FANUC Series 30i/300i/300is-MODEL A. Machining Center System. User's manual - page 59

15.COMPENSATION FUNCTION

PROGRAMMING

B-63944EN/03

- 428 -

Suppose that the workpiece is displaced from the correct workpiece
setting position as with example 1, and set a workpiece setting error in
the same was as in Example 1.
Moreover, add N15,N16,N135 and N136 to O2 as indicated below to
validate the workpiece setting error as in the case of Example 1.

Set bit 0 (RCM) of parameter No. 11200 to 1 to perform tool direction
compensation, then execute O2. When the tool moves to cut each
side of the workpiece with the tool tip, the tool is tilted 45 deg relative
to the +Z direction on the plane normal to the movement direction as
shown in Fig. 15.5 (h).

O2 ;
N10 G55 ;

Set coordinate system

N15 G05.1 Q1

AI contour control mode ON

N16 G54.4 P1

Workpiece setting error compensation mode ON

N20 G90 G00 X0 Y0 Z300.0 B0 C0 ;

Move to initial position

N30 G01 G43.4 H01 Z40.0 F500. ;

Start tool center point control

H01 is tool length compensation number.

N40 X50.0 Y50.0 Z20.0 B45.0 C-90.0 ; Z-axis height of machining plane is 20.0.
N50 X150.0 ;
N60 C0.0 ;
N70 Y150.0 ;
N80 C90.0 ;
N90 X50.0 ;
N100 C180.0 ;
N110 Y50.0 ;
N120 X0 Y0 Z40.0 B0.0 C0.0 ;
N130 G49 Z300.0 ;

Cancel tool length compensation

Move to initial position on Z- axis

N135 G54.4 P0 ;

Workpiece setting error compensation mode OFF

N136 G05.1 Q0 ;

AI contour control mode OFF

N140 M30;

B-63944EN/03

PROGRAMMING

15.COMPENSATION FUNCTION

- 429 -

Fig. 15.5 (h) Operation of tool center point control when there is a workpiece

setting error

Restrictions (general)

Described below is the restriction related to workpiece setting
compensation errors.
Note that, for 5-axis machines of tool rotation or composite type, the
restriction, “Restrictions (only with a 5-axis machine of table rotation
or composite type),” described later, in addition to the above, is
applied.

- Specifiable G codes

When workpiece setting error compensation is enabled, the G codes
listed below can be specified.

G00 Positioning
G01 Linear

interpolation

G04 Dwell
G05.1 Q0/Q1 AI contour control mode OFF/ON
G10

Programmable data input

G11

Programmable data input mode cancel

G17

Plane selection (XY)

G18

Plane selection (ZX)

G19

Plane selection (YZ)

G40 Tool

radius

⋅

tool nose radius compensation / 3-dimensional

cutter compensation cancel

G41.2/G41.4/G41.5 3-dimensional

cutter compensation left (type 1)

(only if also tool center point control is used)

N50

N70

N110

N90

Workpiece setting coordinate system X'Y'Z'

Displaced workpiece.
Operation is performed to
cut four sides.

Workpiece coordinate system XYZ

Correct workpiece
setting position

Workpiece

15.COMPENSATION FUNCTION

PROGRAMMING

B-63944EN/03

- 430 -

G41.6 3-dimensional cutter compensation left (type 2)

(only if also tool center point control is used)

G42.2/G42.4/G42.5 3-dimensional cutter compensation right (type 1)

(only if also tool center point control is used)

G42.6 3-dimensional cutter compensation right (type 2)

(only if also tool center point control is used)

G43

Tool length compensation +

G43.4  Tool center point control (type 1)
G43.5  Tool center point control (type 2)
G49 (G49.1)  Tool length compensation cancel
G53.1  Tool axis direction control
G65

Custom macro call

G66

Custom macro modal call

G67

Custom macro modal call cancel

G68.2 Tilted working plane command

G69 Coordinate system rotation/three-dimensional coordinate

system conversion/tilted working plane command cancel

G90 Absolute

programming

G91 Incremental

programming

G94

Feed per minute

G95

Feed per revolution

G69.1 Coordinate system rotation/three-dimensional coordinate

system conversion/tilted working plane command cancel

G90

Absolute programming (for G code system B and C)

G91

Incremental programming (for G code system B and C)

G94

Feed per minute (for G code system B and C)

G95

Feed per revolution (for G code system B and C)

- Modal G codes usable when workpiece setting error compensation is specified

In a modal G code state listed below, workpiece setting error
compensation can be specified.

