Page 1
Page 2
www.cncdata.co.uk 1
O0001;
O9010;
Main Program
Sub Program
Local & Common Variables > Introduction
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, the only
difference being; we can pass information into the sub program and manipulate it
as we want.
;
;
G65 P9010 A1. B26. F500.
;
;
M30;
G91;
N100 #101=#2/2
G#1 G42 X#101 Y#1 F#9
IF[#5021LT100]GOTO100;
M99;
Page 3
www.cncdata.co.uk 2
#2=0
G01 X#1 F200;
Local & Common Variables > Local & Common Variable
In the world of Macro B, everything revolves around variables, that is because
90% of the information visible on a Fanuc control, has its own variable address,
these are called System Variables. Fanuc has also given the end user its own set
of variables, two types, local and common, located: [OFFSET] – {MACRO} (see
page 5).
Here are some of the System variables available:
• Tool Offsets
• Work Offsets
• Axis Positions
• Modal Information
• PMC Signals
• Alarms
• Automatic Operation Control
• Timers and Counters
Plus many more
An ordinary machining program specifies a G code and the travel distance
directly with a numeric value; examples are G01 X100.0
With a custom macro, numeric values can be specified directly or using a
variable number. When a variable number is used, the variable value can be
changed by a program or using operations on the MDI panel.
#1=#2+100;
When specifying a variable, specify a number sign (#) followed by a variable
number. General–purpose programming languages allow a name to be assigned
to a variable, but this capability is only available for custom macros on a 30xi
Series.
Example: #1
An expression can be used to specify a variable number. In such a case, the
expression must be enclosed in brackets.
Example: #[#1+#2–12]
Page 4
www.cncdata.co.uk 3
Variable number
Type of variable
Function
#0
Always null
This variable is always null. No value can
#1 – #33
Local variables
Local variables can only be used within a
local variables are initialized to null. When a
#100 – #149 (#199)
Common Variables
Common variables can be shared among
#1000 +
System variables
System variables are used to read and
Note
Local and common variables can have value 0 or a value in the
Local & Common Variables > Local & Common Variables
Variables are classified into four into four dif ferent types.
be assigned to this variable. It is not a
value, it is nothing/empty/null.
macro to hold data such as the results of
operations. When the power is turned off,
macro is called, arguments are assigned to
local variables. These should only be used
to pass values, not for calculations
#500 - #531 (#999)
different macro programs. When the power
is turned off, variables #100 to #149 are
initialized to null. Variables #500 to #531
hold data even when the power is turned
off. As an option, common variables #150
to #199 and #532 to #999 are also
available.
write a variety of NC data items such as
the current position and tool compensation
values.
Common variables #150 - #199 and #532 - #999 are a purchasable option from
Fanuc GE (J887)
Range of Variables:
following ranges:
–10
47
to –10
–29
0
10
–29
to 10
47
If the result of calculation turns out to be invalid, a P/S alarm
No. 111 is issued.
No decimal point is required with variables.
Example
When #1=123; is defined, the actual value of variable #1 is
123.000.
Page 5
www.cncdata.co.uk 4
When #1 = < vacant >
When #1 = 0
G01 X100 Y #1
G01 X100 Y #1
When #1 = < vacant >
When #1 = 0
#2 = #1
#2 = #1
#2 = #1*5
#2 = #1*5
#2 = #1+#1
#2 = #1 + #1
Local & Common Variables > Examples of Variables
When the value of a variable is not defined, such a variable is referred to as a
“null” variable. Variable #0 is always a null variable. It cannot be written to, but it
can be read. If you look at variables #100 - #149 they are empty, this is written as
#0.
When an undefined variable is quoted, the address itself is also ignored
G01 X100
G01 X100 Y0
When < vacant > is the same as 0 except when replaced by < vacant>
#2 = < vacant >
#2 = 0
#2 = 0
#2 = 0
#2 = 0
#2 = 0
Page 6
www.cncdata.co.uk 5
< vacant > differs from 0 only for EQ and NE.
When #1 = < vacant >
When #1 = 0
#1 EQ #0
#1 EQ #0
Established
Not established
#1 NE 0
#1 NE 0
Established
Not established
#1 GE #0
#1 GE #0
Established
Established
Conditions Expressions
EQ
EQUAL
NE
NOT EQUAL TOO
LT
LESS THAN
LE
LESS THAN OR EQUAL TOO
GT
GREATER THAN
GE
GREATER THAN OR EQUAL TOO
Local & Common Variables > Examples of Variables
To display the macro variables press [OFFSET] – {MACRO}
If ******** is displayed then an overflow has occurred. An overflow means the
variable is either greater than 99999999 or less than 0.00000001.
Page 7
www.cncdata.co.uk 6
#1000–#1015
A 16–bit signal can be sent from the PMC to a custom
#1100–#1115
A 16–bit signal can be sent from a custom macro to the
bits of a signal at one time.
#1133
Variable #1133 is used to write all 32 bits of a signal at
one time from a custom macro to the PMC.
System Variables > PMC Variables
System variables can be used to read and write internal NC data such as tool
compensation values and current position data. Note, however, that some
system variables can only be read. System variables are essential for automation
and general–purpose program development.
Interface signals can be exchanged between the programmable machine
controller (PMC) and custom macros. In order to use these variables the PMC
must be programmed to do this. PMC’s should only be written or modified by
MTB’s. Do not alter your PMC.
Variable
number
#1032
Function
macro. Variables #1000 to #1015 are used to read a
signal bit by bit. Variable #1032 is used to read all 16
bits of a signal at one time.
#1132
PMC. Variables #1100 to #1115 are used to write a
signal bit by bit. Variable #1132 is used to write all 16
For detailed information, refer to the connection manual (B–63523EN–1).
