Content      ..     10      11      12      13     ..

9/Series CNC Lathe. Operation and Programming Manual - page 12

Chapter 12

Overtravels and Programmable Zones

12.2

The coordinate values of the points defining the software overtravels are

set in AMP by your system installer. This overtravel can only be disabled

Software Overtravels

by your system installer in AMP. If your system installer has enabled the

software overtravels, the control is not allowed to exit the area defined by

the software overtravels.

Figure 12.2

Software Overtravels Established in AMP

Hardware

overtravel

Entry into this

area is prohibited by

the software overtravel

Cutting

tool

Software

overtravel

Absolute position is prohibited

from entering the software

overtravel (no offsets considered)

Your system installer selects values that represent a maximum and a

minimum value in the form of coordinate values for each axis. These

coordinate values define points on the machine coordinate system. The

axes are not allowed to move past the coordinate value representing the

maximum and minimum value on each axis. This limited range of motion

is referred to as the software overtravels.

12-3

Chapter 12

Overtravels and Programmable Zones

Figure 12.3

Area Defining Software Overtravel

X

Software overtravel area as defined in AMP by minimum and

maximum axis values

Max X

value

Machine

coordinate

zero

Z

Min X

value

Max Z

Min Z

value

value

Typically the software overtravels are located within the hardware

overtravels (maximum axis travel defined by the limit switches on each

axis), and they are used to keep the axes within the range your system

installer determines is usable for that particular machine’s application.

The area defined by the software overtravels becomes effective after

completion of the initial homing operation at power up. For details on how

the control reacts to a entry into an overtravel area, see page 12-13.

CAUTION: The area defined by a software overtravel does not

take in to account any offsets. This allows the actual tool to

enter the restricted area without the axes absolute position

entering it. Make sure this is considered when the software

overtravel is established.

12-4

Chapter 12

Overtravels and Programmable Zones

12.3

Programmable zone 2 defines an area which the tool cannot enter.

Generally, zones are used to protect some vital area of the machine or part

Programmable Zone 2

located within the software overtravels.

Important: Programmable zones are defined using coordinates in the

machine coordinate system. They are not affected by any changes in the

work coordinate system, including external offsets.

WARNING: Programmable zones only protect the tool tip

from entering the zone (as determined with the currently active

tool length offset). They do not protect other moving members

from collision with objects in the programmable zone’s

boundary.

Values for programmable zone 2 are entered in the programmable zone

tables as described on page NO TAG. These values represent a maximum

and a minimum value in the form of machine coordinate values for each

axis. The area defined by these points establishes the boundaries for

programmable zone 2.

Figure 12.4

Area Defining Programmable Zone 2

X

Max X

value

Programmable Zone 2

as defined by minimum

and maximum axis values

Min X

value

Machine

coordinate

zero

Z

Min Z

Max Z

value

value

Important: When changing a tool offset or activating a programmable

zone 2, the current tool tip location must be outside of the area defined by

programmable zone 2.

12-5

Chapter 12

Overtravels and Programmable Zones

Programming

turns Zone 2:

turns Zone 3:

this G-code:

G22

On

On

G22.1

Off

On

G23

Off

Off

G23.1

No Change*

Off

* A G23.1 turns on programmable zone 2 ifitis the default

power up condition configured in AMP (also activated at a

control reset). G23.1 does not turn on programmable zone 2

when it is activated in a part program.

G23 is normally automatically made active at power up, though this is

ultimately determined by the system installer in AMP. Your system

installer also determines in AMP if an M02 or M30, control reset, or

E-STOP reset cancels programmable zones that you have turned on or off

while executing your program.

Important: If you program a G22, any axis words included in the block

are stored as the coordinates for programmable zone 3. See page 12-7 .

If you attempt to program some other command in a G22 or G23 block, for

example:

G22 G01 X12.;

the control issues the error message:

“UNUSABLE WORDS IN ZONE BLOCK”

12-6

Chapter 12

Overtravels and Programmable Zones

Figure 12.5

Programmable Zone 2

Software overtravel

Tool tip can not

Programmable

enter zone 2

Zone 2

For details on how the control reacts to entry into a prohibited area, see

page 12-13.

