hitachi seiki ST200, ST 250 Programming Manual

ST200/250

CNC LATHE

PROGRAMMING

65 Edition 1.01

PM-1782-1-0300-E-1-01

Hitachi Seiki Deutschland Werkzeugmaschinen GmbH

Introduction

Thank you for your having purchased the machine, favoring our product lines for your use. This manual contains fundamental information on the programming. Please read and fully understand the contents for your safe machine operation. In particular, the content s of the items concerning safety in this manual and the descriptions on the “caution plates” attached to the machine are important. Please follow the instructions contained and keep them always in mind to ensure safe operation. The reference record papers on adjusting setting values such as a parameter list are attached to the machine unit and enclosed in the packing. These are necessary for maintenance and adjustment of the machine later on. Please keep them safely not to be mislaid. The design and specifications of this machine may be changed to meet any future improvement. As the result, there may arise some cases where explanations in this manual could become partly inconsistent with the actual machine. Please note this point in advance. In this manual, items on the standard and optional specifications are handled indiscriminately. Please refer to the “delivery note” for the detailed specification of your machine confirmation.

CONTENTS

1. PREPARATION FOR TOOL LAYOUT ....................................................................... 1 - 1

1-1 Tool Set..............................................................................................................................1 - 2

1-2 Tool Layout ........................................................................................................................ 1 - 4

1-3 NC Address and Range of Command Value .....................................................................1 - 5

2. PROGRAMMING........................................................................................................ 2 - 1

2-1 Basis for Programming ....................................................................................................2 - 1

2-1-1 Program Reference Point and Coordinate V alues.................................................... 2 - 1

2-1-2 Regarding Machine Zero Point.................................................................................. 2 - 2

2-1-3 Program Example..................................................................................................... 2 - 3

2-2 Details of F, S, T and M Functions.................................................................................... 2 - 4

2-2-1 F Function (Feed Function) ...................................................................................... 2 - 4

2-2-2 S Function (Spindle Function)...................................................................................2 - 5

2-2-3 T Function (Tool Function)........................................................................................ 2 - 8

2-2-4 M Function (Miscellaneous Function) List............................................................... 2 - 12

2-3 Details of G Function ...................................................................................................... 2 - 20

2-3-1 List of G Function.................................................................................................... 2 - 20

2-3-2 G50 Maximum Spindle Speed Setting..................................................................... 2 - 23

2-3-3 G00 Positioning ...................................................................................................... 2 - 23

2-3-4 G01 Linear Cutting.................................................................................................. 2 - 25

2-3-5 G02, G03 Circular Cutting ...................................................................................... 2 - 27

2-3-6 G04 Dwell ............................................................................................................... 2 - 31

2-3-7 G09 Exact Stop....................................................................................................... 2 - 31

2-3-8 G61 Exact Stop....................................................................................................... 2 - 32

2-3-9 G10 Programmable Date Input............................................................................... 2 - 32

2-3-10 G20, G21 Inch Input/Metric Input ........................................................................... 2 - 33

2-3-1 1 G22, G23 Stored S troke Limit.................................................................................2 - 34

2-3-12 Stroke Limit Check Before Move........................................................................... 2 - 35

2-3-13 G28 Automatic Reference Point Return................................................................ 2 - 36

2-3-14 G30 2nd Reference Point Return ......................................................................... 2 - 36

2-3-15 G31 Skip Function ............................................................................................... 2 - 39

2-3-16 G54 Work Coordinate System Setting (Work Length).......................................... 2 - 40

2-3-17 Canned Cycle ....................................................................................................... 2 - 41

2-3-18 Multiple Repetitive Cycle ....................................................................................... 2 - 50

2-3-19 G32, G92, G76 Thread Cutting ............................................................................. 2 - 68

2-3-20 G32 Continuous Thread Cutting .......................................................................... 2 - 88

2-3-21 Multi-thread Cutting............................................................................................... 2 - 89

2-3-22 G34 Variable Lead Thread Cutting....................................................................... 2 - 90

2-3-23 G150, G151, G152 Groove Width Compensation................................................ 2 - 91

3. AUTO MATIC CALCULATING FUNCTION OF

TOOL NOSE RADIUS COMPENSATION ................................................................. 3 - 1

3-1 Outline ............................................................................................................................... 3 - 1