Page 8
www.cncdata.co.uk 7
System Variables for Tool Compensation Memory A
Compensation Number
System Variable
1
#10001(#2001)
System Variables for Tool Compensation Memory B
Compensation Number
Wear Compensation
1
#10001(#2001)
Geometry Compensation
#11001(#2201)
System Variables for Tool Compensation Memory C
Cutter Compensation (D)
1
#10001(#2001)
Tool Length Compensation (H)
#11001(#2201)
Geometric
Wear
Geometric
Wear
#13001
#12001
System Variables > Tooling Variables
Tool compensation values can be read and written using system variables.
Usable variable numbers depend on the number of compensation pairs, whether
a distinction is made between geometric compensation and wear compensation,
and whether a distinction is made between tool length compensation and cutter
compensation. When the number of compensation pairs is not greater than 200,
variables #2001 to #2400 can also be used.
:
200
:
999
:
#10200(#2200)
:
#10999
:
200
:
999
:
#11200(#2400)
:
#11999
:
#10200(#2200)
:
#10999
Compensation
Number
:
200
:
999
Compensation
:
#11200(#2400)
:
#11999
Compensation
:
#10200(#2200)
:
#10999
Compensation
:
#13200
:
#13999
Compensation
:
#12200
:
#12999
Page 9
www.cncdata.co.uk 8
#100=#11001
System Variables > Tooling Variables
If the control being used has memory C (below) and we want to read the length
of Tool 1 into common variable 100, we need:
#100=#11001
The value of specified in the offset table for the length of tool 1 is now input into
variable 100.
Page 10
www.cncdata.co.uk 9
System Variables > Alarms
Using system variables we can make the machine stop instantly and display a
custom message. When a value from 0 to 200 is assigned to variable #3000,
the CNC stops with an alarm. After an expression, an alarm message not longer
than 26 characters can be described. The CRT screen displays alarm numbers
by adding 3000 to the value in variable #3000 along with an alarm message.
Example:
#3000=1(TOOL LIFE EXPIRED)
If you program #3000=23 (TOOL LIFE EXPIRED) then “3023 TOOL LIFE
EXPIRED” is dispalyed.
Page 11
www.cncdata.co.uk 10
System Variables > Messages
Operator messages are a good way of letting the operator know what is going on
in the program and also any checks or inspections they need to make.
When “#3006=1 (MESSAGE);” is commanded in the macro, the program
executes blocks up to the immediately previous one and then stops.
When a message of up to 26 characters, which is enclosed by a control–in
character (“(”) and control–out character (“)”), is programmed in the same block,
the message is displayed on the external operator message screen. The
message can be cleared with #3006=0.
#3006=1(CHECK COMPONENT SEATED)
Page 12
www.cncdata.co.uk 11
#3001
0.
#3011
#3012
System Variables > Timers and Counters
Information regarding time, whether is be the actual time or time to complete
something, this can be read using system variables.
System Variables for Time Information
Variable
number
Function
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 2147483648 milliseconds is
reached, the value of this timer returns to 0.
#3002 This variable functions as a timer that counts in 1–hour
increments when the cycle start lamp is on. This timer
preserves its value even when the power is turned off. When
9544.371767 hours is reached, the value of this timer returns to
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, September 28, 2001 is
represented as 20010928.
This variable can be used to read the current time (hours/minutes/seconds). Hours/minutes/seconds information is converted
to an apparent decimal number. For example, 34 minutes and
56 seconds after 3 p.m. is represented as 153456.
As #3001 is constantly running, if we want to use it then we must reset it first.
Example:
#3001=0;
M98 P1000 (CONTOURING CYCLE);
#500=#3001;
#500=#500/1000;
Using these functions it is possible to calculate things such as:
• The percentage of the shift the machine was actually in cycle.
• Cycle time.
• Downtime.
Page 13
www.cncdata.co.uk 12
#3003
Single block
Completion of an auxiliary function
0
Enabled
To be awaited
1
Disabled
To be awaited
2
Enabled
Not to be awaited
3
Disabled
Not to be awaited
System Variables > Automatic Operation Control
Using system variables we are able to disable and enable program control
functions such as:
• SINGLE BLOCK
• FEED RATE OVERRIDE
• FEED HOLD
• EXACT STOP
These groups of variables are called Automatic Operation Control.
System Variable (#3003) for Automatic Operation Control
Example:
#3003=3 – single block is instantly disabled.
#3003=2 – single block is instantly enabled.
When using this variable, there are a few things to be aware of:
• When the power is turned on, the value of this variable is 0.
• When single block stop is disabled, single block stop operation is not
performed even if the single block switch is set to ON.
• When a wait for the completion of auxiliary functions (M, S, and T
functions) is not specified, program execution proceeds to the next
block before completion of auxiliary functions. Also, distribution
completion signal DEN is not output.
Page 14
www.cncdata.co.uk 13
System Variable (#3004) for Automatic Operation Control
#3004
Feed hold
Feed Rate Override
Exact stop
0
Enabled
Enabled
Enabled
1
Disabled
Enabled
Enabled
2
Enabled
Disabled
Enabled
3
Disabled
Disabled
Enabled
4
Enabled
Enabled
Disabled
5
Disabled
Enabled
Disabled
6
Enabled
Disabled
Disabled
7
Disabled
Disabled
Disabled
O0001 ;
System Variables > Automatic Operation Control
Example:
#3004=2 – this will only disable the Feed rate override.
When using this variable, there are a few things to be aware of:
• When the power is turned on, the value of this variable is 0.
• When feed hold is disabled:
(1) When the feed hold button is held down, the machine stops in the
single block stop mode. However, single block stop operation is not
performed when the single block mode is disabled with variable #3003.
(2) When the feed hold button is pressed then released, the feed hold
lamp comes on, but the machine does not stop; program execution
continues and the machine stops at the first block where feed hold is
enabled.
• When feed rate override is disabled, an override of 100% is always
applied regardless of the setting of the feed rate override switch on the
machine operator’s panel.
• When exact stop check is disabled, no exact stop check (position check) is
made even in blocks including those which do not perform
cutting.
