13.

Sample Programming [Advanced]

13.1 Tool Position Offset ................................................................................................................................. 13-3
13.1.1 Examples of offset specification ........................................................................................................ 13-4
13.2 Bar Feed Program Enable/Terminate (M08, M09) .................................................................................. 13-7
13.3 Bar Feed (M54, M55) .............................................................................................................................. 13-8
13.4 Automatic Bar Feeder ............................................................................................................................. 13-9
13.4.1 M108 (Material change using an argument) ...................................................................................... 13-9
13.4.2 General-purpose material change program (by user program) ....................................................... 13-15
13.5 Subprogram (M98) ................................................................................................................................ 13-16
13.5.1 Subprogram call instruction ............................................................................................................. 13-16
13.5.2 Calling a subprogram from the main program ................................................................................. 13-16
13.5.3 Example of using a subprogram ...................................................................................................... 13-17
13.6 Spindle Speed Change Detection Function (M94, M95, M96, M97) ..................................................... 13-19
13.7 Constant Surface Speed Control (G96, G97)........................................................................................ 13-20
13.8 Tool Nose Radius Compensation Function ........................................................................................... 13-22
13.8.1 Tools subject to tool nose radius compensation and virtual tool nose numbers .............................. 13-23
13.8.2 Basic pattern of tool nose radius compensation G code ................................................................. 13-24
13.9 Cut-off Tool Breakage Detection (M51) ................................................................................................. 13-27
13.10 Corner Chamfering / Corner Rounding ................................................................................................. 13-30
13.11 Thread Cutting (Equal Pitch Thread Cutting and Continuous Thread Cutting) (G32) ........................... 13-32
13.12 Longitudinal Cut-Off Cycle (G75) .......................................................................................................... 13-34
13.13 Deep Hole Drilling Cycle 2 (G79, G80) ................................................................................................. 13-36
13.14 Synchronized Tapping Functions (G88, G84, G80) .............................................................................. 13-38
13.14.1 Synchronized tapping for outer circumference with a rotary tool (G88 and G80) ............................ 13-38
13.14.2 Synchronized tapping for the end face of a workpiece with a rotary tool (G84, G80) ................... 13-41
13.14.3 Synchronized tapping for the center of the end face of a workpiece (main or back) (G84, G80) .. 13-43
13.14.4 Continuously synchronized tapping ................................................................................................. 13-45
13.15 Arc Threading (G35, G36) .................................................................................................................... 13-47
13.16 Differential Rotary Tool Function (G164) ............................................................................................... 13-49
13.17 Canned Cycle Longitudinal Machining (G90)........................................................................................ 13-52
13.18 Thread Cycle Canned Cycle (G92) ....................................................................................................... 13-55
13.19 Link-Thread Machining ......................................................................................................................... 13-59
13.20 Multi-thread Screw Cutting.................................................................................................................... 13-62
13.21 Machine Coordinate System Command (G53) ..................................................................................... 13-64
13.22 Y-axis Holder......................................................................................................................................... 13-65
13.23 Multi-piece Machining ........................................................................................................................... 13-67
13.24 Rapid Feed Acceleration/Deceleration Time Constant Setting ON/OFF (M360/M361) ......................... 13-69
13.25 Medium-pressure Coolant Device ......................................................................................................... 13-71
13.26 Rapid Feed Rate Setting ON/OFF (M350/M351) .................................................................................. 13-72
13.27 Cutting Start Interlock Enabled/Disabled (M86, M87) ........................................................................... 13-73
13.28 Error Detect ON/OFF (M92, M93) ......................................................................................................... 13-74
13.29 Start Position Queuing (Type 1) (G115) ................................................................................................ 13-75
13.30 Start Position Queuing (Type 2) (G116) ................................................................................................ 13-76
13.31 Auxiliary Function Output during Axis Feed (G117) .............................................................................. 13-77

13-1
 13.32 Arbitrary Axis Change (G140) ............................................................................................................... 13-78
13.33 End Position Specified Queuing (G149) ............................................................................................... 13-79
13.34 Arbitrary Axes Superimposition (G156) ................................................................................................. 13-80
13.35 Line Angle Command ........................................................................................................................... 13-83
13.36 Geometric Command ............................................................................................................................ 13-85
13.37 Free Tool Layout Pattern (Holder Name = Free Tool) ........................................................................... 13-86
13.38 Custom Macro Program (Program Call by G code) .............................................................................. 13-87
13.39 DPRINT Function (POPEN, PCLOS, BPRNT, DPRNT) ........................................................................ 13-88
13.40 Running the Program in External Memory ............................................................................................ 13-89
13.41 Collision Detection Function ................................................................................................................. 13-90
13.42 Optional Block Skip ............................................................................................................................... 13-91
13.42.1 Expansion of the optional block skip function .................................................................................. 13-91
13.42.2 Optional block skip M code (M238) ................................................................................................. 13-93
13.43 Thermal Displacement Correction Function .......................................................................................... 13-95
13.43.1 Environmental requirements and restrictions on use....................................................................... 13-95
13.43.2 Setting thermal displacement correction function ............................................................................ 13-96
13.44 B Code Function (MB) .......................................................................................................................... 13-97
13.45 Simultaneous Machining ....................................................................................................................... 13-98
13.45.1 Simultaneous machining for outer and inner diameters .................................................................. 13-98
13.45.2 Pinch Milling .................................................................................................................................. 13-101
13.45.3 Pinch Turning ................................................................................................................................ 13-102
13.46 Major restrictions of tooling setup ....................................................................................................... 13-103

13-2
 L220E

13.1 Tool Position Offset

This function compensates for the difference between actually machined dimensions and dimensions on the drawing.
Coordinates on the program need not be changed. If a difference is entered in advance, dimensions are automatically
corrected. Before this automatic correction can be made, an instrument for giving the difference must be provided.

[Command format]
Tool selection and offset specification at the same time: T (4 digits)
When only compensation value is given after tool selection: T (2 digits)

Description
 An offset command T is given with a two-digit number.
 T (4 digits):
Tool selection and offset specification (only for the diameter direction) are given at the same time.
The first two digits are a tool number and the last two digits are an offset number.
 T (2 digits):
When the tool has already been selected, this format is used to give or change an offset value without
changing the tool. (Generally, the two-digit format is used.)
 Actual offset values are entered by the machine operator. The programmer gives offset numbers at places where
coordinate correction seems necessary on the program. Generally, the following positions require an offset:
 At the time of tool selection and positioning
 At each step
 At the beginning of longitudinal feed for end-face drilling or tapping
 The current offset remains in effect until the next tool selection command or another tool offset command comes.
 Any offset can be canceled by a T00. Cancellation is needed when:
 The machine returns to the start point because cutting-off is completed.
 The machine returns in the longitudinal direction after end-face drilling or tapping.
 Offset values are modal.
 The available offset numbers are 01 to 40. 41 through 80 are optional.
 When a T (4-digit) command is given, the machine moves to the position calculated with the offset value
included (only in the diameter direction).
If a T (2-digit) command is given, the offset will be in effect when the next X and Z command
is given.

13-3
L220E

13.1.1 Examples of offset specification

Outer diameter machining
Outline of machining

Guide bushing

(6.0 0.02)

( 0.02)
8.0

10.0
C0.5
C0.5
15 7

[Sample program]
N0112 T0200
An offset command is given in a block which brings the tool close to the
G00 X4.0 Z–0.5 T01 ...............................
workpiece at the rapid feed rate.
(an offset for the dimension of a 6.0 mm diameter).
G01 X6.0 Z0.5 F0.03
Z15.0
If steps are involved, an offset is specified for each step.
X7.0 T02 .................................................
(an offset for the dimension of an 8.0 mm diameter)
X8.0 Z15.5
Z22.0

[Note]
Assumes that offset values of T01 and T02 on Z axis are the same.
If not, chamfering angle of the next block may get out of position. In some cases, it is required to enter the offset value
of T02 in the preceding block, and add Z-axis offset T03 in the block containing Z22.0.

13-4
 L220E

Face drilling (with a drill or tap)

Outline of machining

0.5
Guide bushing

15

[Sample program]
N0323 T2300
G00 Z–0.5
Specifies offset value to correct the drill depth.
G01 Z15.0 F0.08 T13 .............................
Offset cancel (required at the time of return)
G00 Z–0.5 T00 .......................................

13-5
L220E

Cutting-off
Outline of machining
Guide bushing

20

[Sample program]
N0401 T0100
The product length is decided by the Z axis direction offset.
G00 X21.0 Z22.0 T01 .............................
G650
!2 L1
G01 X–3.0 F0.02
G600
M05
M07
Offset cancel.
G00 X–3.0 Z0 T00 ..................................
Always specify this command when returning the spindle to the start
position.
If it is not specified, the position in the longitudinal direction will shift in
every workpiece separation, and it finally causes a Z axis over-travel error.
M56
G999
N999
M02
%

13-6
 L220E

13.2 Bar Feed Program Enable/Terminate (M08, M09)

These codes enable and terminate a bar changing program. The commands in the block (= bar changing program)
enclosed between M08 and M09 are executed when the material shortage signal is received. They are otherwise
skipped. (A block skip symbol "/" is used.)
The bar changing program is inserted between the cut-off and end processes.

[Command format]
Bar feed program enable/terminate
M08 Enable the bar changing program
M09 Terminate the bar changing program

[Sample program]

:
G113 ........................................... Spindle synchronization cancel
M08 ............................................. Enable the bar changing program
M08
/( ) ...........................................
/( ) ........................................... Program for removing burr from the outer diameter of the material
/( ) ...........................................
/ G01 X33.0 W–25.0 F0.2 .... Move the cut-off tool by the material outer diameter + 1 mm upon extracting the
material from the guide bushing
/ M53 ........................................... Turn off coolant supply
/ M05 ........................................... Stop rotating the main spindle
/ M54 ........................................... Stop the machining torque of the bar loader
/ M07 ........................................... Open the spindle chuck
/ M55 ........................................... Issue the material replace command (to start replacing the material on the bar
loader)
/ M06 ........................................... Close the spindle chuck
/ G4 U2.0 ................................... Prevent bar loader torque switch time delay
/ M52 ........................................... Turn on coolant supply
/ M03 S1= ..................... Rotate the main spindle forward
/ G04 U2.0 ................................ Time for regulating the main spindle speed
/ W25.0 F0.2 ............................ Insert a material in the guide bushing
/ X–4.0 F0.02 ........................... Shortcut the tip of material
M09 .............................................. Terminate the bar changing program

[Note]
 The M08 and M09 codes can be specified for both axis control groups.
 While synchronizing with the main spindle, be sure to specify G113 to cancel the spindle synchronization mode
before executing bar change.

13-7
L220E

13.3 Bar Feed (M54, M55)

These codes are used to operate the bar loader.

[Command format]
Bar feed
M54 Turn off the bar loader torque
M55 Start the bar loader

The bar loader performs the following operations:

Actions of M55 (Synchronous bar loader)

Open the stabilizer.

Move the pushrod to the material extract position.

Turn on the material clamp.

Move the pushrod to the material extract position (= return position). Extract a remaining material

Turn off the material clamp.

Turn on the material clamp.

Detect any material remaining
Turn off the material clamp.

Turn on the shelf material motor to move the rail backward. Feed a shelf material.

Move the pushrod to the primary feed position.

Move the pushrod to the return position.

Turn on the shelf material motor to move the rail forward. Insert a material.

Turn on the material clamp.

Move the pushrod to the material insert position.

Turn off the material clamp.

Move the pushrod to the shortcut position. Feed a material.

Close the stabilizer.

13-8
 L220E

13.4 Automatic Bar Feeder

When removing the residual material or supplying material using the automatic bar feeder unit, the following process
must be inserted between the cut-off process and the ending process.
13.4.1 M108 (Material change using an argument)
Using an argument with the M code allows you to change material without writing program.

[Command format]
M108 U C D B S W F A R1 K1 M1 T

U Movement of the X axis for deburring (in mm dia.). With no argument specified, this point is set
at the point "Tool Positioning Point (DIA)" in the machining data. Do no omit the decimal point.
C Feedrate to position the deburring point (mm/min). With no argument specified, the feedrate is
150.0 mm/min. Do not omit the decimal point.
D Movement of Z axis for deburring (mm). With no argument specified, deburring is not performed.
B Movement of X axis for deburring (in mm dia.). With no argument specified, deburring is not
performed.
S Spindle speed at withdrawing the residual material and inserting the material (min –1). With no
argument specified, the spindle speed is 300 min–1. If the specified value exceeds 2000 min –1, the
spindle speed is clamped at 2000 min–1.
W Movement of spindle at withdrawing the residual material and inserting the material (mm). With
no argument specified, movement is 30.0mm.
F Feed rate (per minute) of the headstock (Z1 axis) when withdrawing the residual material and
inserting the material. With no argument specified, feed rate is 3000.0 mm/min. Do not omit the
decimal point.
A Dwell time after the spindle is chucked (second). With no argument specified, the dwell time is 2
seconds.
R1 Specify this argument to rotate the spindle during changing material.
Omitted: The spindle stops.
1: The spindle rotates.
K1 Specify this argument to stop supplying coolant before unloading the material.
When omitted, the supplying coolant is stopped.
T Dwell time (second) after tuning the coolant on. With no argument specified, the dwell time is 3.0
seconds. Do not omit the decimal point.
I This is a CAV specific argument.
During inching of non-conformed materials, adjust the torque value (%) to suit the type of
material and its diameter. For details, refer to the CAV instruction manual.

13-9
L220E

[Sample program 1]
All arguments necessary are input.
Preparation process
M09
↓
Machining Process
↓
T0100
G00 X Z T
G650
!2 L1
G01 X–3.0 F0.02
G600
M08
M08
/M108 U1.0 C150.0 D1.5 B3.0 S800 W30.0 F3000.0 A3.0 R1 K1 M1 T3.0
M09
M05
M07
G00 X–3.0 Z0 T00
M56
%

[Sample program 2]
Chamfering of residual material is not performed.
M108 S800 W30.0 F3000.0 A3.0 R1 T3.0

13-10
 L220E

M108 Material Change Flow

1. The material shortage signal is issued from the bar feeder unit.
2. Cutting-off process is terminated at cutting-off end position in the machining data. ...Fig. (a)
3. Read the program Material Exchange (M108).
4. The spindle rotates at the "Cut-off Speed" in the machining data.
5. The tool moves to the "Bar Stock O.D." (machining data) + "U argument value" position at the feed rate
specified by the C argument. ... Fig. (b)
6. The Z axis advances by the distance specified by the D argument. ... Fig. (c)
7. The residual material is chamfered according to the values specified by the D and B arguments at the "Cut-off
Feed" in the machining data. ... Fig. (d)
8. If the K1 argument is omitted, Coolant OFF and Stop Medium-pressure Coolant Pump commands are issued.
9. The spindle speed is changed to the speed specified by the S argument.
10. The "Tool Positioning Point" in the machining data is shifted by the value specified by the W argument and at
the same time the residual material is withdrawn from the guide bushing at the feed rate specified by the F
argument. ... Fig. (e)
11. The spindle stops or keeps rotating according to the setting at the R argument.
12. Feed torque of the bar loader is turned off.
13. The main spindle chuck opens.
14. Bar stock is exchanged.
(The residual material is brought to the retraction end of the bar loader and withdrawn by the finger chuck. The
new bar stock is taken from the rack and inserted into the finger chuck. The bar loader pushes the bar stock up to
the position set at the bar loader.) The bar stock exchange completed signal is returned from the bar loader to the
machine.
15. The main spindle chuck closes.
16. The machine dwells for the period specified by the A argument.
17. The main spindle rotates at the speed specified by the S argument.
18. If the M1 argument is specified, phase adjustment of guide bushing is performed.
19. The bar stock is inserted into the guide bushing by the amount specified by the W argument. The bar stock is
then fed forward by the front end cut length at the feed rate specified by the F argument.
20. Specify (Coolant ON) and Stop Medium-pressure Coolant Pump commands.
21. The machine dwells for the period specified by the T argument.
22. The spindle speed is changed to the speed specified at the "Cut-Off Speed" in the machining data.
23. Cutting-off is performed up to the position specified at "Cut-Off End" in the machining data at the feed rate
specified at "Cut-Off Feed" in the machining data.
24. The Material Change OFF M code is read.
25. The M108 program ends.
[Note]
 When material change is specified according to Sample program 1, all steps from step 3 to step 25 are performed.
 When material change is specified according to Sample program 2, steps are performed from step 3 to step 25
omitting steps 4 to 7.
 Chamfering of the residual material is not performed unless arguments D and B are specified.
 Specify the material change operation (M108) in axis control group 1 ($1).
 In the material change operation (M108) commands, if "rotate (1)" is specified by spindle rotation selection (R
argument), the spindle speed is clamped at 2000 min–1 when a value larger than 2000 min–1 is specified for the
spindle speed (S argument) to be applied to residual material withdrawal and new bar stock insertion operation.

