Content      ..     24      25      26      27     ..

9/Series CNC Lathe. Operation and Programming Manual - page 26

Chapter 30

Using a 9/Series Dual--Processing System

Synchronization in MDI Mode

Synchronization M-codes can be programmed in MDI mode. These can

prove useful when attempting to manually start multiple programs from

some point other than the beginning or when it is necessary to execute

MDI programs on both processes simultaneously. By inserting a

synchronization M-code (by using MDI and pressing cycle start) you can

start a process executing, but place it in pause until you start the second

process and it executes the corresponding synchronization code.

Example 30.5

Synchronization in MDI Mode

Process 1 (MDI mode)

Comment

Process 2 (MDI mode)

Comment

N1 M100;

You can press <CYCLE START> and

this block will pause while you MDI the

necessary information into process 2.

N1 M100;

Pressing <CYCLE START> at this

block has the effect of starting both

processes’MDI program at the same

time.

G28 X10 Z10;

G28 X10 Z10;

Program Interrupts During Synchronization Blocks

Program interrupts can be performed while a process is being paused by a

synchronization M-code (see chapter 29 for details on interrupts). If the

process is paused when the interrupt is requested, the request will be

recognized; however, the interrupt will not execute until the

synchronization M-code is released by the other process, executing the

appropriate synchronization code.

<CYCLE STOP> During Synchronization Blocks

Press <CYCLE STOP> places in cycle suspend mode while it is paused by a

synchronization M-code. This lets you perform most manual operations

(such as jog retract) and other functions normally available to a process in

cycle suspend mode. No loss of synchronization occurs while the process

is in cycle suspend.

Block retrace will not retrace through part program blocks with

synchronization M-codes in them. The error message “NO FURTHER

RETRACE ALLOWED” appears.

30-11

Chapter 30

Using a 9/Series Dual--Processing System

For example, press <CYCLE STOP> to place process 1 in cycle suspend

mode, while process 1 is waiting for process 2 to execute an M101. Later,

when you request <CYCLE START> for process 1, the synchronization

M-code is re-activated and process 1 is again paused, waiting for process 2

to execute an M101. If, while process 1 is in cycle suspend mode, process

2 executed an M101, process 2 will pause at that synchronization block.

Pressing <CYCLE START> for process 1 releases the pause for both process,

and they will resume program execution.

30.4

There are two basic configurations for the spindle with dual-processing

systems. These are:

Spindle Control for

Dual- Processing Systems

Shared Spindle Configuration -- The system contains one spindle that is

controlled by both processes (in addition to any other spindles the

system may contain).

Separate Spindle Configuration -- The system contains one or more

separate spindles for each process. In some cases these spindles are on

completely separate machines.

Figure 30.4

Example of Different Dual-Processing Spindle Configurations

Shared Spindle Configuration

Separate Spindle Configuration

Dual-Turret Lathe

Dual-Spindle Lathe

Process 2

Process 1

2nd Threading Pass

Process 1

1st Threading Pass

Process 2

12599-I

Both the shared and separate spindle configurations can have additional

spindles. These spindles must be assigned to only one process and cannot

be controlled by more than one process. When a process has more than

one spindle under its control, use a G12.x command to select the currently

active spindle. Refer to chapter 17 for details.

30-12

Chapter 30

Using a 9/Series Dual--Processing System

30.4.1

Shared spindle configurations are for those dual-processing systems that

have one spindle that must be controlled by both processes. See

Shared Spindle

Figure 30.4. As a general rule for this type of machine, spindle control is

Configurations

given to the process currently requesting spindle control.

WARNING: It is the programmer’s responsibility to watch for

conflicting overlap of spindle control between the two

processes. For example, one process should not request

clockwise spindle rotation while the other process requires

counterclockwise rotation. Prevention of overlapping spindle

control can be accomplished through synchronization M-codes.

See page 30-7.

Simple Spindle Speed and Direction

The process that requests a change in spindle speed or direction gets

control of the shared spindle. This can cause problems when both

processes are performing operations that require control over the spindle.