G00 Positioning
G01 Linear

interpolation

G13.1 Polar coordinate interpolation mode cancel
G15

Polar coordinate command cancel

G17

Plane selection (XY)

G18

Plane selection (ZX)

G19

Plane selection (YZ)

G21 Metric

input

G23

Stored stroke check function OFF

G25

Spindle speed fluctuation detection OFF

B-63944EN/03

PROGRAMMING

15.COMPENSATION FUNCTION

- 431 -

G40 Tool

radius

⋅

tool nose radius compensation / 3-dimensional

cutter compensation cancel

G49 (G49.1) Tool length compensation cancel
G50 Scaling

cancel

G50.1 Programmable mirror image cancel
G50.2 Polygon turning cancel
G54 to G59, G54.1 Workpiece coordinate system selection
G64 Cutting

mode

G67

Custom macro modal call cancel

G80

Canned cycle cancel

G80.5 (G80.8) Electronic gear box synchronization cancel
G97

Constant surface speed control cancel

G40.1

Normal direction control cancel

G54.2 P0 Rotary table dynamic fixture offset cancel
G69

Coordinate system rotation/three-dimensional coordinate
system conversion/tilted working plane command cancel

G90 Absolute

programming

G91 Incremental

programming

G94

Feed per minute

G95

Feed per revolution

G98

Canned cycle initial level return

G99

Canned cycle R point level return

G69 Mirror image for double turret OFF/balanced cutting mode

cancel

G69.1

Coordinate system rotation/three-dimensional coordinate
system conversion/tilted working plane command cancel

G90  Absolute programming (for G code system B and C)
G91  Incremental programming (for G code system B and C)
G94  Feed per minute (for G code system B and C)
G95  Feed per revolution (for G code system B and C)
G98  Canned cycle initial level return (for G code system B and C)
G99  Canned cycle R point level return (for G code system B and C)

- Manual intervention and handle interruption

In the workpiece setting error compensation mode, do not perform
manual intervention and handle interruption.

- Positioning in the machine coordinate system

In the workpiece setting error compensation mode, do not perform
positioning in the machine coordinate system (such as G28, G30, or
G53 command).

15.COMPENSATION FUNCTION

PROGRAMMING

B-63944EN/03

- 432 -

- Rapid traverse command

When using workpiece setting error compensation, specify linear
rapid traverse (by setting set bit 1 (LRP) of parameter No. 1401 to 1).

- Relationships with other modal commands

The commands for the functions listed below must be nested with a
workpiece setting error compensation command and must be placed
between G54.4 P_ and G54.4 P0.
Namely, specify G54.4 P_ when the mode of a desired function below
is off. Next, turn on then off the mode of the function, then specify
G54.4 P0.

•

Cutter compensation (G40, G41.2, G41.4, G41.5, G41.6, G42.2,
G42.4, G42.5, G42.6)

•

Tool length compensation (G43, G43.4, G43.5, G49)

•

Tilted working plane command (G68.2, G69)

- PMC axis control

In the workpiece setting error compensation mode, do not perform
PMC axis control to the axes which are for workpiece setting error
compensation.

- Movement of start-up and cancel of Tool length offset

To perform tool length compensation (including tool center point
control) in the workpiece setting error compensation mode, set bit 6
(TOS) of parameter No. 5006 to 1 (perform tool length compensation
by shifting a coordinate system). If parameter TOS = 0, alarm
PS0438 is issued.

- Mirror image

Do not use programmable mirror imaging or external mirror imaging
(based on a mirror image signal or setting) during workpiece setting
error compensation.

- Stroke limit check before movement

In the mode of Workpiece setting error compensation, Stroke limit

check before movement is not available.

B-63944EN/03

PROGRAMMING

15.COMPENSATION FUNCTION

- 433 -

- Feedrate override

When tool direction is compensated (bit 0 (RCM) of parameter

No.11200=1), the rotation axis compensation is performed to the
movement which is modified by the override signals. If a large
movement of rotary axis occurs for the compensation, the feedrate of
the rotary axis is clamped by the speed which is generated by
calculation that the parameters No.11202,No.11203 override the
maximum cutting feedrate/rapid traverse.

While rotary axes move with this override, even when the override

signals change, the actual feedrate may not change, and, even when
feed hold or the like is done, the actual rotary axes movements may
not stop immediately because automatic operation stops after the
movement caused by rotation axis compensation has been completed.

