Content      ..     21      22      23      24     ..

9/Series CNC Lathe. Operation and Programming Manual - page 23

Chapter 26

Drilling Cycles

Figure 26.14

G88: Boring Cycle, Spindle Stop/Manually Out

Cutting feed

Rapid feed

Manual operation

R point level

Initial point

level

Hole bottom

1

3

2

Z

R

4

Spindle or live tool stops at

hole bottom after dwell

5

6

Cycle start

7

Spindle rotation in

the forward direction

In the G88 boring cycle, the control moves the axis in this manner:

1.

The tool rapids to the initial point level above the hole location.

2.

The boring tool then rapids to the R point level, slows to the

programmed cutting feedrate and begins the boring operation.

3.

The boring tool bores at the programmed feedrate until it reaches the

depth specified with the Z-word.

4.

If the user has entered a value for the P parameter, the boring tool

dwells after it reaches the bottom of the hole.

5.

After the tool reaches the Z depth, the spindle or live tool stops

revolving. At this point, the operator must perform a manual

retraction of the drilling axis as described in chapter 4.

(Press

<CYCLE START> to return the control to automatic mode.)

26-35

Chapter 26

Drilling Cycles

6.

The boring tool is then retracted at a rapid feedrate to initial point

level, as determined by G98.

7.

At this point, the rotation of the spindle or live tool changes to the

clockwise direction.

When the single block function is active, the control stops axis motion

after steps 1, 2 and 5.

(G89): Boring Cycle,

The operations in G89 are identical to as those of the G85 boring cycle

with the exception that the control executes a dwell at hole bottom.

Dwell/Feed Out

The format for the G89 cycle is:

G89X__Z__R__P__F__L__;

Where :

Is :

X

specifies location of the hole.

Z

defines the hole bottom.

R

defines the R point level.

P

defines the dwell period at hole bottom.

F

defines the cutting feedrate.

L

defines the number of times the drilling cycle is repeated.

See page 26-7 for a detailed description of these parameters.

Important: The programmer or operator must start spindle or live tool

rotation.

26-36

Chapter 26

Drilling Cycles

Figure 26.15

G89: Boring Cycle, Dwell/Feed Out

Cutting feed

Rapid feed

R point level

Initial point

level

Hole bottom

1

4

3

2

Z

R

Dwell

5

6

In the G89 boring cycle, the control moves the axes in this manner:

1.

The tool rapids to initial point level above the hole location.

2.

The boring tool then rapids to the R point level, slows to the

programmed cutting feedrate and begins the boring operation.

3.

The boring tool bores at the programmed feedrate until it reaches the

depth of the hole specified by the Z-word.

4.

If the user has entered a value for the P parameter, the boring tool

dwells after it reaches the bottom of the hole.

5.

The control retracts the boring tool at the cutting feedrate to the R

point level.

6.

The boring tool accelerates to the rapid feedrate and retracts to the

initial point level.

When the single block function is active, the control stops axis motion

after steps 1, 2 and 5.

26-37

Chapter 26

Drilling Cycles

2.

Press the {PRGRAM PARAM} softkey.

(softkey level 2)

PRGRAM

AMP

DEVICE

MONI-

TIME

PARAM

SETUP

TOR

PARTS

PTOM

SYSTEM

SI/OEM

TIMING

3.

Press the {DRLCYC PARAM} softkey. The Drilling Cycle

Parameter screen is displayed. Figure 26.16 shows a typical Drilling

Cycle Parameter screen.

(softkey level 3)

ZONE

F1-F9

DRLCYC

INTERF

LIMITS

PARAM

CHECK

Figure 26.16

Drilling Cycle Parameter Screen

ENTER VALUE:

DRILLING CYCLE PARAMETERS

G83.1 DEEP HOLE PECK DRILLING CYCLE

RETRACT AMOUNT

1.000 [ MM]

G83 DEEP HOLE DRILLING CYCLE

CLEARANCE AMOUNT

1.270 [ MM]

G86.1/G87 FINE/BACK BORING CYCLE

G18

SHIFT DIRECTION

+Z

G92/G78/G21 SINGLE THREADING CYCLE

PULLOUT DISTANCE

5.1

[THRD]

PULLOUT ANGLE

5

[DEG]

REPLCE

ADD TO

UPDATE

QUIT

VALUE

VALUE

& EXIT

Important: Parameter values are displayed in inch or metric depending on

which is the currently active program mode.