For example, consider the following program segments.

Process 1

Process 2

Shared Spindle Operation

N51 G97 S200 M04;

200 RPM, counterclockwise

N21 G97 S500 M03;

500 RPM, clockwise

N52 G01 X10 Z5;

500 RPM, clockwise

(cutting with process 2 direction

and RPM)

N22 G01 X12 Z--1

500 RPM, clockwise

N53 X12 Z3 S275;

275 RPM, counterclockwise

(cutting with process 1 direction

and RPM)

30-13

Chapter 30

Using a 9/Series Dual--Processing System

Use the synchronization M-codes to properly dictate which process has

control of the spindle at any given time. Adding a synchronization M-code

to the above program segments would remedy the problem of process 1

cutting at the wrong RPM and in the wrong direction. For example:

Process 1

Process 2

Shared Spindle Operation

N51 G97 S200 M04;

200 RPM, counterclockwise

N21 M101;

200 RPM, counterclockwise

(process 2 pauses, waiting for

M101 in process 1)

N52 G01 X10 Z5;

200 RPM, counterclockwise

N53 X12 Z3 S275;

275 RPM, counterclockwise

N53 M101;

275 RPM, counterclockwise

N22 G97 S500 M03;

500 RPM, clockwise

N22 G01 X12 Z--1;

500 RPM, clockwise

Multiple Spindle Systems

Your system installer has the option of assigning additional spindles (in

addition to the shared spindle) to the different processes. These spindles

cannot be shared. Your system can have only one shared spindle between

processes. Additional spindles must be assigned to specific processes in

AMP and can be controlled by only that process.

Controlling these additional spindles in the part program is accomplished

in the same way as single processing systems. The spindle being

controlled must first be selected by using a G12.1, G12.2, or G12.3. Refer

to page 17-9 for details on programming these spindle G codes. Your

system installer selects in AMP which spindle (spindle 1, spindle 2, or

spindle 3) is the shared spindle.

Exclusive Operations on a Shared Spindle.

There are several features that require exclusive use of the spindle. When

you execute these features, changes to the spindle cannot be performed by

another process until the feature is completed or canceled. These features

include:

M19 -- Spindle Orient

G96 -- Constant Surface Speed (CSS)

G16.1, G16.2 -- Virtual C, Cylindrical and End-Face Milling

Fixed cycles that require spindle control include:

- G84 (right hand tapping cycle)

- G84.1 (left hand tapping cycle)

- G86.1, G87, G88 (boring cycles)

30-14

Chapter 30

Using a 9/Series Dual--Processing System

An error is generated and the process enters cycle stop if you attempt to

activate one of these features while one is already active in another

process. For example, if process 1 is currently performing virtual C on the

shared spindle and process 2 attempts to execute a G84 right hand tapping

block, process 2 will generate an error and enter cycle stop. Process one

will continue until completion or until it encounters a synchronization

M-code. Any attempt to change the spindle speed or direction (via M03,

M04, or M05) will have the same results.

Threading on a Shared Spindle

Simple threading (G33 or G34) and the threading cycles (G21 and G78)

can be performed on a shared spindle. Make sure that the spindle speed or

direction is not changed by process 2 (see page 30-13).

Process 1

Process 2

Spindle Operation

N15 G33 X10 Z10 F20 S100;

Synchronizes Z axis motion

with spindle for threading.

N17 M03 S200;

Will not cancel threading

synchronization on process 1;

however, it will change

threading speed or direction or

both.

Both processes can also perform threading from the same spindle.

Synchronization of the spindle will be performed from the same marker

point. Both processes can cut the same thread if the same thread lead is

programmed in both processes.

Important: When you use two processes to cut the same thread, the

position of the cutting tool has a significant impact on the thread being cut.

Both processes key off of the same spindle marker, so it is necessary to

alter the start point of one of the processes. Failure to do so results in a

multistart thread.