N1 G00 G90 X#24 Y#25
;
N2 Z#18 ;
G04 ;
N3 #3003=3 ;
N4 #3004=7 ;
N5 G01 Z#26 F#9 ;
N6 M04 ;
N7 G01 Z#18 ;
G04 ;
N8 #3004=0 ;
N9 #3003=0 ;
N10M03 ;
Page 15
www.cncdata.co.uk 14
#4001
#4007
#4013
#4002
#4008
#4014
#4003
#4009
#4015
#4004
#4010
#4016
#4005
#4011
#4017
#4006
#4012
#4018
System Variables > Modal Information
The image above is a screen shot of a standard Fanuc program display.
Below the axis positioning you can see the MODAL information. Modal means
active G code or active commands. Everything except the actual spindle speed in
the red ring can be read.
#4109
#4111
#4107
#4119
#4113
#4120
Page 16
www.cncdata.co.uk 15
System Variables for Modal Information
#4001
G00, G01, G02, G03, G33
Group 1
#4002
G17, G18, G19
Group 2
#4003
G90, G91
Group 3
#4004
Group 4
#4005
G94, G95
Group 5
#4006
G20, G21
Group 6
#4007
G40, G41, G42
Group 7
#4008
G43, G44, G49
Group 8
#4009
G73, G74, G76, G80–G89
Group 9
#4010
G98, G99
Group 10
#4011
G98, G99
Group 11
#4012
G65, G66, G67
Group 12
#4013
G96,G97
Group 13
#4014
G54–G59
Group 14
#4015
G61–G64
Group 15
#4016
G68, G69
Group 16
: : :
#4022
Group 22
#4102
B code
#4107
D code
#4109
F code
#4111
H code
#4113
M code
#4114
Sequence number
#4115
Program number
#4119
S code
#4120
T code
System Variables > Modal Information
Variable
Number
Function Group
Example:
When #1=#4001; is executed, the resulting value in #1 is 0, 1, 2, 3, or 33.
If the specified system variable for reading modal information corresponds to a G
code group that cannot be used, a P/S alarm is issued.
Page 17
www.cncdata.co.uk 16
System Variables for Positioning Information
Variable number
Read
movement
#5001–#5008
Block end point
Workpiece
system
Not included
Enabled
#5021–#5028
Current position
Machine
system
Included
Disabled
#5041–#5048
Current position
Workpiece
#5061–#5068
Skip signal
Enabled
#5081–#5088
Tool length
Disabled
#5101–#5108
Deviated servo
Here the axis numbers are as follow:
#5021
Here the absolute positions are shown
System Variables > Positioning Information
Position information can be read but not written.
position
offset value
position
The first digit (from 1 to 8) represents an axis number.
Position
information
#5022
#5023
#5024
#5025
Coordinate
system
coordinate
coordinate
coordinate
system
X=1
Y=2
Z=3
A=4
C=5
Always follow this rule or check
parameter 1022.
as there variable numbers:
X=#5021
Y=#5022
Z=#5023
A=#5024
C=#5025
Tool
compensation
value
operation
during
Page 18
www.cncdata.co.uk 17
number
#5201
First–axis external workpiece zero point offset value
:
:
#5208
Eighth–axis external workpiece zero point offset value
#5221
First–axis G54 workpiece zero point offset value
:
:
#5228
Eighth–axis G54 workpiece zero point offset value
#5241
First–axis G55 workpiece zero point offset value
:
:
#5248
Eighth–axis G55 workpiece zero point offset value
#5261
First–axis G56 workpiece zero point offset value
:
:
#5268
Eighth–axis G56 workpiece zero point offset value
#5281
First–axis G57 workpiece zero point offset value
:
:
#5288
Eighth–axis G57 workpiece zero point offset value
#5301
First–axis G58 workpiece zero point offset value
:
:
#5308
Eighth–axis G58 workpiece zero point offset value
#5321
First–axis G59 workpiece zero point offset value
:
:
#5328
Eighth–axis G59 workpiece zero point offset value
System Variables > Work Offset Information
Using system variables, zero offset (datum) positions can be read and written
too.
Variable
Function
To use variables #2500 to #2806 and #5201 to #5328, optional variables for the
workpiece coordinate systems are necessary.
Optional variables for 48 additional workpiece coordinate system s are #7001 t o
#7948 (G54.1 P1 to G54.1 P48).
Optional variables for 300 additional workpiece coordinate systems are #14001
to #19988 (G54.1 P1 to G54.1 P300).
With these variables, #7001 to #7948 can also be used.
Check the Fanuc operator manual with the machine for additional variables.
Page 19
www.cncdata.co.uk 18
Axis
Function
Variable number
First axis
External workpiece zero point offset
#2500
#5201
G54 workpiece zero point offset
#2501
#5221
G55 workpiece zero point offset
#2502
#5241
G56 workpiece zero point offset
#2503
#5261
G57 workpiece zero point offset
#2504
#5281
G58 workpiece zero point offset
#2505
#5301
G59 workpiece zero point offset
#2506
#5321
Second
External workpiece zero point offset
#2600
#5202
axis
G54 workpiece zero point offset
#2601
#5222
G55 workpiece zero point offset
#2602
#5242
G56 workpiece zero point offset
#2603
#5262
G57 workpiece zero point offset
#2604
#5282
G58 workpiece zero point offset
#2605
#5302
G59 workpiece zero point offset
#2606
#5322
Third axis
External workpiece zero point offset
#2700
#5203
G54 workpiece zero point offset
#2701
#5223
G55 workpiece zero point offset
#2702
#5243
G56 workpiece zero point offset
#2703
#5263
G57 workpiece zero point offset
#2704
#5283
G58 workpiece zero point offset
#2705
#5303
G59 workpiece zero point offset
#2706
#5323
Fourth axis
External workpiece zero point offset
#2800
#5204
G54 workpiece zero point offset
#2801
#5224
G55 workpiece zero point offset
#2802
#5244
G56 workpiece zero point offset
#2803
#5264
G57 workpiece zero point offset
#2804
#5284
G58 workpiece zero point offset
#2805
#5304
G59 workpiece zero point offset
#2806
#5324
System Variables > Work Offset Information
The following variables can also be used to read and write zero offset positions.