26-39

Chapter 26

Drilling Cycles

4.

From this screen select the parameter that it is desired to change by

pressing the up or down cursor keys. The selected parameter is

shown in reverse video.

5.

There are two options:

To replace the current value of the parameter with a new value,

key in the new value on the input line of the CRT and press the

{REPLCE VALUE} softkey. The new value replaces the old

value.

To add an amount to the current value of the parameter, key in the

amount to add to the current parameter value on the input line of

the CRT and press the {ADD TO VALUE} softkey. The value just

keyed in is then added to the old value for the selected parameter.

6.

To leave the Drilling Cycle Parameter screen, there are two options:

To save the changes just made to the parameters and leave the

Drilling Cycle Parameter screen press the {UPDATE & EXIT}

softkey.

To discard any changes just made to the parameters and leave the

Drilling Cycle Parameter screen, press the {QUIT} softkey.

(softkey level 4)

REPLCE

ADD TO

UPDATE

QUIT

VALUE

VALUE

& EXIT

26.6

The following are example programs and an illustration of G83, deep hole

Examples of Drilling Cycles

drilling cycle. Example 27.2 is in incremental mode; Example 27.3 is in

absolute. Figure 26.17 illustrates the result for both programs individually.

Example 27.2

Programming G83, Deep Hole Drilling Cycle in Incremental Mode

N10

M19 S0;

N20

G00 X5 Z0 G90;

N30

G83 X1 Z3 R5 Q1.5 F.1

N40

M19 S90;

N50

Z3;

N60

M30;

26-40

Chapter 26

Drilling Cycles

Example 27.3

Programming G83, Deep Hole Drilling Cycle in Absolute Mode

N10

G90 G00 X5 Y12 Z0 G17 F200;

N20

G83 X1 Y10 Z-5 R-2 Q1.5;

N30

X5 Y5 Z-8;

N40

X9 Y10 Z-5;

N50

M30;

Figure 26.17

Result of Example 27.2 and Example 27.3

N20

( 5,3 )

( 5,0 )

Second Hole

N30

90°Spindle

N50

( 1,3 )

First Hole

END OF CHAPTER

26-41

Chapter

27

Skip and Gauge Probing Cycles

27.0

This chapter describes the external skip and gauging functions available on

the 9/Series control. External skip functions are motion generating G-code

Chapter Overview

blocks that can be aborted when the control receives an external signal

through the PAL program. Gauging functions are similar to the external

skip functions except that the axis coordinates (at the time the external

signal is received) can be used to modify the tool offset table.

This chapter describes theses major topics in detail.

Topic:

On page:

External skip functions

27-2

Tool gauging external skip function

27-3

Important: The G04 dwell feature may also be enabled as an external skip

or tool gauging command. For details on programming a G04, see chapter

14.

The 9/Series control provides several means of triggering an external skip

or gauging block:

discrete inputs on the I/O ring

any one of the four available “high speed inputs”

a “probe” input that directly latches the feedback counters

These inputs, each with different degrees of precision, may be used to

signal the control to store the current axes positions. See the

documentation prepared by your system installer for details on your

specific machine.

These conditions must be satisfied when an external skip or gauging bock

is executed:

cutter compensation must be disabled (G40 mode) when the block is

executed

the block that contains the external skip G-code (excluding G04 as

external skip) must be a linear block.

27-1

Chapter 27

Skip and Gauge Probing Cycles

CAUTION: We do not recommend using a skip block from any

fixed cycle block (such as drilling or turning). If you do choose

to execute a skip block in a fixed cycle mode, be aware that the

block that is skipped when the trigger occurs can be a cycle

generated block. If this is the case the cycle will continue

normal execution skipping only the portion of the cycle that was

executing when the trigger occurred. If the generated block

skipped is a crucial portion of the cycle, damage to the part or

machine tool can occur.

27.1

Use external skip functions to terminate the execution of motion

External Skip

commands in a block when the control receives a signal through PAL.

