9/Series CNC Lathe. Operation and Programming Manual

Chapter 17

Spindles

17.6

Use this feature to synchronize the position and/or velocity between two

spindles with feedback using your 9/440, 9/260, or 9/290 control.

Synchronized Spindles

Two types of synchronization are available:

Velocity — synchronizes only the speed between two spindles

Velocity and Position — synchronizes the speed and angular

position between two spindles

Prior to activation, you are responsible for selecting the proper gear ranges

and ratios. The gear ratio between the feedback device and the spindle

must be 1:1. Any other type, including nonunit ratios, will not allow

repeatability of the orientation of your spindle and may cause positioning

offset inaccuracies.

Spindle Configuration

Your system installer selects two spindles to make up the synchronization

pair, which consists of the controlling and follower spindles. During

synchronization, the controlling spindle initiates spindle motion while the

follower spindle attempts to synchronize with it. Your system installer

determines the configuration of these spindles. Refer to your system

installer’s documentation for more information about spindle

configuration.

Gear ranges are set separately for each spindle. If the controlling spindle

speed is outside of the current follower spindle gear range when a seek is

attempted, the controlling spindle will ramp to within the follower’s limits

set in AMP.

Selecting the Controlling Spindle

The synchronized spindle’s controlling spindle, which is determined by

your system installer, must be programmed as the part program’s

controlling spindle in your part program prior to synchronization. Use one

of the G12 codes (G12.1, G12.2, and G12.3) to designate the active

controlling spindle for spindle synchronization. Refer to page 17-9 for

more information about the G12 codes and your system installer’s

documentation to identify your controlling spindle.

Important: Typically, the programmed speed of the controlling spindle

dictates the speed of the follower spindle. For more information about

valid gear ranges, refer to page 17-28.

17-23

Chapter 17

Spindles

17.6.1

Use these three G--codes to manipulate the spindle synchronization feature:

Using the Spindle

Set spindle positional synchronization (G46)— sets the follower spindle

Synchronization Feature

speed/direction and relative position offset to match the controlling

spindle.

Set active spindle speed synchronization (G46.1)— sets the follower

spindle speed/direction to match the controlling spindle.

Deactive spindle synchronization (G45)— shuts off synchronization

while maintaining the controlling and follower spindles’current speed

and direction.

Activate Spindle Positional Synchronization (G46)

Use the “Activate Spindle Positional Synchronization” to synchronize

speed and position. The position is based on a programmed S--word

(degrees). If you do not program an S--word in the G46 block, it will

automatically go to the relative positional offset, set by your system

installer. Refer to your system installer’s documentation for more

information.

During a G46, the spindles attempt to match speeds. Once the speeds are

matched, the spindles attempt to synchronize their relative positional

offset. Once synchronization is achieved, the active spindle speed and

mode (M03, M04, M05, or M19) programmed for the follower spindle is

replaced by the current controlling spindle speed and mode.

Important: Changes in spindle speeds that would normally occur as a

result of CSS or other programmed changes to spindle speeds, directions,

and spindle speed override will not occur until synchronization is achieved.

The format for the G46 block is as follows:

G46S__;

Where:

Defines:

the angular offset between two spindles (degrees)*

*The range for the S--word is 0 to 360. Your system installer defines where 0_ is for each

spindle. The value defined as the offset value is absolute and independent of spindle direction.

Important: No other program letters are allowed in the G46 block except

auxiliary letters and system installer M--codes.

17-24

Chapter 17

Spindles

The following example assumes that the controlling and follower spindles

were defined as spindle 2 and spindle 1, respectively, by your system

installer.

Example 17.4

Spindle Synchronization

M03 S200;

Spindle 1 clockwise 200 rpm

M04.2 S400;

Spindle 2 counterclockwise at 400 rpm

G12.2;

Spindle 2 as controlling spindle

G46 S90;

Spindle 1 changes direction and accelerates to spindle

2’s speed; spindle 1 synchronizes angular position with

spindle 2 (offset 90 degrees)

Example 17.5 shows two spindles attempting synchronization to

transferring a part. The following steps describe the synchronization

process in this example.

The follower spindle, B, attempts to match its velocity with the

controlling spindle (A).

Once velocities are matched, spindle B reaches its relative position,

which is offset from the position of spindle A.

