CNC Lathe Setup: Workholding, Tool Offsets and Part Zeroing

A CNC lathe program can be geometrically perfect; the cutting tool can be well chosen and the cutting speed and feed correctly calculated. Even so, if the workpiece is clamped wrong, the tool offsets are incorrect or the workpiece zero is not registered correctly, the machine cannot produce a correct part. More importantly, such a setup error does not only cause a dimensional problem; it can make the tool crash into the chuck, part, tailstock or another tool.

In CNC lathe production, three pieces of information work together: the program states which coordinates the tool goes to; the workpiece zero defines the start point of those coordinates on the part; and the tool offsets tell the CNC where each turret tool’s real cutting tip is. If one is wrong, the whole system works wrong. For example, G00 X42 Z2 in the program does not, by itself, guarantee the tool actually stops at Ø42 and 2 mm in front of the face: the part must be in the right position in the chuck, the face correctly registered as Z0, the tool’s X–Z geometry correctly measured, and the correct tool/offset called. In this lesson we cover safe workholding, chuck and tailstock use, establishing the workpiece zero, tool geometry/wear offsets, nose radius, first-part setup and running the program under control.

1. What Does Preparing the Machine (Setup) Mean?

Preparing the machine is not just loading the program. Before production, in general the following are done: studying the drawing, choosing the raw material, preparing the operation order, choosing the chuck/jaws, clamping the part, using a tailstock if needed, mounting the cutting tools in the turret and setting station numbers, sending the machine to reference, registering the workpiece zero, measuring each tool’s X–Z geometry offset, entering nose radius/direction, checking cutting values, simulating the program, running first in single block at low speed, measuring the first part, and correcting with wear offsets if needed. All of this is generally called setup. A good setup increases production safety, brings the first part closer to size, reduces tool breakage, shortens setup time and ensures parts are machined in the same position in series production.

2. Why Is Workholding Important?

A CNC lathe works at high speed and high cutting force; the part not only turns but also resists cutting forces. If clamping is insufficient, the part can slip in the chuck, be pushed in Z, run off center, vibrate or be thrown from the chuck. If clamping is too strong, thin-walled parts especially can be crushed, go oval and change shape when measured correctly while clamped and then removed. Correct clamping is not just “gripping as tight as possible”; it strikes this balance: the part must be clamped firmly enough not to move under cutting forces, but in a controlled way that does not distort its shape. Because CNC machines are powerful and high-removal, the workholding system is critical for both machining quality and safety.

3. Basic Workholding Systems

Different systems are used by part shape, production volume and precision: 3-jaw hydraulic chuck, 4-jaw chuck, collet system, soft/hard jaws, tailstock, steady rest, mandrel and special fixtures.

• 3-jaw chuck: the most common system. The three jaws approach/retreat from the center together; it clamps cylindrical, hexagonal and bar stock quickly. On CNC it mostly clamps hydraulically/pneumatically (by pedal or command). Advantages: fast clamping, automatic centering, repeatability. Limits: unsuitable for very irregular parts, can over-clamp a thin part, worn jaws can cause runout.
• Hard jaws: heat-treated, durable, standard jaws; for various raw diameters and roughing. They grip on a small surface; can mark a thin part, and their precision centering is lower than soft jaws. It must be checked that the part is not gripped by only a small corner.
• Soft jaws: jaws turned to the part diameter (usually low-carbon steel); they create a wide contact surface. Ideal for precise clamping, thin-walled parts, re-clamping on a machined surface and jobs needing low runout.
• Collet system: grips a cylindrical part over a wide, even circumferential surface; suitable for small diameters, bar stock, high speed and series production. Low runout, fast open/close. Limits: the diameter working range is narrow, each diameter may need a suitable collet; chips/dirt prevent proper closing.

Why Are Soft Jaws Turned?

Soft jaws are machined to form a seat matching the part diameter. For example to clamp a Ø50 part, the jaws are pre-loaded in the working clamping direction and turned to about Ø50. Thus the jaws contact the part over a wider surface, centering improves, clamping force distributes evenly, marking on the part decreases and re-clamping precision rises. Note: the jaws must be pre-loaded in the real working direction, machined to match the clamping diameter, with jaw faces at the same Z, and the seat must not be left tapered/stepped. Wrongly prepared soft jaws (e.g. loaded the wrong way) can seat differently under real clamping and cause runout.

