Three parts of 20 ±0.1, 30 ±0.05 and 15 ±0.05 mm: total 65 mm. Worst case ±(0.1 + 0.05 + 0.05) = ±0.2 mm. Statistical ±√(0.1² + 0.05² + 0.05²) ≈ ±0.12 mm.

On the shop floor

If on the CNC you program each dimension from the previous one, you accumulate errors. Take all dimensions from the same origin, which usually matches the datum on the drawing.

Tool holder taper

Tools

ES
Cono portaherramientas
DE
Werkzeugkegel
IT
Cono portautensili
PT
Cone porta-ferramentas
FR
Cône d'attachement

Part of the toolholder that goes into the spindle and centers it. The most common systems are the 7:24 taper (SK, BT, CAT) and HSK, hollow and short, which seats on both taper and face.

Typical values

7:24 taper for automatic tool change in sizes 40, 45 and 50 (ISO 7388-1; SK40 is one of them). HSK (ISO 12164-1): types A, AB and EB for automatic change; C and CB, manual only.

On the shop floor

Before ordering a tool holder, check the exact standard and form of your spindle: ISO 7388-1 has six shank forms (A, AD, AF, U, UD and UF).

Tool length offset

CNC programming

ES
Corrector de longitud
DE
Werkzeuglängenkorrektur
IT
Correzione lunghezza utensile
PT
Compensação do comprimento da ferramenta
FR
Correction de longueur d'outil

Value that stores the length of each tool so the control takes it into account in Z. This way the program gives the tip position, whatever tool is mounted.

Example

T3 M06 · G43 H3 Z50. With offset 3 at 125.400 mm, the tip ends at Z50 and the spindle nose at Z175.4. On Siemens it is activated with D1 and on Heidenhain, with TOOL CALL.

On the shop floor

The error that breaks tools: G43 without H, or with another tool's H (T5 with H3). After every change, check that the H number matches the T number.

Tool life

Cutting parameters

T · min
ES
Vida de la herramienta
DE
Standzeit
IT
Durata dell'utensile
PT
Vida útil da ferramenta
FR
Durée de vie de l'outil

Cutting time an edge withstands until it reaches the allowed wear. The Taylor equation relates that life to the cutting speed.

Example

With n = 0.25, lowering vc by 20 % multiplies tool life by (1 / 0.8)^(1 / 0.25) ≈ 2.4: from 15 to about 37 min.

Typical values

For uncoated carbide, Stephenson and Agapiou give n = 0.2-0.25 (cited by Karandikar et al., 2014). The value depends on the tool-material pair and the allowed wear: adjust it with your own tests.

On the shop floor

Change edges by part count, not when they break: Sandvik proposes setting the change 10-20 % below the number of parts that still give the required finish.

Tool overhang

Tools

DrawingCalculator
mm
ES
Vuelo de la herramienta
DE
Auskraglänge
IT
Sbalzo dell'utensile
PT
Balanço da ferramenta
FR
Porte-à-faux de l'outil

Length the tool or the bar sticks out from its clamping. The more overhang, the more it deflects and vibrates; that is why it is expressed as a multiple of the diameter (L/D).

Example

Going from 30 to 45 mm of overhang on a cutter: (45 / 30)³ ≈ 3.4. With the same force, the tip deflects about 3.4 times more.

Typical values

Maximum overhang of boring bars in turning according to Sandvik: steel 4 × D; carbide 6 × D; anti-vibration steel 10 × D; carbide-reinforced anti-vibration 14 × D.

On the shop floor

Deflection grows with the cube of the overhang: stick the tool out just enough to avoid collisions. With long overhangs, Sandvik raises the edge 0.1 mm above center to compensate for it dropping.

Tool presetter

Machine

ES
Preajustador de herramientas
DE
Werkzeugvoreinstellgerät
IT
Presetting utensili
PT
Pré-ajustador de ferramentas
FR
Banc de préréglage

Device outside the machine that measures the length and diameter of each tool already mounted in its holder. The values go to the offset table and the machine doesn't stop to measure.