30-15

Chapter 30

Using a 9/Series Dual--Processing System

Figure 30.5

Multi-Start Thread When Same Start Point Is Used

Process 2

2nd Threading Pass

If both processes key off same

marker pulse, then multi-start thread

results.

Marker

Process 1

12600-I

1st Threading Pass

Use this formula to calculate the amount the start points must be offset:

Shift = q / 360 * F

Where:

Shift - is the amount the start point of the threads should be offset

q- the angular distance around the spindle between the two processes

(always measured in the direction of spindle rotation)

F - the length of the thread lead

For example, assuming your cutting tools are on directly opposite sides of

the spindle, q would be 180 degrees. If the thread lead were 20 threads per

inch, F would be 1 / 20. The shift would then equal:

Shift = 180 / 360 * 1/20 = .025 inch.

In cases where the second process is not exactly 180 degrees opposite the

other process, consider the above equation for the direction of spindle

rotation. This consideration is made by always measuring q in the

direction of spindle rotation.

30-16

Chapter 30

Using a 9/Series Dual--Processing System

Figure 30.6

Identical Thread Is Cut When Start Point Is Shifted Using Equation

Process 2

2nd Threading Pass

.025

Marker

Process 1

1st Threading Pass

12601-I

Example 30.6

Threading on Both Processes with a Shared Spindle

Process 1

Comment

Process 2

Comment

N1 G00 X10. Z10 S500. M03;

Move to process 1 start point and start

spindle rotation

N1 G00 X10. Z11.;

Z start point is shifted one inch from

process 2

N3 G21 X4.8 Z5. E2.;

Start threading on process 1

N2 M100;

Synchronize to make sure process two

cuts thread behind process 1

N2 M100;

Allow process 2 to start threading

N3 G21 X4.65 Z5. E2.;

Start threading on process 2

N4 X4.5;G04P5;

N4 X4.4;

N5 X4.35;

N5 4.3;

30-17

Chapter 30

Using a 9/Series Dual--Processing System

Figure 30.7

Cutting a Thread Using Both Processes

Process 2

2nd Threading Pass

Process 1

1st Threading Pass

12602-I

Spindle Orient on a Shared Spindle

Both processes can request a spindle orient. If one process requests a

spindle orient while the other process’s spindle orient command has not

completed, the control generates an error. The process that requested the

second spindle orient is forced into cycle stop mode.

30.4.2

This system configuration contains a separate spindle for each process. In

Separate Spindle

some cases the spindles are on completely separate machines. At no time

are spindle commands shared by both processes.

Configuration

This type of system operates identically to a single-process system. Each

process has full and total control of its assigned spindles. Each process can

be assigned multiple spindles, but each spindle is specifically assigned to

that process. No other process can control a spindle assigned to a specific

process. The spindle currently being controlled by a process is selected

with a G12.x command. See chapter 17 for details.

Important: Do not assume that because your system has more than one

spindle that you have this separate spindle configuration. It is possible that

one of your spindles is shared by both processes, and the additional

spindle(s) is assigned to a specific process(es). Refer to your system

installer’s documentation to determine what type of spindle configuration

your system contains.

30-18

Chapter 30

Using a 9/Series Dual--Processing System

30.5

The Interference Checking feature is designed to help prevent collisions by

the axes of a dual-processing machine.

Using Interference Checking

with a Dual-Process Lathe

Interference checking provides an area (usually around the cutting tool or

tool turret for each process) that defines a boundary that moves with the

tool. The other process cannot enter into this boundary. This helps prevent

collisions.

For interference checking to function properly, you must define and

activate this boundary for both processes. When one process’s boundary

attempts to enter another process’s boundary, one process enters cycle

suspend, preventing it from entering the protected area. In the case of an

unavoidable direct collision, both processes stop. An error message is

displayed for both processes. The two boundaries cannot intersect.

CAUTION: These interference boundaries only help prevent

collision with another interference boundary configured for

another process. They do not protect against collisions with

other machine fixtures that may or may not be protected by a

programmable zone or software overtravel. They do not

account for any tool offsets that are active at the time. They are

absolute positions.