WARNING

Rotation axis compensation near a singular point
causes a rotation axis to move largely, thus
resulting in a symptom that it is impossible to
change override or to reset feed hold during the
axis movement being likely to occur. If it is
necessary to stop the axis immediately during this
symptom, use the emergency stop function.

- In the case that Tool posture control is used with Type-2 of Tool center point

control

In the case that Tool posture control is used with Type-2 of Tool
center point control, when the angle between a tool posture and the
singular posture is less than the parameter No.19738, the tool posture
at the end of the block is changed so that the tool posture passes the
singular posture.
But, when tool direction is compensated (bit 0 (RCM) of parameter
No.11200 = 1), the tool posture may not pass the singular posture
because of the compensation after tool posture control.

- Distance-to-go display

The distance-to-go display is one before workpiece setting error
compensation is performed.
It is not the actual machine’s distance to go.

- Program restart

Do not restart a program if workpiece setting error compensation is
being performed for it.

15.COMPENSATION FUNCTION

PROGRAMMING

B-63944EN/03

- 434 -

- Reset

To cancel the workpiece setting error compensation mode, be sure to
use a reset by resetting bit 2 (D3R) of parameter No. 5400 to 0.
Performing tool length compensation (including tool center point
control) in the workpiece setting error compensation mode causes the
tool length compensation mode and tool length compensation vector
to be canceled by a reset no matter what the setting of the following
parameters:

•

Bit 6 (CLR) of parameter No.3402

•

Bit 0 (C08) of parameter No.3407

•

Bit 6 (LVK) of parameter No.5003

- Setting not involving tool direction compensation

For 5-axis machines, be sure to select tool direction compensation (set
bit 0 (RCM) of parameter No. 11200 to 1).
For machines other than 5-axis machines, workpiece setting error
compensation is carried out with no tool direction compensation
selected (bit 0 (RCM) of parameter No. 11200 is 0).  However, do
not specify rotation errors other than those about the tool direction.
Otherwise, machining will not be performed properly.  (Example:
If the tool is in the Z direction, do not specify rotation errors about the
X- or Y-axis.

- Synchronous slave axis absolute coordinates

If feed axis synchronization is in effect, no slave axis absolute
coordinate is displayed properly.

- Workpiece coordinate system shift

Do not perform workpiece setting error compensation with G52 (local
coordinate system setting) or G92/G50 (T series) (workpiece
coordinate system shift) executed.
Once the workpiece coordinate system has been shifted, preset it using
G92.1 or axis-specific workpiece coordinate system preset functions
before starting workpiece setting error compensation.

Canned cycle

In the workpiece setting error compensation mode, do not carry out
canned cycles.

Restrictions (only with a 5-axis machine of table rotation or composite type)

For 5-axis machines of table rotation or composite type in particular,
this restriction, in addition to "Restrictions (general)" above, is
applied.

- Hypothetical axis used for a table rotation axis

If a hypothetical axis is used as a table rotation axis, compensation is
performed with the angle of the table rotation axis set to 0 degree.

B-63944EN/03

PROGRAMMING

15.COMPENSATION FUNCTION

- 435 -

- Acceleration/deceleration at a corner

When a command for linear interpolation is specified, linear
interpolation is performed as viewed from the workpiece on the table.
So, even when the command specifies a linear interpolation, the
control point may make a curved motion. This means that a corner
operation may be performed with some commands.

So, if a small value is set as an allowable feedrate difference
(parameter No. 1783) or as an allowable acceleration/deceleration rate
(parameter No. 1660 and No. 1737) for a corner, the tool may be
decelerated.

- G codes that must not be specified

Among the "Specifiable G codes" in "Restrictions (general)" above,
the G codes listed below must not be specified when tool direction
compensation is performed with a 5-axis machine of table rotation
type or composite type.

G95 Feed per revolution

G95 Feed per revolution (for G code system B and C)

- Modal G codes not usable when workpiece setting error compensation is

specified

Among the "Modal G codes usable when workpiece setting error
compensation is specified" in "Restrictions (general)" above, the G
codes listed below must not be specified with a 5-axis machine of
table rotation type or composite type in the modal G code state
indicated below.

G95 Feed per revolution

G95 Feed per revolution (for G code system B and C)

- Command for an axis not related to 5-axis machining

Those axes that are not related to 5-axis machining must not be
specified. Otherwise, alarm PS0439 is issued.

Content .. 57 58 59 60 ..