3-2 Preparation to Execute the Automatic Calculating Function of Tool Nose Radius Compensa-

tion .................................................................................................................................... 3 - 2

3-3 Three Conditions of Nose Radius Compensation ............................................................. 3 - 3

3-3-1 Tool Nose Radius Compensation Block (During Cutting) .......................................... 3 - 4

3-3-2 Start-up Block and Compensation Cancel Block (Approach/Retreat) ....................... 3 - 6

3-4 Caution Point of Approach to W orkpiece.........................................................................3 - 10

3-5 Tool Nose Radius Compensation to Direct Designation G Code (G141, G142).............. 3 - 1 1

4. PROGRAM EXAMPLE (NC PROGRAM) .................................................................. 4 - 1

4-1 Chuck Work ...................................................................................................................... 4 - 1

4-1-1 Machining Drawing .................................................................................................... 4 - 1

4-1-2 Chuck Work Program................................................................................................ 4 - 2

4-2 Center Work ...................................................................................................................... 4 - 6

4-2-1 Machining Drawing .................................................................................................... 4 - 6

4-2-2 Center Work Program ............................................................................................... 4 - 7

4-3 Bar Work ...........................................................................................................................4 - 9

4-3-1 Machining Drawing .................................................................................................... 4 - 9

4-3-2 Bar Work Program .................................................................................................. 4 - 10

4-4 Grooving .......................................................................................................................... 4 - 12

4-4-1 OD Grooving............................................................................................................ 4 - 12

4-4-2 ID Grooving.............................................................................................................. 4 - 13

4-4-3 End Face Grooving.................................................................................................. 4 - 15

4-5 1st and 2nd Process Continuous Machining Method ...................................................... 4 - 16

4-5-1 Machining Method by Single Program...................................................................... 4 - 17

4-5-2 Machining Method by Subprogram Calling............................................................... 4 - 18

4-6 Operation Example of Many Short Length Works ........................................................... 4 - 19

5. REFERENCE MATERIALS ....................................................................................... 5 - 1

5-1 How to Calculate the Tool Nose Radius Compensation Amount Without Using the Tool Nose

Radius Compensation Function........................................................................................5 - 1

5-2 Calculation Formulas ...................................................................................................... 5 - 10

5-2-1 How to Obtain Side and Angle of Right T riangle....................................................... 5 - 10

5-2-2 How to Obtain Side and Angle of Inequilateral T riangle............................................ 5 - 12

5-2-3 How to Obtain Taper and Intersecting Point of Circular Arc..................................... 5 - 13

5-2-4 Others ..................................................................................................................... 5 - 17

1. PREP A RATION FOR TOOL LAYOUT

There are limit of range of travel and other limits according to the machine specifications and safety. Refer to “Specifications Manual” of each machine type for stroke, work operation range, tool interference diagram and Q setter•work interference diagram of the machine, which should be fully understood as they are premises for machine operation, programming and tool layout.

1 - 1

1-1 Tool Set

Standard Tool Set

In order to keep operation procedure of the work and to avoid interference of the tool and the chuck large tools such as the base holder shall be set permanently.

Further, set the tools as you like in order to satisfy the operation accuracy of the small tools such as the boring bar, and also to perform the turret indexing by one rotation.

The standard tool set is shown as below.

T08 ID grooving

T07 OD grooving

T06 ID rough boring

T09 OD and face finishing

T10 ID finishing

T11 OD threading

T12 ID threading

T05 OD profiling or face grooving

T03 OD profiling or face grooving

T01 Rough cutting for face and OD

T02 Center drill or Starting drill

Specifications of 12-station Variable turret

T04 Drill

1 - 2

Standard Tool Set

T07 OD grooving

T09 OD and face finishing

T10 ID finishing

T11 OD threading

T08 ID grooving

T06 ID rough boring

T05 OD profiling or face grooving

T04 Drill

T03 OD profiling or face grooving

T12 ID threading

T02 Center drill or Starting drill

T01 Rough cutting for face and OD

Specifications of 12-station QCT turret

1 - 3

1-2 Tool Layout

Example of tool layout for chuck work

Process : Process 1, 2

NC unit

CNC LA THE: TOOL LAYOUT DRAWING

Part name SAMPLE

Material S48C

R0.8

OD roughing

T1 T3 T5 T7 T9

Width 2mm

OD grooving

R0.8

OD finishing

OD threading

T2 T4 T6 T8 T10

R0.8

φ20 ID finishing

φ25 ID threading

φ30

R0.8

φ20 ID roughing

1 - 4

1-3 NC Address and Range of Command Value

Function Address Range of command value Program No. O 1~99999999 Sequence No. N 1~99999999 Preparatory function G 0~999 Coordinate value X, Y, Z, U, V, ±99999.999(mm) ±9999.999(inch)