Figure 30.8

Interference Check Helps Prevent Tool Fixtures from Colliding

Programmable

Zone 1

Tailstock

Interference checking does not protect programmable zones.

Area protected against

Only tool tip location is monitored for a programmable zone. Possible

collision by interference

collision between these areas.

checking. No collision

12603-I

between these areas.

30-19

Chapter 30

Using a 9/Series Dual--Processing System

Using Interference Checking to Prevent Collisions

When two protected areas are about to collide, the control suspends

motion, stopping one or both of the processes and preventing a collision.

In Example 30.7, process 1 will collide with process 2. Since process 2 is

stationary, the control puts process 1 in cycle suspend to prevent a

collision. Once the control detects the collision, it suspends the action.

Interference checking operates in real time. It is not checked in block

lookahead. The control detects a collision immediately before the

boundaries overlap and suspends one or both of the processes, halting the

axes with an abrupt, undecelerated stop.

Example 30.7

Collision Programmed with Interference Checking On

Process 1

Process 2

N1 G90 G70;

N1 G90 G70;

N2 G00 Z-2.1 X-2.1;

N2 G00 Z6 X6;

N3 G00 Z8 X9;

N3 M30;

N4 M30;

Figure 30.9

Results of Example 30.7

X

Process 2

Collision avoided

10

immediately before

boundaries overlap

8

6

4

Process 1

2

Z

-2

2

4

6

8

10

--2

12604-I

30-21

Chapter 30

Using a 9/Series Dual--Processing System

30.5.1

The control can store as many as 32 different boundaries for each process.

Two separate areas make up each of these boundaries. Both axes are

Measuring Interference

activated when the boundary is activated through PAL. Figure 30.10

Boundaries

illustrates the use of two areas to make up interference boundary 01.

Figure 30.10

Using Two Areas to Define an Interference Checking Boundary

Area 2

These areas define an interference boundary.

A maximum of 32 boundaries can be defined

containing 64 actual areas (two areas in each

boundary).

Area 1

12605-I

At least one area must be defined for a boundary to be considered valid for

activation. If only one area is defined, the control assumes the second area

does not exist.

Areas for interference checking are defined in the machine coordinate

system for the fixtures positions as the axis sits at the home position.

Only two axes can be entered into the interference tables to define a

boundary. Your system installer selects these two axes in AMP. Follow

this procedure to measure values defining your interference areas:

1.

Return the axes to the home position (with no offsets active). This

can be accomplished by manually homing the machine (see chapter

4) or by programing a G28 (see chapter 14).

2.

Measure the values defining the interference area for each axis as

shown in Figure 30.11.

You will probably need to take different measurements for all of the

different fixtures and tools you will be using. Regardless of the tool

or fixture being used, the machine must remain at machine home

(with no offsets active) when the measurements are taken.

Interference areas are always measured as radius values. Data cannot

be entered into the interference tables as diameter values.

30-22

Chapter 30

Using a 9/Series Dual--Processing System

Important: Your system installer determines the relationship of the

machine coordinate systems between processes (relative location of zero

points and direction of positive travel) in AMP and through hardware.

This manual assumes the machine coordinate systems of both processes are

as shown in Figure 30.11. Refer to your system installer’s documentation

for details on how your machine coordinate systems are configured.