4. Overhang, Gripping Length, Chuck Pressure and Runout

Overhang: the part sticking out in front of the chuck. Too much overhang causes vibration, bending, taper, a poor surface and the risk of being thrown; too little brings the tool near the chuck and a groove/parting tool can hit the jaws. In setting the right overhang, the finished length, facing allowance, parting-tool width, second-operation allowance and safety margin are considered together. For example if the finished length is 60 mm, facing allowance 2 mm, parting tool 3 mm and safety 5 mm, the minimum overhang can be 60 + 2 + 3 + 5 = 70 mm. But if the diameter is small, 70 mm can vibrate; then a tailstock, bar feeder or different operation order may be needed.

Gripping length: the part gripped inside the jaws. If insufficient, the part slips or wobbles under rotation/Z force. There is no single fixed value; it depends on diameter, length, material, cutting force, pass, chuck/jaw type, pressure and tailstock use. A part to be heavily roughed needs more gripping length than one to be lightly finished.

Chuck pressure: in a hydraulic chuck the clamping force relates to pressure and is balanced between two dangers: low pressure (part slips/is thrown) and excessive pressure (part crushed/distorted). Material, wall thickness, diameter, jaw contact area, speed, cutting force and internal/external clamping affect it. A thin-walled bushing must not be clamped with the pressure used for a solid shaft. Also, as speed rises the jaws’ centrifugal force increases; in external clamping the real grip drops at high speed, so the chuck maker’s speed–force charts are considered.

Runout: the surface running off-center as the part turns. Causes: a bent part, dirty/worn jaws, wrongly turned soft jaws, burrs, the part not seating fully. Checked with a dial indicator. Seating surface: in series production, to clamp parts at the same Z each time, an in-chuck stop, jaw step or special stop is used. If the part does not seat fully, the stock removed from the face changes, lengths differ and Z0 seems to shift each part. “The chuck closed” is not enough to check; it must also be confirmed that the part actually contacts the stop.

5. Tailstock Support and Special Fixtures

A long part held only by the chuck bends/vibrates under cutting force; the tailstock supports the free end, keeps the part on the lathe axis and enables safe cutting. General order: face the end → drill a center hole with a center drill → bring the live center into the hole → apply suitable pressure → check axis and clearance. If tailstock pressure is low, the part is unsupported and vibrates; if too high, a thin part bends and the center hole is damaged. A heated long part expands lengthwise; a fixed, very high pressure can bend it.

Using a tailstock also changes the tool motion envelope. The programmer must check: does the turret hit the tailstock body; does a long OD holder near the center; can the boring bar hit the tailstock during a tool change; does a long drill enter the tailstock area as the turret indexes; is the reference-return path safe. So it is not enough that the tool does not hit the part during cutting; the turret’s indexing envelope must be considered too. For irregular, thin or eccentric parts that cannot be held safely by a standard chuck/collet, special fixtures can be made; in design, centrifugal force, clamping direction, balancing, chip evacuation, tool access and operator safety are considered.

6. Reference Return and the Meaning of Workpiece Zero

After the part and tools are mounted, the CNC must recognize the axis positions correctly. Reference return verifies the machine coordinate system, registers the axes’ physical position and forms the basis of the tool/work coordinates. But going to reference does not automatically create the workpiece zero: reference return is the machine recognizing its own position; workpiece zeroing is binding the program coordinates to the part. On some systems the work coordinate is set automatically after reference; on others G50 or G54–G59 is used.

The workpiece zero is the point where all program dimensions start. In standard OD turning it is usually X0 = the part’s rotation center and Z0 = the finished face; so X40 Z-30 means Ø40 diameter and 30 mm inside from the face. If the workpiece zero is wrong, all program points move to the wrong place on the part: if Z0 is 2 mm off, all shoulders, grooves, thread starts and lengths shift 2 mm; if the X zero/diameter offset is off, all diameters come out large, small or off-center.

7. Establishing Z Zero and X Zero

Z zero (face): a suitable tool is called, approached slowly, a thin chip is taken off the face, and the tool is retracted only in X without moving in Z, then this surface is registered as Z0. If the tool moves in Z, the real zero surface is lost; if it retracts only in X, the Z position of the cut surface is preserved. Some shops use a paper-contact method, but it gives an approximate value, includes the paper thickness and is dangerous on a rotating part; the safest/most precise methods are taking a thin chip and measuring, a tool-measuring probe or the maker’s automatic measuring function.