12.4

Programmable zone 3 can define an area which the tool cannot enter or

an area the tool cannot exit. The current tool location determines when

Programmable Zone 3

programmable zone 3 is made active. Generally, zones are used to protect

some vital area of the machine or part located within the software

overtravels.

Important: Programmable zones are defined using coordinates in the

machine coordinate system. They are not affected by any changes in the

work coordinate system, including external offsets.

WARNING: Programmable zones only protect the tool tip

from entering the zone (as determined with the currently active

tool length offset). They do not protect other moving members

from collision with objects in the programmable zone’s

boundary.

12-7

Chapter 12

Overtravels and Programmable Zones

Values for programmable zone 3 are entered either in the programmable

zone table (described on page NO TAG) or through a G22 program block.

A maximum and a minimum coordinate value (in the machine coordinate

system) are assigned for each axis. The resulting coordinates define the

boundaries for programmable zone 3.

Figure 12.6

Area Defining Programmable Zone 3

Inside or outside border of

X

Programmable Zone 3

as defined by minimum

and maximum axis values

Max X

value

Tool tip can not

Tool tip can not enter if

exit if zone is activated

zone is activated while

while tool is inside zone.

tool is outside zone.

Min X

value

Machine

coordinate

zero

Z

Min Z

Max Z

value

value

Unlike the software overtravels and programmable zone 2, programmable

zone 3 can define either an area that the cutting tool can not exit or an area

that the cutting tool can not enter. This is determined by the current tool

location when programmable zone 3 is made active.

The software overtravels: define an area that the cutting tool may not

exit if the tool is currently inside the zone when the zone is activated.

Programmable Zone 3: defines an area that the cutting tool cannot enter

if the tool is outside the zone when activated or: defines an area that the

cutting tool cannot exit if the tool is inside the zone when activated.

12-8

Chapter 12

Overtravels and Programmable Zones

Figure 12.7

Programmable Zone 3

This area becomes Programmable

Zone 3 if the zone is enabled

when tool is inside of this area

Programmable Zone 3

if enabled when tool

is outside of this area

Programmable zone 3 becomes active when either the G22 or G22.1 code

is executed. It is made inactive when the G23 or G23.1 code is executed.

Program

To turn on

To turn off

G-code:

these zones:

these zones:

G22

2 and 3

not applicable

G22.1

3

2

G23

not applicable

2 and 3

G23.1

2*

3

* A G23.1 only turns on programmable zone 2 ifitis

activated via a control reset or power up condition.

G23.1 does not turn on programmable zone 2 if it is

programmed. To turn on programmable zone 2 and

turn off programmable zone 3, first program a G22

followed by a G23.1 to turn off programmable zone

3. Programming G23.1 has no affect on zone 2.

G22.1 and G23.1 are modal (G22.1 cancels G23.1, and G23.1 cancels

G22.1).

Important: G22.1, G23, and G23.1 must be programmed in blocks

without other commands. If you program a G22, any axis words included

in the block are stored as the coordinates for programmable zone 3.

12-9

Chapter 12

Overtravels and Programmable Zones

If you program other commands other than a G-code in the same modal

group in a G22, G22.1, G23, or G23.1 block, this error message appears:

“UNNECESSARY WORDS IN ZONE BLOCK”

Programming zone 3 values (3 or less axes)

You can reassign values for the parameters that establish programmable

zone 3 by programming axis words in a G22 program block. Two methods

are available. This section discusses programming values for zone 3 when

3 or less axes have been configured on the system (this does not include

any spindle).