Example

The presetter gives L 142.315 mm and Ø 15.992 mm. You enter 142.315 in the length (H) and 7.996 in the radius (D), or send them over the network. When it is mounted, G43 with its H and start machining.

Typical values

Haimer Microset UNO optical presetters: repeatability of ±5 µm on the entry model (smart); the higher ones, ±2 µm and 2 µm of runout in the device's spindle.

Tool radius compensation

CNC programming

ES
Compensación de radio
DE
Werkzeugradiuskorrektur
IT
Correzione raggio utensile
PT
Compensação do raio da ferramenta
FR
Correction de rayon d'outil

Function that offsets the toolpath by the cutter radius (or the nose radius on a lathe) to follow the drawing contour. Looking in the feed direction, G41 keeps the tool on the left, G42 on the right and G40 cancels.

Example

G00 X-20 Y-20 · G01 G41 X0 Y-10 D12 F300 · Y50 · … · G40 G01 X-20 Y-20. Activate and cancel on straight lead-in and lead-out moves longer than the cutter radius.

Typical values

In Heidenhain it is programmed as RL (left), RR (right) and R0 (no compensation). To fine-tune the size, touch the wear offset, not the program.

On the shop floor

Forgetting G40 at the end carries the compensation over to the next contour or tool. With G41 and clockwise spindle you climb mill: feed and edge rotation go in the same direction.

Torque

Cutting parameters

Calculator
Mc · N·m
ES
Par de corte
DE
Drehmoment
IT
Coppia
PT
Binário
FR
Couple

Turning effort that the cut asks of the spindle. At low rpm the motor's available torque is the limit, not the power: large diameters, big taps, large drills.

Example

6 kW of cutting power at 1273 rpm: Mc = 6 × 30000 / (π × 1273) ≈ 45 N·m. With the same 6 kW at 300 rpm, ≈ 191 N·m would be needed.

On the shop floor

With the same power, torque grows as rpm drops. On large diameters, taps or thick drills, compare the torque the cut requires with the spindle torque curve, not just with its power.

Touch probe

Machine

ES
Palpador
DE
Messtaster
IT
Tastatore
PT
Apalpador
FR
Palpeur

Sensor mounted in the spindle, or fixed on the table, that gives a signal when it touches the part or the tool. Used to set work offsets, measure parts on the machine and detect broken tools.

Example

Heidenhain: TCH PROBE 417 touches the top face of the part and saves the Z origin there, in the preset table. Then cycle 247 activates that origin from the program.

Typical values

Renishaw workpiece probes (OMP40-2, RMP60): repeatability of 1.00 µm (2σ). The radio ones are used when there is no line of sight between the probe and the receiver.

On the shop floor

Renishaw gives that repeatability probing at 480 mm/min with a 50 mm stylus: if you probe faster or with longer styli, don't expect the same figure.

Trapezoidal thread

Drilling and threading

Calculator
ES
Rosca trapecial
DE
Trapezgewinde
IT
Filettatura trapezoidale
PT
Rosca trapezoidal
FR
Filetage trapézoïdal

Metric thread with a trapezoidal profile and 30° flanks (ISO 2904, DIN 103), strong and with low friction. Used to transmit motion and force: vise screws, presses, jacks and sluice gates.

Example

Tr 20 × 4: h3 = 0.5 × 4 + 0.25 = 2.25 mm; minor diameter d3 = 20 − 2 × 2.25 = 15.5 mm; pitch diameter d2 = 20 − 0.5 × 4 = 18 mm.

Typical values

Clearance ac according to pitch: 0.15 mm (P 1.5), 0.25 mm (P 2-5), 0.5 mm (P 6-12) and 1 mm (P 14 or more). In the table, Tr 40 × 7 has d3 = 32 mm.

On the shop floor

The tool tip is flat, not pointed. Since the thread is deep, on a lathe it takes many small passes and enters along one flank so the insert does not cut with the whole profile at once.