When synchronization is achieved, the spindle axis advances to

engage the part.

Spindle B clamps the part held by spindle A.

Spindle A unclamps, transferring the part to spindle B.

The spindles move apart and synchronization is disabled (G45).

Example 17.5

Spindle B moves into spindle A.

17-25

Chapter 17

Spindles

Activate Spindle Speed Synchronization (G46.1)

Use the “Activate Spindle Speed Synchronization” to synchronize speed

and direction only. Using G46.1 does not guarantee a consistent positional

offset between the two spindles. During a G46.1, the follower spindle

attempts to synchronize speeds with the controlling spindle. Once

synchronization is achieved, the current spindle speed and mode (M03,

M04, M05, or M19) programmed for the follower spindle is replaced by

the current controlling spindle speed and mode programmed. The original

follower spindle speed and direction is not retained.

Important: Changes that occur as a result of CSS or other programmed

changes to spindle speeds, directions, and spindle speed override will not

occur until synchronization is achieved.

The format for the G46.1 cycle is as follows:

G46.1;

Important: No other program letters are allowed in the G46.1 block

except auxiliary letters and system installer M--codes.

Deactivate Spindle Synchronization (G45)

Use G45 to deactivate the synchronized spindle feature. When

synchronization is deactivated, the follower spindle will remain in the

same state (M03, M04, M05, or M19) and at the last programmed speed

for controlling spindle until you change the program settings or if your

system installer writes PAL to recommand the spindle.

In a multiprocess system, if the spindles are synchronized, and an

end--of--program (M02) is reached on the process synchronizing the

spindles, both spindles will obey the end--of--program commands. Then

synchronization will be disabled.

The format for the G45 cycle is as follows:

G45;

Important: No other program letters are allowed in the G45 block except

auxiliary letters and system installer M--codes.

17-26

Chapter 17

Spindles

17.7

When using the synchronized spindle feature, remember:

Special Considerations for

you cannot retrace through a synchronization block (G45, G46, or

Spindle Synchronization

G46.1). However, you can retrace through blocks where

synchronization was already active.

in dual--process systems, both spindles used for synchronization

must be configured in the process that is programming spindle

synchronization. Shared spindles are acceptable if they area

already controlled by the process requesting synchronization.

gear changes are not allowed during synchronization. If spindle

speeds exceed the gear range of either spindle, the spindles will be

limited to the more restrictive spindle’s values.

due to the servo switch from open-- to closed--loop during

synchronization, a one--iteration hesitation in the spindles may be

seen when this switch occurs. This small deceleration may be

more apparent in systems with a smaller spindle motor or if

synchronization is done at higher speeds.

Program Restart, Mid--Start, and Interrupt Macros will be allowed.

If synchronization is disabled during an interrupt macro, it will

resynchronize upon return, in the event that all of the condition

checks listed in this section allow it to, otherwise a decode error

will result. Mid--Start and restart must also pass all conditions

described in this section.

you are responsible for selecting proper gear ranges prior to

activating synchronization.

The following features cannot be used while synchronization is active:

solid--tapping

Virtual C programming

The following features cannot be used while synchronization is ramping:

deep--hole peck drilling

threading

Important: Virtual C and threading are available on synchronized spindles

once synchronization is achieved.

17-27

Chapter 17

Spindles

When synchronization is active, any part program commands

destined for the follower spindle (i.e., M03, M03.2,

M03.3...G12.1, G12.2, and G12.3) will cause an error. On a

multiprocess configuration, this is true of either process.

On a multiprocess 9/Series, the process controlling the controlling

spindle also controls the follower spindle when spindle

synchronization is active. If it is unable to obtain control, an error

results: UNABLE TO SYNCH IN CURRENT MODE.