W, I, J, K, Q, ±99999.999(deg) ±99999.999(deg)

R, A, B, C Feedrate F 0.001~999.999(m/rev) 0.0001~99.9999(inch/rev) Spindle function S 0~99999999 Tool function T 0~999999 Auxiliary function M 0~99999999 Dwell P, X, U 0~99999.999(sec) Call up program No. P 1~99999999 Number of repetition L 1~99999999

1 - 5

1 - 6

2. PROGRAMMING

2-1 Basis for Programming

2-1-1 Program Reference Point and Coordinate Values

For a CNC lathe, coordinate axes X and Z are set on the machine and their intersecting point is called a “program reference point”. The X axis assumes a spindle center line to be a position of “X0”, and the Z axis assumes a workpiece finish end face on the tail stock side to a position of “Z0”.

To move a tool, specify its moving position, adding signs “+” and “−” to both X and Z axes, with this program reference point as a datum point.

•Position of the tool A ...

Since it is locates a plus 50 dia. on the X-axis and plus 35mm (1.4”) on the Z-axis,

X50.0 Z35.0 ..... (Omit the plus sign)

•Position of the tool B ...

Since it is locates a plus 80 dia. on the X-axis and minus 25mm (1.0”) on the Z-axis, X80.0 Z−25.0

2 - 1

2-1-2 Regarding Machine Zero Point

Properly speaking, the machine zero point and reference point is a different position, however, as for our NC lathe make the both points the same position.

Therefore, here in after the reference point calls as the machine zero point in this manual. It is a position which is the machine proper and the machine zero point which is the basis

of program set the end of each axis. This machine zero point utilizes an electrically identical point, a grid point, and stop a

servo motor at the certain point. Turn on the power at the starting time in the morning, it can be entered a program

operation .

2 - 2

2-1-3 Program Example

NC Program

2 - 3

2-2 Details of F, S, T and M Functions

2-2-1 F Function (Feed Function)

G99 mode F ooo.ooo(Up to 6 digits in increment of 0.001) mm/rev Specify a cutting “feed rate” per spindle revolution or a lead of the threading.

(Example) 0.3 mm/rev = F0.3 or F30

1.0 mm/rev = F1.0 or F100

1.5 P thread = F1.5 or F150 In case of thread cutting, it is possible to command down to 5 digits of decimals. F

ooo.ooooo(0.00001 unit; max. 8 digits)

Max. feed rate 5,000mm/min. A maximum feed rate depends on the spindle speed used.

Assuming the spindle speed to be N;

5000

(Example) When the spindle speed is 1,000 rpm, the maximum feed rate is;

G98 mode F mm/min Feed rate per minute

oooooo A decimal point cannot be used.

Generally, you specify a feed rate per spindle revolution for in case of turning. However, if specified in the G98 mode,

(Example) 200 mm/min = F200

5000

1000

= 5.0 F = 5.0 mm/rev

a feed rate per minute is set.

2 - 4

Notes) 1. Since the G99 mode is set when turning on the power, you do not have to specify it,

unless G98 is to be used.

2. A cutting feed in taper cutting or circular cutting is that of a tool advance direction (tangent direction).

3. If a cutting feed in G98 mode (G01, G02, G03) is specified, the turret head moves even if the spindle is not running.

4. When commanding G98 from G99 mode or G99 mode from G98, be sure to command

F .... as well.

In case of F command is missing in the block, F value is effective which is designated just preceding block in G98, G99 mode respectively.

To be concrete, it becomes as follows: Indicate “F” that becomes effective in that block with [ ] .

