The bits from t1 to t4, corresponding to the 1st to 6th axes, have the fol- lowing meanings: 0: Distribution data is always constant. 1: Distribution data is variable or fixed. When the distribution data is variable or fixed, the bits from r1 to r4, corre- sponding to the 1st to 4th axes, have the following meanings: 0: Distribution data is read forward. 1: Distribution data is read backwards. Because the data consists of bits, it is necessary to use a binary�coded dec- imal value when setting it using the macro compiler and macro executor. Example) When constant data is assigned to the 1st and 2nd axes and variable data is assigned to the 3rd and 4th axes, #20004=12; (t4 and t3: 1, t2 and t1: 0)
⋅Constant data When the corresponding data type bit (t4 to t1) is 0, specify “distribution data value”.
⋅Variable data When the corresponding data type bit (t4 to t1) is 1 and the total number of fixed data items = 0, specify “(Storing start data variable No. of the distribution data)/10”.
⋅Fixed data When the corresponding data type bit (t4 to t1) is 1 and the total number of fixed data items is other than 0, specify “(Storing start data variable No. of the distribution data)/10”. The applicable value for the variable data and fixed data is 2001 to 8553. It is not possible to start storing data in the executable format from a variable No. that is not a multiple of 10. To read the distribution data backwards, set the variable No. of the data to be distributed last. For example, to read the distribution data in #25000 to #25999 backwards, set 2500 as the data assignment variable.
Set the length of the fixed data for the cycle. The first address of the fixed data must be specified by the data assignment variable. When the total number of fixed data items = 0 and the corresponding data type bit (t4 to t1) is 1, the data is regarded as a variable data.
� ����� ����
� Cycle repetition count
� Cycle connection data
� Number of data items
� Data type
� Variables assigned to data for the 1st to 4th axes
� Total number of fixed data items for the first to 4th axes
B–61393E–2/02 11. PROGRAM COMMAND
581
#7 0055
#6 IT2
#5 IT1
#4 IT0
#3 #2 #1 #0 CSP (T series)
IT2 IT1 IT0 (M series)
[Data type] Bit
CSP Cs contouring control function dedicated to a piston lathe is 0: Not used. 1: Used.
IT0, IT1, IT2 IT2 IT1 IT0
0 0 0 Interpolates the G05 data in 8ms
0 0 1 Interpolates the G05 data in 2ms
0 1 0 Interpolates the G05 data in 4ms
0 1 1 Interpolates the G05 data in 1ms
1 0 0 Interpolates the G05 data in 16ms
1 1 1 Interpolates the G05 data in 0.5ms
0597 Maximum number of simultaneously controlled axes when G05 is specified during high–speed cycle cutting or No. of controlled axes in high–speed remote buffer
[Data type] Word
[Unit of data] 1 to 4 This parameter sets the maximum number of simultaneous control axes when G05 is specified during high�speed cycle cutting or sets the number of control axes in a high�speed remote buffer.
Parameter
11. PROGRAM COMMAND B–61393E–2/02
582
������ Message Description
115 ILLEGAL VARIABLE NUMBER
The header contents are improper in a high–speed cycle cutting. This alarm is given in the following cases: 1. The header corresponding to the spe-
cified cutting cycle number called is not found.
2. The cycle connection data value is out of the allowable range (0 – 999).
3. The number of data in the header is out of the allowable range (0 – 32767).
4. The storing start data variable number of executable format data is out of the allowable range (#20000 – #85535).
5. The storing data variable number of executable format data is out of the allowable range (#85535).
6. The storing start data variable number of executable format data is over- lapped with the variable number used in the header.
Modify the program.
178 G05 COMMANDED IN G41/G42 MODE
G05 was commanded in the G41/G42 mode. Correct the program.
179 PARAM. (NO. 0597) SETTING ERROR
The number of controlled axes set by the parameter 0597 exceeds the maximum number. Modify the parameter setting val- ue.
WARNING Single block stop, dry run, feedrate override, automatic acceleration/deceleration and handle interruption are disabled during high�speed cycle cutting.
Alarm and Message
Warning
B–61393E–2/02 11. PROGRAM COMMAND
583
NOTE 1 Use of the high–speed cycle cutting function requires
expanded RAM and limits the maximum specifiable size of part program memory to within 80 m in terms of tape length.
2 Set the total number of distribution data items for one cycle to a multiple of the following values, according to the distribution cycle. This does not apply when the distribution cycle is 16 ms or 8 ms. If the total number is not a multiple of one of the following values, movement in the remaining cycle becomes zero.
Distribution cycle 4 ms: Multiple of 2 Distribution cycle 2 ms: Multiple of 4 Distribution cycle 1 ms: Multiple of 8
For example, when all 41 data items (distribution cycle: 2 ms) are specified, movement is zero in the remaining 3 ms.
OPERATOR’S MANUAL (For Machining Center) (B–61404E)
II.20 HIGH SPEED CYCLE CUTTING
OPERATOR’S MANUAL (For Lathe) (B–61394E)
II.20 HIGH SPEED CYCLE CUTTING
Note
Reference Item
11. PROGRAM COMMAND B–61393E–2/02
584
Although subprograms are useful for repeating the same operation, the custom macro function also allows use of variables, arithmetic and logic operations, and conditional branches for easy development of general programs such as pocketing and user–defined canned cycles. A machining program can call a custom macro with a simple command, just like a subprogram.
O0001 ;
:
:
:
G65 P9010 R50.0 L2 ;
:
:
M30 ;
Machining program Custom macro
O9010 ;
#1=#18/2 ;
G01 G42 X#1 Y#1 F300 ;
G02 X#1 Y–#1 R#1 ;
:
:
:
M99 ;
This means that a function of general use can be formed when programming a certain function as a custom macro. That is, programs can be written using variables for data that might change or be unknown. This can be further applied to group technology. Similar workpieces can be collected as a group and a universal custom macro body can be programmed using variables applicable to each group. In this way, programming is not required for the workpieces in the group. The programmer only need to assign actual values to the variables.
r β
α
Bolt hole circles as shown in the above figure can be made easily. Once a custom macro body for the bolt hole circle is programmed and registered, the CNC can operate as if it has the bolt hole circle cutting function.
11.6 CUSTOM MACRO
11.6.1 Custom Macro
General
B–61393E–2/02 11. PROGRAM COMMAND
585
Programmers can use the bolt hole circle function by using the following command only: (Example of calling bolt hole circle) G65 Pp Rr A α Bβ Kk ; P :Macro number of bolt hole circle r : Radius α : Start angle β : Angle between circles k � Number of circles
(Specification Custom Macro B)
[Classification] Input signal
[Function] No function is provided for the control unit. These signals can be read by a custom macro as a type of system variable, and are used for interface signals between custom macros and the PMC. These signals correspond to system variables as indicated below.
Signals Q’ty Variables Correspondenceof values
UI000 UI001 UI002 UI003
: UI014 UI015
1 1 1 1 : 1 1
#1000 #1001 #1002 #1003
: #1014 #1015
“0” at “0” and “1” at “1”
UI000 to UI015 16 #1032 16–bit binary code *1
*1 Variable value #1032 �� 15
i�0
{#[1000 � i] � 2i}
Signal
Custom Macro Input Signal UI000 to UI015 <G130, G131>
11. PROGRAM COMMAND B–61393E–2/02
586
[Classification] Output signal
[Function] No function is provided for the control unit. These signals can be read or written by a custom macro as a type of system variable, and are used for interface signals between custom macros and the PMC.
These signals correspond to system variables as indicated below.
Signals Q’ty Variables Correspondence ofvalues
UO000 UO001 UO002 UO003
: UO014 UO015
1 1 1 1 : 1 1
#1100 #1101 #1102 #1103
: #1114 #1115
“0” at “0” and “1” at “1”
UO000 to UO015 UO100 to UO115
16 32
#1132 #1133
16–bit binary code *1 32–bit binary code *2
*2 Variable value #1133 ��{ 30
i�0
2i � Vi}–2 31 � V31
Where Vi=0 when UO1i is 0 and Vi=1 when UO1i is 1
*1 Variable value #1132 �� 15
i�0
{#[1100 � i] � 2i}
These system variables can be used on the left side of an assignment statement as well as on the right side. The value assigned to the system variable used on the left side last is used for the value of the system variable to be assigned on the right side.
#7 UI007G130
#6 UI006
#5 UI005
#4 UI004
#3 UI003
#2 UI002
#1 UI001
#0 UI000
UI015G131 UI014 UI013 UI012 UI011 UI010 UI009 UI008
#7 UO007F162
#6 UO006
#5 UO005
#4 UO004
#3 UO003
#2 UO002
#1 UO001
#0 UO000
UO015F163 UO014 UO013 UO012 UO011 UO010 UO009 UO008
UO107F196 UO106 UO105 UO104 UO103 UO102 UO101 UO100
UO115F197 UO114 UO113 UO112 UO111 UO110 UO109 UO108
UO123F198 UO122 UO121 UO120 UO119 UO118 UO117 UO116
UO131F199 UO130 UO129 UO128 UO127 UO126 UO125 UO124
Custom Macro Output Signal UO000 to UO015 <F162, F163> UO100 to UO131 <F196 to F199>
Signal address
B–61393E–2/02 11. PROGRAM COMMAND
587
#7 0011
#6 #5 SBKM
#4 #3 #2 #1 #0
[Data type] Bit
SBKM Custom macro statement 0 : Not stop the single block 1 : Stops the single block
#7 LOCC0040
#6 COMC
#5 TMCR
#4 #3 #2 #1 DPOSUP
#0
[Data type] Bit
DPOSUP Reading zero when data is output using a DPRNT command 0 : Outputs a space 1 : Outputs no data
TMCR Custom macro (subprogram) 0 : Not called using a T code 1 : Called using a T code
COMC Custom macro B’s common variables Nos. 100 through 149 0 : Cleared to “vacant” by reset 1 : Not cleared by reset
LOCC Custom macro B’s local variables #1 through #33 0 : Cleared to “vacant” by reset 1 : Not cleared by reset
#7 0057
#6 #5 #4 CROUT
#3 #2 #1 #0
[Data type] Bit
CROUT In BPRNT or DPRNT, after the data is outputted in ISO code: 0 : Only the “LF” is outputted. 1 : “LF” and “CR” are outputted.
Parameter
� Setting for single block stop
� Other settings
11. PROGRAM COMMAND B–61393E–2/02
588
#7 *70042
#6 *6
#5 *5
#4 *4
#3 *3
#2 *2
#1 *1
#0 *0
=70043 =6 =5 =4 =3 =2 =1 =0
#70044 #6 #5 #4 #3 #2 #1 #0
[70053 [6 [5 [4 [3 [2 [1 [0
]70054 ]6 ]5 ]4 ]3 ]2 ]1 ]0
[Data type] Bit These parameters are used to input/output macro statements.
The numeral of a suffix indicates the bit position in a code.
*0 to *7 Set the hole pattern of an EIA code indicating *. =0 to =7 Set the hole pattern of an EIA code indicating =. #0 to#7 Set the hole pattern of an EIA code indicating #. [0 to [7 Set the hole pattern of an EIA code indicating [. ]0 to ]7 Set the hole pattern of an EIA code indicating ].
0 : Corresponding bit is 0 1 : Corresponding bit is 1.
0248 M code that calls the program entered in file
[Data type] Byte
[Valid data range] 0, and 1 to 255 When the subprogram call function is used, this parameter sets the M code for calling a program in a file stored on the external input/output device.
NOTE The M code is judged to be M198 when zero is specified as the setting value.
� Setting when macro statement is input/output with EIA code
� Setting an M code that calls a program entered in a file
B–61393E–2/02 11. PROGRAM COMMAND
589
0220 G code that calls the custom macro of program number 9010
0221 G code that calls the custom macro of program number 9011
0222 G code that calls the custom macro of program number 9012
0223 G code that calls the custom macro of program number 9013
0224 G code that calls the custom macro of program number 9014
0225 G code that calls the custom macro of program number 9015
0226 G code that calls the custom macro of program number 9016
0227 G code that calls the custom macro of program number 9017
0228 G code that calls the custom macro of program number 9018
0229 G code that calls the custom macro of program number 9019
[Data type] Word
[Valid data range] 1 to 9999 These parameters set the G codes that call the custom macros of program numbers 9010 through 9019.
NOTE Setting value 0 is invalid. No custom macro can be called by G00.
0240 M code that calls the subprogram of program number 9001
0241 M code that calls the subprogram of program number 9002
0242 M code that calls the subprogram of program number 9003
[Data type] Two–word
[Valid data range] 1 to 99999999 These parameters set the M codes that call the subprograms of program numbers 9001 through 9003.
NOTE Setting value 0 is invalid. No custom macro can be called by M00.
� Setting G codes that call custom macros of program Nos.9010 to 9019
� Setting M codes that call subprograms of program Nos.9001 to 9009
11. PROGRAM COMMAND B–61393E–2/02
590
0230 M code that calls the sub program of program number 9020
0231 M code that calls the sub program of program number 9021
0232 M code that calls the sub program of program number 9022
0233 M code that calls the sub program of program number 9023
0234 M code that calls the sub program of program number 9024
0235 M code that calls the sub program of program number 9025
0236 M code that calls the sub program of program number 9026
0237 M code that calls the sub program of program number 9027
0238 M code that calls the sub program of program number 9028
0239 M code that calls the sub program of program number 9029
[Data type] Two–word
[Valid data range] 1 to 99999999 These parameters set the M codes that call the sub programs of program numbers 9020 through 9029.
NOTE Setting value 0 is invalid. No custom macro can be called by M00.
� Setting M codes that call custom macros of no.9020 to 9029
B–61393E–2/02 11. PROGRAM COMMAND
591
������ Message Description
076 ADDRESS P NOT DEFINED
Address P (program number) was not commanded in the block which in- cludes an M98, G65, or G66 com- mand. Modify the program.
077 SUB PROGRAM NESTING ERROR
The subprogram was called in five folds. Modify the program.
078 NUMBER NOT FOUND A program number or a sequence number which was specified by ad- dress P in the block which includes an M98, M99, M65 or G66 was not found. The sequence number specified by a GOTO statement was not found. Otherwise, a called program is being edited in background processing. Cor- rect the program, or discontinue the background editing.
110 DATA OVERFLOW The absolute value of fixed decimal point display data exceeds the allow- able range. Modify the program.
111 CALCULATED DATA OVERFLOW
The result of calculation is out of the allowable range (–1047 to –10–29, 0, and 10–29 to 1047).
112 DIVIDED BY ZERO Division by zero was specified. (in- cluding tan 90�)
113 IMPROPER COMMAND A function which cannot be used in custom macro is commanded. Modify the program.
114 FORMAT ERROR IN MACRO
There is an error in other formats than <Formula>. Modify the program.
115 ILLEGAL VARIABLE NUMBER
A value not defined as a variable number is designated in the custom macro, or the header contents are im- proper in a high–speed cycle cutting. This alarm is given in the following cases: High speed cycle machining 1. The header corresponding to the speci-
fied machining cycle number called is not found.
2. The cycle connection data value is out of the allowable range (0 to 999).
3. The number of data in the header is out of the allowable range (0 to 32767).
4. The storing start data variable number of executable format data is out of the allowable range (#20000 to #85535).
5. The storing data variable number of executable format data is out of the al- lowable range (#85535).
6. The storing start data variable number of executable format data is overlapped with the variable number used in the header.
Modify the program.
116 WRITE PROTECTED VARIABLE
The left side of substitution statement is a variable whose substitution is in- hibited. Modify the program.
Alarm and message
11. PROGRAM COMMAND B–61393E–2/02
592
������ DescriptionMessage
118 PARENTHESIS NESTING ERROR
The nesting of bracket exceeds the upper limit (quintuple). Modify the program.
119 ILLEGAL ARGUMENT The SQRT argument is negative, BCD argument is negative, or other values than 0 to 9 are present on each line of BIN argument. Modify the program.
122 DUPLICATE MACRO MODAL–CALL
The macro modal call is specified in double. Modify the program.
123 CAN NOT USE MACRO COMMAND IN DNC
Macro control command is used dur- ing DNC operation. Modify the program.
124 MISSING END STATEMENT
DO – END does not correspond to 1 : 1. Modify the program.
125 FORMAT ERROR IN MACRO
<Formula> format is erroneous. Modify the program.
126 ILLEGAL LOOP NUMBER In DOn, 1� n � 3 is not estab- lished. Modify the program.
127 NC, MACRO STATEMENT IN SAME BLOCK
NC and custom macro commands coexist. Modify the program.