Figure 30.11

Measuring Interference Checking Areas

Z Plus

+X

Area 2

Process 1

Z Plus

Area 1

Z Minus

Area 2

Z Minus

Area 1

Area 1

Area 2

Machine

X Plus

X Plus

Home

Area 1

Area 2

Process 1

X Minus

Area 1

X Minus

Area 2

Machine

Coordinate

X Minus

Area 1

Z

System Zero Point

Area 1

(Both Processes)

X Plus

Area 1

Machine Home

Z Minus

Process 2

Area 1

Z Plus

Area 1

+X

Process 2

12606-I

30-23

Chapter 30

Using a 9/Series Dual--Processing System

Figure 30.12

Protecting Additional Axes with Interference Checking

Though only X and Z define this interference area,

some protection is also offered to W since an X or Z collision

Process 1

would be detected anytime W would collide. This protection,

however, will cause the control to detect a collision even if

sufficient clearance exists on the W axis. Disable interference

No limits

checking when it is necessary to overlap a third axis.

for the W

axis

W

Process 2

Z

X

12607-I

30.5.2

To manually enter values into the interference checking tables, follow this

procedure:

Entering Interference Values

Manually

1.

Press the {SYSTEM SUPORT} softkey.

(softkey level 1)

PRGRAM

FRONT

MACRO

PRGRAM

SYSTEM

MANAGE

PANEL

PARAM

CHECK

SUPORT

OFFSET

ERROR

PASS-

SWITCH

MESAGE

WORD

LANG

2.

Press the {PROGRAM PARAM} softkey.

(softkey level 2)

PRGRAM

AMP

DEVICE

MONI-

TIME

PARAM

SETUP

TOR

PARTS

PTOM

SI/OEM

30-25

Chapter 30

Using a 9/Series Dual--Processing System

3.

Press the {INTERF CHECK} softkey to display the interference

checking data entry screen shown in Figure 30.13.

(softkey level 3)

ZONE

F1-F9

DRLCYC

INTERF

LIMITS

PARAM

CHECK

Figure 30.13

Interference Checking Data Table

INTERFERENCE TABLE

PAGE

1

OF 32

TOOL NO

AREA 1

AREA 2

*1

[INCH]

[INCH]

X PLUS

1.5000

1.5000

X MINUS

-.5000

-1.0000

Z PLUS

1.5000

6.0000

Z MINUS

0.0000

1.5000

<FRONT TURRET>

SEARCH

REPLCE

ADD TO

MORE

BACKUP

NUMBER

VALUE

VALUE

ZONES

INTERF

4.

Select a process. Refer to the system installer’s documentation for

details on selecting a process, or press the [PROC SELECT] key.

5.

Select a boundary number to enter by using one of these two

methods. Press:

the {MORE ZONES} softkey, or press the [Ø] key while holding

down the [SHIFT] key.

the {SEARCH NUMBER} softkey. Enter the desired boundary number

to search for and press the [TRANSMIT] key.

30-26

Chapter 30

Using a 9/Series Dual--Processing System

This boundary number should be the same as the tool geometry

number (T-word) that will be active when the tool and/or fixture is

being controlled. Refer to your system installer’s documentation for

details on which tool or fixture corresponds to which interference

boundary number (1-32).

6.

Use the up or down cursor keys to move the block cursor to the

interference area parameter to be changed. The selected field appears

in reverse video.

7.

If necessary, change the measurement units by using MDI. Units

currently used in the table are determined by the current mode of the

process (G70 inch or G71 metric).

8.

Enter the boundary area values as determined on page 30-22. Enter

values in one of two ways:

Press This

Then:

Press:

The New Value:

Softkey:

{REPLCE

Type in the new value.

[TRANSMIT]

replaces the old value

VALUE}

for that feedrate.

{ADD TO

Type in the new value.

[TRANSMIT]

is added to the old

VALUE}

value for that area.

9.

Repeat this procedure for each process until all boundaries are

entered.

30.5.3

You can enter data in the interference tables by programming the correct

G10 command. This section describes the use of the G10 commands.

Entering Interference Values

through Programming

Important: The active boundary and the value in the interference

(G10L5 and G10L6)

boundary table change when a G10 code modifies the table value. Both

changes activate immediately.

When the process is in incremental mode (G91), any values entered in the

table with the G10 command are added to the currently existing offset

values. When the process is in absolute mode (G90), any values entered in

an offset table with the G10 command replace the currently existing offset

values.