Define values for programmable zone 3 using the G22 command followed

by axis words in the following format:

G22 X__ Z__ U__ I__ K__ J__;

Where:

Defines:s

Absolute axis words

maximum zone limits

(normally X, Z, and U)

Integrand words

minimum zone limits

(normally I, K, and J)

These axis words can vary. Refer to your system installer’s

documentation. The following example assumes a three axis lathe

configuration. Absolute axis names are X, Z, and U. Integrands for these

axis words are I, K, and J respectively.

This block:

Results in:

G22 X10 I--10 Z14 K--14 U1 J--1;

upper and lower zone 3 limits for X, Z, and U axes

are changed. Zones 2 and 3 are both activated,

G22 X10 Z10 U20;

upper zone 3 limits are changed for X, Z, and U

axes. Zones 2 and 3 are both activated.

G22 I--10 Z10 K--5 J--3;

lower zone 3 limits for X and U axes are changed.

Both upper and lower limits for Z axis zone 3 are

changed. Zones 2 and 3 are both activated.

G22 K--10;

lower zone 3 limit for Z axis is changed. Zones 2

and 3 are both activate.

The zone values entered in a G22 block always reference coordinate values

in the machine coordinate system.

12-10

Chapter 12

Overtravels and Programmable Zones

If a value for a maximum axis parameter is less than the value set for an

axis current minimum parameter, or if a value for a minimum axis

parameter is set greater than the value set for an axis current maximum

value, the control displays the message:

“INVALID VALUE (MAX < MIN) FOR ZONE 3 AXIS (X)”

This message displays the name of the axis that has been set incorrectly. It

does not indicate if it is the minimum or maximum value that is incorrect.

If the same integrand word is assigned in AMP by the system installer to

more than one axis, that integrand word will set the lower zone 3 limit for

all axes with that integrand.

Programming zone 3 values (4 or more axes)

You can reassign values for the parameters that establish programmable

zone 3 by programming axis words in a G22 program block. Two methods

are available. This section discusses programming values for zone 3 when

4 or more axes have been configured on the system (this does not include

any spindle).

This method differs from the three axis method in that the same integrands

can be used again for different axes (necessary since the control only

supports three integrand words). Assume the following AMP

configuration:

Absolute Axis name

X

Y

Z

U

V

W

A

B

C

Axis Integrand

I

J

K

I

J

K

I

J

K

These axis words can vary. Refer to your system installer’s

documentation.

Define values for programmable zone 3 using the G22 command followed

by axis words in the following format:

G22 X__ Y__ Z__ I__ J__ K__;

G22 U__ V__ W__ I__ J__ K__;

G22 A__ B__ C__ I__ J__ K__;

Where:

Defines:

Absolute axis words

maximum zone limits

Integrand words

minimum zone limits

(normally I, J, and K)

12-11

Chapter 12

Overtravels and Programmable Zones

Using this method, the same integrand word assigned in AMP to more than

one axis correspond only to the absolute axis words programmed in the

G22 block. Integrand words cannot be programmed alone (without a

absolute axis word in the G22 block). The following example assumes a

machine with axes configured as shown above.

These blocks:

Results in:

G22 X10 I--10 Y14 J--14 Z1 K--1;

upper and lower zone 3 limits for all 9 axes are

G22 U5 I--5 V13 J--2 W11 K10;

changed. Zones 2 and 3 are both activated when

G22 A3 I2 B7 J--7 C12 K11;

the first block in this series of blocks is executed.

G22 X1 Y2 Z3 U4 V5 W6 A7 B8 C9;

upper zone 3 limits are changed for all 9 axes.

Zones 2 and 3 are both activated.

G22 X1 Y2 Z3 U4 V5 W6 A7 B8 C9 I--1 J--2 K--3;

upper and lower zone 3 limits for all 9 axes are

changed. (I sets lower for X, U, and A: J sets

lower for Y, V, and B: K sets lower limits for Z, W,

and C). Zones 2 and 3 are both activate.

G22 K--10;

error is generated. Current status of zones

remains in current state (on or off).

WARNING: When using multiple blocks to set the zone 3

limits, keep in mind zone 3 is activated after the first G22 block.

