In the block of the plane grinding canned cycle,
when L is not commanded, or when LO is
commanded, the compensation operation is not
performed.
(2) Compensation operation
Performed for each grinding operation of the
operation sequence during the grinding canned
cycle (for each shift of X axis), and becomes
simultaneous 3 axis interpolation simulta-
neously with the shift of the X axis by
compensation of the Y axis (grindstone cutting)
direction and V axis (dresser cutting) direction.
15. COMPENSATION FUNCTIONS
The Y axis shift amout (compensation amount)
becomes a value twice the specified dressing
amout, and the V axis shift amount becomes a
value twice the specified dressing amount
(diameter).
Dresser
l-90
16. MEASUREMENT FUNCTION
16.1 Skip Function (G31)
Actual tool
------- Tool path without skip signal
Linear interpolation can be designated as in
GO1 by programming axis movement following
G31. Input of the skip signal during execution
of this command interrupts the rest of the block
and executes the next block. G3l is one-shot
command, effective only in the block
concerned.
The custom macro can use the coordinate
values of the position where the skip signal
was issued, since they are stored in system
variables #5061 and #5062 of
macro.
the custom
#5061 . . . . X coordinate value
#5062 . . . . ZN coordinate value
#5063 . ..- Z coordinate value (Only M series)
The skip function can be used when the
movement amount is not clear, as in fixed
amount feed by grinder.
16.2 High-speed Skip Signal Input
Delay and error of skip signal input is 0 - 2
msec at the NC side (not Considering those at
the PMC side).
This high speed skip signal input function
keeps this value to 0.1 msec or less, thus
allowing high precision measurement. This
signal is connected directly to the NC; not via
the PMC.
16. MEASUREMENT FUNCTIONS
16.3 Tool Length Measurement
Difference set as
Call offset value display screen on the CRT.
Relative positions are also displayed on this
screen. Reset the displayed relative position to
zero. Set the tool for measurement at the
same fixed point on the machine by hand.
The relative position display at this point shows
difference between the reference tool and the
tool measured. The relative position display
value is then set instead of numerals as offset
amounts, with the same operation as offset
amount setting.
16.4 Automatic Tool Offset
A Tool offset value
Cr edict ed Measuring measuring position position
G36Xxa ; or G37Zzc~ ; + Revision of offset amount -
When a tool is moved to the measurement
position by execution of a command given to
CNC, the CNC automatically measures the
difference between the current coordinate
value and the coordinate value of the commnad
measurement position and uses it as the offset
amount for the tool. When the tool is moved to
the measurement position in offset mode and
an amount to be further offset is generated as
the result of the measurement, the current
off set amount is further offset. When the tool
geometry offset & tool wear offset option is
selected, the tool wear amount (wear offset
amount) is compensated.
1-91
16. MEASUREMENT FUNCTIONS
(1) Coordinate system
When moving the tool to a position for
measurement, the coordinate system must be
set in advance. GSOXxZz ; sets the coordinate
system. (Automatic coordinate system setting
may be designated.) (The work coordinate
system for programming is used in common.)
(2) Movement to measurement position
A movement to a measurement position is
performed by specifying G36Xxa or G37Zza in
the MDI or AUTO mode. In this case, the
measurement position should be xa or za
(absolute command).
Execution of this command moves the tool at
the rapid traverse rate toward the measurement
position, lowers the feed rate halfway, then
continues to move it until1 the approach end
signal from the measuring instrument is issued.
When the tool tip reaches the measurement
position, the measuring instrument sends a
signal to the CNC which stops the tool.
(3) Offset
The current tool offset amount is further offset
by the difference between the coordinate value
(a, p) when the tool has reached the
measurement position and the value of xa or za
specified in G36 Xxa or G37Zza.
Offset amount x
= current offset amount x + (CT - xa)
Offset amount z
= current offset amount z + (j3-za)
These offset amounts can also be altered from
the MDI keyboard.
(4) Feed rate and alarm
The tool, when moving from the starting
position toward the measurement position
predicted by xa or za in G36 or G37, is fed at
the rapid traverse rate across area 0. Then
the tool stops at point T (xa - yx or za - yz) and
moves at the measurement feed rate set by
parameter across areas @, 0 and 0. If the
approach end signal turns on during movement
across area @I, alarm No. 80 is generated. If
X
F, Predicted
measyring position . I
Of Start point
Z @ 1. 03 WV
S or ZS) T ’ i .
14 Ixa- xsl or iza- zsl xa or za
FR : Rapid traverse rate Fp : Measurement feedrate (set by parameter)
the approach end signal does not turn on
before point V, the tool stops at point V and
alarm No. 80 is generated.
16.5 Direct Measured Value Input A of Tool Offset
0 Lathe A face (B face}
@I Measure ,&(a) 0 Input B(a) from MDI
1 Offset value is revised.
The following convenient method can be used
to set the offset value as the difference
between a standard point, such the tip of the
standard tool or the turret center, and the tip of
the tool actually used.
A work coordinate system is assumed to have
been set in advance.
l-92
(1)
(2)
(3)
(4)
Cut the workpiece with the tool used in
actual machining along surface A in manual
mode.
Release the tool along X axis direction
without Z axis movement and stop spindle
rotation.
Measure distance “p” between surface A
and the zero point in the work coordinate
system , and set it to the offset number
desired as the Z offset value (MZ). Cut the workpiece along surface B in
manual mode.
Release the tool along Z axis direction
without X axis movement and stop spindle
rotation.
Measure distance “a” and set it to the
offset number desired as the X offset value
(MX)=
Repeat the above operation for each tool used.
If the coordinate value of the tool as surface B
is 105.0, the measured distance a is 104.0 and
104.0 is set to offset number 3 of address X as
MX, the offset value 1 .O is automatically set to
offset number 3 of address X.
(Note 1) This function is effective only when the parameter DOFSI. is set to 1.
(Note 2) The X axis must always be measured in diameter.
(Note 3) When the measured value is input
as the geometry offset amount, and the
corresponding wear offset amount becomes
zero.
(Note 4) When the measured value is input
as the wear offset amount becomes zero.
Geometry offset amount does not change,
while the difference between the whole offset
amount and the geometry offset amount is set
as the wear offset amount.
(Note 5) This function can be performed by retracting both axes, when PMC and RECORD
button are provided.
16. MEASUREMENT FUNCTIONS
16.6 Offset Value Counter Input
Relative coordinate valve (CRT screen)
u 0000000
w 0000000
u Tool offset vaiue
Push the INPUT button when an address (X, Z,
U or W) but not a number has been keyed in to
set an offset value, of relative coordinate value
U (when the address is X or U) or W(when the
address is 2 or W) is set as an offset value.
This is used as follows :
( ) a
(b)
( ) C
(d)
Move a standard tool to the standard point
manually.
Reset the relative coordinate values U and
w to 0.
Move the tool to set an offset value to the
standard point.
A desired offset value can be set by setting
the offset number and pushing 4X and
INPUT button 52 and INPUT button.
16.7 Direct measured Value Input B of Tool Offset
+x
t + P .._._._. I_._._._. Touch sensor
The tool offset amount of a tool is automatically
settable into the tool offset amount memory
simply by bringing the tooi into contact with the
touch sensor by manual operation. The work
coordinate system shift amount is automatically
settable .
Preset the distance up to the measuring
position (contact face of the touch sensor) as a
reference value by a parameter using a certain
1 - 93
16. MEASUREMENT FUNCTIONS
intrinsic point on the machine tool as the
reference measureing position.
By selecting a tool whose tool offset amount is
to be measured and positioning it to the
measuring position by bringing it into contact
with the touch sensor, and sets a difference
between the reference value(parameter set
value) and the machine coordinate value at the
time into the tool offset amount memory as a
tool geometry offset value.
The
uo”.
corresponding tool wear offset value is
1 - 94
17. CUSTOM MACRO
17. CUSTOM MACRO 17.1 Custom Macro A
Regular
program
Custom macro
instruction
Custom macro body
/
\
G65Hm
P Q R ; --- A gorup of
instructions for a
certain function
The custom macro function previously loads
macro instructions created by user into
memory as subprograms, and uses them from
CNC command programs by a simple
procedure at all times.
This custom macro function can employ macro
instructions, such as CNC commands using
variables, arithmetic operation, conditional
branch, etc. as well as ordinary CNC
commands.
The following functions are applicable when
programming the custom macro body.
Variables
Representation of variables
Variables are represented by variable
numbers following # as follows.
#i (i = 1, 2, 3, . . . . ...)
Quotation of variables
Numeric values following an address can
be replaced with variables.
(Examples)
F#lO3 I..... Specifies the feedrate of #103
value.
GOOZ-#lOO . . Specifies the positioning to
the 4100 position.
G#130 I..... Specifies G code by the #I30
value.
(3)
If variable number i is replaced with
variable #j, don’t describe ##j, but describe
#9j.
(where #j = i)
(Example)
#9100 = -500 when #lOO = 105 and #IO5
= -500
Kinds of variables
Common variables
The common variables are variables
common to main programs and respective
macros to be called by these main
programs. Accordingly, a common variable
value arithmetically operated in a certain
macro can also be used in the other
macros.
System variables
The system variables mean the variables
whose applications are predetermined by
the system. The offset amount, interface
input signals, position information, and
other data can be known from the
predetermined variables. The offset
amount can also be set by substituting the
off set amount.
Macro instruction
The macro instruction is generally
represented in the following format.
G65HmP#iQ#JR
#i: Name of variable to which arithmetic
result is entered.
#j: Name of variable to be calculated (A
constant is also allowable.)
#k: Name of variable to be calculated (A
constant is also allowable.)
Hm: Operator (For details, refer to the
following table.)
(Note 1) Be careful since no decimal point is applicable to a variable value.
(Note 2) The unit of angle is 0.001 O.
1 - 95
17. CUSTOM MACRO
Macro Instructions
G code I H code I Functions I Definition
G65 I HO1 I Definition, substitution I #i = #j
G65 I HO2 I Addition #i = #j + #k
G65 I HO3 I Subtraction #i = #j - #k
I #i = #j x #k -1 I G65 I HO4 I Multiplication I G65 I HO5 I Division I #i = #j + #k I I G65 I HI1 OR I I #i = #j. OR. #k I I G65 I H12 I AND I #i = #j . AND. #k I I G65 I Hl3 I Exclusive OR I #i = #j . XOR . #k I I G65 I H21 I Square root I G65 I H22 I Absolute value I #i = I #j I I G65 I H23 I Remainder I #i = #j - trunc (#j / #k) x#k
trunc : Truncation of decimal part I #i = BIN (#j) I G65 ii24 Conversion from BCD
G65 I f-f25 I Conversion into BCD I #i = BCD (#j)
G65 H26
I I
Composite multiplication and
I #i = (#i x #j) + #k
diviation
G65 I H27 I Composite square root 1 #i = l/#+#kz G65 f-l28 Composite square root 2
I
#i = 1/#j2-#k2
I G65 I H31 I Sine #i = #j l SIN (#k) I I G65 I H32 I Cosine #i = #j . COS (#k) I rG65 1 H33 I- Tangent #i = #j l TAN (#k) I I G65 I H34 I Arc tangent #i = ATAN (#j / #k) I I G65 I H80 I Unconditional branch GOTOn I I G65 I H81 I Conditional branch 1 IF#j = #k, Go To n I I G65 1 H82 Conditional branch 2 IF#j * #k, Go To n
I G65 I H83 I Conditional branch 3 IF#j > #k, Go To n I G65 I H84 I Conditional branch 4 lF#j < #k, Go To n I G65 I H85 I Conditional branch 5 lF#j L #k, Go To n I G65 I H86 I Conditional branch 6 lF#j s #k, Go To n
Generation of P/S afarm 500 + n I G65 I H99 I P / S alarm generation
(4) Others
The following functions are available when PMC is combined as an option.
(i) Entry of 16.bit external input signals.
(ii) Output of 16-bit data to the external devices.
l-96
17. CUSTOM MACRO
17.2 Custom Macro B
(1) Use of variables Variables: #i (i = 1, 2, 3, . . . . .)
Quotation of variables: F#33 (#33: speed
expressed by variables)
(2) Operation between variables
Various operation can be done between
variables and between variables and
constants.
The following operations, and functions can
be used:
+ (sum), -(difference), *(product),/
(quotation), OR (logical sum), XOR
(exclusive logical sum), AND (logical
product), SIN (sine), COS (cosine), TAN
(tangent), ATAN (arc tangent), SQRT
(square roots), ABS (absolute value), BIN
(conversion from BCD to binary), BCD
(conversion from binary to BCD), FIX
(truncation below decimal point), FUP
(raise fractions below decimal point),
ROUND (round)
Example)
#5 = SIN #2 + #4 *3.14 + #4 * ABS
(#I 0)
(3) Control command
Program flow in the custom macro body is
controlled by the following command.
(a) If [ < Conditional expression > ] GOT0 n
(n = sequence number)
When < conditional expression > is
satisfied, the next execution is done from
block with sequence number n.
When [ <conditional expression > ] is not
satisfied, the next block is executed.
When the [ < IF conditional expression ) ]
is committed, it executes from block with n
unconditionally.
The following < conditional expressions >
are available:
#j EQ #k whether #j =#k
#jNE#k whether #j *#k
#j GT#k whether #j >#k
#j LT#k whether #j <#k
#j GE#k whether #j Z#k
#j LE #k whether #j s#k
(b) WHILE [ <conditional expression >] DO m
(m= 1, 2. 3)
END m
While <conditional expression ) is
satisfied, blocks from DO m to END m is repeated.
When <conditional expression > is no
more satisfied, it is executed from the
block next to
END m block.
Example #120 = 1 ;
WHILE #I20 LE 10 DO 1 ;
r ~~~~~~~~-------~ 7
I t I I I I I :
: : Repeated 10 times
: I
I I I #120=#120+1 ; I I I L ~~~~~~~~-------~ 4
(4) Format of custom macro body
The format is the same as the sub
program.
Custom macro body
(5) ( ) a
(b)
Custom macro instruction
Simple call
G65P (macro number) L (times to repeat)
< argument assignment ) ;
A value is set to a variable by <argument
assignment ).
Write the actual value after the address.
Example A5.OE3.2M 13.4
There is a regulation on which address (A -
2) corresponds to which variable number.
Modal call A
G66P (macro number) L (times to repeat)
< argument assignment > ;
Each time a move command is executed,
the specified custom macro body is called.
This can be cancelled by G67.
This function is useful when drilling cycles
are programmed as custom macro bodies.
l-97
Macro call by G codes
The macro can also be called by the G
codes set by parameters. Instead of
commanding:
N G65 P - < argument assignment >;
or
N G66 P < argument assignment >; ,
m&o canTe called just by commanding:
N G < argument assignment) ; .
Gcode G for calling the macro, and
macro program number P to be called,
are coupled togehter and set as parameter.
Maximum ten G codes from GO1 to G255
can be used for macro call (GO0 cannot be
used).
The G code macro call cannot be used in
the macro which was called by a G code.
It also cannot be used in sub programs
called by sub program call with M codes or
T codes.
Sub program call by M code
An M code can be set by parameter to call
a sub program. M98 P ; ,
the same operation c& be performed
simply by commanding:
N G X Y . . ..M ;. -- Asfor%l98, M codes are not transmitted.
The M code M for calling the sub
program and the sub program number
P to be called are coupled together and
sgby parameter.
Maximum three M codes from MO3 to M97
can be used for macro call (M30 cannot be
used).
Arguments cannot be transmitted. It also
cannot be commanded in the same block
as the block with M98 command.
When these M codes are commanded in
macro called by G code or in sub program
called by M code or T code, they are
regarded as ordinary M codes.
Sub program call by T code
By setting parameter, sub program can be
called by T codes. When commanded:
N G X Y . . ..Tt. , w--p
1
( 1 a
(b)
( 1 ‘C
98
17. CUSTOM MACRO
the same operation is done as when
commanded:
#I49 = t;
NGXY . . ..M98 P90000; .
The Tcoder is stored as arguments of
common variable #I 49.
This command cannot be done in the same
block with a sub program calling M code,
or with M98 command.
When T code is commanded in macros
called by G code, or in sub programs
called by M codes or T codes, the T code
is treated as ordinary T codes.
Types of variables
Variables are divided into local variables,
common variables, and system variables,
according to their variable numbers. Each
type has different use and nature.
Local variables #l - #33
Local variables are variables used locally in
the macro. Accordingly, in case of
multiples calls (calling macro B from macro
A), the local variable used in macro A is
never cleared by being used in macro B.
Common variables #1 00-#149, #500 - #531
Compared with local variables used locally
in a macro, common variables are common
throughout the main program, each sub
program called from the main program, and
each macro. The #l used in a certain
macro is the same as the #i used in other
macros. Therefore, a common variable #i
calculated in a macro can be used in any
other macros.
Common variables WOO to #149 are
cleared when power is’ turned off, but
common variables #500 to #531 are not
cleared after power is turned off.
(Note) It is possible to increase number of common variables. For details, see
” Number of common variables”.
System variables
A variable with a certain variable number
has a certain value. If the variable number
(7) ( 1 a
(b)
0 i (ii)
(iii)
(iv)
( ) V
(Vi)
(vii)
(viii)
Ox)
( ) X
( ) e
(0
(cl)
is changed, the certain value
changed.
The certain value are the following:
48 points Di (for read only)
48 points DO (for output only)
Tool offset amount, work zero point
off set amount
is also
17. CUSTOM MACRO
17.3 Custom Macro Modal Call
Position information (actual position,
skip position, block end position, etc.)