(Feed per minute) (Feed per revolution) When the power is turn ON 0 0.00 N1 G99 F1.23 ; 0 [1.23] N2 —— ; 0 [1.23] N3 G98 F1000 ; [1000] 1.23 N4 —— ; [1000] 1.23 N5 G32 F2.34567 ; 1000 [2.34567] N6 —— ; 1000 [2.34567] N7 G99 ; 1000 [2.34] N8 —— ; 1000 [2.34] N9 G98 ; [1000] 2.34 N10 —— ; [1000] 2.34 N11 G32 ; 1000 [2.34567]

2-2-2 S Function (Spindle Function)

Specify a spindle speed or surface speed (cutting speed) with S 4-digit numeral (S

oooo).

Command Description

oooo Max. spindle speed limit

G50S

(Example) G50 S1800 : A maximum spindle speed is limited to 1,800 (mim

oooo Constant surface speed cancel

G97S

Specify a spindle revolution with S (Example) G97 S1000 : A spindle speed per minute is set to 1,000 (mim

2 - 5

oooo .

−1

)

−1

)

G96S

oooo Constant surface speed control

When performing constant surface speed control, specify a cutting speed “V” (m/min) with an S 4-digit code (S

(Example)G96 S150 : A spindle speed is controlled to 150

oooo ).

150 m/min cutting speed at the cutting point.

..... Refer to the left figure.

* Formula for calculating the spindle speed from the

surface speed

N =

1000 × V

× D

V : Surface speed (m/min) π : 3.14 D : Tool nose position (ø mm)

-1

N : Spindle speed (mim

Spindle speed “N” at the position A = = 1193 (mim

Spindle speed “N” at the position B = = 795 (mim

Spindle speed “N” at the position C = = 682 (mim

)

1000 × 150

3.14 × 40ø

1000 × 150

3.14 × 60ø

1000 × 150

3.14 × 70ø

-1

)

-1

)

-1

)

As mentioned above, an automatic change of the spindle speed relating to the work diameter is called as the constant surface speed control.

Notes) 1. Considering a workpiece chucking condition, specify the maximum spindle speed limit

with S 4-digit code in a G50 block at the beginning of a program.

2. When roughing with G96, calculate maximum and minimum spindle speeds so that cutting will be performed in a constant power range as much as possible.

3. When changing over from G96 to G97 and vice versa, specify not only a G code, but also an S code.

4. When changed over from G96 to G97 and no S code is specified, the spindle is run with the speed specified in the latest S code in G96 mode.

5. When changed over from G96 to G97 and no S code is specified, the spindle turns with the previously used surface constant speed is S code had been specified in G96 mode.

Also, when no S code is specified in G96 mode, S results in 0.

2 - 6

6. The following interlocks are provided as the rotating conditions of spindle.

(1) The direction of the chuck inner clamp and outer clamp key shall be the same

direction as that of chuck clamping. (2) Q-setter shall be stored. (3) Rotating speed shall be command with G96 Sxxx. (4) The lamp of advance or retract of center support shall be on. (Option) (5) The door shall be closed.

2 - 7

2-2-3 T Function (Tool Function)

The tool used and its offset No. can be selected with a 4-digit number following “T”.

Turret face selection Offset No. Face 01 ~ maximum number of faces

1. Setting Coordinate of Tool-nose Position As a general usage, it is not necessary to command of offset No. Only command of

calling of turret as shown below can set the tool-nose position. Example) If the turret No. 3 is to be called, program as follows:

2. Setting Coordinate of Tool-nose Position for Arbitrary Offset No. When using an

arbitrary offset No., program as follows. Setting is done with the tool mounting position (diameter, length) of the offset No. 13. Example)

oo∆∆

T0300

T0313 Turret No. 3 Offset No. selected

Note 1. Be sure to input the tool-nose point on the tool layout screen.

2. Input “9” to the tool-nose point for drilling end-milling tool. (When a rotating tool

is equipped.)

Caution When “T ∆ ∆” command is specified on the same line as the axis travel command,

the indexing of turret is made simultaneously with traveling and a coordinate is set after completion of traveling. Be careful not to command T function together with the travel command.

2 - 8

3. Compound Offset When an adjustment is made on diametrical dimension of 50 and 70mm respectively at

the following workpiece, two or more offset can be applied on one tool.

Example 1)

T0900 G97 S2546 M08 G00 X50.0 Z10.0 M03 G96 Z3.0 S200 G01 Z−15.0 F0.2

X70.0 T0919 Compound offset Z−40.0 Offset No. 19 X84.0 T0900 Compound offset

cancel G00 G97 Z10.0 G30 U0 W0 M01

Example) Input status of dimension adjustment when the part

0.03.

