CNC Milling Training 6: Part Zeroing and Tool Length (G43)

On a CNC mill, writing the program correctly is not enough on its own. If the workpiece is clamped incorrectly, the part zero is set wrong, or the tool length offset is entered incorrectly, even a correct program runs in the wrong place. Three basic relationships must be established: the machine must know where the workpiece is, it must know where the tool tip is, and the workpiece must not move under cutting forces. This lesson covers safe workholding, part zero (G54–G59) and tool length compensation (G43/G49). (Cutter radius compensation G40/G41/G42 is covered in a separate lesson.)

1. Objectives of the lesson

After this lesson the student will be able to explain the importance of workholding; understand the roles of vise, clamp, fixture and stop; select suitable clamping surfaces; choose the workpiece zero; grasp the logic of edge finders and probes; transfer X/Y/Z values into G54–G59; explain the relationship between tool length and its offset; safely call the H address and G43 compensation; and assess the risks of a wrong H value or wrong Z zero.

2. Preparation sequence

General preparation: technical drawing → check stock dimensions → order the operations → decide the clamping method → clamp the part in the vise/fixture → prepare the cutters → load the magazine → measure tool lengths → find the X/Y/Z zeros → record G54–G59 → compare program, tool and offset values → test safely. A small mistake at this stage can affect all subsequent operations.

3. Why is workholding important?

The cutting tool applies forces in different directions; it can push, pull, rotate, lift or vibrate the part. If clamping is inadequate, the part can move during cutting even if it started in the right position, resulting in dimensional errors, poor surface finish, tool breakage, the part coming out of the vise, or a collision. Workholding is not only about holding the part still — it is about maintaining its position and rigidity throughout machining.

4. Requirements of good workholding

Proper clamping must resist cutting forces; prevent lifting, rotation and sliding; not block the surfaces to be machined or the movement of the tool/holder; not distort the part unnecessarily; provide a similar position on re-clamping; prevent chips from being trapped; and allow measuring and safe removal. Being tight is not enough on its own: a thin part over-clamped at the wrong point will bend, and spring back when the vise is opened, spoiling the dimension.

5. Reference surfaces and the 3-2-1 principle

Before clamping, decide which surfaces will serve as references: the bottom face (sits on parallels), a side face (rests against the fixed jaw) and an end face (rests against a stop). This way the part locates in nearly the same position each time. A part has six degrees of freedom in space; in the 3-2-1 principle, 3 points define the primary plane (bottom), 2 points the secondary plane (side) and 1 point the tertiary plane (length) — locating the part without over-constraining it. A vise plus parallels is the practical application of this principle.

6. Clamping with a CNC vise

The most common workholding element is the precision machine vise (fixed jaw, movable jaw, body, clamping mechanism, replaceable jaw plates). The fixed jaw is the primary reference for repeatability. Alignment: the vise is not just set on the table — its fixed jaw must be parallel to the machine axes. A dial indicator is mounted in the spindle, moved along the fixed jaw, deviation is observed, the vise is adjusted, and the bolts are tightened in a controlled way. If alignment is off, a straight line in the X direction in the program will not run parallel to the real edge on the part.

7. Use of parallels and clamping force

Parallels hold the part at a set height above the base (access to the bottom face, repeatable height). They must be of equal height, clean and undamaged, and must not sit on chips. As the vise is tightened the movable jaw can lift the part; the part is seated onto the parallels with a soft mallet (never a steel hammer), and the parallels are checked to make sure they are not loose. Clamping force: too little causes slipping; too much bends a thin part, marks soft material and distorts geometry. The force is set according to material, cutting force, contact area, thickness and machining direction.

8. Use of soft jaws

Soft jaws are jaws machined specifically to the part: they hold specially shaped parts, grip over a wider area, distort thin parts less, and improve repeatability and protection of finished surfaces. When machining them, a preload close to the real clamping condition must be applied; if the jaw is machined unloaded and the part is then clamped, the jaw geometry can change.