13-11
L220E

Material change flow

Material change flow when cutting-off procedure is complete, change material using an automatic bar feeder is
performed in the following sequence illustrated. Chamfering of residual material can be performed as needed.

G00 -3.0 Z0 T00

Push rod in
continuous
machining

Limit switch or specified value

(bar shortage signal on)
G01X–3.0
(Cut-off completion)

Perform chamfering of residual material (if necessary).

See (a) to (e) in the figure on the next page.
Chamfering is needed when the residual material is difficult to be withdrawn or may cause damage on the guide
bushing due to burrs generated.

F
W30.0 movement of spindle when extracted from guide bushing = argument W
Feedrate = argument F

W Residual material Pushrod backward end

Finger chuck retract Draw material from finger chuck

Remnant box Limit switch

Insert material into finger chuck

Spindle rotates at low speed during material changing

(from retracting of pushrod to inserting of material)= argument R

(W30.0 F0.5) M6 A3.0 is dwell time after spindle chuck = argument A

Arguments W and F W30.0 is a spindle return amoun = argument W

G01 -3.0F0.02 F is a feedrate of machining data

G00 -3.0 Z0 T00

M07

When the cutting-off tool is moved to G01 X–3.0,

M108 program terminates and returns to the main program.

13-12
 L220E

Chamfering of residual workpiece

(a) Guide bushing When the steps 6 through 12 are completed.
The spindle rotates at the cutting-off speed specified in the
machining data.
The tool moves upward to the position (b) at the feedrate
specified by an argument C.

(b)  The tool moves to the position of material outer diameter +

value of argument U.

Note
The position described above is not the tool positioning
point in the machining data. If 0 is specified for argument
U, the next material is fed to the point where the tool tip is
Argument U/2 positioned. So care must be taken.

(c)  The Z axis advances by the amount specified by the

argument D at the feed rate specified by the argument C.
(The material protrudes from the guide bushing.)
 Chamfering of residual material is ready.

Advance

Argument D

13-13
L220E

(d)  The tool moves downward from point (A) to (B), Z axis
returns to the point specified by an argument D. Then the
chamfering of residual material can be performed.
 Movement is specified by an argument B for X axis, by D
for Z axis.
(Select either axis as needed.)
(A)

(B)

(Example) When an argument U = 1.0

Width Height D argument B argument
1.0 mm 0.364 mm 1.4 2.8
1.5 mm 0.546 mm 1.55 3.1
2.0 mm 0.728 mm 1.7 3.4
20° Height
In this setting chamfering of C0.5 on the residual material is
performed.
Width

(e)  The tool moves to the position of material diameter +U

argument value. At the same time, the residual material
is returned as specified by an argument W at the
feedrate specified by an argument F.
F

Argument U/2

13-14
 L220E

13.4.2 General-purpose material change program (by user program)

The material change program prepared by the user can be stored as a subprogram and called and executed by
specifying M98.

[Command format]
M98 P
P Material change program number (numbers only)

See <13.5 Subprogram (M98)> for details of M98.

[Sample program]

$1 $2
Preparation process
M09 O□□□□ Material change program
↓ $1 $2 (prepared by user)
M03 S1=800 Spindle rotates forward at 800 min–1
Machining Process G01 X21.0 W–30.0 Withdraw material from the guide bushing,
F0.5 and at the same time, escape tool to material
outer diameter
↓ M53 Coolant OFF
Cut-off process M05 Spindle stop
G01 X–3.0 F M54 Turn off the machining torque of bar feeder
M08 M07 Main spindle chuck open
M08 M55 Material change command
/ M98 P□□□□ M06 Main spindle chuck close
M09 G04 U3.0 Dwell for 3 second
M05 M52 Coolant ON
M07 M03 S1=800 Spindle rotates forward at 800 min–1
G00 X–3.0 Z0 T00 G01 W30.0 F0.5 Inserts the material into the guide bushing
up to the short cut position.
M56 M03 S1=2000 Spindle rotates forward at 2000 min–1
M02 M02 G01 X–3.0 F0.02 Cut the material tip (short-cut)
% % M99 End of subprogram
%

[Note]
 The material change program shown above is an example. Change values as needed.
 The program number must be 4 digits or less. Numbers 9000s cannot be used.
–1
 The M7 (Chuck Open) command is valid when the spindle speed is 2000 min or slower.
–1
Specifying the M7 command when the spindle speed exceeds 2000 min causes an alarm to occur.

13-15
L220E

13.5 Subprogram (M98)

Once you store a coding sequence (that is going to be repeatedly used within a program) in advance as a subprogram,
you can call this subprogram from the main program each time that sequence is needed in the program. And you can
make the main program structure simple.

13.5.1 Subprogram call instruction

The subprogram call has the following regulations.
M98 P H L ,D2

P Program number (1 to 99999999) of the subprogram to be called

(If omitted, the main program is called.)
H Sequence number (1 to 99999) in the subprogram to be called
(If omitted, the program is executed from the beginning of the main program.)
L The number of times (1 to 9999) the subprogram is to be repeated.
(If omitted, L1 is assumed.)
,D2 Specify this when calling a program stored in the compact flash card (CF).
Specify a program number by the P argument.
See <13.40 Running the Program in External Memory> for details.

13.5.2 Calling a subprogram from the main program

 The subprogram is executed only once if the number of repetition is not specified.
 The subprogram can be repeated up to 9,999 times when it is called from a main program once.
 Subprograms can be nested to eight levels.
 The subprogram call command can be specified in either of the axis control groups ($1 and $2) in the main
program.
 The main program and subprogram are called for each axis control group.

(Main program) (Subprogram)

$1 $1
$2 $2

13-16
 L220E

[Sample program]

Main program Subprograms

O0001 O0002
$1 $2 $1

M98 P0002
G00 X21.0 Z15.0 M99
%

M02 M02
M99 M99

 The M99 command must always be placed at the end.

 The subprogram does not require M02.

13.5.3 Example of using a subprogram

Dimensions and machining layout

T01

(1) T01 (2) T03 (3) T01

2
3 –ø6

ø10

T03
20 14 14 17
C1 1 1 1 C1
SUS303
68 (Free cutting stainless steel) 1

13-17
L220E

[Sample program]

Main program
O0001
$1 $2
G50 Z0
M06
G00 Z–0.5
M03 S1=1800 G99
G600 G600
N0101 T0100
G00 X11.0 T01
Z1.5
G01 X7.0 Z–0.5 F0.015
G00 X11.0 Subprogram
N0203 T0300 O0002
G00 X11.0 Z21.0 T03 $1 $2
M98 P0002 L3 G00 X11.0
N0301 T0100 G01 X6.0 F0.01
G00 X11.0 Z70.0 T01 (Repeated 3 times) X11.0 F0.2
G01 X8.0 F0.015 W–0.6
X11.0 F0.2 X9.8 W0.6 F0.01
W–1.5 X11.0 F0.2
X8.0 W1.5 F0.015 W0.6
M320 X9.8 W–0.6 F0.01
X-3.0 X11.0 F0.2
G600 G600 W15.0
M05 M99
M07 %
G00 Z0 T00
M56
G999 G999
N999 N999
M02 M02
M99 M99
% %

13-18
 L220E

13.6 Spindle Speed Change Detection Function (M94, M95, M96, M97)
The spindle speed change detection function monitors the spindle speed. If the speed change exceeds a preset rate, this
function automatically stops the machine. This prevents operation overload and damage to the guide bushing baking.
Both main spindle and back spindle have this spindle speed change detection function.

[Command format]
M97 Main spindle speed change detection OFF
M96 Main spindle speed change detection ON
M95 Back spindle speed change detection OFF
M94 Back spindle speed change detection ON

[Note]
 The main spindle speed change detection function is on by default when the power supply is turned on. To turn the
detection function off, include the M97 or M95 command in the program.
Normally, the program should contain M96 or M94 in the beginning to turn on the detection function for safety.
 Turn off the spindle speed change detection function to perform tapping with a dice, constant surface speed
control or spindle synchronization control.

13-19
L220E

13.7 Constant Surface Speed Control (G96, G97)

While the material is cut in a diametrical direction or while cutting off the workpiece after finishing a machining
process, the diameter of the material may vary depending on the portion of a workpiece, and the surface speed (the
relative speed of the workpiece and tool) may also change. The control unit can detect the tool position, calculate the
spindle speed, and change the spindle speed accordingly by using this command to instruct a relative speed.

[Command format]
G50 S Q : Specifies the spindle speed limitation
The speed is controlled so that the spindle speed does not exceed the limitation during constant surface speed
control.
S: Maximum spindle speed (min–1) clamp value
Q: Minimum spindle speed (min–1) clamp value
G96 S : Starts constant surface speed control
S: Constant surface speed value (m/min.)
G97 S1= : Ends constant surface speed control
(S2= ) S1= min–1 Main spindle speed after canceling the constant
surface speed control mode
S2= min–1 Back spindle speed after canceling the constant
surface speed control mode

[Note]
 If an S value is not specified when switching the mode between G96 and G97, the S value previously used is valid
in the new mode.
 The spindle speed fluctuation detection cannot be turned on during constant surface speed control.
 G50 S is effective only when the constant surface speed control command is effective by entering the G96
command.
 Specify Q, when the minimum spindle speed may change too lower.
 The tool selection command (T) cannot be used during constant surface speed control.
 When selecting the tool, specify the tool selection command after a cancel command (G97) is specified.

13-20
 L220E

[Sample program]

$1 $2

Preparation process

Front turning process

Thread cutting process

Other processes

(Constant surface speed control of spindle) (Constant surface speed control of back spindle)
M95 ......................... Back spindle speed fluctuation
detection OFF
M23 S2=1000
G44 ......................... Back spindle feed control ON
T3200
G00 X16.0 Z0
G50 S3500 ............. Maximum spindle rotation clamp
(3500 min–1)
G96 S40 ................. Constant surface speed control ON
G01 X–1.0 F0.03
G97 ......................... Constant surface speed control OFF
M25 ......................... Stops the back spindle rotation.
G43 ......................... Back spindle feed control OFF
M94 ......................... Back spindle speed fluctuation
detection ON
N501 T0100 ............................. Select the cut-off tool
G00 X21.0 Z50.0 M97 ............. Cut-off positioning by rapid feed
Main spindle speed change
detection OFF
G50 S5000 ............................... Maximum clamp set command
of spindle (5000 min–1)
G96 S100 ................................. Constant surface speed control
ON (Surface speed: 100 m/min)
G01 X –3.0 F0.02 .................... Cut-off
G97 (S1=500) .......................... Constant surface speed control
cancel (Normal rotation
command of 500 min–1)
M96 ........................................... Main spindle speed change
detection ON
M05
M07
G00 Z T00
M56 M56
G999 G999
N999 N999
M02 M02
M99 M99
% %

* The above program does not cover product separation.

13-21
L220E

13.8 Tool Nose Radius Compensation Function

If a rounded tool-bit is used, the rounded tool nose can cause an error between the programmed form and the cutting
form during taper cutting or circular cutting.
The tool nose R compensation function automatically calculates the error and compensates. The command code can
fix the compensation direction.

[Command format]
G40 Tool nose radius compensation mode Cancel
G41 Tool nose radius compensation left mode ON
(Offsets the tool to the left in reference to the tool advancing direction.)
G42 Tool nose radius compensation right mode ON
(Offsets the tool to the right in reference to the tool advancing direction.)

Enter tool nose R data in advance in <R> (tool nose radius value) and <P> (virtual tool nose No.) on the Tool Data
screen.
Note that the meaning of <R> on the Offset screen is different from <R> on the Tool Data screen.

Virtual tool nose

 The virtual tool nose is the point of a nonexistent tip of the tool, corresponding to the zero point shown below.
 Be sure to set the tool bit in the holder as shown in the diagram.

Virtual tool nose number

 The direction of the virtual tool nose viewed from the tool nose radius center is determined as the virtual tool nose
number.
 Tool nose between 0 and 9 is determined according to tool noses.

13-22
 L220E

13.8.1 Tools subject to tool nose radius compensation and virtual tool nose numbers
These diagrams illustrate some commonly used tools with the associated virtual tool nose numbers.

<P> <P>
8 3
R R
Diamond point tool Rear turning tool

Tool data Virtual tool nose Tool data Virtual tool nose
No. 8 No. 3

<P>
4
R
Tool data Boring tool Front turning tool

R Virtual tool nose Tool data Virtual tool nose

<P>
No. 1 No. 4
1

13-23
L220E

13.8.2 Basic pattern of tool nose radius compensation G code

The conception of the tool nose radius compensation is described below.

<P> Machining
1 direction
Boring tool T11 T11 T11 T11
(2) (3) (4)

T11
(1)
<P>
4
Front turning tool

T02
G40
G41
<P>
8 G42
Diamond point tool

T03

<P>
3
Rear turning tool

T04

[Note]
 When positioning in rapid feed or canceling the tool nose radius compensation, pay attention to the interference
with the material.
The tool nose must be kept apart from the material by more than nose radius.
 If some improper G commands are specified during tool nose radius compensation execution, an alarm occurs.
For the contents of the alarm, see the Instruction's manual of the NC manufacturer.
 While the tool nose radius compensation is being executed, tool exchange command (T) is disabled.

13-24
 L220E

Machining drawing

C2 C2

5.45

8.0
14

C0.2
Z26.0 8.5 C0.5
6.0
34.5

Machining layout drawing

Front turning
throwaway tool
T03
T03 T02 T01 nose R0.2
(1) (2) (3)

Machining
direction
Rear turning
T02 throwaway tool
nose R0.2

T01
Cut-off tool
nose

13-25
L220E

[Sample program]

O0300
$1 $2
G50 Z0
M06
G00 X15.0 Z–0.5
G99 M03 S1=2000
G630 G630 Front/back parallel machining
................................................................

N103 T0300
G00 X15.0 Z–0.5 T03
G42 G01 X4.05 F0.2 Tool nose radius compensation right mode ON
................................................................
G41 X5.45 Z0.2 F0.03 Tool nose radius compensation left mode ON
................................................................
Z6.0 F0.04
G04 U0.3
X10.0 F0.2
X15.0 Z8.5 F0.03
G40 G00 X16.0 T00 Tool nose radius compensation OFF
................................................................

N202 T0200
G50 W–3.0
G41 G00 X15.0 Z23.5 T02 Tool nose radius compensation left mode ON
................................................................
G01 X10.0 Z26.0 F0.03
X8.0 F0.015
Z34.0 F0.03
X6.8 Z34.6 F0.02
X15.0 F0.2
G40 G00 X16.0 T00 Tool nose radius compensation OFF
................................................................
G50 W3.0

N301 T0100
G50 W–3.0
G00 X15.0 Z34.5 T01
G01 X9.0 F0.2
X–3.0 F0.03
G50 W3.0
M05
M07
G00 Z0 T00
M56
G999 G999
N999 N999
M02 M02
M99 M99
% %

[Note]
This program example does not contain product separation.

13-26
 L220E

13.9 Cut-off Tool Breakage Detection (M51)

When the machine is equipped with a cut-off tool break detection unit, the cut-off tool breakage detection function is
activated by specifying M51.

[Command format]
M51 X W F Cut-off tool breakage detection

[Argument]
X Specify the position of X1 axis to move the tip of touch sensor. If this argument is omitted, the X1
axis moves to the position –1.0 of the workpiece coordinate. In usual case, this argument is not
required. Specify this argument only when the cut-off tool breakage detector cannot reach the
workpiece.
Specify the X arguemnt so that the tip of the touch sensor surely pushes the material diameter.
W Move distance (incremental) of workpiece on Z1 axis. If this argument is omitted, the Z1 axis
does not move.
F Specify the feed rate (per minute) to move the detection axis from the positioning point. If this
argument is omitted, the detector moves at 2000 mm/min.

Detection method
Cut-off Tool Breakage Detection is performed as follows:
1. The tip of the touch sensor moves to the positioning point.
2. If the W argument is specified, the workpiece (Z1 axis) moves backward.
3. The touch sensor starts operating.
4. The tip of the touch sensor moves down to the position －1.0 of the workpiece coordinate. If X and F arguments
are specified, the touch sensor moves down to the position specified by X argument at the feed rate specified by
F argument.
The tool post detects a cut-off tool breakage by sensing remaining workpiece. When the workpiece contacts with
the touch sensor, it is determined that the cut-off tool is broken and an alarm is issued. Otherwise, the detection
device proceeds to the next step.
5. The tip of the touch sensor moves to the positioning point.
6. If the workpiece (Z1 axis) has been moved by W argument in Step 2, the workpiece (Z1 axis) goes back to the
position before the M51 command is issued.

CAUTION
If the workpiece is short or a large start position shift amount is set, specify the W argument to advance
the spindle to the position where the sensor touches the material.
The advance amount varies according to the shift amount (shifted 4.0 mm from the zero point) shown in
Fig. 2 on the next page, the start position shift amount, the workpiece length and the cut-off width. Enter
an appropriate W argument value meeting the conditions.