X zero (OD tool): on a lathe X0 is physically the part center, but taking the tool straight to the center is not suitable. The common method is to machine a diameter and measure it to register the X geometry: approach the tool, take a light cut over a short length, retract the tool in Z without moving in X, measure the machined diameter with a micrometer, and enter the measured value (e.g. 39.86) into the tool’s X measurement. The control compares the current machine position with the real diameter and computes the geometry offset. For an ID tool the logic is the same but the error risk is higher (taper, chips, temperature, bar deflection). For the center-line drill/reamer/tap, X0 is the basis; the real center setting is machine-specific.

8. Tool Offset: Why Needed, Geometry and Wear

Each tool in the turret has a different physical length (OD holder short, grooving longer, boring bar much longer, drill tip at a different Z). If the programmer had to add each tool’s length to every coordinate separately, programming would be very complex. The tool offset system solves this: the programmer writes the part’s real geometry (X40 Z-30), and the control uses the called tool’s offset to compute where the axes must physically go. The offset balances the X and Z difference between the default standard tool and the real tool.

The tool offset is split in two. The geometry offset is the basic difference due to the tool’s mounting position and physical length (X, Z geometry, nose radius, tip direction); measured at first setup and largely constant unless the holder/mounting changes. The wear offset compensates the small size change as the tool cuts. For example if the target is Ø40.00 but Ø40.06 comes out, the program X40 is correct and the geometry is correct; the tip has not reached the target due to wear, so we correct the wear offset by a small value, not the geometry.

9. X and Z Wear Correction (Diameter–Radius)

The most confused topic in X correction is diameter vs. physical tool movement. Target Ø40.00, measured Ø40.06: the part is 0.06 mm large on diameter; the tool must physically move 0.03 mm closer to the center. In a common diameter-based system the diameter difference -0.06 is entered into the X wear offset; in a radius-based system the physical correction -0.03. So no correction should be made before verifying whether the X wear offset is read as diameter or radius; a wrong interpretation doubles the error. Z correction usually relates directly to the length; e.g. if a shoulder is 30.08 instead of 30.00, the tool may not have advanced enough. For the sign, look not only at the number but at which way the tool moves and which way the offset shifts the axis: mark the error direction on the drawing, enter a small correction, machine one part and re-measure.

10. T Code with Offset, Nose Radius and Imaginary Tip Direction

On FANUC lathes the tool and offset are mostly called by the T address: T0101 in the common scheme means turret station 01 and offset 01; T0303 tool 3 and offset 3. The T-code digit scheme and the geometry–wear relationship can vary by machine parameters; two- or four-digit schemes can be used. The exact structure must be verified from the real machine’s control.

Nose radius: the insert is not a theoretical sharp point; it has a nose radius (e.g. 0.4 / 0.8 / 1.2 mm). For simple straight OD/facing moves, programming on the imaginary tip can be enough; but in taper, radius, profile, chamfer and linked X–Z moves the real nose radius creates a dimensional difference, removed by nose radius compensation (G41/G42). On the offset screen, R (nose radius) and T/TIP (imaginary tip direction) are defined for the tool. The imaginary tip direction indicates which corner of the round tip is assumed as the zero point; it varies with the tool’s OD/ID, front/rear turret and right/left mounting. If the wrong direction is entered, G41/G42 shifts to the wrong side, machines the profile large/small or causes a crash. So entering the radius alone is not enough; the direction must be defined correctly too.

11. Offset Screen: GEOM/WEAR and INPUT / +INPUT

On a FANUC control, offset data is shown on different screens: GEOM (geometry offsets), WEAR (wear offsets), X, Z, R (nose radius), T/TIP (tip direction). When entering an offset, check that you are on the correct tool row, the GEOM/WEAR screen is selected correctly, the X/Z column and the sign are correct, and the decimal point is entered — entering 5 instead of 0.05 can turn a small correction into a serious crash risk.