9. Clamping with T-slots, bolts and clamps

Large parts that do not fit in a vise are clamped directly to the table using a T-nut, stud, clamp, step block, support element and locating pin. The rear support of the clamp must be at a suitable height, and the part of the clamp near the bolt must transfer force to the part. Cautions: the clamp must not enter the tool path, the stud must not stick up too far, the tool holder must not hit the stud, the block must not slip, the clamping force must not bend the part, and the T-nut must seat correctly in the slot.

10. Fixture, vacuum and magnetic clamping

Fixture: a special device that locates and clamps the part quickly and repeatably (locating pins, stop surfaces, mechanical/hydraulic/pneumatic clamping, sensors, chip clearance); it makes re-finding the program zero easier in mass production and for irregular parts. Vacuum: for wide/thin plates; requires sufficient sealing area, the cutter not opening the vacuum zone, monitoring of vacuum loss and limited cutting force. Magnetic: clamps ferromagnetic material over a wide surface; material suitability, sufficient force, cutting direction and residual magnetism must be considered.

11. Chip/burr hazard and clamping height

If even a tiny chip gets under the part or on a stop surface, the part clamps crooked; the top face will not be parallel, holes may not be perpendicular, and dimensions and zero will change. Before clamping, the table, vise, parallels, part surfaces and stops must be cleaned and burrs removed. Height: if the part is too low the holder can hit the jaw or a short tool cannot reach; if too high, rigidity drops and vibration increases. The part must be clamped at a height that gives access but stays as rigid as possible.

12. Post-clamping checklist

Is the vise/fixture firmly bolted to the table, is the alignment correct, does the part sit on the parallels?
Are there chips on the stop surfaces, has the part lifted, is the clamping force sufficient, could the part be distorted?
Can the tool reach all surfaces, will the holder hit the jaw/bolt, in which direction will the part be loaded?
Is the part zero measurable?

13. What is the workpiece zero and how is it chosen?

The workpiece zero is the starting point from which all coordinates in the program are measured; it is the introduction of the drawing’s dimension origin to the machine. It can be a corner, the center, a hole center or a fixture pin. When choosing: where are the dimensions given from, is the part symmetric, can the same zero be re-found, are the edge/center measurable, does the clamping block access, are there multiple operations, and to which origin was the CAM prepared? If dimensions are given from the lower-left corner, that corner is convenient; for a symmetric part, the center may be more suitable.

14. G54–G59 work coordinates

On FANUC machining centers the common work coordinates are G54, G55, G56, G57, G58, G59. Each stores the distances between the machine zero and a separate workpiece zero. For example G54 → part in the first vise, G55 → second vise, G56 → a special fixture. When G90 G54 G00 X0. Y0.; is written, the tool goes to X0 Y0 relative to the zero saved as G54.

The X, Y, Z values on the G54 screen define where the part zero is relative to the machine coordinate system: the machine knows its own zero, the operator measures the part zero, and G54 stores the relationship between the two. Example values (different for every machine and setup): G54 X−520.000, Y−245.000, Z−410.000.

15. Methods for finding the X and Y zero

To find the part edge or center you can use: touching with the cutter, a mechanical edge finder, an electronic edge finder, a dial indicator, a probe system, a precision pin/gauge, or a fixture reference point. Each method has different accuracy and safety.

15.1. Touching the edge with the cutter

The simplest method, but applied carefully because of the risk of damaging tool/part. Example: if a Ø20 mm tool touches the left edge, the tool center is inside the edge by the tool radius (10 mm); applying a 10 mm correction to the reading gives the real edge. Risks: approaching from the wrong direction, feeding too far into the part, catching the cutting edge, tool runout, and using the wrong diameter. A low jog rate and authorized supervision are required.

15.2. Mechanical and electronic edge finders

A mechanical edge finder is mounted in the spindle, rotated at a suitable low speed, and approached to the edge in a controlled way; it shows a specific contact behavior, the machine position is read and the finder’s radius is accounted for. For example a finder with a 10 mm tip has a 5 mm radius; if the left edge is found, the 5 mm difference between tool center and edge is taken into account. An electronic edge finder gives a light/sound/screen signal on contact; some models work without spindle rotation. Electrical conductivity, contact sensitivity and calibration must be considered.