When the program block is terminated any remaining axis motion

Functions (G31

codes)

generated by the block that has not been performed remains unexecuted

(other non-motion commands are still performed). The control continues

normal program execution at the beginning of the next block following the

skipped block.

The external skip function is controlled by G31, G31.1, G31.2, G31.3, and

G31.4. The system installer determines what signal (such as a touch probe,

manual switch, etc.) corresponds to each G31 code in PAL. The system

installer can choose different signals to correspond to G31.2, G31.3, and

G31.4. G31 and G31.1 are functionally the same, always using the same

external signal and the same AMP defined feedrate. With proper PAL

programming, a G04 dwell in seconds may also be used as an external

skip function.

Format for any G31 external skip blocks is:

G31 X__ Z__ F__;

Where :

Is :

G31

Any of the G-codes in the G31 series or G04. Use the one that is configured to

respond to the current external skip signal device that is being used.

X, Z

The endpoint of the move if no external skip signal is received. These also

determine the direction that the tool travels in.

F

The external skip function feedrate. If no value is entered here, the external skip

function executes at either the currently active feedrate, or the feedrate defined

for it in AMP (based on whether the AMP parameter Use AMP Skip Feedrate is

set to ”NO”or ”YES”). A value entered here replaces the currently active

feedrate and supersedes the AMP defined feedrate.

The G31 series of G-codes always produce linear motion regardless of the

current mode active at their execution. After their completion the control

returns to the operating mode active before the external skip block was

read (G00, G01, G02, G03).

27-2

Chapter 27

Skip and Gauge Probing Cycles

The format for any G37 skip blocks is:

G37 Z__ F__;

Where :

Is :

G37

Corresponds to any of the G-codes in the G37 series. Use the one that is

configured to respond to the current skip signal device that is being used.

X, Z

The axis on which the length offset measurement is to be taken is specified here

as either X or Z. Only one axis may be specified in a G37 block. The numeric

value following the axis name corresponds to the exact coordinate at which the

skip signal is expected to occur. This value is a signed value (+ or --) and

determines the initial direction of travel.

F

The tool gauging external skip function feedrate. If no value is entered here, the

external skip function executes at either the currently active feedrate or at the

feedrate defined for it in AMP (based on whether the AMP parameter Use AMP

Skip Feedrate is set to ”NO”or ”YES”). A value entered here replaces the

currently active feedrate and supersedes the AMP-defined feedrate.

Important: The G37 series G-codes cannot be used to modify the tool tip

radius values. Only the tool length offset values can be modified.

The target offset value for these gauging operations is determined by the

currently active tool offset number

CAUTION: If modifying a tool length offset, the offset value

generated with this gauging operation is immediately loaded

into the offset table. Since this offset must be the currently

active offset, it becomes effective either immediately when the

next block is executed or delayed until the next block that

contains motion on the tool length axis is executed (when an

offset is activated is determined in AMP by the system

installer).

The G37 series of G-codes always produce linear motion regardless of the

current mode active at their execution. After their completion, the control

returns to the operating mode active before the skip block was read (G00,

G01, G02, G03).

The system installer determines (in AMP) a position tolerance for the G37

functions. This tolerance defines a legal range before and after the

coordinate position programmed with the axis word in the G37 block.

If the skip signal is received before the tool enters or after the tool exits the

position tolerance range, a PROBE ERROR occurs. This error appears on

the screen as a warning but does not place the control in E-Stop. Instead

the G37 block is aborted and program execution proceeds to the next

block. No modification of the tool offset table is performed.

27-4

Chapter 27

Skip and Gauge Probing Cycles

Figure 27.1

Typical Tool Gauging Configurations

Tool

Tool

Tool

--X

--X

Probe

+Z

Probe

Probe

Probe

length

radius

radius

Probe

radius

Probe

Probe

Case 1

Case 2

Case 3

Figure 27.1 illustrates 3 typical tool gauging configurations. All 3 cases

assume that the probe is at a known, fixed point on the machine.