Page 20
www.cncdata.co.uk 19
Function
Format
Remarks
Definition
#i=#j
Sum
#i=#j+#k;
Difference
#i=#j–#k;
Multiply
#i=#j*#k;
Divide
#i=#j/#k;
Sine
#i=SIN[#j];
An angle is specified in de-
Arcsine
#i=ASIN[#j];
Cosine
#i=COS[#j];
Arccosine
#i=ACOS[#j];
Tangent
#i=TAN[#j];
Arctangent
#i=ATAN[#j]/[#k];
Square root
#i=SQRT[#j];
Absolute value
#i=ABS[#j];
Rounding off
#i=ROUND[#j];
Rounding down
#i=FIX[#j];
Rounding up
#i=FUP[#j];
Natural logarithm
#i=LN[#j];
Exponential function
#i=EXP[#j];
OR
#i=#j OR #k;
bit by bit.
XOR
#i=#j XOR #k;
AND
#i=#j AND #k;
Conversion from BCD to BIN
#i=BIN[#j];
and from the PMC
Conversion from BIN to BCD
#i=BCD[#j];
Functions > Function List
The operations listed in the table below can be performed on variables. The
expression to the right of the operator can contain constants and/or variables
combined by a function or operator. Variables #j and #K in an expression can be
replaced with a constant. Variables on the left can also be replaced with an
expression.
grees. 90 degrees and 30
minutes is represented as
90.5 degrees.
A logical operation is performed on binary numbers
Used for signal exchange to
Page 21
www.cncdata.co.uk 20
Functions > Function Descriptions
Definition - #i=#j
This is what’s used to transfer data from one variable to another. The left variable
is where the result is.
So if #1=10 and #2=12
#1=#2
Both variables now equal 12.
Sum - #i=#j+#k
This is what’s used to add variables, or values on their own together.
So if #2=12
#1=#2+10
The value of #1 is now 22.
Difference - #i=#j-#k
This is what’s used to subtract variables, or values on their own together.
So if #2=12
#1=#2-10
The value of #1 is now 2.
Multiply - #i=#j*#k
This is what’s used to multiply variables, or values on their own together.
So if #2=12
#1=#2*10
The value of #1 is now 120.
Divide - #i=#j/#k
This is what’s used to divide variables, or values on their own together.
So if #2=20
#1=#2/10
The value of #1 is now 2.
All of the above can be put together using brackets to perform larger calculations.
So if #1=2 and #2=5
#100=#1*[#2-3]
The value of #100 is now 4, because 2 x (5 – 3) = 4
For more information on the priority of operations when using brackets see page
23. Macro B also conforms to the Precedence Rule.
Page 22
www.cncdata.co.uk 21
Sine
#i=SIN[#j];
Tangent
#i=TAN[#j];
Cosine
#i=COS[#j];
50
#1
#2
Functions > Function Examples
In Macro B, Sine, Cosine and Tangent follow the same pattern.
30°
In the example above, #1=30 and #2=50
In mathematics the equation to calculate the length of:
X is (cos30) x 50 = 43.301
Y is (sin30) x 50 = 25
In Macro B it’s the same
X is #100=[cos[#1]*#2]
Y is #101=[sin[#1]*#2]
To actually move the axis incrementally the result of this calculation we can write
the following:
G1 G91 X[cos[#1]*#2] Y[sin[#1]*#2]
Or
#100=[cos[#1]*#2]
#101=[sin[#1]*#2]
G1 G91 X#100 Y#101
It is a good idea to use a Zeus book if you’re unsure of the formulae.
Arcsine, Arccosine and Arctangent are inverse trigonometric functions of Sine,
Cosine and Tangent.
There are sme parameters related to Arcsine, Arccosine and Arctangent, for
further details see the manual B–63534EN
Page 23
www.cncdata.co.uk 22
Functions > Function Examples
Round Function - #i=ROUND[#j];
When the ROUND function is included in an arithmetic or logic operation
command, IF statement, or WHILE statement, the ROUND function rounds off at
the first decimal place.
When #1=ROUND[#2]; is executed where #2 holds 1.2345, the value
of variable #1 is 1.0.
Rounding Up and Down - #i=FUP[#j] & #i=FIX[#j]
With CNC, when the absolute value of the integer produced by an operation on a
number is greater than the absolute value of the original number, such an
operation is referred to as rounding up to an integer.
Conversely, when the absolute value of the integer produced by an operation on
a number is less than the absolute value of the original number, such an
operation is referred to as rounding down to an integer.
Be particularly careful when handling negative numbers.
Suppose that #1=1.2 and #2=–1.2.
When #3=FUP[#1] is executed, 2.0 is assigned to #3.
When #3=FIX[#1] is executed, 1.0 is assigned to #3.
When #3=FUP[#2] is executed, –2.0 is assigned to #3.
When #3=FIX[#2] is executed, –1.0 is assigned to #3.
Page 24
www.cncdata.co.uk 23
1
2
3
1,2 and 3 indicate the order of
1,2,3,4 and 5 indicate the order of
Functions > Function Rules
When programming larger calculations, it is important to make sure your
calculations are in the correct order, this is called the Priority of Operations.
The priority of operation for Macro B statements is as follows:
1. Functions
2. Operations such as multiplication and division (*,/,AND)
3. Operations such as addition and subtraction (+,-,OR,XOR)
Example
#1=#2+#3*sin[#4]
Brackets are used to change the order of operations. Brackets can be used to a
depth of five levels including the brackets used to enclose a function.
When a depth of five levels is exceeded, P/S alarm No. 118 occurs.
#1=sin[[#2+#3]*#4+#5]*#6]
operations.
operations.