15.3. Zeroing with a probe

A touch probe can measure the part edge, corner, center, hole center, surface height and part angle. It reduces setup time and operator errors and can write coordinates automatically. However, the probe program and protective moves must be prepared correctly; a probe can also break with a wrong rapid move.

16. Edge and center calculation (mind the sign)

If a Ø10 edge finder touches the left edge, the tool center is 5 mm to the left of the edge; the real edge is 5 mm further in the positive X direction. If the same device touches the right edge, the tool center is 5 mm to the right; the real edge is 5 mm away in the negative X direction. The signs differ for left and right — a single memorized “add/subtract” rule does not apply to all edges. Always make a small sketch: where is the part, where is the tool center, which way is positive X, on which side of the center is the real edge.

Finding the center: to find the X center of a rectangular part, measure the left and right edges. Example: left edge X−500.000, right edge X−400.000 gives center X = (−500 + −400) / 2 = −450.000. If the edge finder radius is used symmetrically in both measurements it can cancel out. The same method applies to the Y axis. A circular part/hole center is found with a probe cycle, dial indicator, coaxial center finder or multiple edge measurements; when indicating, the spindle motor is not run — it is turned by hand to compare deviations.

17. Determining the Z zero

The Z zero is commonly taken from the workpiece top face, fixture top face, vise reference face, table face or a fixed measuring plane. In introductory training the part top face is usually taken as Z0: Z+ above the part, Z0 the part surface, Z− into the part. The tool tip is approached to the surface in a controlled way; for contact you can use thin paper, a feeler gauge, a gauge block, an electronic Z setter or a tool probe. The paper/feeler method is used only by a trained operator and at a very low handwheel step; for example if a 0.10 mm feeler is used, the contact position is not the surface itself and the feeler thickness must be accounted for.

Choosing the fixture face as Z0

Z0 does not always have to be the part top face. If the top face of the fixture is chosen as Z0, the part thickness is accounted for inside the program. For example, if the part clamped on the fixture is 20 mm thick, the part’s top face becomes Z20 in the program.

This method can be preferred in production where parts of different thicknesses are machined on the same fixture: the Z zero is not re-measured for every new part, only the thickness value in the program is updated. However, the part thickness must be measured correctly; if the thickness is wrong, all Z dimensions come out wrong.

18. Why is tool length needed?

Not all tools loaded in the magazine have the same length (e.g. a face mill is short, an end mill medium, a drill long, a boring tool longer). If the control only knows the position of the spindle nose, it cannot know the real location of each tool tip. Therefore the tip position of each tool is measured and saved as a tool length offset, called within the program using G43 and the H address.

19. Tool length compensation, the H address and G43/G49

Tool length compensation lets the control account for the distance between the spindle reference point and the real cutting tip; the programmer does not have to write a separate Z for each tool. When G43 H02 Z50.; is written, the control reads the length in cell H02 and positions the tool tip at Z50 relative to the part coordinate.

The H address selects the tool length offset number (e.g. T01→H01, T02→H02). Keeping T and H the same is not a mandatory FANUC rule but is good shop practice that reduces error risk. G43 is positive tool length compensation: G43 H01 Z50.; → activate the H01 offset and move the tool tip to Z50 relative to the selected part coordinate. G49 cancels compensation: G00 Z100.; G49;. But since the Z-axis behavior at the moment of G49 depends on the current position, the tool is first moved to a safe zone and then compensation is canceled — canceling randomly near the part can produce an unexpected Z move.

A note on G44: On some controls G44 is used for negative tool length compensation. Standard vertical machining center practice almost always uses G43; G44 appears only in special applications that depend on the machine and its tool measuring setup. Do not use G44 instead of G43 without confirming it in the programming manual – a wrongly signed length compensation can move the tool in an unexpected Z direction.