Modal information (F code, G code for
each group, etc.)
Alarm message (Set alarm number and
alarm message, and the NC is set in an
alarm status. The alarm number and
message is displayed on the CRT.)
Clock (Time can be known. A time can
also be preset.)
Single block stop, Miscellaneous
function end wait hold
Feed hold, Feedrate override, Exact
stop inhibition
Mirror image status
Limitations
Usable variables
#I - #33, #IO0 - #149, #500 - #531, and
system variables.
Usable variable values
+, 1038 - +, IO-38
Constants usable in expression
2 0.0000001 - 2 99999999
Arithmetic precision
8-digit decimal number (in trigonometrical
functions, some value may cause fail in
precision).
Custom macro body call nesting
Maximum 4 folds .
( ) nesting
Maximum 5 folds.
The full key type CRT/MD1 is used.
G66P [Macro prowam No.
The macro call mode can be specified by
executing the following command.
G66 P (program number);
The macro call mode can be cancelled by
executing the following command.
G67;
A macro designated by address P of G66 block
is called every CNC command block in the
macro call mode.
Ail commands of each block other than address
0 and N
executed.
serve as arguments without being
(Note 1) No call is done in G66 and G67 blocks.
(Note 2) No call is done even in G66 mode in the G65 block, but the command is executed
as normal macro command.
(Note 3) The macro mode and macro call cancel mode are selectable by specifying G66
and G67 in the MDI mode. However, if another
command is specified, it is processed as a
normal command without executing any macro
call.
(Note 4) Ail commands other than addresses 0, N and P specified in G66 and
G67 blocks are neglected.
(Note 5) The number of repetition times of macro call cannot be specified. For the
address P specified by G66 block, the lower
significant 4 digits only are effective.
(Note 6) The multiplicity is 1 in macro call. The multiplicity of subprograms is maximum 4.
The multiplicity is maximum 4 when macro call
and a subprogram combined with each
l-99
17. CUSTOM MACRO
17.4 Pattern Data Input
I Load variable name I
j,
PENJ: HoLE~l-lERN 01000 N1000
1. BOLT MILE 2. GRID 3. LINE m8a.E 4. TWIN 5. DRILLING 6. KRtNG
‘7. FlxKET 8. PECK 9. TEST
10. BFcK
1 Select 1 a. : BOLT HOLE 00188 NW12
WTR CUPPENT 0
501 KIJLN X *WTT HOLE 502KIJWY ii CIRCLE* 503 RRDIUS 0 sETRmERN 504 s. WGL 0 DFITQ TO UN?. 585HaE. No
4: NO. 5bzts05.
G?iih_ POSITION cRnFlTt& X 0.888 Y 0.888 2 0.000
No. 588= S 01 MD1
This function is provided to enable users to
conduct CNC machining by taking numeric
data (pattern data) only out of a drawing and
setting these numerical values from CRT/MD1
unit without any need of programming using an
existing CNC language.
With the aid of this function, a machine tool
builder can freely prepare a boring cycle
(boring cycle, tapping cycle, or the like), for
example, by utilizing the custom macro
function, and load the boring cycle into the
program memory.
(1) This cycle is designated as pattern names
like BORl, TAP3, DRL2, . . . .
An operator can select a desired pattern
out of the menu of pattern names being
displayed on CRT.
(2) A cycle should be prepared by using
variables (pattern data) which are specified
by the operator.
The operator can identify these variables
as depth, return relief, feed, blank, and
other pattern data names. The operator
gives values (pattern data) to these names.
17.5 Order-made Macro
Macro A,D I Macro b,d I Selection by 1 1 machine tools builder CNC
0tder;made macro
A machine tools builder is requested to
optionally select macros out of the standard
macro prepared by FANUC and macros
requested by the machine tool builder. These
macros are loaded into an ROM cassette. This
ROM cassette can be mounted inside CNC,
and optionally called in the programming
process.
(Note) The macro executer and order-made macro cannot be specified at the same time.
l-100
17. CUSTOM MACRO
17.6 Macro Executer 17.7 Interruption Type Custom Macro
The macro executer is a control function of
reading a macro program from the macro onnna;
cassette for execution.
It is possible to execute the following two
macro programs at the same time.
(1) Macro program called and executed by
M/T/G codes from the machining program
(2) Screen preparing macro program called by
macro screen (AUX screen) selection
The macro program should be created at the
machine tool builder side. Do this in the same
procedure as in the custom macro program
and store it in ROM cassette. Consequently,
unlike the custom macro, the macro program
does not occupy the tape storage area. Since
the macro program is converted to an
executable format for storaae, the execution
M96 Pxxxx;
Noooo; I f I I
Y .
speed is higher than that for custom macro,
thus allowing high-speed machining operation.
The macro program has the following functions:
M97;
i
; I I
Interrupt signar
(UNIT)
(1) Fl O/l l/l 2 format custom macro
(2) Generation of unique graphic screen
(3) Reading PMC status via PMC window and
outputting it to PMC
Outline of Interruption type custom macro
Entering an interrupt signal (UNIT) from the
machine during execution of a program permits
ca”-out Of another programm This function is called the interruption type
custom macro.
(Note) When a macro executer is equipped,
no order-made macro can be designated.
The interrupt command is executed by
specifying, in programming,
M96Pxxxx ;( Custom macro interrupt on)
M97 ;(Custom macro interrupt off)
This function permits any execution block of
the program to call out another program, thus
enabling program operations according to the
ever changing conditions.
l-101
18. AXIS CONTROL
18.1 Mechanical Handle Feed
Brake n
No Excitation
(Servo off)
It is possible to move the machine by hand,
using the mechanical handle installed on the
machine; not by the CNC (servo motor).
Move distance by the mechanical handle is
followed up and actual position in the CNC is
revised. The mechanical handle feed is done
by inputting the servo off signal of the axis fed.
Machine side signal desides on/off of follow up
function when servo off. However, the follow
up can not be applied when emergency stop is
on or when servo alarm is on. Inch/metric
conversion cannot be used when mechanical
handle feed function is used.
18.2 Servo Off
Servo motor Brake n
Servo on
(Servo motor drive)
Servo off
(Servo motor not drive) Mechanical u
handle
18. AXIS CONTROL
Following functions can be executed by servo
off. Workpiece install/remove fixing the
machine at stated position.
Machine operation by operator with
mechanical handle.
18.3 Mirror Image (M series)
Mirror image on+Y axis motion is inverted
18.4 X-Axis Mirror Image (T series) A
Mirror image on+X axis motion is inverted
18.5 Additional Axis Neglect
Signal from machine side (4 NG)
By the signal from machine, CNC with
additional axis can be set as if without
additional axis.
The signs of the X, Y axis motion can be
inverted in automatic operation mode.
This mirror image is effective or ineffective
according to setting parameters.
Servo on/off control per axis is possible by
signals from the machine side.
l-102
19. AUTOMATIC OPERATION
19. AUTOMATIC OPERATION
19.1 Operation Mode
(i)Memory operation
CNC Machine
* 4
ul Memory
Memory operation
r _____I 1 I I L --1--- 1
t
After the program is once registered in
memory, the machine can be run according
to the program instructions. This operation is
called memory operation.
(ii) MDI operation
CNC MDI Keyboard Machine
program input
After the program is entered, as an command group, from the MDI keyboard, the machine
can be run according to the program. This operation is called MDI operation.MDI
operation is executed by 1 block.
19.2 Selection of Execution Program
Data format in memory or on tape
.OlOOl
G92 ------e---_-
M30
01002
G92 ------______
M30
01003
G92 -~~~~~~~_~_~
- Program No.
>
Work- 1 program
- Program number
>
Wok-2 program
- Program number
1 I‘ Work-3 program
Program No. search
Sequence No.
search
Automatic operation
Program
number
search
Program number search by MD1 (0 . . ...)
Sequence
number
Sequence number (N . . ...) search by MDI
l-103
19. AUTOMATIC OPERATION
19.3 Activation of Automatic 19.5 Automatic Operation Stop Operation 19.5.1 Program stop (MOO, MOl)
Cycle start
Feed hold
Reset
Program stop
zEinate Jii?
Stop by Program end programming
Manual activation
Pressing the cycle start pushbutton causes
automatic operation start. By pressing the feed
hold or reset pushbutton, automatic running
pauses or stops. By specifying the program
stop or program termination command in the
program, the running will stop during automatic
operation. When each machining is completed,
automatic operation sops.
19.4 Execution of Automatic Operation
Pre read of 1
block
(Buffer register) 1: Execution of program 4
Buffer register equivalent to one block is
available for program read and control of CNC
command operation intervals caused by
preproces time.
MOO,MOl command
M2-digit BCD output
Y- lr .~.~.~.~.~.~.~.~. -.-.-
Waiting for FIN , .-.-.w.-.-.
OFF
tool side
I Program is continued +- I
in a block where MOO (program stop) or MO1
(optional stop) is specified, M code and M code
read signals are sent to the machine tool in the
same way as in general M codes.
Program stop processing must be done on the
machine tool side.
Set CNC to be waiting for the end signal in
case of MOO (program stop), and the CNC
stops operating.
Send the end signal to CNC by the cycle start
signal, and the program is continued.
Perform the same processing as in MOO only
when the optional stop switch is turned on by
the machine tool operator’s panel in case of
MO1 (optional stop).
I-104
19. AUTOMATIC OPERATION
19.5.2 Program end (M02, M30)
I M02,M30 command 1
t-l M2-digit BCO output Strobe signal output i-1 Waiting for FIN
*7Wpi
Machining
tool side
\ processing Turn on FIN
I 1
In a block where MO2 (end of program) or M30
(end of tape) is specified, M code and M code
read signals are sent to the machine tool in the
same way as in general M codes.
Program end processing must be done on the
machine tool side. By returning an external
reset signal to MO2 or M30, processing returns
to the start of the executing program to reset
the program.
By returning the end signal to MO2 or M30,
processing returns to the start of the executing
program to continue the execution from the
start again l
19.5.3 Feed hold
Owing Automatic operation
1 FeedholdbuttonON , ,
Automatic operation hold status
The CNC can be brought to an automatic
operation hold status by pressing the feed hold
button on the operator’s panel. When feed
hold is commanded during motion, it
decelerates to a stop.
Automatic operation can be restarted by the
cycle start button.
19.5.4 Thread cutting cycle retract
When feed hold is commanded during thread
cutting cycle by G76 or G78, the tool rapidly
relieves to the cycle start point,like the final
chamfering of the thread cutting cycle.
Thread cutting cycle restarts by cycle start
command.
Without this function, if feed hold is
commanded during thread cutting,it stops at
the end point of the block next to the block in
which thread cutting has ended.
Hold point
tij
Feed hold button was pressed here.
- Ordinary cycle
----- Move with feed hold
l-105
19. AUTOMATIC OPERATION
19.5.5 Reset
)I1
Reset signal input
22 I Reset status
The automatic operation can be ended in a
reset status by the reset button on the
CRT/MD1 panel or by the external reset signal,
etc. When reset is commanded during motion,
it decelerates to a stop.
Modal information can be initialized by the
parameter.
19.5.6 Sequence number comparison and stop
Program
c I 0001; NOOl_; N002_;
N003_;
NO04 l -’ . .
NlOO_; +
NW1 ; - . .
1 Sequence number where
single block stop is done
I NlOO
Single block stop is done
here.
When a block having the same sequence
number as the preset sequence number
appears during plotting the machining process,
the single block stop condition is set after
executing the block.
This function is effective only when graphic
drawing.
Program path
19.6 Manual Interruption during Automatic Operation
19.6.1 Handle interruption v
Machine movement
Movement commanded by handle interruption
Handle interruption is executed here.
During automatic operation, tool can be
adjusted by the manual pulse generator without
changing the mode. The pulse from the
manual pulse generator is added to the
automatic operation command and the tool is
moved for the recommended pulses. The work
coordinate system thereafter is shifted for the
pulses commanded.
Movement commanded by handle interruption
can be displayed on the CRT screen.
l-106
19.6.2 Position signal output ’
19. AUTOMATIC OPERATION
19.7 Program Restart
Machine
tool
position -10000 0 10000 20000 30000
I I I I I I
I Position : I I I I I I I I
I signal I I I I I I
output I -1 ; 0 : 1 : 2 ) I I I I I I
The full stroke of each axis of the machine tool
is divided into 256 grids respectively, and the
grid number is output as a binary 8-bit position
signal every axis according to on which grid the
machine is positioned at present.

Z)When the switch is OFF.
Y2
I Y P **-=*-- ..- . . .
P2
.  m . . . . . . w Manual
operation
The coordinate values do not change.
machining operation can be performed from the block to be restarted.
when a tool is damaged power is turned OFF once the emergency stop button is depressed once the coordinate system is changed after stopping automatic operation previously
d
When a tool is damaged, or it is desired to
restart machining after the stopping machining
once, specity a sequence No. of the block to
be restarted:
Machining will be restarted from its block.
Further, this function can be used as a high- speed tape checking function.
This switch selects whether the amount of
manual movement is to be added to the
absolute value.
l-107
20. MANUAL OPERATION
20. MANUAL OPERATION
20.1 Manual Feed
, 1 1 T series ’ 1
bl-bi Machine operator’s panel
B M series -
Machine operator’s panel
(1) Jog feed The jog feedrate can be
selected in 15 steps as tabulated below by
a rotary switch.These 15step ratios form
geometrical series.(Refer to the next table.)
(2) Manual rapid traverse The rapid traverse
is also effective during manual operation.
Manual rapid traverse is set as parameter,
but this parameter is different from the
automatic operated rapid traverse.The rapid
traverse rate preset by parameters can also
be overridden in 4 steps.
I 7 I 2.0 I 0.08 I I 2 I 3.2 I 0.12 I I 3 I 5.0 I 0.2 I
0.3
I 5 I 12.6 6
I 7 I 32 I 1.2 I
79
I 10 I 126 I 5.0 I I 11 I 200 I 8.0 I I 12 I 320 I 12 I I 13 I 500 I 20 I
14 790 30
15 1260 50
(Note) Manual pulse generator is usable in the JOG mode by a parameter.
1-108
20. MANUAL OPERATION
LU.Z Incremental Feed
n T series s
b!___2___P -j. Step value
Manual operator’s panel
Hode se let t ion &is selection Step feed
- M series I
Step value
Manual operator’s panel
MD1 +x l Y +z +a
Am~HANDLEs2ggg x;&,m EDIT JOG
Mode selection Axis wlrcrion Step feed
-L
m
l-109
b
High-efficiency positioning can be realized in
the manual mode by using the step value given
below.When the manual pulse generator
(option) is used,this function is not applicable.
I I I Input X7 Xl0 Xl00 X 1000
Metric 0.00 1 mm 0.01 mm O.lmm lmm
Inch input 0.000 0.00 0.01 inch 0.1 inch
1 inch 1 inch
input
20. MANUAL OPERATION
20.3 Manual Handle Feed
Machine operator’s panel
Hanual pulse generator
I
MODE SELECTION AXIS SELECTIOti WNDLE HULTlPLlER
b 1 M series j
work
Machine operator’s panel
0 ct
MODE SELECTION ASIX SELECTION HANDLE MULTIPLIER
By rotating the manual pulse generator, the
axis can be moved for the equivalent
distance-Manual handle feed is controlled 1
axis at a time.The manual pulse generator
generates 100 pulses per rotation. Move
amount per pulse can be specified from the
following magnifications:
xl, x10, xm
With this function incremental feed function
cannot be specified. I I 1 I 1
I Input I Xl I x10 I xm I Metric input 0.001 mm 0.0 1 mm 0.001 mm x m
Inch input 0.0001 inch 0.001 inch 0.0001 inch
Xm
Up to three manual pulse generators can be
connected. Manual pulse generator is usable in
the Jog mode by a parameter.
l-110
21 l PROGRAM TEST FUNCTIONS
21.1 Machine Lock
T series I I
Workpiece ~.~.~.~.~.~.~.~. .I._
t J
CRT / MDI I 1
x00000
/
200000
The tool remains stopped,and only the positional
displays of the axes change.
-1 M series ll I I
CRT / MDI
I I
TOOI T
x00000 LJ Y00000 The tool remains stopped,and only the positional displays of the axes change.
In machine lock condition,the machine does not
move,but the position display is updated as if
the machine were moving.
(Note 1) When the G27, G28 or G30 command is specified, the machine does not
move to the reference point and the
REFERENCE POINT RETURN lamp does not
light.
(Note 2) The M,S and T functions are
executed.
21. PROGRAM TEST FUNCTIONS
21.2 Auxiliary Function Lock
-?pI@$
If automatic operation is executed in the
condition of auxiliary function lock,the auxiliary
functions (such as spindle rotation,tool
change,coolant on/off) stop operation.
21.3 Dry Run
#m--M :
0 0
0 0
-,---------d
Dry run
1 M series 1
Table
Remove the work,check only movement of
tool. Select the tool movement rate using
dial on the operator’s panel
the
the
l-111
21. PROGRAM TEST FUNCTIONS
The feed rate specified in the program is
ignored,and the machine is fed at the following
feed rate.
k
Rapid traverse Rapid traverse
button ON/OFF Cutting feed
Rapid traverse Rapid traverse Max. JOG feed
button ON rate
Rapid traverse JOG feed JOG feed rate
button OFF t=ate( Note)
(Note) Dry run for rapid traverse can be made effective by the parameter setting.