In Case 1, the Z axis tool offset length is being gauged, while in Case 2,

the X axis tool offset length is being gauged. In both cases:

only the probe tip radius is significant to the control in calculating the

offset adjustment

the reference position is the center of the probe ball

In Case 3, the X axis tool offset length is being gauged; and both the probe

radius and the probe length are significant to the control’s offset

adjustment calculations. In this case, the reference position is the bottom

of the probe.

Important: We do not recommend the tool gauging configuration Case 3

depicted in Figure 27.1 due to the risk of probe damage.

END OF CHAPTER

27-6

Chapter

28

Paramacros

28.0

The Paramacrost feature is similar to a subprogram with many added

features. Special features available with a paramacro include:

Chapter Overview

Computable variables

Computable word address fields in any block type

Variable to and from PAL

Access to certain modal system parameters for computations

Arithmetic operators and expressions for computations

Conditional Branching, Subroutines, and Subprogram calls based upon

logical function results

Parametric programs, Subroutines, and Subprograms

Parametric Autocycles

User-definable prompts to aid in program generation and execution

Prompting of parameters for main program execution

Calculator function under prompt edit

All of these features are valid in any block within a main program,

subprogram, or paramacro program. Most are permitted in an MDI

program unless otherwise stated; the only restriction being that no other

program commands, except other paramacro commands, may exist in a

block that contains paramacro commands. Macro and non-macro

commands may not exist in the same program block.

This chapter describes paramacros and and how to program them. Use this

table to find information:

Information on:

On page:

Parametric Expressions

28-2

Transfer of Control Commands

28-7

Parameter Assignments

28-12

Assigning Parameter Values

28-34

Backing Up Parameter Values

28-41

Macro Call Commands

28-42

Macro Output Commands

28-52

28-1

Chapter 28

Paramacros

28.1

It may be necessary for mathematical expressions to be evaluated in a

complex paramacro. This requires that some form of mathematical

Parametric Expressions

equation be written in a paramacro block. The following is a discussion of

the operators and function commands available for use on the control.

These operators and function commands are valid in any block within a

program, subprogram, paramacro, or MDI program.

28.1.1

This subsection lists the mathematical operators that are available on the

9/Series controller. Use these operators to accomplish mathematical

Basic Mathematical

operations that are necessary to evaluate the basic mathematical equation

Operators

such as addition, multiplication, etc. Table 18.A lists the operators and

their meanings.

Table 28.A

Mathematical Operators

Operator

Meaning

+

Addition

-

Subtraction

Multiplication

/

Division

[]

Brackets

OR

Logical OR

XOR

Logical Exclusive OR

AND

Logical AND

MOD

Modulus

The control executes a mathematical operation in this order:

1.

Any part of the expression between the brackets [] is evaluated first.

2.

Multiplication, division, and MOD are evaluated second.

3.

All other operations are evaluated third.

If the same level of evaluation is performed, the left-most operation takes priority.

28-2

Chapter 28

Paramacros

Example 28.1

Mathematical Operations

Expression entered

Result

12/4*3

9

12/[4*3]

1

12+2/2

13

[12+2]/2

7

12-4+3

11

12-[4+3]

5

All logical operators have the format of:

A logical operator B

where A and B are numerical data or a parameters with a value assigned.

If B is negative in the above format, an error will occur.

If A is negative, the absolute value of A is used in the operation and the

sign is attached to the final result.

Before evaluation, A and B are made integers by rounding and truncating.

Example 28.2

Logical Operation Examples

Expression Entered

Result

[16.2MOD3]

1.0

[-16.2MOD3]

-1.0

[-17.6MOD3]

0.0

[16.0MOD3]

1.0

[-5AND4]

-4.0

[4.4AND3.6]

4.0

[5AND-4]

ERROR

[83886079AND83886080]

67108864

28-3

Chapter 28

Paramacros

28.1.2

This subsection lists the basic mathematical functions that are available on

the control and their use. Use these functions to accomplish mathematical

Mathematical Function

operations that are necessary to evaluate the trigonometric and other

Commands

complex mathematical equation such as rounding off, square roots,

logarithms, exponent, etc. NO TAG lists the basic functions that are

available and their meanings.