128 ILLEGAL MACRO SEQUENCE NUMBER
The sequence number specified in the branch command was not 0 to 9999. Or, it cannot be searched. Modify the program.
129 ILLEGAL ARGUMENT ADDRESS
An address which is not allowed in <Argument Designation > is used. Modify the program.
199 MACRO WORD UNDEFINED
Undefined macro word was used. Modify the custom macro.
CAUTION Machine tool builders: You are requested to attach your custom macro program tape or program list to the CNC unit without fail. If it is necessary to replace part program storage memory due to a failure, FANUC servicemen or end user in charge of maintenance should know the contents of your custom macro for the purpose of repairing the trouble immediately.
OPERATOR’S MANUAL (For Machining Center) (B–61404E)
II.15 and 16 CUSTOM MACRO A/B
OPERATOR’S MANUAL (For Lathe) (B–61394E)
II.15 and 16 CUSTOM MACRO A/B
Caution
Reference item
B–61393E–2/02 11. PROGRAM COMMAND
593
When a program is being executed, another program can be called by inputting an interrupt signal (UINT) from the machine. This function is referred to as an interruption type custom macro function. Program an interrupt command in the following format:
M96 P���� ;
M97 ;
Enables custom macro interrupt
Disables custom macro interrupt
Use of the interruption type custom macro function allows the user to call a program during execution of an arbitrary block of another program. This allows programs to be operated to match situations which vary from time to time.
(1) When a tool abnormality is detected, processing to handle the abnormality is started by an external signal.
(2) A sequence of machining operations is interrupted by another ma- chining operation without the cancellation of the current operation.
(3) At regular intervals, information on current machining is read.
Listed above are examples like adaptive control applications of the interruption type custom macro function.
Interrupt signal (UINT)*
Interrupt signal (UINT)*
Interrupt signal (UINT)*
M96 Pxxxx;
N����;
M97 ;
M99 (P����);
O xxxx;
Fig 11.6.2 Interruption type custom macro function
When M96Pxxxx is specified in a program, subsequent program operation can be interrupted by an interrupt signal (UINT) input to execute the program specified by Pxxxx. When the interrupt signal (UINT, marked by * in Fig. 11.6.2) is input during execution of the interrupt program or after M97 is specified, it is ignored.
11.6.2 Interruption Type Custom Macro
General
11. PROGRAM COMMAND B–61393E–2/02
594
[Classification] Input signal
[Function] This signal calls and executes a program in memory. During execution, a program in automatic operation is suspended. To enable this signal to be accepted, a particular miscellaneous function must be specified in a command program for automatic operation. In addition, automatic operation must already be started to accept this signal. The particular miscellaneous function code is set by parameter 0056, 0246 and 0247.
#7 G140
#6 #5 #4 #3 UINT
#2 #1 #0
#7 MUSR0056
#6 MCYL
#5 MSUB
#4 MPRM
#3 MTSE
#2 MBLK
#1 MSKT
#0
[Data type] Bit
MSKT Absolute coordinates at that time during custom macro interrupt 0 : Not set to the skip coordinates (system variables #5061 and later) 1 : Set to the skip coordinates (system variables #5061 and later)
MBLK Custom macro interrupt 0 : Performed by interrupting an in–execution block (Custom macro
interrupt type I) 1 : Performed after an in–execution block is completed (Custom macro
interrupt type II)
MTSE Custom macro interrupt signal UINT 0 : Edge trigger method (Rising edge) 1 : Status trigger method
MPRM Custom macro interrupt valid/invalid M code 0 : M96/M97 1 : M code set using parameters (Nos. 0246 and 0247)
MSUB Interrupt program 0 : Uses a dedicated local variable (Macro–type interrupt) 1 : Uses the same local variable as in the main program (Subprogram–
type interrupt)
Signal
Interrupt Signal for Custom Macro UINT<G140#3>
Signal address
Parameter
� Various Setting for Custom Macro
B–61393E–2/02 11. PROGRAM COMMAND
595
MCYL Custom macro interrupt 0 : Not performed during cycle operation 1 : Performed during cycle operation
MUSR Interrupt–type custom macro 0 : Not used 1 : Used
0246 M code that validates a custom macro interrupt
0247 M code that invalidates a custom macro interrupt
[Data type] Byte type
[Valid data range] 0 to 255
These parameters set the custom macro interrupt valid/invalid M codes.
NOTE These parameters can be used when MPR, #4 of parameter No. 0056, is 1. M96 is used as a valid M code and M97 is used as an invalid M code when MPRM is 0, irrespective of the state of this parameter.
OPERATOR’S MANUAL (For Machining Center) (B–61404E)
II.16.11 INTERRUPTION TYPE CUSTOM MACRO
OPERATOR’S MANUAL (For Lathe) (B–61394E)
II.16.11 INTERRUPTION TYPE CUSTOM MACRO
� Setting M code that makes interruption effective and ineffective
Reference item
11. PROGRAM COMMAND B–61393E–2/02
596
In 0–TTC, common variables are provided separately for each tool post; variable #n used with a tool post 1 is different from variable #n used with tool post 2. By parameter setting (No. 0047#5(VR1), #6(VR5) and No. 0218), however, some or all of common variables #100 to # 149 and #500 to #531 can be made usable commonly by tool post 1 and tool post 2 so that such variables can be written or read for either tool post. Such variables are referred to as custom macro variables common between tool posts.
#7 0047
#6 VR5
#5 VR1
#4 #3 #2 #1 #0
[Data type] Bit
VR1, VR5 Specify the first number for custom macro variables common to both tool posts in the 0–TTC.
VR5 VR1 First number for custom macro variables com- mon to both tool posts
0 0 None (no common custom macro variable is used.)
0 1 No. 100
1 0 No. 500
1 1 Nos. 100 and 500
0218 Number of custom macro variables common between tool posts
[Data type] Byte
[Unit of data] Number of custom macro variables
[Valid data range] 0 to 50
This parameter specifies the number of variables commonly used for both tool posts 1 and 2 (custom macro variables common between tool posts) that are part of custom macro variables 100 to 149 and 500 to 532. The custom macro variables common to tool posts can be written or read for either of the tool posts.
OPERATOR’S MANUAL (For Lathe) (B–61394E)
II.24.5 CUSTOM MACRO VARI- ABLES COMMON TO TOOL POSTS
11.6.3 Custom Macro Variables Common between Tool Posts (0–TTC)
General
Parameter
� Setting the no. of custom macro variables common between tool posts
Reference item
B–61393E–2/02 11. PROGRAM COMMAND
597
Canned cycles make it easier for the programmer to create programs. With a canned cycle, a frequently–used machining operation can be specified in a single block with a G function; without canned cycles, normally more than one block is required. In addition, the use of canned cycles can shorten the program to save memory.
A canned cycle consists of a sequence of six operations.
Operation 1 Positioning a hole position Operation 2 Rapid traverse up to point R level Operation 3 Hole machining Operation 4 Operation at the bottom of a hole Operation 5 Retraction to point R level Operation 6 Rapid traverse up to the initial point
Operation 1
Operation 2
Operation 3
Operation 4
Operation 5
Operation 6
Rapid traverse Feed
Initial level
Point R level
Fig. 11.7 (a) Canned cycle operation sequence
11.7 CANNED CYCLE (M SERIES)/CANNED CYCLE FOR HOLE MACHINING (T SERIES)
General
11. PROGRAM COMMAND B–61393E–2/02
598
In some canned cycles, a spindle command to rotate the spindle in reverse direction may be output.
The following canned cycles require spindle control:
M series T series
Reverse tapping cycle G74 Face tapping cycle (G84)
Fine boring cycle G76 Side tapping cycle (G88)
Tapping cycle G84
Boring cycle G86
Back boring cycle G87
Boring cycle G88
For spindle control, the following normal miscellaneous functions are
used:
See the description of the miscellaneous functions.
M03: CW spindle rotation
M04: CCW spindle rotation
M05: Spindle stop
M19: Spindle orientation (M series)
When the rotation direction of the spindle is to be switched from one
direction to the other (for example, when M04 is output during M03
operation), a parameter can specify whether to send M05 at the time
switching.
Timing charts are described in the following page:
SPINDLE CONTROL
B–61393E–2/02 11. PROGRAM COMMAND
599
Note) It is possible to not output M05 code by using parame- ter FXCS (No.0012#4).
Next block (G99 mode)
FIN FIN
MF MF
M03M05
FIN FIN
MF MF
M05 M04
Z
X, Y
Z
Z
� G74 (Counter tapping cycle)
FIN FIN
MF MF
M19M05
FIN FIN
MF MF
M03 M03
Z
Z
Z
Return to ini- tial level in G98 mode
X, Y
X, Y
Z Z
FIN FIN
MF MF
M04M05
FIN FIN
MF MF
M05 M03
Z
Dwell Dwell
(Note) (Note)
Next block (G98 mode)
� G76 (Fine boring cycle)
� G84 (tapping cycle)
X or Y
X or Y
Next block (G98 mode)
Next block (G99 mode)
Note) It is possible to not output M05 code by using parame- ter FXCO (No.0012#5).
Note) It is possible to not output M05 code by using parame- ter FXCS (No.0012#4).
Dwell
(Note)
(Note) (Note)
Dwell Dwell
Next block (G99 mode)
Next block (G98 mode)
Fig.11.7 (b) Canned cycle for M series (1/2)
11. PROGRAM COMMAND B–61393E–2/02
600
FIN FIN FIN
MF MF
M03M03M05
MF
Next block (G98 mode)
Return to initial level in G98 mode
X, Y
Z Z
FINFIN
MF MFMFMFMF
M05 M1 9 M03 M05 M19
MF
M03
FINFINFIN FIN
Z Z
Z
X, Y
(Note) It is possible to not output M05 code using pa- rameter FXCO (No.0012#5). Back boring cycle is not used in G99 mode but in G98 mode.
FIN
M03
MF
Z
FIN
M05
MF
Z Z
Return to initial level in G98 mode or R point level in G99 mode.
Z
X, Y
� G86 (Boring cycle)
Dwell
(Note)
Next block (G99 mode)
X or Y
X or Y
X or Y
(Note)
Dwell
Manual feed Cycle start
� G88 (Boring cycle)
� G87 (Back boring cycle)
Fig.11.7 (b) Canned cycle for M series (2/2)
B–61393E–2/02 11. PROGRAM COMMAND
601
X, C (Z, C)
Z
(X)
Z (X)
FIN FIN
MF MF
M04M05
FIN FIN
MF MF
M05 M03
ZZ
(X) Dwell
(Note 1)
� G84 (Face tapping cycle) G88 (Side tapping cycle)
Next block (G98 mode)
Next block (G99 mode)
(Note 2)
Dwell
(Note 1) (Note 2)
(Note 1) When parameter TAPM (No. 0031#2)=0, M05 is not output.
(Note 2) Another M code may be used by parameter No. 0212 and 0213.
Fig 11.7 (c) Canned cycle for T series
When an M code specified in parameter No.0204 for C–axis clamp/unclamp is coded in a program, the CNC issues the M code for C–axis clamp after the tool is positioned and before the tool is fed in rapid traverse to the point–R level. The CNC also issues the M code (M code C–axis clamp +1) for C–axis unclamp after the tool retracts to the point–R level. The tool dwells for the time specified in parameter No. 0591.
During a tapping cycle, the tapping signal is output. The tapping signal is also output while the G code of the tapping cycle is valid.
During tapping, cutting feedrate override is always set to 100%.
When the feed hold key is pressed during tapping, the movement is not stopped immediately but the movement is stopped when the tool is returned to level R.
In M series, the TAPDRN (bit 5 of parameter No.0065) specifies whether dry run is valid during tapping.
� M code used for C–axis clamp/unclamp (T series)
Tapping signal
Override
Feed hold
Dry run
11. PROGRAM COMMAND B–61393E–2/02
602
[Classification] Output signal
[Function] Reports that the system is in tapping mode.
[Output condition] The signal is set to 1 when: – The system is in tapping cycle mode.
G74, G84: M series G84, G88: T series
– The system is in tapping mode. G63: M series
The signal is set to 0 when: – The system is in neither tapping cycle mode nor tapping mode. – A reset or emergency stop is specified.
#7 F149
#6 #5 TAP
#4 #3 #2 #1 #0
#7 0002
#6 #5 PMXY2
#4 PMXY1
#3 #2 #1 #0 (M series)
[Data type] Bit
PMXY2, PMXY1 Set the axis and direction in which the tool in drilling canned cycle G76 or G87 is got free. RD2 and RD1 are set as shown below by plane selection.
PMXY2 PMXY1 G17 G18 G19
0 0 +X +Z +Y
0 1 –X –Z –Y
1 0 +Y +X +Z
1 1 –Y –X –Z
#7 0011
#6 #5 #4 MCF
#3 #2 #1 #0 (M series)
[Data type] Bit
MCF G81 0 : Specifies a drilling canned cycle 1 : Specifies an external operation command
Signal
Tapping signal TAP<F149#5>
Signal address
Parameter
B–61393E–2/02 11. PROGRAM COMMAND
603
#7 0012
#6 #5 FXCO
#4 FXCS
#3 #2 #1 #0 (M series)
[Data type] Bit
FXCS When a spindle rotates from the forward to the reverse direction and vice versa in tapping cycles G84 and G74 for M series (G84 and G88 for t series), befor M04 or M03 is output: 0 : Outputs M05 1 : Not output M05
FXCO In drilling canned cycles G76 and G87: 0 : Outputs M05 before an oriented spindle stops 1 : Not output M05 before an oriented spindle stops
#7 0031
#6 #5 #4 RTCT
#3 ILVL
#2 TAPM
#1 #0
[Data type] Bit
TAPM When a spindle rotates from the forward to the reverse direction and vice versa in tapping cycles G84 and G74 for M series (G84 and G88 for T series), befor M04 or M03 is output: 0 : Not output M05 1 : Outputs M05
ILVL Initial point position in drilling canned cycle 0 : Not updated by reset 1 : Updated by reset
RTCT For drilling, G83 and G87 0 : Make a return by a specified escape amount. 1 : Make a return to the R point level.
#7 0057
#6 FXY
#5 #4 #3 #2 #1 #0 (M series)
[Data type] Bit
FXY The drilling axis in the drilling canned cycle is: 0 : Always the Z–axis 1 : The axis selected by the program
0204 C–axis clamp M code in drilling canned cycle (T series)
[Data type] Byte
[Valid data range] 0 to 99
This parameter sets the C–axis clamp M code in a drilling canned cycle.
11. PROGRAM COMMAND B–61393E–2/02
604
0212 Spindle forward–rotation M code in drilling canned cycle (T series)
[Data type] Byte
[Valid data range] 0 to 255
This parameter sets the spindle forward–rotation M code in a drilling canned cycle.
NOTE M03 is output when “0” is set.
0213 Spindle reverse–rotation M code in drilling canned cycle (T series)
[Data type] Byte
[Valid data range] 0 to 255
This parameter sets the spindle reverse–rotation M code in a drilling canned cycle.
NOTE M04 is output when “0” is set.
0591 Dwell time when C–axis unclamping is specified in drilling canned cycle (T series)
[Data type] Word
[Unit of data] ms
[Valid data range] 0 to 32767
This parameter sets the dwell time when C–axis unclamping is specified in a drilling canned cycle.
0592 Return value of canned cycle G83 for drilling (T series)
0531 Return value of high–speed peck drilling cycle G73 (M series)
[Data type] Word
Increment system ���� ���� ���� Unit
Metric input 0.01 0.001 0.0001 mm
Inch input 0.001 0.0001 0.00001 inch
[Valid data range] 0 to 32767
For M series, this parameter sets the return value in high–speed peck drilling cycle G73 (G83 for T series).
[Unit of data]
B–61393E–2/02 11. PROGRAM COMMAND
605
q : Depth of cut
d : Return value
Z point
G73 for M series
R point
q
d
d q
q
Fig. 11.7 (d) High–speed peck drilling cycle (G73) for M series
For T series, this parameter sets the return or clearance value in drilling canned cycle G83.
q : Depth of cut
d : Clearance value
q : Depth of cut
d : Return value
Parameter No. 0031#4 RTCT=0
(High speed peck drilling cycle) Parameter No. 0031#4 RTCT=1
(Peck drilling cycle)
G83 for T series
R point
Z point
q
q
q
d
d
R point
Z point
q
q
q
d
d
Fig. 11.7 (e) Drilling canned cycle (G83) for T series
11. PROGRAM COMMAND B–61393E–2/02
606
0532 Clearance canned cycle G83 (M series)
[Data type] Word
Increment system ���� ���� ���� Unit
Metric input 0.01 0.001 0.0001 mm
Inch input 0.001 0.0001 0.00001 inch
[Valid data range] 0 to 32767 This parameter sets the clearance value in peck drilling cycle G83.