Trochoidal milling

Milling

ES
Fresado trocoidal
DE
Trochoidalfräsen
IT
Fresatura trocoidale
PT
Fresagem trocoidal
FR
Fraisage trochoïdal

Strategy in which the cutter advances in chained circular loops, working with a small width of cut and a large depth. It keeps the load constant and allows slotting without engaging 180°.

Typical values

Sandvik: maximum ae of 20 % of D, ap up to 2 × D, stepover between loops under 10 % of D and cutter under 70 % of the slot width.

On the shop floor

With so small an ae the chip thins: raise the feed per tooth to recover the real thickness. Otherwise the edge rubs and wears out.

Turret

Machine

ES
Torreta
DE
Werkzeugrevolver
IT
Torretta
PT
Torreta
FR
Tourelle

Lathe disc or drum that carries several tools and rotates to bring the next one into working position. It can have fixed and live stations for drilling and milling.

Example

T0303 on Fanuc: station 3 with offset 3. T0313 uses the same tool with offset 13, useful for giving another size. In Siemens it is written T3 D1.

Typical values

The most widespread mounting is VDI, with a cylindrical shank: standard DIN 69880, replaced in 2023 by DIN ISO 10889-1. On Fanuc, the offset number can be any in the register.

On the shop floor

Before rotating the turret, retract to a safe position in X and Z: a long boring bar or a drill can hit the chuck or the part when indexing.

Twist drill

Drilling and threading

Calculator
ES
Broca helicoidal
DE
Spiralbohrer
IT
Punta elicoidale
PT
Broca helicoidal
FR
Foret hélicoïdal

Tool with two cutting edges at the tip and two helical flutes that evacuate the chip. It is the normal way to make holes on a machine, in high-speed steel or carbide.

Example

High-speed steel drill Ø 10 mm at vc 30 m/min: n = 30 × 1000 / (π × 10) ≈ 955 rpm. With f = 0.2 mm/rev, the feed rate comes out 955 × 0.2 ≈ 191 mm/min.

Typical values

Hartner table, HSS and HSS-E drills in structural steel: about 27-35 m/min. Feed grows with diameter: at Ø 10 mm, from 0.08 to 0.5 mm/rev depending on material and drill.

On the shop floor

If the hole comes out oversize, Sandvik says to check the drill's radial runout and the coolant flow before changing tools.

U

Undercut

Turning

ES
Garganta de salida
DE
Freistich
IT
Gola di scarico
PT
Ranhura de saída
FR
Gorge de dégagement

Small groove next to a shoulder that lets the threading tool or the grinding wheel run out. That way the thread or the ground diameter reaches the shoulder in full.

Example

DIN 76 thread undercut for M12 × 1.75: root Ø = 12 − 2.6 = 9.4 mm, 6.1 mm wide and 1 mm radius, according to the table used by Heidenhain cycles.

Typical values

DIN 76 for thread undercuts; DIN 509 for grinding: form E (cylinder only) and F (cylinder and face at 90°), in sizes such as E 0.6 × 0.3, E1 × 0.2 or E1 × 0.4.

On the shop floor

Take it from the standard's table for your pitch or diameter: if you make it shallower, the threading insert collides; if you make it deeper or without the table radius, you weaken the shaft.

V

Variable pitch end mill

Milling

ES
Fresa de paso variable
DE
Fräser mit ungleicher Teilung
IT
Fresa a passo variabile
PT
Fresa de passo variável
FR
Fraise à pas variable

Cutter with teeth spaced at unequal distances, and sometimes with different helixes. The impacts of each tooth do not repeat at the same rhythm, so vibration does not build up.

Typical values

Sandvik recommends it mainly with a wide width of cut and long overhangs; with long overhangs or low stability, on insert cutters, it advises coarse pitch and differential pitch.

On the shop floor

Calculate the feed with the number of teeth as on a normal cutter. Do not confuse this pitch with that of face mills (coarse, normal or fine), which is the number of teeth.

Vernier caliper

Measurement

ES
Calibre o pie de rey
DE
Messschieber
IT
Calibro a corsoio
PT
Paquímetro
FR
Pied à coulisse

Sliding instrument that measures outside with the large jaws, inside with the small ones and depths with the depth rod. It is the quick shop-floor measurement, not the precision one.

