FANUC Offset Systems: Lathe Geometry/Wear and Milling H, D, G54-G59

Estimated reading time: 7 minutes

What Will You Learn in This Lesson?

In this lesson you will examine the offset screens on a FANUC control through two different machine types.

On a FANUC lathe

Geometry Offset
Wear Offset
X and Z tool values
The tool measuring screen
Tool nose radius and orientation data

On a FANUC milling machine / vertical machining centre

Tool Length Offset
Cutter Radius Offset
H and D numbers
G54-G59 Work Offset screens
MEASURE and data entry methods

The aim is not to teach tool selection or metal cutting theory, but to show where the offset data is held on a FANUC control, how it is entered and how it is checked.

What Is an Offset?

A CNC program cannot know by itself the real length of the tool or the position where it is mounted. The FANUC control uses offset tables to relate the programmed coordinates to the real tool and workpiece positions.

In general, offsets carry the following information:

The measured position of the tool
The tool length or radius
Small wear corrections on the tool
The place of the workpiece zero in the machine coordinate
On a lathe, the tool nose radius and the nose orientation

A wrong offset number or value can cause the tool to move to the wrong position even if the program is correct.

Caution: although changing an offset does not produce a real axis movement, it can change the target of the next program movement. Every value entered should be verified before the program is run.

Reaching the Offset Screen

On FANUC controls the offset screen is mostly reached with one of the following function keys:

OFFSET/SETTING
OFFSET SETTING
OFS/SET
OFFSET

The relevant table is then selected with the soft keys at the bottom of the screen.

On a lathe control, for example:

GEOM
WEAR
OFFSET
WORK
SETTING

On a milling control:

OFFSET
TOOL OFFSET
GEOM
WEAR
WORK
MACRO
SETTING

options such as these may be seen.

The Offset System on a FANUC Lathe

On a FANUC lathe control the position of the tool in each turret station is different. The Geometry Offset table carries these basic differences, while the Wear Offset table carries the small corrections needed during use.

Geometry Offset

The Geometry Offset is the main tool value that tells the control the real position of the tool in the turret.

The table generally has the following columns:

X
Z
On some machines Y
Tool nose radius R
Imaginary tool nose orientation T

Each row corresponds to an offset number:

Offset	X	Z	R	T
01	Measured value	Measured value	Nose radius	Nose orientation
02	Measured value	Measured value	Nose radius	Nose orientation

These values show an example structure; the real values are different for every machine and tool setup.

A large value in the Geometry table should not automatically be considered wrong. The value depends on the tool measuring and coordinate creation method of the machine.

Wear Offset

The Wear Offset is used to make small corrections without changing the Geometry value.

For example, if the measured part size deviates slightly from the target value, an authorised operator can make a small correction in the X or Z wear offset.

The advantage of the Wear screen is this:

The main tool geometry is preserved.
The correction made can be seen separately.
The amount of the correction can be followed.
When a new tool is fitted, the wear value can be zeroed in a controlled way.

Common mistake: constantly changing the Geometry value for a small dimensional correction. Geometry should be used as the basic tool definition and Wear as the small working correction.

The direction of the X correction

Whether an X correction on a lathe makes the part larger or smaller should be evaluated according to:

whether the operation is external or internal diameter,
the orientation of the tool,
the axis arrangement of the machine,
whether the X value is processed as a diameter or as a radius.

For this reason a single rule of thumb such as “a positive value always makes the part larger” should not be used. A small correction should be entered, the value read again, and the first part measured under control.

The Relationship Between Tool and Offset Number

A common way of calling a tool on FANUC lathes is as follows:

T0101

In the common interpretation:

the first two digits indicate the turret station,
the last two digits indicate the offset number.

Accordingly, T0101 may match tool station 1 with offset number 1.

However, the digit structure of the T code and the turret behaviour can be determined by the machine tool builder. Some machines use more digits or a different tool-offset pairing.

The operator should check three items together:

The tool physically present in the turret
The T code called in the program
The offset row in the Geometry and Wear tables

The Tool Measuring Screen on a Lathe

During tool measuring, the aim is to tell the Geometry table the relationship of the tool nose to a known part or measuring point.