Table 28.B

Mathematical Functions

Function

Meaning

SIN

Sine (degrees)

COS

Cosine (degrees)

TAN

Tangent (degrees)

ATAN

Arc Tangent (degrees)

ASIN

Arc Sine (degrees)

ACOS

Arc Cosine (degrees)

SQRT

Square Root

ABS

Absolute Value

BIN

Conversion from BCD to Decimal

BCD

Conversion from Decimal to BCD

ROUND

Rounding Off (nearest whole number)

FIX

Truncation Down

FUP

Truncation Up

LN

Logarithms (base e)

EXP

Exponent

When programming these functions, the value on which that function is to

be performed must be included in brackets: for example, SIN [10]. The

exception to this is the arc tangent function. The format to ATAN requires

the division of two values. For example, ATAN [10]/[2] is used to

calculate the arc tangent of 5.

The functions in NO TAG are executed from left to right in a program

block. These functions are executed before the control executes any

mathematical operators such as addition or subtraction. This order of

execution can be changed only by enclosing operations in brackets [].

Operations enclosed in brackets are executed first.

28-4

Chapter 28

Paramacros

Example 28.3

Format for Functions

SIN[2]

This evaluates the sine of 2 degrees.

SQRT[14+2]

This evaluates the square root of 16.

SIN[SQRT[14+2]]

This evaluates the sine of the square root of 16.

LN[#2+4]

This evaluates the logarithm of the value of parameter #2 plus 4.

Example 28.4

Mathematical Function Examples

Expression Entered

Result

SIN[90]

1.0

SQRT[16]

4.0

ABS[-4]

4.0

BIN[855]

357

BCD[357]

855

ROUND[12.5]

13.0

ROUND[12.4]

12.0

FIX[12.7]

12.0

FUP[12.2]

13.0

FUP[12.0]

12.0

LN[9]

2.197225

EXP[2]

7.389056

Important: Precaution must be taken when performing calculations within

the brackets [] following a mathematical function. The operations within

the bracket are performed first, and then the function is performed on this

resultant.

Example 28.5

Precaution for Order of Operation

N1#1=1.6;

Parameter #1 is set at 1.6

N2#2=2.8;

Parameter #2 is set at 2.8

N3#3=ROUND[#1+#2];

Parameter #3 is set at 4.0

Note that the values composing parameter #3 are added together first and

then rounded, not rounded and then added together.

28-5

Chapter 28

Paramacros

28.1.3

You can use parametric expressions to specify G-codes or M-codes in a

program block.

Parametric Expressions as

G- or M-Codes

For example:

G#1 G#100 G#500 M#1 M#100 M#500;

G#520 G[#521-1] G[#522+10] M#520 M[#522+1] M[#522+10];

When using a parametric expression to specify a G-- or M-code, remember:

When specifying more than one G-- or M-code in a block from the same

modal group, the G-- or M-code closest to the End-of-Block of that

block is the one activated. All others in that modal group are ignored.

Parametric expressions that generate G-- or M-codes used to call a

paramacro are invalid. If the result of the paramacro expression for a

G-code is 65, 66, 66.1, or any AMP-defined G-code, the error

“ILLEGAL G-CODE” appears. If the result of the paramacro

expression for an M-code is any AMP-defined M-code, the control will

not execute the macro but interpret the M--code as either a system

defined M--code or a user defined M--code. No error is generated.

To get the G-- or M-code value, the system will truncate, after the tenths

position, the result of the mathematical expression. The following

example assumes #1=37.0:

This Block

Generates This G-Code

G#1

G37.0

G[#1+0.32]

G37.3

G[#1+0.49]

G37.4

Illegal Paramacro Commands

It is possible to call subprograms or paramacros within an MDI program,

however, there are limitations to the allowable commands. The following

lists examples of illegal MDI commands for these features:

G66

G66.1

G67

DO--END

WHILE--DO--END

GOTO

IF--GOTO

M99

Amp--defined Modal G--code Macro Calls

Attempting to use any of the above as MDI commands, 9/Series generates

an “ILLEGAL MACRO CMD VIA MDI” error message.

28-6

Chapter 28

Paramacros

28.2

Use transfer of control commands to alter the normal flow of program

execution. Normally the control executes program blocks sequentially.