This will result in zone 3 being activated before you have

completed changes to the zone 3 values. This can cause the

control to miss-interpret zone 3 as an internal or external zone,

depending on the tool location at the time of the zone activation.

The zone values entered in a G22 block always reference coordinate values

in the machine coordinate system.

If a value for a maximum axis parameter is less than the value set for an

axis current minimum parameter, or if a value for a minimum axis

parameter is set greater than the value set for an axis current maximum

value, the control displays the message:

“INVALID VALUE (MAX < MIN) FOR ZONE 3 AXIS (X)”

This message displays the name of the axis that has been set incorrectly. It

does not indicate if it is the minimum or maximum value that is incorrect.

12-12

Chapter 12

Overtravels and Programmable Zones

12.5

Tool motion stops during overtravel conditions that occur from 3 causes:

Resetting Overtravels

Cause:

Description:

Hardware overtravel

the axes reach a travel limit, usually set by a limit switch or sensor

mounted on the axis. Hardware overtravels are always active.

Software overtravel

commands cause the axis to pass a software travel limit. Software

overtravels are active only after the axis has been homed provided the

feature has been activated in AMP by the system installer.

Programmable zone

The tool reached a travel limit established by independent

overtravel

programmable areas. Programmable Zones are activated through

programming the appropriate G-code.

In all cases, the control issues an error message.When an overtravel

condition occurs, all axis motion stops, the control goes into cycle stop and

one of the these error messages appears.

Error Message:

Description:

HARDWARE OVERTRAVEL

indicates that the specified axis has tripped either the + or -

(-) BY AXIS (X)

hardware limit switch mounted on the machine.

SOFTWARE OVERTRAVEL

indicates that the specified axis has entered the overtravel

(+) BY AXIS (X)

area defined by the software overtravel limits in either a

positive or negative direction.

VIOLATION OF ZONE (2) BY

indicates that a tool has reached the specified axis overtravel

AXIS (X)

area defined by either programmable zone 2 or 3.

When an overtravel of any type occurs, axes cannot move in the same

direction as the feed causing the overtravel. Only axis motion in the

reverse direction is possible.

How a hardware overtravel condition is reset depends on the E-Stop circuit

design and the way PAL was programmed by your system installer.

To reset a software or programmable zone overtravel condition:

1.

Determine whether the control is in E-Stop. If it is not, go to step 4.

2.

Eliminate any other possible conditions that may have caused an

emergency stop, then make sure that it is safe to reset the emergency

stop condition.

3.

Press the <E-STOP RESET> button to reset the emergency stop

condition. If the E-Stop does not reset, it is a result of some cause

other than overtravel.

4.

Make sure it is safe to move the axis away from the overtravel limit.

5.

Use any of the jog features described on page 4-1 except homing, to

manually move the axis away from the limit.

END OF CHAPTER

12-13

Chapter

13

Coordinate Control

13.0

This chapter describes 9/Series coordinate control.

Chapter Overview

For information about:

See page:

Plane selection G17, G18,G19

13-1

Absolute/Incremental modes G90, G91

13-2

Inch/Metric modes G70, G71

13-4

Radius/Diameter modes G07, G08

13-5

Scaling G14, G14.1

13-7

13.1

The 9/Series control has a number of features that operate in specific

planes. For that reason, it is frequently necessary to change the active

Plane Selection

plane by using a G17, G18, or G19 code. The G18 plane is always active

(G17, G18, G19)

at power-up.

Some of the features that are plane-dependant are:

Circular interpolation

Tool tip radius compensation

Many fixed cycle operations

Important: Your system installer determines the axis names and planes

defined by G17, G18, and G19 in AMP. Your system may not have planes

assigned exactly as listed below. Refer to the documentation prepared by

your system installer.

Typical axis names and their corresponding plane assignment are shown

below (this manual assumes this configuration throughout):

Code:

Plane defined by the:

G17

none

G18

Z and X axes (or axes parallel to Z and X)

G19

none

Planes can be altered to accommodate additional axes parallel to the

principle axes by programming those axes in a G17, G18, or G19 block.