The general control logic is as follows:

The correct tool is called safely.
A low step is selected in HANDLE mode.
The tool is brought up to the known surface according to the authorised measuring method.
The relevant Geometry offset row is selected.
The known X or Z value is typed.
MEASURE or the measuring soft key of the machine is used.
The calculated offset value is checked.
The tool is withdrawn to a safe position.
The X and Z measurements are verified separately.

For example, if the tool has been brought into contact with a known outside diameter, the real diameter value can be entered in the X field and MEASURE used, according to the measuring procedure of the control. If the face of the part is taken as Z zero, Z0 can be measured with the relevant procedure.

This explanation shows only the control logic. The contact method, the tool probe, the gauge, the part surface and the soft keys used may differ from machine to machine.

Caution: tool measuring should only be carried out by people with training and authorisation to operate the machine. A low HANDLE step should be used while the tool is close to the part; the wrong axis, the wrong direction and the wrong offset row should be checked.

Tool Nose Radius and Nose Orientation

The Geometry table of a turning tool may contain more than just the X and Z values. For tool nose radius compensation the following data is generally also needed:

R: the tool nose radius
T: the imaginary tool nose orientation number

This data helps the control to evaluate the tool path correctly when tool nose radius compensation is used in the program. On a lathe this compensation is activated with G41 and G42 and cancelled with G40.

The operator should check the following:

Is the radius value consistent with the insert being used?
Is the nose orientation suitable for the real mounting orientation of the tool in the turret?
Is the correct offset row active?
Is there an unexpected value in the Geometry and Wear tables?

A wrong nose orientation can produce an unexpected tool path, particularly on tapered and curved profiles.

The Offset System on a FANUC Milling Machine / Machining Centre

On milling machines and machining centres, the tool offsets and the workpiece coordinates are managed in separate tables.

The basic distinction is as follows:

Tool Length Offset: the tool length
Cutter Radius Offset: the tool radius or a value related to the diameter
Work Offset: the place of the workpiece zero in the machine coordinate

Tool Length Offset and the H Number

The Tool Length Offset allows tools of different lengths to be used within the same program coordinate system.

In the program the tool length offset is mostly called with an H number:

G43 H01

Here H01 selects length offset number 1 in the tool offset table.

Having the H number the same as the tool number is a common arrangement:

T01 M06
G43 H01

However, this equality is not a compulsory FANUC rule. A different H number can be called in the program. For this reason the operator should not look only at the active tool number, but should also check the H address in the program.

Depending on the control type, the Tool Length Offset screen may contain:

a single offset value,
Geometry and Wear columns,
Length Geometry and Length Wear fields.

The main measurement can be held in the Geometry field and, if present, the small corrections in the Wear field.

Measuring the Tool Length

The tool length offset can be determined by different methods such as:

contact with a reference surface,
a tool setting gauge,
a tool measuring probe on the machine,
an external tool presetter.

The general procedure on the FANUC screen:

The correct tool is called.
The correct H offset row is selected.
The tool is measured according to the authorised measuring method.
The calculated or measured value is entered.
If necessary the MEASURE soft key is used.
The sign of the entered value and the row number are checked.

The sign and reference logic of the tool length value may change according to the measuring method used. Copying a value from another machine directly is not correct.

Cutter Radius Offset and the D Number

The Cutter Radius Offset holds the cutter compensation value used by the program. In the program it is mostly called with the D address:

G41 D01

or:

G42 D01

Here D01 selects radius offset number 1 in the offset table.

Depending on the control and the working practice, the D field may hold:

the tool radius,
the tool diameter,
only a small correction value.

It should not be assumed whether the value in the table is a diameter or a radius without knowing the programming method.

The H and D addresses have different tasks:

H: generally the tool length offset
D: generally the cutter radius offset

Common mistake: thinking that the control will automatically use H01 and D01 because T01 has been called. The active offset is determined by the H and D addresses in the program.

Cancelling Compensation: G49 and G40

Cancelling compensation in the right place is as important as activating it.

G49: cancels tool length compensation (G43 / G44).
G40: cancels cutter radius compensation (G41 / G42).

If the machine moves to the tool change position or to the end of the program without the compensation being cancelled, the control still takes the active offset value into account and the tool may travel to an unexpected point. This is one of the most common causes of collision in milling programs.