Important: Typically, the programmed speed of the controlling spindle

dictates the speed of the follower spindle. In the event that the

programmed speed exceeds the maximum or drops below the minimum

allowable values for the synchronized pair, the spindle speed will be

restricted to those allowable values, as shown on page 17-28.

the example below shows what will happen when:

no overlap occurs between the controlling and follower

spindles’gear ranges

the controlling spindle has a higher gear range than the

follower spindle

the controlling spindle has a lower gear range than the

follower spindle

Example 17.6

Valid Gear Ranges for Synchronized Spindles

Controlling Spindle

Follower Spindle

Requested

Valid Programmed

Spindles will

Gear Range

Spindle Speed

Spindle Speeds

Synchronize at

(RPM)

(RPM):

1000 to 3000

100 to 300

1500

None

N/A

1000 to 3000

800 to 1500

1800

1000 to 1500

1500

1000 to 3000

1800 to 3200

1500

1800 to 3000

1800

in a multiprocess system, if the spindles are synchronized, and an

end--of--program is reached on the process synchronizing the

spindles, both spindles will obey the end--of--program commands

and synchronization is disabled.

END OF CHAPTER

17-28

Chapter

Programming Feedrates

18.0

This chapter describes 9/Series control feedrates, including special AMP

assigned feedrates and automatic acceleration/deceleration.

Chapter Overview

For information about:

See page:

Feedrates

18-1

Special AMP-assigned Feedrates

18-8

Automatic Acceleration/Deceleration

18-10

18.1

Feedrates are programmed by an F-word followed by a numeric value.

You can enter feedrates in a part program block or through MDI. They

Feedrates

become effective in the block in which they are programmed and apply to

all G01, G02 and G03 axis motion. If the block requires rapid traverse

motion (G00), the programmed feedrate is ignored for that block, but is

stored in control memory as the active feedrate.

Feedrates are modal. They remain active in control memory unless

replaced with a different feedrate programmed with an F-word.

Feedrate modes are either G95 (cutting tool distance per workpiece

revolution) or G94 (cutting tool distance per minute). Table 18.A shows

the possible feedrate units depending on axis type.

Table 18.A

Feedrate Units

Active G-code

Linear Axis Feed

Rotary Axis Feed

G71 and G94

millimeters/min.

degrees/min.

G71 and G95

millimeters/rev.

degrees/rev.

G70 and G94

inches/min.

degrees/min.

G70 and G95

inches/rev.

degrees/rev.

Feedrates for linear and circular interpolation are “vector” feedrates. All

axes move simultaneously at independent feedrates so that the rate along

the effective path is equal to the programmed feedrate. See Figure 18.1.

18-1

Chapter 18

Programming Feedrates

Figure 18.1

Programming a Tangential Feedrate

Linear interpolation

Circular interpolation

programmed

end

feedrate

end point

point

X axis

feedrate

X axis

feedrate

start

point

Z axis

start

feedrate

point

For example, if a feedrate is programmed as F100.0 millimeters per

minute, and a linear move is made from X0, Z0 to X10, Z10, the feedrate

along that 45 degree angular path would be 100.0 mmpm. The actual

feedrate of each axis is approximately 70.7 millimeters per minute.

18.1.1

When the cutting tool is offset from a programmed path (as in the case of

TTRC), the programmed feedrate is applied to the center of the tool radius

Feedrates Applied During

for all linear and outside arc paths.

TTRC

For these paths:

The result:

linear

is not significant because the speed of the tool tip relative to the part

surface remains the same as the programmed feedrate.

outside arc

speed of the tool tip relative to the part surface is less than the

programmed feedrate. This generally causes no problem and so the

control does not take corrective action.

inside arc

speed of the tool tip relative to the part surface would be greater than

the programmed feedrate. Since this could cause excessive tool

loading and poor cutting performance, the 9/Series control

automatically takes corrective action.

18-2

Chapter 18

Programming Feedrates

For outside arc paths, the speed of the tool tip relative to the part surface

can be determined using the following formula:

R_p

Tool tip speed

= F x

----

R_c

Where :

Is :

programmed feedrate

R_c

radius of the arc measured to the center of the tool radius

R_p

programmed radius of the arc

Figure 18.2

Inside and Outside Arc Feedrates with TTRC

programmed tool path

tool radius center path

Cutting

outside arc

Cutting

inside arc

R_c < R_p

F is reduced

R_c > R_p

R_p Rc

F as programmed

R_c

R_p

For inside arc paths, the control automatically maintains the programmed

feedrate at the tool tip. The actual tool radius center feedrate reduces as

needed through the arc path, and then it returns to the programmed feedrate

after the arc is completed.

During inside arc paths, the control decreases the tool radius center

feedrate by the ratio of R_c/R_p. If the R_c value is very small compared to

R_p, as in the case of a small arc being cut with a large diameter tool, the

value of R_c/R_p is nearly zero, and the tool radius center feedrate becomes

excessively small.