See Example 13.1.

13-1

Chapter 13

Coordinate Control

In the above block, the control moves the cutting tool away from the

current axis position, a distance of 40 units on the X axis and 20 units on

the Z axis.

G91 is a modal G-code and remains active until cancelled by a G90.

Example 13.2

Absolute vs Incremental Commands

Absolute Command

Incremental Command

G90X20.Z10.;

G91X10.Z-25.;

Figure 13.1

Results of Incremental VS Absolute Example

X

End point

20

Start point

10

Z

10

35

Lathe G-code, System A

If using G-code system A, G90 and G91 are not available. To program

moves in absolute mode using G-code system A, call out axis positions

using X, Z, and C axis words.

Important: Absolute and incremental axes addresses are assigned in AMP

by your system installer, and they differ from those shown here.

Absolute command, G code system A

X40.Z20.;

13-3

Chapter 13

Coordinate Control

To program incremental moves using G-code system A, call out axis

positions using U, W, and V.

Incremental command, G code system A

U20.W-25.;

The above commands are not modal. Incremental and absolute commands

can be programmed at any time, even in the same block.

Table 13.A shows the typical command addresses for absolute and

incremental programming in G-code system A. See the documentation

provided by your system installer for axis names in your system.

Table 13.A

Absolute and Incremental Addresses, G-code System A

Absolute Commands

Incremental Commands

Remarks

X

U

X axis motion command

Z

W

Z axis motion command

C

V

C axis motion command

13.3

The selection of a unit system (inch or metric) can be done by

Inch/Metric Modes (G70,

programming either G70 for the inch system or G71 for the metric system.

These unit system G-codes should be among the first blocks written in a

G71)

program.

Both G70 and G71 are modal, and they cancel each other. The default unit

system selected by the control at power-up is determined in AMP by your

system installer.

The currently active unit system is usually displayed on the screen for

softkey level 1 in lines 3 or 4 between the [ ] symbols. If the screen

selected for display of softkey level 1 is the status screen, the active system

G-code (G71 or G70) is displayed among the active system G-codes.

Some of the functions that are affected by the active unit system (inch or

metric) are:

Position commands

Feedrate commands

Axis feed amount for fixed amount feed operation

Unit system for hand pulse generator (HPG)

13-4

Chapter 13

Coordinate Control

Figure 13.2

Diameter/Radius Programming

Diameter

Radius

Programming Programming

X

Mode (G08) Mode

(G07)

G90G08X12.; G90G07X6

or

or

G91G08X-8.; G91G07X-4.;

15

10

5

10

20

6

12

Z

Important: The following must always be programmed as radius value,

regardless of whether G07 or G08 is active:

Most of the X axis infeed amounts or similar values (addresses D, I, K)

used in Simple and Compound fixed cycles (G70 - G78).

Center point designation (addresses R, I, K) for circular interpolation.

Feedrates in the X-axis direction (change in radius per revolution G95

or radius per minute G94).

The threading cycle parameter E or F when face threading is being

programmed.

Position displays are impacted by radius diameter mode. The

diameter/radius axis selected in AMP displays either an R or a D next to it,

indicating which mode it is currently in and represented on the CRT. This

even applies to the machine coordinate system (absolute display).

13-6

Chapter 13

Coordinate Control

13.5

Use the scaling feature to reduce or enlarge a programmed shape. Enable

this feature by programming a G14.1 block as shown below:

Scaling

G14.1 X__ Z__ P__;

Where :

Is :

X and Z

the axis or axes to be scaled and the center of scaling for those axes.

P

the scaling magnification factor for the specified axes.

The axes programmed in the G14.1 block determine which axes are scaled.

The corresponding axis word values specify the center of scaling for each

axis. This position is the axis coordinate around which the scaling

operation is performed.