20. Tool length measuring methods

Tool lengths can be measured with different systems: (a) Difference from a reference tool — one tool is taken as reference and the length differences of the others are measured; (b) Against a fixed measuring surface — all tools touch the same reference face, and the machine position for each becomes its length offset; (c) In-machine tool measuring probe — the tool touches a sensor and length/diameter/breakage are checked; (d) External tool presetter — tool and holder are measured off the machine, so preparation is done without stopping the machine and tool cards are created.

21. Absolute length and difference length systems

Absolute system: the real length of each tool from a set reference is stored (e.g. H01=125.430, H02=163.250, H03=98.670). Difference-from-reference system: the reference tool is taken as zero/base and the others’ differences are written (e.g. H01=0.000, H02=+37.820, H03=−26.760). No offset value should be entered without knowing which method is in use. Absolute length measurement is common on modern machines.

22. Geometry and Wear offsets

Some FANUC systems have Geometry and Wear sections on the tool offset screen. Geometry contains the tool’s main dimension (real length/radius). Wear is for small wear and dimensional corrections; for example if a machined surface is left 0.03 mm high, a small wear correction is made. Instead of constantly changing the main length, production corrections are made from the wear field — but no value should be entered without checking the effect of the sign on the part dimension.

23. Safety when entering offsets and in T–H matching

When entering H values, the correct tool number must be checked, Geometry/Wear columns not mixed up, the decimal point and sign verified, the value re-read and the tool physically measured. For example entering 1524.30 instead of 152.430 produces a serious Z error. T–H matching error: if T03 M06; G43 H02 Z50.; is written, H02 is applied to T03; if the length difference is large the tool may hit the part, stay too high or go into the table. The safe habit is to keep the T03→H03 match. When the tool changes, G43 must be called again with the new H — do not assume the previous offset is still valid.

Tool pull-out from the holder

If the tool slips downwards in the holder under cutting force, pocket depths gradually increase, holes come out too deep, the tool can break and it can crash into the table or fixture. The most characteristic symptom is a depth that keeps changing as the operation progresses.

Do not continue production by adjusting the H offset in this situation. The offset only hides the problem while the root cause keeps growing. Check the collet and nut, the cleanliness of the tool shank, the clamping torque, whether the holder type suits the operation, and the depth of cut and cutting conditions.

Offsets after a broken or replaced tool

When a broken or worn tool is replaced, never blindly reuse the old Geometry value. Even with the same tool model, the clamped length, the tip length and the collet position can differ. Re-measure the real length (and diameter if needed) of the new tool, review the wear value, run the first part at reduced speed while watching the Z approach carefully, and re-measure the part.

24. The relationship between part Z zero and tool length

For the Z position to be correct, two pieces of information are needed together: the position of the workpiece top face inside the machine (in the G54 Z value) and the position of the tool tip relative to the spindle (in the H offset). Simply: G54 Z → where is the part, H01 → where is the tool tip, Z in the program → where should the tip go on the part. The control combines these three to compute the real axis move. Two shop approaches exist: (A) part-top G54 Z + absolute tool lengths, (B) difference relative to part top with a reference tool. The values of the two approaches must not be mixed.

25. Saving G54 values and the INPUT/MEASURE difference

General logic: OFFSET/SETTING screen → Work Coordinate page → coordinate system (e.g. G54 X) → evaluate the measured machine position → apply edge-finder/radius correction → save with MEASURE or INPUT → repeat for Y and Z → re-check the values. Key names vary by model (MEASURE, PART ZERO SET, ORIGIN, etc.) and must be learned from the manufacturer’s manual. INPUT writes the typed number directly into the cell; +INPUT on some screens adds to the existing value (if misused, it adds onto the old offset); MEASURE computes the offset from the current machine position and the typed dimension. The behavior of these functions must be verified for the control model.