Values can be entered into the table as inch or metric values. Select the

values you intend to enter by first programming the G-code that establishes

the mode you wish to use (G70 or G71).

30-27

Chapter 30

Using a 9/Series Dual--Processing System

This is a representation of the basic format for modifying the tables.

5

G10 L{

} P__ X___ Z___ I___ K___;

6

Where :

Is :

L(5-6)

The definition of which area in the table is being modified.

L5 - Modifies the Area 1 values

L6 - Modifies the Area 2 values

P

The boundary number of the interference boundary that is having its values changed is

specified following the P address.

X

The value to add to (in G91 mode) or replace (in G90 mode) the positive X axis value. This

value is always a radius value.

Z

The value to add to (in G91 mode) or replace (in G90 mode) the positive Z axis value.

I

The value to add to (in G91 mode) or replace (in G90 mode) the negative X axis value. This

value is always a radius value. I is the integrand word of the X axis.

K

The value to add to (in G91 mode) or replace (in G90 mode) the negative Z axis value. K is the

integrand word of the Z axis.

Programming this G10 code can change only the table values for the

process that has the G10 part program currently active. You must run

separate G10 programs in each process to set up each area.

Important: G10 blocks cannot be programmed when TTRC is active.

Example 30.8

Using G10 to Change the Interference Boundaries

N1 G90

G70;

N2 G10

L5 P1 Z19.5 K13 X19 I15;

Boundary number 1 area 1 is defined.

N3 G10

L6 P1 Z23 K19.5 X18.5 I11; Boundary number 1 area 2 is defined.

30-28

Chapter 30

Using a 9/Series Dual--Processing System

Example 30.9

Resulting Boundary from Example 30.8

+X

23”

Process 1

19.5”

13”

Area 1

Area 2

Machine

18.5”

19”

Home

Process 1

15”

Machine

11”

Coordinate

System Zero Point

(Both Processes)

+Z

12608-I

30.5.4

The control can save all of the information that is entered in the

interference tables as a backup. This is done by the control generating a

Backing Up Interference

program consisting of G10 blocks. These G10 blocks contain the

Tables

boundary numbers and their respective interference boundary values. Any

time you run this program, the set of values contained in these G10 blocks

replaces the current values in the interference tables. See page 30-27 for

details on the format of this G10 program.

The interference table program can be saved in control memory as a

program, or it can be sent to a peripheral device. The interference tables

can be easily setup again by executing this program in the appropriate

process.

To back up the interference tables, follow these directions:

1.

Press the {SYSTEM SUPORT} softkey.

(softkey level 1)

PRGRAM

FRONT

MACRO

PRGRAM

SYSTEM

MANAGE

PANEL

PARAM

CHECK

SUPORT

OFFSET

ERROR

PASS-

SWITCH

MESAGE

WORD

LANG

30-29

Chapter 30

Using a 9/Series Dual--Processing System

2.

Press the {PRGRAM PARAM} softkey.

(softkey level 2)

PRGRAM

AMP

DEVICE

MONI-

TIME

PARAM

SETUP

TOR

PARTS

PTOM

SI/OEM

3.

Press the {INTERF CHECK} softkey to display the interference

checking data entry screen as shown in Figure 30.13.

(softkey level 3)

ZONE

F1-F9

DRLCYC

PRBCYC

INTERF

LIMITS

PARAM

PARAM

CHECK

4.

Press the {BACKUP INTERF} softkey. Figure 30.14 shows the backup

interference boundary screen.

(softkey level 4)

SEARCH

REPLCE

ADD TO

MORE

BACKUP

NUMBER

VALUE

VALUE

ZONES

INTERF

30-30

Chapter 30

Using a 9/Series Dual--Processing System

Figure 30.14

Backup Interference Boundary Screen

STORE TO BACKUP

INTERFERENCE TABLE

TO

TO

TO

PORT A

PORT B

FILE

5.

Determine the destination for the G10 program:

To Send the G10 Program To:

Press This Softkey:

Go to Step:

peripheral attached to port A

{TO PORT A}

7.

a peripheral attached to port B

{TO PORT B}

7.

to control memory

{TO FILE}

6.