The scaling magnification factor (P) is the amount of scaling to be applied

to the programmed axes. Each axis can have a different scale factor by

programming them in separate G14.1 blocks. The scaling range is from

0.00001 to 999.99999. A scale factor less than one reduces a programmed

move, while a scale factor greater than one enlarges a programmed move.

If no P-word is programmed or if P0 is programmed in the G14.1 block,

the default magnification factor is used. If the programmed P-word value

is out of range, the CRT displays an error message.

When absolute mode (G90) is active, scaling moves are referenced from

the programmed center of scaling.

Example 13.4

Scaling with Absolute Mode Active

Program block

Comment

G07 G90 G00 X30. Z60.;

radius mode, absolute mode

G14.1 X0 P.5;

scale X axis only, by .5

G01 X12.;

feedrate move X to X6

Z38.;

feedrate move Z to Z38

X20.;

feedrate move X to X10

G14;

cancel scaling

G00 X30. Z60.;

rapid return

13-7

Chapter 13

Coordinate Control

Figure 13.3

Results of Example 13.4

X

Original part contour

Contour after scaling

X axis only by .5 in

30

G90 absolute mode

20

10

6

Z

20

40

60

When incremental mode (G91) is active, the control ignores the

programmed centers of scaling. The control performs scaling on the axes

programmed in the G14.1 block, but the scaling moves are referenced from

their current axis positions, not the programmed center of scaling or the

active coordinate zero point.

Important: The center of scaling may be specified in either incremental or

absolute mode (G90/G91) in the G14.1 block. But unlike other features in

the control, both modes cannot be programmed in the same block.

Example 13.5

Scaling with Incremental Mode Active

Program block

Comment

G07 G90 G00 X30. Z60.;

radius mode, absolute mode

G91;

incremental mode

G14.1 X1.023 P.5;

scale X by .5 (X value is ignored)

G01 X-18.;

feedrate move X to X21

Z-22.;

feedrate move Z to Z38

X8.;

feedrate move X to X25

G14;

cancel scaling

G00 X5. Z30.;

rapid return

13-8

Chapter 13

Coordinate Control

Figure 13.4

Results of Example 13.5

Original part contour

Contour after scaling

X axis only by .5 in

G91 incremental mode

X

30

--9

20

10

Z

20

40

60

G14 disables scaling on all axes. When you disable scaling, the center of

scaling and any scaling magnification factors are cleared. The next time

you enable scaling, these values must be reset. In addition to G14, M99 in

the main program, M02, M30, and a control reset operation disables

scaling. The system powers up with scaling disabled.

Your system installer specifies in AMP, on an axis by axis basis, whether

scaling is allowed. Refer to the literature provided by your system installer

for additional information.

The control provides the PAL program with the option of monitoring

which axes are currently being scaled, on an axis-by-axis basis, through the

PAL flag $SCAX. See the PAL Reference manual for additional

information.

13-9

Chapter 13

Coordinate Control

13.5.1

When you enable scaling for a particular axis, the letter “P” is displayed

next to the axis name on all axis position display screens. Figure 13.5

Scaling and Axis Position

shows scaling enabled on all axes.

Display Screens

Figure 13.5

Axis Position Display Screen Showing Scaling Enabled

E-STOP

PROGRAM[ MM

]

F

0.000 MMPM

PR

X

1234.567

S

00

P

Z

9876.000

T

0

(ACTIVE PROGRAM NAME)

MEMORY

MAN STOP

PRGRAM

OFFSET

MACRO

PRGRAM

SYSTEM

MANAGE

PARAM

CHECK

SUPORT

13.5.2

The scaling magnification data screen lists for all axes, the:

Scaling Magnification Data

currently active scaling magnification amount

Screen

current center of scaling

default scaling magnification amount

The currently active scaling magnification amount and the current center

of scaling for the axes can only be monitored through this screen. The

default scaling magnification amount for the axes can be monitored or

changed through this screen.

The default scaling magnification values should be changed only when the

control is in a stopped state. If the default values are changed, the new

default values do not become active until the next G14.1 block is executed.