13-27
L220E

T10 T09 T08 T07 T05 T04 T03 T02 T01

Touch sensor
T11

T12

T13

T14

Figure 1

Cut-off tool

Machining point

Shift amount: 4

ø2
Sensor stroke: 40

Figure 2

13-28
 L220E

[Sample program]
$1 $3
G50 Z0
G600 G600
M06

G00 X13.0 Z–0.5

Cut-off tool breakage detection
M51 ..........................................................
M03 S1=3000 G99

[Note]
When returning the Z axis by specifying the W argument, the return distance must be within the range the material
does not come off from the guide bushing. Burrs on the workpiece causes slippage of the chuck, and may result in
machine damage.

13-29
L220E

13.10 Corner Chamfering / Corner Rounding

The corner chamfering/rounding function chamfers or rounds a corner, at the point of intersection of lines, by entering
the chamfering or rounding size in the block that contains the coordinate value representing the corner.
Therefore, this function allows specification of chamfering or rounding at a corner without requiring coordinate
calculation usually necessary for corner chamfering or rounding.

[Command format]
Corner chamfering:
G1 X(Z) ,C F

Corner rounding:
G1 X(Z) ,R F
X: Specify the X coordinate of a corner.
Z: Specify the Z coordinate of a corner.
,C: Specify the corner chamfering size.
,R: Specify the corner rounding size.
F: Specified the feed rate.

[Sample program]
Corner chamfering:
:
Coordinate values of the point preceding the corner
G1 X1.0 Z1.0 ...........................................
Coordinate values representing the corner and the chamfering size
X5.0 ,C0.5 ...............................................
Coordinate values of the point that follows the corner to be chamfered
Z10.0 .......................................................

C0.5

(X5.0 Z10.0)
(X5.0 Z1.0)

(X1.0 Z10.0)

13-30
 L220E

Corner rounding:
:
Coordinate values of the point preceding the corner
G1 X1.0 Z1.0 ...........................................
Coordinate values representing the corner and the corner rounding size
X5.0 ,R0.5 ...............................................
Coordinate values of the point that follows the corner to be rounded
Z10.0 .......................................................

(X5.0 Z10.0)
(X5.0 Z1.0)

R0.5

(X1.0 Z1.0)

[Note]
 This function does not compensate for tool nose R.
To reflect the nose R to the workpiece shape by using the dimensions specified on the drawing, use the nose R
compensation function.
 If both ",C" and ",R" values are specified in the same block, the command specified later is valid.
 If "," is not specified in ",C", the command is assumed as a C command.
 If "," is not specified in ",R", the command is assumed as an R command.
 Tool offset is calculated for the shape after the execution of corner chamfering or rounding.
 If the shape specified in the block that follows the corner chamfering or rounding block is not a line, program error
(P382) occurs.

13-31
L220E

13.11 Thread Cutting (Equal Pitch Thread Cutting and Continuous Thread
Cutting) (G32)
This function performs thread cutting by controlling the feed and the phase of main spindle rotation. Use this function
to perform a straight and equal pitch screw thread cutting and tapered thread cutting. Continuous thread cutting that
controls axis feed to maintain synchronization with spindle rotation with minimal errors at the shape changing point
when cutting screw thread when shapes change is also possible.
This function is effective for thread cutting to the part of smaller diameter (machined in back turning process), which
cannot be performed by the canned threading cycle. G32 command is used in G92 (canned threading cycle).

[Command format]
G32 X(U) Z(W) F Q E

[Argument]
X(U) Specify the thread cutting infeed position. (U: Incremental command)
Z(W) Specify the thread cutting end position in longitudinal direction. (W: Incremental command)
F Specify the pitch (lead) in longitudinal direction.
Q Enter the Q argument to specify the thread cutting start shift angle (0 to 359.999)
E Specify the number of threads per inch. The E argument is used instead of the F
argument that specifies the longitudinal thread pitch/lead.

[Sample program]

45

P0.4
P0.3
5.5
5.8

5.0

This program is an example of machining a workpiece into a form as shown above. An outline cutting tool for front
turning is used to finish-machine the top end of the workpiece into this form. Thread cutting is performed twice: the
first infeed amount is 0.4 mm in the diameter, the second one is 0.2 mm in the diameter, and the final thread cutting is
finished at 45°.

13-32
 L220E

:
M3 S1=800
G99
T200
G0 X6.5 Z–1.0 T2 ............................. The tool is positioned to the thread cutting start point
X4.43
G32 X5.1 Z3.0 F0.3
X5.4 Z5.0 F0.4
X6.5 Z5.55 Specify a thread cutting cycle in the program because the continuous
G0 Z–1.0 threading function does not provide a canned cycle. Thread cutting is
X4.23 repeated twice in this program. If the thread cutting count increases,
subprograms should be used.
G32 X4.9 Z3.0 F0.3
X5.2 Z5.0 F0.4
X6.5 Z5.65
G0 X6.5 Z–1.0 T0 ............................. The tool returns to the thread cutting start point
:

When machining a workpiece into a generally threaded form, you can also use this function to change the amount of
infeed or the angle of final thread cutting.

[Note]
 If screw thread changes in lead or geometry consecutively at very short intervals, the workpiece may not be
machined correctly into the specified form.
 The program above is given as a sample, so specify machining conditions in consideration of the actual material to
be machined, etc.
 G32 comamnd is canceled when G0 or G1 command is issued. To return the main spindle from the threading end
position to threading start position, specify G0 or G1 at the top of every coordinate command.

13-33
L220E

13.12 Longitudinal Cut-Off Cycle (G75)

The longitudinal cut-off is a canned cycle which automatically performs grooving in outer diameter direction of
workpieces by specifying the grooving end position, infeed amount, tool shift amount, and move distance of tool at
fillet. This cycle is used for rough grooving on outer diameter and step machining in cutting-off operation on the fixed
headstock lathes.

[Command format]
G75 R(1)
G75 X Z P Q R(2) F

[Argument]
R(1) Specify the return amount for every step.
X Specify the grooving end position of X axis.
Z Specify the grooving end position of Z axis.
P Specify the infeed amount (steps) for every step.
Q Specify the tool shift amount.
R(2) Specify the move distance of Z axis at fillet.
F Specify the cutting feed rate. (If omitted, the feed rate used in previous cycle is used.)

[Sample program]
:
(1) T200 ....................................................... Call the tool
(2) G0 X20.0 Z7.0 T2 ................................... Position to the grooving position (start position of canned
cycle)
(3) G75 R0.2 ................................................ Specify the return amount for every step
(4) G75 X10.0 Z15.0 P2.0 Q2.5 R0 F0.1 ..... Perform grooving to the fillet position X10.0, Z15.0:
X direction: 2 mm at every step (P2.0)
Z direction: Grooving 2.5 mm at every step (Q2.5)
Z axis: Does not move (R0)
(5) G0 X20.0 T0 ........................................... Move the tool away (including canned cycle cancel)
:

(Start point)
P

R (1)

R (2) X, Z

13-34
 L220E

Sample program for rough grooving to outer diameter

:
T300
G0 X18.0 Z3.0 T3
G75 R0.2
G75 X5.0 P1.5 F0.08
G0 X18.0 T0
:

[Note]
 Position the tool to the threading start point before specifying the cycle command.
 If Z and P arguments are omitted or 0 is specified, only the X axis moves.
 If the value of P argument is larger than the hole depth, step machining is not performed.
 The following conditios cause an alarm to occur.
 The Z argument is specified, but the P argument is omitted or 0 is specified.
 The value for P argument is larger than groove width.
 The value for R(2) argument is larger than that for Q argument.
 The value for R(1) argument is larger than that for P argument.
 The canned cycle is canceled when 01 group of G code (G0, G1, G2, or G3) is specified.

13-35
L220E

13.13 Deep Hole Drilling Cycle 2 (G79, G80)

Deep hole drilling can be specified by one line of commands when [Deep Hole Drilling Cycle 2 (G79)] is used.
The deep hole drilling cycle 2 allows specification of the first infeed depth and the second infeed depth independently.
Furthermore, drilling in the end face direction and that in the cross direction are automatically distinguished by the
arguments specified in the program.

[Command format]
G79 Z(X) R I K A Q J F ,F
G80

[Argument]

Z Specify the coordinate value of the bottom (end point) of a hole

machined on the end face. Always specify either Z or X.
Specification of both Z and X is not
X Specify the coordinate value of the bottom (end point) of the cross permitted.
hole.

R Specify the distance from the drill positioning point to the drilling cycle start position in a radial value.
I Specify the depth of first infeed in a radial value. If neither I nor K is specified, step
machining is not performed.
K Specify the depth of the second and successive infeed in a radial If only either I or K is specified, I = K
value. is assumed.

A Specify the drill stop safety distance in a radial value. (See the figure below.)
Q Specify the dwell at the bottom of a hole. (In each drilling cycle, dwell is performed at the hole bottom.)
J Specify the dwell at the return position. (In each start of infeed from the return position, dwell is
performed at the first positioning point.)
F Specify the cutting feed rate. If F argument is not specified, the cycle is executed at the feed rate
which is valid before the start of the drilling cycle. If G98 is specified before the specification of the
cycle, specify the feed rate in a feed per minute value.
,F Specify the rapid feed rate in a feed per minute value.

Q
J

I K A
Z

Cutting feed Rapid feed

13-36
 L220E

[Sample program]
:
:
T1200
G0 Z–1.0
G79 Z20.0 I6.0 K3.0 A0.5 J500 F0.1 T12
G80
G0 Z–1.0 T0
:
:

[Note]
 For the dwell command (Q and J arguments), a decimal point must not be specified. To specify 0.5 seconds, for
example, input "Q (J) 500". If these arguments are omitted, dwell is not performed.
 If the A argument (drill return safety distance) is omitted, the value set at "G83 Retract" in the preparation
parameter is used.
 The drilling cycle is canceled when G80, or G0, G1, G2 or G3 is specified. At the same time, argument values are
cleared to zero.
 When a drilling cycle is performed in the 1-block state, operation does not stop during the execution of the cycle
but it stops after the completion of the cycle.
 When the Hold key is pressed during the execution of a drilling cycle, the cycle stops immediately. The operation
can be restarted from the stopped position.

13-37
L220E

13.14 Synchronized Tapping Functions (G88, G84, G80)

The synchronized tapping functions perform tapping while fully controlling the feed and rotational phase.
This feature brings about merits such as the use of an ordinary drill holder instead of a floating tap holder. The thread
length is easily calculated by using an ordinary drill holder.

[Note]
The tapping speed becomes slower or faster than the value specified in the program, depending on the type of the
holder to be used. When using holders with which the tapping speed changes, specify the tapping speed in
consideration of deceleration or acceleration. For example, if the holder of 1/2 deceleration is used, specify the value
for F argument as a half of the standard value. Specify the rotary tool speed S in consideration of
deceleration ratio (twice as standard value in case of 1/2 deceleration).

13.14.1 Synchronized tapping for outer circumference with a rotary tool (G88 and G80)
This function performs tapping while synchronously controlling the rotary tool and the X axis (NC axis).
This function enables tapping for outer circumference, which makes a tapped hole in highly accurate depth.

[Command format]
G88 X R F D S Q , R1 or R2 Tapping cycle
G80 Tapping cycle cancel

[Argument]
X Specify the tapping end position. The value must be specified for the diameter.
R Specify the distance from the point where the tap is positioned to the position where synchronized
tapping starts. The distance must be specified with a value for the radius.
F Specify a screw pitch.
D± Specify the rotary tool and the rotation in which the spindle rotates.
3: The rotary tool on gang tool post
5: The rotary tool on back spindle
4: The front rotary tool on opposite tool post.
+ denotes forward rotation, – denotes reverse rotation.
S Specify the spindle speed.
Q Specify this argument to speed up the tap when it returns. A multiple of 100 can be specified in
the range 100 to 500. For example, when Q200 is specified, the tap returns twice as fast as when
it heads toward the specified position. The default is Q100. In this case, the tap returns at the same
speed as when it heads toward the specified position. A value "300" is recommended for the Q
argument. However, the value of the Q argument depends on the conditions and the material.
Determine the value in accordance with the shape of the tap. To specify the Q argument,
high-speed synchronized tapping option (different from the synchronized tapping option).
,R1 Specify the synchronized tapping mode. Unless ",R1" is specified, the feed with the G98
command specified is used in the previous mode. If only "G88, R1" is specified, the mode is
switched, but tapping is not performed.
,R2 Specify the synchronized tapping mode and phase adjustment. Specify this argument, for
example, if you execute synchronized tapping, execute other machining process, and then execute
synchronized tapping again for deburring. The starting positions of first and second synchronized
tapping must be same. When using R2 argument (phase adjustment), the gear ratio of the motor
and the holder must be 1:1.
This argument is available only to B-axis rotary tools on the gang tool post (S3). It is not available
to tools other than B-axis rotary tools on the gang tool post (S3) such as the front rotary tool on
opposite tool post (S4) and the rotary tool on back tool post (S5). To use the R2 argument, the
phase adjustment for synchronized tapping option (differs from the synchronized tapping) is
required.

13-38
 L220E

Tap (1) Point where the tap spindle is

Rapid Cutting positioned (diameter specification)
feed rate feed rate (2) Rapid feed positioning (radius
specification) for the amount
equivalent to the R value
(synchronized tapping start
position). The distance between
the position (2) and the material
(1) (5) Point where the outer diameter must be as long as
tap is positioned 3 pitches or more.
R value (3)(3)’ Tapping end position (Tapping
For distance , secure (2) end position and tool backward
(4) Synchronized tapping rotation)
at least 3 pitches. start position
(Radial value)  (4) The tool moves by the amount
equivalent to the R value and
returns to the synchronized
tapping start position.
(5) The tool returns to the point where
(3) (3')
X the tap spindle is positioned, at
the rapid feed rate.
End point Tool rotating direction is reversed.

[Sample program]
Material diameter: ø12.0
When the screw pitch is 0.7:
When using the cross machining tool on front side (L20X)

$2
: Clearance between the workpiece and tap
M28 S0 Pitch × 3
M83 S4=0 Doubled because of
diameter specification
T2300
G98 G00 X18.2 Z25.0 T13...................... X18.2 = ø12.0 + {(1 + 2.1) × 2} = 18.2
G88 X0.0 R1.0 F0.7 D4 S500, R1
G80
G00 X18.2
M85
:

[Sample program]
G84 command
When the screw pitch is 0.7:
When using the front rotary tool on opposite tool post (T20's)
$2
:
M28 S0
M83 S4=0
T2300
G98 G0 X0 Z-3.1 T23
G84 Z8.0 R1.0 F0.7 D4 S500, R1
Z8.0 R1.0
G80
G00 Z-3.1 T0
M85
:

13-39
L220E

G88 command
Material diameter: ø12.0
When the screw pitch is 0.7:
When using the front rotary tool on opposite tool post (T20's cross machining tool)
$2
:
:
M28 S0
M80 S4=0 G98
N0711 T2300
G00 X18.2 Z25.0 T23
G88 X5.0 R1.0 F0.7 D3 S500, R1
X0.0 R1.0
G80
G00 X18.2
M82
:
:

13-40
 L220E

13.14.2 Synchronized tapping for the end face of a workpiece with a rotary tool
(G84, G80)
While stopping the main spindle from rotating and synchronously controlling the rotary tool and the Z1 axis (or Z2
axis), this function performs tapping for the end face of the workpiece (center or eccentric). This function makes a
tapped hole in highly accurate depth.

[Command format]

G84 Z R F D S Q , R1 or R2 Tapping cycle

G80 Tapping cycle cancel

[Argument]
Z Specify the tapping end position.
R Specify the distance from the point where the Z1 axis is positioned to the position where
synchronized tapping starts.
F Specify a screw pitch.
D Specify the rotary tool and the rotation in which the spindle rotates.
3: The rotary tool on gang tool post
5: The rotary tool on back spindle
4: The front rotary tool (end-face drilling tool) on opposite tool post
+ denotes forward rotation, – denotes reverse rotation.
S Specify the spindle speed.
Q Specify this argument to speed up the tap when it returns. A multiple of 100 can be specified in
the range 100 to 500. For example, when Q200 is specified, the tap returns twice as fast as when
it heads toward the specified position. The default is Q100. In this case, the tap returns at the same
speed as when it heads toward the specified position. A value "300" is recommended for the Q
argument. However, the value of the Q argument depends on the conditions and the material.
Determine the value in accordance with the shape of the tap. To specify the Q argument,
high-speed synchronized tapping option (different from the synchronized tapping option).
,R1 Specify the synchronized tapping mode.
,R2 Specify the synchronized tapping mode and phase adjustment. Specify this argument, for
example, if you execute synchronized tapping, execute other machining process, and then execute
synchronized tapping again for deburring. The starting positions of first and second synchronized
tapping must be same. When using R2 argument (phase adjustment), the gear ratio of the motor
and the holder must be 1:1.
This argument is available only to B-axis rotary tools on the gang tool post (S3). It is not available
to tools other than B-axis rotary tools on the gang tool post (S3) such as the front rotary tool on
opposite tool post (S4) and the rotary tool on back tool post (S5). To use the R2 argument, the
phase adjustment for synchronized tapping option (differs from the synchronized tapping) is
required.