G83 (M series)
q : Depth of cut
d : Clearance value
R point
Z point
q
q
q
d
d
Fig. 11.7 (f) Peck drilling cycle (G83)
�� � � Message Description
044 G27–G30 NOT AL- LOWED IN FIXED CYCLE (M series)
One of G27 to G30 is commanded in a canned cycle mode. Modify the program.
NOTE A parameter FXY (No.0057#6) can be set to the Z axis always used as the drilling axis. When FXY=0, the Z axis is always the drilling axis. (M series)
OPERATOR’S MANUAL (For Machining Center) (B–61404E)
II.13.1 CANNED CYCLE
OPERATOR’S MANUAL (For Lathe) (B–61394E)
II.13.3 CANNED CYCLE FOR DRILLING
[Unit of data]
Alarm and message
Note
Reference item
B–61393E–2/02 11. PROGRAM COMMAND
607
A tool with an overload torque detection function can change the spindle speed and cutting feedrate during peck drilling, using an overload torque detection signal received from the tool as a skip signal. Such peck drilling enables small–diameter peck drilling. The sequence chart of a small–diameter peck drilling cycle is shown below.
Tool (1)
(2)
(3)
(6)
(5)
Q
�
Overload torque Overload
torque Dwell
R point
Z point
� : The first minute escape amount used in moving back to the R point, and an amount of clearance at the start point (end point of the previous cycle) of the second and subse- quent cycles
Q : Cutting depth per cycle
: Movement at a rapid traverse rate
: Movement at a parameter– or program–specified rate
: Movement at a program–specified cutting feedrate
The steps of the small–diameter peck drilling cycle are as follows:
(1)Position along the X– and Y–axes.
(2)Position to the R point along the Z–axis.
(3)Cut along the Z–axis (maximum cutting depth Q).
(4)Repeat the following steps until the hole bottom along the Z–axis is reached.
� Reverse (→ minute escape amount ∆). � Reverse (→ R point). � Advance (R point → start point + clearance ∆). � Cut (cutting depth Q + ∆).
(5)Dwell at the hole bottom.
(6)Return to the R point (or initial point) along the Z–axis.
11.8 SMALL–DIAMETER PECK DRILLING CYCLE (M SERIES)
General
11. PROGRAM COMMAND B–61393E–2/02
608
(1)A small–diameter peck drilling cycle is executed by issuing a G83 after a small–diameter peck drilling cycle M code. The small–diameter peck drilling cycle in progress signal is output when R point positioning along the drill axis begins, and kept output until a return to the R point/initial level is completed.
(2)A skip signal (X008#7) is used as the overload torque detection signal. The skip signal is valid only when the drill is moving forward or cutting between the R and Z points. If the skip signal is input when the drill is moving forward or cutting, the drill starts to move backward immediately.
(3)Cutting conditions are changed for each pecking cycle (advance → cut → reverse) during one G83 cycle.
� Changing the cutting feedrate
A cutting feedrate specified in a program using an F code is changed for each of the second and subsequent cutting cycles. Parameter No. 307 specifies the ratio of a change to be used when a skip signal has been received during the previous cutting cycle. Parameter No. 308 specifies that to be used when a skip signal has not been received during the previous cutting cycle.
Cutting feedrate�F�α
(First cutting cycle) α = 1.0 (Second and subsequent cutting cycles)α = α � β ÷100
where β is a change ratio for one cutting cycle If a skip signal is input during the previous cutting cycle:
β = parameter No. 307 If a skip signal is not input during the previous cutting cycle:
β = parameter No. 308 If the cutting feedrate change ratio (α) becomes less than a value specified in parameter No. 309, no further change will be made to the cutting feedrate.
� Changing the spindle speed
A spindle speed specified in a program using an S code is changed for each of the second and subsequent cutting cycles. Parameter No. 305 specifies the ratio of a change to be used when a skip signal has been received during the previous cutting cycle. Parameter No. 306 specifies that to be used when a skip signal has not been received during the previous cutting cycle.
Spindle speed �S�γ
(First cutting cycle) γ = 1.0 (Second and subsequent cutting cycles)γ = γ � δ ÷100
where δ is a change ratio for one cutting cycle If a skip signal is input during the previous cutting cycle:
δ= parameter No. 305 If a skip signal is not input during the previous cutting cycle:
δ= parameter No. 306 If the cutting feedrate is clamped at the lowest limit, no change will be made to the spindle speed.
Specification
B–61393E–2/02 11. PROGRAM COMMAND
609
(4)During pecking, advance and reverse movements are performed as cutting feed rather than rapid positioning.
(5) If pecking advance and reverse feedrates are specified using an I code, the same format as for F codes is used. An I code specified using a G83 remains valid until a G80 is issued or a reset occurs.
[Classification] Input signal
[Function] Used as a spindle overload torque detection signal during the execution of a small–diameter peck drilling cycle.
[Operation] If the drill is moving forward or cutting between the R and Z points during the execution of a small–diameter peck drilling cycle, setting the skip signal to 1 causes the drill to move backward.
[Classification] Output signal
[Function] Indicates the operating status of a small–diameter peck drilling cycle.
[Operation] The signal is 1 during the execution of a small–diameter peck drilling cycle. It is 0 when a small–diameter peck drilling cycle is not being executed.
#7 SKIPX008
#6 #5 #4 #3 #2 #1 #0 (M series)
PECK2F180 (M series)
Signal
Skip signal SKIP <X008#7>
Small–diameter peck drilling cycle execution in progress signal PECK2 <F180#7>
Signal address
11. PROGRAM COMMAND B–61393E–2/02
610
#7 CHGNRM0398
#6 CHGSKP
#5 #4 #3 #2 #1 #0
CHGSKP If an overload torque signal is received: 1 : The feedrate and spindle speed will be changed.
0 : Neither the feedrate nor spindle speed will be changed.
CHGNRM If a cutting depth per cycle is completed before an overload torque signal is received: 1 : The feedrate and spindle speed will be changed.
0 : Neither the feedrate nor spindle speed will be changed.
0304 PECK_M
Specify a small–diameter peck drilling cycle M code.
[Valid data range] 3 to 999
0305 SSOPR1
Specify a percentage at which the spindle speed is to be changed when the drill is caused to move back as directed by an overload torque signal.
[Valid data range] 0 to 255%
0306 SSOPR2
Specify a percentage at which the spindle speed is to be changed when the drill is caused to move back without receiving an overload torque signal.
[Valid data range] 0 to 255%
0307 FROPR1
Specify a percentage at which the cutting feedrate is to be changed when the drill is caused to move back as directed by an overload torque signal.
[Valid data range] 0 to 255%
0308 FROPR2
Specify a percentage at which the cutting feedrate is to be changed when the drill is caused to move back without receiving an overload torque signal.
[Valid data range] 0 to 255%
Parameter
B–61393E–2/02 11. PROGRAM COMMAND
611
0309 FROLMT
Specify a lower limit to the percentage of the after–change cutting feedrate to the specified cutting feedrate.
[Valid data range] 0 to 255%
0327 PEKMCV
Specify a custom macro common variable number used to output the total number of times that the drill reverses during cutting. If 0 is specified, no output is made.
[Valid data range] 100 to 149
0328 SKPMCV
Specify a custom macro common variable number used to output the total number of times that the drill reverses during cutting as directed by an overload signal. If 0 is specified, no output is made.
[Valid data range] 100 to 149
0492 PEKFD1
Specify the speed at which the drill moves back to the R point if I is omitted.
[Valid data range] 1mm/min (mm input) 0.01inch/min (inch input)
0493 PEKFD2
Specify the speed at which the drill moves to the previous machined point if I is omitted.
[Valid data range] 1mm/min (mm input) 0.01inch.min (inch input)
0941 DLTPRM
Specify the first minute escape amount to be used in moving back to the R point during a cycle, and a clearance amount at the start point of the second and subsequent cutting cycles.
[Valid data range] Least input increment
11. PROGRAM COMMAND B–61393E–2/02
612
The following self–diagnosis information is displayed on the diagnosis screen. Parameter Nos. 520 and 521 are reset using a G83 command.
No. 520 : Total number of times the drill reverses during cutting after a G83 is issued.
No. 521 : Total number of times the drill reverses as directed by an overload signal during cutting after a G83 is issued.
No. 522 : Coordinate from which the drill began to reverse (in least input increments).
No. 523 : Difference between the previous coordinate from which the drill began to reverse and the current coordinate from which the drill began to reverse (in least input increments).
NOTE 1 A small–diameter peck drilling cycle M code is issued in an
M code–only block before a G83 is issued. The M code is processed internally; it will not be output.
2 The advance and reverse movements are accelerated/decelerated according to the cutting feedrate acceleration/deceleration time constant. For the reverse movement, a position check is performed at the R point.
3 When the drill is moving forward, if a skip signal is received, the drill is caused to move backward.
4 During a small–diameter peck drilling cycle, changing the spindle speed during pecking requires a 4– or 5–digit S command.
5 The R point must be separated by a specified clearance amount (∆) from the workpiece plane.
Self–diagnosis
Note
B–61393E–2/02 11. PROGRAM COMMAND
613
Upon completion of positioning in each block in the program, an external operation function signal can be output to allow the machine to perform specific operation.
G81 IP_ ; (The IP_ is axis move command )
Every time positioning for the IP_ move command is completed, the CNC sends an external operation signal to the machine. An external operation signal is output for each positioning operation until canceled by G80 or a group 01 G code.
No external operation signals are output during execution of a block that contains neither X nor Y.
1 Once positioning for a move command has been completed, the CNC sets the external operation signal EF to 1.
2 When the EF signal is set to 1, the PMC executes drilling or another operation. Once the operation has been completed, the PMC sets completion signal FIN to 1.
3 The CNC resets the EF signal to 0 upon the elapse of the time (TFIN) specified in parameter No.0009 after the FIN signal is set to 1.
4 When the EF signal is set to 0, the PMC resets the FIN signal to 0.
5 The CNC starts executing the next block.
The timing diagram is shown below:
EF
G81 command
Positioning
Machine operation
FIN
Next block
TFIN
Fig. 11.9 Timing diagram of basic procedure
11.9 EXTERNAL MOTION FUNCTION (M SERIES)
General
Basic procedure
11. PROGRAM COMMAND B–61393E–2/02
614
[Classification] Output signal
[Function] Reports that the positioning of G81 has been completed in the external motion function, and that a special external operation is required.
[Output condition] For details of the output condition and procedure, see the “basic procedure”, described previously. For details of completion signal FIN, see section 8.1.
#7 F150
#6 #5 #4 #3 #2 #1 EF
#0
#7 0011
#6 #5 #4 MCF
#3 #2 #1 #0
[Data type] Bit
MCF G81: 0 : Specifies a drilling canned cycle 1 : Specifies an external operation command
CAUTION 1 When this function is used, canned cycles (G73, G74, G76,
and G82 to G89) cannot be used. 2 When the high–speed M, S, T, or B interface is used, the
signals used by this function are transferred in high–speed mode. See Section 8.4.
OPERATOR’S MANUAL (For Machining Center) (B–61404E)
II.13.8 EXTERNAL MOTION FUNCTION
Signal
External Operation Signal EF<F150#1> (M series)
Signal address
Parameter
Caution
Reference item
B–61393E–2/02 11. PROGRAM COMMAND
615
This option canned cycles to make CNC programming easy. For instance, the data of the finish work shape describes the tool path for rough machining. And also, a canned cycles for the thread cutting is available. The following example shows stock removals in turning type I. If a finished shape of A to A’ to B is given by a program as in the figure below, the specified area is removed by ∆d (depth of cut), with finishing allowance ∆u/2 and ∆w left.
B
(F) (R)
e
A
C
∆d
A’
45,
(R)
(F)
∆u/2
∆w
N (ns)⋅⋅⋅⋅⋅⋅⋅⋅⋅⋅⋅ ⋅⋅⋅⋅⋅⋅⋅⋅⋅⋅⋅⋅⋅⋅⋅⋅
F____ S____ T____
N (nf)⋅⋅⋅⋅⋅⋅⋅⋅⋅⋅⋅�
∆d : Depth of cut (radius designation) Designate without sign. The cutting direction depends on the direction
AA’. This designation is modal and is not changed until the other value
is designated. Also this value can be specified by the parameter (No.0717),
and the parameter is changed by the program command.
e : Escaping amount
This designation is modal and is not changed until the other value
is designated. Also this value can be specified by the parameter (No.0718),
and the parameter is changed by the program command.
ns : Sequence number of the first block for the program of finishing shape.
nf : Sequence number of the last block for the program of finishing shape.
∆u : Distance and direction of finishing allowance in X direction (diameter / radius designation).
∆w : Distance and direction of finishing allowance in Z direction. f,s,t : Any F , S, or T function contained in blocks ns to nf in the cycle is ignored,
and the F, S, or T function in this G71 block is effective.
G71 U (∆d) R (e) ; G71 P (ns) Q (nf) U (∆u) W (∆w) F (f ) S (s ) T (t) ;
Program command
��� � ���� �� � ��� � ��� ���� ��
The move command of a finished shape of A to A’ to B is specified in the blocks from sequence number ns to nf.
11.10 CANNED CYCLE (T SERIES)/MULTIPLE REPETITIVE CANNED CYCLE (M SERIES)
General
11. PROGRAM COMMAND B–61393E–2/02
616
[Classification] Input signal
[Function] Executes chamfering in a threading cycle. Specify the chamfering distance in parameter No.0109.
[Operation] When the signal is set to 1, chamfering is not executed in the threading cycle. When the signal is set to 0, chamfering is executed in the threading cycle.
γ
Approx. 45�
Approx. 45�
γ
Fig.11.10 (a) Straight thread cutting cycle Fig.11.10 (b)Taper thread cutting cycle
Set the chamfering distance� to the parameter No.0109. When the optional multiple repetitive canned cycle is provided, the chamfering distance can be specified in G76. The chamfering angle is made smaller than 45� by the remaining pulses in the automatic acceleration/ deceleration circuit and servo system.
CDZF126 (T series)
#7 0393
#6 #5 #4 CHKMRC
#3 #2 #1 MCQSCH
#0
[Data type] Bit
CHKMRC When a target figure other than a monotonically increasing or monotonically decreasing figure is specified in a multiple repetitive turning canned cycle (G71, G72): 0 : No alarm occurs. 1 : P/S alarm No. 064 is occurs.
NOTE This parameter is valid for multiple repetitive turning canned cycle type I.
Signal
Chamfering signal CDZ<G126#7> (T Series)
Signal address
Parameter � Various setting for
multiple repetitive canned cycle
B–61393E–2/02 11. PROGRAM COMMAND
617
MCQSCH Before a multiple repetitive canned cycle (G70 to G73) is started, a check to see if the program contains a block that has the sequence number specified in address Q is: 0 : Not made. 1 : Made. (If the sequence number specified in address Q cannot be
found, an alarm occurs and the canned cycle is not executed.)
0109 Chamfering distance in thread cutting cycles G76 and G92
[Data type] Byte
[Unit of data] 0.1
[Valid data range] 0 to 127
This parameter sets the chamfering distance in thread cutting cycles G76 and G92.
0717 Depth of cut in multiple repetitive canned cycles G71 and G72
[Data type] Two–word
Increment system ���� ���� ���� Unit
Metric input 0.01 0.001 0.0001 mm
Inch input 0.001 0.0001 0.00001 inch
[Valid data range] 0 to 99999999
This parameter sets the depth of cut in multiple repetitive canned cycles G71 and G72.
0718 Escape in multiple repetitive canned cycles G71 and G72.
[Data type] Two–word
Increment system ���� ���� ���� Unit
Metric input 0.01 0.001 0.0001 mm
Inch input 0.001 0.0001 0.00001 inch
[Valid data range] 0 to 99999999
This parameter sets the escape in multiple repetitive canned cycles G71 and G72.
� Chamfering distance in thread cutting cycles G76 and G92
� Depth of cut in multiple repetitive canned cycles G71 and G72
[Unit of data]
� Escape in multiple repetitive canned cycles G71 and G72.
[Unit of data]
11. PROGRAM COMMAND B–61393E–2/02
618
0719 Escape in multiple repetitive canned cycle G73 in X–axis direction
0720 Escape in multiple repetitive canned cycle G73 in Z–axis direction
[Data type] Two–word
Increment system ���� ���� ���� Unit
Metric input 0.01 0.001 0.0001 mm
Inch input 0.001 0.0001 0.00001 inch
[Valid data range] –99999999 to 99999999
This parameter sets the escape in multiple repetitive canned cycle G73 of an X, then Z axis.