Entry can be done two ways. INPUT: the entered value replaces the current one (current 0.020, 0.030 INPUT → result 0.030). +INPUT: the entered value is added to the current one (current 0.020, entered −0.010 → result 0.010). So use +INPUT with a positive/negative value to add to the current value, and INPUT to replace it entirely; the wrong key makes the size correction very different from expected.

12. Tool-Measuring Probe and External Presetter

Some lathes have a tool-measuring probe that swings out near the turret; the tool tip is touched to the probe surfaces to measure X and Z. Advantages: fast setting, less manual calculation, repeatable measurement, easy check after an insert change. But the probe is not automatically error-free: the correct tool/offset row, correct probe surface, low approach speed, tool direction, probe calibration and cleanliness must be checked; a wrong-direction/fast approach can break the probe and tool. Tools can also be measured off the machine on an external presetter (X/Z geometry, nose radius, direction); it reduces setup time in multi-tool production. But the presetter’s tool reference point must match the machine’s; otherwise the measured value cannot be used directly.

13. Setting the Work Coordinate; Workpiece Zero vs. Tool Offset

On a FANUC lathe the work coordinate is set in several ways: setting coordinates with G50, G54–G59 work coordinates, setting after automatic reference, entering values on the work-offset screen, or the maker’s special zeroing functions. In the older G50 method, the work coordinate is defined relative to the tool’s known start position with G50 X... Z.... In more modern use, G54–G59 stores the work zero in an offset table; G54 is selected in the program to activate it. This system makes the program independent of the machine position and lets separate zeros be used for different setups.

14. First-Part Setup: Mechanical and Program Checks

After all clamping and offset work, running the program on a real part for the first time is one of the most critical stages. On the first part the aim is not only to produce but to verify the program, tool path, offsets, clamping, cutting values and dimensions. The first part is not started at series-production speed.

Mechanical check: correct material, part seated on the stop, sufficient overhang/gripping length, suitable chuck pressure and runout, tailstock engaged if needed, jaws not in the tool path; correct tools in correct stations, sound inserts, tight holders, boring bar entering the hole, no collision during turret indexing; coolant nozzle aimed at the correct tool. Program check: program number, unit, active work coordinate, T codes, geometry/wear offsets, nose radius/direction, G96/G97, G50 limit, G98/G99, spindle direction, coolant commands, safe start/return (G28/G53), P–Q lines in cycles, and the safe retract at program end.

15. Tools for a Controlled First Run

Graphics/simulation can show the tool path, a reversed profile direction, a wrong coordinate and a G02/G03 direction error; but the real jaws, tool body, tailstock and nozzle are mostly not modeled, so even a correct graphic can still crash on the real machine. Machine lock runs the program while blocking axis motion to check flow; when the lock is released, a difference can arise between real and program position, so follow the maker’s procedure. Dry run shows the tool path at a different test speed; since dry-run speed can exceed the programmed feed, tool–part distance and E-stop access must be watched.

Single block stops after each line; on the first part you check the tool’s direction, distance to the chuck, whether the X diameter makes sense, and the correct tool/spindle direction — especially important at the first approach, turret change, G00 moves and cycle start. Rapid override is set to 25%/10% on the first run; a wrong approach is noticed earlier (but low speed does not replace a wrong offset). With feed override the first chip is watched under control (F0.30 + 50% ≈ F0.15); it can be limited in threading/synchronous operations. General approach: run in single block, low rapid, watch X–Z on the POSITION screen, stop while the tool is far from the part and check the remaining distance, take a very small first chip. Letting the tool enter with a full pass on the first part is an unnecessary risk.

16. Measuring the First Part; Which Dimension, Which Offset

On the first part you do not measure one diameter and go to series production; check OD/ID diameters, total length, shoulder lengths, groove width/position, thread diameter/pitch, chamfers, radii, surface quality, concentricity and runout. If the part is at machining temperature, the size can change when it cools; in tight tolerances, consider temperature. Compare the results with the drawing to find which tool affects which dimension:

• OD large/small → the X wear offset of that OD tool.
• Shoulder length wrong → the Z wear offset of the tool that machined that shoulder.
• Groove position wrong → the groove tool’s Z offset or the program coordinate.
• Groove width wrong → not only offset; tool width, side moves and squareness.
• Hole diameter wrong → the ID tool’s X offset, bar deflection and measuring method.
• If all tools’ Z is wrong by the same amount → not each tool offset, but the workpiece zero or the stop.