[Note]
The rotation direction of rotarytool may change depending on tool layout or the selected tool number. See <14.4
Automatic Control of Rotation Direction of Tool Spindle> for more information.

13-41
L220E

[Sample program]
When the screw pitch is 0.7:
Rotary tool on back tool post
$2
:
M78 S0
G98 M180 S5=0
T3200
G0 X0 Z–3.1 T32
G84 Z8.0 R1.0 F0.7 D5 S500, R1
G80
G0 Z–3.1 T0
M182
:

When the screw pitch is 0.7:

Rotary tool on gang tool post
$2
:
M28 S0
M83 S4=0
T2100
G98 G00 X0 Z–3.1 T32
G84 Z8.0 R1.0 F0.7 D4 S500, R1
G80
G0 Z–3.1 T0
M85
:

13-42
 L220E

13.14.3 Synchronized tapping for the center of the end face of a workpiece
(main or back) (G84, G80)
While rotating the spindle (main or back) and synchronously controlling the spindle and the Z axis (Z1 axis for main
spindle, Z3 axis for back spindle), this function performs tapping for the center of the end face of the workpiece (main
or back). This function makes a tapped hole in highly accurate depth.

[Command format]

M97(M95) Main spindle speed change detection

OFF
(Back spindle speed change detection
OFF)
G84 Z R F D S Q , R1 or R2 Tapping cycle
G80 Tapping cycle cancel
M96(M94) Main spindle speed change detection
ON
(Back spindle speed change detection
ON)

[Argument]
Z Specify the tapping end position.
R Specify the distance from the point where the Z1 axis is positioned to the position where
synchronized tapping starts.
F Specify a screw pitch.
D Specify the spindle and the rotation in which the spindle rotates.
1: Main spindle
2: Back spindle
+ denotes forward rotation, – denotes reverse rotation.
S Specify the spindle speed.
Q Specify this argument to speed up the tap when it returns. A multiple of 100 can be specified in
the range 100 to 500. For example, when Q200 is specified, the tap returns twice as fast as when
it heads toward the specified position. The default is Q100. In this case, the tap returns at the same
speed as when it heads toward the specified position. A value "300" is recommended for the Q
argument. However, the value of the Q argument depends on the conditions and the material.
Determine the value in accordance with the shape of the tap. To specify the Q argument,
high-speed synchronized tapping option (different from the synchronized tapping option).
,R1 Specify the synchronized tapping mode.
,R2 Specify the synchronized tapping mode and phase adjustment. Specify this argument, for
example, if you execute synchronized tapping, execute other machining process, and then execute
synchronized tapping again for deburring. The starting positions of first and second synchronized
tapping must be same. When using R2 argument (phase adjustment), the gear ratio of the motor
and the holder must be 1:1.
To use the R2 argument, the phase adjustment for synchronized tapping option (differs from the
synchronized tapping) is required.

[Note]
Be sure to execute the M97 (M95) command (spindle speed change detection OFF) before the G84 command. If the
spindle speed change detection is not OFF, synchronized tapping ends up with an alarm.

13-43
L220E

[Sample program]
When the screw pitch is 0.7:
Front side

$1
: Clearance between the workpiece and tap
G99 M3 S1=0 Pitch × 3
M97
T2300
G0 X0 Z–3.1 T23 ................................ Z–3.1= –(1 + 2.1) = –3.1
G84 Z10.0 R1.0 F0.7 D1 S500, R1
G80
G0 Z–3.1 T0
M5
M96
:

Back side
$2
:
G44
G99 M23 S2=0
M95
T3300
G0 X0 Z–3.1 T33
G84 Z10.0 R1.0 F0.7 D2 S500, R1
G80
G0 Z–3.1 T0
M25
M94
:

13-44
 L220E

13.14.4 Continuously synchronized tapping

This function performs synchronized tapping continuously. If ordinary synchronized tapping is unable to make a
tapped hole in desired depth because the cutting load, this function achieves the desired depth by performing
synchronized tapping continuously while changing the amount of infeed.

[Command format]
Synchronized tapping to end face of the workpiece:
G84 Z R F D S Q , R1 or R2 Tapping cycle
Z R Continuous tapping cycle

Synchronized tapping to outer circumference of the workpiece:

G88 X R F D S Q , R1 or R2 Tapping cycle
X R Continuous tapping cycle
G80 Tapping cycle cancel

[Argument]
X Specify the tapping end position. The value must be specified for the diameter.
R Specify the distance from the point where the tap is positioned to the position where synchronized
tapping starts. The distance must be specified with a value for the radius.
F Specify a screw pitch.
D Specify the rotary tool and the rotation in which the spindle rotates.
3: The rotary tool on gang tool post rotates forward.
4: The front rotary tool on opposite tool post rotates forward.
5: The rotary tool on back spindle rotates forward.
+ denotes forward rotation, – denotes reverse rotation.
S Specify the spindle speed.
Q Specify this argument to speed up the tap when it returns. A multiple of 100 can be specified in
the range 100 to 500. For example, when Q200 is specified, the tap returns twice as fast as when
it heads toward the specified position. The default is Q100. In this case, the tap returns at the same
speed as when it heads toward the specified position. A value "300" is recommended for the Q
argument. However, the value of the Q argument depends on the conditions and the material.
Determine the value in accordance with the shape of the tap. To specify the Q argument,
high-speed synchronized tapping option (different from the synchronized tapping option).
,R1 Specify the synchronized tapping mode. Unless ",R1" is specified, the feed with the G98
command specified is used in the previous mode. If only "G88, R1" is specified, the mode is
switched, but tapping is not performed.
,R2 Specify the synchronized tapping mode and phase adjustment. Specify this argument, for
example, if you execute synchronized tapping, execute other machining process, and then execute
synchronized tapping again for deburring. The starting positions of first and second synchronized
tapping must be same. When using R2 argument (phase adjustment), the gear ratio of the motor
and the holder must be 1:1.
This argument is available only to B-axis rotary tools on the gang tool post (S3). It is not available
to tools other than B-axis rotary tools on the gang tool post (S3) such as the front rotary tool on
opposite tool post (S4) and the rotary tool on back tool post (S5). To use the R2 argument, the
phase adjustment for synchronized tapping option (differs from the synchronized tapping) is
required.

13-45
L220E

[Sample program]
Material diameter: ø12.0
When the screw pitch is 0.7:
$1
:
:
M28 S0
S3=0 M80 G98
N0711 T1300
G00 X18.2 Z25.0 T13
G88 X5.0 R1.0 F0.7 D3 S500, R1
X0.0 R1.0
G80
G00 X18.2
M82
:
:

Material diameter: ø12.0

When the screw pitch is 0.7:
Front rotary tool on opposite tool post
$2
:
:
M28 S0
M83 S4=0
N0711 T2300
G98 G00 X18.2 Z25.0 T13
G88 X5.0 R1.0 F0.7 D4 S500, R1
X0.0 R1.0
G80
G00 X18.2
M85
:
:

13-46
 L220E

13.15 Arc Threading (G35, G36)

The arc threading function performs arc threading through circular interpolation while controlling the feed of the tool
synchronized with the spindle. Use of the continuous threading function enables the switching of machining - for
example, from arc threading to linear threading or from arc threading to taper threading.

[Command format]
G35(G36) X(U) Z(W) I K (R ) F(E) Q
G35 Clockwise threading
G36 Counterclockwise threading

[Argument]
X(U) X-axis coordinate as the arc end point
Z(W) Z-axis coordinate as the arc end point
I X-axis coordinate as the center of the arc (increment to the center of the arc when viewed from
the start point)
K Z-axis coordinate as the center of the arc (increment to the center of the arc when viewed from the
start point)
R Radius of the arc (Specify the argument I, K, or R.)
F(E) Lead (F: General lead screw, E: Precision lead thread or inch screw thread)
Q Shift angle at which threading starts (0.001 to 360.000°)

X axis

Z W

Arc threading
End point

U/2
Start point

X
Z axis

R
I

Center

13-47
L220E

[Sample program]
$1
T300
G50 W–10.0
G0 X11.0 Z–1.0 T3
X0.98
G35 U1.638 W4.48 R12.66 F0.9.............. Arc threading
Taper threading
G32 U0.682 W4.52 F0.9 ..........................
G0 X5.0
Z–1.0
G50 W10.0

Arc thread part Taper thread part

13-48
 L220E

13.16 Differential Rotary Tool Function (G164)

This function controls spindles by superimposing the speed of a spindle on the speed of another spindle.
Use this function when you need to rotate a rotary tool by imposing it on the rotation of the main spindle. For example,
the function performs tapping at the center of the workpiece with the rotary tool while the workpiece chucked by the
main spindle is rotating.
The G164 command specifies the reference spindle and superimposed spindle, and places the two specified spindles in
the superimposed status.
The G113 command frees the two spindles from the superimposed status in which they are rotating by the differential
rotary tool command.

CAUTION
To specify G164 (differential speed rotary tool function), specify it after the tool has been selected. See
<14.4 Automatic Control of Rotation Direction of Rotary Tool>.

[Command format]
G164 H D Differential rotary tool command
G113 Differential rotary tool cancel command

[Argument]
H Specify the reference spindle. 1 is the main spindle, 2 is the back spindle.
D Specify the rotation direction of the axis relative to superimposed and reference spindles.
–3: The rotary tool on gang tool post
–4: The front rotary tool (end-face drilling tool) on opposite tool post
–5: The rotary tool on back spindle

13-49
L220E

[Sample program]
$1
M3 S1=3000
M81 S3=2000
T1200
G164 H1 D–3 ........................................... Differential rotary tool command
M77
G0 Z–2.0
G84 X0.0 Z10.0 R1.0 F1.0 D3 S2000 ,R1 Synchronized tapping
.................................................................
G80
G113 ........................................................ Differential rotary tool cancel command

$2
M23 S2=5000
M81 S3=1000
T5200
G164 H2 D–3 ........................................... Differential rotary tool command
M77
G0 Z–2.0
G84 X0.0 Z10.0 R1.0 F1.0 D3 S1000 ,R1 Synchronized tapping
G80
G113 ........................................................ Differential rotary tool cancel command

Front rotary tool on opposite tool post

$2
M3 S1=3000
M83 S4=2000
T2100
G164 H1 D–4 ........................................... Differential rotary tool command
M77
G0 Z–2.0
G84 X0.0 Z10.0 R1.0 F1.0 D4 S2000 ,R1 Synchronized tapping
G80
G113 ........................................................ Differential rotary tool cancel command

13-50
 L220E

[Note]
 Be sure to specify the command M77 (spindle synchronization completion queuing) after specifying the command
G164.
 The spindle rotating by the differential rotary tool function stops when the machine enters the emergency stop
state. The differential rotary tool mode is canceled at the same time.
 Be careful of the maximum spindle speed clamp when specifying the differential rotary function. While the
maximum spindle speed clamp command is active, the superimposed spindle is unable to maintain the speed
difference specified for the reference spindle.
 Indexing for the reference spindle is not permitted in the differential rotary tool mode.
 To index the reference spindle, cancel the differential rotary tool mode.
 An alarm is issued if the spindle speed is clamped when a synchronized tapping command is executed in the
differential rotary tool mode.
M181 S5=4000
T3100
G4 H2 D-5
M77
G0 Z-2.0
G84 X0.0 Z10.0 R1.0 F1.0 D–5 S4000 ,R1
G80
G113
In the example above, the speed of the superimposed spindle ranges from 1000 min –1 (tapping) to 9000 min–1 (tap
returning). Since some values exceed clamp speeds of the superimposed spindle (rotary tool on gang tool post):
5000 min–1, an alarm is generated before tapping.
 In the differential rotary tool mode, specification of “,R2” (synchronized tapping phase adjustment) is not
permitted.
 The rotation direction of rotary tool may change depending on tool layout or the selected tool number. See <14.4
Automatic Control of Rotation Direction of Rotary Tool> for more information.

13-51
L220E

13.17 Canned Cycle Longitudinal Machining (G90)

When machining a workpiece with simple shape, usually the linear interpolation (G1) function is used. However, if
the workpiece has large allowance, the turning fixed canned cycle is used. The following explains the canned cycle
longitudinal machining (G90).

[Command format]
G90 X(U) Z(W) R F

[Argument]
X Coordinate value of the end point in the diametric direction (X axis) (Absolute command)
U Coordinate value of the end point in the diametric direction (X axis) (Incremental command)
Z Coordinate value of the end point in the longitudinal direction (Z axis) (Absolute command)
W Coordinate value of the end point in the longitudinal direction (Z axis) (Incremental command)
R Taper amount (in a radial value)
F Feed rate (mm/rev)

Outline of machining
Straight and taper cutting in the longitudinal direction is performed in the cycle as shown below.

(1) (4) (1) (4)

Guide bushing
(2) (3)

Cutting feed

Material Rapid feed

(2) (3)

13-52
 L220E

Straight cutting cycle

[Sample program]
Cutting ø20.0 mm to ø15.0 mm material × 5.0 mm long product
Infeed depth: 0.5 mm/infeed
G90 X(U) Z(W) F

Cutting feed rate

Rapid feed rate

ø15.0 ø20.0

(X0,Z0)
5.0

G99 M3 S1=4000; ................................... Feed per revolution mode, spindle forward rotation,
4000 min–1
T500; ....................................................... T05 tool selection
G0 X21.0 Z-1.0 T5; ................................. Positioning point, offset
G90 X19.0 Z5.0 F0.1; ............................. 1st infeed
X18.0; ..................................................... 2nd infeed
X17.0; ..................................................... 3rd infeed
X16.0; ..................................................... 4th infeed
X15.0; ..................................................... 5th infeed
G0 X21.0 Z-1.0 T0; ................................. Tool returns, offset is canceled
:

13-53
L220E

Taper cutting cycle

[Sample program]
Cutting ø20.0 mm material × 5.0 mm long product
Infeed depth: 0.5 mm/infeed
G90 X(U) Z(W) R(I) F

Cutting feed rate

Rapid feed rate

ø15.0 ø20.0

(X0, Z0)

5.0

G99 M3 S1=4000; ................................... Feed per revolution mode, spindle forward rotation,
4000 min–1
T500; ....................................................... T05 tool selection
G0 X21.0 Z-1.0 T5; ................................. Positioning point, offset
G90 X20.0 Z5.0 R-1.0 F0.1; .................... 1st infeed
X19.0; ..................................................... 2nd infeed
X18.0; ..................................................... 3rd infeed
X17.0; ..................................................... 4th infeed
X16.0; ..................................................... 5th infeed
X15.0; ..................................................... 6th infeed
G0 X21.0 Z-1.0 T0; ................................. Tool returns, offset is canceled
:

[Note]
The canned cycle longitudinal machining is canceled by G0 and G1. After the completion of the canned cycle, always
specify G0 or G1 in the coordinate value command that specifies tool return operation.

13-54
 L220E

13.18 Thread Cycle Canned Cycle (G92)

This thread cutting cycle machines thread by controlling axis feed and spindle phase.

[Command format]
G92 X Z R Q F

[Argument]
X Specify the thread cutting infeed position in the X axis direction.
Z Specify the thread cutting infeed position in the Z axis direction.
R Specify the taper size (r) for taper thread cycle canned cycle.
Q Enter the Q argument to specify thread cutting start shift angle (0.001 - 360.000 degrees)
F Specify a screw pitch.

Example of machining with M10 P=1.5

Machining a non-ferrous material (right-hand thread)
G92 X Z F

L (1.5 mm): Thread lead

Za (12 mm): Effective length
a (10.5 mm): Tool shift
Xn: In-feed
* Uneven thread ridge portion
For the details on the in-feed, see <9.3 Thread Cutting Count> in
[Introduction] of the Instruction Manual (Optional).