0721 Division count in multiple repetitive canned cycle G73
[Data type] Two–word
[Unit of data] Cycle
[Valid data range] 1 to 99999999
This parameter sets the division count in multiple repetitive canned cycle G73.
0722 Return in multiple canned cycles G74 and G75
[Data type] Two–word
Increment system ���� ���� ���� Unit
Metric input 0.01 0.001 0.0001 mm
Inch input 0.001 0.0001 0.00001 inch
[Valid data range] 0 to 99999999
This parameter sets the return in multiple repetitive canned cycles G74 and G75.
� Escape in multiple repetitive canned cycles G73
[Unit of data]
� Division count in multiple repetitive canned cycle G73
� Return in multiple canned cycles G74 and G75
[Unit of data]
B–61393E–2/02 11. PROGRAM COMMAND
619
0723 Repetition count of final finishing in multiple repetitive canned cycle G76
[Data type] Two–word
[Unit of data] Cycle
[Valid data range] 1 to 99999999
This parameter sets the repetition count in multiple repetitive canned cycle G76.
0724 Tool nose angle in multiple repetitive canned cycle G76
[Data type] Two–word
[Unit of data] Degree
[Valid data range] 0 to 120 when FS15 tape format is used 0, 29, 30, 55, 60 and 80 when FS15 tape format is not used.
This parameter sets the tool nose angle in multiple repetitive canned cycle G76.
0725 Minimum depth of cut in multiple repetitive canned cycle G76
[Data type] Two–word
Increment system ���� ���� ���� Unit
Metric input 0.01 0.001 0.0001 mm
Inch input 0.001 0.0001 0.00001 inch
[Valid data range] 0 to 99999999
This parameter sets the minimum depth of cut in multiple repetitive canned cycle G76.
0726 Finishing allowance in multiple repetitive canned cycle G76
[Data type] Two–word
Increment system ���� ���� ���� Unit
Metric input 0.01 0.001 0.0001 mm
Inch input 0.001 0.0001 0.00001 inch
[Valid data range] 0 to 99999999
This parameter sets the finishing allowance in multiple repetitive canned cycle G76.
� Repetition count of final finishing in multiple repetitive canned cycle G76
� Tool nose angle in multiple repetitive canned cycle G76
� Minimum depth of cut in multiple repetitive canned cycle G76
[Unit of data]
� Finishing allowance in multiple repetitive canned cycle G76
[Unit of data]
11. PROGRAM COMMAND B–61393E–2/02
620
������ Message Description
061 ADDRESS P/Q NOT FOUND IN G70–G73
Address P or Q is not specified in G70, G71, G72, or G73 command. Modify the program.
062 ILLEGAL COMMAND IN G71–G76
1 The depth of cut in G71 or G72 is zero or negative value.
2 The repetitive count in G73 is zero or negative value.
3 The negative value is specified to ∆i or ∆k in G74 or G75.
4 A value other than zero is specified to address U or W, though ∆i or ∆k is zero in G74 or G75.
5 A negative value is specified to ∆d, though the relief direction in G74 or G75 is determined.
6 Zero or a negative value is specified to the height of thread or depth of cut of first time in G76.
7 The specified minimum depth of cut in G76 is greater than the height of thread.
8 An unusable angle of tool tip is speci- fied in G76.
Modify the program.
063 SEQUENCE NUMBER NOT FOUND
The sequence number specified by address P in G70, G71, G72, or G73 command cannot be searched. Modify the program.
064 SHAPE PROGRAM NOT MONOTONOUSLY
A target shape which is not monotone increase or decrease was specified in a repetitive canned cycle (G71 or G72).
065 ILLEGAL COMMAND IN G71–G73
1 G00 or G01 is not commanded at the block with the sequence number which is specified by address P in G71, G72, or G73 command.
2 Address Z(W) or X(U) was comman- ded in the block with a sequence num- ber which is specified by address P in G71 or G72, respectively.
Modify the program.
066 IMPROPER G–CODE IN G71–G73
An unallowable G code was comman- ded beween two blocks specified by address P in G71, G72, or G73. Modify the program.
067 CAN NOT ERROR IN MDI MODE
G70, G71, G72, or G73 command with address P and Q was specified. Modify the program.
069 FORMAT ERROR IN G70–G73
The final move command in the blocks specified by P and Q of G70, G71, G72, or G73 ended with cham- fering or corner R.
OPERATOR’S MANUAL (For Lathe) (B–61394E)
II.13.1 II.13.2
CANNED CYCLE MULTIPLE REPETITIVE CYCLE
Alarm and message
Reference item
B–61393E–2/02 11. PROGRAM COMMAND
621
Mirror image can be applied to X–axis with G code.
G68 : Double turret mirror image on
G69 : Mirror image cancel
When G68 is designated, the coordinate system is shifted to the mating turret side, and the X–axis sign is reversed from the programmed command to perform symmetrical cutting. To use this function, set the distance between the two turrets to a parameter (No. 0730). Program example for double turrets.
X
60 120
180
(2)
(1)
(3)
12 0
Z
80 φ 4
0φ
Offset value of tool post A
Offset value of tool post B
Tool post A
Tool post B
12 0φ
X40.0 Z180.0 T0101 ; Position turret A at (1) G68 ; Shift the coordinate system by the distance A to B
(120mm), and turn mirror image on. X80.0 Z120.0 T0202 ; Position turret B at (2) G69 ; Shift the coordinate system by the distance B to A,
and cancel mirror image. X120.0 Z60.0 T0101 ; Position turret A at (3)
11.11 MIRROR IMAGE FOR DOUBLE TURRETS (T SERIES)
General
11. PROGRAM COMMAND B–61393E–2/02
622
0730 Distance between two turrets in mirror image
[Data type] Two–word
[Unit of data]
Increment system IS–A IS–B IS–C Unit
Millimeter machine 0.01 0.001 0.0001 mm
Inch input 0.001 0.0001 0.00001 inch
[Valid data range] 0 to 999999999
Set the distance between two turrets in mirror image.
OPERATOR’S MANUAL (For Lathe) (B–61394E)
II.13.6 MIRROR IMAGE FOR DOUBLE TURRETS (G68, G69)
Parameter
� Distance between two turrets
Reference Item
B–61393E–2/02 11. PROGRAM COMMAND
623
By specifying indexing positions (angles) for the indexing axis (one rotation axis, A, B, or C), the index table of the machining center can be indexed. Before and after indexing, the index table is automatically unclamped or clamped .
The control axis that indexes the index table can be named A, B or C. It will be referred to as “B” in the following discussion.
The positioning angle for the index table is commanded by the numerics following “B” in the program command, which is an independent block. Both absolute and incremental commands are possible, but the value after “B” is the integer times the numeric set by the parameter:
(Example) G00G90B100000; Absolute command (Positioning angle 10 degrees)
G00G91B20.0; Incremental command (Move distance 20 degrees)
There are two variations of the procedure (type A and type B) to set the index table position; the difference is in the ON/OFF timing of the position control servo. The sequence of events and the difference between the variations are described below, followed by time charts showing them graphically.
(1)Assume Bbbbb is ordered by the command program. (2)The CNC turns the B axis unclamp signal BUCLP <F188#2> to “1”.
(Type B -- When BUCLP is turned to “1”, the position control servo for the B axis is turned ON.)
(3)On the PMC side, the clamp of the B axis is released; when completed, the B axis unclamp completion signal *BEUCP <G143#6> turns to “0”.
(4)The CNC then turns the B axis unclamp signal BEUCP to “0”, to indicate it received the *BEUCP signal.
(5)When the PMC is notified that BUCLP has been turned to “0”, the PMC should turn *BEUCP to “1”. In type B, B–axis unclamp signal BUCLP is turned to “0”, B–axis position control is made in servo–on state, B–axis is rotated, and the B axis is stopped at the specified position. B axis always moves at rapid traverse.
(6)When the B axis stops at the specified position, CNC turns B–axis clamp signal BCLP<F188#3>to 1. In type A, signal BCLP is set to “1” and B–axis position control is made in servo–off state.
(7)When BCLP is turned to “1” on the PMC side, the B axis is clamped mechanically (with a clutch or shot pin, for example). When the clamp is completed, the B axis clamp completion signal *BECLP <G143#7> is turned to “0”.
11.12 INDEX TABLE INDEXING FUNCTION (M SERIES)
General
Basic Procedure
11. PROGRAM COMMAND B–61393E–2/02
624
(8)When *BECLP is turned to “0”, the CNC then turns BCLP to “0”, informing it received the *BECLP signal. (Type B -- When BCLP turns to “0”, the B axis position control servo is turned off.)
(9)On the PMC side, when BCLP changes to “0”, *BECLP is turned to “1”. This completes the sequence.
The time charts for these operations are shown in the figures below.
B command (independent) Bbbbb
B axis servo on for position control
B axis unclamp signal BUCLP<F188#2>
B axis unclamp completion signal *BEUCP<G143#6>
B axis rotation
B axis clamp signal BCLP<F188#3>
B axis clamp completion signal *BECLP<G143#7>
(1) (2) (3) (4) (5) (6) (7) (8) (9)
Fig. 11.12 (a) Time chart for positioning index table (type A)
B command (independent) Bbbbb
B axis servo on for position control
B axis unclamp signal BUCLP<F188#2>
B axis unclamp completion signal *BEUCP<G143#6>
B axis rotation
B axis clamp signal BCLP<F188#3>
B axis clamp completion signal *BECLP<G143#7>
(1) (2) (3) (4) (5) (6) (7) (8) (9)
Fig. 11.12 (b) Time chart for positioning index table (type B)
B–61393E–2/02 11. PROGRAM COMMAND
625
Manual reference position return of B axis time chart (type A) is shown in the figure below.
B axis manual feed selection signal +4
B axis position control servo ON
B axis unclamp signal BUCLP<F188#2>
B axis unclamp completion signal *BEUCP<G143#6>
B axis rotation
B axis deceleration signal *DEC4<X019#5>
B axis return completion signal ZP4<F148#3>
B axis clamp signal BCLP<F188#3>
B axis clamp completion signal *BECLP<G143#7>
Fig. 11.12 (c) Manual reference position return of B axis time chart (type A)
As described in the basic procedure, type A differs from type B in that the servo used for B–axis position control is turned on or off at the different timing. Type A is suitable for a system in which the B–axis is clamped with shot pins. Type B is suitable for a system in which the B–axis is clamped with a clutch.
When the B–axis is clamped with shot pins, the mechanism can be indexed at only a limited number of positions. The minimum indexing angle can be specified in parameter No. 0839. If an angle which is not a multiple of this minimum indexing angle is specified in indexing, alarm No. 135 is issued.
The direction of rotation can be set to one of the following.
– Whichever direction has the shorter distance (IXINC, bit 3 of parameter No. 0079)
– Direction specified with a command
– Usually the positive direction. Only when a particular M code is specified in the same block, the axis rotates in the negative direction (parameter No. 0249).
Setting IXG90, bit 4 of parameter No. 0079, specifies absolute programming, irrespective of G90/G91 mode.
Type A and Type B
Minimum indexing angle
Direction of rotation
Absolute/incremental programming
11. PROGRAM COMMAND B–61393E–2/02
626
[Classification] Output signal
[Function] Instructs the PMC side to clamp the B axis mechanically with a clutch or shot pin.
[Output condition] The output condition and procedure are the same as those described in the basic procedure for positioning the index table.
[Classification] Input signal
[Function] Notifies the CNC of completion of the B axis clamp operation.
[Operation] The operation and procedure are the same as those described in the basic procedure for positioning the index table.
[Classification] Output signal
[Function] Instructs the PMC side to release the B axis from the mechanical clamp.
[Output condition] The output condition and procedure are the same as those described in the basic procedure for positioning the index table.
[Classification] Input signal
[Function] Notifies the CNC of completion of the release of the B axis from the mechanical clamp.
[Operation] The operation and procedure are the same as those described in the basic procedure for positioning the index table.
#7 *BECLPG143
#6 *BEUCP
#5 #4 #3 #2 #1 #0
#7 F188
#6 #5 #4 #3 BCLP
#2 BUCLP
#1 #0
Signal
B axis clamp signal BCLP<F188#3>
B axis clamp completion signal *BECLP<G143#7>
B axis unclamp signal BUCLP<F188#2>
B axis unclamp completion signal *BEUCP<G143#6>
Signal address
B–61393E–2/02 11. PROGRAM COMMAND
627
#7 0011
#6 #5 #4 #3 #2 ADLN
#1 #0
[Data type] Bit
ADLN 0 : 4th axis is rotation axis. 1 : 4th axis is linear axis.
#7 IXTYP0079
#6 #5 #4 IXG90
#3 IXINC
#2 IXABS
#1 IXREL
#0 IXDDP
[Data type] Bit
IXDDP Selection of decimal–point input method of index table indexing axis 0 : Conventional method (Example IS–B: B1; = 0.001 deg) 1 : Pocket calculator method (Example IS–B: B1; = 1.000 deg)
IXREL Relative position display of index table indexing axis 0 : Not rounded by 360 degrees 1 : Rounded by 360 degrees
IXABS Displaying absolute coordinate value of index table indexing axis 0 : Not rounded by 360 degrees
The index table indexing axis rotates 720 degrees (two rotations) when G90 B720.0; is specified from the 0–degree position. It rotates in reverse direction 720 degrees (two rotations) when G90 B0.; is specified. The absolute coordinate value then becomes 0 degree.
1 : Rounded by 360 degrees The index table indexing axis is positioned in 40 degrees when G90 B400.0; is specified from the 0–degree position. The index table indexing axis does not rotate by two or more turns when this parameter is set to 1. It also does not move when G90 B720.0; is specified from the 0–degree position.
IXINC Rotation in the G90 mode when negative–direction rotation command M code (parameter No. 0249) is not set 0 : Not set to the shorter way around the circumference 1 : Set to the shorter way around the circumference (Set IXABS, #2 of
parameter No. 0079, to 1.)
IXG90 Index table indexing command 0 : Judged to be an absolute/increment command according to the
G90/G91 mode 1 : Judged to be an absolute command
IXTYP Index table indexing sequence 0 : Type A 1 : Type B
Parameter
� Setting linear or rotation axis
� Various setting for index table indexing
11. PROGRAM COMMAND B–61393E–2/02
628
0249 Negative 0 direction rotation command M code
[Data type] Byte
[Valid data range] 0 to 255
0 : Not use an M code that sets the index table rotation to the negative direction. The rotation direction is specified using a command and parameter (IXINC, #3 of parameter No. 0079).
1 to 255: Sets an M code that sets the index table rotation to the negative direction. The rotation is set to the negative direction only when an M code set here is specified in the same block as an index table indexing command. If the M code is not specified in the same block, the rotation is always set to the positive direction.
WARNING Set IXABS, #2 of parameter No. 0079, to 1.
0839 Unit of index table indexing angle
[Data type] Two–word
[Unit of data]
Increment system IS–A IS–B IS–C Unit
Metric input 0.01 0.001 0.0001 mm
[Valid data range] 0 to 360000 This parameter sets the unit of index table indexing angle. A P/S alarm is generated when movement other than integer multiple of the setting value is specified.
NOTE If zero is specified as the setting value, any command can be specified irrespective of the unit of angle.
������ Message Description
135 SPINDLE ORIENTATION PLEASE
Without any spindle orientation , an attept was made for spindle indexing. Perform spindle orientation.
136 ILLEGAL AXIS COM- MAND
In index table indexing , another con- trol axis was instructed together with the B axis. Modify the program.
� Negative direction rotation command M code
� Unit of index table indexing angle
Alarm and Message
B–61393E–2/02 11. PROGRAM COMMAND
629
WARNING 1 The secondary auxiliary function can be used if the address
is different from that of the indexing axis. 2 If the incremental command is used for indexing of the index
table, the workpiece zero point offset value on the index table axis must always be 0. That is, the machine coordinate system must always agree with the workpiece coordinate system of the index table axis.
3 The dry run signal DRN is ineffective during positioning of the B axis.
4 The machine lock signal MLK is functional during positioning of the B axis. However, while the B axis is moving, after the movement ends, the MLK is functional.
NOTE 1 Specify a rotation axis as the index table indexing axis. 2 The servo off signal for the index table indexing axis is
invalid. 3 Single direction positioning (G60) cannot be specified. 4 While the index table is being positioned, input signals that
reset the CNC, such as *ESP (emergency stop), ERS (external reset), and RRW (reset & rewind), are functional. When reset is applied to the CNC, this operation stops. Further, if *SP (automatic operation stop signal) turns to “0”, axis movement is stopped and the equipment enters the automatic operation stop state. If a stop at an any position is not suitable for the machine, appropriate processing is required on the machine.
