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
2
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.
1
2
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
i
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
ii
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
N
(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
π
× 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∆∆
T
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
-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
Loading...