To avoid this problem, your system installer must set a minimum feed

reduction percentage (MFR) in AMP. This sets a minimum feedrate to be

used whenever the value of R_c/R_p is very small. If R_c/R_p < MFR, the

control reduces the tool radius center feedrate no more than the MFR

percentage.

18-3

Chapter 18

Programming Feedrates

18.1.2

In the G94 mode (feed per minute), the numeric value following address F

represents the distance the axis or axes move (in inches or millimeters) per

Feed Per Minute Mode (G94)

minute. If the axis is a rotary axis, the F-word value represents the number

of degrees the axis rotates per minute.

To program a feedrate of 55 mm of tool motion per minute program:

G94 F55.;

Figure 18.3

Feed Per Minute Mode (G94)

Cutting tool

Chuck

Workpiece

“F” is the distance

the tool moves per minute.

When changing from G95 to G94 modes, you must program a feedrate in

the first G94 block.

Since the G94 code is modal, any F-word designated in any block after the

G94 is considered a feed distance per minute until a G95 is executed.

Important: The controlling spindle determines which spindle per

revolution value to use when calculating the feed per revolution.

18.1.3

In the G95 mode (feed per revolution), the numeric value following

Feed Per Revolution Mode

address F represents the distance the axis or axes move (in inches or

millimeters) per revolution of the spindle. If the axis is a rotary axis, the

(G95)

F-word value represents the number of degrees the axis rotates per

revolution of the spindle.

To program a feedrate of 1.5 mm per revolution of workpiece program:

G95 F1.5;

When changing from G94 to G95 modes, you must program a feedrate in

the first G95 block.

18-4

Chapter 18

Programming Feedrates

18.1.4

Rapid feedrate drives all active axes at a speed which creates a linear

move. The control determines which axis must travel the furthest and

Rapid Feedrate

drives that axis at its maximum feedrate assigned in AMP. Use rapid

feedrate to position the tool to a specified point at a high speed. It is called

during the execution of a G00 code followed by an axis motion command

and in many of the canned cycles for positioning.

After the execution of a rapid move the control restores the previously

commanded feedrate.

You can drive axes at their maximum allowable speeds during the jogging

operations by holding down the <TRVRS> button while executing a jog

move. (For details on jogging an axis see chapter 4).

Use rapid feedrate to position axes to a specified point at a high speed. It

is called by executing a G00 followed by an axis motion command. It also

is called automatically for some of the motions made by the fixed cycles.

See the fixed cycle specifications.

When you command more than one axis to move at rapid feedrate, they are

driven together to produce a linear move. The control drives one of the

axes at its rapid feedrate and reduces the feedrate of the others as required

to make certain that all axes start and stop at the same time.

18.1.5

<FEEDRATE OVERRIDE> Switch

Feedrate Overrides

You can override feedrates programmed in any of the feedrate modes

(G93/94/95) using the <FEEDRATE OVERRIDE> switch on the MTB panel.

The <FEEDRATE OVERRIDE> switch has a range of 0-150% of the

programmed feedrate, and it can alter the programmed feedrate in 10

percent increments.

The control checks whether the feedrate resulting from the

<FEEDRATE OVERRIDE> switch setting exceeds the maximum cutting

feedrate set in AMP. If it does, the feedrate is restricted to the AMP

maximum.

An M49 (overrides disabled) causes the override amounts that are set by

the switches on the MTB panel to be ignored by the control. With M49

active, the override switches for feedrate, rapid feedrate, and spindle speed

are all set to 100%. They can be enabled by programming an M48

(overrides enabled). See chapter 10 for details.

The feedrate override switch overrides the current axis feedrate. This may

or may not be the currently programmed feedrate. In cases where Acc/Dec

or the feedrate clamp features have overridden the programmed feedrate,

the feedrate override switch adjusts the new Acc/Dec or clamped feedrate.

18-6

Chapter 18

Programming Feedrates

Use <RAPID FEEDRATE OVERRIDE> on the MTB panel to override the

rapid feedrate for G00 mode in four increments:

F1 ---- percent value set in AMP by your system installer

25%

50%

100%.