5 If a reset occurs while the system is awaiting the completion of clamping or unclamping, the clamp or unclamp signal is cleared. The CNC exits from the completion wait status.
6 Manual operation of jog feed, incremental feed and handle feed cannot be used with the B axis, but manual reference position return is possible. If reset is applied during the movement of B axis, the manual reference position return operation is performed.
7 No movement can be performed by automatic return from the reference position (G29), return to the second reference position (G30), or selection of the machine coordinate system (G53).
OPERATOR’S MANUAL (For Machining Center) (B–61404E)
II.14.10 INDEX TABLE INDEXING FUNC- TION
Warning
Note
Reference Item
11. PROGRAM COMMAND B–61393E–2/02
630
A programmed figure can be magnified or reduced (scaling). The dimensions specified with X_, Y_, and Z_ can each be scaled up or down with the same or different rates of magnification. The magnification rate can be specified in the program. Unless specified in the program, the magnification rate specified in the parameter is applied.
Least input increment of scaling magnification is: 0.001 or 0.00001. It depends on parameter SCR (No. 0036#07) which value is selected. If scaling P is not specified on the block of scaling (G51X_Y_Z_P_ ;), the scaling magnification set to parameter (No. 0731) is applicable. If X,Y,Z are omitted, the tool position where the G51 command was specified serves as the scaling center.
G51X_Y_Z_P_ ; Scaling start
Scaling is effective.
(Scaling mode)
Format Meaning of command
X_Y_Z_ : Absolute command for center coordinate value of scaling
P_ : Scaling magnification
G50 ; Scaling cancel
SCALING UP OR DOWN ALONG ALL AXES AT THE SAME RATE OF MAGNIFICATION
Y
X
P4
P4′
P1
P1′
P3′
P2′
P2
P3
P0
P0:Scaling center 0
Fig. 11.13 (a) Scaling (P 1 P2 P3 P4�P1′ P2′ P3′ P4′)
11.13 SCALING (M SERIES)
General
� Scaling up or down along all axes at the same rate of magnification
B–61393E–2/02 11. PROGRAM COMMAND
631
Each axis can be scaled by different magnifications. Also when a negative magnification is specified, a mirror image is applied. First of all, set a parameter ESCAL (No.0063#6) which validates each axis scaling (mirror image). Then, set parameter SCLx (No. 0036#0 to #2) to enable scaling along each axis. Least input increment of scaling magnification of each axis (I, J, K) is 0.001 or 0.00001( set parameter SCR (No.0036#7)). Magnification is set within the range ±0.00001 to ±9.99999 or ±0.001 to ±9.999. If a negative value is set, mirror image is effected. If magnification I, J or K is not commanded, a magnification value set to parameter (Nos. 0731 to 0733) is effective. However, a value other than 0 must be set to the parameter.
G51_X_Y_Z_I_J_K_; Scaling start X_Y_Z_: Absolute command for center coordinate value of scaling
I_J_K_: Scaling magnification for X axis, Y axis and Z axis respectively
G50 Scaling cancel
Format Meaning of command
Scaling is effective. (Scaling mode)
SCALING UP OR DOWN ALONG EACH AXES AT A DIFFERENT RATE OF MAGNIFICATION (MIRROR IMAGE)
c
Y axis
X axis
b a
d
a/b : Scaling magnification of X axis
c/d : Scaling magnification of Y axis
0 : Scaling center
Programmed figure
Scaled figure
0
Fig. 11.13 (b) Scaling of each axis
� Scaling of each axis, programmable mirror image (negative magnification)
11. PROGRAM COMMAND B–61393E–2/02
632
#7 SCR0036
#6 #5 #4 #3 #2 SCLZ
#1 SCLY
#0 SCLX
[Data type] Bit
SCR Scaling magnification unit 0 : 0.00001 times (1/100,000) 1 : 0.001 times
SCLx Scaling for each axis 0 : Invalidated 1 : Validated
#7 0063
#6 ESCAL
#5 #4 #3 #2 #1 #0
[Data type] Bit
ESCAL Axis scaling and programmable mirror image 0 : Invalidated (The scaling magnification is specified by P.) 1 : Validated
0731 Magnification used when scaling magnification is not specified
[Data type] Two–word
[Unit of data] 0.001 or 0.00001 times (Selected using SCR, #7 of parameter No. 0036)
[Valid data range] 1 to 999999 This parameter sets the scaling magnification. This setting value is used when a scaling magnification (P) is not specified in the program.
WARNING Parameter Nos.0731 to 0733 becomes valid when scaling for every axis is valid. (ESCAL, #6 of parameter No. 0063 is “1”.)
0731 Scaling magnification for X axis
to
0733 Scaling magnification for Z axis
[Data type] Two–word
[Unit of data] 0.001 or 0.00001 times (Selected using SCR, #7 of parameter No. 0036)
[Valid data range] –999999 to –1, 1 to 999999 This parameter sets the scaling magnification for each axis.
Parameter
� Setting valid/invalid and magnification of scaling
� Magnification used when scaling magnification is not specified
� Scaling magnification for each axis
B–61393E–2/02 11. PROGRAM COMMAND
633
������ Message Description
141 CAN NOT COMMAND G51 IN CRC
G51 (Scaling ON) is commanded in the tool offset mode. Modify the program.
142 ILLEGAL SCALE RATE Scaling magnification is commanded in other than 1 – 999999. Correct the scaling magnification set- ting.
143 SCALED MOTION DATA OVERFLOW
The scaling results, move distance, coordinate value and circular radius exceed the maximum command val- ue. Correct the program or scaling magnification.
OPERATOR’S MANUAL (For Machining Center) (B–61404E)
II.14.8 SCALING (G50, G51)
Alarm and Message
Reference Item
11. PROGRAM COMMAND B–61393E–2/02
634
A programmed shape can be rotated. By using this function it becomes possible, for example, to modify a program using a rotation command when a workpiece has been placed with some angle rotated from the programmed position on the machine. Further, when there is a pattern comprising some identical shapes in the positions rotated from a shape, the time required for programming and the length of the program can be reduced by preparing a subprogram of the shape and calling it after rotation.
(α,β)
Angle of rotationCenter of rotation
�
Rotation plane G17
Y
X
R
Fig. 11.14 Coordinate system rotation
G17 (G18 or G19) : Select the plane in which contains the figure to be rotated.
α_β_ Absolute command for two of the x_,y_,and Z_ axes that correspond to the current plane selected by a command (G17, G18, or G19). The command specifies the coordinates of the center of rotation for the values specified subsequent to G68.
R_ Angular displacement with a positive value indicates counter clockwise rotation. Parameter 0041#0 selects whether the specified angular displacement is always considered an absolute value or is considered an absolute or incremental value depending on the specified G code (G90 or G91).
Least input increment : 0.001 deg Valid data range : –360.000 to 360.000
G68 α�β�R� ; Start rotation of a coordinate system.
Coordinate system rotation mode
(The coordinate system is rotated.)
G69 ; Coordinate system rotation cancel command
FORMAT
MEANING OF COMMAND
G17 G18 G19
11.14 COORDINATE SYSTEM ROTATION (M SERIES)
General
B–61393E–2/02 11. PROGRAM COMMAND
635
#7 0041
#6 #5 #4 #3 #2 #1 #0 RIN
[Data type] Bit
RIN Coordinate rotation angle command (R) 0 : Specified by an absolute method 1 : Specified by G90 or G91
0730 Angular displacement used when no angular displacement is specified for coordinate system rotation
[Data type] Two–word
[Unit of data] 0.001 degrees
[Valid data range] –360000 to 360000 This parameter sets the angular displacement for coordinate system rotation. When the angular displacement for coordinate system rotation is not specified with address R in the block where G68 is specified, the setting of this parameter is used as the angular displacement for coordinate system rotation.
������ Message Description
144 ILLEGAL PLANE SE- LECTED
The coordinate rotation plane and arc or cutter compensation C plane must be the same. Modify the program.
OPERATOR’S MANUAL (For Machining Center) (B–61404E)
II.14.9 COORDINATE SYSTEM ROTATION (G68, G69)
Parameter
� Angle specification method of coordinate system rotation
� Angular displacement used when no angular displacement is specified for coordinate system rotation
Alarm and Message
Reference Item
11. PROGRAM COMMAND B–61393E–2/02
636
There are two types of NC programs; those which, once created, are scarcely changed, and those which are changed for each machining type. The former are programs created by the custom macro, and the latter are machining programs. If programs of these types are executed simultaneously, a battery may run out or the custom macro may be destroyed by error operation. Such problems can be solved by this function. The custom macro created by a machine tool builder is converted to an execute-form program, be stored in the ROM cassette, and be executed.
Features (1) Since the program is stored after converted to an execute-form
program, the execution speed is high. The machining time is then reduced, and the precision is improved.
(2) Since the program is stored in ROM cassette, there is no problem of battery extinction or custom macro destruction by error operation. The reliability is improved.
(3) Since the stored program is not displayed on a program screen, the know-how of the machine tool builder is protected.
(4) Since the custom macro is stored in ROM cassette, the program edit memory can be used efficiently.
(5) The user can call the macro easily without knowing the stored program. A custom macro can be created and executed in the program edit memory as usual.
(6) An original screen can be created by using the graphic display or selecting screens by the soft key. The machine tool builder can extend the control function by using such functions as machining program creation and edit control, reader/punch interface control, and PMC data read/write functions.
NOTE When the macro executor is attached, the order-made macro cannot be specified.
Macro compiler/executer programming manual (B–61393E–1)
11.15 MACRO COMPILER/ MACRO EXECUTER
General
Note
Reference Item
B–61393E–2/02 12. DISPLAY/SETTING/EDIT
637
12 DISPLAY/SETTING/EDIT
12. DISPLAY/SETTING/EDIT B–61393E–2/02
638
[Classification] Input signal
[Function] Setting this signal to 1 disables the updating of relative coordinates. Subsequently setting this signal to 0 causes the updating of relative coordinates to be resumed.
[Classification] Input signal
[Function] This signal enables or disables the display of ladder diagrams. *LDSP = 1: Does not display ladder diagrams. *LDSP = 0: Displays ladder diagrams.
NOTE This signal is enabled only when bit 2 (LDDSPG) of parameter No. 0060 is set to 1. When LDDSPG is 0, dynamic ladder display is disabled regardless of the state of this signal.
#7 G119
#6 #5 #4 #3 #2 #1 #0 *LDSP
G127 DLK
#7 0060
#6 #5 #4 #3 #2 LDDSPG
#1 #0
[Data type] Bit
LDDSPG Dynamic ladder display is: 1 : Performed. 0 : Not performed.
12.1 DISPLAY/SETTING
Signal
Relative coordinate update disable signal DLK<G127#6>
Ladder display signal *LDSP<G119#0>
Signal address
Parameter
B–61393E–2/02 12. DISPLAY/SETTING/EDIT
639
Time is displayed in the hour/minute/second format on each display screen. Some screens allows display of the year, month, and day. The custom macro system variable can be used to read the time. The time will be told through the window on the PMC side.
Time information can be read and written.
System variables for time information
Variable number
Function
#3001 This variable functions as a timer that counts in 1–millisecond increments at all times. When the power is turned on, the value of this variable is reset to 0. When 65535 milliseconds is reached, the value of this timer returns to 0.
#3002 This variable functions as a timer that counts in 1–hour incre- ments when the cycle start lamp is on. This timer preserves its value even when the power is turned off. When 1145324.612 hours is reached, the value of this timer returns to 0.
#3011 This variable can be used to read the current date (year/ month/day). Year/month/day information is converted to an apparent decimal number. For example, March 28, 1995 is represented as 19950328.
#3012 This variable can be used to read the current time (hours/min- utes/seconds). Hours/minutes/seconds information is con- verted to an apparent decimal number. For example, 34 min- utes and 56 seconds after 3 p.m. is represented as 153456.
OPERATOR’S MANUAL (For Machining Center) (B–61404E)
III.11.5.5 Displaying and Setting Run Time,Parts Count, and Time
OPERATOR’S MANUAL (For Lathe) (B–61394E)
III.11.5.3 Displaying and Setting Run Time,Parts Count, and Time
12.1.1 Clock Function
General
Reference item
12. DISPLAY/SETTING/EDIT B–61393E–2/02
640
On the servo tuning screen, parameters required for basic adjustment of the servo motor and statuses being monitored are listed for each axis.
#7 0389
#6 #5 #4 #3 #2 #1 #0 SRVSET
[Data type] Bit
SRVSET Servo tuning screen 0 : Displayed 1 : Not displayed
MAINTENANCE MANUAL (B–61395E)
5.2 SERVO TUNING SCREEN
On the spindle tuning screen, parameters required for basic adjustment of the serial spindle and statuses being monitored are listed. The screen is only for the main spindle connected to the first amplifier.
#7 0389
#6 #5 #4 #3 #2 #1 SPPRM
#0
[Data type] Bit type
SPPRM Spindle tuning screen 0 : Not displayed 1 : Displayed
MAINTENANCE MANUAL (B–61395E)
6.4 SPINDLE TUNING SCREEN
12.1.2 Servo Tuning Screen
General
Parameter
Reference item
12.1.3 Spindle Tuning Screen
General
Parameter
Reference item
B–61393E–2/02 12. DISPLAY/SETTING/EDIT
641
Servo waveform display provides graphs of waveforms to illustrate changes in the following data.
a. Servo motor error value along each axis, number of distributed pulses and torque
b. On/off status of the machine signal, specified by a signal address
#7 0077
#6 #5 #4 #3 #2 SGD
#1 #0
[Data type] Bit
SGD Servo waveform 0 : Not displayed 1 : Displayed
NOTE Servo waveform display is enabled when bit 2 (SGD) of parameter No. 0077 is set to 1. To perform waveform diagnosis, a graphics board is required.
MAINTENANCE MANUAL (B–61395E)
1.8 WAVEFORM DIAGNOSTIC DIS- PLAY
12.1.4 Servo Waveform Display
General
Parameter
Note
Reference item
12. DISPLAY/SETTING/EDIT B–61393E–2/02
642
When a breakdown occurs, in order to quickly determine the cause, the following should be done. First, it has to be determined as to whether the breakdown occurred in the NC internal section, or the PMC or machine side. There are times when it appears that a breakdown has occurred even when the breakdown has not actually occurred. For example, when the machinery ceases to operate because it is waiting for an external signal. In this case, the condition of the interface between the CNC and PMC, or between the CNC and the machinery, and the conditions within the CNC need to be investigated. The NC checks the following itself.
1) Abnormality of detection system
2) Abnormality of position control unit
3) Abnormality of servo system
4) Overheat
5) Abnormality of CPU
6) Abnormality of ROM
7) Abnormality of RAM
8) Abnormality in data transfer between CRT/MDI
9) Abnormality of part program storage memory
10)Abnormality in tape reader read function
11)Abnormality in data transfer between PMC
Input/output signals from PMC to CNC, or vice versa, and inner status of the NC can be displayed on the CRT screen.
OPERATOR’S MANUAL (For Machining Center) (B–61404E)
III.7.2 CHECKING BY SELF–DIAGNOS- TIC SCREEN
OPERATOR’S MANUAL (For Lathe) (B–61394E)
III.7.2 CHECKING BY SELF–DIAGNOS- TIC SCREEN
12.1.5 Self–diagnosis
General
Reference item
B–61393E–2/02 12. DISPLAY/SETTING/EDIT
643
Indication of the current position can be suppressed by setting parameters. (except for basic axes of T series)
#7 0029
#6 DSPSUB
#5 #4 #3 #2 #1 DSP4
#0 DSP3 (T series)
[Data type] Bit
DSPx Specifies whether to display the current position of the third axis, as follows: 1 : Display 0 : Do not display
DSPSUB Fifth and Sixth axes in absolute and relative screens 0 : Display 1 : Do not display
#7 0035
#6 #5 #4 #3 NDSP4
#2 NDSP3
#1 NDSPY
#0 NDSPX (M series)
[Data type] Bit
NDSPx Display of the current position for each axis 0 : The current position is displayed. 1 : The current position is not displayed.