Diagnostic rule: if an error is only in dimensions machined by one tool, look at the tool offset; if it is common to all tools, look at the workpiece zero or clamping position.

17. Separating a Program Error from an Offset Error

Not every dimensional error is fixed with an offset. Fixable with an offset: tool wear, insert-change difference, the dimension shifting the same way on all related surfaces, a small diameter/length deviation. The program must be fixed: a wrong step length, wrong chamfer, wrong radius, a groove at the wrong coordinate, a wrong taper angle, a wrong P–Q profile or a wrong cycle parameter. For example if only one shoulder is 3 mm out of place, fixing it with the tool’s Z offset shifts all Z dimensions machined by that tool by 3 mm — here the program coordinate must be fixed. In offset correction, first verify the diameter/radius logic, apply part of the error, machine one part and re-measure; do not make big changes at once.

18. Insert Change, Tool Breakage and Series Stability

Insert change: even a same-code new insert can have a small size difference. Clean the pocket, fit the insert the right way, review the wear offset, machine the first part under control and re-check the critical dimension. Carrying the whole old wear offset to the new insert may be wrong (if the old insert was worn and a large correction was entered, the new insert machines the part small). On tool breakage, changing only the insert is not enough; check the holder, pocket, shim, screw, turret seat, part, jaws and turret alignment — a severe crash can bend the holder, in which case the geometry offset is re-measured.

Series stability: after the first part is correct, dimensions are monitored; tool wear, part/coolant temperature, chuck pressure, chips in the jaws, raw-diameter variation and machine warm-up can change the size. Not the geometry but small changes are managed with the wear offset each part; the size trend (parts slowly growing) is tracked to plan tool life. If the clamping changes (soft jaws re-turned, stop/raw length changed, chuck/collet changed), the tool geometry offsets can stay largely the same but the workpiece zero must be re-verified; if the turret/holder changes, the geometry is re-measured.

19. Second Setup, Protection Zones and a Parameter Warning

Many parts cannot be finished in one setup; after parting from the bar, the back face is machined in a reversed setup. In the second setup, protect the finished surface, check runout, set the new Z zero, adjust clamping force and check that the jaws do not crush the finished surface; soft jaws are a big advantage here. A separate work coordinate can be used for the second operation (e.g. G54 first, G55 second setup). Some machines allow chuck/tailstock protection zones; but they can be wrongly defined/disabled or not represent the real tool length — electronic protection does not replace the operator’s physical collision check. When a tool/work-zero problem occurs, do not touch CNC parameters: use the work-offset, geometry and wear screens; service parameters like axis direction, unit and reference behavior are changed only by authorized personnel.

20. Example Full Setup Scenario

Part: raw Ø50 steel bar, finished length 60 mm, Ø40 and Ø30 steps, Ø12 center hole, groove and external thread, to be parted from the bar. Tools:

Setup order: (1) Chuck prep — suitable/soft jaws, stop, pressure to suit the material. (2) Clamp part — required overhang, seat on the stop, safe procedure, runout with an indicator if needed. (3) Mount tools — correct stations, groove/parting squareness, drill on center, short overhang, turret-indexing collision check. (4) Reference return. (5) Z zero — thin chip off the face with T0101, retract only in X, register Z0. (6) T0101 X geometry — machine a short diameter, retract in Z, measure, enter into X geometry. (7) Measure other tools — Z from the common face, X from a test diameter/probe. (8) Tip data — radius and direction. (9) Program check — T codes, G50/G96/G99, work coordinate. (10) Controlled run — low rapid, single block, light first chip. (11) First-part measurement — all dimensions, small differences via wear, re-measure the second part; do not go to series production before stability is seen.

21. Common Mistakes in First Setup

• Gripping the part with the jaw tips (contact drops, the part slips).
• Closing the chuck without seating the part on the stop (Z changes each part).
• Excessive pressure on a thin part (goes oval when removed).
• Being on the wrong offset row while measuring a tool.
• Entering a large value in WEAR instead of GEOM; entering the measured diameter as radius.
• Not entering the nose radius or direction (error in profiles/tapers).
• Not checking G54/the work coordinate; not physically checking turret indexing.
• Running the first program at full rapid; fixing all dimensional errors with the wear offset.