OFFSET

XZRT

19 0.03 0 Note) Be sure to input zero for R and T.

Example 2) Cutting with taper of −0.3 at

T0500 G97 S2000 M08 G00 Z3.0 M03

G01 X24.0 F1.0

G00 G97 Z10.0

OFFSET

25 X-0.3 Z0 R0 T0

G30 U0 W0

0 0

φ30 part

X40.0

Z1.0 F0.2 X30.0 Z−2.0 Z−90.0 T0525 Compound offset

X57.00 T0500 Compound offset X62.0 Z−92.5 cancel X68.0

M01

φ70 is made larger by

Offset No. 25

2 - 9

4. Multi tool compensation When set up tools 2 or more on the same face on the turret described below, give

plural compensation on a face and set up the coordinate for each tool respectively.

Command system of compound compensation, different one by setting data in nose radius and control point.

(Example) N100 T0100 A tool with turret face No.1 is indexed and setting-up

〜

T0131 A tool with turret face No.1 is indexed and setting-up

〜

Note 1) When a tool, which is not required tool point and tool nose R such as drill etc., is

applied to multi tool, set a tool point as 9. (Tool nose R may be set as zero.)

2) When set the Q setter, the cursor position of tool offset coincide with the tool No. mounted on the turret face indexed at machining position at this moment.

Any No. can be selected by moving the cursor by cursor key.

Multi tool compensation and compound compensation is divided by data of tool point and tool nose R as follows:

Tool nose R and tool point of offset No. on effect the compound compensation and multi tool compensation.

is performed by the data of offset No.1.

is performed by the data of offset No.31.

and furthermore, set up tools deem as

1 Both tool nose R and tool point are zero 2 Data of tool point from 1 to 9 and setting of tool nose R

→ Compound compensation

→ Multi tool cutting

3 Tool point is zero and set a tool nose R

2 - 10

→ Alarm (No.182)

5. Program example

T01

T06

T03

Turret face No.1

Offset No.1

Turret face No.3

Offset No.3

Turret face No.6

(Compound compensation 33, 34) (Offset No.6, Multi tool

conpensation, 36)

N100 T0100 The turret face No.1 is indexed and setting-up is

〜

performed by the data of offset No.1.

M01

N300 T0300 The turret face No.3 is indexed and setting-up is

〜〜〜〜〜〜

performed by the data of offset No.3.

G01 Z− T0333 Compound compensation ON (Offset No.33)

X Z T0334 Compound compensation ON (Offset No.34)

T0300 Cancel compound compensation (Offset No.3)

M01

N600 T0600 The turret face No.6 is indexed and setting-up is

performed by the data of offset No.6.

T0636 Multi tool compensation ON (Offset No.36)

M01

Example of compensating data No. X Z R T 01 Q-setter Q-setter 0.8 3 03 Q-setter Q-setter 0.8 3 06 Q-setter Q-setter 0.4 2 33 Extremely Extremely

small amount small amount 0 0

34 Extremely Extremely

small amount small amount 0 0

36 Q-setter Q-setter 0.4 2

2 - 11

2-2-4 M Function (Miscellaneous Function) List

Please refer to the details on the Delivery specifications as to the discrimination between Standard or Option.

M code Function Description

M00

M01

M02

PROGRAM STOP

OPTIONAL STOP

PROGRAM END

This code can stop the machine during its operation, when measuring a workpiece or removing cutting chips. (The spindle and coolant also stop.) To restart, press the CYCLE START key. However, since the spindle and coolant are being suspended, specify M03/M08 in a subsequent block.

Same function as M00. An M01 command on a program can be either executed or ignored by means of the OPTIONAL STOP key on the operation panel.

Executed when a lamp is lit up. (optional stop is effective)

Sheet key

This code is used in the tape operation and is programmed at the end of the program.

Ignored when a lamp is lit off. (optional stop is not effective)

M03

M04

M05

M07

M08 M09 M12

SPINDLE FORWARD START

SPINDLE REVERSE START

SPINDLE STOP & ROTARY TOOL STOP

OPTIONAL COOLANT START

COOLANT STA RT COOLANT STOP WORK COUNT

It stops the spindle and coolant, and resets NC. Viewing from the spindle motor side, this code starts the

spindle in the clockwise direction. Viewing from the spindle motor side, this code starts the

spindle in the counterclockwise direction. This code stops the spindle.