#7 0061
#6 DSP78
#5 #4 #3 #2 #1 #0
[Data type] Bit
DSP78 Seventh and Eighth axes in absolute and relative screens 0 : Display 1 : Do not display
12.1.6 Position Display Neglect
General
Parameter
12. DISPLAY/SETTING/EDIT B–61393E–2/02
644
This function displays the integrated cycle operation time and the integrated cutting time on the CRT display screen. The integrated cycle operation time, the integrated cutting time can be altered and preset, using the MDI. In addition to the above, this function displays the count of the total number of parts machined, the number of parts required and the number of parts machined on the CRT screen. Each time M02, M30 or a parameter set M code is executed, the count of the total number of parts machined and the number of parts machined in memory is incremented by 1. If a program is prepared so as to execute M02, M30 or a parameter set M code each time one part machining is completed, the number of parts machined can be counted automatically. If the count of the number of parts machined reaches the number of parts required, a signal is output to the PMC side. It is possible to change and preset the number of parts required and the number of parts machined using MDI.
[Classification] Output signal
[Function] Reports to the PMC that the specified number of parts have been machined.
[Output condition] The PRTSF signal is set to 1 when: � Machining of the specified number of parts has been completed.
When 0 (infinity) is set as the required number of parts, this signal is not output.
The PRTSF signal is set to 0 when:
� Machining of the specified number of parts has not yet been completed.
� The system is reset.
#7 PRTSFF164
#6 #5 #4 #3 #2 #1 #0
12.1.7 Run Hour and Parts Count Display
General
Signal
Required parts count reached signal PRTSF<F164#7>
Signal address
B–61393E–2/02 12. DISPLAY/SETTING/EDIT
645
#7 0040
#6 #5 #4 #3 RWCNT
#2 #1 #0
[Data type] Bit
RWCNT M code that counts the total number of machined parts and the number of machined parts 0 : M02, or M30, or an M code specified by parameter No.0219 1 : Only M code specified by parameter No.0219
0219 M code that counts the total number of machined parts and the number of machined parts
[Data type] Byte [Valid data range] 0 to 255 except 98 and 99
The total number of machined parts and the number of machined parts are counted (+1) when the M code set is executed.
NOTE Set value 0 is invalid (the number of parts is not counted for M00). Data 98 and 99 cannot be set.
0600 Number of required parts
[Data type] Word [Unit of data] One piece
[Valid data range] 0 to 9999
This parameter sets the number of required machined parts.
Required parts finish signal PRTSF is output to PMC when the number of machined parts reaches the number of required parts. The number of parts is regarded as infinity when the number of required parts is zero. The PRTSF signal is then not output.
0779 Total number of machined parts
[Data type] Two–word [Unit of data] One piece
[Valid data range] 0 to 99999999
This parameter sets the total number of machined parts.
The total number of machined parts is counted (+1) when M02, M30, or an M code specified by parameter No.0219 is executed.
OPERATOR’S MANUAL (For Machining Center) (B–61404E)
III.11.5.5 Displaying and Setting Run Time, Parts Count, and Time
OPERATOR’S MANUAL (For Lathe) (B–61394E)
III.11.5.3 Displaying and Setting Run Time, Parts Count, and Time
Parameter
Reference item
12. DISPLAY/SETTING/EDIT B–61393E–2/02
646
It is possible to draw the programmed tool path on the CRT screen, which makes it possible to check the progress of machining, while observing the path on the CRT screen. In addition, it is also possible to enlarge/reduce the screen. The drawing coordinates (parameter) and graphic parameters must be set before a tool path can be displayed. In the 0–TTC, the tool paths of two tool posts are displayed on the same screen, one on the right and the other on the left.
O9501 N0014
X 0.000 Y 0.000 Z 0.000
S 0 T 10:17:21 AUTO [ G.PRM ][ GRAPH ][ AUX ][ ][ ]
Z
X Y
0–MC
S 0.33 O0001 N0022 X 200.000 Z 220.000 C 0.000 Y 0.000
S 0 T0101 21:46:31 AUTO [ GRAPH ][ G.PRM ][ ZOOM ][NORMAL ][ AUX ]
X
Z
0–TC
12.1.8 Graphic Display/ Dynamic Graphic Display
General
Graphic Display
B–61393E–2/02 12. DISPLAY/SETTING/EDIT
647
HEAD2 :O0210 N2930
S 0 T 15:33:55 BUF AUTO [ GRAPH ][ G.PRM ][ ZOOM ][NORMAL ][ AUX ]
X
Z
0–TTC
There are the following two functions in Dynamic Graphics.
Path graphic
Solid graphic
This is used to draw the path of tool center com- manded by the part program.
This is used to draw the workpiece figure machined by tool movement commanded by the part program.
The path graphic function is used to precisely check the part program for drawing the tool path with a line. The solid graphic function is used to draw the workpiece figure to be machined with a program. Thus, it is easy to recognize roughly the part program. These two functions can be used freely by switching them.
 DISPLAY/SETTING/EDIT B–61393E–2/02
648
O1126 N01126
ÂÂÂÂÂÂ ÂÂÂÂÂÂ ÂÂÂÂÂÂ ÂÂÂÂÂÂ ÂÂÂÂÂÂ ÂÂÂÂÂÂ ÂÂÂÂÂÂ ÂÂÂÂÂÂ
ÄÄ ÄÄ
ÄÄ ÄÄ
F.ST STOP REWINDA.ST
SOLID GRAPHIC (EXECUTION)
Z Y
X
Part Machined
[Classification] Output signal
[Function] Reports that a machining drawing is being created.
[Operation] The signal becomes 1 when: �Creation of a machining drawing is started. The signal becomes 0 when: �Creation of a machining drawing is stopped.
#7 F164
#6 #5 CKGRP
#4 #3 #2 #1 #0
#7 0024
#6 #5 #4 #3 GNSR
#2 #1 #0 (T series)
[Data type] Bit
GNSR Current position display on the graphic display screen 0 : Displays the actual position to ensure tool nose radius compensation 1 : Displays the programmed position
Signal
Drawing signal CKGRP <F164#5>
Signal address
Parameter
B–61393E–2/02 12. DISPLAY/SETTING/EDIT
649
#7 0046
#6 #5 GRPOS
#4 #3 #2 #1 #0
[Data type] Bit
GRPOS Current position on the graphic display screen 0 : Not appear 1 : Appears
#7 0047
#6 #5 #4 #3 #2 #1 SP2C
#0 (0–TTC)
[Data type] Bit
SP2C Graphic display (0–TTC) is done 0 : on two spindles and two tool posts 1 : on one spindle and two tool posts
#7 0058
#6 #5 SGCSR
#4 SGFIN
#3 SGPLN
#2 SG3PL
#1 SGTLC
#0 SGORG (M series)
[Data type] Bit
SGORG Movement when coordinate system is altered during drawing 0 : Draws in the same coordinate system 1 : Draws in the new coordinate system (only for the path drawing)
SGTLC In solid drawing 0 : Not compensate the tool length 1 : Compensates the tool length
SG3PL Tri–plane drawing in solid drawing 0 : Drawn by the first angle projection 1 : Drawn by the third angle projection
SGPLN In solid drawing 0 : Draws a plane without edges. 1 : Draws a plane with edges.
SGFIN Machining profile drawing in solid drawing 0 : Displayed in the coarse mode 1 : Displayed in the fine mode
SGCSR While the screen image is enlarged, the shape of the graphic cursor is: 0 : A square. (�) 1 : An X. (�)
12. DISPLAY/SETTING/EDIT B–61393E–2/02
650
0123 Coordinate system for drawing (0–TTC)
[Data type] Byte
[Valid data range] 0 to 5
The following shows the relationship between the settings and the drawing coordinate systems:
Z
X1X2
X1
X2
Z
X1
X2
Z
(0) (1) (2)
Z
X1X2
X1
X2
Z
X1
X2
Z
(3) (4) (5)
B–61393E–2/02 12. DISPLAY/SETTING/EDIT
651
0123 Coordinate system for drawing (T series)
[Data type] Byte
[Valid data range] 0 to 7
This parameter specifies the drawing coordinate system for the graphic function.
The following show the relationship between the set values and the drawing coordinate systems.
X
Z
Z
Z
Z
Z
Z
Z
Z
X
X
X
X
X
X
X
Set value = 0 Set value = 1 Set value = 2 Set value = 3
Set value = 4 Set value = 5 Set value = 6 Set value = 7
NOTE This parameter is specified for each tool post in the 0–TTC. A different drawing coordinate system can be selected for each tool post.
0253 Change in cross–section position in tri–plane drawing (M series)
[Data type] Byte
[Unit of data] Dot
[Valid data range] 0 to 10
This parameter sets the change in the cross–section position when a soft key is continuously pressed in tri–plane drawing. When zero is specified, it is set to 1.
12. DISPLAY/SETTING/EDIT B–61393E–2/02
652
0589 Right margin in solid drawing (M series)
0590 Left margin in solid drawing (M series)
0591 Upper margin in solid drawing (M series)
0592 Lower margin in solid drawing (M series)
[Data type] Word
[Unit of data] Dot
These parameters set the machining profile drawing position in margins on the CRT screen. The unit is a dot.
Standard set value
Parameter No.
Margin area
GRPOS (No.0046#5) is 0 GRPOS (No.0046#5) is 1
9” CRT 14” CRT 9” CRT 14” CRT
0589 Right 0 0 200 100
0590 Left 0 0 0 0
0591 Upper 25 32 25 32
0592 Lower 0 10 0 10
NOTE When the dynamic graphics function is used, the graphics function cannot be used. (M series)
OPERATOR’S MANUAL (For Machining Center)
III.12.1 GRAPHICS DISPLAY (For Machining Center) (B–61404E) III.12.2 DYNAMIC GRAPHIC DISPLAY
OPERATOR’S MANUAL (For Lathe) (B–61394E)
III.12.1 GRAPHICS DISPLAY
Note
Reference item
B–61393E–2/02 12. DISPLAY/SETTING/EDIT
653
The reading on the load meter can be displayed for each servo axis and the serial spindle.
The reading on the load meter can be displayed for servo axes.
When serial spindles are used, the reading on the load meter and speedometer can be displayed.
Although the speedometer normally indicates the speed of the spindle motor.
#7 0060
#6 #5 OPMNDP
#4 #3 #2 #1 #0
[Data type] Bit
OPMNDP Operating monitor 0 : Not displayed 1 : Displayed
6627 Load meter displayed value for maximum output
[Data type] Word
8x86 Rated current parameter (RTCURR)
[Data type] Word
NOTE The reading on the load meter depends on servo parameter 8x86 and spindle parameter 6627. These parameters are set by the automatic setting.
OPERATOR’S MANUAL (For Machining Center) (B–61404E)
III.11.1.6 Operating Monitor Display
OPERATOR’S MANUAL (For Lathe) (B–61394E)
III.11.1.6 Operating Monitor Display
12.1.9 Operating Monitor Display
General
� Display of the servo axes
� Display of the spindle axes
� Speedometer
Parameter
Note
Reference item
12. DISPLAY/SETTING/EDIT B–61393E–2/02
654
The software operator’s panel function replaces part of the control switches on the machine operator’s panel with soft switches which can be turned on or off using the CRT/MDI of the control unit.
The control switches for the functions listed in the following table can be replaced with soft switches. Also available are eight general–purpose soft switches which can be used additionally by the machine tool builder. These eight general–purpose soft switches can be optionally named by the machine tool builder. For control switches in groups 1 to 7, parameter (No.0017) can be used to select whether the control switches on the machine operator‘s panel or soft switches on the CRT/MDI of the control unit are used for each group.
Group1 :Mode selection
Group2 :Selection of jog feed axis, manual rapid traverse
Group3 :Selection of manual pulse generator feed axis, selection of manual pulse magnification
Group4 :Jog feedrate, feedrate override, rapid traverse override
Group5 :Optional block skip, single block, machine lock, dry run
Group6 :Protect key
Group7 :Feed hold
Group8 :General purpose
The states of all soft switches are informed to the PMC by output signals. Based on these output signals, the PMC should turn “1” or “0” input signals related to soft switch functions. In other words, turning “1” the soft switch assigned to single block operation, for example, does not cause the control unit to select single block operation internally. Single block operation is selected when the PMC turns to “1” the input signal for single block operation, instead.
12.1.10 Software Operator’s Panel
General
B–61393E–2/02 12. DISPLAY/SETTING/EDIT
655
Group Function Output signal Related input signal
1 Mode selection MD1O<F174#0> MD2O<F174#1> MD4O<F174#2> ZRNO<F174#3>
MD1 MD2 MD4 ZRN
2 Jog feed axis se- lect
+XO to +4O –XO to –4O <F177>
+X to +4 –X to –4
Manual rapid tra- verse
RTO<F178#6> RT
3 Handle feed HXO to H4O <F174#4 to #7>
HX HY HZ H4
Handle feed mag- nification
MP1O<F175#6> MP2O<F175#7>
MP1 MP2
4 Jog feed rate over- ride
JV1O to JV8O <F175#0 to 3>
*OV1 to *OV8
Feed rate override OV1O to OV8O <F176#0 to 3>
*OV1 to *OV8
Rapid traverse override
ROV1O<F175#4> ROV2O<F175#5>
ROV1 ROV2
5 Optional block skip BDTO<F176#4> BDT
Single block SBKO<F176#5> SBK
Machine lock MLKO<F176#6> MLK
Dryrun DRNO<F176#7> DRN
6 Protect key KEYO<F178#5> KEY
7 Feed hold SPO<F178#7> *SP
8 General purpose (Switch from 1st line to the 8th line on CRT)
OUT0 to OUT7 <F171>
Signal
12. DISPLAY/SETTING/EDIT B–61393E–2/02
656
#7 OUT7F171
#6 OUT6
#5 OUT5
#4 OUT4
#3 OUT3
#2 OUT2
#1 OUT1
#0 OUT0
H4OF174 H3O HZO HXO ZRNO MD4O MD2O MD1O (T series)
H4OF174 HZO HYO HXO ZRNO MD4O MD2O MD1O (M series)
MP2OF175 MP1O ROV2O ROV1O JV8O JV4O JV2O JV1O
DRNOF176 MLKO SBKO BDTO OV8O OV4O OV2O OV1O
–4OF177 +4O –3O +3O –ZO +ZO –XO +XO (T series)
–4OF177 +4O –ZO +ZO –YO +YO –XO +XO (M series)
SPOF178 RTO KEYO
#7 0017
#6 OP7
#5 OP6
#4 OP5
#3 OP4
#2 OP3
#1 OP2
#0 OP1
[Data type] Bit
OP1 Mode selection on software operator’s panel 0 : Not performed 1 : Performed
OP2 JOG feed axis select and manual continous rapid traverse buttons on software operator’s panel 0 : Not performed 1 : Performed
OP3 Manual pulse generator’s axis select and manual pulse generator’s magnification switches on software operator’s panel 0 : Not performed 1 : Performed
OP4 Jog feedrate override, feedrate override, and rapid traverse override switches on software operator’s panel 0 : Not performed 1 : Performed
OP5 Optional block skip, single block, machine lock, and dry run switches on software operator’s panel 0 : Not performed 1 : Performed
OP6 Protect key on software operator’s panel 0 : Not performed 1 : Performed
OP7 Feed hold on software operator’s panel 0 : Not performed 1 : Performed
Signal address
Parameter
Arrow keys on the CRT/MDI panel
� �
���
� � �
B–61393E–2/02 12. DISPLAY/SETTING/EDIT
657
0130 Jog–movement axis and its direction on software operator’s panel [↑ ]
0131 Jog–movement axis and its direction on software operator’s panel [↓ ]
0132 Jog–movement axis and its direction on software operator’s panel [→]
0133 Jog–movement axis and its direction on software operator’s panel [←]
0134 Jog–movement axis and its direction on software operator’s panel [ ]
0135 Jog–movement axis and its direction on software operator’s panel [ ]
0136 Jog–movement axis and its direction on software operator’s panel [ ]
0137 Jog–movement axis and its direction on software operator’s panel [ ]
[Data type] Byte
[Valid data range] 0 to 8
On software operator’s panel, set a feed axis corresponding to an arrow key on the CRT/MDI panel when jog feed is performed.