26. G54 selection and multiple parts

If G54 is not explicitly selected in the program, a G55 left over from the previous program or a default coordinate may be active; the tool runs the correct geometric program in the wrong place. So the coordinate system is stated explicitly at the start of each program: G90 G54;. If there are two vises on the table, left → G54, right → G55, and the same geometry can be machined at two zeros: G54; M98 P2000; G55; M98 P2000; — each offset must be measured and verified separately.

27. Safe G43 calling and part-zero check

G43 is activated with a safe Z move after a tool change. Example: T01 M06; G17 G90 G54; S1500 M03; G00 X20. Y20.; G43 H01 Z50.;. What matters: the tool not being inside the part, the correct H number, a safe Z target and the correct G54 Z value. After the offset is saved the tool is not plunged straight into the part; first a check at safe Z: G90 G54; G00 X0. Y0.; moves the tool to X0 Y0, it is checked whether it is physically over the zero point, then G43 H01 Z50.; is called. No direct rapid to Z0; the tool is approached in steps Z50→Z20→Z10→Z5 (Single Block on, Rapid Override low, Distance to Go visible).

28. Machine, Absolute and Relative coordinates

The operator must distinguish three displays: Machine is the real axis position relative to machine zero; Absolute is the position relative to the active work coordinate (if G54 is active, relative to the G54 zero); Relative is a relative display the operator can temporarily zero. Zeroing Relative does not zero G54 — these concepts are frequently confused by beginners.

29. Short introduction to G41–G42 cutter radius compensation

Tool length compensation accounts for the length along Z; cutter radius compensation shifts the tool center off the programmed contour by the radius. Basic codes: G40 cancels radius compensation, G41 offsets the tool to the left of the path, G42 to the right. The radius value is usually called with the D address (G41 D01). Because G41/G42 depend on feed direction, whether the contour is internal or external, the approach/exit move and the offset sign, the detailed treatment is given in a separate lesson.

30. Tool length compensation example (full program)

Tool data: T01 = Ø50 face mill, H01 = 135.420 mm; T02 = Ø10 end mill, H02 = 168.750 mm. Each tool is called with its own H number.

O1600 (TOOL LENGTH APPLICATION);
G17 G21 G40 G49 G80 G90 G94;
(T1 FACE MILL)
T01 M06;
G54 S1200 M03;
G00 X0. Y0.;
G43 H01 Z50.;
M08;
G00 Z5.;
G01 Z0. F100.;
...
G00 Z100.;
M09;
M05;
G49;
(T2 D10 END MILL)
T02 M06;
G54 S3000 M03;
G00 X20. Y20.;
G43 H02 Z50.;
M08;
G00 Z5.;
G01 Z-3. F120.;
...
G00 Z100.;
M09;
M05;
G49;
G91 G28 Z0.;
G90;
M30;

31. Common mistakes in zeroing and offsets

Entering a value on the wrong G54 line (measurement belongs to G54 but the value is written to G55).
Not accounting for the edge-finder radius; the tool center is taken as the edge.
Applying the plus-minus correction on the wrong side (the error grows by two radii).
Forgetting the gauge/feeler thickness; the Z zero shifts by 0.10 mm.
Entering a large value in the Wear field instead of Geometry.
Calling the wrong H number (T03 length applied to T04).
Using the decimal point incorrectly (a different magnitude instead of 125.430).
Re-clamping the part and using the old zero; seating the part on a chip-covered surface; issuing G49 while inside the part.

32. Offset checklist and first run

Before the program: is the active coordinate G54; are the G54 X/Y/Z values correct; is the zero the same as the drawing; are the tool and H numbers correct/matched; is H Geometry correct and is there an old correction in Wear; is G43 called at a safe Z; is G49 canceled in a safe place; is the program in G90; is the first Z target safe? First run: the correct program is selected, the tool list and G54–G59/H offsets are checked, the graphic is reviewed, Single Block is turned on, Rapid Override is lowered, the tool is sent to the X–Y zero at safe Z, the physical position is checked by eye, Z is approached in steps, the first depth of cut is watched under low control, the part is measured, and if needed only a controlled wear correction is made. Offset changes during production (time, tool, offset, old/new value, reason) are recorded.