22. Boring Soft Jaws: When, Why and How

Recommendation of the Mentor CNC editorial team. This section is based on our team’s shop-floor experience; the chuck and machine manufacturer’s manual always takes priority. The question is simple: which operation calls for hard jaws, which one for soft jaws, and why must soft jaws always be bored before use?

First operation (OP10): hard jaws on scaled, raw stock

Castings, forgings and hot-rolled bar come with a hard outer skin (mill scale, slag). Scaled stock can be held in soft jaws, but our recommendation is to use hard jaws for the first roughing operation whenever possible. The reason: the hard skin crushes the gripping surface of a soft jaw, the grip deteriorates, and under a heavy cut the part shifts or can even be thrown out of the chuck. Even if it stays in, a part that has moved is machined with runout and the reference surfaces cut in OP10 come out wrong.

The serrations of a hard jaw bite into the skin and hold the part securely. The marks they leave do not matter, because that surface will be machined in the next operation anyway. The goal of OP10 is to machine the back of the part — the diameter and the shoulder that will be gripped in the second setup — clean and free of chatter. Those surfaces become the locating references for OP20.

Second operation (OP20): soft jaws, and the two reasons for them

A lathe machines parts of revolution — a shaft, a bushing, a flange, it makes no difference. When the part is gripped on a machined surface, soft jaws are used, and those jaws are bored in the machine’s own spindle axis. There are two reasons:

1. Removing runout. A small runout in the chuck body grows in unbored jaws and grows again in the part. Our team’s shop observation: a chuck runout of about 0.02–0.03 mm becomes 0.07–0.08 mm at unbored jaws and, depending on the case, as much as 0.1–0.2 mm at the workpiece. When the jaws are bored in the machine’s own axis the part runs true, and no step or eccentricity shows between the surface machined in OP10 and the surface machined in OP20.
2. Holding the part firmly without damage. Gripping a finished surface in hard jaws crushes it and the surface finish is lost. Unbored soft jaws, depending on the diameter, touch the part only at their outer edges or only at the centre — line contact. Jaws bored to the gripping diameter wrap the part all the way round: the clamping force is spread over the surface, the grip is both runout-free and far stronger.

How to bore soft jaws, step by step

1. Fit the soft jaws to the chuck and tighten the jaw bolts as the manufacturer specifies. Set the chuck clamping pressure to the pressure the part will actually be machined at.
2. Never bore jaws unloaded. Clamp a ring or spacer slightly smaller than the gripping diameter (for a Ø30 part, roughly Ø28–29) in the jaws so that they are preloaded in their real working direction while being bored. For OD gripping the ring sits inside the jaws, behind the area to be bored; for ID gripping it goes around the outside of the jaws. It is the jaws that are machined, not the ring.
3. Bore the jaws to the actual diameter of the surface to be gripped and to the depth of the gripping length, leaving a clean, flat locating shoulder at the bottom. Keep the door closed, use a low spindle speed and light cuts.
4. Remove the ring, clamp the part and check runout with a dial indicator. If it is outside the acceptable limit, re-bore the jaws; tapping the part with a hammer to “seat” it is not a solution.

Rule of thumb: scaled raw stock → hard jaws; machined surface → soft jaws bored under load to the gripping diameter. Re-bore the jaws whenever the clamping pressure, the jaw bolts or the spacer ring changes.

23. Chuck Controls on the Lathe Panel: Runout Check (Spindle Jog) and Clamping Direction (Chuck Clamp)

Most CNC lathe operator panels carry two chuck-related controls. Their names and positions vary between builders; confirm them in your machine’s panel manual.

• Spindle Jog (runout check): With the part clamped, holding this button turns the chuck at a low speed (typically a few hundred rpm) and releases it when let go. Its purpose is to check by eye or with a dial indicator whether the part is running true; it has no effect on anything else. For an indicator reading the chuck can also be turned by hand.
• Chuck Clamp — Inside / Outside (clamping direction): In Outside the jaws close inward and grip from the outside (shafts, solid stock); in Inside they open outward and grip a bore (tubes, flanges). If the direction is wrong the control receives the “chuck clamped” signal while the part is actually loose: an alarm at spindle start, or a thrown part. Whenever the clamping direction changes, the clamping pressure and the direction in which the soft jaws were bored must be reconsidered.
• M10 / M11 and the foot pedal: On hydraulic chucks the chuck is normally clamped and released with a foot pedal; some machines also accept M10 (clamp) and M11 (unclamp) from the program. The code numbers are builder-specific; check the machine’s M-code list.

