FANUC Series 30i/300i/300is-MODEL A. Machining Center System. User's manual - page 89

 PROGRAMMING 

B-63944EN/03

 

 

- 668 - 

20. HIGH-SPEED CUTTING 

FUNCTIONS 

 CAUTION 

1  The speed control with the cutting feed is effective 

only when the tool is parallel with the Z-axis.   
Thus, it may not be possible to apply this function, 
depending on the structure of the machine used. 

2  In the speed control with the cutting feed, the travel 

direction on the Z-axis is determined with the 
appropriate NC command.    If, therefore, manual 
intervention is performed on the Z-axis with manual 
absolute on, or if a mirror image is applied on the 
Z-axis, the direction on the Z-axis cannot be 
determined.    When using the speed control with 
the cutting load, do not use these functions. 

3  When performing three-dimensional coordinate 

conversion, determine the descent angle on the 
Z-axis using the converted coordinate system. 

4  Speed control with the cutting load is enabled for 

all interpolations in the AI contour control mode.   
This function, however, can be made valid only for 
linear interpolations by setting bit 4 (ZOL) of 
parameter No. 19503 to 1. 

 

  - Ignoring feedrate commands 

In a block in which AI contour control is enabled, all feedrate 
commands (F commands) can be ignored by setting bit 7 (NOF) of 
parameter No. 8451. 
The term feedrate commands, as used here, refer to the following 
commands: 
 
<1>  Modal F commands before the block in which AI contour control 

is enabled 

<2> F commands and modal F commands in the block in which AI 

contour control is enabled 

 
When the feedrate commands are ignored, it is assumed that the upper 
feedrate limit specified for parameter No. 8465 is specified. 
Note, however, that any issued F commands and modal F commands 
are stored within the CNC. 
Thus, in a block in which AI contour control changes from the 
enabled state to the disabled state, the modal values of the F 
commands described in <1> and <2> described above are used as 
modal F commands, instead of the modal values of the F commands 
calculated by AI contour control. 
 

  - Another example of determining the feedrate 

If a specified feedrate exceeds the upper feedrate limit of AI contour 
control (in parameter No. 8465), the feedrate is clamped at the upper 
feedrate.  The upper feedrate limit is clamped at the maximum 
cutting feedrate (parameter No. 1432). 
 

B-63944EN/03

 PROGRAMMING 

 

 

- 669 - 

20.HIGH-SPEED CUTTING

FUNCTIONS

Limitation 
  - Conditions for temporarily canceling the AI contour control mode 

If one of the commands listed below is issued in the AI contour 
control mode, the AI contour control mode is canceled temporarily. 
If the system becomes ready for AI contour control after it is canceled, 
the AI contour control mode is restored automatically. 

•

  Positioning (rapid traverse) 

•

  Single direction positioning 

•

 Spindle 

positioning 

•

 Rigid 

tapping 

•

  Hypothetical axis interpolation 

•

  Threading (single type, combined type) 

•

  Electronic gear box 

•

 Superimposed 

control 

•

  When no move command is specified 

•

  One-shot G code other than the following: 

Tool offset 
Cutter compensation vector retention 
Cutter compensation corner rounding 
Exact stop 

 

  - Functions that cannot be specified in the AI contour control mode 

In the AI contour control mode, the functions listed below cannot be 
specified.    Before specifying these functions, turn off the AI contour 
control mode; after the command ends, turn on the mode again. 

•

 Threading 

•

 Circular 

threading 

•

  Variable lead threading 

Threading, circular threading, and variable lead threading can be 
specified in the AI contour control mode by setting bit 1 (THA) of 
parameter No. 1611.  However, the AI contour control mode is 
automatically canceled. 
 

Notes

 

  - About processing macro statements

 

In AI contour control mode, the NC statements of multiple blocks are 
looked ahead. Macro statements such as

 

arithmetic expressions and 

conditional branches

 

are processed as soon as they are read into the 

buffer. Therefore, the timing of the macro statement execution is not 
always the specified order. 
In case that you need to execute the macro statement after completing 
the NC block just before the macro statement, specify M code or G 
code that is not buffered just before the macro statement. Specially, in 
case of reading/writing the system variables to control signals, 
coordinates, offset value, etc., it may be different system variable data 
by the timing of the NC statement execution. To avoid this 
phenomenon, specify such M codes or G codes before the macro 
statement, if necessary.