Important: Normally this override is not active for any dry run motions

(see chapter 7) unless otherwise specified in PAL by your system installer.

Important: This override is also effective for jog moves that use the rapid

feedrate (see jogging using the <TRVRS> button in chapter 4).

Feedrate override switches disable

An M49 forces the override amounts that are set with the MTB panel to be

ignored by the control. With M49 active, the overrides for feedrate, rapid

feedrate, and spindle speed are all set to 100 percent. You can enable them

by programming an M48 (overrides enabled). See chapter 10 for details.

Feedhold

Your system installer can write PAL to allow the activation of a feedhold

state through the use of a button or switch. When activated, the control

decelerates and holds the current feedrate for all axes to zero until the

feedhold state is deactivated. For details on using feedhold, refer to

documentation provided by your system installer.

18-7

Chapter 18

Programming Feedrates

18.1.6

The maximum allowable speed for each axis is set in AMP. If any axis

feedrate exceeds the maximum allowable speed for that axis the control

Feedrate Limits (Clamp)

automatically adjusts the feedrate to a value that does not cause axis speed

to exceed its set limit.

Figure 18.5

Feedrate Clamp

F_XMAX

F_p

F_XMAX : maximum X axis feedrate

F_ZMAX : maximum Z axis feedrate

F_p

: programmed feedrate

: actual feedrate

F_ZMAX

In Figure 18.5, when the commanded feedrate is Fp it causes the Z-axis

feedrate to exceed the maximum feedrate (FzMAX). The control then

adjusts the feedrate for both axes so that F becomes the actual feedrate.

When the feedrate is “clamped” to a value below the programmed feedrate

the control displays a flashing C next to the current axes feedrate. The

displayed axis feedrate is the actual feedrate of the tool, not necessarily the

programmed feedrate.

18.2

You can select special feedrates that are assigned in AMP. This section

covers the feedrates assigned in AMP for the single-digit F-word and the

Special AMP-assigned

external feedrate switch.

Feedrates

18.2.1

Program a one-digit numeric value (1-9) following the F-code to select

various pre-set feedrates. The digits 1-9 have corresponding numeric

Single-digit F-words

values for feedrates set in the F1 - F9 table described in chapter 2.

18-8

Chapter 18

Programming Feedrates

Important: Single-digit feedrates are always entered as per minute

feedrates (IPM or MMPM) regardless of the control’s current feedrate

mode. When a single-digit feedrate is programmed, the control

automatically switches to the IPM or MMPM mode. The control

automatically switches back to the previously active feedrate mode when

the next feedrate is programmed that is not a single-digit feedrate.

If there are no feedrates set in the tables that correspond to F1-F9. The

control treats F1-F9 as commanded feedrates.

Single-digit F-word feedrates are affected by the setting of the

<FEEDRATE OVERRIDE> switch as regular feedrates. Blocks that are

programmed to move at the rapid feedrate are still executed in the rapid

mode.

Important: A programmed F0 corresponds to the maximum cutting

feedrate (not normally the rapid feedrate) set in AMP by your system

installer. F0 generates an error if the feature is not used.

When you call a single-digit F-word, the F-word must be programmed

with no decimal point and a single digit. For example, F1 calls an assigned

feedrate correlating to the value set as feedrate 1. Designating F1. in a

program assigns a feedrate of 1 in the current feedrate mode.

18.2.2

Your system installer can install an optional external deceleration switch.

External Deceleration

Typically this is a mechanical switch mounted on the machine axes inside

the hardware overtravel switches. Refer to documentation prepared by

Feedrate Switch

your system installer for details on the application and location of this

switch.

When you activate this feature, any axis moves that are to take place at a

cutting feedrate (G01, G02, G03, etc.) use a special feedrate assigned in

AMP. Any axis moves that are to take place at a rapid feedrate (G00, etc.)

also uses a special feedrate assigned in AMP. These feedrates are

independent of each other and typically have different values. These

feedrate changes take place immediately when the feature becomes active,

even if this is in the middle of block execution.

Important: The feedrate set for the external deceleration feature for

cutting moves cannot exceed the maximum cutting feedrate.

18-9

Chapter 18

Programming Feedrates

If you use this feature simultaneously with the Dry Run feature, the

feedrates that are assigned to the External deceleration feature are used.