Start point

Xn
M10 Z

L
Z point to be specified
in program
*2L Za *L

13-55
L220E

Outline of machining
Perform threading with a tool in the following cycle:

(1) (4)

(2) (3)

(1) (4)

a
a

Initial point

2L Za Za L

(2) (3)

a a

2L Za L Za L

13-56
 L220E

[Sample program]
Selects the T03 tool
T0300 ......................................................
G50 W-10.5
M03 S1=1500 ......................................... Specifies spindle forward rotation at 1500 min –1
Makes the machine dwell for 1.0 second for stable rotation.
G4 U1.0 ..................................................
G00 X13.0 Z-3.0 T Positions the tool at the initial point (Z = 2L)
..........................
G92 X9.3 Z15.0 F1.5 .............................. 1st in-feed (X1 0.35) (Z = Za ) (F = L)
2nd in-feed (X2 0.25)
X8.8 ........................................................
3rd in-feed (X3 0.16)
X8.48 ......................................................
4th in-feed (X4 0.1)
X8.28 ......................................................
5th in-feed (X5 0.06)
X8.16 ......................................................
6th in-feed (X6 0.05)
X8.06 ......................................................
0 cut (same as final in-feed)
X8.06 ......................................................
G00 X Z To initial point of next process
................................
G50 W10.5

 The spindle speed is limited as specified by the following equation:

N: Main spindle speed

8000 (mm/min) L: Thread lead (mm)

N (min–1) ≦ L (mm)

8000: Maximum feed rate

–1
 The standard spindle speed for thread cutting is 500 to 2000 min .
 Uneven thread ridges are produced at the threading start and end points due to the delay of the servo system. The
length of uneven thread portions at a spindle speed of 1,500 min –1 is approximately two times of the thread lead
length (2L) at the entry area, and the thread lead length (L) at the exit area. This uneven thread ridges, length
becomes shorter as the spindle speed lowers.
 When selecting right-handed or left-handed threading, reverse the rotation of the main spindle either by changing
the Z-axis start position or by using the reverse holder.
 For chamfering (round-up on the screw trailing end), 0 to 89 degrees can be set using a parameter. (See the
Instruction Manual of the NC manufacturer.)

[Note]
 For the details on the in-feed, see <9.3 Thread Cutting Count> in [Introduction] of the Instruction Manual
(Optional).
 In the G92 thread cutting programming, if EOB (;) is specified for an infeed command, the infeed command in the
preceding block is used as modal command.
G92 X11.0 Z F ;
X10.0;
X9.0;
; (Thread cutting at X9.0)
; (Thread cutting at X9.0)
G0 ;

13-57
L220E

G92-Taper thread cutting canned cycle

G92 can be used for taper thread cutting.
Taper thread cutting is performed in a canned cycle from (1) to (2), (3) to (4), then back to (1). The coordinate
reference point is (3).
The sign (+ or –) of the slope "r" indicates the direction of the location of the start point from the end point.
Outline of machining
G92 X Z R r F

L: Thread lead
Za: Effective length
a: Tool shift
r: Slope
* Uneven thread ridge portion

(1) (4)
X0 ①
(3)
r (2)

② Z
③
④
Z program zero point
L
2L * Za L*

[Sample program]
T ..................................................... Select threading tool
M S1= .................................. Command for spindle forward or reverse rotation at a spindle speed
of min–1
G4 U1.0 ................................................... 1.0 second dwell for stabilize rotation
G00 X ① Z T .................... Positioning tool at initial point.
X (thread diameter + 2L), Z (a –2L)
G92 X ② Z R –r F ........ 1st in-feed
X (③) ....................................................... 2nd in-feed
X (④) ....................................................... 3rd in-feed
X (④) ....................................................... Zero cut
G00 X Z ................................ Move to initial point of next process. (Threading cycle OFF)

13-58
 L220E

13.19 Link-Thread Machining

With a machine equipped with guide bushing, if the thread length in Z direction is longer than the hold length of inner
diameter of guide bushing, the workpiece becomes apart from the guide bushing when it returns to the thread
positioning point. Thus, the machining is discontinued. In such a case, repeat a cycle of "outer diameter turning to
thread cutting" several times to link the thread to subsequent threads. It enables thread cutting in Z direction without
being broken.
This function performs thread cutting by controlling the feed and the phase of main spindle rotation. Using this
function enables link-thread cutting by specifying the link position in the same Z direction.
[Sample program]
Hold length of guide bushing inner diameter: 25.0 mm
Material diameter ø20.0
Thread shift amount 1.5 mm
M12 × pitch 1.5

(2) (4) (6)

(1) (3) (5)

50.0

13-59
L220E

T300 (Front turning (1)) Subprogram

G0 X21.0 Z–0.5 T3
G1 X9.0 F0.1 O0007
G1 X12.0 Z1.0 F0.05 G0 X14.3
Z19.0 F0.1 G32 X11.3 W1.5 F1.5
X18.0 W15.0 (*)
X21.0 W1.5 U3.0 W1.5
: G0 W–18.0
T400 (Thread cutting (2)) X13.8
G50 W–1.5
G0 X21.0 Z–1.5 T4 G32 X10.8 W1.5 F1.5
M98 P0007 ................................ To subprogram W15.0
G0 X21.0 Z–1.5 T0 U3.0 W1.5
G50 W1.5 G0 W–18.0
X13.48
T300 (Front turning (3))
G0 X21.0 Z18.0 T3 G32 X10.48 W1.5 F1.5
G1 X14.0 F0.1 W15.0
G3 X12.0 Z19.0 R1.0 F0.05 U3.0 W1.5
G1 Z33.0 F0.1 G0 W–18.0
X18.0 X13.28
X21.0 W1.5
: G32 X10.28 W1.5 F1.5
T400 (Thread cutting (4)) W15.0
G50 W-1.5 U3.0 W1.5
G0 X21.0 Z12.0 T4 ................... Z: Distance from the first threading position G0 W–18.0
M98 P0007 multiple of pitches X13.16
G0 X21.0 Z12.0 T0 First threading position Z –1.5 to Z12.0
13.5 mm
G50 W1.5 G32 X10.16 W1.5 F1.5
13.5 / 1.5 = 9 Divided out
W15.0
T300 (Front turning (5)) U3.0 W1.5
G0 X21.0 Z32.0 T3 G0 W–18.0
G1 X14.0 F0.1 X13.06
G3 X12.0 Z33.0 R1.0 F0.05
G1 Z47.0 F0.1 G32 X10.06 W1.5 F1.5
X18.0 W15.0
X21.0 W1.5 U3.0 W1.5
: G0 W–18.0
T400 (Thread cutting (6)) X13.06
G50 W–1.5
G0 X21.0 Z25.5 T4 G32 X10.06 W1.5 F1.5
M98 P0007 ............................. To subprogram W15.0
G0 X21.0 Z25.5 T0 U3.0 W1.5
G50 W1.5 G0 W–18.0
:
: M99

13-60
 L220E

[Note]
 The program is an example for the reference. Specify an appropriate depth of cut and the cutting condition,
according to the workpiece and the tool.
 Specify the thread length so that the workpiece will not be apart from the guide bushing. Note that the length to be
held by the guide bushing depends on the material diameter.
 Be sure to deburr from the workpiece diameter at the end of front turning. If the burr is remained, the workiece
cannot be returned into the guide bushing. It may cause an accident and the pitch may be shifted.
 Determine the Z coordinate position to connect the second and the subsequent screws by calculating the distance
(the first threading point + multiple of pitch). The length of thread cutting (shown by (*) in the sample program)
must be a multiple of pitch. If these values are inaccurate, a pitch shift may occur.
 If the chuck opens during thread cutting, the shift phase of thread occurs and it causes link-thread cutting to fail.
Be sure to perform link-thread cutting within one chuck.
 The program is an example when machining a thread of 1L. Take 2L or more margin for first and the final thread
cuttings.
 It is recommended that the second and the subsequent infeed and the final thread cutting is finished at 45°.

13-61
L220E

13.20 Multi-thread Screw Cutting

Multi-thread screw
Generally used screw is called as a single-thread screw, which has a spiral in one pitch, and advances only one pitch
per one revolution. With the single-thread screw, the lead (distance per one rotation) is equal to the pitch. In contrary,
the screw that has two or three spirals within one lead is called multi-thread screw. With the multi-thread screw, the
lead is multiple of pitches.
Pitch × Number of threads = Lead
Pitch 0.75 × double-thread screw = Lead 1.5

Double-thread screw
0° Two spirals in
one lead
180°
Single-thread screw

Pitch

Pitch = Lead
Lead

[Sample program]
The G32 command performs thread cutting by controlling the feed and the phase of main spindle rotation.
The position of spindle rotation direction where the infeed starts with G32 command is always the same. Define this
position (angle) as 0°. If the infeed of first thread starts from 0°, start the infeed of second thread from the position
shifted by 180°. This can make the multi-thread screw.
* See <13.11 Thread Cutting (Equal Pitch Thread Cutting and Continuous Thread Cutting)> for command format.
Material diameter ø20.0
Thread shift amount 1.5 mm
Machining of double-thread screw of M12 × Pitch 0.75 (Lead = 1.5)

13-62
 L220E

Front turning process Subprogram 1 Subprogram 2

:
: O0077 O0777
: G0 X11.76 G0 X11.76
T300 (Multi-thread cutting) G32 W15.0 F1.5 Q0 G32 W15.0 F1.5 Q180000
G50 W–1.5 U5.196 W1.5 F1.5 U5.196 W1.5 F1.5
G0 X21.0 Z–3.0 T3 G0 W–16.5 G0 W–16.5
X14.0 : :
M98 P0077 To subprogram 1 G0 X11.56 G0 X11.56
G0 X14.0 Z–3.0 G32 W15.0 F1.5 Q0 G32 W15.0 F1.5 Q180000
M98 P0777 To subprogram 2 U5.196 W1.5 F1.5 U5.196 W1.5 F1.5
G0 X21.0 Z–3.0 T0 G0 W–16.5 G0 W–16.5
G50 W1.5 : :
: G0 X11.36 G0 X11.36
: G32 W15.0 F1.5 Q0 G32 W15.0 F1.5 Q180000
: U5.196 W1.5 F1.5 U5.196 W1.5 F1.5
G0 W–16.5 G0 W–16.5
: :
G0 X11.2 G0 X11.2
G32 W15.0 F1.5 Q0 G32 W15.0 F1.5 Q180000
U5.196 W1.5 F1.5 U5.196 W1.5 F1.5
G0 W–16.5 G0 W–16.5
: :
G0 X11.1 G0 X11.1
G32 W15.0 F1.5 Q0 G32 W15.0 F1.5 Q180000
U5.196 W1.5 F1.5 U5.196 W1.5 F1.5
G0 W–16.5 G0 W–16.5
: :
G0 X11.1 G0 X11.1
G32 W15.0 F1.5 Q0 G32 W15.0 F1.5 Q180000
U5.196 W1.5 F1.5 U5.196 W1.5 F1.5
G0 W–16.5 G0 W–16.5
: :
M99 M99

By applying this program, change the infeed start angle to make triple- or quad-thread screw.

[Note]
 The program is an example for the reference. Specify an appropriate depth of cut and the cutting condition,
according to the workpiece and the tool.
 Specify the thread length so that the workpiece will not be apart from the guide bushing.
 Be sure to deburr from the workpiece diameter at the end of front turning. If the burr is remained, the workiece
cannot be returned into the guide bushing. It may cause an accident and the pitch may be shifted.
 If the chuck opens during thread cutting, the shift phase of thread occurs and it causes multi-thread cutting to fail.
Be sure to perform multi-thread cutting within one chuck.
 Consider the lead angle to perform high-lead threading, and select an appropriate tool.
 For the high-lead threading, specify the cutting condition not to exceed the maximum feedrate.

13-63
L220E

13.21 Machine Coordinate System Command (G53)

The machine coordinate system command (G53) function specifies the positioning point in the machine coordinate
system.

[Command format]
G53 X Z Y ,F
X: Specify the X axis coordinate in the machine coordinate system. The axis in the specified axis control group
moves to the machine coordinate specified by X.
Z: Specify the Z axis coordinate in the machine coordinate system. The axis in the specified axis control group
moves to the machine coordinate specified by Z.
Y: Specify the Y axis coordinate in the machine coordinate system. The axis in the specified axis control group
moves to the machine coordinate specified by Y.
,F: Specify the feed rate. If this argument is omitted, the axis moves in rapid feed rate.

13-64
 L220E

13.22 Y-axis Holder

The Y-axis holder performs cutting in Y direction. The cutting chips are dropped naturally from the cutting position,
and effective for the chip removal.
[Procedure]
1. Press the Preparation key to display the Preparation screen.
2. Mount the Y-axis holder while pushing its shoulder part to the gang tool holder.

Mount the Y-axis holder by pushing it against the gang tool holder.

3. Move the cursor to "Tool Typ" of the tool for which the Y-axis holder is mounted and set "L Y" for the tool
name.
If the "Tool Type" was "12R", change it to "12L Y".
*0
Usually the tool name is "R". By changing this to "L Y", the tool is positioned at the position shown in Figure A
or Figure B when "DIA" or "Core" is executed.
4. Press the menu key [DIA], and press the Start key several times until the cursor reaches the position "DIA". Then,
align the outer diameter of the material with the tool nose. (Figure A)
5. Move the tool away from the material, and move the material backward so that it is placed behind the end-face
of guide bushing.
6. With the menu key [Core DWN] being selected, press the Start key continuously until the cursor reaches the
position "Core DWN". Then, align the outer diameter of the material with the tool nose. (Figure B)
* When adjusting the position by "Core DWN", pay attention to interference between the tool at left and the
material.
7. Move the tool away from the material, and move the material backward so that it is placed behind the end-face
of guide bushing.
8. Repeat Step 5. Now the setting completes.

Figure A Figure B

13-65
L220E

[Sample program] Material dia.: 20 mm

T500 (Front turning) ;
G0 X21.0 Z0 T5 ;
G1 X-0.5 F0.1 ;
X18.0 ;
Z15.0 ;
X19.2 ;
X20.2 W0.5 ;
G0 X21.0 W0 T0 ;
T300 (Y axis back turning) ← Moves to the position shown in Figure A.
G50 W-3.0 ;
G0 Y21.0 Z20.0 T3 ;
X0.0 ; ← Moves to the position shown in Figure B.
G1 Y16.0 F0.05 ; ← Cutting is performed in Y direction.
Z30.0 ;
Y15.4 W0.3 ;
Y21.0 ;
X21.0 ;
G0 U0 V0 W0 T0
G50 W3.0 ;

[Note]
 The Y-axis holder size differs according to the machine model. Select the holder meeting the machine model.
 Do not mount a Y-axis holder next to a rotary tool. If mounted, the tool may interfere with the material during
machining depending on the material diameter.

13-66
 L220E

13.23 Multi-piece Machining

In ordinary operation, material is re-chucked after machining of one workpiece is completed. In the multi-piece
machining, however, multiple workpieces are machined continuously in single material chucking operation.

[Note]
Machining data
Material diameter 10.0 mm
Machining length 27.6 mmTotal workpiece length + Cut-off tool width + Shift amount
for end face turning＋Margin
＝25.0＋2.0＋0.1＋0.5
Number of workpieces/chucking 3 pcs.
Back spindle chuck position 20.0 mm

Setting the machining data

After setting the machining length of a workpiece to "Machining Length" on the Machining Data screen, set the
number of workpieces to be machined in one chucking to "Pieces/1Chuck".

Main Program
O0002
$1 $2
G50 Z0
M6
G99

!2L15 !1L15
Calling subprogram O0005
M98 P5 L3 ............................................... Same as $1
M98 P5 L3 ...............................................
Number of repetitive calling times: 3
!2L20 !1L20
M8
M8
Material change program
/M98 P7000..............................................
M9
M5
M7
Move to the starting point.
G0 X-3.0 W-81.3* T00 .............................
W value = (Total workpiece length +
Cut-off tool width + Shift amount for
end face turning) × (Number of
products / chucking)
G999 G999
N999 N999
M2 M2
M99 M99

13-67
L220E

Subprogram
O0005
Shift amount for end face turning:
G50 Z-0.1 .................................................
0.1 mm
M9
M6
G113
G0 X11.0 Z-1.0
： ：
： ：
[Front machining] [Back machining]
： ：
： ：
T3000
!2L1 !1L1
M24 S2=2500 M3 S1=2500
G114.1 H1D-2

T100 (CUT-OFF)
Z27.0 = Total workpiece length +
G0 X11.0 Z27.0 T1 ..................................
Cut-off tool width
G650 G650
G0 Z-1.0
M72
G98 G1 Z5.0 F2000
M77
G4 U0.3
M15
M73
G4 U0.2
!2L10 !1L10
G99 G1 X-1.0 F0.03
G600 G600
G98 G1 X-3.0 F0.05 M25
G113
M5
M56
M99 M99

[Note]
 The Z1 axis starts retracting from the forward end position by "Machining Length × Pieces/1Chuck" when the
start point operation is executed.
 When 1-cycle operation completes, make sure that the start point is identical to the end point by executing the start
point operation.
If they do not match, over-travel or interference may occur.

13-68
 L220E

13.24 Rapid Feed Acceleration/Deceleration Time Constant Setting

ON/OFF (M360/M361)
While running a program, rapid feed acceleration/deceleration time constant of individual axis (X1, Z1 and Y1 axes)
can be changed. This feature is especially effective in G630 front/back parallel machining. By changing the
acceleration/deceleration time constant of the gang tool post (X1 and Y1 axes) the workpiece can be finished at high
accuracy in back machining.
To the contrary, rapid feed acceleration/deceleration will be slowed in tool selection for the gang tool post when the
acceleration/deceleration time constant is changed, causing the cycle time to be increased.