Page 25
www.cncdata.co.uk 24
Functions > Function Rules
Brackets ([, ]) are used to enclose an expression. Note that parentheses (,)are
used for comments.
Errors may occur when operations are performed.
1 The relative error depends on the result of the operation.
2 Smaller of the two types of errors is used.
3 The absolute error is constant, regardless of the result of the
operation.
4 Function TAN performs SIN/COS.
5 If the result of the operation by the SIN, COS, or TAN
function is less than 1.0 x 10–8 or is not 0 because of the
precision of the operation, the result of the operation can be
normalized to 0 by setting bit 1 (MFZ) of parameter No. 6004
to 1.
The precision of variable values is about 8 decimal digits. When very large
numbers are handled in an addition or subtraction, the expected results may not
be obtained.
Example:
When an attempt is made to assign the following values to variables
#1 and #2:
#1=9876543210123.456
#2=9876543277777.777
the values of the variables become:
#1=9876543200000.000
#2=9876543300000.000
In this case, when #3=#2–#1; is calculated, #3=100000.000 results.
(The actual result of this calculation is slightly different because it is
performed in binary.)
When a divisor of zero is specified in a division or TAN[90], P/S alarm No. 112
occurs.
Page 26
www.cncdata.co.uk 25
Macro Statements > Definitions
The following blocks are referred to as macro statements:
• Blocks containing an arithmetic or logic operation (=)
• Blocks containing a control statement (such as GOTO, DO, END)
• Blocks containing a macro call command (such as macro calls by G65,
G66, G67, or other G codes, or by M codes)
Any block other than a macro statement is referred to as an NC statement.
Differences from NC Statements
Even when single block mode is on, the machine does not stop. Note,
however, that the machine stops in the single block mode when bit 5
of parameter SBM No. 6000 is 1.
Macro blocks are not regarded as blocks that involve no movement in
the cutter compensation mode (seeII–15.7).
NC statements that have the same property as macro statements
NC statements that include a subprogram call command (such as
subprogram calls by M98 or other M codes, or by T codes) and not
include other command addresses except an O,N or L address have the
same property as macro statements.
The blocks not include other command addresses except an O,N,P or
L address have the same property as macro statements.
Page 27
www.cncdata.co.uk 26
If the condition
Specify a conditional expression after IF.
Unconditional Branch
If the value of variable #100 is not equal to 20, a branch to sequence
number N5 occurs.
IF[#100 NE 20] GOTO 5
Processing
If the condition is
IF[<conditional
If the specified conditional expression is
If #1 is empty (no value in it), then the following statement is satisfied.
IF[#1EQ#0] THEN #3000=1(TOOL NOT ENGAGED);
Macro Statements > GOTO
In a program, the flow of control can be changed using the GOTO statement and
IF statement. Three types of branch and repetition operations are used:
Branch and Repetition
Unconditional Branch (GOTO Statement)
IF[<conditionalexpression>]GOTOn
(GOTO Statement)
IF[<conditional
expression>]GOTOn
is not satisfied
expression>]THEN
A conditional expression must include an operator inserted between two
variables or between a variable and constant, and must be enclosed in
brackets ([, ]). An expression can be used instead of a variable.
GOTO statement (unconditional branch)
IF statement (conditional: IF…,THEN…)
WHILE statement (repetition)
If the specified conditional expression is satisfied,
a branch to sequence number n occurs. If the
specified condition is not satisfied, the next block
is executed.
satisfied
N5 G0 G54 X50.
satisfied, a predetermined macro
statement is executed.
Only a single macro statement is executed.
Page 28
www.cncdata.co.uk 27
Operator
Meaning
EQ
Equal to(=)
NE
Not equal to()
GT
Greater than(>)
GE
Greater than or equal to()
LT
Less than(<)
LE
Less than or equal to()
O9500;
Macro Statements > IF Statement
Operators each consist of two letters and are used to compare two values to
determine whether they are equal or one value is smaller or greater than the
other value. Note that the inequality sign cannot be used.
The sample program below finds the total of numbers 1 to 10.
#1=0; . . . . . . . . . . . . . . . . . . Initial value of the variable to hold the sum
#2=1; . . . . . . . . . . . . . . . . . . Initial value of the variable as an addend
N1 IF[#2 GT 10] GOTO 2; . . Branch to N2 when the addend is greater than 10
#1=#1+#2; . . . . . . . . . . . . . . Calculation to find the sum
#2=#2+1; . . . . . . . . . . . . . . . Next addend
GOTO 1; . . . . . . . . . . . . . . . Branch to N1
N2 M30; . . . . . . . . . . . . . . . . End of program
Page 29
www.cncdata.co.uk 28
If the condition
If the condition
Specify a conditional expression after WHILE.
WHILE [conditional expression] DO n (n=1,2,3)
Processing
END n
Macro Statements > WHILE Statement
Repetition
(WHILE statement)
While the specified condition is satisfied, the
program from DO to END is executed. If the
specified condition is not satisfied, program
execution proceeds to the block after END.
is satisfied
is not satisfied
While the specified condition is satisfied, the program from DO to END after
WHILE is executed. If the specified condition is not satisfied, program execution
proceeds to the block after END. The same format as for the IF statement
applies. A number after DO and a number after END are identification numbers
for specifying the range of execution. The numbers 1, 2, and 3 can be used.
When a number other than 1, 2, and 3 is used, P/S alarm No. 126 occurs.
The sample program below finds the total of numbers 1 to 10.
O0001;
#1=0;
#2=1;
WHILE[#2 LE 10]DO 1;
#1=#1+#2;
#2=#2+1;
END 1;
M30;
Page 30
www.cncdata.co.uk 29
The identification numbers (1 to 3)
DO loops can be nested to a
WHILE […] DO 1;
Processing
END 1;
WHILE […] DO 1;
Processing
END 1;
DO ranges cannot over lap.