1.4 Single Block
Cycle start Cycle stat-t I I
v v Cycle start ‘$
IJ
J Cycle start
~I=, tool
I 1
M series Cycle
start
Cycle
start
When the cycle start pushbutton is pressed,
the tool executes one operation then stops. By
pressing the cycle start again, the tool
executes the next operation then stops.The
program is checked in this manner.
(Note 1) SINGLE BLOCK is effective at an intermediate point in G28,G30.
(Note 2) SINGLE BLOCK is not effective to the block M98 ;,M99,and G65However if
M98,M99 blockshave the address other than
O,N,P,SINGLE BLOCK is effective.
21.5 Z-axis Command Cancel
Z-axis
4 . . . .
t t
. 1 t
Only the Z axis can be locked by the machine
side signal.
It is effective when using pen writing a
movement for CNC program check.
l-112
22. CRT/MD1
22. CRT/MD1
22.1 CRT/MD1 Panel
Small 9 inch monochrome CRT/MD1 (with softwares key)
O-T CRT character display (9”) Reset key
I
Data input key
I
Program - edit key
Input key
t Page change key
Function key -Start/output key
CRT character display (9”)
(b) O-M I cursor move key
Reset key Data input key
Program - edit key
Input key
I
4
I -Page
change key Function key L Start/output key
L______ CUl-SOr; move key
l-113
22. CRT/MD1
0 9 inch monochrome CRT/MD1 (without softwares key)
( 1 a O-T CRT character display Reset key Data input key
, Rogram edit key
- Input key
L wiv change key Function key Start/output key
- Cursor move key
(b) O-M
CRT character display (9”)
I Reset key
I Data input key
I
Program - edit key
I 1 --Page I change key L_____ Cursor
. move key
Input key
Function key L Start/output key
l-114
22. CRT/MD1
(3) Small 9 inch color CRT/MD1
(a) O-T
Reset key
@_ 1
Data input key
7- I
--I- - Program
edit key
- input key
Cursor move key -
Page change key -
Function key Start/output key
(b) O-M
Reset key Data input key
cl lNSR1 cl DELE - f. * cl EOB cl CAN
-Program edit key
- Input key
Function key Start/output key Cursor move key -
Page change key -
l-115
22. CRT/MD1
(4) “Full key CRTiMDlpanel
(a) O-T
Reset key Data input key
POWER
-Program edit key
Input key PACE
El i
t El WT cl 1
/ 1 f
w I
I w I I a
Cursor move key 1 Function key Start/output key
Page change key J
(b) O-M
Reset key Data input key
Cursor move key -
PACE
Program edit key
-- Input key
Page change key -
I
Function key
I
Start/output key
l-116
22. CRT/MD1
(5) CRT/MD1 panel for MMC
( > a 00-T
(b)
MMC/ CNC
Reset key Sw i th key 1 1 Shift key
c 1 f
Fun&n key
00-M
Reset key MMC/CNC switch key
\ I Shift key \ I i
! -.-_-_a
Q
SU/output key
b Program edit key
&Input key
- Start/ output key
c Program edit key
CC Input key
Function key
l-117
22. CRT/MD1
. Keyboard functions
.
No.
(1)
(2)
(3)
(4)
(5)
(6)
Name
RESET key
. START key
Address and
numerical
key
INPUT key
Cancel
(CAN) key
Cursor shift
keys
Changeover
key
Functions
Press this key to reset the CNC, to cancel an alarm, etc.
Press this key to start the MDf commands, or to start the automatic operation cycle.Since this key’s
operating method differs according to the machine tools, refer to the machine tool builder’s operation
manual.
Press these keys to input alphabetic, numeric, and other characters.
Press this key to input parameter or offset etc. and also to start inputting of 110 device, or to input
command data under MDI mode.
Press this key to delete the character or symbol input to the key input buffer.
(example):When key input buffer display is NOOOI, press the cancel (CAN) key to cancel and delete
the NO001 .
There are two kinds of cursor shift key described below.
J+ : This key is used to shift the cursor a short distance in the forward direction.
T : This key is used to shift the cursor a short distance in the reverse direction.
Two kinds of page changeover keys are described below.
J : This key is used to changeover the page on the CRT screen in the forward direction.
T : This key is used to changeover the page on the CRT screen in the reverse direction.
Function buttons
Function buttons indicate large items like chapters in a document.
 Indicates the current position.

MENU OFSET . . Setting and display of offset value.Display menu screen
DGNOS PARAM Setting and display of parameter, and display of self diagnostic data.
OPR ALARM . . . Alarm number display and setting and display of software operator’s panel.
AUX GRAPH . . . Graphic display
Several pages are included in the chapter selected with each function button. The page is selected
with PAGE button.
(Note) The data displayed on the screen disappears when one of the function buttons and the
CAN key are pressed.Thereafter, when either function button is pressed, the corresponding screen
. is displayed again.When the unit is not used with the power turned on for long time, turn off the
screen.This is effective to prevent the image quality from deteriorating.
I-118
22. CRT/MD1
22.2 Setting and Display
,
1 Screen/key
CRT / MDI
Data
I/ CNC memory
With keys, data stored in CNC memory is
updated and displayed on the screen .
22.2.1 MDI operation / MDI operation B
CRT / MDI
r , Key input
1 jScreen/ke y ] Display
X
Machine
I I Command of V _, travel
1 ’ one block
_
(T series) t .
(M series)
In MDl mode, one block operation is possible.
Also, plural blocks operation is possible for
MDI operation B (option).
1 - 119
22.
Setting data
TV check
ISO-EIA selection l
I l
0 I CNC memory
Operational . .
~jG!$~b movement
(T series) f
JuN=0 193 = 0 <0:E1A 1:IsQ ) INCH = 0 ce:r?l l:INcw
&ii =0 20
luN=s Is0 = 0 C0:EIA 1:Iso 1 --- INCH = s c0:r?l l:INcHl iizi = 0 = 0 t0:rNc l:RBs 1 SEQ =e
Apart from parameters, there is data that is set
by the operator in operation. This data causes
machine characteristics to change. For
example, it specifies the following:
(1) Setting of TV check effective/ineffective
(2) ISOEIA setting
(3) Inch/metric setting
The above data is called setting data.
l-120
22. CRT/MD1
22.2.4 Setting and display of 22.2.5 Setting and display of parameter custom macro variables
Setting
Display
CRT/MD1
CNC memory
Operational
characteristics 1
Parameter
Rapid traverse
Reference point return
system
Backlash compensation dat 0 l
0
4 Program (T series)
+ Machine
operation
IIS?
Jai& sxm l~lrn
EE. iiizzi@ 01110111
EIcB5 01110111
fzE EiiIEzz
ZEz tzEawGu1 010m1m
8810 ll6B0188
Nl. 8681=
mml-l&k 7i
(M series)
Zi ml2 ml3 ml4 8815 ml6 0017 8818 ml9
The CNC functions have versatility in order to
take action in characteristics of various
machines.For example, CNC can specify the
following:
(1) Rapid feed rate of each axis.
(2) Setting of least input increment (inch
system/metric system)
(3) Setting of CMR/DMR
Data to make the above specification is called
parameters. Parameters are characterized by
each machine tool.
w I (T series)
wIR1crB-E NO. IBTQ 1tiM IeeS 101 1CWB 182 0 103 120 104 105 5tiEdi 106 187 :
01000 Ma00 No- IBTCI 108 0 109 110 ii 111 -22ma 112 113 :
214 1m 115 0
FyTN# FUSITI(E( CFEMTICIE) U a 888 w 0.W
No. 114 = S BT IQ1
(M series)
~IQBLE 020@0lQBB _sti
DATFl No. BiTA lEEEM
101 1'iz! 40az 102 & 110 153020 103 0 111 104 123E0l :z tl 105 0 a
Common variables (#l 00-H 49, #500-#531)
can be set and displayed on CRT.
l-121
22. CRT/MD1
22.2.6 Program display 22.2.7 Program list display
1 T series a ,
Currently executed Currently executed
program number sequence number
olwe Pals5
Nmlwxlw. a. : NlWWlxae. 2%. J Nlw u-10. f Nlm lbla. : N185 m ; 4
EDxt- -
mnnnm
.
1 Program J
contents
Cursor indicates the point currently executed.
M series
Currently executed
program number
Currently executed
sequence number
/ f
Nl3B 617 641 (381 X17-S HZ? FZElB ; Nl4I3 W G39 l-17.5 i NlSB 641 683 X-17. S Y17.S R17.5 ; N160 Wl X-25. J Nl70 GB2 X27.5 KZ7.S RZ7.S : N188 Wl X-15. : Nl98 GW )(s YB :
1 Program J
contents
Cursor indicates the point currently executed.
(T series)
(M series)
oaazl N0138 SYSTEM EDITION 8488 - 81
FfaswND. Ilc;m: : rEm?Ymm l.s&D: 38Kg: m$
pf2miwl LImM?Y LIST . mml CBml mme cmMe lam%3 01234 mB2cEm3
GDRS. EDIT
L=lnllr-lII
( > a PROGRAM NO. USED: The number of the programs registered
(including the subprograms).
FREE: The number of programs which can be
registered additionally.
(b) MEMORY AREA
USED: The capacity of the program memory in
‘which data is registered (indicated by
the number of characters).
FREE: The capacity of the program memory
which can be used additionally
(indicated by the number of
characters).
(c) PROGRAM DIRECTORY:
Program Nos. registered are indicated. When
more than 48 programs are registered and PI
or P2 is designated, 48 program Nos. from the
beginning are indicated. When P3 or P4 is
designated, 48 program Nos. from the last are
indicated.
1 - 122
22. CRT/MD1
22.2.8 Current Position Display
I Work coodinate
system
\ b Over all position display
X
Position of the current tool can be displayed by
coordinate values of each coordinate
system.The distance from the current position
to the target position can also be displayed.The
actual speed can be displayed on the actual
position display screen at the same time.
(1) In the work coordinate system (T series)
00001 NOOOO X 412.526 7 618 l 882
~CaNr 1s m TIE lH17MCKLE TIrE GM ltU!S
leeet?Ml . $iz: 14 lmI
(M series)
S’IWm fJUSITI(M CWSUME)
00001 NOOOO X 226.261 Y 271.587 2 339 l 4’83
(2) In the relative coordinate system
(T series)
CIcrwL PrEfTIQJ WfiSTIE)
00001 NOOOO X 272.449 z 408.766
(M series) / Y
ClcTwL i’l3SfTION CRflBTIIIE) 00001 NOOOO X 190.29s Y 228.359 2 285 l 449
The relative position is displayed in which the
position reset by an operator is zero.
Reset operation
When this is displayed, press the X,Y,Z,or 4th
key-The address on the display will flicker.Then
press the CAN button.The relative position of
the flickering address will be reset to zero.
The current value in a programmed coordinate
system set with G92 or G50, is displayed.
l-123
(3)Overall display
22. CRT/MD1
22.2.9 Alarm Display The current position in the following coordinate
system is displayed simultaneously: .
( > a
(b)
( > C
0
Position in the relative coordinate system
(RELATIVE)
Position in the work coordinate system
(ABSOLUTE)
Position in the machine coordinate system
(MACHINE)
Residual movement amount
(DISTANCE TO GO)
(T series)
(M series)
‘I
I a:si:38 wx I
The residual movement amount indicates the
movement amount remaining in one block of a
command, and is displayed in AUTO or MDI
mode. The unit of the machine coordinate
system is the same as that of the machine
(T series)
(M svstem)
When an alarm occurs, the screen
automatically displays the alarm screen. Alarm
numbers and simple messages are displayed.
svstem.
l-124
22. CRT/MD1
22.2.10 Command value display
(T series)
G0lz F T
288.000 aai n ll.GmB0
zo
G21w Gbeuz
(M series)
a2Em NEl130 CCUIREKT) WlD~)
X 17.588 F (381 F 2888 081R G1'7 H 2 617 P
I391 Q G94H 2 G21 tl
G41 G41s I39 T
E G67
22.2.11 Run time display / parts count display
(T series)
0100s N0002 X 100.000 7 200.000
(M series)
ACTUL POSITION CRBSOUJTE~ 02000 N0198 X -12.500 Y -42.500 z 0.000
Fm?TcIxM RN TIE 8Hl2MCXLETIfE BH&
~~mEk-r7
PART COUNT:
Indicates the number of parts.When MO2
M30 is executed, it is increased by + 1.
3r
To preset the PART COUNT to “O”, press
NO.LQP and CAN key.
When the number of parts reach a target
value, the signal is sent to PMC.
RUN TIME:
Indicates the total run time during
automatic operation,excluding the stop and
feed hold time.To preset the RUN TIME to
“O”, press 3 and CAN key. (It is not preset
to “0” by cutting off power.)
CYCLE TIME:
Indicates the run time of one automatic
operation, excluding the stop and feed hold
time. This is automatically preset to “0”
when a cycle start is performed at reset
status.
(It is preset to “0” by cutting off power.)
l-125
22.  X 0.888 Y 9.888 z 0.888
MDIS 01
With this function, functions of the switches on
the machine operator’s panel can be
conducted from the CRT/MD1 panel. In other
words, mode switch and jog override switch
can be eliminated from the machine operator’s
panel. The following can be conducted from
the CRT/MD1 panel.
(a) Group 1:
Mode selection
(b) Group 2:
Selection of jog feed axis, jog rapid
traverse
(c) Group 3:
Selection of manual pulse generator feed
axis, selection of manual pulse
magnification
(d) Group 4:
Jog feedrate, feedrate override, rapid
traverse override
(e) Group 5:
Optional block skip, single block, machine
lock, dry run
(f) Group 6:
Protect key
(g) Group 7:
Feedhold
Whether to operate these switches from the
CRT/MD1 or machine operator’s panel can be
determined by the parameter for each group.
l-126
22. CRT/MD1
22.4 General Purpose Switch for Software Operator’s Panel
Screen Key
Machine
operator’s
CRT / MDI J
f
(T series)
W’EFWTCR’S PRNEL 01888 Nwa
_SIGmL 0 : SIpyy.1 : :EF ii SIGMx2 : SIGWL3 : lg
ION
SIG?sL4 : A SIpyllS : E mm SIGWL6 : KIFF SIGNFy.7 ’
RCTWL F’OSITIOC; CR&&JTE1 E
X 0.000 z 0.000
S 0T
mmnnn
(M series)
WERGTU?‘S PANEL 01888 Nlma
_srcrru. 0 : SIGwLl : ZE E SIGhaL : ION SIGr+L 3 : ,EF CN SIGWL4 : SIGhaS : aF :ii SIGbR6 : SIGN&7 : :ar E
- ?EE c-uTE’ ii 0:000
Y 0. aim
NDIS 01
Machine tool builder can add eight optionally
definable switches as an extended function of
the software operator’s panel.The name of
these switches can be set by parameters as
character strings of max. 8 charactors.
l=-lmr-lrll-l
22.5 Program Protect Key
mg I Screen Key I I
CRT / MDI Protection
key
Operator’
panel
I Data Oprotection key Registration/setting I Signal 1 1 inhibition
CNC memory
Program memory is protected from breaking
according to error operation by outputting the
signal from machine side to inhibit the writing
to program memory.Provide this switch on
machine side operator’s panel
22.6 Graphic Display
Machine program CRT screen
I Tool path I Tool path can be plotted during operationIn the
program debug mode, a program can be
checked using tool paths plotted on the CRT
screen by turning on machine lock (MLK)
without moving the machine tool.
l-127
22. CRT/MD1
22.7Dinamic graphic display ) T series
08.8. 18888
It 14a. 8.0 z loa. 888
.
AUTO (GRA?sl )(c. ?RM )(A ?Rx )( RRAIR )( 1
The blank figure,chuck and tailstock are ail
realistically described, and cutting progress can
be checked as the tool moves on the CRT
screen.
(2) M series
/ \
SOLID GRAPHIC (REVIEW 01126 N1126
i kr
I
( ANEw I(- ROT )(- ROT )(+iILT )(-TILT )
The changing profile of the workpiece is
simulated according to the movements of the
tool as programmed.Because the profile is
shown in 3 dimensions,the operator can check
the machining program in detail with great
ease.
The coodinate axis and projection angle can be
changed at random.
SOLID GRAPHIC I3-PLANE1 01126 N1126
In addition to 3-dimensional drawings, it is also
possible to describe 2-dimensional drawings or
tri-plane drawings simultaneously.
22.8 Language
. Japanese (Kanji)
. English
. Germany
. French
. Chinese
. Korean
. Italian
. Spanish
22.9 Created Tool Post Name Display (IT)
Any character strings composed of numerals,
alphabets and symbols can be displayed on
the CRT screen as a name of a tool post as
well as “Tool Post 1” and “Tool Post 2”.
Character codes are set in the parameter Nos.
257 to 263 and the corresponding characters
are displayed on the CRT screen. However, if
0 is set as a character code, the character of
“Tool Post 1” or “Tool Post 2” corresponding
to the position in which 0 has been set will be
displayed.
l-128
23. PART PROGRAM STORAGE & EDITING
23. PART PROGRAM STORAGE & EDITING
23.1 Part Program Storage & Editing
I
I Program storage
I CNC CRT/MD
Correction and
alternation of
program I
L
\ CNC tape
(Program)
CNC
(1) A number of main programs and
subprograms can be input from MDI and
stored into the memory.Programs can also
be input from the paper tape, etc. by using
the optional reader/puncher interface.
(2) Main programs and subprograms being
stored in the memory can be edited
(modified, deleted, or inserted).