24. Tool Geometry Offset (X and Z) on a FANUC 0i-T, Step by Step

Here is the key sequence on a FANUC 0i-T for the logic explained in sections 7 and 11. The geometry offset holds the tool’s basic position; the wear offset holds the small corrections made during production. On first setup only the geometry is measured.

1. Z geometry: Call the tool safely in MDI or HANDLE, start the spindle and take a light skim cut across the face by hand. Without moving Z, retract the tool in X only and stop the spindle. If the machined face is the part zero the measurement is 0; otherwise measure the distance from part zero to the face.
2. Go to OFFSET/SETTING → [OFFSET] → GEOMETRY and move the cursor to the tool’s offset number (01 for T0101). Press the Z address key, type the measured value (Z0 if the face is Z0) and press [MEASUR]. The control calculates the Z geometry from the tool’s current machine position.
3. X geometry: Take a light cut over a short length of the outside diameter. Without moving X, retract the tool in Z, stop the spindle and measure the machined diameter with a micrometer (for example 39.86).
4. On the same GEOMETRY line press the X address key, type the measured diameter (X39.86) and press [MEASUR]. On a diameter-programmed axis the diameter is entered; entering the radius doubles the error.
5. Enter the nose radius (R) and the imaginary tip number (T) on the same line. A MEASUR on the GEOMETRY screen resets that line’s WEAR value to zero. Repeat for every tool, retract to a safe position and machine the first part in single block, then measure it.

Later size corrections go into the WEAR screen, not the geometry: type the deviation with its sign and add it to the existing value with [+INPUT] (the diameter difference for X), then machine and measure one more part. Soft-key names and the measuring method (probe, gauge, part surface) can differ between control versions and machines; the machine’s operator manual takes priority.

The Core Logic of Setup: Three Layers

CNC lathe setup is thought of in three layers: Where is the machine? (reference return and machine coordinate system) → Where is the part? (workpiece zero and work coordinate) → Where is the tool tip? (tool geometry and wear offsets). Only when the control knows all three correctly can it move the program’s X40 Z-30 point to the physically correct place. So setup is not a side task separate from programming but the direct foundation of CNC lathe production. When the program, part zero and tool offset work correctly together, the machine applies the same program precisely, again and again, with different tools, in different clampings and in series production.

Assessment Test

1. Which of the following does sending the machine to reference do automatically? A) Creates the workpiece zero B) Registers the machine’s own position C) Corrects tool wear D) Enters the nose radius
2. In standard OD turning, where is Z0 usually? A) The part center B) The finished face C) The chuck face D) The tailstock tip
3. (True/False) The geometry offset is the large value measured at first setup; the wear offset is used for small size corrections.
4. Target Ø40.00 but the part is Ø40.06. In a diameter-based system, roughly what is entered into the X wear offset? A) +0.06 B) -0.06 C) -0.03 D) +0.12
5. If all tools’ Z dimension is wrong by the same amount, where do you look first? A) Each tool’s separate offset B) The workpiece zero/clamping stop C) The nose radius D) The cutting speed
6. (True/False) Entering only the nose radius is enough; the imaginary tip direction is unimportant.
7. What is the main difference between the workpiece zero and the tool offset? A) They are the same B) The work zero defines the part’s position, the tool offset each tool’s tip position C) The tool offset is common to all tools D) The work zero is separate for each tool

Open-Ended Questions

• Why are soft jaws turned, and what are the conditions for preparing them correctly?
• Explain the difference between the geometry offset and the wear offset.
• Why is diameter–radius confusion dangerous in X wear correction?
• How do you decide whether a dimensional error is fixed with an offset or a program correction?
• Explain the three layers of setup (machine, part, tool tip) in your own words.

Summary and Next Lesson

In this lesson we learned workholding, chuck/tailstock use, the workpiece zero, tool geometry and wear offsets, nose radius and first-part setup. You now know how the program, part zero and tool offset work together. In the next lesson we move on to basic G and M codes and manual programming, turning our coordinate, tool, cutting-value and setup knowledge into a real CNC lathe program.