When changing over spindle revolution from forward to reverse (or the other way), stop the spindle once with M05, and then specify M04 (M03).

This code starts discharging coolant. This code stops discharging coolant. Normally, this code starts a work counter or tool counter

to count up.

Note) : • M05 and M09 are executed after the completion of the axes travel.

• Do not specify M codes in the same block duplicately.

2 - 12

M code Function Description

M13

M14

M15 M18

M19

M23

ROT ARY TOOL FORWARD ROTATION

ROT ARY TOOL REVERSE ROTATION

ROT ARY TOOL STO P SPINDLE

POSITIONING OFF SPINDLE

POSITIONING CHAMFERING ON

The rotary tool runs in the forward direction at C-axis coupling time.

The rotary tool runs in the reverse direction at C-axis coupling time.

Stops the rotary tool spindle . Cancels M19.

Indexes the spindle by one position.

This code performs automatic thread chamfering during a threading cycle (G92). A chamfering length can be set in the parameter in increment of 0.1 L.

M24 M25 M26 M28

M30

M31

CHAMFERING OFF T AILSTOCK ADV ANCE TAILSTOCK RETRACT CENTER STOPOVER

RETRACT END OF PROGRAM,

NC RESET & REWIND

NO-WORKPIECE CHUCK& COUNT UP CHECK

When M23 is specified.

This code cancels M23.

Use when the center position detector is set.

End of the program in case of memory operation. Stops the spindle and coolant, and resets the NC unit to return the program to the beginning. Specify this code in an independent block.

1. Tool life check

2. Work quantity check of the preset work counter

3. No-workpiece check when the bar feeder is attached

2 - 13

M code Function Description

M32

M33 M34

M36

M37

M38

M39

TOP CUT CHECK

TOP CUT RESET BAR LOAD COMMAND

POWER OFF IS EFFECTIVE AT PROGRAM STOP

POWER OFF IS NOT EFFECTIVE AT PROGRAM STOP

CENTER AIR BLOW ON

CENTER AIR BLOW OFF

Block ship ON, however, block skip becomes OFF by the top cut signal ON.

Reset the top cut signal.

Power is off by command of M00, M01, M02 or M30 when the power cut off is ON.

Power does not off even the command of M00, M01, M02 or M03 when the power cut off is ON.

Air is blown to the center.

Stop the air.

M40

M41

M43

M44

M45

M46

SPINDLE LOW WINDING SELECT & CANCEL C-AXIS COUPLING

SPINDLE HIGH WINDING SELECT & CANCEL C-AXIS COUPLING

C-AXIS COUPLING ON

ROTARY TOOL COUPLING ON

ROTARY TOOL COUPLING OFF

SPINDLE OVERRIDE

30 ~ 1000min

30 ~ 6000min

-1

Switches from the cutting mode to the milling (rotary tool) mode.

The spindle override can be applied.

M47

IS EFFECTIVE SPINDLE OVERRIDE

IS NOT EFFECTIVE

The spindle override is ignores.

2 - 14

M code Function Description

M48

M49

M51

M52

M53

M54

M55

FEEDRA TE OVERRIDE IS NOT EFFECTIVE

FEEDRA TE OVERRIDE IS EFFECTIVE

SPINDLE AIR BLOW ON

SPINDLE AIR BLOW OFF

TOOL EDGE MEASURING SENSOR AIR BLOW ON

TOOL EDGE MEASURING SENSOR AIR BLOW OFF

TOOL EDGE MEASURING ARM OUT

The feedrate override can be applied.

The feedrate override is ignores.

Discharge the air at the chuck section.

Stop the air.

Air is blown to the measuring sensor section.

Air blow at the sensor section stops.

Measuring sensor swings out.

M56

M61 M62 M63 M64 M65

M66

M67

M68

TOOL EDGE MEASURING ARM RETURN

AUTO DOOR OPEN AUTO DOOR CLOSE UNLOADER ADV ANCE UNLOADER RETRACT BAR FEEDER SUPPL Y

COMP.CHECK(ASQ 80) CHUCK CLAMPING

PRESSURE IS LOW CHUCK CLAMPING

PRESSURE IS HIGH CHUCK CLOSE

Measuring sensor is stored.