(3) An optional main program being stored in
the memory can be called and edited.
(4) An optional program can be deleted.
(5) Several sequential blocks can be deleted at
a time (program delete).
23.2 Number of Registered Programs
pjz~---- : 0
: I
=I 02000 .63/l 251200
programs
(Note) Part program storage length is 1 m shorter in case of 200 registered programs.
23.3 Part Program Storage Length
Program capacity 1 O/20/40/80/1 201320m
Memory element IC memory
Battery Back-Up 1. -I I - 129
23.4 Play Back
----a I I
.-*-i
I
&__________t____~ I I I I Manual l Input of
i operation coodinate
1
value
/
Prepared program
When selecting the playback option, the
TEACH IN JOG mode and TEACH IN HANDLE
mode are added.ln these modes, programs can
be created by loading the machine tool position
obtained by manual operation into memory as a
program position. Words (0, N, G, R, F, H, I,
K, M, S, T, P, Q, C, EOB) other than X, Y, Z,
A,B, C are also be loaded into memory by just
the same operation as in the EDIT mode.
23.5 Graphic conversational Input
See item 14.10
23.6 Pattern Data Input
See item 17.4.
23.7 Menu Programming
See item 14.11.
23.8 I/o Device External Control
I/O device
External Read Start Signal
23. PART PROGRAM STORAGE & EDITING
Part program registration can be commanded
external1y.A part program can be registered in
memory in the edit mode through the input
device selected for editing using the external
read start signal .
23.9 Background Editing
Regardless of mode selection and CNC status
(during automatic operation or not, etc.),
background editing operation can be
performed-No alarm taking place in background
edit affects foreground operation.
In contrast,background editing is not affected
by foreground alarm.
In background editing, the following operation
becomes possible.
(1) Program registration from MDI
(2) Program registration from CNC tape
(3) CNC tape punching
(4) Program editing
23.10 Simple Synchronous Control
The travelling command of master axis is given
to two motors of master and slave axes in a
simple synchronous control.However,no
synchronous error compensation or
synchronous error alarm is detected for
constantly detecting the position deviation of
the master and slave axes to compensate the
deviation.
In the reference point return,the master and
slave axes similarly move until the deceleration
operation is performed. After that, the
detection of grid is performed independently.
The pitch error and backlash compensation are
independently performed for the master and
slave axes.
An input signal from the machine side can
select whether the axis travelling is carried out
based on the traveiling command for that axis
as in normal case or whether the axis traveiling
is carried out while synchronizing with the
traveiiing of any other axis.
Simple synchronous operation is allowed in the
automatic operation by tape command,manual
data input,or memory command and in the
manual operation such as manual continuous
feed,manual handle feed,incremental feed,or
manual reference point return.
23.11 Expanded Part Program Editing
The following editing is possible.
(1) ( ) a
Conversion
(b)
Conversion of address
An address in the program can be
converted to another address.
For example address X in the program can
be converted to address Y
Word conversion
(2)
A word in the program can be converted to
another word. For example, a programmed
MO3 can be converted to MO4
Program copy
Program can be copied to make a new
program
( ) a Copy of ail the program
(b) Copy of part of a program
(3) Program move
(6)
Part of a program can be moved to make a
new program
Program merge
New program can be created by merging
two programs.
Copy and move to the key-in buffer
Part of a program can be copied or moved
to the key-in buffer.
Sequence number automatic insertion
The sequence number, where a certain
increment value is added to the sequence
number of the previous block can be
automatically inserted at the head of each
block in preparation of programs by the
part program editing.
The initial value of sequence number and a
certain increment amount can be set.
l-130
23. PART PROGRAM STORAGE & EDITING
23.12 Input/Output Simultaneous Operation
If a cycle operation is put into effect with DNC
signal being ON, an external program is
executed for operation and simultaneously the
external program is stored in the memory of
the control.
Also, a program in the memory of the control is
executed and simultaneously output to an
external device.
1) Input and machining simultaneous
operation
a) Search a head of a program to be
executed.
urn on DNC operating signal GO127
(DNCI).
Turn on the input and machining
simultaneous operation signal GOI 40
(STRD).
Press the cycle start button.
e) A program is executed for operation
and input in the memory block by
block.
2) Output and machining simultaneous
operation’
a) Select a program to be executed.
b) Turn on DNC operating signal GO127
(DNCI).
Turn on the output and machining
simultaneous operation signal GO1 40
(STWD).
Press the cycle start button.
A program is executed for operation
and output to an external device block
by block.
23.13 Operation When Converting the Machining Program Prepared by Graphic Conversation to an NC Format Program and Outputting Externally Via the Reader/puncher Interface
The machining program prepared by graphic
conversation is stored in the tape memory
areas as a special data type. Therefore, of
course, the data cannot be displayed merely as
it is in NC format and one part of the data
cannot be changed.
However, after that machining program
prepared by graphic conversation has been
converted to an NC format program, it is
possible to output it outside the NC via the NC
reader/puncher interface.
After conversion, the NC format program
outputted outside the NC will be of the form
displayed by the NC program form by the NC
operation command automatically prepared
when executing that machining program.
Accordingly, it is normal that I NC operation
command is converted as 1 block program.
For example. one group of bar machining is not
indicated by canned cycle G71.
In other words, in order to convert the canned
cycle to a form can be resolved into each
operation unit, after actual conversion, the
outputted NC format program becomes longer
in proportion to the machining operation.
When the machining program is converted to
NC format and output to outside the NC, be
sure to set the memory protect switch on the
machine operator’s panel to the lock state.
l-131
24. HIGH-SPEED MACHINING FUNCTION
24. HIGH-SPEED MACHINING FUNCTION
The function converts the figure to be
machined to a data group that can be high-
speed pulse distribution by a macro
compiler/macro executor,and calls and
executes the data group as a machining cycle
by the CNC command(GO5 command)
Number of controlled axes
4 axes maximum.(Simultaneous 4 axes
control is possible.)
Pulse distribution cycle
Set the pulse amount equivalent to this
cycle as a macro variable for high-speed
cycle machining bY a macro
compiler/macro executor.The pulse amount
unit should be the least input increment.)
Command format
Call and execute the high-speed cycle data
by the following command.
Go5 PI OnnnL999;
PlOOOl - P10999;
First number of the machining
cycle to call
L999;
Repetition count of machining cycle
The cycle data can be prepared for up to 999
cycleSpecify the machining cycle by the
address “P“ .Each cycle can be continuously
called and executed by the connection data (in
the header).Specify the repetition count of
machining cycle by the address n L”.The
repetition count (in the header) can be
specified for each cycle.The connection and
repetition count are explained with an example.
Example)
Cycle 1 Connection data 2
Repetition count 1
Cycle 2 Connection data 3
Repetition count 3
Cycle 3 Connection data 0
Repetition count I
G05PlOOOl L2
In this condition, the cycles to be executed
are:
(4)
1,2,2,2,3,1,2,2,2,3 cycles are continuously
executed.
Data configuration
The following data is converted to a high-
speed cycle machining variable(#ZOOOO-
#85535) by a macro compiler/macro
executor.
Configuration of high-speed cycle machining data
#20000
#20001
#20017
#20033
1 Registered cycle number
Header of cycle 1
Header of cycle 2 I Header of cycle 3 . . . m
.
.
Data group of cycle 1 J Data group of cycle 2
I I- Data group of cycle 3
1-132
25. POLIGONAL TURNING
25. POLIGONAL TURNING
Polygonal turning means machining a polygonal
figure by rotating the workpiece and tool at a
certain ratio.
(1) Rotation ratio of workpiece and tool
(2) Number of cutter
By changing these conditions,the machining
figure can be changed to a square or
hexagon-The machining time can be reduced
as compared with polygonal figure machining
using C and X axes of the polar coodinate.The
machined figure however,is not exactly
polygonal .Generally,polygonal turning is used
for the heads square and/or hexagon bolts or
hexagon nuts.
n------/
Tool rotation for polygonal turning is controlled
by CNC controlled axis.
The rotary axis of tool is called Y axis in the
following description.
The Y axis is controlled by G25.1 command,so
that the rotation speeds of the workpiece
mounted on the spindle (previously specified by
S-command)and the tool become the specified
ratio.
G251 P Q ; -w P ,Q : Rotation ratio of spindle and Y axis
Specify range :Integer 1 to 9 for both P
and Q .
When Q is a positive value, Y axis
makes positive rotation.
When Q is a negative value,\/ axis makes
negative ratation.
(Example)Rotation ratio of workpiece( spindle)
to Y axis is 1:2,and the Y axis makes positive
rotation.
G51.2P1 Q2;
When simultaneous start is specified by
G251,the one-rotation signal sent from the
position coder set on the spindle is
detected,and the Y axis rotation is controlled
according to the rotation ratio(P:Q)while
synchronizing with the spindle
speed.Namely,the Y axis rotation is controlled
so that the spindle and Y axis stand in a
relation of P:Q.This relation will be maintained
until the polygonal turning cancel command is
executed(G50.2 or reset operation).The
direction of Y axis rotation is determined by the
sign of Q and not affected by that of the
position coder rotation.
Synchronization of the spindle and Y axis is
cancelled by the following command:
G250;
When G250 is specified,synchronization of the
spindle and Y axis is cancelled and the Y axis
stop.This synchronization is also cancelled in
the
0 i
(ii)
(iii)
(iv)
following cases:
Power off
Emergency stop
Servo alarm
Reset(external reset signal ERS, reset /
rewind signal RRW,and RESET key on the
CRT/MD1 panel)
( ) V When P/S alarm 217-221 is occured.
(Example of program)
GOOX 00 220 Sl OOOM03;
Workpiece rotation speeed 1 OOOrpm
G251 Pl G2;
Tool rotation start (tool rotation speed
2000)rpm
GOlX80.FlO;
X axis infeed
G04X2;
GOOX 00;
X axis escape
G250;
Tool rotation stop
G05;
Spindle stop
Be specify G250 and G251 with single block.
26. SELF-DIAGNOSTIC
26. SELF-DIAGNOSTIC FUNCTION
CRT/MD1
Gsplay
Output signal
CNC Input signal Machine
Alarm status
I
Various status can be displayed by the
CRT/MD1 panel.
(1)
(2)
(3)
(4)
(5)
On-off signals input to the NC can be
indicated on the CRT display.
All on-off signals output from CNC can be
sent in the unit of bit via MDI panel.
Various parameter values such as
acceleration/deceleration time
constant,rapid traverse rate, etc. can be
checked on the CRT display.
Details of alarms which may occur
accidentally can be classified and checked
on the CRT display. These alarms
comprise overheat, overtravel, servo alarm,
tape check(horizontal and vertical
directions) and program errors.
The’ condition of servo system can be
observed.
l-134
27. DATA INPUT / OUTPUT
27. DATA INPUT I OUTPUT
27.1 I/O Device Interface
CNC
Memory
Program t-l Offset Parameter
/ : l l
Reader/puncher interface
FANUC
cassette
adapter
reader or FANUC PPR
t FANUC 1 Cassett Fl Paper tape Cassette Bl/BZ
The following can be input/output via the
reader/puncher interface.
(1) Part program registration
(2) Tool offset amount input
(3) Parameter input
(4) Part program punch
(5) Tool offset amount punch
(6) Parameter punch
In order to input a program into CNC memory
or output the input program to an external data
storage medium by using the MDI panel, a unit
equipped with such FANUC reader/puncher
interface as FANUC cassette/FANUC PPR/
portable tape reader or ASR33 interface can be
connected. EIA RS244-A or IS0840 is
employable as data codes.
These lSO/EiA codes are automatically
identified from each other in case of data input.
Either IS0 codes or EIA codes is selectable by
setting parameters in case of data output.
Since program input/output can be started by
signals from the machine tool as well as by
MDI panel operations, program can be loaded
automatically.
Number of the reader/puncher interface channel
(1) Channel 1 :Reader/puncher interface,
ASR33 interface
(2) Channel 2:Reader/puncher interface
27.2 Input Devices
27.2.1 FANUC FLOPPY CASSETTE
Data can be stored in the floppy cassette and
also data can be input to the CNC.
The interface is reader/puncher interface.
Refer to the Floppy Cassette Operator‘s
Manual (B-66040E) for the operation of the
floppy cassette.
27.2.2 FANUC PPR
PApw trp
CANUC WA
J
An i/O device with paper tape reader, tape
punch, and printer in one system.
Paper tape reader read speed:
l-135
27. DATA INPUT / OUTPUT
150 ch./sec or more
Paper tape punch punching speed : 50 ch./sec
Printer characters per line:
40 ch. (dot impact method)
Printing speed : 1.2 linekec
27.2.3 Portable Tape Reader
Optic81 terdcr pu
The portable tape reader is a carrying type
paper tape reader.Used to load program, data,
and parameter to the CNC.
Read speed :
300 ch/sec (60Hz), 250 ch/sec (50Hz)
Read method : Opto-electrical (LED)
27.2.4FANUC PROGRAM FILE Mate
It can be connected to the remote buffer to
achieve high-speed transfer of maximum 86.4
kbps.
The hard disk is sealed to be continuously
used under the factory environment.
27.2.5 FANUC FA Card The FANUC FA Card ism a memory card which
has nonvolatile solid state memories as
memory element. By connecting the FA Card
to’ the FANUC CNCs via the FA Card
Adapter,part programs stored in the CNC can
be transfered to and saved in the FA Card.
Also, part programs written in the FA Card can
be trancefered to the CNC as well.
- Compact, high density and easy-to-use
20m to 160m paper tape equivalent data
storage in 54mm X 85.6 mm X5mm size
l Maintenance free
Nonvolatile solid state memory requires no
battery
- Stand alone type and Built in type FA Card
Adapter are available
The built-in hard disk enables data to be stored
and it can be connected to the reader/puncher
interface to input data to CNC.This hard disk
has a large storage capacity of approximately
50,OOOm of paper tape data,so it can register
maximum 1024 command proarams.
1 - 136
28. SAFETY FUNCTIONS
28. SAFETY FUNCTIONS
28.1 Emergency Stop
Emzop buttom
With the emergency stop, all commands stops,
and the machine stops immediately.Connect
the “emergency stop” signal both to the control
unit and to the servo unit side.
When emergency stop is commanded, servo
excitation is also reset, and servo ready signal
will also turn off-After resetting the emergency
stop, continue the operation after performing
the reference point return operation.
28.2 Over-travel Functions
28.2.1 Overtravel
- ,-b- iT_ Limit switch
’ X axis movable range
As this CNC’s basic specifications cover the
software limit detection function, it is generally
unnecessary to provide the limit switch and dog
function on the machine tool side for the
purpose of overtravel detection.
In order to solve such a case as the stroke end
position in the + 2 direction changes each time
the tailstock travels in keeping with th’e
movement of a workpiece, an interface is
provided to be able to receive a signal from the
limit switch as an overtravel signal in the + 2
direction only. In other words,the limit switch is
mounted to the tailstock and its contact is
connected to * + LZ terminal, so that the stroke
and position can be detected correctly in
keeping with the travel of the tailstock.
28.2.2 Stored stroke limit
B(X2 ’ Cl Forbidden area of tool
Points A and B are set by parameters
The area outside an area preset by a
parameter is defined as a forbidden area.If the
machine tool enters the forbidden area, the
axis motion is decelerated and stopped with
overtravel alarm display.(stored stroke limit)
The distance from the reference return position
is set to the parameter. Stored stroke limit
function can be made to be ineffective by
parameter setting.
28.2.3 External setting function of stored stroke limit
When changing a tool, this function rewrites the
machine position (machine coordinate) of that
time into parameter values (No. 700-702, 704.
706) as the stored stroke limit by adapting its
tip position to the end of the limit area and
depressing the SETTING key.
Setting signals are provided for each axis and
direction ( + X, + Y, + Z, -X, -Y, -Z).
In addition, by turning the common LIMIT
RELEASE button for all axes to the ON
position, it is also possible to arrange that the
stroke limit may not be checked.
28. SAFETY FUNCTIONS
28.2.4 Expanded Stored Stroke check
1 St limit
The area in which a tool may not travel
(forbidden area) can be divided into the
following two blocks for setting.The shaded
portions above show the area in which no tool
can move.
1st limit:
2sl
Set the boundary,using parametersThe
outer side of boundary thus preset
corresponds to the forbidden area.This is
normally not changed once the machine
tool builder sets this area.Therefore,always
set the boundary to the maximum stroke of
a machine.
limit:
Set the boundary,using parameters or
program command.The inner or outer side
of boundary preset corresponds to the tool
entry prohibited area.The inner or outer
side is determined by parameter. G22
prohibits the tool from entering the
forbidden area of the 2nd limit.
28.3 Interlock
Motor speed
A
axes is inhibited or the movement of Z axis
only is inhibited can be set by parameters.
When all axes movement is inhibited, high
speed interlock input can be used. Interlock
also can be applied to each axis independently
by parameter,.
When this interlock signal is applied, the
moving part of the machine tool stops after
being decelerated. When this interlock signal is
released, the machine tool starts moving again
after being accelerated.
This interlock function is effective for both
automatic and manual operation modes.
28.4 External Deceleration
Feed rate can be decelerated by an external
deceleration signal from the machine side. A
feed rate after deceleration can be set by
parameter. External deceleration is prepared
every axis and every direction.
When the tool is to be moved in the reverse
direction, futile time may not be wasted since
no external deceleration is applied.
Conditions to make this signal effective are set
by parameters:
(1) Whether this signal is applied to rapid
traverse only or to all feeds.