About rapid feed acceleration/deceleration time constant

An axis for which rapid feed (G0) is specified is accelerated to the rapid feed rate at a constant slope and then
decelerated at a constant slope to stop at the target point of positioning. The duration in which the axis is accelerated
or decelerated is called the acceleration/deceleration time constant. Note that the acceleration time and deceleration
time are the same time.

Rapid feed rate

Feed rate

Time constant Time constant Time

Time necessary for the axis to be Time necessary for the axis to be
accelerated to the rapid feed rate decelerated to zero speed (stop)

Initial Value of Rapid Feed Acceleration/Deceleration Time Constant of Each Axis

Acceleration/Decelerati
Axis Name
on Time Constant
X1 45 msec
Z1 100 msec
Y1 100 msec
X2 120 msec
Z2 90 msec
Y2 60 msec

[Command format]
M360 X Z Y Rapid feed acceleration/deceleration time constant setting ON

X Specify an integral multiple of the initial value of X1 axis acceleration/deceleration time constant. Specify a
value with a decimal point. Specification range: 1 to 6
Z Specify an integral multiple of the initial value of Z1 axis acceleration/deceleration time
constant. Specify a value with a decimal point. Specification range: 1 to 6
Y Specify an integral multiple of the initial value of Y1 axis acceleration/deceleration time constant. Specify a
value with a decimal point. Specification range: 1 to 6

M361 Rapid feed acceleration/deceleration time constant setting OFF

The acceleration/deceleration time constant of the X1, Z1 and Y1 axes is reset to the initial value.
When execution of a program is terminated halfway, it is possible to reset the acceleration/deceleration time constants
to the initial values by pressing the Reset key.

13-69
L220E

[Sample program]
In the program below, M361 and M360 are specified before and after the tool selection command in $1 in the
operation where back finish machining in $2 and tool selection in $1 are overlapped. Tool selection operation in $1 is
performed at a restricted speed and finishing accuracy in back machining is secured.
$1 $2
:
:
Multiplies the X1 and Y1 axis
M360 X4.0 Y4.0 ....................................... :
acceleration/deceleration time
constant by four
Select the tool
T300 ......................................................... Back finish machining
Resets the X1 and Y1 axis
M361 ........................................................ :
acceleration/deceleration time
constant to the initial values
:
:

[Note]
 Specify axis control group 1 ($1) as rapid feed acceleration/deceleration time constant setting (M360/M361) for
X1, Z1 and Y1 axes and specify axis control group 2 ($2) as rapid feed acceleration/deceleration time constant
setting for (M360/M361).
 Changing the acceleration/deceleration time constants may increase a cycle time.
 Determine the multiplication value for changing the acceleration/deceleration time constants according to the
machining accuracy required in the back machining.
 To achieve better finishing accuracy in back machining, use M350/M351 (rapid feed rate setting ON/OFF)
together with M360/M361.
See <13.26 Rapid Feed Rate Setting ON/OFF (M350/M351)> for the use of M350/M351.
 M360/M361 cannot be specified in the superimposition (G620 or G650) mode.

13-70
 L220E

13.25 Medium-pressure Coolant Device

Medium-pressure coolant is available by opening the valve to be used and operating the separately installed pump.
This is effective to remove chips by supplying powerful coolant.

[Command format]
Trochoid pump (separately installed pump)
M452 Trochoid pump ON
M453 Trochoid pump OFF

Valves
M430 Back spindle oil blow ON
M431 Back spindle oil blow OFF
M432 Opposite tool post ON
M433 Opposite tool post OFF
M434 Back tool post ON
M435 Back tool post OFF
M436 Guide bushing or Ceiling ON
M437 Guide bushing or Ceiling OFF

[Note]
 Open any of the valves before turning on the trochoid pump.
 If the valve is closed immediately after stopping the trochoid pump, pressure remains in the coolant line.
Therefore, make a program so that the valve is closed allowing a certain interval after stopping the trochoid pump.
 At the end of the program, open all valves to release internal pressure. If residual internal pressure remains, the
pump motor or a valve may be damaged.
 The M codes described above show the position to where the coolant is to be discharged when U74R
(medium-pressure coolant device, optional) is installed. The position may differ depending on customer's
requirement.

13-71
L220E

13.26 Rapid Feed Rate Setting ON/OFF (M350/M351)

The standard rapid feed rate for each axis is set to 32 m/min for the X1, Y1, Z1, X2 and Z2 axes and 8 m/min is set for
the Y2 axis. Use this to change the feed rate of parts that operate at G0 (feed rate) when a canned cycle, etc. is used.

[Command format]
M350 X Y Z Rapid feed rate setting ON
M351 Rapid feed rate setting OFF (Restores the standard rapid feed rate)

[Argument]
When specifying the function in axis control group 1 ($1)
 X Specify the rapid feed rate of the X1 axis. Specification range: 0 to 32000 mm/min
 Y Specify the rapid feed rate of the Y1 axis. Specification range: 0 to 32000 mm/min
 Z Specify the rapid feed rate of the Z1 axis. Specification range: 0 to 32000 mm/min

When specifying the function in axis control group 1 ($2)

 X Specify the rapid feed rate of the X2 axis. Specification range: 0 to 32000 mm/min
 Z Specify the rapid feed rate of the Z2 axis. Specification range: 0 to 32000 mm/min

[Sample program]
$1
:
:
M350 Z18000 ...................................................... Sets the Z1 axis rapid feed rate at 18000 mm/min (18 m/min)
T1200
G0 Z-1.0
G79 Z20.0 I6.0 K3.0 A0.5 J500 F0.1 T12 The Z1 axis operates at 18 m/min until M351 is specified
G80
G0 Z-1.0 T0
M351 .................................................................... Turns off the rapid feed rate setting function for the Z1 axis and
restores the standard rapid feed rate
:
:

[Note]
 After turning on the rapid feed rate setting function by specifying M350, make sure to turn the function off by
specifying M315 when the function is no more necessary. If the function is not turned off, the axis moves at the
specified rapid feed rate in tool selection and the G0 mode, causing the operation to be executed slower than usual.
There are cases the cycle time is considerably increased.
 Pressing the Reset key restores the standard rapid feed rate.
 M350/M351 cannot be specified in the superimposition (G620 or G650) mode.

13-72
 L220E

13.27 Cutting Start Interlock Enabled/Disabled (M86, M87)

The cutting start interlocks are automatically turned ON/OFF when the machining pattern is changed. In general, you
do not have to turn ON/OFF the cutting start interlocks by using the M codes.

[Command format]
M86 Cutting start interlock enabled
(The cutting start interlock of a specified axis control group is set back to original.)
M87 Cutting start interlock disabled (All the cutting start interlocks of a specified axis control group
are disabled.)

Relationship between the machining patterns and cutting start interlocks:

Machining S1 S2
pattern S1 S2 S3 S4 S5 S1 S2 S3 S4 S5
G600     
G610  
G620    
G630    
G650 Depending on the previous machining pattern
G660    
: Cutting start interlock enabled

[Note]
 Cutting start interlock function may not work correctly if the cutting feed is specified immediately after the
spindle or rotary tool rotation command, even if this function is enabled. In this case, insert two or mroe G4 codes
between the rotation command and the cutting block.

13-73
L220E

13.28 Error Detect ON/OFF (M92, M93)

Use this command when higher precision in edge processing is required. If the error detect is enabled (ON), cutting
feed proceeds to the next block after confirming the speed is completely decelerated. Thus, the desired edge precision
can be obtained.

[Command format]
M92 Error detect ON
M93 Error detect OFF

[Sample program]
$1
:
T0200 (Front turning)
G0 X11.0 Z-1.0 T02
X6.0
M92 (ON)
G1 Z0 F0.05
X7.0
X8.0 Z0.5 F0.03
Z10.0 F0.05
X10.0
G0 X11.0 T00
M93 (OFF)
:

[Note]
 Error detect function is disabled at power on (error detect OFF (M93)).
 Error detect function is effective only when G1, G2, or G3 command is specified.
 Difference from the exact stop check (G9) function
The exact stop check function is enabled only in the block where G9 is specified. Meanwhile, the error detect ON
(M92) is enabled until the error detect OFF (M93) is specified.
 When the error detect function is enabled, the longer cycle time is required than that in disabled state because the
completion of cutting feed is prolonged.

13-74
 L220E

13.29 Start Position Queuing (Type 1) (G115)

[Command format]
!L G115 X Z C
Operation example
 This command specifies a start position to provide a queuing point halfway through a block.
(1) When queuing is specified in the program for an axis control group (local axis control group), the other axis
control group (remote axis control group) starts moving first.
(2) The local axis control group starts moving when the remote axis control group reaches the specified start
position.
(3) If the start position specified by G115 does not exist on the next-block moving path of the remote axis control
group, the local axis control group starts moving when the remote axis control group reaches all axis coordinate
values of the commanded position.
(4) The start position check applies only to the axis specified by G115.
(5) If the start position is not found when the remote axis control group moves to the next block, the local axis
control group waits until the remote axis control group reaches the start position by moving beyond the next
block.
(6) If the two axis control groups overlap by the G115 command, they remain queued.
(7) When specifying the start position, use the work coordinate values of the remote axis control group.
(8) Specifying G115 for more than three axis control groups results in the program error P33.
(9) The G115 block is not subject to single-block stop.
(10) If two or more G115 blocks are specified consecutively, the block specified last is valid.
(11) The addresses that follow G115 are the X-axis, Z-axis, and C-axis workpiece coordinates.

13-75
L220E

13.30 Start Position Queuing (Type 2) (G116)

[Command format]
!L G116 X Z C
Operation example
 When queuing is specified in the program for an axis control group (local axis control group), the local axis
control group starts moving first.
(1) The other axis control group (remote axis control group) starts moving when the local axis control group reaches
the specified start position.
(2) If the start position specified by G116 does not exist on the next-block moving path of the local axis control group,
the remote axis control group starts moving when the local axis control group reaches all axis coordinate values of
the commanded position.
(3) The start position check applies only to the axis specified by G116.
(4) If the start position is not found when the local axis control group moves to the next block, the program error P33
occurs before the local axis control group starts moving.
(5) If the two axis control groups overlap by the G116 command, they remain stopped.
(6) When specifying the start position, use the work coordinate values of the remote axis control group.
(7) If G116 is specified for more than three axis control groups, multiple remote axis control groups start moving
simultaneously.
(8) The G116 block is not subject to single-block stop.
(9) If two or more G116 blocks are specified consecutively, the block specified last is valid.
(10) The addresses that follow G116 are the X-axis, Z-axis, and C-axis work coordinates.

13-76
 L220E

13.31 Auxiliary Function Output during Axis Feed (G117)

[Command format]
G117 X Z C 
Auxiliary function
Operation example
This command specifies an intermediate point and the auxiliary function to be output at that point, allowing the
auxiliary function to be executed during movement.
(1) This command is placed independently immediately before the moving command block in which you want the
auxiliary function to be executed.
(2) This command is not subject to single-block stop.
(3) In the G117 block, auxiliary functions can be specified within the limit indicated below.
M command: 4 sets (M code used for macro: No more than 2 sets)
S command: 1 set each
T command: 1 set
(4) This command can be specified for up to two consecutive blocks.
If three blocks or more are specified consecutively, the last two blocks are valid.
(5) If the operation start position specified by G117 does not exist on the moving path, the auxiliary function is output
when all axis coordinate values of the operation start position are reached. Only the specified axes are checked.
(6) At the operation start position, after checking that the previous auxiliary function has been output, the next
auxiliary function is output. The PC interface can be used as usually without modification.
(7) The auxiliary function specified along with a moving command block is output before movement is started.
Movement does not stop at the operation start position. Note that, at the block end position, after checking that all
auxiliary functions have been output, the next block is executed.
(8) G117 should be specified in the order of operation start positions. The program error P33 occurs if the order of
operation start positions is opposite to the moving sequence.
When the operation start positions match the moving sequence, auxiliary functions are output in the order in
which they are specified.
(9) If the operation start position for the next block is not found, the program error P33 occurs before moving to the
next block.
(10) The descriptions (8) to (9) above can be summarized as in the following table:

First block Intermediate point found during

No intermediate point during movement
Second block movement
Intermediate point found The order in (8) is followed. Program error occurs as in (8).
during movement
No intermediate point The order in (9) is followed for the The order in (9) is followed. Auxiliary
during movement second block. functions are output in the order of the first
block, then the second block regardless of the
order of the specified points.

(11) The addresses that follow G117 are the X-axis, Z-axis, and C-axis work coordinates.

13-77
L220E

13.32 Arbitrary Axis Change (G140)

Use the G140 command to declare the axis you want to use.
Use the G140 command to declare the axes you want to superimpose on each other.

[Command format]
G140 X=X1 Z=Z1 Y=Y1 The command specifies the axes to be used in the subsequent operations as follows:
X=X1, Z=Z1, Y=Y1
G140 X=X1 Z=Z2 Y=Y1 The command specifies the axes to be used in the subsequent operations as follows:
X=X1, Z=Z2, Y=Y1
Gang tool post: X1 Z1 Y1 C1 (Z1: Main headstock, C1: Main spindle C axis)
Opposite tool post: X2 Z2 C2 (C2: Back spindle C axis) Y2

[Sample program]
$1 $2

Machining pattern cancel G600 ........................................................

G600 ........................................................ Machining pattern cancel
T0800
:
:
!2L1 !1L1
The G4 command is executed to prevent
G4 ............................................................
the read ahead of G140 while $1 is using
the X1 axis and Y1 axis
G140 X=X1 Z=Z2 The arbitrary axis change (G140)
Y=Y1 command is executed after $1 finishes
using the X1 axis and Y1 axis

:
G140 X=_ Z=_
Must be returned to the previous axis.
Y=_; .........................................................
:

[Note]
Before the arbitrary axis change (G140) command can be executed to declare the number of an axis being used by
another axis control group, the queuing command must be executed for the axis control group to finish using the axis.
At this time, the G4 command must also be executed to prevent the read ahead of G140 after the queuing command.

CAUTION
Be careful when using the G140 command (arbitrary axis change). If the G140 command is specified to
declare an axis that is being used by another axis control group, the machine may encounter an
interference problem.

13-78
 L220E

13.33 End Position Specified Queuing (G149)

This command enables queuing between an arbitrary position in an arbitrary block in the local axis control group and
an arbitrary block position in the remote axis control group.
While the standard queuing function adjusts the start timing between the queuing axis control groups, this function
adjusts the end timing of the end block specified by the block ID number.

[Command format]
!L G149 Q X Z C End position specified queuing

Q represents the end position block number. It is specified by BN .

[Sample program]
$1 $2

G98 G0 X1.1
Queuing block specification
!2 G149 Q100 X1.0 .................................. Queuing block specification
!1 Q120 ....................................................
Queuing time
................................................................. Queuing time
................................................................
G1 X5.0 F50
BN100 G1 X–1.0 F10 BN120 G1 Z50.0 F100

With this example, block BN120 in $2 is completed when the X axis in $1 passes a point of 1.0 in block BN100.
(1) The end position queuing position must be specified in the work coordinate system.
(2) Only the axis on which a queuing position has been specified is checked for its passing the end position.
(3) If the queuing position is specified on multiple axes, the queuing time is the time by which all the specified axes
have passed the specified point.
(4) If the specified axis does not pass the point specified in the block of the specified end position block number, a
program error (P33 format error) occurs when the G149 command is issued.
(5) If the end position block number of the G149-specified axis control group is not found within 10 blocks from the
end position specified queuing command or if no P code has been specified, the required time is calculated
assuming the moving block in which all the specified axes has passed the specified point as the end position
specification block. Note, however, that a program error (P700BN No number) occurs if the moving block is not
found within 10 blocks from the end position queuing command.)
(6) The program error (P700BN No number) also occurs if the end position block number of an axis control group not
specified by G149 is not found within 10 blocks from the end-pint queuing command.
(7) If a macro call or subprogram call is included within the range specified for end position specified queuing, the
macro call or subprogram call and M99 are counted as one block.
(8) Whichever axis control group that requires shorter run time for the range of program specified for end position
specified queuing waits for processing to be started. ($2 may move first.)
(9) The end position queuing position is not aligned if the range of program specified for end position specified
queuing requires run time exceeding two hours.
(10) Do not place an end position specified queuing command within 10 blocks from another end position specified
queuing command. Doing so causes a program error (P700BN No number).
(11) Within the range specified for end position specified queuing, do not include any command for changing the
workpiece coordinate system, shifting the local coordinate system, presetting the counter, or for milling.
Otherwise, the end position specified queuing position is mis-aligned because the specified position is calculated
on the workpiece coordinate system effective in the block in which end position queuing is specified.
(12) The end position may not be able to be obtained if any of the following commands is placed, in the range of
program specified for end position specified queuing, for controlling the axis having the specified end position.
Do not include the following commands concerning the end position specified axis.
 Arbitrary axis exchange control, Direct axis control
 Arbitrary axis superimpose control
(13) Address Q that follows G149 specifies a queued block; X1, Z1, and C specify their respective work coordinates.
(14) If an axis passes the queuing position even once in the range of the program from the block of G149 to the block
immediately before the BN block, queuing is not executed correctly.