Transfer of Control

By using control commands, the programmer can alter this normal flow of

Commands

execution and transfer execution to a specific block or begin looping

(executing the same set of blocks repetitively).

Important: Transfer of control commands call a block by its N number. If

more than one N number exists in a block, the control uses only the

left-most N number in that block. If the same N number is used for more

than one block, the control will use the first block it encounters with the

correct N number (the control searches in the forward direction first, then

starts at the top of the program).

Two types of transfer of control commands are available:

Conditional ---- The execution of a jump or loop is dependant on

whether a mathematical condition is true.

Non-Conditional ---- The execution of a jump or loop is always

performed when that block is executed.

28.2.1

This section describes conditional operators that are available for

paramacro programming. A conditional operator causes a comparison

Conditional Operators

between two values and yields a result of true or false. Use conditional

operators in “IF” or “WHILE” commands as described on page 28-9 and

28-10.

Use the true or false condition to determine whether the “IF” or “WHILE”

blocks are executed. NO TAG lists the conditional operators available for

paramacro programming:

Table 28.C

Conditional Operators

Operator

Condition Tested

EQ

Equal

NE

Not Equal

GT

Greater Than

LT

Less Than

GE

Greater Than or Equal

LE

Less Than or Equal

28-7

Chapter 28

Paramacros

Program a condition between the [ and ] brackets in this format:

[A EQ B]

where A and B represent some numerical value. The values for A and B

can be in the form of some mathematical equation or in the form of a

paramacro parameter.

Example 28.6

Evaluation of Conditional Expressions

Expression

Evaluation

[6.03 EQ 6.0301]

FALSE

[6.03 NE 6.0301]

TRUE

[2.5 GT 2.5]

FALSE

[2.5 LT 2.51]

TRUE

[2.51 GE 2.5]

TRUE

[2.5 LE 2.5]

TRUE

[[2.5-3] LE 1]

TRUE

[#1 GT #2]

This depends on the value of the parameters #1 and #2

For details on the use of conditional expressions, refer to page 28-9 on

“IF” statements and page 28-10 on “WHILE” statements. For details on

the use of paramacro parameters, refer to page 28-12.

28.2.2

Unconditional GOTO

GOTO and IF-GOTO

Any time the control executes a GOTO block, the unconditional GOTO

Commands

command automatically transfers control.

Use this format for the GOTO command:

GOTO n;

Where :

Is:

n

Execution is transferred to the block with the sequence number specified as n

any time that the GOTO block is executed.

28-8

Chapter 28

Paramacros

Example 28.7

Unconditional GOTO

N1...;

N2...;

N3GOTO5;

N4...;

N5...;

N6...;

/N7GOTO1;

In Example 28.7, execution continues sequentially until block N3 is read;

then execution transfers to block N5 and again resumes sequential

execution to block N6. If optional block skip 1 is off, block N7 will

transfer execution back to block N1.

Conditional IF-GOTO

The conditional IF-GOTO command is dependent on whether a

mathematical condition is true. If this condition is true, execution will

transfer to the block specified.

Use this format for the IF-GOTO command:

IF [(condition)] GOTO n;

Where :

Is :

(condition)

some mathematical condition. This condition is tested by the control to determine if

it is true or false.

n

if the condition is tested as true, execution is transferred to the block specified as n

If the condition is tested as false, execution falls through the block and the

GOTO is not executed. Program execution continues in a normal fashion.

Example 28.8

Conditional IF

N1...;

N2IF[#3EQ-1.5]GOTO5;

N3...;

N4...;

N5...;

N6IF[#4LT3]GOTO1;

N7...;

28-9

Chapter 28

Paramacros

Use this format for the WHILE-DO-END command:

WHILE [ (condition) ] DO m;

;

;

;

END m;

Where :

Is :

(condition)

some mathematical condition. This condition is tested by the control to

determine if it is true or false.

m

an identifier used by the control to relate a DO block with an END block. The

value of m must be the same for the DO as it is for the corresponding END. This

value can be either 1, 2, or 3.

All blocks between the DO and the END command are executed until the

condition is tested as false. This set of blocks is referred to as a

WHILE-DO-END program segment.