(2) Whether external deceleration in the +
direction is made effective (each axis).
(3) Whether external deceleration in the -
direction is made effective (each axis).
This function allows the maximum of valid
strokes and keeps shock to the machine to a
minimum, to stop at stroke end. This function
is also useful when overtravel of the machine
from the stroke end in, for example, ATC
reference points , must be kept to a minimum.
This function inhibits the axis movement of the
machine tool. Whether the movement of all
1 - 138
29. STATUS OUTPUT
29. STATUS OUTPUT
29.7 Feed Hold Signal
CNC
[I Status signal
4
This signal is sent out when automatic
operation is holded by feed hold. CNC ready signal Sew0 ready signal
I Machine 29.8 Power Ready Signal side
29.1 CNC Ready Signal
This signal is sent to the machine side when
CNC power is on and control becomes
possible. Sending of this signal will be stopped
when CNC power is turned off.
This signal is output when input power is
supplied to the CNC, and output voltage of the
stabilizer power circuit in the CNC has reached
the standard value.lf abnormality in power
circuit is detected, this signal will no more be
output. Stop power supply at once in this case.
29.2 Servo Ready Signal
This signal is sent to the machine side when
the servo system becomes operatable. Axes
necessary to be braked must be braked when
this signal is not sent. When this signal is
interrupted, NOT READY is displayed on
CRT/MD1 panel.
29.3 Alarm Signal
This signal is transmitted when the CNC comes
under an alarm statusAlarm type signal is also
sent out.
29.4 Distribution End Signal
This signal is sent out when pulse distribution
of the M,S, or T functions has ended, so that
they can be used after move of the
commanded block ends.
29.5 Automatic Operation Signal
This sign
automatic
al is sent out when it is under
operation.
29.6 Automatic Operation Start Lamp Signal
This signal is sent out
operation is being activated.
when automatic
29.9 Reset Signal
This signal is sent out to show that the CNC
has been reset.
29.10 Battery Alarm Signal
This signal is output when the voltage of the
battery for holding memory data during power
interruption has become lower than the
specified value. Since the above condition is
usually indicated as the battery alarm display
on the CRT/MD1 panel, this signal is not
required normally. .lf the detachable CRT/MD1 is
employed, inform an operator of the necessity
of battery exchange by the lamp indication
using this signal.
29.11 Clock function
This function displays the status indicating line
on each CRT screen and the present time on
the parameter setting screen. The time is
corrected on the parameter setting screen.
It is aiso possible to know the current time.
(year/month/hour/minute/second) through the
PMC.
29.12 Position Switch Function
The position switch function outputs a signal to
a specified controlled-axis when the machine
coordinates of the controlled-axis are within the
range specified by the corresponding
parameter.
29. STATUS OUTPUT
The parameter specifies an arbitrary controlled-
aixs and the operating range (machine
coordinates) within which the position switch
signal is output.
Up to ten position switch signals can be output.
l-140
30. EXTERNAL DATA INPUT
30. EXTERNAL DATA INPUT
30.1 External Tool Compensation
CNC
This function is provided to change the tool
I Calculation of
Compensation tool
data Compensation
value
offset amount from the machine tool or other
external devices. Input data are added to the
offset amount having the offset number
specified by the program when the tool offset
amount is externally input. The offset amount
may also be processed as input data by
specifying an input signal.
When the machine tool provides an automatic
measuring function for tools and workpieces,
the offset amount can be changed to a correct
value by inputting an error from the correct
value into CNC by using this function.
If the tool offset amount is externally input
when the offset number 0 is selected by a
program, (that is, offset cancel), the work
coordinate system shifts by the input data
amount.
The external tool offset amount is 0 -
2 7.999mm or k 0.7999 inch at a time.
30.2 External Message Function
For the message function applied by external
data input signals, two functions are available.
However, either the PMC-L or M is requried to
use this function.
(1) External alarm message
“External alarm message” means a
function which puts the CNC in the alarmed
condition by sending alarm numbers
externally and in addition, sends messages
to the CNC externally and allows them to
be displayed on the CNC’s CRT screen.
Four alarm numbers and four messages
can be sent at the same time. The length
(2)
of a message which can be sent against an
alarm No. is within 15 characters. The alarm No. which can be sent will come
from numbers between 0 and 999.
However, when the CNC displays, it will
add 1000. It is also executed using
external data, to release the alarmed
condition.
External operator message
“External operator message” means a
function which sends a message and a
number for the operator to the CNC
externally and allows to display the
message on the CNC’s CRT screen.
Only one message can be sent at one time
with the message length within 127
characters. The number which can be sent
is a number between 0 and 999, however,
a message of up to No. 99 will be
displayed with its number to which 2000 is
added. As to the message of Number from
100 to 999,. only characters will be
displayed without its number.
30.3 External Key-Input Function
“External Key-Input” means a function which
can control the CNC by informing CNC of key
input data from the PMC as if an operator
entered it into the CRT/MD1 unit. For instance,
it becomes possible to edit programs (the
searching for a program No.) by PMC.
30.4 External Data input
The following data can be entered,using
external data input.
(1) External tool off set
(2) External message function
(3) External key input
(4) External program No. serach
This function inputs any one of the program
number 1 to 9999 to CNC from the
outside,such as the machine side and
searchs the program from the memory
For a machine provided with a function of
loading several types of workpieces
1 - 141
(5)
automatically, this function can be used to
search a program automatically according
to workpiece for execution.
External work coodinate system shift ( Only
M series)
The external work coodinate system shift is
a function of shifting the work coodinate
system according to the external shift
amount.
This shift amount for each axis is all added
to the work coodinate system for use. This
shift amount is not lost even when power is
turned off.
This shift amount is not integrated
incrementally but the input shift amount
corresponds to a new shift amount. The
shift amount which can be input is 0 to
2 0.7999 inch.
30.5 External Machine Origin Shift
The machine coordinate system is
compensated by offset amount given from
outside. This offset amount always take
absolute value; never an increment value.
The offset amount range is:
0 2 9999
in detection unit.
When offset amount is
machine move distance
input, the actual
is the difference
between the previous offset amount and
current off set amount.
This function is used t compensate the
machine coordinate system error caused by
mechanical deformation.
30. EXTERNAL DATA INPUT
l-142
31. EXTERNAL WORK NUMBER SEARCH
31 l EXTERNAL WORK NUMBER SEARCH
CNC
Program memory
00001
: :
Program selection switch
By specifying work numbers of 01 - 15
externally (from the machine side,etc.), a
program corresponding to the work number can
be selected. The work number equals the
program number. For example, when work
number 12 is specified, program 00012 is
selected. (The first 2 digits of the program
number is 00.)
l-143
32. MACHINE INTERFACE
32. MACHINE INTERFACE
CNC
Master
I/O
40140
l/O c3
107/72
I/O c2 . 80 / 56
I/O Cl .
40/40
Magnetic
b cabinet
7 I/O Cl Kinds of l/O card
‘\Remaks
40 I 40 -1 l/O c2
I/O c3
Additional
l/O 81
80 56
104 72
104 72 Available
with PMC-
M
(Note) Either I/O Cl, C2 or C3 can be selected. When PMC-M is provided, either Cl, C2 or C3
and additional I/O Bl can be employed
Number of Inputs/Outputs
Input (total) output
(total)
Remarks
40 40
80 56
104 72
144 112
184 128
208 144
With PMC-UPMC-M
With PMC-M
1 -144
33. PROGRAMMABLE MACHINE CONTROLLER (PMC)
33. PROGRAMMABLE MACHINE CONTROLLER(PMC)
CNC
b Machine interface
Window
Magnetics sequence circuit can be incorporated in the CNC.
The following two tl
PMC-Model L 104 72
(PMC-L )
PMC-Model M
(PMC-M )
Window Function
les of PMC is available.
Max.No. of
inputs
Max.No. of
outputs No. of step
3000 steps
3000/5OOOsteps
Time of
processing
1 SF/step
Machine
side
Remarks
High-speed M, S and
T interface is
available.
High-speed M, S ad
T interface and no
dividing method is
available.
In this function, PMC can request CNC to transfer data to the PMC side.
The following kinds of data are transferred from the CNC.
(1) Present position
(2) Machine position
(3) Skip position
l-145
34. CONTROL UNIT
34. CONTROL UNIT
34.1 Cabinet
Unit;mm
w: Control unit A: 250
Control unit B: 450
Weight : Aboutl6kg Coating color: P-LT;SGY 3.5/0.5(Dark grey)
-00
34.2 Power
pizzq
&I Power unit
I Multi-tap transformer I I t----AC200/220V
AC power
34.2.1 Input power voltage
200VAC + lo -15
% ,50160Hz f: 1 Hz, 1 phase
Or
220VAC + lo - IS
%,60Hz + 1 Hz,1 phase
34.2.2 Input unit
Power ON/OFF control is made easy by the
input unit setting to machine side.tnput power
of unit is as following.
200VAC + lo %,50/60Hz t I Hz -1s
or
220VAC + lo %,60Hz 5 1 Hz -1s
34.2.3 Multi-tap transformer
Multi-tap transformer may be necessary for the
control unit according to input power voltage.
Multi-tap transformer is not necessary when
input power is:
200VAC + lo -1s
% ,50/60Hz k 1 Hz, 1 Q
or
ZOOVAC + lo -IS
%,60Hz 2 1 Hz,1 +
When multi-tap transformer is equipped with,
allowable input power becomes:
200/220/ 230/240/380/ 419 4401 460/ 4801
550VAC + lo - 15
% ,50/60Hz 2 1 Hz, 1 phase
The multi-tap transformer must be mounted on
the machine side.
34.3 Battery Unit Mount the battery unit to the machine side
where it is replaced easily.
l-146
34. CONTROL UNIT
34.4 Environmental Requirements
(1)
(2) (3)
(4) (5)
Ambient temperature
O°C - 45OC when operating
-20°C - 60° C when stored or delivering
Change in temperature Max. I .l OC/min
Humidity 75% or less (relative humidity)
generally Max. 95% for a short time
Vibration 0.5G or .less when operating
Circumstances
When using in places with thick dust,
cutting oil, or organic solvent, consult
us.
34.5 Weight
Control unit (Panel mount type):About 16kg
CRT/MD1 :About 5kg
CRT/MD1 (Detachable type) :About 11 kg
Weight may differ according to system
configuration
l-147
35. CABLES AND CONNECTORS
35. CABLES AND CONNECTORS
Cables and connectors are offered for
connection between units.
l-148
36. SERVO SYSTEM (Digital Servo)
36. SERVO SYSTEM (Digital Servo)
36.1 Position Detection System
Pulse coder . 4
36.2 Position Detector .
incremental pulse coder .
Absolute pulse coder
Position is detected by the feed-back signal
from the pulse coder. The following move
distance/rotation of the pulse coder is offered.
Table36.2 Kind of pulse coder ”
Ball screw Pulse coder Move distance/rotation
unit of pulse coder
Metric 2000p /rev 2,3,4,6,8mm
25OOp/rev 5,lOmm
3000p /rev 3,6,12mm
Inch 2000p /rev 0.1 ,0.15,0.2,0.3,0.4inch
2500~ /rev 0.25 ,O.Sinch
3000p /rev 0.15,0.3,0.6inch 4
36.3 Servo Motor
FANUC AC SERVO MOTOR MODEL 4-0, 3-0, 2-0, l-0, 0, 5, 10, 20, 20M, 30, 30R
+
36.4 Velocity Control Unit
Various velocity control units are offered
according to types of AC servo motors.
36.5 Regenerative Electric Discharge Unit
Various regenerative electric discharge unit are
offered according to type of AC servo motor.
36.6 Servo Power Transformer
Various power transformers are offered
according to types of AC servo motors.
1 - 149
37. POSITION CODER
37. POSITION CODER
CNC
Position coder
A position coder is connected to the spindle
and generates square wave voltage signal the
frequency of which is proportional to the
spindle speed. This synchronizes the feed with
the spindle speed.
(1) Position coder A
(a) Number of square waves per revolution ,
Channel Number of square waves
Ich 1024~ /rev (A,A,B,B phases)
2ch 1 p /rev (A,Aphase) 4
(b) Maximum response revolutions 4,000 rpm
(c) Range of operating temperatureo” - 50°C
(2) Position coder B
(a) Number of square waves per revolution
Channel Number of square waves
lch 1024~ /rev (A,A,B,Bphases)
2ch 1 p /rev (A,Aphase)
(b) Maximum response revolutions 6,000 rpm
(c) Range of operating temperature 0” - 50” C
l-150
38. FUNCTION FOR 41AXIS LATHES(O-TTC)
38.1 General
0-TTC can independently operate two tool
posts and control a lathe which simultaneously
cuts and machines on the two tool posts.
It can be applied on two tool posts and the
lathe which machines two workpieces with two
spindles on them.
Single spindle and two tool posts
--- --
l
-
I wi
Twin spindles and two tool posts
(1) Application to lathes with twin spindles and
two tool posts
The system can be applied to turning tasks in
which a single workpiece attached to a single
38. FUNCTION FOR 4-AXIS LATHES (0-TTF)
spindle is machined using two tool posts
simultaneously. For example,while one tool
post performs machining of the outer dimeter, it
is possible to machine the inner diameter with
the other tool post. The result is a sharp
savings in machining time.
(2) Application to lathes with twin spindles and
two tool posts
The system can also be applied to turning
tasks where two workpieces attached to twin
separate spindles are simultaneously machined
using the two tool posts. Because machining
can thereby be performed with one lathe with
equal efficiency to two conventional lathes, a
dramatic increase in productivity can be
achieved.
(3) Simultaneousiy,independent control of two
tool posts
Using the tool post selection key on the NC
operator’s panel, the operator selects the
programs for each of the two tool posts from
among the programs registered in the memory.
When the start signal is issued,the system
simultaneously and independently executes the
selected two programs, controlling the Xl,Zl
axes and X2,22 axes respectively.
Only one operator’s panel is provided for the
two tool posts. Panel operation and display
functions for each tool post are determined by
the tool post selection key provided.
(4) Tool post waiting function
The movement of each of the two tool posts
can be programmed independently, as in the
case of an ordinary two-axis lathe. M codes
control the first and second tool posts to wait
for each other during machining. Or only one
tool post to machine.
l-151
38. FUNCTION FOR 4-AXIS LATHES (0-TTF)
38.2 Balance Cut(G68,G69)
.
G68 : Balance cut mode
G69 : Balance cut cancel
When machining the workpieces shown in the
figure above in a four-axis lathe, machining the
workpiece with cutters applied to its sides
simultaneously prevents sagging of the
workpiece, which would be caused by
machining from one side only. This results in
more accurate machinng. if ,however,the
cutters do not move sysnchronousiy, the
workpiece will chatter, resulting in no correct
machining. The use of this function permits
easy synchronization.
.
38.3 Interference Check Function
breakage of the machne tool itself, may
happen.
A 4-axis. lathe is normally provided with two tool
posts. When a blank is concurrently machined
by using these two tool posts,it is possible that
a part of each tool post approaches each other
very closely. if two tool posts should make
contact with each other due to a machining
program failure or other setting failures, a
serious accident like the damage of tools or the
l-152
39. MACHINE OPERATOR’S PANEL
39. MACHINE OPERATOR’S PANEL
Standard machine
operator’s panel External dimensions No. of keys External view Remarks
Standard machine
operator’s panel for
small 9”
monochrome
CRT/MD1
400x180x150
w NH ND 1
46 keys
46LED( red)
Appendix4
Fig. -14
Override switch,Emergency stop
button, Program protect key are
provided
Standard machine
operator’s panel for
small 9” color
CRT/MD1
4OOx18Ox1’5O
(W )(H )(D 1
46 keys
46LED( red)
Appendix4
Fig. -15
Override switch,Emergency stop
button, Program protect key are
provided
Standard machine
operator’s panel A for
full key 9” CRT/MD1
Standard machine
operator’s panel B for
full key 9” CRT/MD1
520x180~150
(W )W )(D )
520x180~150
W NH ND 1
53key
53LED(red)
53 key
53LED( red)
Appendix4
Fig. -16
Appendix4
Fig. -17
Override switch, Emergency stop
Program protect key, Manual
pulse generator are provided
Program protect key is provided
A switch can be equipped on the
blind plate by the machine tool
builder.
The standard machine operator’s panel can work using DI 22 points and DO 8 points only.
However, PMC-L or PMC-M is required.
l-153
40. REMOTE BUFFER
40. REMOTE BUFFER
40.1 REMOTE BUFFER
The remote buffer is option and is used to
allow a large number of data to be continuously
supplied to the CNC at high speed by
connecting it to the host computer or I/O
device through a serial interface.
The following can be performed by the remote
buffer.
1 )lt is used to perform DNC operation at high
speed and with high reliability by performing
on-line connection to the host computer.
2)lt is used to download the NC program and
parameters from the host computer.
3)lt is used to perform DNC operation and
download various kinds of data by connecting
to the l/O device.The following I/O devices can
be connected.
0 FANUC PPR
@ FANUC CASSETTE Bl/B2(Bubble
cassette)
@ FANUC CASSETTE F3(Floppy
cassette)
@ FANUC PROGRAM FILE
0 FANUC PROGRAM FILE Mate
4)There are following 2 types as protcol.
Protcol A Thehand shake way,that it is repeated
transmission and receptopn between
them
Protcol B
The way that the communication
between them is controlled by control
code output from remote buffer
40.2 High-speed Remote biffer A High-speed remote buffer A for FANUC 0
series is started by a block command
“GO5; “,thus allowing high-speed
processing,using the subsequent travel data for
the specified axes.