13-79
L220E

13.34 Arbitrary Axes Superimposition (G156)

Use the G156 command to declare the axes you want to superimpose on each other.

[Command format]
G156 Z2=Z1 Superimpose ON The Z2 axis is superimposed on the Z1 axis.
G156 Z2 Superimpose OFF The superimposition of the Z2 axis on the Z1 axis is
canceled.
(To cancel superimposition, specify the superimposed
axis.)
Gang tool post: X1Z1Y1C1 (Z1: Main headstock, C1: Main spindle C axis)
Back spindle head stock: X2Z2C2 (C2: Back spindle C axis)

[Sample program]
$1 $2
Machining pattern cancel
G600 ........................................................ Machining pattern cancel
G600 ........................................................
T0300 T3300
!2L1 !1L1
: Arbitrary axis superimpose
G156 Z2=Z1 ............................................
!2L2 !1L2
: Coordinate system setting
G50 Z*** ..................................................
: :
: :
: :
!2L3 !1L3
Superimpose cancel
G156 Z2...................................................
!2L4 !1L4
: :

[Note]
 Before the arbitrary 1-pair axes (G156) command can be executed, the queuing command must be executed for
stopping the base axis and the axis to be superimposed. The queuing command must also be executed before the
superimposition cancel command.
 After executing the arbitrary 1-pair axes superimposition command (G156), set the coordinate system of the
superimposed axis conforming to the coordinate system of the base axis.
 The G53 command cannot be executed for a superimposed axis during execution of the superimpose function.
 By specifying a sign preceding an axis name like "G156 Y2=－Y1", the superimposed axis can be moved in the
opposite direction of the reference axis movement direction.
 To cancel superimposition, specify G156 and the superimposed axis in the program of the axis control group that
contains the superimposed axis.

13-80
 L220E

Pinch milling
$1 $2
T700 (D6-ENDMILL)
G50
W-15.0
End mill dia. + Machining
G0X10.0Y-[6.0+3.0+1.0]T6 ......................
outer dia. + Clearance
End mill radius + Clearance
Z-[3.0+1.0] ..............................................
Machining Pattern Cancel
G600 ........................................................ Machining Pattern Cancel
G600 .......................................................
M28S0 T2200 (D6-ENDMIL)
Cannot approach unless
M88 .........................................................
INT. CHK is disabled.
G0 X10.0 Y-[6.0+3.0+1.0] Y coordinate is same as
$1.
T22 ..........................................................

G53 Z-179.0 (*1) .......................................

Position where the center
of front rotary tool on
gang tool post aligns with
that on opposite tool post
G1 X-5.0 F500
Wait for !1 L10
!2 L10 ....................................................... Wait for !2 L10
!1 L10 ......................................................
M83 S4=3000 (*2)
G98 G19
M80 S3=3000 (*2)
Arbitrary axes
G156 X2=Y1 ............................................
superimposition
X2 (motor axis) (*3)
superimposes on Y axis
(ARA)
End mill dia. + Product
G1 Y-[6.0+1.1] F250 ................................
thickness + Cutting stock
Z10.0 F100
G3 V-0.5 Z11.323 R2.0 F50
Retract
G1 Y-[6.0+3.0+1.0] F1000 .......................
G1 Z-[3.0+1.0] F5000
(SIAGE)
End mill dia. + Product
G1 Y-[6.0+1.0] F250 ................................
thickness
Z10.0 F100
G3 V-0.5 Z11.323 R2.0 F50
G1 Y-[6.0+3.0+1.0] F1000
G1 Z-[3.0+1.0] F5000
G0 X10.0 T0
G50 W15.0
Wait for !1 L112
!2 L112 ..................................................... Wait for !2 L112
!1 L122 ....................................................
M82 M85 Cancel superimposition
G156 X2 ..................................................
Retract (*4)
G98 G1 X10.0 F1000 ..............................
G0 U0 V0 W0 T0
M1
Alternate machining pattern
G610 ........................................................ Alternate machining
G610 .......................................................
pattern
Opposite tool post retracts
Enable INT. CHK
M89 .........................................................

13-81
L220E

15 mm
+Z1
$1 (G600)
10 mm

Gang tool post (T6) +Y1

Width:

ø3
1 mm
R5

Opposite tool post (T22)

+Y2 +X2
Tool diameter: ø6
$2 Machining direction: Down cut
$2 (T2200) +Z2 (Motor axis) +Z2

[Note]
 *1
The axis moves in raid feed rate.
Use M350 command to change axis feed rate for safe operation as needed.
*2
Be sure to specify the same rotational speed for both rotary tools. Otherwise, the finish surface will not be even.
*3
If T2200 is called, the axis that moves parallel to Y1 axis (X2 of motor axis) is changed to Y2 axis.
*4
If the machining pattern is changed after T2200 is called, the command axis is changed to motor axis.
(In the sample program above, machining pattern is not changed.)

 Parameter for superimposition control direction of Y1 and Y2 axes needs to be changed manually.
(Base axis parameter 1010: polar(X2)=0 must be changed to 1.)
 In tool layout, use GSE3110 in cross machining direction. If GSE3110 is used in end-face direction, it will
interfere with opposite tool post. Change the tool name for T22 to "Cross" on Preparation screen.

13-82
 L220E

13.35 Line Angle Command

This command is used to define the end position of a line by specifying the angle of the line and the coordinate value
of either of two axes of the end position. The command automatically calculates the coordinate value of the end
position of the other axis and controls axis movement accordingly.
Therefore, the line that has the desired angle can be directly specified using the angle without calculating the
coordinate values of the end position.

[Command format]
G1 X (Y) (Z) A F

[Argument]
X: Specify the X coordinate of the end position.

Y: Specify the Y coordinate of the end position. For the coordinate value of the end position,
specify either of the axes in the selected plane.
Z: Specify the Z coordinate of the end position.

A: Specify the angle of the line.

F: Specify the feed rate.

[Sample program 1]
(X9.0, Z8.464) ③
X
(X9.0, Z15.0) ④
① 30
(5.0, Z0) (X5.0, Z5.0) ②

:
G1 X5.0 F0.03.......................................... ①
Z5.0.......................................................... ②
X9.0 A30.0 ............................................... ③
Z15.0........................................................ ④
:

13-83
L220E

[Sample program 2]

X ②
(X10.0, Z4.0)

45
①
(X4.0, Z12.0)
(X10.0, Z0) (X4.0, Z7.0) ④

:
G1 X10.0 F0.05 ........................................①
Z4.0 ..........................................................②
Z7.0 A-45.0 ..............................................③
Z12.0 ........................................................④
:

[Note]
 Specify the angle of the line by measuring it in reference to the positive direction of the horizontal axis in the
selected plane (G18). The angle measured in the counterclockwise direction is expressed with the " " (plus) sign
and that in the clockwise direction with the "–" (minus) sign.

+
Z
－

 For the end position, specify either of the axes constituting the selected plane (G18).
If the angle and the coordinate value of both axes are specified, the angle is disregarded.
 This command is valid only in the G1 mode.
It is not valid for other interpolation modes or positioning modes.

13-84
 L220E

13.36 Geometric Command

It is possible to define the chamfering or rounding shape on the corner formed by arbitrary lines by combining the
corner chamfering/rounding command, explained in <13.10 Corner Chamfering / Corner Rounding>, and the line
angle command explained in <13.35 Line Angle Command>.
If the coordinate values of the point of intersection of two lines cannot be calculated easily, the geometric command
function calculates the coordinate values of such a point by simply specifying the angle of the first line and the
coordinate values (absolute values) of the end position and the angle of the second line. The function automatically
calculates the coordinate values of the end position of the first line and controls axis movements.

[Command format]
G1 A ① ,R(C) F ;
X(Y) Z A ② ;

[Argument]
A ① Specify the slope (angle) of the first line.
,R(C) Specify the rounding (chamfering) amount at the corner formed between two lines.
(This argument can be omitted if corner rounding (chamfering) is not necessary.)
F Specify the feed rate.
X Specify the X coordinate value (absolute value) of the end position of the second line.
Y Specify the Y coordinate value (absolute value) of the end position of the second line.
Z Specify the Z coordinate value (absolute value) of the end position of the second line.
A ② Specify the slope (angle) of the second line.

[Sample program]

Second line
(X19.0, Z9.732)

(X19.0, Z20.0)
? 15°

R0.3
First line

(X9.536, Z5.0) 75°

:
G1 Z5.0 F0.1;
X9.536;
G1 A75.0 ,R0.3 F0.03;
X19.0 Z9.732 A15.0;
Z20.0 F0.1
:

13-85
L220E

13.37 Free Tool Layout Pattern (Holder Name = Free Tool)

This command allows the number of tools to be increased by changing the pitch between the tools on the tool post.
Usualy, 18 gang tools is available on gang tool post. Specify "Free Tool" as holder names on the Machining Data
screen. However, you will need to manufacture a special holder in accordance with your requiremnet.

[Command format]
T (Four-digit T code)
This command is much the same as an ordinary tool selection command.
Usually, T01 to T19,T21 to T29, T51 to T59, T30, and T31 to T39 can be used.

Tool Layout Pattern screen

Enter the tool position data on the Tool Pattern screen shown below.

Like the ordinary machining, an ordinary command can be issued in the X-Y coordinates after tool selection. Each
program can be created as before.

[Note]
 Notice that the tool moves using the T code.
 Confirm the contents of the following before machining when the free tool layout is used.
1. Check whether "Free Tool" has been specified as holder name 1 to 3 on the Machining Data screen.
2. Check the position of each tool from the guide bushing center as the reference point.
 Sufficient T codes are provided in the machine software. In actual, the tool size and other mechanical factors are
limited during use.

13-86
 L220E

13.38 Custom Macro Program (Program Call by G code)

To call the custom macro program that has been edited and registered, you can use G code number instead of using O
number. Up to 200 code numbers (between G1200 and G1399) can be registered. O8100 to O8999 are used as
program numbers for this function. You may use the conventional method, calling by O number.

[Command format]
G65 P8101; Program call by O number (conventional method)
G1201; Program call by G code

[Procedure]
1. Press the Parameter key .

2. Press the menu key [Set Up 1].

3. Specify values according to the table below.

Preparation Parameter screen

Available
Number Item Description
value
8071 For G1200 to Type 0:M98 P**** 0 to 3
G1299 1:G65 P****
2:G66 P****
3:G66.1 P****
8072 Program No. Specify the numerical value for the hundreds place of the user 1 to 9
program number to be called. If "3" is specified, G1200 to
G1299 correspond to O8300 to O.8399.
Ex.) G1256 calls O8356.
8073 For G1300 to Type 0:M98 P**** 0 to 3
G1399 1:G65 P****
2:G66 P****
3:G66.1 P****
8074 Program No. Specify the numerical value for the hundreds place of the user 1 to 9
program number to be called. If "5" is specified, G1300 to
G1399 correspond to O8500 to O.8599.
Ex.) G1356 calls O8556.

[Note]
 G1200 to G1399 must be specified in single block. These codes cannot be specified together with any other codes
in the same block.
 A, B, C, G, M, N, O, P, S, or T cannot be used as an argument.
 The argument cannot be used when the user macro G code call type is M98.
 G, L, N, O and P cannot be used as an argument when the user macro G code call type is G65, G66 or G66.1.

13-87
L220E

13.39 DPRINT Function (POPEN, PCLOS, BPRNT, DPRNT)

Use this function to output values or characters of variables according to NC program, via RS-232C interface.

[Command format]
POPEN Preparation for data output
PCLOS End processing for data output
BPRNT Outputs characters and variable values in binary format
DPRNT Outputs characters and variable values by every digit

[Sample program]
$1
POPEN;
DPRNT [ABC #500 [53] DEF #800 [44]];
PCLOS;

Variable #500:-400.000, #800:1.2346

In [53] and [44], specify the number of digits required for integral and decimal parts.
Note: Total number of digits for integral and decimal parts must not exceed 8.
(For example, [53] represents that five digits for integral part and three digits for decimal part are specified.)

Output format to RS-232C

Communication parameter: CRLF for EOB output, 0 for feed count

DC2％CRLF
ABC-400.000DEF1.2346CRLF
％DC4

[Note]
To output data to RS-232C, be sure to specify PCLOS command to close the line. Do not terminate communication
with the line being opened by POPEN command. The line is closed by Reset command, but it is not closed at 1-cycle
stop. If an operation is attempted on the Input/Output screen while the line is open, machine operation is not
guaranteed.

13-88
 L220E

13.40 Running the Program in External Memory

Outline
This function allows the use of subprograms stored in the CF (Compact Flash) memory card. Insert the CF card into
the CF card slot at the front of the operation panel.

[Procedure]
See <6.9 Running the Program in External Memory> in the Operator's Manual.

[Command format]
M98 P H L ,D2

P Program number (1 to 99999999) of the subprogram to be called

(If omitted, the main program is called.)
H Sequence number (1 to 99999) in the subprogram to be called
(If omitted, the program is executed from the beginning of the main program.)
L The number of times (1 to 9999) the subprogram is to be repeated.
(If omitted, L1 is assumed.)
,D2 Specify this when calling a program stored in the compact flash memory card (CF).

[Sample program]

M98 P1000 L3 ,D2............................. Runs the O1000 subprogram stored in the CF card three times.

[Note]
 The programs stored in external memory can be called and executed only as subprogram. They cannot be used as a
main program.
 During the operation using the subprogram stored in the CF card, do not remove the CF card from the slot.

13-89
L220E

13.41 Collision Detection Function

When an interference is detected, this fucntion suppress the excessive torque of the motor to minimize the mechanical
damage to the machine.

CAUTION
This function is aimed to minimize the machine damage due to interference. This function does not
protect the machine from interference, nor guarantee the maintenance-free operation.

When the machine is running at rapid feed rate and the motor torque exceeds the boundary to detect a collision, this
function reduces the speed and stops the machine, then issue an alarm. This function generates a bring back torque to
pull the motor to the reverse direction by about 100 to 200 µ.
The Collision Detection Function is valid only when the machine is running at rapid feed rate (G00), not at cutting
feed rate.

Speed command
Speed
Constant speed

Acceleration Deceleration
Time

Torque
: Torque estimated from inertia
: Torque in actual operation
: Boundary to issue an alarm

Torque

Time

Torque diagram in rapid feed

The boundary for detecting collisions is set with a leeway based on the torque estimated from the inertia. If a collision
alarm has occurred, one of the following problems might be causing the alarm.
 Interference has occurred among the workpiece, tools, and machine.
 There is a load on the machine’s feed mechanism.
 The clearance between the guide bushing and the workpiece is insufficient and seizure has occurred between
them.
In these cases, take necessary measures such as reviewing the machining layout and programs, inspecting the machine,
or adjusting the guide bushing clearance.

13-90
 L220E

13.42 Optional Block Skip

13.42.1 Expansion of the optional block skip function
By specifying a number "1" to "9" following the slash code "/" at the beginning of a program block, up to nine kinds
of optional block skip can be used. Specification of a multiple block skip commands in a single block is also allowed.
If only a slash code "/" is specified without a number, it is regarded as "/1".

[Procedure]
Setting valid/invalid for the optional block skip "/1" ("/") function
1. On the Automatic Operation, On-Machine Check or MDI screen, press the menu key [Skip1].
The menu item is highlighted and the optional block skip "/1" ("/") function is enabled.
To make the function invalid, press the menu key [Skip1] again. The menu item display returns to the normal
display and the optional block skip "/1" ("/") function is disabled.

Setting valid/invalid for the optional block skip "/2" to "/9" function
2. Press the menu key [Set SW].
The Set SW screen is displayed.
3. On the Set SW screen, turn on the optional block skip switch for the optional block skip 2 to 9 functions to be
used. This enables the selected optional block skip function.
Turn off the optional block skip switch to disable the optional block skip function.

[Command format]
/1 to /9
Specification of only a slash code "/" without a number is equivalent to "/1".

[Sample program]
When optional block skip 2 is enabled.
$2
:
/2 M23 S2=3000
/2 T3100
/2 :
/2 : Optional block skip 2 *1
/2 T3300
/2 :
/2 :
M25
M16

:
*1
Turning on of the optional block skip 2 switch on the Set SW screen skips the blocks preceded by "/2" when the
program is executed.

13-91
L220E

When optional block skip 1 or 3 is enabled.