The feedrates for this feature are not related to the Dry Run feedrates,

although the operation of this feature is similar to Dry Run.

This feedrate is unaffected by the <FEEDRATE OVERRIDE> switch and the

<RAPID FEEDRATE OVERRIDE> settings, and it operates as if the switches

are set at 100 percent. Blocks that are programmed to move at the rapid

feedrate are still executed in the rapid mode.

Use this feature to protect the machine from harsh or sudden stops. If a

very high feedrate is active at the time that a hardware overtravel occurs,

damage to the machine can result or the machine can coast past a safe

range for axis motion. If the switch is installed before the overtravel area,

the feedrate of the move is reduced and the amount of coast into the

overtravel area is much less.

If the current feedrate is less than the feedrate set for the external

deceleration feature, it is accelerated to the external deceleration feedrate.

This can cause problems with part finish or can damage the tool if this

feedrate is higher than that which the part should be cut.

WARNING: Your system installer can write PAL to allow the

operator to select the external deceleration feedrate at any time.

This means that during normal automatic operation, you can

select external deceleration and replace all feedrates in the

program with the external deceleration feedrates. This can

result in damage to the machine, part, or injury to the operator.

18.3

There are two types of axis acceleration/deceleration available. They are:

Automatic

Exponential Acc/Dec

Acceleration/Deceleration

Uniform or Linear Acc/Dec

S--Curve Acc/Dec

These are used to produce smooth starting and stopping of the machines

axes and prevent damage to the machine resulting from harsh movements.

Your system installer determines the acc/dec parameter type (exponential

or linear) for some manual motion types. To determine which motion

types are configurable, refer to the following table. Refer to your system

installer’s documentation for more information about how your system is

configured.

18-10

Chapter 18

Programming Feedrates

Refer to the table below to determine the type of acceleration/deceleration

performed for manual motion and programmed moves.

Table 18.B

Acc/Dec Type Performed with Manual Motion and Programmed Moves

Motion Type

Always Uses Exponential

Configurable in AMP by

Always Uses Linear

Linear or S- Curve

Acc/Dec

System Installer via

Acc/Dec

Acc/Dec per G- code

Manual Acc/Dec Mode

Hand--pulse generator

Arbitrary angle moves (i.e.,

hand--pulse generator and

continuous and incremental

motion)

Homing

All programmed moves except

for G00 and exact stop

Manual continuous motion

Manual incremental motion

PAL axis mover

All moves programmed in G00

(positioning) mode

18-11

Chapter 18

Programming Feedrates

18.3.1

To begin and complete a smooth axis motion, the 9/Series control uses an

exponential function curve to automatically accelerate/decelerate an axis.

Exponential Acc/Dec

Your system installer sets the acceleration/deceleration time constant “T”

for each axis in AMP. Figure 18.6 shows axis motion using exponential

Acc/Dec.

Figure 18.6

Exponential Acceleration/Deceleration

Velocity

“F”is the programmed feedrate

“T”is the acceleration/deceleration

time constant

Time

18-12

Chapter 18

Programming Feedrates

18.3.3

When S--Curve Acc/Dec is enabled, the control changes the velocity

profile to have an S--Curve shape during acceleration and deceleration

S-Curve Acc/Dec

when in Positioning or Exact Stop mode. This feature reduces the

machine’s axis shock and vibration for the commanded feedrates.

Figure 18.8 shows axis motion using S--Curve Acc/Dec.

Figure 18.8

S-Curve Acc/Dec

S--Curve

Acceleration

Deceleration

Commanded

Feedrate

Linear

Acc

Dec

Jerk

Time (sec)

Acceleration

Ramp

Time (sec)

Jerk

Time (sec)

18-14

Chapter 18

Programming Feedrates

18.3.4

Programmable Acc/Dec allows you to change the Linear Acc/Dec modes

and values within an active part program via G47.x and G48.x codes.

Programmable Acc/Dec

You cannot retrace through programmable acc/dec blocks (G47.x and

G48.x). However, you can retrace through blocks where programmable

acc/dec was already active.

Selecting Linear Acc/Dec Modes (G47.x - - modal)

Programming a G47.x in your part program allows you to switch Linear

Acc/Dec modes in nonmotion blocks. If S--Curve Acc/Dec is active, all

positioning moves within fixed cycles will use this mode.