 

 

 PROGRAMMING 

B-63944EN/03

 

 

- 670 - 

20. HIGH-SPEED CUTTING 

FUNCTIONS 

20.2 

MACHINING CONDITION SELECTING FUNCTION 

 

Overview 

By setting a speed- or precision-focused parameter set in an AI 
contour control function and specifying a precision level in 
accordance with the machining conditions during machining, 
parameters suitable to the conditions can be automatically calculated 
so that machining can be performed. 
This function is an optional one. 
 

Format 
  - Changing the precision level using a program 

 
In addition to being switched on the precision level selection screen, 
the precision level can be changed using a program in the format 
below. 
 

G05.1 Q1 Rx ;   

x .......Level (1 to 10) 

 
The precision level can also be changed in the format used with 
conventional "advanced preview control", "high precision contour 
control", and "AI high precision contour control". 
 

G05 P10000 Rx ;   

x .......Level (1 to 10) 

G08 P1 Rx ;   

x .......Level (1 to 10) 

 

 CAUTION 

    Once specified, a level remains effective even if the 

AI contour control mode is canceled. 

 

B-63944EN/03

 PROGRAMMING 

 

 

- 671 - 

20.HIGH-SPEED CUTTING

FUNCTIONS

20.3 

JERK CONTROL 

20.3.1 

Speed Control with Change of Acceleration on Each Axis 

 

Overview 

In portions in which acceleration changes largely, such as a portion 
where a programmed figure changes from a straight line to curve, 
vibration or shock on the machine may occur.  Speed control with 
change of acceleration on each axis is a function to suppress 
machining errors due to vibration and machine shock generated by 
change of acceleration.  This function obtains a feedrate so that 
change of acceleration is within the parameter-set permissible accel-
eration change amount for each axis, and performs deceleration by 
using acceleration/deceleration before interpolation. 
 

 CAUTION 

 

Before speed control with change of acceleration 
on each axis can be used, the options for jerk 
control and AI contour control are required. 

 

Explanation 

In the following example, the Y-axis acceleration changes largely at 
the contact point between a linear interpolation and circular interpo-
lation, so deceleration is performed. 
 

From linear interpolation (N1) to circular interpolation (N2)

Y

X

Vibration due to change

of acceleration

N1

N2

Tangential

feedrate

Y-axis

acceleration

Feedrate

Time

N1

N2

Time

Feedrate

Acceleration

Time

Acceleration

Time

 

 PROGRAMMING 

B-63944EN/03

 

 

- 672 - 

20. HIGH-SPEED CUTTING 

FUNCTIONS 

  - Setting the permissible acceleration change amount 

The permissible acceleration change amount for each axis is set in 
parameter No. 1788.  When 0 is set in this parameter for a certain 
axis, speed control with change of acceleration is not performed for 
that axis. 
 

•

 

Parameter setting example 

Suppose a figure shown below in which a straight line is followed by 
an arc.    Let the specified feedrate and the arc radius be 6000 mm/min 
and 10 mm, respectively.  Then, the Y-axis acceleration change 
amount at the contact point of the linear and arc portions is obtained 
as follows: 

Y

X

Y-axis

acceleration

Acceleration

Time

From straight line to arc

Specified feedrate:  6000 mm/min

Acceleration
change amount:

 1000 mm/s

2

Arc radius:    10 mm

 

 
To suppress the change of acceleration to 300 mm/s

2

, set 300 mm/s

2

 

for the Y-axis in parameter No. 1788. 
Note that the change of acceleration is determined from the 
interpolation data of the CNC, so it may differ from the theoretical 
value. 
The actual machine is affected by acceleration/deceleration and other 
factors, so the value to be set in the parameter should be determined 
after adjustments are made. 
 

2

2

/

1000

s

mm

r

v

=

B-63944EN/03

 PROGRAMMING 

 

 