6.

Press the {TO FILE} softkey. The control asks for a program name.

By using the alphanumeric keys on the operator panel, enter the

program name you wish to call the backup program . Press the

[TRANSMIT] key once you have entered the program name. See

chapter 10 on program names. The G10 program is saved under the

file name just entered.

7.

Press the {TO PORT A} or {TO PORT B} softkey. A {YES} or {NO}

softkey is displayed. Press {YES} to confirm or {NO} to abort. If you

confirm the operation, the G10 program is written to a peripheral

attached tot he selected port.

30-31

Chapter 30

Using a 9/Series Dual--Processing System

30.6.2

The system installer determines what axes are shared and how a shared

Switching a Shared Axis to a

axis is changed from process to process. Using AMP and PAL the system

installer determines the process for a shared axis at power up, control reset,

Different Process

and E-Stop reset. Refer to your system installer’s documentation for

details.

Even though the system installer’s PAL program determines how and when

a shared axis changes processes, there are some global restrictions that can

not be altered. Before a request to change a shared axes process is

performed, both processes that share the axis must be in one of the

following states:

- E-Stop

- Cycle Stop (not cycle suspend)

- Manual mode with the shared axis not being positioned

- Executing an M99 in a main program

- Postlude State (established through PAL)

Other restrictions are as follows:

If the shared axis is currently:

Then:

performing a manual motion (including

the request to change process for that axis is ignored until the

continuous, incremental, or handwheel jog,

manual motion is completed^¶

homing, jog on the fly, or angled jogs)

being positioned by the PAL axis mover

the request to change processes is ignored until the PAL axis

mover has completed moving the shared axis^¶

in the active plane and cutter compensation is

the request to change processes is ignored until the plane is

active

changed or cutter compensation is deactivated^¶

used to perform CSS calculations (the shared axis

the request to change processes is ignored until CSS mode is

has been assigned as the CSS axis and the

canceled^¶

control is currently in CSS mode)

involved in a modal fixed cycle (such as drilling,

the request to change processes is ignored until the cycle is

turning, threading, or 7300 cycles)

canceled^¶

If either process is performing a:

Then:

jog retract or block retrace

shared axes can not be switched into or out of the process.

This is independent of whether the shared axis is involved in

the jog retract or block retrace operation^¶

program interrupt

a shared axis can not be switched into or out of the process^¶

synchronization operation with a synchronization

a shared axis can not be switched into or out of the process^¶

M--code

¶ The request for an axis to change processes is ignored until the prohibiting feature is completed or canceled.

Then the change in process only takes place provided the request for the axis change is still true.

30-34

Chapter 30

Using a 9/Series Dual--Processing System

Example 30.10

Changing Processes with Tool Offsets

Process One

Process Two

Shared Axis

Activates this Tool

Activates this Tool

T1010;

T000;

Process one activates tool offset on shared axis as defined in AMP

(controls shared axis)

(delayed/immediate shift/move). When process two takes control of the

shared axis, the shared axis tool offset is canceled on the shared axis until it

is returned to the process.

T1111;

T1111;

Has same offset for both processes. When you shift the shared axis between

(controls shared axis)

processes, the offset remains active on the axis. When the shared axis

changes processes the tool offsets are re-initialized and the AMP selected

activation method (delayed/immediate shift/move) still occurs.

T1111;

T2222;

Process two activates tool offset on shared axis as defined in AMP

(controls shared axis)

(delayed/immediate shift/move). When you switch the shared axis to

processes one, the offset changes to the tool offset value requested in

process one. Since the offsets are re-initialized when shared axes change

processes, the AMP selected activation method (delayed/immediate

shift/move) still occurs.

30.7

The Dual--Axis feature allows the part programmer to simultaneously

Dual- Axes on a

control multiple axes while programming commands for only one. It

differs from the split axis feature of the control in that the split axis feature

Dual- Processing System

is used to control a single axis positioned by two servo motors.