33. Setup sheet and program-zero consistency

The programmer may have taken the part center as zero; if the operator sets the left edge to G54 X0, the program runs in the wrong place. So the zero point must be clearly shown on the drawing or the CAM setup sheet. The setup sheet should contain: a picture of the zero point, the G54–G59 selection, the X/Y/Z reference surfaces, the tool list, the H and D numbers, the clamping layout and the safe Z height.

34. Practice: setting the part zero (G54) from an edge and from the centre on a FANUC vertical machining center

Here is the key sequence, on a FANUC 0i-M class vertical machining center, for the logic explained in sections 13–17. The method is based on a reference tool: the Z value of the part zero is taken with the reference tool, and the lengths of all other tools are entered as differences relative to it (section 35). Soft-key names may differ slightly between control versions.

If the lower-left corner is the part zero

With the reference tool in the spindle, select HANDLE mode and a low increment (x10, x1 close to contact). If you touch with the tool itself, run the spindle at low speed; with an edge finder, follow the device’s own rule.
Touch the tool to the left edge of the part in X. On the POS → [REL] screen press the X address key, then the [ORIGIN] soft key that appears: REL X becomes 0.000. This only zeroes the counter; it is not yet the part zero.
Lift the tool in Z and move in +X by one tool radius (REL X = 5.000 for a Ø10 tool). The tool centre is now exactly over the edge.
Open OFFSET/SETTING → [WORK], move the cursor to the X cell of the G54 (01) line, type X0. and press [MEASURE]. The control writes the tool’s current machine coordinate into G54 X by itself.
Repeat for Y on the front edge: touch → REL Y [ORIGIN] → move +Y by one radius → WORK G54 Y cell → Y0. → [MEASURE].
Z: Touch the reference tool to the top face of the part (with thin paper or a feeler gauge); in the WORK G54 Z cell type Z0. and press [MEASURE]. This Z refers to the tip of the reference tool, whose H offset stays 0.
Send the axes to reference (Z first, then X and Y). As a check, run G90 G54 G00 X0 Y0; in MDI: at a safe height the tool centre must come to rest exactly over the lower-left corner of the part.

If the part centre is the zero: the halving method

Touch the tool to one edge of the part (say the left) and zero REL X with [ORIGIN].
Lift the tool, go over to the opposite edge (right) and touch it from the outside. Read REL X; this value is the part width plus the tool diameter, but the centre is still exactly at half of it.
Lift the tool and move back until REL X shows half the reading (example: 70.000 read → go to 35.000). The tool centre is now at the part centre. In the WORK G54 X cell type X0. and press [MEASURE].
Do the same for Y using the front and back edges; take Z as above.

With this method the tool diameter does not need to be accounted for; halving cancels it out. With a touch probe the same logic is performed automatically by the probe’s measuring macro.

35. Practice: measuring tool length differences against a reference tool with a dial-type Z setter

Where the machine has no tool-setting probe this is the most common method. The tool needed is a Z-axis setter of known height (usually 100 mm) with a dial indicator on top. The setter’s height does not actually matter here, because what is measured is not an absolute length but the difference relative to the reference tool.

The reference tool is the tool you took the part-zero Z with; its H value stays 0. Place the Z setter on the table or on the part and remove its cap.
In HANDLE, lower the reference tool onto the setter until the dial reads zero. Without touching the handwheel, POS → [REL] → Z → [ORIGIN]: REL Z = 0.000.
Retract Z to a safe height. Call the next tool in MDI (for example T02 M06;) and lower it onto the same setter until the dial again reads zero.
Without moving Z, the Z value on the POS → [REL] screen is the length difference between this tool and the reference tool: positive if the tool is longer than the reference, negative if shorter.
On OFFSET/SETTING → [OFFSET] move the cursor to this tool’s H line (H02 for T02), type the value with its sign and press [INPUT]. Many FANUC controls also have the [INP.C.] soft key, which transfers the REL value directly: press the Z address and then [INP.C.].
Repeat steps 3–5 for every other tool. In the program each tool is called with G43 H..; watch the first Z plunge of every tool in single block with the Rapid Override turned down.