G47 -- Linear Acc/Dec in All Modes

G47.1 -- S--Curve Acc/Dec for Positioning and Exact Stop Mode Only

G47.9 -- Infinite Acc/Dec (No Acc/Dec) (Enabled by your system

installer in AMP)

Important: For optimum S--Curve Acc/Dec functionality, any block

preceding a G47.1 block will decel to 0.

The table below shows you the interaction between contouring,

positioning, exact stop moves, and acc/dec type (i.e., linear, exponential,

S--Curve, and disabled).

Table 18.A

Interaction Between Contouring, Positioning, Exact Stop, and

Acc/Dec Modes

Programming:

In this mode will result in:

G00

G01

G02

G03

G47

Linear/

Linear

Exponential¹

G47 & G09/G61

Linear/

Linear

Exponential¹

G47.1

S--Curve/

Linear

Exponential²

G47.1 & G09/G61

S--Curve/

S--Curve

Linear

Exponential²

G47.9

Disabled

G47.9 & G09/G61

Disabled

¹Linear/Exponential is a function of Positioning Acc/Dec. If Exponential is AMPed, this is the acc/dec type,

otherwise, the type is Linear.

²S--Curve/Exponential is a function of Positioning Acc/Dec. If Exponential is AMPed, this is the acc/dec type,

otherwise, the type is S--Curve.

18-15

Chapter 18

Programming Feedrates

Selecting Linear Acc/Dec Values (G48.n - - nonmodal)

Programming a G48.x in your part program allows you to switch Linear

Acc/Dec values in nonmotion blocks. Axis values in G48.n blocks will

always be treated as absolute, even if the control is in incremental mode.

Below is the format for calling G48 commands. Use this format with the

axis names assigned by your system installer:

G48.n X_Y_Z_

Where :

In this mode :

Units of

Sets up :

Macros :

measure :

XYZ

G48

N/A

acceleration, deceleration, and jerk

N/A

ramps back to the AMPed values

Important: All axis words in a G48 are

ignored.

XYZ

G48.1

in./sec² or

acceleration ramps for Linear Acc/Dec

#5631 to 5642

mm/sec²

mode

G48.2

in./sec² or

deceleration ramps for Linear Acc/Dec

#5651 to 5662

mm/sec²

mode

G48.3

in./sec² or

acceleration ramps for S--Curve Acc/Dec

#5671 to 5682

mm/sec²

mode

G48.4

in./sec² or

deceleration ramps for S--Curve Acc/Dec

#5691 to 5701

mm/sec²

mode

G48.5

in./sec3 or

jerk limits

#5711 to 5722

mm/sec3

Important: The allowable programmed range for the axis word depends

on the configured format. If you exceed these allowable ranges set by your

system installer, you may use paramacros to override this limit.

For example, if the allowable programmed range for the axis word is 3.4

(e.g., 999.9999 max input) and the desired jerk limit is 100,000 mm/sec³,

you may set Paramacro #1 to 100,000 and program a G48.5 X#1 to set the

jerk limit to 100,000. This method can be used for any of the G48

programming blocks.

Example 18.1

Allowable Programmed Range

#1 = 100000;

G48.5 X #1;

Important: The part program G48.n adjustments to Acc/Dec Ramps are

not applied to jog moves. The AMPed Linear Acc/Dec mode rates are

used when Manual Acc/Dec mode is linear.

18-16

Chapter 18

Programming Feedrates

18.3.5

When Acc/Dec is active, the control automatically performs Acc/Dec to

give a smooth acceleration/deceleration for cutting tool motion.

Precautions on Corner

Cutting

However, there are cases in which Acc/Dec can result in rounded corners

on a part during cutting. In Figure 18.9, this problem is obvious when the

direction of cutting changes from the X axis to the Z axis. In this case, the

X axis decelerates as it completes its move, while the Z axis is at rest. As

soon as the X axis reaches the AMP defined in-position band, the Z axis

begins accelerating to make its commanded move. Since the Z axis begins

motions before the X axis finishes, a slight rounding results.