$2
:
/1 M23 S2=3000
/1 /3 T3100
/1 /3 : *1
/1 /3 : *2
/1 T3300
/1 :
/1 :
M25
M16

:
*1
Turning on of the optional block skip 3 switch on the Set SW screen skips the blocks preceded by "/3" when the
program is executed.
*2
Pressing the menu key [Skip1] on the Automatic Operation screen skips the blocks preceded by "/1" or "/" when the
program is executed.

[Note]
 Optional block skip 1 to 9 functions are invalid when the power supply to the NC operation panel is turned on.
 Although "/" is equivalent to "/1", use "/1" if several slash codes are to be specified in a block. Specification of
several slash codes in the form of "/ /3 N20 G1 X25.0", for example, causes an alarm.
 For the slash code "/", only a number in the range from 1 to 9 is allowed. Specification of "/13 N20 G1 X25.0", for
example, causes an alarm.
 For the slash code "/", a variable cannot be used instead of a number. Specification of "/#502 N20 G1 X25.0", for
example, causes an alarm.
 For the slash code "/", only an integer can be used. Specification of "/1.2 N20 G1 X25.0", for example, causes an
alarm.

13-92
 L220E

13.42.2 Optional block skip M code (M238)

By specifying M238, it is possible to skip program blocks between M238 and a sequence number.
The optional block skip function, specified by the slash code "/", can be used together.

[Command format]
M238 A1 to 9
N9991 to N9999

[Argument]
 A number (1 to 9) that follows the A argument corresponds to the last digit of a four-digit sequence number (9991
to 9999). The combinations of an A argument and a sequence number are "A1 and N9991", "A2 and N9992", "A3
and N9993" to "A9 and N9999".
 If the A argument is omitted, it is regarded as A1.
 Sequence numbers N9991 to N9999 must not be used for other purposes. If a sequence number in this range is
used incorrectly, blocks will be skipped unexpectedly.

[Sample program]
When optional block skip 2 is enabled.
$2
:
M238 A2
M23 S2=3000
T3100
:
: Optional block skip 2 *1
T3300
:
:
N9992
M25
M16

:
*1
Turning on of the optional block skip 2 switch on the Set SW screen skips blocks from M238A2 to N9992 when the
program is executed.

13-93
L220E

When optional block skip 1 or 3 is enabled.

$2
:
M238 (A1)
M23 S2=3000
M238 A3
T3100
: *1
: *2
N9993
T3300
:
:
N9991
M25
M16

:
*1
Turning on of the optional block skip 3 switch on the Set SW screen skips blocks from M238A3 to N9993 when the
program is executed.
*2
Pressing the menu key [Skip1] on the Automatic Operation screen skips the blocks from M238 (A1) to N9991 when
the program is executed.

13-94
 L220E

13.43 Thermal Displacement Correction Function

The thermal displacement correction function observes the components of machine and predicts the amount of thermal
displacement of the machine. This function automatically adds the correction amount to the tool positioning
coordinate.
By using this function, the amount of thermal displacement can be reduced at the cold start or during halting state.
If a tool is selected by T code, it is positioned to the point where the thermal displacement correction amount is
reflected. This reflection is performed internally in the NC unit. Thus, tool wear compensation and shape
compensation can be performed as usual.
Target axes
 X1 axis (T01 to T05): when 5 turning tools are used
 X2 axis (T31 to T35)

[Note]
 Correction will be performed on the target axis only.
This function is unavailble for rotary tool on gang tool post.
 If the tool is positioned without using the T code command, the amount of thermal displacement correction will
not be reflected.
 The amount of thermal displacement correction is updated at the cycle start, when M2 is specified, or when the bar
stock change is executed.
Accordingly, the amount of thermal displacement correction is not changed within a cycle operation.
 After enabling the thermal displacement correction function, be sure to perform cutting to check the size of
machined workpiece.

13.43.1 Environmental requirements and restrictions on use

Required environmental conditions for thermal displacement correction function are as follows:
In an environment where the temperature is out of this range or obstruction frequently occurs, the thermal
displacement correction function may not work correctly. In such a case, disable this function.

Environmental condition
 Ambient temperature at site: 10 to 30°C
 Range of temperature change in a day: Within 10°C

The default setting of thermal displacement correction function is "Enabled". However, some restrictions are imposed
on using this function as described below.

* For how to enable or disable the thermal displacement correction function, see <13.43.2 Setting thermal
displacement correction function>.

Restrictions
 The thermal displacement correction function is unavailable if water-soluble coolant is used.
Disable the thermal displacement correction function.
 The correction results may not be constant even if the same machining program is used, due to characteristics of
the thermal displacement correction function.

13-95
L220E

13.43.2 Setting thermal displacement correction function

Use Machine Structure screen to enable or disable the thermal displacement correction function.

[Procedure]
1. Press the Manual select key or Preparation key to enter the EDIT mode.

2. Open the Machine Structure screen.

Press the Parameter key and press the Menu selection key several times until the menu key [MC-STRCT]
appears. Then, press the menu key [MC-STRCT].
3. Set the thermal displacement correction function.

When the following screen appears, press the menu key [Set].
Use the Arrow keys to move the cursor onto "T.D.C. FUNCTION", and press the Input key to
put a checkmark in checkbox.
 : Enabled state
: Shows Disabled state
4. Be sure to power on the machine to make effective the new setting.

13-96
 L220E

13.44 B Code Function (MB)

The B code function is used to control external peripheral equipment via I/O.

[Command format]
MB B code command

：Specify any integer.Specify an integer between 1 and 255.

Enter a value between 1 and 255 in the box after "MB" and the corresponding binary Y output signal will go on (1).
Y87 Y86 Y85 Y84 Y83 Y82 Y81 Y80
MB1 0 0 0 0 0 0 0 1
MB2 0 0 0 0 0 0 1 0
MB3 0 0 0 0 0 0 1 1
MB4 0 0 0 0 0 1 0 0
･･･

･･･
MB255 1 1 1 1 1 1 1 1

For example a "MB3" specification will result in "00000011" and the Y81 output signal (I/O:Y8.1) and the Y80
output signal (I/O:Y8.0) go on (1). And when the common X input signal X82 (I/O: X8.2) is on (1), the above Y
output signal goes off (0).

[Note]
 Only 1 B code can be executed per block.
 The B code command in a multi-axis system can be executed independently for each system.

13-97
L220E

13.45 Simultaneous Machining

The Z1 and Z2 axes can be specified independently. This enables free simultaneous machining. The way to machine
with superimposition and the way to machine without superimposition are available for simultaneous machining.

13.45.1 Simultaneous machining for outer and inner diameters

For the simultaneous machining, perform the outer diameter machining by T02, and the hole machining by a T21
(recommended), T22 on T03 tool. However, some restrictions for stroke exist depending on the relation between the
tool shape and the diameter of front drilling tool.
Interference may occur if another combination of tools are used for simultaneous machining.
 Select tools for each axis control group ($1 (gang tool post) and $2 (opposite tool post)) by the ordinary T
command.
 After machining is complete, be sure to move the tool to the positioning point.
 The machining is performed at the feed rate (F) specified in each axis control group.
As shown in the figure below, the machining is performed by combining the vertical tools and the tools on the
opposite tool post.

T11
T05 T04 T03 T02 T01
T12
T09 T08 T07
T21/T24
T22/T25
T23/T26

T13

T14

Figure 1 Simultaneous machining for outer and inner diameters

[Note]
 The opposite tool post assumes tools whose maximum drilling diameter is 10 mm. Be careful when using tools
exceeding the diameter or odd-shaped tools because they have potential risk of interference.
 Be careful in simultaneous boring with the opposite tool post, when the gang tool and the tool on the opposite tool
post are off-centered, causing some tools to interfere with each other.
 When GSE1407 (rotary cross-machining tool) is mounted on opposite tool post, the tool may interfere with the
guide bushing. Move the Z2 axis 20 mm to the negative (–) direction to avoid an interference.

13-98
 L220E

Outer diameter cutting and drilling simultaneous machining

Outline of machining

φ16 φ10 φ12

17
0.5 1.0 15 30
Returns by G600.

[Sample program]

Machining process

$1 $2
T0200 T2100 ............... Tool selection (in both axis control groups 1 and
2)
G00 Z–0.5 ............... Rapid feed positioning
(in longitudinal direction) For axis
X8.0 ............... Rapid feed positioning control group
(in diametrical direction) 1 only
G01 X10.0 Z0.5 F ............... Chamfering (C0.5)
Z15.0 ............... Cut to the position of 15.0 in the longitudinal
direction.
G620 G620 Z–1.0 ............... Z1-Z2 superimpose
X11.0 G01 Z17.0 F ...............
Drilling in axis control group 2
X12.0 Z15.5 G00 Z–1.0 ...............
Z30.0 ............... Outer diameter cutting in axis control
group 1
X17.0 Z31.0 ...............
G600 G600 ............... Z1-Z2 superimpose command OFF (Axis
control group 1)
Return the opposite tool post to machine zero
point. (Axis control group 2)

Machining process

13-99
L220E

Outer/Inner diameter simultaneous machining (boring)

Outline of machining

φ20.0
φ7

12
0.5 φ16.0
φ19.0
Returns by G600

[Sample program]

Machining process

$1 $2
T0200 T2100 ............... Tool selection (in both axis control groups 1 and 2)
G00 Z–0.5 ............... Rapid feed positioning
(in longitudinal direction)
X14.0 ............... Rapid feed positioning
Operates in axis
(in diametrical direction)
control group 1 only.
G01 X16.0 Z0.5 F ............... Chamfering (C0.5)
Z11.0 ............... Cut to the position of 11.0
in the longitudinal direction.
G620 G620 Z–0.5 ............... Z1-Z2 superimpose (opposite tool post positioning in
longitudinal direction)
X17.0 G50 U ............... Cut to ø17.0 Coordinate system shift
ON
X19.0 Z12.0 G00 X9.0 ............... Chamfering (C1.0) Rapid feed positioning
Z30.0 G01 X7.0 Z0.5 F ............... Cut to the position Inner diameter
of 30.0 in the $1 chamfering (C0.5)
longitudinal direction.
X21.0 Z31.0 Z12.0 F ............... Move to the outer Cut to the position of $2
diameter while 12.0 in inner diameter in
chamfering and cutting. the longitudinal
direction
X5.8 F ............... Cut to ø5.8 in diameter.
(Move the tool bit away.)
G00 Z–0.5 ............... Return in rapid feed.
G50 U– ............... Coordinate system shift OFF
G600 G600 ............... Z1-Z2 superimpose command OFF (Axis control
group 1)
Return the opposite tool post to machine zero point.
(Axis control group 2)

Machining process

13-100
 L220E

13.45.2 Pinch Milling

Use the GSC1407 cross rotary tool for pinch milling using the vertical tool and the front rotary tool on the opposite
post.
Mount the GSC1407 on T21 and T22 to perform pinch milling with rotary tools T07 to T10 on gang tool post.
Note, however, the axis stroke may be limited depending on the tool shape, protrusion length of front drilling tool,
protrusion length of cross machining tool, and workpiece length on the back chucking device. In addition, condition to
avoid interference becomes harder if any other combination of tools are used in pinch milling.
 Select tools for each axis control group ($1 (gang tool post) and $2 (opposite tool post)) by the ordinary T
command.
 After machining is complete, be sure to move the tool to the positioning point.
 The machining is performed at the feed rate (F) specified in each axis control group.
The pinch milling is performed by using the vertical tool along with the tool on opposite tool post, as shown in the
figure below.

T09

T09 T08 T07

T11
T05 T04 T03 T02 T01
T12
T22 T21
T13

T14 T25 T24

Figure Tool layout pattern for pinch milling

[Note]
 The tool on opposite tool post is intended to drill a hole up to ø10 mm. An interference may occur depending on
tool of larger diameter or tool shape. Care must be taken.
 When GSE1407 (rotary cross-machining tool) is mounted on opposite tool post, the tool may interfere with the
guide bushing. To machine the workpiece with the end-face tool on opposite tool post, move the Z2 axis 20 mm to
the negative (–) direction to avoid an interference.
 The BSE607, BSE707 and GDF1207 cannot be used together with the GSE1407.
 In pinch milling, the workpiece chucked by the back spindle may interfere with the vertical tool. Pay strict
attention to protrusion length of rotary cross-machining tool and outer diameter of workpiece. Collect the
machined workpiece first, then perform the pinch milling.
 If the vertical tool is equipped with slitting cutter, it may interfere with the end-face machining tool on opposite
tool post.
 To put the end mill through the Y axis direction, the workpice on front side may interfere with the cap nut of
end-face machining tool on opposite tool post if the workpiece is protruded 45 mm or more.
 If the protrusion length of tool is shorter than 30 mm, the stroke will be limited depending on combination of
vertical tool and the tool on opposite tool post, to avoid interference between tools.
 Pay strict attention to interference when machining the workpiece by moving the upper and lower milling tool in
opposite direction.
 If the shift tool holder GTF3312 or GTF3313 is used, it will interfere with the workpiece chucked by the back
spindle. Perform product collection before starting pinch milling.
 If U35B and GSE3210 are used together, the angle of rotary tool is limited to 45° to 90°.

13-101
L220E

13.45.3 Pinch Turning

The pinch turning with the vertical tool and the tool on opposite tool post can be performed. Mount the SAU1019
sleeve adapter on T26 and the vertical tool equipped with GTF3312 (or GTF3313) shift tool holder (15-mm shift) on
T02, T03, or T04. (Mounting on T03 is recommended.)
Use the tool of 10-mm shift as shown in the figure below. Set the tool nose to the position 109 mm away from the tool
mounting end face of opposite tool post.

 Select tools for each axis control group ($1 (gang tool post) and $2 (opposite tool post)) by the ordinary T
command.
 After machining is complete, be sure to move the tool to the positioning point.
 The machining is performed at the feed rate (F) specified in each axis control group.
The pinch turning is performed by using the vertical tool along with the tool on opposite tool post, as shown in the
figure below.

T21
T11 T05 T04 T03 T22
T02
T12 T01
T09 T08 T07 T25 T24
T13

T14

Figure Tool layout pattern for pinch turning

[Note]
 To perform the pinch turning along with the pinch milling, mount the GSC1407 rotary cross-machining tool on
T21. Perform the pinch turning with the combination of T26 and T02.
An interference will occur in any other combination of tools.
 The SAU1019 cannot be used on the machine equipped with U126B (deep-hole drilling on opposite tool post).
Use the SAU919 to perform pinch turning.
The stroke and the tool layout may be limited on using SAU919.
 To set the tool nose upward and perpendicularly in pinch milling, the tool nose position in longitudinal direction
differs from that of T20's end-face drilling tool used generally.
(Tool nose position in pinch milling = T20's end-face drilling tool position + 2 mm)
Strict care must be taken when setting a tool or changing a program.

13-102
 L220E

13.46 Major restrictions of tooling setup

This chapter shows the major restrictions of tooling setup.

The restriction on back tool post.

The restriction of length of the tooling on back tool post.

Max distance of tool nose 【Reference】

from U155B surface Max tool protrusion length
L1 [mm] L2 [mm]

GDS210 30
T31
GSE3507 20
62
GDS210 30
T32
Upper GSE3507 20
position GDS210 44 (ø8.0、M6)
T33
Back tool GSE3507 34 (ø5.0、M4)
post 74
GDS210 44 (ø8.0、M6)
(U155B) T34
GSE3507 34 (ø5.0、M4)
T35 GDS210
62 30
Lower T36 GDS210
position T37 GDS210
74 44 (ø8.0、M6)
T38 GDS210

L1

L2

L2

13-103
L220E

The restriction of the toolings on opposite tool post in case cross drill spindle (GSC1507/GSS1530) is mounted on
back tool post.

Back tool post (U155B)

GSC1507 GSS1530
T31 T32 T33 T34 T34
T21 (T24) × × ○ ○ ○
Opposite tool post
T22 (T25) × × × ○ ○
（U125B,U126B,U128B)
T23 (T26) × × × △ ×
○：No restriction on opposite tool post.
△：Only center drilling is possible by opposite tool post.
×：No machining is possible by opposite tool post.

Restriction of Pinch-milling
 GDF1207, BSE607, BSE707 cannot be mounted.
 Need to collect the work-piece on the back spindle before Pinch-milling if shift bite holder (GTF3312, GTF3313)
is mounted.
 Position the B-axis tool (MEU307) at a 90° angle.

Gang tool post

GSC1310
T7 T8 T9
T21 ○ ○ △
Opposite tool post
T22 ○ ○ △
（U128B)
T23 ○ ○ ○
○：Need to collect the work-piece on the back spindle if its protrusion length is or is longer than 17mm.
△：The workpiece on the back spindle and the tool on the gang tool post interfere with each other. Collect the
workpiece before start of processing.

13-104
 L220E

（Blankpage）

13-105
L220E

Product Code C-L220E XII

Document Code 2E1-1301
Mfg. No. L220E/0001 ~
Issue Date 2014.1

13-106