(1) Data format
The tool moving distance for 4/8 msec shall be
expressed in binary data.
Travel sequence ~~~II~-~~~~~~~ _,
(a) Designate the number of command axes
N,using parameter No.597.
(b) One block shall be (27\L + 1)bytes.
(c) Command the moving distance of each axis
in 2 bytes-However, be sure to set LSB of each
byte to 0 . Using the remaining 14
bits,command the moving distance at intervals
of 8 msec in the following unit. Command the
moving distance in the negative direction ,
using the complement of two.
(Example) When the moving distance in
8msec is 700 $8 msec:
IS 8 7 0
0000101 *0111100*
“*” should be always 0.
(d) The check byte is the sum of (2*N) bytes
data of 8 bits,but the overflown value
exceeding the 8 bit value is discarded.
(2) High-speed remote buffer A mode
For high-speed remote buffer A, its mode
should be designated.
High-speed remote
“G05; u
High-speed remote
the moving distance
buffer A mode ON:
buffer A mode OFF:
is 0 for all the N axes.
(Note) After commanding “GO5; u block with a nomal NC command format,command the
moving distance in the aforementioned format.
Then, command 0 for the moving distances of
all axes. Therefore,the high-speed remote
buffer is placed in the OFF
mode;hereafter,command the moving distance
again in a normal NC command format.
(3)lt is remarkable speed of 15m/min under the
conditions that the command program
l-154
40. REMOTE BUFFER
containing continuous blocks with travel
increment of lmm per 4msec for 3-axis
simultaneous control and transfer speed of
38.4Kbaud.
(4)Requirements
(a) Only the linear incremental command is
used.
(b) If “G05;“ is commanded in the current
compensation mode, an alarm will be
produced.
. (c) The feedrate override is ignored.
(d) No storage is possible.
(e) The feed hold is operational.
(f) Interlock is operational.
(g) The clamp for maximum speed cutting feed
is not operational.
(5) Transfer speed
The minimum transfer speed required is
obtained regarding 11 bits/byte as follows:
[ i’(ZXN+l)byteXll / Sm-seeHO %
baudrate]
If the data is transferred at a lower rate than
the above, the desired speed will not be
produced.
40.3 High-speed remote buffer B The use of NC language prepared by an
automatic programming unit,for example,
permits high-speed machining.
(1) Data format
Designate the high-speed machining
section,using the following commands.
Command Contents
GOSPOl; High-speed
machining start
GOSPOO; High-speed
machining end
x Y 2 ; ---
GOSPOO; . . . . _ _ . High-speed machining end
n/lo;; (2) Command contents
The following can be commanded in the high-
speed machining section.
I Command address Contents I X X-axis moving
distance
Y Y-axis moving
distance
2 Z-axis moving
distance
F I Cutting feedrate I
No other than the above can be commanded.
(3) It is remarkable speed of 12m/min under the
conditions that the command program
containing continuous blocks with travel
increment of lmm for 3-axis simultaneous
control and transfer speed of 38.4Kbaud.
 High-speed machining start
l-155
II. CONVERSATIONAL AUTOMATIC
PROGRAMMING FUNCTION
(O-TC, O-TF, O-MC, 0-MF, O-Mate MF)
1. GENERAL
1. GENERAL
The conversational automatic function is
prepared for 2-axis lathe by 0-TC / TF and for
machining center by O-MC / MF / Mate MF.
Machining programs can be prepared easily,
just by following the illustrative drawings and
operating guides. Program checking and
correction / changing can also be carried out
with remarkable ease.
2-1
2. GRAPHIC CONVERSATION FOR 2-AXES LATHE
2. GRAPHIC CONVERSATION FOR 21AXES LATHE (0-TF)
(1) illustrative drawings
Illustrative drawings are provided for each type
of machining process. During input, each
portion of the illustration flashes in succession
to indicate where data is being asked for. This
feature greatly sinmplifies data input operations.
(3) Profile description check
Once data input is complete, the rasulting
machining profile can be displayed on the
screen as programmed. This feature makes it
possible to detect input errors immediately for
quick correction.
comimSATIONAL PROGRAMKING Plt0GBA.M -f~fjlg 8~8 INITIAL SET *** MATERIAL W- PC25 SHAPE F- CYLINDER OUTSIDE DIA D- 158.000 INSIDE DIA H= LENGTH LS MAX SPINDLE S- 3000 -L- FINISHING x-
zm END REMOVAL E- M-CODE H-
DATA+INPUT Ii
( )(Nx-PRC)(NEW pR)( PLOT )(GUIDB )
cO~ERSATIONAL PROGRAMMING PROGRAM -t)@le a$$ PLOTTING OF PART FIGURE s**
( I( I( WTuwt I
(2) Operating guidance
Each impending operation is displayed on the
screen. So even inexperienced operators can
master all operations with no special training.
(4) Program copy
A copy function is provided for copying
previously prepared machining programs. This
feature greatly facilitates preparation of similar
programs.
 CURSOR KBY+PUSH IlOSRT
DELETE A BLOCS5 :SELRCT BY CURSOR KEY+PUSH DBLET
FINISH THIS PROCRSS :PUSH SOFT KEY PRCS-EJ
FIlOISB THIS HACHINflG PROGRAM :PUSH SOFT lfBY WCHN-BJ
( )( )( II )IRRTUm _ -_ -_ me _____---- -
CONVERSATIONAL PROGRUIO1ING *** PROGRAM HEbm *** (PEST NO. OF PROGRAM 24 PCS.) (PEST NO. OF PROCES 91 PCS.) PRG.10. NAMR m: DBHONSTRATION
)(GUIDI ) - _--.a ._ _--.- ___ _ __ -------- -
2-2
2. GRAPHIC CONVERSATION FOR 2-AXES LATHE
2.1 Menu Screen
A complete selection of menus has been
prepared to accommodate ail programming
needs - everything from rod machining, tracing
necking, facing and threading to grooving and
drilling. This enables the inexperienced
operator to proceed with ,effortless ease, and
at the same time permits the experienced
operator to make maximum use of his
machininn knnwhnw
COBVEPSATIONAL PROGRMOIIBG PROGRAM -g@l@ *** PROCES(81) *** MACHINING PATTERN
P- l-CYLINDER A-OUTER END 2-PTTRN RPT
START POINT lb 126. 000 3-RESIDUAL z- 19.960 4-END PACNG
ROUGHHESS SR- 19 5-THREADING PGE TOOL No. RT- 102 6-GBOOVflG OUTPUT T RO- 202 7-NBCRING CUT-SPD. EC- 700 8-CBNTEPDPL PEED/REV, RF- 60.0660 9-DPILLIblG SPINDLE RS- NORMAL 1 B-TAPPING
ll-SINGLE 120MRASuRImrG
DATA+fNPUT (CONTWUR 130SUB CALL (Pm-PR)(Nx-PPC)(NRw PR)( PLOT )(GWfD1 ) -e-m ----___ ___-___.-__ ____ __-- ____--- -
CON'VBRSATIOBAL PROGRAMMING PROGRAY -@@I# t8t PROCESt01) *** HkCHIblIbfG P- CYLINDER PATTERN START POINT
x_m i;~z%g
z- 1e:eee 4-INNER MID ROUGHNESS SR- 10 5-PACE El!ID RGH TOOL NO. RT- 102 G-FACE MID OUTPUT T RO- 202 CUT-SPD, RC- 700 FEBD/REV. RF- 88.8080 SPINDLE RS- NORMAL
DATA+INPUT (CONTINUE (PRE-PR)@X-PRC)(NEW PR)( PLOT )(WIDS ) e-e- -_-_---- _. __ ,~__ _. . ------- -
/ CONVERSATIONAL PROGRAMMING PROGRAM -9916 ttt PROCES (01) *** CUT TYPE(l)- h-1111 l-CON% AMNT
(2) P2-SNGL EDGE 2-CONST. DPTB
No. OF THREAD NT- 1 SPARK OUT SO- 2 THRD URIGBT H- 2. 066 CUT DEPTH MD- 1.696 SPINDLE GEAR P- AUTO. COOLANT H= ON
. DATAtiINPUT (PRR-PR)(NFPRC)(NIIW PR)( PLOT )(WJDB ) ---- _-__--w -_ ___. __ __ __ - ---- _-- -
2.2Arbitrary Profile Machining Programs
Arbitrary profiles can be specified easily using
Symbolic input and the automatic intersection
computation function. The specified profile is
graphically displayed immediately, thus
enabling fast and easy checking.
I-EORIZ# 2-VERTCL 3-TAPER I-ARC 5-CEAMFR 6-CONR-8 'I-TANGIfT
h FIG. TIPEIo-,INPUT (cA~cRL)(YcEI+E)(PR~~~R~[ PLOT )(Gu~DB )
-
2.3Set up Guidance Display
Set up operations that have traditionally been
difficult to perform without sufficient experience
- e.g, measurement of tool offset values,
designation of the zero point, etc. - can be
performed automatically just by following the
instructions as they appear on the screen.
t- a** TOOL PBEPABATIOI *aa m
3.BRfHG TEE TOOL EDGE IN CONTACT WITH A WORK-EBD SURFACE IN MANUAL MODE
AFTER THIS OPERATION, PUSH SOPTXEY [ END ]
(Pm-PG)(NxT-PG)( END )( RETURH)( )
2-3
2. GRAPHIC CONVERSATION FOR 2-AXES LATHE
2.4Automatic Selection of Tools, Cutting Conditions and Pre-tools
The ideal tools and cutting conditions for each
machining process can be automatically set
during program preparation. Automatic
programming for pre-machining , as required
for drilling, is also possible.
(1) Tool file
Up to 40 tools in 17 types - tools for generai-
purpose lathe, tools for thread cutting, etc.- can
be registered. The most suitable tools for each
type of machinig can be selected automatically.
em TOOL DATA (1) *** TOOL TYPE OUTTEB ( LEFT ) T-CODE 01 PFPSET NO. 81 REVOLUTION-D NORMAL GEOHETRY OPS X- 0.009 z- 0.800 WEAR OFFSET X= 0.080 z- 0.008 NOSE-RADIUS RN= 5.000 CUTTING EDGE AC- 130 NOSE ANGLE AN- 30 IHGrSRY NOSE TD- TL MATERIAL TM- HI-SPD TOOL LIFE TT- SPARE TL NO. OFFSET NO [ )( l
(2) Cutting condition file
For all tools registered in the tool file, cutting
speed and feedrate can be set to each of 8
different types of machining materials. Based
on the data determined here, the ideal cutting
conditions for each machining can be set
automatically.
*a* MACHINING CONDITION (GENERAL) S*S ROUGHIHG
HI-SPEED MATERIAL FEED/REVCUT SPD. CUT DPTH
U/REV. 1 WIN. ) w 1, PC25 - 50. 0 2 000 2. FCD45 8.3880 60. 0 1.500 3. ss41 8.8588 120. 0 3.880 4. s45c 0.4808 20. 0 1.200 5. SKDll 0.2500 65. 0 2 800 6. SUS384 0.2000 136.0 1.280 7. AL 9.8000 110.8 3.800 8. 0.0008 PC25 111111 ::rPUT ‘* “’
( I( I( )mT=l( 1 ._ __ __ -_ _ -me- --
(3) Coefficient data file
With general-purpose tools, the ideal cutting
speed for the given feedrate can be
automatically set. Simiarly, for drill tools the
ideal feedrate can be set automatically for each
nominal diameter.
\
~SS MACHINING CONDITION (COEPICGRV.*
GRV WIDTH m 4 10 20 ooo -ef-- wT--J LT--J Lf--J LeT--
HI-SPD 0.500 a 700 0.900 1.008 1. lee CARBID 8.760 0.808 0.900 1.880 1. 190 SPCIAL 8.900 0.950 1.800 I. 050 1. 106
(PEED/REV.) GRV WIDTH
( )( rr*%yf ) . . -_ _ _--- --
(4) Pre-tool list
For drilling tasks, it is possible to register the
tools required for pre-machining prior to final
machining. Based on the pre-machinig data
determined here, it is possible to automatically
prepare the pre-machining program needed for
drilling.
*$$ PRE-TOOL LIST *** NO. 81
TOOL NO. TL NAME NOMINAL DLAST TL m TAP 12. 806
PRE-TOOL 1 701 CNTRDRL 2 681 DRILL ll. 776 3 4 5
I
2-4
2. GRAPHIC CONVERSATION FOR 2-AXES LATHE
2.5 Dynamic Graphic Display (for lathes)
Prepared machining programs can be
graphically displayed on the screen for close
checking prior to actual machining. Two
display methods are offered.
(1) Tool path display
The tool nose movement is described on the
screen as a thin line.
(2) Animated simulation
The material profile, chuck and tailstock are all
displayed on the screen in their true
dimensions. An animated simulation illustrates
how the material will be cut progressively
according to the programmed tool movement.
 GRAPHIC CONVERSATION FOR MACHINING CENTER
3.
(1)
GRAPHIC CO’NVERSATION FOR MACHINING CENTER (O-Mate MF /O-MF)
Operating guidance
Each required operation is displayed in order
on the screen. So even inexperienced
.operators can master all operations with no
special training.
PROGRAM 00002 NO000 CONTOUR POCKET CUTTING (11 G220 COORDINATE 9 1
Z COORDINATE 2 -20. R POINT R 3. CUTT’G AREA X X 0,
(MIN.) Y Y 0. CUTT’G AREA X I 200.
<MAX.) Y J- 200. CHAMFERING C 1. 0:x 1:Y *D 0 RGH.B:EX l:NO*P 0 BOTTOM FINISH V 0. 2 CUTTING DEPTH Q 3.
DATA+il.NPAT LAST!INk ( YENU)( I( 1i 1( 1
/ Y
PROGRAM 00002 NO000 , ** MACHINING PROCESS ** 1. INITIAL SET
2.DRILLING [DWELL] TOOL NO. T-CODE TOOL NAME NORM DIA
2 2 CENTER 2.000 3. DEEP HOLE DBILING TOOL NO. T-CODE TOOL NAME NORM DIA
1 1 DRILL 3. 000 4.TAPPING TOOL NO. T-CODE TOOL NAME NORM DIA.
3 3 TAP 3. 000
t MENU ]( 1( )( 1t I
(2) Process list display
After a machining program has been prepared
through conversational input, a list of its
required processes , including tools to be used,
can be displayed. This feature enables fast,
easy verification of the machining order, tools,
etc.
3.1 Keytouch
(1) Automatic pre-tool selection
During drilling program preparation, once the
final hole depth and tool number have been
input, the system automatically prepares the
preliminary processes that are required prior to
the drilling desired.
PROGRAM 00002 NO020 TAPPING 6113 TOOL NO. *T 3 COOLANT *Id 0
I RET. POINT 1 0. R POINT Z POINT CHAMFERING x DWELL *ctp O:R 1:x *B 0:NORM l:RIGD*Q
OFFSET NO. *H SPINDLE SPEEDeS FEEDRATE F DEPTH OFST. y
(=NtJ I( It )(PBB-TL)( I
(2) Automatic setting of cutting conditions
Once the operator inputs the numbers of the
tools required for the machining at hand, the
system automatically determines the most
suitable spindle speed and feedrate.
PROGRAM 00002 NO050 CONTOUR POCKET CUTTING (21 G221 7 FINISHING J 0. 2 k '_a a.1 ROUGH COOLANT *M 8 v’::.‘! 7 END-ML CUT WIDTH<70XSR 70 12. 000 RGH.TOOL NO. *T 7
SPINDLE *S 2123 7 FINISH FEEDRATE XY F 1274. +;. P END-ML / FEEDRATE Z Q 637. 10. 000
FIN. TOOL NO. tP 8 SPINDLE *J 5095 I TCHAMFR FEEDRATE K 1529. CHF.TOOL NO. *C 9 -",,""g;R
SPINDLE rU 1274 DATA--,ti FEEDRATE V 382. -bAT LAS~m
c MENU It It If It 1
2-6
3. GRAPHIC CONVERSATION FOR MACHINING CENTER
3.2 Menu Screen
A complete selection of menus has been
prepared to accommodate all programming
needs - everything from drilling, facing, side
cutting, grooving and pocketing to auxiliary
functions and NC language menus. This
enables the inexperienced operator to proceed
with effortless ease, and at the same time
permits the experienced operator to make
maximum use of the machining knowhow.
PROGRAM 00002 NO050 *s FACING MENU ** I. SQUARE FACING [Xl 12. SQUARE FACING [Y] !
.- I .B---- : r - * * h / .Z) r....!
PROGRAM 00002 NO050 ** SIDE CUTTING MENU f* l.CIRCLE OUTSIDE 12.SOUARE OUTSIDE ;
.T &I I )*-.I I +.
I + ! I cy I 'u I I v j
3- TRACK OUTSIDE 14. CIRCLE INSIDE I f
.