WHILE […] DO 1;
Processing
END 1;
WHILE […] DO 2;
Processing
END 1;
WHILE […] DO 3;
Processing
END 3;
WHILE […] DO 2;
END 2;
WHILE […] DO 1;
END 2;
:
Control can be transferred to the
WHILE […] DO 1;
Processing
END 1;
IF […] GOTO n;
Processing
Nn;
Macro Statements > Rules & Limitations
The identification numbers (1 to 3) in a DO–END loop can be used as many
times as desired. Note, however, when a program includes crossing repetition
loops (overlapped DO ranges), P/S alarm No. 124 occurs.
can be used as many times as
required.
maximum depth of three levels.
outside of a loop.
Page 31
www.cncdata.co.uk 30
A macro program can be called using the following
methods:
G65 P9010 X10 Y15 Z-10 R2
#24
#25
#26
#18
#24=10
Macro Call > Definitions
Macro Call
Macro Call
Simple call (G65)
Modal call (G66,G67)
Macro call with G code
Macro call with M code
Subprogram call with M code
Subprogram call with T code
Both G65 and M98 will call up and open a subprogram.
The main difference between a Macro Call (G65) and a subprogram call (M98) is
that G65 can pass information from the G65 line into a subprogram as variables.
When an M98 block contains another NC command (for example, G01 X100.0
M98Pp), the subprogram is called after the command is executed. On the other
hand, G65 unconditionally calls a macro.
Think of a normal canned cycle as a macro call( G81 – Drilling). The information
you specify (example X and Y coordinates, depth of hole, return point, etc) is
then passed into a macro program, the data is manipulated, that then drills your
holes. This is what happens on CNC controls, but as Fanuc or the MTB have
written the cycles, they have also hidden all the “behind the scenes” activities. It
is also possible in to do this, once the Macro is complete.
#25=15
#26#=-10
#18=2
Page 32
www.cncdata.co.uk 31
Variable
Variable
Variable
A
#1 I #4 T #20
B
#2 J #5 U #21
C
#3 K #6 V #22
D
#7 M #13
W
#23
E
#8 Q #17
X
#24
F
#9 R #18
Y
#25
H
#11
S
#19
Z
#26
Simple Call (G65)
When G65 is specified, the custom macro
G65 Pp Ln
O0001;
O9010;
Macro Call > Simple Call
specified at address P is called. Data (argument)
can be passed to the custom macro program.
P: Number of the program to call
L: Repetition count
:
G65 P9010 L2 A1 B2;
:
M30;
#3=#1+#2;
IF[#3GT360]GOTO99;
G0 G54 X10;
M99;
After a G65, a P (program number) must be specified, this program is the macro
program needed. When repetitions are required, a L must be specified.
Any other information on a G65 line is passed into the macro program as
variables. This is what we call an argument. The information passed is the
argument.
Two types of argument specification are available. Argument specification 1 us es
letters other than G, L, O, N, and P once each.
Argument specification 2 uses A, B, and C once each and also uses I, J, and K
up to ten times. The type of argument specification is determined automatically
according to the letters used. See the manual B-63534 for further details.
Address
Number
• Addresses G, L, N, O, and P cannot be used in arguments.
• Addresses that need not be specified can be omitted. Local variables
corresponding to an omitted address are set to null.
• Addresses do not need to be specified alphabetically. They conform
to word address format.
I, J, and K need to be specified alphabetically, however.
Address
Number
Address
Number
Page 33
www.cncdata.co.uk 32
O0001;
O0002;
O0003;
O0004;
O0005;
Main Program
Macro
Macro
Macro
Macro
Macro Call > Rules and Limitations
Calls can be nested to a depth of four levels including simple calls (G65) and
modal calls (G66). This does not include subprogram calls (M98).
Level 0
Level 1
Level 2
Level 3
Level 4
:
#1=1;
G65 P2 A2;
:
:
M30;
:
(#1=2);
G65 P3 A3;
:
:
M99;
:
(#1=3);
G65 P4 A4;
:
:
M99;
:
(#1=4);
G65 P5 A5;
:
:
M99;
:
(#1=5);
:
:
:
M99;
• Local variables from level 0 to 4 are provided for nesting.
• The level of the main program is 0.
• Each time a macro is called (with G65 or G66), the local variable level
is incremented by one. The values of the local variables at the previous
level are saved in the CNC.
• When M99 is executed in a macro program, control returns to the
calling program. At that time, the local variable level is decremented
by one; the values of the local variables saved when the macro was
called are restored.
Page 34
www.cncdata.co.uk 33
Once G66 is issued to specify a modal call a macro
G66 Pp Ln
O0001;
O9010;
Macro Call > Modal Call
Modal Call (G66)
is called after a block specifying movement along
axes is executed. This continues until G67 is
issued to cancel a modal call.
P: Number of the program to call
L: Repetition count
:
G66 P9010 L2 A1 B2;
G00 X100.;
Y300.
M30;
G00 Z-#1
G01 Z-#2
M99;
• After G66, specify at address P a program number subject to a modal
call.
• When a number of repetitions is required, a number from 1 to 9999 can
be specified at address L.
• As with a simple call (G65), data passed to a macro program is
specified in arguments.
When a G67 code is specified, modal macro calls are no longer performed
in subsequent blocks.
• Calls can be nested to a depth of four levels including simple calls (G65)
and modal calls (G66). This does not include subprogram calls (M98).
• Modal calls can be nested by specifying another G66 code during a modal
call.
Page 35
www.cncdata.co.uk 34
Program Number
Parameter Number
O9010
6050
O9011
6051
O9012
6052
O9013
6053
O9014
6054
O9015
6055
O9016
6056
O9017
6057
O9018
6058
O9019
6059
Macro Call Using
By setting a G code number used to call a macro
G65 Pp = G100
O0001;
O9010;
Macro Call > G Code
G Code
program in a parameter, the macro program can be
called in the same way as for a simple call (G65).
By setting parameter 6050 to 100, G65 Pn is now
replaced by G100
:
G100 L2 A1 B2;
:
M30;
By setting a G code number from 1 to 9999 used to call a custom macro program
(O9010 to O9019) in the corresponding parameter (N0.6050 to No.6059), the
macro program can be called in the same way as with G65.