- 673 - 

20.HIGH-SPEED CUTTING

FUNCTIONS

  - For successive linear interpolations 

When there are successive linear interpolations, speed control with 
change of acceleration obtains the deceleration feedrate from the 
change in acceleration between the start point and end point of a 
specified block. 
When a curve is specified using successive minute straight lines, 
programmed values are rounded to the least input increment before 
issued, so the machining profile is approximated with a broken line.   
The error due to rounding may increase change of acceleration, and 
especially when the line segments specified by blocks are short, 
deceleration is performed frequently.  As a result, the machining 
speed cannot increase enough.  In such a case, a relatively large 
value should be set in parameter No. 1789 as the permissible 
acceleration change amount for each axis in successive linear 
interpolations to improve the machining speed. 
When a value other than 0 is set in parameter No. 1789 for an axis for 
which deceleration with change of acceleration is enabled, this setting 
is regarded as the permissible acceleration change amount at corners 
in which linear interpolations meet.  (For portions where a linear 
interpolation and circular interpolation meet and where circular 
interpolations meet, the setting in parameter No. 1788 is used.) 
When 0 is set in parameter No. 1789 for an axis, the setting in 
parameter No. 1788 specifying the ordinary permissible acceleration 
change amount is used even at a corner in which linear interpolations 
meet. 
When smooth speed control is used in speed control with permissible 
acceleration in AI contour control (named temporarily), the 
deceleration feedrate is obtained from the change of acceleration 
calculated by smooth speed control. 
Therefore, the deceleration feedrate may be higher than the ordinary 
deceleration feedrate. 
 

When linear interpolation is followed
by circular interpolation, speed
control is performed using the
permissible acceleration change

amount set in parameter No. 1788.

Linear
interpolation

Circular
interpolation

For successive linear interpolations,
speed control is performed using the
permissible acceleration change

amount set in parameter No. 1789.

Linear
interpolation

 

 PROGRAMMING 

B-63944EN/03

 

 

- 674 - 

20. HIGH-SPEED CUTTING 

FUNCTIONS 

20.3.2 

Look-Ahead Smooth Bell-Shaped Acceleration/Deceleration 

before Interpolation 

 

Overview 

In look-ahead bell-shaped acceleration/deceleration before interpo-
lation performs smooth acceleration/deceleration by changing the 
acceleration at a constant rate in specified acceleration change time. 
In look-ahead smooth bell-shaped acceleration/deceleration before 
interpolation, the jerk change time is specified in parameter No. 1790 
by using the percentage to the acceleration change time for look-ahead 
bell-shaped acceleration/deceleration before interpolation, and change 
of acceleration is also controlled so that the change is bell-shaped. 
This enables smoother acceleration/deceleration, therefore reducing 
machine vibration and shock due to acceleration/ deceleration. 

 

(Look-ahead bell-shaped 
acceleration/deceleration before interpolation)

(Look-ahead smooth bell-shaped 

acceleration/deceleration before interpolation) 

Time

Tangential feedrate 

Acceleration 

Jerk 

acceleration 

Jerk 

acceleration 

Acceleration change time
Time set in parameter No. 

1772 

Jerk change time 
Time set in parameter No. 
1790 by using the 
percentage to the 

acceleration change time 

Tangential feedrate 

Time

Time

Time

Time

Time

Acceleration

 

 

 CAUTION 

  Before look-ahead smooth bell-shaped acceleration/deceleration before interpolation 

can be used, the option for jerk control and AI contour control II is required. 

B-63944EN/03

 PROGRAMMING 

 

 

- 675 - 

20.HIGH-SPEED CUTTING

FUNCTIONS

Explanation 
  - Setting the jerk change time 

The jerk change time is set in parameter No. 1790 by using the 
percentage to the acceleration change time. 
The actual jerk change time is represented by the percentage to the 
acceleration change time set in parameter No. 1772. 
The jerk change time must be within a half of the acceleration change 
time, so the value to be set in the parameter ranges 0 to 50 (percent). 
If 0 or a value beyond the specifiable range is specified in parameter 
No. 1790, look-ahead smooth bell-shaped acceleration/deceleration 
before interpolation is not enabled. 
 

  - Acceleration/deceleration before interpolation for linear type rapid traverse 

When bell-shaped acceleration/deceleration is used in acceleration/ 
deceleration before interpolation for linear type rapid traverse, 
enabling look-ahead smooth bell-shaped acceleration/deceleration 
before interpolation applies smooth bell-shaped acceleration/decel-
eration to acceleration/deceleration before interpolation for linear type 
rapid traverse. 
In this case, the jerk change time is represented by the percentage set 
in parameter No. 1790 to the acceleration change time set in parameter 
No. 1672. 
 

  - Optimum torque acceleration/deceleration 

When bell-shaped acceleration/deceleration is used in optimum torque 
acceleration/deceleration, enabling look-ahead smooth bell-shaped 
acceleration/deceleration before interpolation applies smooth 
bell-shaped acceleration/deceleration to optimum torque acceleration/ 
deceleration. 
In this case, the jerk change time is represented by the percentage set 
in parameter No. 1790 to the acceleration change time set in parameter 
No. 1672.