Frequently Asked Questions About CNC Lathe Setup

How do I set the part zero (Z0) on a CNC lathe?

The finished face is taken as Z0. Approach at low speed, take a light skim cut across the face, retract the tool in X only without moving Z, and register that face as Z0 in the control. On a FANUC 0i-T this is done by typing Z0 on the tool's GEOMETRY offset line and pressing [MEASUR]. The paper-touch method is approximate and dangerous on a rotating part; a skim cut or a tool-setting probe is preferred.

How are tool offsets entered, and what is the difference between geometry and wear?

The geometry (GEOM) offset holds the tool's real position in the turret and is measured at first setup: for Z, skim the face and use Z0 with [MEASUR]; for X, cut a short diameter, measure it with a micrometer and use that diameter with [MEASUR]. The wear (WEAR) offset corrects the small deviations measured during production: type the deviation with its sign and add it with [+INPUT]. Large values never go into the WEAR screen.

Why and when are soft jaws bored?

Soft jaws are used in the second operation, when the part is gripped on a machined surface, and they are bored to the gripping diameter in the machine's own spindle axis. This removes chuck and jaw runout, makes the part run true and lets the jaws wrap the part instead of touching it along a line. Boring is done under load, with a ring slightly smaller than the gripping diameter clamped in the jaws, never with the jaws open. This is a recommendation of the Mentor CNC editorial team based on shop-floor experience.

Can scaled or slag-covered raw stock be held in soft jaws?

It can, but it is not recommended. The hard skin crushes the gripping surface of the soft jaw; under a heavy cut the part shifts or can be thrown out. Use hard jaws for the first roughing operation; the jaw marks land on a surface that the next operation machines away. In that operation, machine the diameter and the shoulder that the second setup will grip, clean and chatter-free.

The part came out oversize or undersize; which offset do I correct?

First decide whether it is a program error or an offset error: if every dimension cut by one tool is off in the same direction by the same amount, correct that tool's wear (WEAR) offset. For a diameter error enter the diameter difference in X wear (for example −0.06 for Ø40.06 instead of 40.00); for a length error enter the length difference in Z wear. Change the geometry offset only when the tool is re-mounted or the first measurement was wrong.

How is chuck runout checked?

With the part clamped, rest a dial indicator on a machined diameter or on the face, turn the chuck by hand or with the panel's runout-check (Spindle Jog) button at low speed, and read the total indicator movement. If it exceeds the acceptable limit, re-clamp the part or bore the soft jaws; a part held in properly bored jaws normally needs no further check within the same operation.

How is a tool set with a tool setter (tool-setting arm)?

A tool setter writes the geometry offset automatically by touching the tool tip against a calibrated probe face. The general sequence is: send the machine to reference; swing the arm down from the panel or by hand and check that the turret cannot collide with it; activate offset-write mode (a button on some machines, automatic when the arm is lowered on others; on a FANUC 0i-T the GEOMETRY page opens and OFST blinks in the status line); call the tool to be set and put the cursor on its offset line; using the handwheel at x10 and then x1 with a low feed override, bring the tool tip toward the probe face. At contact the control stops the axis in that direction and writes the measured value into the geometry offset under the cursor. The X-direction face is used for diameter and the Z-direction face for length; OD tools and boring tools touch opposite faces of the probe. When all tools are done, raise the arm and cancel write mode. Never approach the probe in RAPID; a damaged stylus mis-measures every tool.

A tool set with the tool setter is off by a constant amount — why?

The tool setter touches the tool against the probe face, not the part; the distances between the probe faces and the machine’s measuring reference are stored in the control as calibration parameters. If the arm has been crashed, the stylus is worn, or those parameters have been corrupted, every tool set with the arm is off in the same direction by the same amount. Diagnosis is simple: machine a short test diameter with a tool set by the arm and measure it with a micrometer; if the error is identical on every tool, the problem is calibration, not the tool. The correction is done with the machine builder’s calibration procedure. On the FANUC 16i/18i/21i-T and 0i-T families these distances live in the parameter group 5015–5018; which number belongs to the X+/X− and Z+/Z− faces depends on the series and the builder, so no value is entered without checking the machine’s parameter manual, and a parameter backup is taken first. Writing the error into each tool’s wear offset only hides the problem; it returns at the next tool measurement.