13-10

Chapter 13

Coordinate Control

To access the scaling magnification data screen, follow these steps:

1.

Press the {OFFSET} softkey on the main menu screen.

(softkey level 1)

PRGRAM

OFFSET

MACRO

PRGRAM

SYSTEM

MANAGE

PARAM

CHECK

SUPORT

FRONT

ERROR

PASS-

SWITCH

PANEL

MESAGE

WORD

LANG

2.

Press the {SCALNG} softkey to display the scaling magnification

data screen. See Figure 13.6.

(softkey level 2)

WORK

TOOL

TOOL

TOOL

RANDOM

CO-ORD

WEAR

GEOMET

MANAGE

TOOL

COORD

SCALNG

BACKUP

ROTATE

OFFSET

Figure 13.6

Scaling Magnification Data Screen

SCALING MAGNIFICATION

CENTER

CURRENT

DEFAULT

X

+ 123.00000

2.00000

1.00000

Z

+ 123.00000

2.00000

1.00000

REPLCE

VALUE

13-11

Chapter 13

Coordinate Control

CAUTION: This cycle cuts more metal when scaling is

enabled.

G21

G21 X_Z_F_E_

X (scaled)

Z (scaled)

F (not scaled)

E (not scaled)

G24

G24 X_Z_K_

X (scaled)

Z (scaled)

K (scaled)

CAUTION: This cycle cuts more metal when scaling is

enabled.

G81

G81 X_Z_R F_L_

X (scaled)

Z (scaled)

R (scaled)

F (not scaled)

L (not scaled)

Important: R uses the scale factor associated with the axis that is

perpendicular to the active plane.

END OF CHAPTER

13-16

Chapter

14

Axis Motion

14.0

This chapter covers the group of G-words that generates axis motion or

dwell data blocks. Major topics include:

Chapter Overview

Information about:

On page:

Positioning axes

14-1

Automatic machine home

14-12

Dwell (G04)

14-18

Programmable mirror image

14-19

Axis clamp

14-22

14.1

Use these 4 basic G-codes to produce axis motion:

Positioning Axes

G00 Rapid Positioning

G01 Linear interpolation

G02 Circular interpolation (clockwise)

G03 Circular interpolation (counterclockwise)

After the execution of a positioning command the program proceeds to the

next block only after an in-position check function confirms that all

commanded axes have reached the in-position band. Your system installer

sets the in-position band width in AMP. See chapter 18 for details on the

G-codes that you can use to modify the in-position band check.

14.1.1

Format for the rapid positioning mode is:

Rapid Positioning Mode

G00X__ Z__ ;

(G00)

Where :

Is :

G00

The G00 code establishes the positioning mode. In positioning mode, the cutting

tool is fed along a straight line at the rapid feedrate determined in AMP by your

system installer.

XZ

The end point of the move generated by the G00 block in the current work

coordinate system.

You can perform a rapid positioning in the absolute mode (G90), or the

incremental mode (G91).

14-1

Chapter 14

Axis Motion

Your system installer determines the feedrate for the rapid positioning

mode in AMP, individually for each axis. The feedrate of a positioning

move that drives more than one axis is limited by the rapid rate set for the

slower axis. The slower axis is driven at its rapid rate, while the feedrate

for other axes is reduced to maintain a linear move. This also assures that

all axes start and stop at the same time.

G00 is a modal command and remains in effect until it is cancelled by a

G-code of the same group. For a listing of G-code groups, see appendix C.

Example 14.1

Positioning (G00)

Absolute command

Incremental command

G08

G08

G90G00X75.Z55.;

G91G00X-35.Z-80.;

Figure 14.1

G00 Positioning, Results of Example 14.1

X

80

55

35

75

Z

Important: Any F-word designated in the positioning mode is stored as

the active feedrate in control memory, but it is ignored during positioning

mode (G00).

14-2

Content      ..     10      11      12      13     ..