The door opens by a program command. Closes the door.

This function is the bar feeder start check of bar feeder (ASQ type) made by ALPS.

The pressure of spindle chuck shift to low side.

The pressure of spindle chuck shift to high side.

The spindle chuck closes.

M69 M70

CHUCK OPEN SP ARE OUTPUT

SIGNAL

The spindle chuck opens. For bar feeder (ASQ type) made by ALPS.

2 - 15

M code Function Description

M71

M72

M73

M74

M75

M76

M81

WORK MEASURING ARM OUT

WORK MEASURING ARM RETURN

WORK MEASURING SENSOR AIR BLOW ON

WORK MEASURING SENSOR AIR BLOW OFF

CHIP CONVEYOR START

CHIP CONVEYOR STOP

ROBOT SERVICE

Work measuring sensor swings out.

Work measuring sensor is stored.

Air is blown to work measuring sensor. (In the custom macro of WORK MEASUREMENT FUNCTION)

Air blow at the measuring sensor stops. (In the custom macro of WORK MEASUREMENT FUNCTION)

Chip conveyor rotates to normal direction.

Chip conveyor stops.

ROBOT START-1

M82

M83

M84

M88

M89

M98

REQUEST-1 ROBOT SERVICE

REQUEST-2 AUTO PRESETTER

CHUCK INTERLOCK OFF

AUTO PRESETTER CHUCK INTERLOCK ON

MACHINE PROPER STANDBY

FEEDER STANDBY OFF

SUBPROGRAM CALLING

ROBOT START-2

When measuring arm swings, chuck open/close condition is neglected.

When measuring arm swings, chuck open/close condition becomes effective.

The NC unit temporarily stand by. It is restarted by cancel signal from the robot.

Robot on standing by is restarted by cancel signal from the machine. This code switches program from a main program to a subprogram.

M99

M100

SUB PROGRAM END

C - AXIS BRAKE ON

This code returns control from a subprogram to a main program. If specified in the main program, the program returns to its top.

Used during C-axis couplig. With the brake applied, spindle rotation or C-axis move are disabled.

2 - 16

M code Function Description

M101 M102

M110

M111

M122

M123

M132

C - AXIS BRAKE OFF SPINDLE FORWARD

START (CHUCKING CONDITION IS NEGLECTED)

TURRET HEAD AIR BLOW ON

TURRET HEAD AIR BLOW OFF

AIR BLOW FROM SPINDLE ON

AIR BLOW FROM SPINDLE OFF

SPINDLE THROUGH COOLANT ON

Air is blown from turret head.

Air blow from iturret head stops.

Air is blown inside spindle.

Air blow from inside spindle stops.

Dischage the coolant from spindle.

M133

M140 M141

M142

M143

M144

M145

M162

SPINDLE THROUGH COOLANT OFF

WORK SETTING CHECK M CODE EXTERNAL

FUNCTION 1 M CODE EXTERNAL

FUNCTION 2 M CODE EXTERNAL

FUNCTION 3 M CODE EXTERNAL

FUNCTION 4 M CODE EXTERNAL

FUNCTION 5 SP. ROTATE CW + AIR

Stops dischaging the coolant from spindle.

M163

BLOW ON SP. ROTATE CW + AIR

BLOW OFF

2 - 17

M code Function Description

M167

M171

M172

M173

M174

M201

M231

DOOR OPEN +SP. STOP +COOLANT STOP

AUTO DOOR OPEN (ONE SHOT)

AUTO DOOR CLOSE (ONE SHOT)

CENTER FORWARD (ONE SHOT)

CENTER RETRACT (ONE SHOT)

ROBOT SERVICE REQUEST 1

ROBOT SERVICE REQUEST 31

M260

M263

M264

M285

M286

M292

M293

WORK SETTING CHECK SOL ON (ONE SHOT)

UNLOADER FORWARD (ONE SHOT)

UNLOADER RETRACT (ONE SHOT)

SPINDLE SPEED CHANGE CONTROL ON

SPINDLE SPEED CHANGE CONTROL OFF

CENTER FORWARD OT LS DISABLE

CENTER FORWARD OT LS ENABLE

2 - 18

+ 128 hidden pages