Typical values

Resolution of 0.05 or 0.02 mm with vernier and 0.01 mm on digital ones. A 150 mm digital caliper from the catalog allows an error of ±0.02 mm: it is fine for tolerances of a few tenths.

On the shop floor

Measure with the part as close as possible to the scale and without squeezing too hard: the caliper has no ratchet and the force tilts the slider. For dimensions with hundredth tolerances, use a micrometer.

Vernier scale

Measurement

Calculator
ES
Nonio
DE
Nonius
IT
Nonio
PT
Nónio
FR
Vernier

Auxiliary scale that slides alongside the main scale and lets you read fractions of its division. It is read by finding the vernier line that coincides exactly with a line on the rule.

Example

Vernier of 20 divisions on a 1 mm rule: 1 / 20 = 0.05 mm. If the vernier zero is past 23 mm and its 7th line coincides: 23 + 7 × 0.05 = 23.35 mm.

Typical values

Verniers with 10 divisions (0.1 mm), 20 (0.05 mm) and 50 (0.02 mm). The 0.02 mm ones have the lines so close together that they are hard to read.

On the shop floor

Look at the scale head-on, not from the side: parallax error makes you see the wrong line as the one that lines up.

W

Water-miscible coolant

Materials

Calculator
%
ES
Taladrina
DE
Wassermischbarer Kühlschmierstoff
IT
Emulsione lubrorefrigerante
PT
Óleo solúvel
FR
Huile soluble

Mixture of water with soluble or synthetic oil that cools, lubricates and carries away the chip. Its concentration is checked with a refractometer, because emulsion stability and lubrication depend on it.

Example

The refractometer reads 4.0 °Bx and the manufacturer gives a factor of 1.2: C = 4.0 × 1.2 = 4.8 %. If you want 6 %, add concentrate.

Typical values

The usual range is between 3 and 15 %, depending on the operation and material. The manufacturer's data sheet rules, and it also gives the refractometer factor.

On the shop floor

Always pour the concentrate into the water, stirring, not the other way around. Zero the refractometer with clean water before measuring.

Wedge angle

Tools

Calculator
β · °
ES
Ángulo de cuña
DE
Keilwinkel
IT
Angolo di taglio
PT
Ângulo de cunha
FR
Angle de taillant

Angle of the tool material between the rake face and the flank face. The larger it is, the stronger and more heat-resistant the edge; the smaller it is, the sharper and the smoother it cuts.

Example

Positive insert with 7° clearance and 15° rake: β = 90 − 7 − 15 = 68°. A negative insert mounted with α 6° and γ −6° works with β = 90°.

Typical values

Positive geometries (large γ, small β) cut more smoothly but have a weaker edge; negative ones, with larger β, have a stronger edge.

On the shop floor

Sharpening the edge more lowers the force, but it also removes material from the wedge: if the edge chips, move to a more robust geometry. Find the balance with the edge preparation.

Wiper insert

Turning

ES
Plaquita wiper
DE
Wiper-Wendeschneidplatte
IT
Inserto wiper
PT
Pastilha wiper
FR
Plaquette wiper

Insert with the tip formed by several radii that smooths the surface after the cut. It allows more feed with the same roughness; on face mills there is an equivalent wiper insert.

Example

Sandvik table, radius 0.8 mm: the normal insert gives Ra ≈ 1.25 µm at 0.2 mm/rev and ≈ 5.75 µm at 0.4 mm/rev. The wiper of the same radius, at 0.4 mm/rev, gives Ra ≈ 0.7 µm.

Typical values

Sandvik rule: double the feed with the same finish, or the same feed with twice as good a finish. It is designed mainly for straight-line turning and facing.

On the shop floor

It generates more cutting force and more radial deflection than a normal insert: it is not the first choice if there is vibration, and it only performs in very stable setups. On tapers and radii it loses the smoothing effect.