ITEM NO. +m] )
( MENU )( )( )( )( 1
-.-- -“1 : -*. ir I 4 c- T--k =- a -4; “u-
OTHER ITEMS 1
. DE,PRESS THE RIGHT SOFT KEY ITEM NO. +iJNPUT[)
PROGRAM 00002 NO050 F* HOLE MACHINING MENU It* 1 DRILLING . 2.DRILLfNG (DWELL1
I:
m
l&J I 3 . DEEP Hoti DRILLING 4. RAPID DEEP HOLE
?;?,A 1,
I ' ; + I&; I
I' jj,
I / I*: \li
1 J
OTHER ITEMS, DEPRESS THE RIGHT SOFT KEY ITEM NO, *b-a)
PROGRAM 00002 NO050 ** SIDE CUTTING MENU ** 5. CONTOUR SIDE CUT !6. CONTOUR GROOVING 1
OTHER ITEMS, DEPRESS THE RIGHT SOFT KEY ITEM NO. -B-T:)
( MENU )( l( It I( I t MENU )( N I( I( I
PROGRAM 00002 NO050 ** HOLE PATTERN MENU tt 1.4 POINTS '2. LINE AT ANGLE
-. -8 ..C -a _.a
..;? 1-1
3. GRID - I ,z' !4. SQUARE
" j
+ ? I
-b 1 I
Y ” d .A I OTHER ITEMS , DEPRESS THE RIGHT SOFT KEY ITEM NO. +gNPUTi)
PROGRAM 00002 NO050 ** POCKETING MENU ** 1. CIRCLE POCKET 12,SQUARE POCKET I
.-R. m . ., ‘i
I ((I I,jj
‘-zY ,: I ’ ‘W” &TRACK POCKET &CONTOUR POCKET 1
ITEM NO. +=I )
( MENU )( I( I( )( 1
2-7
3. GRAPHIC CONVERSATION FOR MACHINING CENTER
/ 3.30ptimum Tool Order 3SArbitrary Profile Machining
The machining order is automatically adjusted
to carry out the programmed machining task
using the least number of tool changes from
start to finish. This eliminates the need for the
programmer to give consideration to tool order
during program input.
'ROGRAhf 00002 NO050
;TART OF PROCESS G202
CHANGE OF TOOL OPERATION SEQUENCE IS AVASLABLE IN A PROCESS
A PROCESS IS MADE UP OF THE BLOCKS BETWEEN START OF PROCESS AND END OF PROCESS
'kii?j KEY DEPRESS ( MENU It I( I(
3.4 Multi-piece Machining
Programs
Arbitrary profiles can be specified easily using
Symbolic input and the automatic intersection
computation function. The specified profile
appears graphically on the screen immediatery,
thus enabling fast and easy checking and
revisions. It is also possible to perform contour
side cutting, contour grooving and contour
pocketing of specified profiles.
PROGRAM 00002 NO050 CONTOUR FORM [S ELEeT'--6-ih-i-s-s-E_Ncl CROSSING NMB. '- _P
_.-- 1 r--r-- __ -. .- -. . .
X 10+ 000 Yfi 10.000
-. ,‘2 *’ SELECT C&S S 1 NC 1 &--z---+--*-=’
DATA+lNPl+AT LAS#-] c ++ I( t .i---3r---~ I( 1t 0 )(CANCEL)
To machine idential products in multiple
quantities at the same time, the operator need
prepare the program only for one piece. The
remaining pieces can be programmed
automatically, inclusive of the optimum tool
order.
(1) Contour side cutting
Sides of arbitrary profiles which are formed
from lines and circles can be programmed
through conversational input.
/ \ PROGRAM 00002 NO050 MULTI-PIECE COORd'INATE
G206 9
NUX.OF PIECE +P 10 y NUMBER<X> *H 3 X PITCH I 120. Y PITCH J 100.
?
2-8
3. GRAPHIC CONVERSATION FOR MACHINING CENTER
(2) Contour grooving
Grooves of arbitrary profiles where the center
line is formed from lines and circles, as shown
in the illustration, can be programmed through
conversational input.
(3) Contour pocketing
Pocketing of arbitrary profiles having islands
such as shown in the illustration can be carried
out automatically simply by preparing, through
conversational input, the exterior walls of
pockets and islands formed from lines and
circles. Up to 6 islands can be designated,
each with a different height if necessary.
3.6Automatic Selection of Cutting Conditions and Pre-tools
The ideal cutting conditions for each machining
can be automatically set during program
preparation. Automatic selection for pre-
machining, as required for drilling, is also
possible.
(1) Tool file
Up to 45 tools in 9 types - drills, taps, end
mills, etc. - can be registered.
TOOL FILE :03 00002 NO002 TOOL NO. 7 0 9 T-CODE 7 8 9 TOOL NAME -END-ML END-ML CHA?dFR TL MATERIAL HI-SPD HI-SPD HI-SPD NOMINAL DIA. 12. 000 10. 000 20. 000 PITCH/S-DIA 0. 000 0. 000 4. 000
TOOTH/C-DEP. 3 3 0
ANGLE 0 0 90 OFST NO. [HI 7 8 OFST NO. [Dl 17
l 18 19
DEPTH OFST. 0. 000 0. 000 0. 000 OTHER TOOLS. DEPRESS THE RIGHT SOFT KEY NUM. -
(DRILL )(CENTER)( TAP )(REAwR)(BoRE )
(2) Cutting condition file
For all tools registered in the tool file, cutting
speed and feed rate can be set to each of 8
different types of machining materials
MACHINING COND. WILL) :Ol 00002 NO002 HI-SPDEND-ML 1s. DIA OMMI ROUGHING MATERIAL FEED F-XV FEED F-Z SPEED V
(MM/tOfH) (MM/TOTH) <M/MIN.) l.FC25 0. 200 0. 100 80. 000
- 2.FCD45 0. 100 0. 050 90. 000 3. ss41 0. 500 0. 300 120. 000 4. s45c 0. 100 0.080 80.000 5. SKDll 0. 300 0. 100 60. 000 6. SUS304 0. 200 0. 100 50. 000 7. AL 0. 800 0.400 110. 000 a. 0. 000 0. 000 0.000
NUBL -
(FACE-M)(END-ML)( )( 1( 1
2-9
3. GRAPHIC CONVERSATION FOR MACHINING CENTER
(3) Coefficient data file
To accommodate cutting conditions which vary
according to tool diameter, it is possible to
apply a coefficient for each set of cutting
conditions. Used together with the tool fiie
in(l) and the cutting condition file in (2), it is
possible to automatically set the ideal cutting
conditions for each machining.
MACHINING COND. KOEFFl :Ol 00002 NO002
DRILL-DIA. _ 2 6 10 20 <MM)
HI-SPD 0.500 0.800 1.000 1.200 1.500 CARB ID 0. 800 0.900 1.000 1.100 1. 300 SPCIAL 0. 900 1. 000 1. 100 1. 200 1. 300
TAP-DIA 2 3 5 8 (MU)
HI-SPD 0. 500 0. 700 0. 900 1. 000 1. 200 CARBID 0.400 0.600 0.800 1.000 1.200 SPCIAL 0.500 0.700 0.900 1.000 1.200
NUbL -
(4) Pre-tool list
The pre-tool list can be used to register up to
20 pairs of pre-tools, finishing tools and
auxiliary tools in max. 4 tools. Based on the
pre-machining data deteamined here, it is
possible to automatically prepare the pre-
machining program needed for drilling.
/ \
PRE-TOOL LIST :Ol 00002 NO002 TOOL NO. CYCL TOOL NAM NOM DIA
LAST TL. 1 _ 3 6 TAP 3.000 2 1 3 DRILL 3.000
PRE TOOL 3 2 2 CENTER 2.000 4 0 0 0.000 5 0 0 0.000
l-DRILLING ?-COUNTER TAPPING 2-DRILLING [DWELL) 8-BORING 31DEEP HOLE DBILING S-RAPID BORING Q-RAP ID DEEP HOLE lo-BACK BORING S-HOLLOW DRILLING 11 -BORING [DWELL) 61TAPP ING 12-FINE BORING NU?& -
3.7 Dynamic Graphic Display (For machining center)
Prepared machining programs can be
graphically displayed on the screen for visual
checking prior to actual machining. Two
display methods are offered.
(1) Tool path description
The tool path is described on the screen as a
line. This feature enables a close check of the
prepared program.
0 Because description proceeds at high
speed, the program check can be completed
quickly.
PAT 'H GRAPHIC [EXECUTION] :I /I 01 .I 126 N1126
I -*
12. 9
@J An automatic scaling feature is provided
which permits the operator to maintain a
suitable magnification and keep the focus
of attention in the middle of the screen at
all times.
8 During screen monitoring,, the center of
partial enlargements and the rate of
magnification can be commanded when
needed. This feature enables simple
enlargement of sections demanding closer
attention.
2- -lo
3. GRAPHIC CONVERSATION FOR MACHINING CENTER
c I
10. 1 .
8 In addition to 2-dimensional drawings, it is
also possible to describe isometric
projections or bi-plane drawings
simultaneously.
PATH GRAPHIC 01126 N1126
I I 15. 1
( AUTO )(START )( STOP )[I~EwINJJ)(~RASE )
PATH GRAPH1 C [EXECUT 1 ON) 01126 N1126
( AUTO )(STMT )( STOP )(REwIND)(ERASE )
a The precise current position of the tool can
be displayed on tool path description. This
enables the operator to know the exact
machining status at any time.
(2) Machining profile description
The changing profile of the workpiece is
simulated according to the movements of the
tool as programmed. Because the profile is
shown in 3 dimensions, the operator can check
the machining program in detail with great
ease.
SOLID GRAPHIC [BLANK) 01126 N1126
( ANEW )(+ ROT )[- ROT )(+TILT I(-TILT )
SOLID GRAPHIC iREVIEW 01126 N 126
( ANEW )(+ ROT )(- ROT )(+TILT )(-TILT )
Q The coordinate axis and projection angle
can be changed at random.
SOLID GRAPHIC (REVIEW 01126 N1126
[ ANEW )(+ ROT I(- ROT )(+TILT )(-TILT )
2- 11
3. GRAPHIC CONVERSATION FOR MACHINING CENTER
SOLID GRAPHIC [REVJEW] 01126 N1126
2
L * Y
( ANEW )(+ ROT )(- ROT )(+TILT )(-TILT )
SOLID GRAPHIC [REVIEW) 01126 N1126’
( ANEW )(+ ROT )(- ROT )(+TILT )(-TILT )
@ The tool can be attached not only in
paraliel to the Z-axis, but alternately in
parallel with either the X-axis or Y-axis.
8 In addition to 34mensional drawings, it is
also possible to describe 2-dimensional
drawings or tri-plane drawings
simultanenously. .---
SOLID GRAPHIC [REVIEW 01126 N1126
( ANEW )(+ ROT )(- ROT )(+TILT )(-TILT )
SOLID GRAPHIC [3-PLANE1 01126 N1126
29 12
APPENDIX
APPENDIX 1 TABLE OF RANGE OF COMMAND VALUE
APPENDIX 1 TABLE OF RANGE OF COMMAND VALUE
(1) T series
Linear axis (in case of metric thread for feed screw and metric input)
lncremen t system
Standard O.lE(
Least inpt increment [ 0.001 mm IO.0001 mm
I X:0.0005 mm I X:0.00005 mm Least command increment Z:O.OOl mm ZO.0001 mm Max. programmable
dimension I t 99999.999 mm I + 9999.9999 mm
Max.rapid traverse
Feedrate range
*1 100000 mm/min 24000 mm/min
1 - 12000mm/min *I
1 - 100000 mm/min
0.0001 - 500.0000 mm/rev 0.000 1 - 500.0000mm/rev
Step feed
Tool compensation
Backlash compensation
Dwell time
0.001, 0.01, 0.1, 1 mm/step
0- k999.999 mm
0- to.255 mm
0- + 99999.999 set
0.001, 0.01, 0.1, 1 mm/step
0- 2 999.999 mm
0- +, 0.255 mm
0- 2 99999.999 set
Linear axis (in case of metric thread for feed screw and inch input)
I ncrement sys tern
Standard 0.0000 inch
least input increment I 0.001 inch I 0.00001 inch
Least command increment X:0.000005 inch
Z:O.OOOl inch
X:0.000005 inch
Z:O.OOOOl inch .

When regarded as a whoie system, limitations depending on servo system must also be
considered.
A-3
APPENDIX 1 TABLE OF RANGE OF COMMAND VALUE
(2) M series
Linear axis (in case of metric thread for feed screw and metric input)
Increment system
w Standard I 0.1 &I Least input increment 0.01 mm I I 0.001 mm I 0.0001 mm
Least command
increment I -~
0.01 mm 0.001 mm I
0.0001 mm
Max. programmable dimension
Max. rapid traverse *1
k 999999.99 mm 4 99999.999 mm * 9999.9999 mm
240000 mm/min 100000 mm/min 24000 mm/min
Feedrate range *l 1 - 150000mm/min 7 - 1 OOOOOmm/min I- 12000mm/min
Step feed 0.01, 0.1, 1, 10 mm/step 0.001, 0.01, 0.1, 1 mm/step 0.0001, 0,001, 0.01) 0.7,
mm/step
Tool compensation
Sacklash compensation
0- ? 999.99 mm 0- 2 999.999 mm 0- +999.9999 mm
0- t2.55 mm 0- 2 0.255 mm O- 20.255 mm
Dwell time I 0- * 99999.999 set I 0- rf: 99999.999 set I 0- ? 99999.999 set
Linear axis (in case of metric thread for feed screw and inch input)
Increment system
Standard I 0.1 E”
Least input increment 0.001 inch 0.0001 inch 0.0000 1 inch
Least command
increment 0.01 mm 0.001 mm 0.0001 mm
Max. programmable
dimension I 2 99999.999 inch
I + 9999.9999 inch
I k 393.70078 inch
Max. rapid traverse
*7 I 240000 mrn/min I 100000 mm/min I 24000 mm/min
Feedrate range *l 0.01-6000 inch/min 0.01-4000 inch/min 0.0 I- 480 inch/min
Step feed 0.001, 0.01, 0.1, 1 0.0001) 0.001, 0.01, 0.1 0.00001) 0.0001, 0.001, 0.01 inch/step inch/step inch/step
Tool compensation I 0- It99.999 inch I 0- ,+ 99.9999 inch I 0- + 99.9999 inch Backlash
compensation 0- & 2.55 mm 0- f0.255 mm 0- 20.255 mm
Dwell time I O-99999.999 set I 0- 99999.999 set I 0 - 9999.999 9sec
A-4
APPENDIX 1 TABLE OF RANGE OF COMMAND VALUE
Linear axis (in case of inch thread for feed screw and inch input)
Increment system
% Standard 0.1 p
Least input increment 0.001 inch 0.0001 inch 0.00001 inch
Least command increment 0.001 inch 0.000 inch 1 0.00001 inch
Max. programmable dimension ,+ inch 99999.999 5 9999.9999 inch 2 9999.9999 inch
Max. rapid traverse *1 9600 inch/min 4000 inch/min 960 incWmin
Feedrate range *l O-01- 6000 inch/min 0.01 - 4000 inch/min 0.01-480 inch/min
Step feed 0.001, 0.01, 0.1, 1 0.0001, 0.001, 0.01, 0.1 0.00001, 0.0001, 0.001, 0.01
inch/step inch/step inch/step
Tool compensation 0- + 99.999 inch 0- 2 99.9999 inch 0- f 99.9999 inch
Backlash compensation 0- 0.255 inch + 0- 20.0255 inch 0- + 0.0255 inch
Dwell time 0- 99999.999 set 0 - 99999.999 set 0- 9999.9999 set
Linear axis (in case of inch thread for feed screw and metric input)
Increment system
Standard 0.1 p
Least input increment 0.01 mm 0.001 mm 0.0001 mm
Least command increment 0.001 inch 0.000 1 inch 0.0000 1 inch
Max. programmable dimension
Max. rapid traverse *7
& 999999.99 mm
9600 inch/min
T
2 99999.999 mm + 9999.9999mm
4000 inch/min 960 inch/min
Feedrate range *l I 1 - 150000 mm/min I 1 - 100000 mm/min I 1 - 12000 mm/min
Step feed
Tool compensation
0.01, 0.1, 1, 10 mm/step 0.001, 0.01, 0.1, 1 mm/step
0.0001, 0.001, 0.01, 0.1
mm/step
0- f 999.99 mm 0- + 999.999 mm 0- +999.9999 mm
Backlash compensation 0 - 2 0.255 inch 0- 2 0.0255 inch 0- It 0.0255 inch
Dwell time 1 O-99999.999 set I O-99999.999 set 1 O-9999.9999 set
A-5
APPENDIX 1 TABLE OF RANGE OF COMMAND VALUE
Rotation axis
I v
Increment system
Standard 0.0001 deg
Least input increment 0.001 deg 0.0001 deg
Least command increment I 0.001 deg I 0.000 1 deg
Max. programmable
dimension f 99999.999 deg 4 9999.9999 deg
~~ ~~ Max. rapid traverse *l I 100000 deg/min I 24000 deg/min
Feedrate range "1 1 - 100000 deg/min 1 - 12000 deg/min
Step feed 0.001, 0.01, 0.1, 1 .deg/step 0.0001, 0.001, 0.01, 0.1 deg/step
Tool compensation I 0- 2 999.999 mm I 0- ,+ 999.9999 -mm
I
Backlash compensation I 0- 2 0.255 deg I 0- 2 0.255 deg Ilr
*I The feed rate range shown above are limitations depending on CNC interpolation capacity.
When regarded as a whole system, limitations depending on servo system must also be
considered.