The operator should check the following in the program:

Is every G43 H call cancelled with G49 in the right place?
Is every G41 or G42 D call cancelled with G40?
Have the compensations been cancelled before the tool change?
Is the compensation state known at the end of the program?

Caution: on some machines the compensations may be cancelled automatically by the control during a tool change or at M30. This behaviour depends on the configuration of the machine tool builder and should not be assumed.

G54-G59 Work Offset Screens

The Work Offset screen defines the place of the workpiece coordinate systems on the machine.

As standard, the following coordinate systems may be seen:

Each row mostly contains X, Y and Z values. On machines with a fourth axis there may also be an A, B or C column.

An example screen structure:

System	X	Y	Z
G54	Work zero value	Work zero value	Work zero value
G55	Second setup	Second setup	Second setup
G56	Third setup	Third setup	Third setup

If G54 is active in the program, the control uses the values in the G54 row. Even if the operator has entered the correct values into G55, they are not used while the program calls G54.

Entering a Work Offset Value

The workpiece zero can be determined by one of the following methods:

An edge finder or a dial indicator
A gauge
A probe
A known fixture position
Previously prepared job setup data

The general procedure on the FANUC control:

The OFFSET/SETTING screen is opened.
The WORK page is selected.
The G54-G59 row to be used in the program is determined.
The relevant X, Y or Z field is reached.
The calculated value is entered or the appropriate MEASURE operation is used.
The value and its sign are checked again.
It is compared with the active coordinate system in the program.

The INPUT, +INPUT and MEASURE options do not have the same task:

INPUT can write the value directly into the selected field.
+INPUT can add the entered amount to the existing value.
MEASURE can calculate the offset from the current position and the dimension typed.

The exact behaviour may change according to the screen type and the FANUC series. In particular, before using +INPUT it should be understood that the existing value is kept and the amount added on top of it.

Caution: when a G54-G59 value is changed, the physical axis does not move; however, the next target position of the program changes. After the change, the graphics, the position screen and a controlled program trial should be used.

A Safe Checklist When Entering Offsets

The following should be checked before and after an offset value is entered:

Are you on the screen of the correct machine type?
Is the correct tool or Work Offset row selected?
Is Geometry or Wear being changed?
Does the H or D number match the program?
Is the G54-G59 selection the same as in the program?
Has the correct axis column been selected?
Are the decimal point and the unit of the value correct?
Is the sign of the value correct?
Which of INPUT, +INPUT or MEASURE will be used?
Was the old value recorded before the change?
Is the new value of a reasonable magnitude?
Will the program be tried again under control?

FANUC Note

The Geometry/Wear structure is common on lathe controls such as FANUC 0-TC and 0i-TC; the H/D and Work Offset structure is common on milling controls such as FANUC 0-M, 0i-MB and 0i-MF. On newer controls Geometry and Wear may be in separate columns, and on older controls on separate pages.

The layout of the offset screen, the way tools are called, the MEASURE operation and the tool measuring functions may differ according to the FANUC series, the available options and the machine tool builder.

Short Summary

Offsets relate the program coordinates to the real tool and workpiece positions.
On a lathe, Geometry carries the basic tool position and Wear the small corrections.
Lathe offsets may contain X, Z, nose radius and nose orientation data.
The T0101 form is common, but the tool-offset structure may differ from machine to machine.
On a milling machine the H number mostly selects the tool length offset.
The D number mostly selects the cutter radius offset.
It is not compulsory for the tool number and the H or D number to be the same.
The G54-G59 tables hold the workpiece coordinate systems.
INPUT, +INPUT and MEASURE are not the same operation.
Changing an offset can change the target of the next tool movement.

Test Yourself

What is the difference between the Geometry Offset and the Wear Offset?
What data do the R and T fields carry on a lathe?
What is the common tool-offset interpretation of the T0101 code?
Why does a positive X correction on a lathe not give the same result in every case?
What are the general tasks of the H and D addresses on a milling machine?
When T01 is called, can it be assumed that H01 will be used automatically?
Do G54 and G55 use the same work zero at the same time?
Why does the machine not move immediately when a Work Offset is changed?
What is the basic difference between INPUT and +INPUT?
Why should the program be tried under control after an offset change?