For example, when a parameter is set so that macro program O9010 can
be called with G81, a user–specific cycle created using a custom macro
can be called without modifying the machining program.
The following table shows the correspondence between program number and
parameter. If for example your macro program is O9010, enter the value of the G
code you want in parameter 6050. I.E if you want G125 to open O9010 then 6050
must be 125.
#3=#1+#2;
IF[#3GT360]GOTO99;
G0 G54 X10;
M99;
Page 36
www.cncdata.co.uk 35
Program Number
Parameter Number
O9020
6080
O9021
6081
O9022
6082
O9023
6083
O9024
6084
O9025
6085
O9026
6086
O9027
6087
O9028
6088
O9029
6089
Macro Call Using
By setting an M code number used to call a macro
G65 Pp = M100
O0001;
O9020;
Macro Call > M Code
M Code
program in a parameter, the macro program can be
called in the same way as for a simple call (G65).
By setting parameter 6080 to 100, G65 Pn is now
replaced by M100
:
M100 L2 A1 B2;
:
M30;
#3=#1+#2;
IF[#3GT360]GOTO99;
G0 G54 X10;
M99;
By setting an M code number from 1 to 99999999 used to call a custom macro
program (9020 to 9029) in the corresponding parameter (No.6080 to No.6089),
the macro program can be called in the same way as with G65.
Page 37
www.cncdata.co.uk 36
Program Number
Parameter Number
O9001
6071
O9002
6072
O9003
6073
O9004
6074
O9005
6075
O9006
6076
O9007
6077
O9008
6078
O9009
6079
Subprogram Call
By setting an M code number used to call a
replaced by M100
M98 Pp = M100
O0001;
O9001;
Macro Call > Sub Call
Using M Code
subprogram (macro program) in a parameter, the
macro program can be called in the same way as
with a subprogram call (M98).
By setting parameter 6071 to 100, M98 Pn is now
:
M100;
:
M30;
M99;
By setting an M code number from 1 to 99999999 used to call a subprogram in a
parameter (No.6071 to No. 6079), the corresponding custom macro program
(O9001 to O9009) can be called in the same way as with M98.
Page 38
www.cncdata.co.uk 37
Exercises > Joint
Joint Exercise
Scenario
You have a customer that wants you to machine circular holes into a square
billet. Problem is there are over 50 variations of this job. All different hole sizes,
depths and centre points.
Process
1. Move the tool to centre point
2. Move the tool down into the job
3. Interpolate out seve r al t im es unt il diameter is m et
4. Return tool to the centre point
5. Repeat steps 2 and 3 until depth and diameter is met.
Now we have to think about every possibilty and options available to us, to come
up with the best method. Here are a few things to think about:
• Where is the datum point going to be?
•
Absolute or Incremental?
•
Climb milling/direction?
•
What letters to use on the Macro call?
•
What information shall we require?
•
Cutter compensation, yes/no?
•
What error checks can we make?
•
What G code to create?
•
What material is the component?
•
What variables shall we use, #100-#149 or #500-#531?
It’ always a good idea to have a pen and paper to hand to make notes on all of
the above when you’re writing Macro B programs.
Page 39
www.cncdata.co.uk 38
Exercises > Exercise 1
Using the joint the joint exercise just completed, we need to make the macro
machine to the correct sizes specified. Ensuring the macro doesn’t cut oversize,
radially or in depth. We also need to put in place measures to prevent the macro
running without all the necessary information. For example if the user forgets to
input the diameter of te circle, then the macro cannot run. This macro should run
with G100.
Page 40
www.cncdata.co.uk 39
Exercises > Exercise 2
Scenario
You have a customer that wants you to create a G-Code to enable him to drill
various PCD’s. These comes with various depths, diameters and the amount of
holes vary.
Process
1. Move the tool to the centre point
2. Using Trigonometry calculate hole position 1
3. Drill the hole
4. Using a WHILE statement repeat steps 2 & 3 until all holes are drilled.
Page 41
www.cncdata.co.uk 40
Exercises > Exercise 3
Scenario
We have just received an order for several thousand components. Each
component has a raised square face on it. There are ten different types of
component, where features such as the height or square size of the component
differ. Rather than write ten different NC programs, we can write one Macro
program instead.
Page 42
www.cncdata.co.uk 41
Exercises > Exercise 4
Scenario
You have just written several macro programs on a cylindrical grinder. All of
these programs use the offsets of Tool 1, as there is only one wheel and the
datum’s positions on G54. If the operator sets any other offsets then your macro
has a problem. The control has 300 tool offsets and 6 work piece offsets. Again if
the operator sets any offset other than G54, your macro has a problem. So we
have to create a check program to make sure no unnecessary information is set,
for tool length, tool radius and work pieces. Also if the external offset is, display a
message so the operator is aware the EXT offset is active.
Page 43
www.cncdata.co.uk 42
Exercises > Exercise 5
Scenario
Thread milling at your place of work is a common operation. Currently for every
cycle a new helical interpolation program is written, consuming a lot of time. Your
task is to create a cycle for thread milling, using G184 to call up the macro; the
G180 line should look similar to a G84 line. Once the tool enters the component,
it must not be stopped, Be sure to rad on and rad off.
Page 44
www.cncdata.co.uk 43
Exercises > Exercise 6
Scenario You have a customer that wants you to machine elliptical bosses into a square billet. Problem is there are over 20 variations of this job. All different major and minor diameters and some are not complete ellipses, i.e start at 90 degrees and finish at 180 degrees.