Two warnings: (1) In the difference system use G43 only and carry the sign in the H value; switching to G44 for shorter tools is a classic source of errors. (2) On a machine set up with an absolute length system (on-machine tool probe or external presetter) G54 Z means something different; the two systems are never mixed on one machine. Do not enter an H value before you know which system is in use.

36. When is the EXT (common) offset used?

The 00 (EXT) line on the WORK screen is a common shift added to all of G54–G59 at once. Typical use: if every tool is to go 2 mm deeper in Z without touching the part zeros, enter EXT Z = −2; the same line is used to shift a fixture that uses several of G54–G59 as a whole on the table. That is also its risk: a value forgotten in EXT silently shifts all six coordinate systems on the next job. Zero EXT when the job is finished and check line 00 of the WORK screen at every setup.

37. Lesson summary

In this lesson we learned that workholding is fundamental to dimensional accuracy and safety; that good clamping prevents sliding, rotation and lifting; the different roles of vise, parallels, clamps and fixtures; that clamping surfaces must be free of chips and burrs; that the workpiece zero is the origin of the program dimensions; that G54–G59 store different part coordinates; that the edge-finder radius must be accounted for; that the Z zero can be taken from the part or a fixed reference surface; that tools of different lengths are introduced to the control via H offsets; that G43 activates compensation and G49 cancels it; that T–H matching reduces error; that G54 Z and the H offset together determine the tool tip’s real position; that a wrong zero or H value can cause serious collisions; and that the first program should be tried with Single Block and low Rapid Override.

Frequently Asked Questions About Part Zeroing and Tool Length on a CNC Mill

What is a reference tool?

It is the tool with which the Z value of the part zero is taken and against which the lengths of all other tools are measured as differences. Its H offset stays 0; longer tools get a positive H value, shorter tools a negative one. If the reference tool is replaced or re-mounted, the part-zero Z and every difference must be measured again.

What is the difference between MEASURE and INPUT on a FANUC?

INPUT writes the number you typed into the cell as it is; +INPUT adds it to the existing value. MEASURE calculates the offset itself by subtracting the value you typed from the tool's current machine coordinate: with the tool centre over the edge, typing X0. and pressing MEASURE writes the machine X coordinate into G54 X. MEASURE is used when setting the part zero, +INPUT for small corrections during production.

How is the tool radius accounted for when zeroing with an edge finder?

When the edge finder or the tool touches an edge, its centre is one radius away from the edge. On the left edge the edge lies one radius in +X; on the right edge one radius in −X; the sign depends on the edge. The safest practice is to move the tool by one radius so that it sits over the edge and then do X0. MEASURE, or to find the centre by moving to half of the REL difference between two opposite edges, where the diameter cancels out by itself.

When is the tool length difference positive and when negative?

After the reference tool's REL Z has been zeroed, the Z shown on the REL screen when the second tool touches the same surface is the length difference including its sign: if the tool is longer than the reference the spindle stops higher and the value is positive; if shorter, negative. The value is entered on the H line with its sign and only G43 is used in the program. On the first run, watch each tool's first Z plunge in single block.

What is the EXT offset and how does it differ from G54?

EXT (line 00 on the WORK screen) is a common shift added to all of G54–G59 at once; G54 defines only its own coordinate system. If every tool is to go 2 mm deeper in Z, enter EXT Z = −2. EXT must be zeroed when the job is finished; a forgotten EXT value shifts every zero on the next job.

Which tool should I use to set the part zero?

In the difference system, the reference tool: usually a rigid, short, easily touched tool (for example the end mill of the first operation); an edge finder can also be used for X and Y. On a machine set up with an absolute length system, G54 Z is taken relative to the reference defined by the tool probe or presetter. The two systems are never mixed on one machine; do not enter an H or G54 Z value before you know which one is in use.