When the condition for the WHILE-DO block is tested as false, execution

is then transferred to the block immediately following the END statement

block.

Example 28.9

WHILE-DO-END Program Segment

N1 #1=1;

N2WHILE[#1LT10]DO1

N3#1=[#1+1];

N4...;

N5...;

N6END1;

N7...;

In Example 28.9, blocks N2 through N6 are executed 9 times. At that

time, the condition in block N2 becomes false, and program execution is

transferred to block N7.

Nesting is possible with a WHILE-DO-END command. Nesting is defined

here as one WHILE-DO-END program segment executing within another

WHILE-DO-END program segment. WHILE-DO-END nesting is limited

to 3 independent segments at one time.

28-11

Chapter 28

Paramacros

Example 28.11

Assigning Using More Than One I, J, K Set

G65P1001K1I2J3J4J5;

The above block sets the following parameters:

parameter #6 = 1

parameter #7 = 2

parameter #8 = 3

parameter #11 = 4

parameter #14 = 5

If the same parameter is assigned more than one value in an argument, only

the right-most value is stored for the parameter.

Example 28.12

Assigning the Same Parameter Twice

G65P1001R3.1A2R-0.5

The above block sets the following parameters:

parameter #1 = 2.0 As set by the A--word

parameter #18 = -0.5 As set by the last R--word.

The 1st value of 3.1, assigned to parameter #18 by the R--word, is

replaced by the 2nd value set by the second R--word.

Example 28.13

Assigning The Same Parameter Twice Using I, J, and K

G65P1001R2I3.4D5I-0.6

The above blocks set the following parameters:

parameter #18 = 2 As set by the R--word.

parameter #4 = 3.4 As set by the 1st I--word.

parameter #7 = -0.6 As set by the 2nd I--word.

The 1st value of 5, assigned to parameter #7 by the D--word,

is replaced by the 2nd value set by the second I--word.

28-14

Chapter 28

Paramacros

Table 28.D

System Parameters

Parameter #

System Parameter

Page

2001 to 2999

Tool Offset Tables

28-17

3000

² Program Stop With Message (PAL)

28-17

3001

System Timer (PAL)

28-18

3002

System Clock

28-18

3003

² Block Execution Control 1

28-19

3004

² Block Execution Control 2

28-19

3006

² Program Stop With Message

28-20

3007

¹ Mirror Image

28-20

4001 to 4120

¹ Modal Information

28-21

5001 to 5012

¹ Coordinates of End Point

28-22

5021 to 5032

¹ Coordinates of Commanded Position

28-22

5041 to 5052

¹ Machine Coordinate Position

28-23

5061 to 5069 or

¹ Skip Signal Position (Work Coordinate)

28-23

5541 to 5552

5071 to 5079 or

¹ Skip Signal Position (Machine Coordinates)

28-24

5561 to 5572

5081 to 5089 or

¹ Active Tool Length Offsets

28-25

5581 to 5592

5095 to 5096

Probe Stylus Length and Radius

28-25

5101 to 5112

¹ Current Following Error

28-25

5201 to 5212

External Offset Amount

28-26

5221 to 5232

G54 Work Coordinate Table Value

28-26

5241 to 5252

G55 Work Coordinate Table Value

5261 to 5272

G56 Work Coordinate Table Value

5281 to 5292

G57 Work Coordinate Table Value

5301 to 5312

G58 Work Coordinate Table Value

5321 to 5332

G59 Work Coordinate Table Value

5341 to 5352

G59.1 Work Coordinate Table Value

5361 to 5372

G59.2 Work Coordinate Table Value

5381 to 5392

G59.3 Work Coordinate Table Value

5630

¹ S--Curve Time per Block

28-28

5661 to 5642

¹ Acceleration Ramps for Linear Acc/Dec Mode

28-29

5651 to 5662

¹ Deceleration Ramps for Linear Acc/Dec Mode

28-28

5671 to 5682

¹ Acceleration Ramps for S--Curve Acc/Dec Mode

28-30

5691 to 5702

¹ Deceleration Ramps for S--Curve Acc/Dec Mode

28-29

5711 to 5722

¹ Jerk

28-30

28-16

Content      ..     21      22      23      24     ..