Set value Feed axis and direction
0 Not moved
1 First axis, positive direction
2 First axis, negative direction
3 Second axis, positive direction
4 Second axis, negative direction
5 Third axis, positive direction
6 Third axis, negative direction
7 Fourth axis, positive direction
8 Fourth axis, negative direction
(Example) Under X, Y, and Z axis configuration, to set arrow keys to feed the axes in the direction specified as follows, set the parameters to the values given below. [8 �] to the positive direction of the Z axis, [2 �] to the negative direction of the Z axis, [6�] to the positive direction of the X axis [4�] to the negative direction of the X axis, [1�] to the positive direction of the Y axis, [9�] to the negative direction of the Y axis
Parameter No.0130 = 5 (Z axis, positive direction)
Parameter No.0131 = 6 (Z axis, negative direction)
Parameter No.0132 = 1 (X axis, positive direction)
Parameter No.0133 = 2 (X axis, negative direction)
Parameter No.0134 = 3 (Y axis, positive direction)
Parameter No.0135 = 4 (Y axis, negative direction)
Parameter No.0136 = 0 (Not used)
Parameter No.0137 = 0 (Not used)
12. DISPLAY/SETTING/EDIT B–61393E–2/02
658
0140 Name of general–purpose switch on software operator’s panel
0203 Name of general–purpose switch on software operator’s panel
[Data type] Byte
(Exapmle)
These parameters set the names of the gen- eral–purpose switches (SIGNAL 1 through SIGNAL 8) on the software operator ’s panel as described be- low.

Parameter No.0140: Sets the character code (083) corresponding to S of SIGNAL 1.
Parameter No.0141: Sets the character code (073) corresponding to I of SIGNAL 1.
Parameter No.0142: Sets the character code (071) corresponding to G of SIGNAL 1.
Parameter No.0143: Sets the character code (078) corresponding to N of SIGNAL 1.
Parameter No.0144: Sets the character code (065) corresponding to A of SIGNAL 1.
Parameter No.0145: Sets the character code (076) corresponding to L of SIGNAL 1.
Parameter No.0146: Sets the character code (032) corresponding to (space) of SIGNAL 1.
Parameter No.0147: Sets the character code (049) corresponding to 1 of SIGNAL 1.
Parameter Nos.0148 to 0155: Set the character codes of SIGNAL 2 shown in the figure above.
Parameter Nos.0156 to 0163: Set the character codes of SIGNAL 3 shown in the figure above.
Parameter Nos.0164 to 0171: Set the character codes of SIGNAL 4 shown in the figure above.
Parameter Nos.0172 to 0179: Set the character codes of SIGNAL 5 shown in the figure above.
Parameter Nos.0180 to 0187: Set the character codes of SIGNAL 6 shown in the figure above.
Parameter Nos.0188 to 0195: Set the character codes of SIGNAL 7 shown in the figure above.
B–61393E–2/02 12. DISPLAY/SETTING/EDIT
659
Parameter Nos.0196 to 0203: Set the character codes of SIGNAL 8 shown in the figure above.
The character codes are shown in character code list on the following page.
Character to Code Correspondence Table
Char- acter Code Comment
Char- acter Code Comment
A 065 6 054
B 066 7 055
C 067 8 056
D 068 9 057
E 069 032 Space
F 070 ! 033 Exclamation mark
G 071 ” 034 Quotation marks
H 072 # 035 Sharpe
I 073 $ 036 Dollar mark
J 074 % 037 Percent
K 075 & 038 Ampersand
L 076 ’ 039 Apostrophe
M 077 ( 040 Left parenthesis
N 078 ) 041 Right parenthesis
O 079 * 042 Asterisk
P 080 + 043 Positive sign
Q 081 , 044 Comma
R 082 – 045 Negative sign
S 083 . 046 Period
T 084 / 047 Slash
U 085 : 058 Colon
V 086 ; 059 Semicolon
W 087 < 060 Left angle bracket
X 088 = 061 Equal sign
Y 089 > 062 Right angle bracket
Z 090 ? 063 Question mark
0 048 @ 064 Commercial at mark
1 049 [ 091 Left square bracket
2 050 ^ 092
3 051 ¥ 093 Yen mark
4 052 ] 094 Right square bracket
5 053 _ 095 Underline
12. DISPLAY/SETTING/EDIT B–61393E–2/02
660
NOTE 1 Only the modes shown below can be selected by soft
switches. When the mode for DNC operation is to be equipped, for example, all control switches for mode selection should be on the machine operator’s panel or a general–purpose soft switch should be used to select the mode for DNC operation. Soft switches available for mode selection ⋅ Manual data input ⋅ Automatic operation ⋅ Memory edit ⋅ Manual handle feed / incremental feed ⋅ Jog feed ⋅ Manual reference position return
2 When the soft switch for feed hold is turned on, output signal SPO is turned to “1”. At this time, the PMC turns feed hold signal *SP to “0”. In contrast to the above, when the soft switch for feed hold is turned off, output signal SPO is turned “0” and the PMC turns signal *SP to “1”. For soft switches other than feed hold and general soft switches, when an output signal informing the state of a soft switch is turned to “1”, the corresponding input signal is turned to “1”.
OPERATOR’S MANUAL (For Machining Center) (B–61404E)
III.11.6.2 Displaying and Setting the Soft- ware Operator’s Panel
OPERATOR’S MANUAL (For Lathe) (B–61394E)
III.11.6.2 Displaying and Setting the Soft- ware Operator’s Panel
Note
Reference item
B–61393E–2/02 12. DISPLAY/SETTING/EDIT
661
The CRT or LCD screens are displayed in a parameter–set language.
#7 0023
#6 DSPN
#5 DHNG
#4 DITA
#3 DCHI
#2 DFRN
#1 DGRM
#0 DJPN
[Data type] Bit type
NOTE When this parameter is set, turn off the power once.
The language used in the display on the CRT is selected.
DSPN DHNG DITA DCHI DFRN DGRM DJPN CRT display language
0 0 0 0 0 0 0 English
0 0 0 0 0 0 1 Japanese
0 0 0 0 0 1 0 German
0 0 0 0 1 0 0 French
0 0 0 1 0 0 0 Chinese (Taiwanese)
0 0 1 0 0 0 0 Italian
0 1 0 0 0 0 0 Hangul
1 0 0 0 0 0 0 Spanish
12.1.11 Multi–language Display
General
Parameter
12. DISPLAY/SETTING/EDIT B–61393E–2/02
662
One of the following part program length.
M series (m) 10 20 40 80 120 320
T series (m) 10 20 40 80 120 320
������ Message Description
070 NO PROGRAM SPACE IN MEMORY
The memory area is insufficient. Delete any unnecessary programs, then retry.
OPERATOR’S MANUAL (For Machining Center) (B–61404E)
III.11.3.1 Displaying Memory Used and a List of Programs
OPERATOR’S MANUAL (For Lathe) (B–61394E)
III.11.3.1 Displaying Memory Used and a List of Programs
One of the following no. of registered programs can be selected. 63/125/200.
������ Message Description
072 TOO MANY PROGRAMS The number of programs to be stored exceeded 63 (basic), 125 (option), or 200 (option). Delete unnecessary programs and execute program registeration again.
12.2 EDIT
12.2.1 Part Program Storage Length
General
Alarm and message
Reference item
12.2.2 No. of Registered Programs
General
Alarm and message
B–61393E–2/02 12. DISPLAY/SETTING/EDIT
663
OPERATOR’S MANUAL (For Machining Center) (B–61404E)
III.11.3.1 Displaying Memory Used and a List of Programs
OPERATOR’S MANUAL (For Lathe) (B–61394E)
III.11.3.1 Displaying Memory Used and a List of Programs
A key called the data protection key is used to prevent part programs from being registered or deleted erroneously.
[Classification] Input signal
[Operation] When a signal is set to 0, the associated operations are disabled. When a signal is set to 1, the associated operations are enabled.
#7 G122
#6 #5 #4 #3 KEY
#2 #1 #0
OPERATOR’S MANUAL (For Machining Center) (B–61404E)
III.11 SETTING AND DISPLAYING DATA
OPERATOR’S MANUAL (For Lathe) (B–61394E)
III.11 SETTING AND DISPLAYING DATA
Reference item
12.2.3 Memory Protection Key
General
Signal
Memory protection signal KEY<G122#3>
Signal address
Reference item
12. DISPLAY/SETTING/EDIT B–61393E–2/02
664
The password function locks PRG9 (bit 4 of parameter No.0010), used to protect program Nos. 9000 to 9999, by using the PASSWD (No.0797) and KEYWD (No.0798) parameters. When PRG9 is locked, PRG9 cannot be set to 0. Therefore, the protection for programs numbered 9000 to 9999 cannot be released unless the correct keyword is entered.
PRG9 is locked when different values are set in the PASSWD and KEYWD parameters. The values set in the two parameters are not displayed. NE9 is unlocked when the value preset in the PASSWD parameter is set in the KEYWD parameter.
#7 0010
#6 #5 #4 PRG9
#3 #2 #1 #0
[Data type] Bit
PRG9 Editing of subprograms with program numbers 9000 to 9999 0 : Not inhibited 1 : Inhibited
The following edit operations are disabled:
(1)Program deletion (Even when deletion of all programs is specified, programs with program numbers 9000 to 9999 are not deleted.)
(2)Program output (Even when outputting all programs is specified, programs with program numbers 9000 to 9999 are not output.)
(3)Program number search
(4)Program editing after registration
(5)Program registration
(6)Program collation
(7)Displaying programs
0797 Password(PASSWD)
[Data type] Two–word
Set a secret number to this parameter. Its value is not displayed.
CAUTION Once a key is lock, parameter PRG9 cannot become 0 and PASSWD cannot be changed unless you perform an unlock operation or perform the memory all clear operation. Special care should be exercised when setting the PASSWD parameter.
12.2.4 Password Function
General
Parameter
B–61393E–2/02 12. DISPLAY/SETTING/EDIT
665
0798 Keyword(KEYWD)
[Data type] Two–word
When the value set as the password (set in parameter No. 0797) is set to this parameter, the locked state is released and the user can now modify the password and the value set in bit 4 (PRG9) of parameter No. 0010 becomes 0.
NOTE The value set in this parameter is not displayed. When the power is turned off, this parameter is set to 0.
Editing a program while executing another program is called background editing. The method of editing is the same as for ordinary editing (foreground editing). A program edited in the background should be registered in foreground program memory. During background editing, all programs cannot be deleted at once.
������ Message Description
??? BP/S alarm BP/S alarm occurs in the same num- ber as the P/S alarm that occurs in or- dinary program edit. (070, 071, 072, 073, 074, 085,086,087, and etc.)
140 BP/S alarm It was attempted to select or delete in the background a program being se- lected in the foreground. Use background editing correctly.
NOTE Alarm in background edit is displayed in the key input line of the background edit screen instead of the ordinary alarm screen and is resettable by any of the MDI key operation.
OPERATOR’S MANUAL (For Machining Center) (B–61404E)
III.9.7 BACKGROUND EDITING
OPERATOR’S MANUAL (For Lathe) (B–61394E)
III.9.7 BACKGROUND EDITING
12.2.5 Background Editing
General
Alarm and message
Reference item
12. DISPLAY/SETTING/EDIT B–61393E–2/02
666
When the playback option is selected, the TEACH IN JOG mode (TJOG) and TEACH IN HANDLE mode (THND) are added. In these modes, a machine position along the X, Y, and Z axes obtained by manual operation is stored in memory as a program position to create a program. The words other than X, Y, and Z, which include O, N, G, R, F, M, S, T, P, Q, and EOB, can be stored in memory in the same way as in EDIT mode.
#7 0002
#6 TJHD
#5 #4 #3 #2 #1 #0
[Data type] Bit
TJHD Manual pulse generator in TEACH IN JOG mode 0 : Valid 1 : Invalid
OPERATOR’S MANUAL (For Machining Center) (B–61404E)
III.10.3 CREATING PROGRAMS IN TEACH IN MODE
OPERATOR’S MANUAL (For Lathe) (B–61394E)
III.10.3 CREATING PROGRAMS IN TEACH IN MODE
CONNECTION MANUAL (This manual)
2.6 MODE SELECTION
12.2.6 Playback
General
Parameter
Reference item
B–61393E–2/02 12. DISPLAY/SETTING/EDIT
667
Programs can be created block after block on the conversational screen while displaying the G code menu. Blocks in a program can be modified, inserted, or deleted using the G code menu and converstional screen.
OPERATOR’S MANUAL (For Machining Center) (B–61404E)
III.10.5 CONVERSATIONAL PROGRAM- MING WITH GRAPHIC FUNC- TION
OPERATOR’S MANUAL (For Lathe) (B–61394E)
III.10.5 CONVERSATIONAL PROGRAM- MING WITH GRAPHIC FUNC- TION
12.2.7 Conversational Programming with Graphic Function
General
Reference item
13 INPUT/OUTPUT OF DATA B–61393E–2/02
668
13 INPUT/OUTPUT OF DATA
B–61393E–2/02 13 INPUT/OUTPUT OF DATA
669
The data shown below can be input/output through reader/puncher interface.
1. Program
2. Offset data
3. Parameter
4. Custom macro common variables.
5. PMC D area data
This CNC has four channels of input/output device interfaces. The input/output device to be used is specified by setting the channel connected to that device in setting parameter I/O. The specified data, such as a baud rate and the number of stop bits, of an input/output device connected to a specific channel must be set in parameters for that channel in advance. For channel 1, two combinations of parameters to specify the input/output device data are provided. The following shows the interrelation between the input/output device interface parameters for the channels.
Stop bit and other data
Number specified for the input/output device
Baud rate
Stop bit and other data
Number specified for the input/output device
Baud rate
I/O =0 : Channel 1
=1 : Channel 1
=2 : Channel 2
=3 : Channel 3
Specify a channel for
an input/output device.
I/O =1
(channel 1)
I/O 0002#0
0038#6, #7I/O =0
(channel 1) 0552
0012#0
0038#6, #7
0553
Input/output channel number
↓
I/O =3
(channel 3)
* Remote buffer
0050#0
0038#4, #5I/O =2
(channel 2) 0250
0051#0
0038#1, #2
0251
0055#2
0055#3
Stop bit and other data
Number specified for the input/output device
Baud rate
Stop bit and other data
Number specified for the input/output device
Baud rate
Selection of protocol
Selection of RS–422 or RS–232C, and other data
13.1 READER/PUNCHER INTERFACE
General
Parameter
13 INPUT/OUTPUT OF DATA B–61393E–2/02
670
Setting entry TVON TV check
0 : Not performed 1 : Performed
ISO Code used for data output 0 : EIA code 1 : ISO code
MAIN CPU BOARD Remote buffer BOARD
CNC
I/ O =0
or
I/ O =1
Channel 1
RS–232–C
Channel 3Channel 2
RS–232–C RS–232–C RS–422
ÂÂÂÂÂ ÂÂÂÂÂ
Reader/puncher ÂÂÂÂÂ ÂÂÂÂÂ
Reader/puncher ÂÂÂÂÂÂ ÂÂÂÂÂÂ
Host computer ÂÂÂÂÂ ÂÂÂÂÂ
Host computer
I/ O =3I/ O =3I/ O =2
(1) Parameters common to all channels #7
0018 #6
TVC #5 #4 #3 #2 #1 #0
[Data type] Bit TVC Character counting for TV check in the comment section of a program.
0 : Performed 1 : Not performed
#7 ICR0070
#6 #5 #4 #3 #2 #1 #0
[Data type] Bit
ICR Output of the end of block (EOB) in ISO code 0 : LF, CR, CR are output. 1 : Only LF is output.
#7 IONUL0075
#6 #5 #4 #3 #2 #1 #0
[Data type] Bit
IONUL Action taken when a NULL code is found during read of EIA code 0 : An alarm is generated. 1: The NULL code is ignored.
B–61393E–2/02 13 INPUT/OUTPUT OF DATA
671
(2) Parameters for channel 1 (I/O =0) #7
NFED0002 #6 #5 #4 #3
RSASCI #2 #1 #0
STP2
[Data type] Bit
STP2 The number of stop bits 0 : 1 1 : 2
RSASCI Code used at data input 0 : EIA or ISO code (automatically distinguished) 1 : ASCII code
NFED Feed before and after the data at data output 0 : Output 1 : Not output
NOTE When input/output devices other than the FANUC PPR are used, set NFED to 1.
#7 RSCMD10038
#6 DEVFL1
#5 RSCMD2
#4 DEVFL2
#3 #2 RSCMD3
#1 DEVFL3
#0
[Data type] Bit
Set the specification of the input/output device for I/O = 0, using the values shown in Table 13.1 (a).
Table 13.1 (a)
(I/O=0, 1, or 2) (I/O=3)
RSCMD* DEVFL* I/O device used RSCMD3 DEVFL3 I/O device used
0 0 Bubble cassette 0 0 Bubble cassette
0 1 Floppy cassette 0 1 Floppy cassette
1 0 RS232C, PPR 1 0 Portable tape reader, etc.
1 1 New type inter- face
1 1 Portable tape reader, etc.
13 INPUT/OUTPUT OF DATA B–61393E–2/02
672
0552 Baud rate (when the I/O is set to 0)
[Data type] Byte
Set baud rate of the input/output device used when the I/O is set to 0, with a set value in Table 13.1 (b).