A-6
APPENDIX 2 FUNCTION AND TAPE FORMAT
APPENDIX 2 FUNCTION AND TAPE FORMAT
(1) T series The symbols in the list represent the followings: P _..X_~-
As seen above, the format consists of a combination of arbitrary axis addresses among X, 2. x- l First basic axis (X) z* l Second basic axis (z)
Functions Illustrations
-inear interpolation(G01)
>ircular interpolation (G02,G03) /
lwell(G04)
Change of offset value by program
I nch/metri conversion
(G20,G21)
Spindle speed fluctuation detection G25;
(G25,G26) G26P-Q-R-;
Reference point return check
(G27)
G27g - ;
L
Tape format
GO@_ ;
GO@_ F_ ;
. GO2
GO3 . >
F-;
GO4 x- ;
i 1 P- Geometry offset amount
G1 OP_X_Z_R_Q_;
P = 10000 + Geometry offset
amount
Wear offset amount
Gl OP_X_Z_C_Q_;
P = Wear offset amount number
Inch input
Metric input
G20;
G21;
A-7
APPENDIX 2 FUNCTION AND TAPE FORMAT
Functions
Reference point return (G28)
2nd Reference point return(G30)
Tool nose R compensation
(G40,G41 ,G42)
Skip function(G31)
illustrations Tape format
Reference point
:n:;z: ~~~~~i
FGQ 1:; ]+;
;z: /;k;s;g;;, p G31P-F-;
Thread cutting(G32) F
A
Equal lead thread cutting
G32P-F-;
Automatic tool compensation
(G36,G37)
Measurement point
Arrival point G36X xa ;
~----- Measure- Start
I-4 ment
point point G372 za ;
Off set value
Coordinate system setting
Spindle speed setting(G50)
X G50X-Z-;
I+
z
(Coodinate system setting)
G50S - ;
(Spindle speed setting)
z
Mirror image for double turret
(G68,G69)
. G68; 9 Mirror image for double turret on
G69;
Mirrur image cancel
A-8
APPENDIX 2 FUNCTION AND TAPE FORMAT
Functions
>ustom macro(G65)
=eed per minute /feed per revolution
Zonstant surface speed control
;G96,97)
Chamfering and corner R
Canned cycle for cutting(G71 -G76)
(G90,G9z,Gw)
liiustrations
Macro instruction
Format
sCifiHmP#iQ#jR#k;
m;Display function of macro by 01 - 99
#i;Name of variable to which arithmetic
result is entered.
j;Name 1 of variable to be calculated.
.k;Name 2 of variable to be calculated.
Meaning)#i = #j@#k
f
Display by operator Hm
nm/min inch/min
n m/rev inch/rev
n/min or feet/min
N&pm)
_.-. ._ 3 1-I 1 . -.-.C) -. ._.-.-. il’-1- _
See “Canned cycle”.
Tape format
365HmP#iQ#jR#k;
G98 ...... F-;
G99 ...... F-;
G96S - ;
G97; . . . . . .  - - -’
A-9
APPENDIX 2 FUNCTION AND TAPE FORMAT
(2) M series
The symbols in the list represent the followings: P :X Y Z A
AsseG above, the format consists of a combination of arbitrary axis addresses among X: First basic axis (X usualiy) Y: Second basic axis (Y usually) Z: Third basic axis (Z usually)
Functions Illustrations
Positioning (GOO)
Linear interpolation
(GOV
Start point /l
Start point /
Circular interpolation
(Gw,G03)
(In case of X-Y plane)
Iwell (GOa)
Exact stop(G04) Speed
l qTime Change of offset value by program
(G10)
Tool length compensation B
(G39-G42)
Tool length compensation C
(G40- G42)
G40
Tape format
GOOP_ ;
GOOP--F-;
GIOP-R-;
H : Tool offset number
A- 10
APPENDIX 2 FUNCTION AND TAPE FORMAT
Functions
Tool length compensation A
(G43, G44, G49)
illustrations
LL
Offset \ / \ / \ /
Z 7
Tape format
G43
{
Z H - G44 J - -’
G43
i
1 H ;
G44 - J
H : Tool offset No.
G49 : Cancel
Tool length compensation B
(G43, G44, G49) {!;) [;~){+_;
i i
b; 1 /G43 1 H ;
G19 J G44 -’ J
H : Tool off set No. G49 : Cancel
Inch/metric conversion
(G20,G21)
Reference point
return check(G27)
Reference point return
W3)
2nd reference
point return(G30)
Return from reference point(G29)
inch input
Metric input
;ta; / p G27P-;
Reference point
ln3 FZrZ ““”
Reference point G29P-;
ap Intermediate point
G20;
G21;
Skip function@31 ) )/) /‘a p
G31P-F-;
Skip signal
A- 11
APPENDIX 2 FUNCTION AND TAPE FORMAT
Functions
Custom macro A
:G65, G66, G67)
illustrations Tape format
Macro instruction G65HmP#iQ#jR#k;
Format
G65HmP#iQ#jR#k;
m;Display function of macro by 01-99
#i;Name of variable to which arithmetic Modal call
result is entered. G66P_;
#j;Name 1 of variable to be calculated. G67: Cancel
#k;Name 2 of variable to be calculated.
(Meaning)#i = #jWk
+
Display by calucurate Hm
Canned cycles
(G73, G74, G80- G89)
See item “Canned cycle” in the main G80; a. - -- Cancel text. G73
G74
G76 1
G81
J
x Y z
p;; F K . ----- .
G89
Absolute/incremental
programming
(GWG91)
Change of work
coordinate (G92) w
L
P
G90 ; Absolute programming ’
G91 ;
Incremental programming
G90_G91 ; Combined use -
G92P ;
Initial point return/
R point return
(G98,G99)
G98 G98 ; + I point G99 l I
R point
Z point
A- 12
APPENDIX 3 LIST OF CODE
APPENDIX 3 LIST OF CODE
(1) T series .
IS0 code I 1 8
1 EIA code Character 7 1 6 3 1 4 ’ ’ 3 1 ! 2 1 Character 8 0. I IO 0
71615141 0. 1 0 0 !ol _ 1 I 01 I ! Numcra I
r fo!o. 101 01
1 I I I I ’ I I0 I Id I Numeral1
M caning
h 6 7 8 9 A I B C D E F / G H
010 IO I I Numeral 5 I
~“!O!OIO!  Numeral8 A - , , _ , I . I I f Oi I Numeral 9
lop!q !olO!Ol 1 Address F ! I !OIOi 1 AddressG
I O i 01 I I ? f Address D 1
L M N 0 P
.Q R S
I 101 ! 1 Address!4
r _-
[o[o/ 1 ~~I”lOIO~ 1 n I I T , oqo
! ! I I I r I r . . _ Y
2 AC.
“1 t”lq”l 1 1 1 s I I O~O! o .OIO 01 AddressX _g_olo 0 1 1 ? Address Y
I ! 01 -0’0 c 0 lo Y
o[ 0 0 0 01 z 0 -.-, 5 I ~ lo r 010 ! 1 Address 2 1 I toro 0 olo 010 0 l 1 bbtp ~~*-~el an mwnt nrtrrrk\ .
VU0 t IO OjOjO OlolO O/O Del
NUL i I 1 I 1 I I - ! - I - I -w*-*~ \.arbbwa -.. ..,“a yur,L,r,.
0 Blank 1 1 / f 1 ] 1 1 0 l Not punched. Cannot be used in
BS HT I ’
01 I I I I I 1 !oloi 1 ! 1 1 1 1
BS 1 significant section in EIA code.
1 01 001 0 1 * 1 Back space ,
1 /dot i /nj Ts), Inle n -lnl-l 1 a 1 -. .
L
ILForNL 1 I 1-1-1 I
, I I - 1 Iabulator I I -_
Absolute rewind stop
1 OPtional block skip
!i I I I I * I Dollar sinn ml
- 1 1 Aiterisk’ B 0
, 1010 0 ’ . B 01 0 oloio 1 1 ,-,- I I iol0lOi
0 0
1 I I vi
l Left angle bracket 1 I+ Fnrt51 .
A- 13
APPENDIX 3 LIST OF CODE
(2) M series
. IS0 code EIA code T
Character 8 7 6 5 4 3 2 1 Character 8 7 6 5 41 131 21 1 _O 00 O 10 . 0
Meaning
I I,
0 Numeral 0 1 1 101 color 101 I JOI 1 I I I I I 0 0 Numeral 1 I
2 0 00 0 0 2 0 2 3 00 0 (3, 0
0 1 Numeral 3 0 01 00 Numeral 3
4 I 1 1
0 loo I I0101 I I4 1 I 1 1 1 IolOl 1 1 INumeral 5 0 0 f 0101 101 5 6
1 I 1 r I T I ! ! ! !Oj !0!0! !O! ! Numeral5 00 I I Ol c\lOl I 6 I I I IOI lo IOIOI I I Numeral6 1
7 0 00 0~000 i 0 0 Ooool
7 8 0 l3-
I 010 Numeral 0 0 Numeral 8
-0.1 9 000 0 Numeral 9
lrxT’
-.__ 1 1 I -_
P
.Q R
T .- - - - . . x ’ 0 -L --.-- 0 --_.. J 0 P
0 0
0 +o o- 0 --I___.- Address P
00 0 0 0 9 6 - -o&J -. Address --- _I_ Q
00 0 0 0 r lo 0 0 0 Address R I 3 a._. 0 .- _.._ -~~, 0 oo’i _-so o__o Address S
3 0 -.-- 00 -t 0 0 0 0 Address T
I0lOl “I I l_ 1 x I I IOWl IOIOIOIOI I AddressX
I NUL , , , ,, , , b,
BS d __ HT __.,e--.*- -..._ _-..-_.__ .- LF
- -- or NL 00 0
CR 0
SP 0 0 :’ % 01 0 ( 1 0 1 01 0
t-illI- I I + I Carriage return
_C_C.U_ $0 ! 0 ! ! l !  _
Qn
Negative sign colon
.-.-_ _ -
Space Absolute rewind stop Conttnl mlt ls rnmmmn* ir r*m-+sA\
1 0 I I I 0 I I Optional block skin Period (A decimal Point)
+ Sharbe I I --a--
* Dollar sign
l
- - I Asterwc 9 010
I 1
0 0 1010 * Comma . I I I- . ; 0 0,o 0 01 0 0 1 I I I I I ololo 40
c
re
1 I tKI* I Semicolon I I I 1 1 I
l Left angle bracket Y
0 000~~~0 01 0
+ Equal 000000 I l
000 0 oofo Right angle bracket
0 I
* Question mark 0 0. *
0 0 01 / I I I I Commercial at mark
1 I l Quotation
1
I
I
A- 14
APPENDIX 3 LIST OF CODE
(Note 1) *When read in the significant data zone,the codes are ignored.
(Note 2) ?:The codes are invalid in the significant data zone, but are registered in the memory. (Note 3) Codes not in this table are ignored if their parity is correct (Note 4) Codes with incorrect parity cause the TH alarm. But they are ignored without
generating the TH alarm when they are in the comment zone.
(Note 5) A character with all eight holes punched does not generate TH alarm even in EiA code.
A- 15
APPENDIX 4
APPENDIX 4 EXTERNAL DIMENSIONS
EXTERNAL DIMENSIONS
w -
OOP
01 082 O--
01
Fig.1 External view of control unit A
A- 16
APPENDIX 4 EXTERNAL DIMENSIONS
C lf- d
- C I(
- 00’0
c
.Ol e
08Z M
01
cs + + ;I III
Fig.2 External view of control unit B
A- 17
! 4 I
& --
-j l . 0 ’
I ’
I
iif
-_
C dn
ne ct
or
K M
1
I I /,i
A I
I I
’ r-
-- r
I I
In st
al la
tio n
di m
en si
on
D
u C
on ne
ct or
’ K
M 1
h,
I --
-,
7- J
-_ A
4
L ^-
#
u m
m
X
-I m
S lIl
Z
D
- 3 m
Z
APPENDIX 4 EXTERNAL DIMENSIONS
288
Fig.4 External view of small 9” color CRTIMDI
A- 19
APPENDIX 4 EXTERNAL DIMENSIONS
0 I-
__
0 I-
O
L
./ P a,
-
-
-
C-
I I LB I 3 c Q
Fig.5 External view af 9” monochrome CRT/MD1 with full-keyboard
A - 20
APPENDIX 4 EXTERNAL DIMENSIONS
184
-a--
[ CNl 4; ‘I--- L
b \\ I
I
1 288 ‘1 3
Fig-6 External view of 9" color CRT/MD1 with full-keyboard
A - 21
APPENDIX 4 EXTERNAL DIMENSIONS
*---
l --
0
1
--4- 4,
0 M
8 0
0 __ 1
. r-7 2 : ___k--
i
0 O
: n ./ : 0
t I
0 t
Fig.71 External view of EUMDI unit (Small Type)
A - 22
APPENDIX 4 EXTERNAL DIMENSIONS
, ml R R R El
-- El. R
I,
El R R R
,El /
Fig. 8 External view of 14” CRTAUIDI unit
A - 23
APPENDIX 4 EXTERNAL DIMENSIONS
+
I
-
Fig. 9
lf
-
External view of 9” monochrome CRT .unit
A - 24
APPENDIX 4 EXTERNAL DIMENSIONS
I I
cu LL-d -t 0
Fig. IO External view of EL unit
A - 25
APPENDIX 4 EXTERNAL DIMENSIONS
Fig. 11 External view of MD1 unit (Smafi Type)
A - 26
APPENDIX 4 EXTERNAL DIMENSIONS
l 061
00 ffl 00 00 .
Fig.12’ External view of MDI unit (Full-keyboard)
A - 27
APPENDIX 4 EXTERNAL DIMENSIONS
H 11
Fig. 13 Extemal view of position coder
A86L4026-0002#102: Max. 4000 rpm A86LOO264002#002: Max. 6OOO.rpm
A - 28
APPENDIX 4 EXTERNAL DIMENSIONS
f
t
I 099
-+-
Fig.1 4 External view of manual puke generator (A860-02OllrOOl)
A- 29
APPENDIX 4 EXTERNAL DIMENSIONS
230 .
7.5 215 7.5
m A -:_ci I r( t 1 1 J
P.C.B.
TP2 EONEOFCOYFARI
Fig.15 External view of input unit.
A - 30
Cover
\/
APPENDIX 4 EXTERNAL DIMENSIONS
Mounting panel hole working position
Mounting hole ‘(countersink)
I
FANUC .--0.
. .I.. ,.-.
. . *-a.
.  l .  /
Fig. 16 Extemai view of battery unit
A-31
APPENDIX 4 EXTERNAL DIMENSIONS
3. OUTER VIEW
Outer View of CRT/MD1 Unit
2-M4 (Bottom)
Color: Mancell N3 GS50 smooth finish
Stand (Example) ’ Jl
Lack for air flow Unit stand
(Example)
4 + +
. z - z$ - _
m
~~
+ I 2
/ 168 170 168
I Machining drawing ] ()_ M4 for mounting hole.

FE ED
.J
1.
I I
I I
I
I ‘I
I I
I I
E X
E C
U T
IO N
. S
P IN
D LE
C
O O
LA N
T
10 .
I
I I
I I
I I
I I
I
I JI
I
\I \
/ I/I
3 + L
-- -_
-l d_
_ h7
-y
“- _o
-
\ /
m
--_ __
_.
40 0
.  I-
C O
O LA
N T,
-1
I- SP
IN D
LE
-I
m
1
2
3
4
5
6
7
8
9
10
1’ 1
1 2
1 3
(C oo
rd in
at e)
APPENDIX 4 EXTERNAL DIMENSIONS
i----i_- _-_J--= -. ----i--_
I I I I I -- l
1 I 5: I I == I I I -- l I I I
1 I I slf I I
3
Fig.22 Machine operator’s for 9” monochrome CRT/MD1
A - 37
APPENDIX 4 EXTERNAL DIMENSIONS
A= I 1 I I
c--c-- L-4
-__
r--q--- -----i____-
I
I
I I
I
I I I I
_---__!----- *. ----i__-- _---!----- ‘\ I-___
-i-__
I I I I I I I 1
I- -1 L! II
51
R3i /
Fig. 23 Machine operator’s panel for 9” color CRT/MD1
A A 38
-M
\
17 0
17 0
]
I 10
_-
~ --_
_ ’ 1
ii
. 7
In st
al la
tio n
di m
en si
on
D
u u -O
A
P -
m
z u x -P m
X
p- I”
I[“ )
0 --
rl -I
m
II z D
I- C I zz
m
7 cn
0 Z m
-l
r- -7
L.. b
i
APPENDIX 4 EXTERNAL DIMENSIONS
0
0
0
-
0
0
0
0 El 0 0 0 .o 0 0
Ll Ll
cl 0 0 El 0 0 0
cl 0
Fig. 25 Machine operator’s panel for 9” CRT/MD1 with full-keyboard
A - 40
APPENDIX 4 EXTERNAL DIMENSIONS
Fig.26 External view of additional l/O B2
A - 41
APPENDIX 4 EXTERNAL DIMENSIONS
r
-
-
-
L
-- \
I
Fig. 27 External vie& of FANUC PPR
A - 42
APPENDIX 4 EXTERNAL DIMENSIONS
l-
N 0-l l-4
-
Fig.28 External view of FANUC cassette adapter
A - 43
APPENDIX 4 EXTERNAL DIMENSIONS
Fig.29 External view of floppy cassette adapter
A-44
APPENDIX 4 EXTERNAL DIMENSIONS
F-- ---
1 0-p -- -- - ‘_ -. r3 1 I I I
I I .~~-~~~~~~~~~~--~-~~~~ 1,:
Fig.19 External view of portable tape reader
A - 45
· No part of this manual may be reproduced in any form.
· All specifications and designs are subject to change without notice.