Work hardening

Materials

ES
Acritud
DE
Kaltverfestigung
IT
Incrudimento
PT
Encruamento
FR
Écrouissage

Hardening a metal undergoes when it is deformed cold. In machining it appears when the edge rubs or crushes instead of cutting, leaving a harder layer that the next pass has to cut.

Typical values

Very pronounced in austenitic stainless steels and superalloys: it leaves hard surfaces and chips that cause notch wear on the insert.

On the shop floor

Don't let the edge rub: use sharp edges and enough feed so the edge cuts below the layer work-hardened by the previous pass.

Working plane

CNC programming

ES
Plano de trabajo
DE
Arbeitsebene
IT
Piano di lavoro
PT
Plano de trabalho
FR
Plan de travail

Plane in which the control makes arcs, cutter compensation and cycles: XY (G17), XZ (G18) or YZ (G19). The axis left out is the tool axis.

Example

G17 G02 X20 Y0 I10 J0 makes the arc in XY; in XZ it would be G18 G02 X20 Z0 I10 K0. Siemens uses the same G17-G19; on Heidenhain it is set by the TOOL CALL axis: TOOL CALL 1 Z works in the XY plane.

Typical values

Siemens associates G17 (XY) with milling and G18 (XZ) with turning; G19 is the YZ plane. Fanuc requires choosing the plane before coordinate rotation (G68), not with the rotation active.

On the shop floor

The plane is modal: if a previous program left G18 or G19 active, arcs and compensation come out in another plane. Put G17 in the safety block at the start.

Workpiece zero

CNC programming

ES
Origen de pieza
DE
Werkstücknullpunkt
IT
Zero pezzo
PT
Zero da peça
FR
Origine pièce

Point on the part from which the program dimensions are measured. Its position relative to the machine zero is stored in a work offset table (G54 to G59) and the program activates it at the start.

Example

You touch off the corner of the part and the screen reads X-412.350 Y-205.100 in machine coordinates: you store those values in G54. With G90 G54 G00 X0 Y0 the tool goes to that corner.

Typical values

Fanuc 0i-F: G54-G59 and 48 additional origins. Siemens: G54-G57 and G505-G599. Heidenhain: preset table, activated with cycle 247. Fagor 8055: G54-G57, G58-G59 incremental and G159 N1-N20.

On the shop floor

The classic error: measuring the origin correctly and storing it in G55 while the program calls G54. Before the first start, check on the absolute position screen that the tool is where you expect.

Z

Z-level machining

Milling

Calculator
ES
Estrategia en Z constante
DE
Z-konstantes Schlichten
IT
Fresatura a Z costante
PT
Maquinagem em Z constante
FR
Usinage en Z constant

CAM strategy that runs over the part in horizontal levels, stepping down in Z between one and the next. It works very well on vertical and steep walls of molds, but poorly in nearly flat areas.

Example

With Δz = 0.2 mm: on an 80° wall the passes are ≈ 0.2 mm apart; on a 20° wall, ≈ 0.58 mm, almost three times as much, and the scallop grows a lot.

On the shop floor

Combine it with a constant-scallop or raster strategy in the shallow areas. Many CAMs separate them with a wall angle limit, like Fusion's Steep and Shallow.

Zero-point clamping system

Machine

ES
Sistema de punto cero
DE
Nullpunktspannsystem
IT
Sistema di bloccaggio a punto zero
PT
Sistema de fixação de ponto zero
FR
Système de bridage point zéro

Quick-clamping system with fixed modules on the table and pull studs screwed under the plate, the vise or the pallet. The fixture is changed in seconds and always returns to the same position, without re-centering.

Example

If each fixture change costs you 20 minutes of centering and setting the origin, and you change 5 times a day, that is 5 × 20 = 100 minutes. With a zero point system, the G54 of each fixture is saved once and is always valid.

Typical values

Repeatability of a few microns: LANG gives less than 0.005 mm on its Quick•Point and Schunk less than 0.002 mm on its SPG pins. There are purely mechanical modules and spring ones with pneumatic opening.

On the shop floor

Blow off module and pin before each clamping (many modules have built-in air blow): a chip underneath eats all the repeatability.