Table 13.1 (b)
Set value Baud rate (bps)
1
2
3
4
5
6
Set value Baud rate (bps)
7
8
9
600
1200
2400
10 4800
960011
50
100
110
150
200
300 (19200)(12) *
* : I/O channel 3 or 2
(3) Parameters for channel 1 (I/O =1) #7
NFED0012 #6 #5 #4 #3
RSASCI #2 #1 #0
STP2
[Data type] Bit
These parameters are used when I/O is set to 1. The meanings of the bits are the same as for parameter 0002.
#7 RSCMD10038
#6 DEVFL1
#5 #4 #3 #2 #1 #0
[Data type] Bit
Set the number specified for the input/output device used when the I/O is set to 1, with one of the set values listed in Table 13.1 (a).
0553 Baud rate (when I/O is set to 1)
[Data type] Byte
Set the baud rate of the input/output device used when I/O CHANNEL is set to 1, with a value in Table 13.1 (b).
(4) Parameters for channel 2 (I/O =2) #7
0038 #6 #5
RSCMD2
#4 DEVFL2
#3 #2 #1 #0
[Data type] Bit
Set the number specified for the input/output device used when I/O is set to 2, with a value in Table 13.1 (a).
B–61393E–2/02 13 INPUT/OUTPUT OF DATA
673
#7 NFED0050
#6 #5 #4 #3 RSASCI
#2 #1 #0 STP2
[Data type] Bit
These parameters are used when I/O is set to 2. The meanings of the bits are the same as for parameter 0002.
0250 Baud rate (when the I/O is set to 2)
[Data type] Byte
Set the baud rate of the input/output device used when I/O CHANNEL is set to 2, with a value in Table 13.1 (b).
������ Message Description
001 TH PARITY ALARM TH alarm (A character with incorrect parity was input). Correct the tape.
002 TV PARITY ALARM TV alarm (The number of characters in a block is odd). This alarm will be generated only when the TV check is effective.
085 COMMUNICATION ER- ROR
When entering data in the memory by using Reader / Puncher interface, an overrun, parity or framing error was generated. The number of bits of input data or setting of baud rate or specifi- cation No. of I/O unit is incorrect.
086 DR SIGNAL OFF When entering data in the memory by using Reader / Puncher interface, the ready signal (DR) of reader / puncher was turned off. Power supply of I/O unit is off or cable is not connected or a P.C.B. is defec- tive.
087 BUFFER OVERFLOW When entering data in the memory by using Reader / Puncher interface, though the read terminate command is specified, input is not interrupted after 10 characters read. I/O unit or P.C.B. is defective.
OPERATOR’S MANUAL (For Machining Center) (B–61404E)
III.8 DATA INPUT/OUTPUT
OPERATOR’S MANUAL (For Lathe) (B–61394E)
III.8 DATA INPUT/OUTPUT
Alarm and message
Reference item
13 INPUT/OUTPUT OF DATA B–61393E–2/02
674
Refer to Descriptions (B–61392EN–1) for Remote Buffer for detailed informetion of remote buffer.
13.2 REMOTE BUFFER
B–61393E–2/02 13 INPUT/OUTPUT OF DATA
675
Refer to FANUC DNC1 DESCRIPTIONS(B–61782E) for detailed information of DNC1 interface.
� Setting entry An input/output unit is selected at I/O on the setting screen. Setting value 10
0251 Baud rate
[Data type] Byte
The baud rate of HDLC is fixed to 460 kbps for DNC1. Set following value:
Set value. :51
NOTE When this parameter is set, the power must be turned off before operation is continued.
0347 System for connection between the CNC and host (DNC1 interface)
[Data type] Byte
[Valid data range] 1 or 2
This parameter specifies the system for connection (DNC1 interface) between the CNC and host.
Set value
1 : Point–to–point connection
2 : Multipoint connection
NOTE When this parameter is set, the power must be turned off before operation is continued.
13.3 DNC1 INTERFACE
General
Parameter
13 INPUT/OUTPUT OF DATA B–61393E–2/02
676
0348 Station address of the CNC (DNC1 interface)
[Data type] Byte
[Valid data range] 2 to 52
This parameter specifies the station address of the CNC when the CNC is connected via the DNC1 interface using multipoint connection.
NOTE When this parameter is set, the power must be turned off before operation is continued.
(SETTING)
DNC FILE SELECTION
The parameter is used to specify a file name for a part program used in DNC operation.
Format: OXXXX.PRG (where XXXX is a four–digit number)
(1) Full keypad
1. Press the rightmost soft key .
* Skip this step if the [STRING] soft key has already appeared.
2. Press the [STRING] soft key.
3. Specify a file name using the MDI panel keys.
4. Assert the entry using the INPUT key.
(Example) To specify O0100:
Key in ”O0100.PRG” using the MDI panel keys, then press INPUT .
(2) Standard keypad
1. Press the rightmost soft key .
* Skip this step if the [CODE] soft key has already appeared.
2. Press the [CODE] soft key.
(SETTING)
DNC FILE SELECTION
↑
The cursor moves to here.
3. Specify a file name in ASCII code using numeric keys.
4. Assert the entry using the INPUT key.
5. Pressing again moves the cursor back to the previous position and cancels the code entry.
MAP parameter description
Setting method
B–61393E–2/02 13 INPUT/OUTPUT OF DATA
677
MAP PARAMETER O0001 N0001
(SETTING)
DNC FILE SELECTION
NUM. MDI
[ PARAM ][ DGNOS ][ MAP ][ ][ ]
[ STRING ][ CODE ][ CLEAR ][VRFY.H][ VRFY ]
[ ][ ][ ][INS.CH][ DEL.CH ]
[STRING] is not displayed with the standard keypad.
NC APPLICATION NAME
NC APPLICATION PASS WORD
MAX MESSAGE LENGTH
MAX INVOKES
DNC1 does not use these items.
MAP PARAMETER O0001 N0001
NC APPLICATION NAME
NC APPLICATION PASS WORD 0
MAX MESSAGE LENGTH 0
MAX INVOKES
NUM. MDI
[ PARAM ][ DGNOS ][ MAP ][ ][ ]
13 INPUT/OUTPUT OF DATA B–61393E–2/02
678
HOST APPLICATION NAME
HOST APPLICATION INSTACE
HOST APPLICATION PASSWORD
DNC1 does not use these items.
MAP PARAMETER O0001 N0001
HOST APPLICATION NAME
HOST APPLICATION INSTACE 0
HOST APPLICATION PASSWORD
NUM. MDI
[ PARAM ][ DGNOS ][ MAP ][ ][ ]
INFORMATION REPORT ENABLE
RISING EDGE 00000000 00000000 FALLING EDGE 00000000 00000000
With these parameters, it is necessary to set the bit information needed when the status information in the CNC is sent to DNC1 at a local request.
The CNC status information consists of the following bit pattern, and corresponds to the RISING EDGE and FALLING EDGE bit parameters. If the bit is 0, it specifies that the information be masked. If the bit is 1, it specifies that the information be sent to DNC1.
RISING EDGE means that when the status information bit changes from 0 to 1, the change is reported.
FALLING EDGE means that when the status information bit changes from 1 to 0, the change is reported.
CNC status information bit pattern configuration
15 14 13 12 11 10 09 08 07 06 05 04 03 02 01 00
Bit position:signal name Description
00 : RWD Rewind signal
01 : AL Alarm output signal
02 : RST Reset in progress signal
03 : SPL Automatic operation at pause signal
04 : STL Automatic operation being started signal
05 : OP Automatic operation in progress signal
06 : SA Servo ready
07 : MA CNC ready
08 : Not used
09 : Not used
B–61393E–2/02 13 INPUT/OUTPUT OF DATA
679
10 : Not used
11 : Not used
12 : M00 M00 decode output signal (*)
13 : M01 M01 decode output signal (*)
14 : M02 M02 decode output signal (*)
15 : M30 M30 decode output signal (*)
* Signals for the 0–TTC
#08 to #11 correspond to M00 to M30 for HEAD2.
#12 to #15 correspond to M00 to M30 for HEAD1.
MAP PARAMETER O0001 N0001
INFORMATION REPORT ENABLE RISING EDGE 00000000 00000000 FALLING EDGE 00000000 00000000
ALARM NOTIFICATION ENABLE UPPER WORD 00000000 00000000 LOWER WORD 00000000 00000000
NUM. MDI
[ PARAM ][ DGNOS ][ MAP ][ ][ ]
ALARM NOTIFICATION ENABLE
UPPER WORD 00000000 00000000 LOWER WORD 00000000 00000000
The parameter is used to specify an alarm type that causes the CNC to inform the host of the CNC status change that is induced by the alarm.
Setting value
0: The occurrence of the alarm does not trigger notification by the CNC.
1: The occurrence of the alarm triggers notification by the CNC.
The parameter bits correspond to each alarm type as listed below.
Upper word bit parameter
15 14 13 12 11 10 09 08 07 06 05 04 03 02 01 00
Bit position Alarm type
01 : P/S alarm
02 : Overheat alarm
05 : P/S 100 alarm
06 : Overtravel
12 : Servo alarm
13 : P/S 101 alarm
14 : P/S 000 alarm
13 INPUT/OUTPUT OF DATA B–61393E–2/02
680
Lower word bit parameter
15 14 13 12 11 10 09 08 07 06 05 04 03 02 01 00
00 : Battery alarm
MAC PRINT FILE → Not used by DNC1. LOGGING MODE → Not used by DNC1.
00000000 00000000
MAP SERVICE MODE→ Not used by DNC1. 00000000 00000000
NC SERVICE MODE → Not used by DNC1. 00000000 00000000
This parameter specifies the behavior of the all–file directory information read function of the CNC as follows:
00000000 00000001 : Only the file number is read.
00000000 00000001 : Both the file number and size are read.
MAP PARAMETER O0001 N0001
MAC PRINT FILE
LOGGING MODE 00000000 00000000
MAP SERVIEC MODE 00000000 00000000
NC SERVIEC MODE 00000000 00000000
NUM. MDI
[ PARAM ][ DGNOS ][ MAP ][ ][ ]
MAP LOG MESSAGE O0001 N0001
NUM. MDI
[ ALARM ][ MSG ][MAPMSG][ ][ ]
Not used with the DNC1 function
MAP LOG MESSAGE screen
B–61393E–2/02 13 INPUT/OUTPUT OF DATA
681
Refer to an item of FANUC DNC2 DESCRIPTIONS (B–61992E) for detailed information of DNC2 interface.
13.4 DNC2 INTERFACE
13 INPUT/OUTPUT OF DATA B–61393E–2/02
682
It is possible to request from the outside that a program be registered, collated, or output.
� Registeration/Collation As triggered by the external read start signal EXRD, the background edit function saves programs from an external input unit onto tape and verifies them.
� Output As triggered by the external punch start signal EXWT, the background edit function outputs all programs stored in the part program memory to an external output device.
[Classification] Input signal
[Function] Programs are registered through the reader/punch interface or remote buffer. Or the read programs are collated with programs already stored in the part program memory.
[Operation] When this signal becomes logical 1, the CNC operates as follows: � In all modes other than the MDI mode, the background edit function
reads programs from an external input device, and register them on the part program memory or collates them with programs already registered in the part program memory. (The memory protection key KEY<G122#3> determines whether to register or collate.)
� Bit 1 (RAL) of parameter No.0045 selects whether to register all programs in a file or one program at a time. Bit 0 (RDL) of parameter No.0045 can be used to delete all programs previously stored in the part program memory. However, it is impossible to delete programs protected by bit 4 (PRG9) of parameter No.0010 and bit 2 (PRG8) of parameter No.0389.
� When programs are being registed or collated, the read/punch busy signal (RPBSY) is kept to be logical 1.
� When the background processing–activated signal BGEACT is logical 1 (for example, during background editing or MDI mode), the external read start signal EXRD is ignored.
� When programs are being registered or collated, if the system is reset or the external read/punch stop signal EXSTP becomes logical 1, the registeration or collation is discontinued.
� If the foreground processing is already using the reader/punch interface (for example, during DNC operation or program reading in the edit mode), the external read start signal EXRD is ignored.
13.5 EXTERNAL I/O DEVICE CONTROL
General
Signal
External read start signal EXRD<G134#1>
B–61393E–2/02 13 INPUT/OUTPUT OF DATA
683
� There are some other conditions to determine whether a program can be registered or collated. For example, a program cannot be registered or collated, if a program with the same program number is being executed in the foreground processing.
[Classification] Input signal
[Function] Programs stored in the part program memory are output to an external unit via the reader/punch interface.
[Operation] When this signal becomes logical 1, the CNC operates as follows: � In all modes other than the MDI mode, the background edit function
outputs all programs stored in the part program memory to an external output device.
� When programs are being output, the read/punch busy signal RPBSY becomes logical 1.
� When the background processing–activated signal BGEACT is logical 1 (for example, during background editing or MDI mode), the external punch start signal EXWT is ignored.
� When programs are being output, if the system is reset or the external read/punch stop signal EXSTP becomes logical 1, the output is discontinued.
� If the foreground processing is already using the reader/punch interface (for example, during DNC operation or program reading in the edit mode), the external punch start signal EXWT is ignored.
� There are some other conditions to determine whether all programs can be output. For example, a program cannot be output, if it is running or protected by bit 4 (PRG9) of parameter No.0010 and bit 2 (PRG8) of parameter No.0389.
[Classification] Input signal
[Function] When the external read/punch stop signal becomes logical 1, it stops program registeration, collation, or output via the reader/punch interface and program registeration and collation via the remote buffer.
[Operation] When this signal becomes logical 1, the CNC operates as follows: � The program registeration, collation or output triggered by the
external read or punch start signal is stopped immediately.
External punch start signal EXWT<G134#3>
External read/punch stop signal EXSTP<G134#2>
13 INPUT/OUTPUT OF DATA B–61393E–2/02
684
[Classification] Output signal
[Function] This signal indicates that the background edit function is operating.
[Output condition] This signal becomes logical 1 when: � The [BG EDIT] soft key is pressed to put the CNC in the background
edit mode.
� The MDI mode is selected.
� The external read or punch start signal starts program registeration, collation, or output.
� When the uploading or downloading of a program from DNC1, DNC2, or MMC is started.
This signal becomes logical 0 when:
� The [BG END] soft key is pressed to terminate the background edit mode.
� The CNC shifts from the MDI mode to another mode.
� Program registeration or output triggered by the external read or punch start signal ends either normally or abnormally (reset or requested by the EXSTP signal).
� When the uploading or downloading of a program from DNC1, DNC2, or MMC is completed.
[Classification] Output signal
[Function] This signal indicates that program registeration, collation, or output triggered by the external read or punch start signal is under way.
[Output condition] This signal becomes logical 1, when: � The external read or punch start signal triggers program registeration,
collation, or output.
This signal becomes logical 0, when:
� Program registeration collation or output triggered by the external read or punch start signal ends either normally or abnormally (reset or requested by the EXSTP signal).
Background editing signal BGEACT<F180#4>
Read/punch busy signal RPBSY<F180#2>
B–61393E–2/02 13 INPUT/OUTPUT OF DATA
685
[Classification] Output signal
[Function] This signal indicates that an alarm condition has occurred during program registeration, collation, or output triggered by the external read or punch start signal.
[Output condition] This signal becomes logical 1, when: � An alarm condition occurs during program registeration, collation, or
output triggered by the external read or punch start signal.
This signal becomes logical 0, when:
� The system is reset, or the external read/punch stop signal EXSTP is input.
#7 G134
#6 #5 #4 #3 EXWT
#2 EXSTP
#1 EXRD
#0
#7 F180
#6 #5 #4 BGEACT
#3 RPALM
#2 RPBSY
#1 #0
Stop bit and other data
Number specified for the input/output device
Baud rate
Stop bit and other data
Number specified for the input/output device
Baud rate
I/O =0 : Channel 1
=1 : Channel 1
=2 : Channel 2
=3 : Channel 3
Specify a channel for
an input/output device.
I/O =1
(channel 1)
I/O 0002#0
0038#6, #7I/O =0
(channel 1) 0552
0012#0
0038#6, #7
0553
Input/output channel number
↓
I/O =3
(channel 3)
* Remote buffer
0050#0
0038#4, #5I/O =2
(channel 2) 0250
0051#0
0038#1, #2
0251
0055#2
0055#3
Stop bit and other data
Number specified for the input/output device
Baud rate
Stop bit and other data
Number specified for the input/output device
Baud rate
Selection of protocol
Selection of RS–422 or RS–232C, and other data