The dual--axis feature is especially useful for twin turret lathes and other

machines running with parallel cutting tools. Figure 30.15 shows a typical

configuration for dual axes.

30-37

Chapter 30

Using a 9/Series Dual--Processing System

Figure 30.15

Dual- Axis Configuration

Lead screw

Axis 1

Encoder

Servo

motor

Dual Axes - two completely separate

axes responding to the same

programming commands.

Encoder

Servo

motor

Axis 2

Lead screw

The 9/Series control supports two groups of dual axes. This is the total

number of groups allowed on the system for both processes (i.e. two

groups in one process or one group in each process).

Dual--axis operation on dual processing systems is virtually identical to

dual--axis operation on single processing systems (see chapter 20 for

details). The difference occurs on dual processing system when one or

more of the axes in the dual group is configured as a shared axis between

processes.

30.7.1

A dual--axis group is assigned in AMP to a specific process. All axes in

the dual group must be configured to be part of the dual--axis group and

Decoupling a

must be AMPed to be in the same process (called the default process for

Dual- Axis Group

the group). Dual axes can only exist as a dual group in their respective

default process. You can not share a dual group as an axis with another

process. You can only share the independent members of the dual group

with another process once the group is decoupled.

Coupling/Decoupling allows all axes in a dual--axis group to be either:

- coupled as a dual--axis group

- decoupled so each axis in the dual group can be programmed as an

independent axis.

30-38

Chapter 30

Using a 9/Series Dual--Processing System

Other restrictions are as follows:

If the dual- axis is currently:

Then:

performing a manual motion (including

the request to decouple that axis is ignored until the manual

continuous, incremental, or handwheel jog,

motion is completed^¶

homing, jog on the fly, or angled jogs)

being positioned by the PAL axis mover

the request to decouple that axis is ignored until the PAL axis

mover has completed moving the dual--axis^¶

in the active plane and cutter compensation is

the request to decouple that axis is ignored until the plane is

active

changed or cutter compensation is deactivated^¶

used to perform CSS calculations (the dual--axis

the request to decouple that axis is ignored until CSS mode is

has been assigned as the CSS axis and the

canceled^¶

control is currently in CSS mode)

in a process that is performing a jog retract or

the dual axes can not be decoupled. This is independent of

block retrace

whether the dual--axis is involved in the jog retract or block

retrace operation^¶

in a process that is performing a program interrupt

a dual--axis can not be switched into or out of the process^¶

involved in a modal fixed cycle (such as drilling,

the request to change processes is ignored until the cycle is

turning, threading, or 7300 cycles)

canceled^¶

¶ The request for an axis to change processes is ignored until the prohibiting feature is completed or canceled.

Then the change in process only takes place provided the request for the axis change is still true.

30.7.2

When coupled all axes of a dual group are programmed by the name of the

AMPed master axis. Axes in a dual--axis group can be programmed as

Independently Programming

independent axes once they have been decoupled. Once decoupled each

Dual- Axis Members

axis gets its own independent axis name and integrand letter (defined in

AMP) as opposed to the dual--axis group name and integrand used to

program the axis when coupled. For example a dual group consisting of

two axes is programmed with a X axis name. Once the dual group is

decoupled both axes in the dual group are programmed with their own axis

name X and W.

Important: Once an axis has been decoupled from the dual group it still

retains many traits from the original dual group. Features such as acc/dec,

CSS, radius/diameter axis, maximum feedrates, jog feedrates and jog

increments are all adopted from the original group.

Shared axes that have been decoupled from a dual group can change

processes. Once a shared axis is controlled by another process it can not

be recoupled with the dual group until it returns to its original default

process.

Slave axes can be defined in active primary or parallel planes (G17, G18,

or G19) however the plane containing a slave axis can not be activated

unless the dual group is decoupled, and the slave axis is in the process

requesting the plane.

30-40

Content      ..     24      25      26      27     ..