Process
1. Move the tool to centre point
2. Move the tool down into the job
3. Interpolate (varying radiuses throughout) out several times until diameter
is met
4. Return tool to the centre point
5. Repeat steps 2 and 3 until depth and diameter is met.
Page 45
www.cncdata.co.uk 44
Variable
Description
Variable
Description
#1
A #119
Common Variable
#2
B #120
Common Variable
#3
C #121
Common Variable
#4
I #122
Common Variable
#5
J #123
Common Variable
#6
K #124
Common Variable
#7
D #125
Common Variable
#8
E #126
Common Variable
#9
F #127
Common Variable
#10
#128
Common Variable
#11
H #129
Common Variable
#12
#130
Common Variable
#13
M #131
Common Variable
#14
#132
Common Variable
#15
#133
Common Variable
#16
#134
Common Variable
#17
Q #135
Common Variable
#18
R #136
Common Variable
#19
S #137
Common Variable
#20
T #138
Common Variable
#21
U #139
Common Variable
#22
V #140
Common Variable
#23
W #141
Common Variable
#24
X #142
Common Variable
#25
Y #143
Common Variable
#26
Z #144
Common Variable
#145
Common Variable
#100
Common Variable
#146
Common Variable
#101
Common Variable
#147
Common Variable
#102
Common Variable
#148
Common Variable
#103
Common Variable
#149
Common Variable
#104
Common Variable
#105
Common Variable
#106
Common Variable
#107
Common Variable
#108
Common Variable
All of these are variables are cleared either on
#109
Common Variable
#110
Common Variable
#111
Common Variable
#112
Common Variable
#113
Common Variable
#114
Common Variable
#115
Common Variable
#116
Common Variable
#117
Common Variable
#118
Common Variable
Variable List > Variable List
reset, at the end of the program or at power off.
Page 46
www.cncdata.co.uk 45
Variable
Description
Variable
Description
#500
Common Variable
#1013
PMC Bit Read
#501
Common Variable
#1014
PMC Bit Read
#502
Common Variable
#1015
PMC Bit Read
#503
Common Variable
#1032
PMC Word Read
#504
Common Variable
#505
Common Variable
#1100
PMC Bit Write
#506
Common Variable
#1101
PMC Bit Write
#507
Common Variable
#1102
PMC Bit Write
#508
Common Variable
#1103
PMC Bit Write
#509
Common Variable
#1104
PMC Bit Write
#510
Common Variable
#1105
PMC Bit Write
#511
Common Variable
#1106
PMC Bit Write
#512
Common Variable
#1107
PMC Bit Write
#513
Common Variable
#1108
PMC Bit Write
#514
Common Variable
#1109
PMC Bit Write
#515
Common Variable
#1110
PMC Bit Write
#516
Common Variable
#1111
PMC Bit Write
#517
Common Variable
#1112
PMC Bit Write
#518
Common Variable
#1113
PMC Bit Write
#519
Common Variable
#1114
PMC Bit Write
#520
Common Variable
#1115
PMC Bit Write
#521
Common Variable
#1132
PMC Word Write
#522
Common Variable
#1133
PMC Double Word Write
#523
Common Variable
#524
Common Variable
#525
Common Variable
#526
Common Variable
#527
Common Variable
#528
Common Variable
#529
Common Variable
#530
Common Variable
#531
Common Variable
#1000
PMC Bit Read
#1001
PMC Bit Read
#1002
PMC Bit Read
#1003
PMC Bit Read
#1004
PMC Bit Read
#1005
PMC Bit Read
#1006
PMC Bit Read
#1007
PMC Bit Read
#1008
PMC Bit Read
#1009
PMC Bit Read
#1010
PMC Bit Read
#1011
PMC Bit Read
#1012
PMC Bit Read
Variable List > Variable List
Page 47
www.cncdata.co.uk 46
Variable
Description
Variable
Description
#3000
Alarm & Stop
#4119
Modal S Code
#3001
Timer (m/s)
#4120
Modal T Code
#3002
Timer (hourly)
#4130
Modal P Code
#3003
Single Block
#3004
Feed control
#5001
Workpiece Position 1st Axis (B)
#3005
:
:
#3006
Operator Message
#5008
Workpiece Position 8th Axis (B)
#3007
#5021
Machine Position 1st Axis
#3008
:
:
#3009
#5028
Machine Position 8th Axis
#3010
#5041
Workpiece Position 1st Axis (C)
#3011
Date :
:
#3012
Time #5048
Workpiece Position 8th Axis (C)
#5061
Skip Signal Position 1st Axis
#3901
Machine Parts
:
:
#3902
Required Parts
#5068
Skip Signal Position 8th Axis
#4001
Modal Group 1
#5201
1st Axis EXT Zero Offset
#4002
Modal Group 2
:
:
#4003
Modal Group 3
#5208
8th Axis EXT Zero Offset
#4004
Modal Group 4
#5221
1st Axis G54 Zero Offset
#4005
Modal Group 5
:
:
#4006
Modal Group 6
#5228
8th Axis G54 Zero Offset
#4007
Modal Group 7
#5241
1st Axis G55 Zero Offset
#4008
Modal Group 8
:
:
#4009
Modal Group 9
#5248
8th Axis G55 Zero Offset
#4010
Modal Group 10
#5261
1st Axis G56 Zero Offset
#4011
Modal Group 11
:
:
#4012
Modal Group 12
#5268
8th Axis G56 Zero Offset
#4013
Modal Group 13
#5281
1st Axis G57 Zero Offset
#4015
Modal Group 15
#5288
8th Axis G57 Zero Offset
#4016
Modal Group 16
#5301
1st Axis G58 Zero Offset
#4017
Modal Group 17
:
:
#4018
Modal Group 18
#5308
8th Axis G58 Zero Offset
#4019
Modal Group 19
#5321
1st Axis G59 Zero Offset
#4020
Modal Group 20
:
:
#4021
Modal Group 21
#5328
8th Axis G59 Zero Offset
#4022
Modal Group 22
#4102
Modal B Code
#4107
Modal D Code
#4109
Modal F Code
#4111
Modal H Code
#4113
Modal M Code
#4114
Modal Sequence No
#4115
Modal Program No
Variable List > Variable List
#4014 Modal Group 14 : :
Loading...