Figure 18.9

Rounding of Corners

Programmed tool path

Actual tool path

G64, G63

G09, G61

Cutting tool

Use these G-codes to eliminate corner rounding:

Exact Stop (G09 - - non-modal)

If a programmed motion block includes a G09, the axis moves to the

commanded position, decelerates, and comes to a complete stop before the

next axis motion block is executed. The G09 can be programmed in rapid

(G00), feedrate (G01), or circular (G02/G03) motion blocks, but it is active

only for the block in which it is programmed.

18-17

Chapter 18

Programming Feedrates

Exact Stop Mode (G61 - - modal)

G61 establishes the exact stop mode. The axes move to the commanded

position, decelerate and come to a complete stop before the next motion

block is executed. To cancel this mode, program G62, or G63.

Cutting Mode (G64 - - modal)

G64 establishes the cutting mode. This is the normal mode for axis motion

and is generally selected by your system installer as the default mode

active on power up. Block completes when the axes reach the interpolated

endpoint. To cancel this code, program G61, G62, or G63.

Tapping Mode (G63 - - modal)

In the G63 tapping mode, the feedrate override value is fixed at 100

percent, and a cycle stop is ignored. Axis motion commands are executed

without deceleration before the end point. The program proceeds to the

next block without checking in position status, similar to the operation of

G64. To cancel this code, program G61 or G62.

Automatic Corner Override (G62 - - modal)

In cutter compensation mode (G41/G42), the load on the cutter increases

while moving inside a corner. If the G62 automatic corner override mode

is active, the control automatically overrides the programmed feedrate to

reduce the load on the cutter. To cancel this code, program G61 or G63.

Figure 18.10

Automatic Corner Override (G62)

programmed tool path

tool center path

a b

18-18

Chapter 18

Programming Feedrates

When the corner angle, A, is larger than the value set for “min. angle for

corner override” in AMP, the programmed feedrate is overridden from

point “a” to point “b,” and from point “b” to point “c.”

The system installer sets these values in AMP:

Min angle for corner override -- minimum angle (A) between

programmed paths before corner override is activated

Corner override distance (DTC) -- vector distance from, and of current

move (b) to point on programmed path (a) where corner override is

activated

Corner override distance (DFC) -- vector distance from end of current

move (b) to point on programmed path (c) where corner override is

deactivated

Corner override percent -- amount that feedrate is to be reduced once

corner override is activated

To use an exact stop function while the automatic corner override mode

(G62) is active, use the G09 instead of the G61. This is because G61 and

G62 belong to the same G modal group and cancel each other if

programmed. Be aware that G09 is non-modal.

18.3.6

Your system installer has the ability to change the rate in which a spindle is

Spindle Acceleration (Ramp)

accelerated. AMP allows the option of either a 20 millisecond ramp (2ms

intervals) or an immediate step in spindle speed. By writing the

appropriate PAL your system installer may also in effect generate a spindle

“ramp” for even smoother spindle acceleration. Refer to documentation

prepared by your system installer.

18.3.7

In the default mode (G36), the Acc/Dec feature sometimes limits axis

feedrates far below the programmed feedrate. This occurs when the length

Short Block Acc/Dec Check

of axis motion in a block is short relative to the length of time necessary to

G36, G36.1

accelerate and decelerate the axis.

In the default mode (G36), the control limits the axis feedrate in any block

to the maximum speed from which it can properly decelerate to a stop

before that block ends. For example, consider the velocity profile of an

axis moving from Z4.8 to Z4.9 in Figure 18.11.

18-19

Chapter 18

Programming Feedrates

Figure 18.11

Programmed Feedrate Not Reached

F100

Programmed

feedrate

Feedrate clamped here to allow

F60

time for deceleration

Linear

Deceleration

Linear

Accel

Z4.8

Z4.9

Z5.0

Z5.1

12162-I

DISTANCE

Normally this causes no problem. However, in cases where a series of

very short axis moves in separate blocks exist, this limitation to the

feedrate can cause finish problems as well as increased cycle time.

Figure 18.12 shows the velocity profile that would result from a series of

short Z axis moves from 4.8 to 4.9 to 5.0 to 5.1 to 5.2.

Figure 18.12

Feedrate Limited Because of a Series of Short Moves

F100

Programmed

feedrate

Feedrate clamped

F60

Linear

Acceleration

Z4.8

Z4.9

Z5.0

Z5.1

Z5.2

DISTANCE

12163-I

18-20

Chapter 18

Programming Feedrates

To avoid this feedrate limitation, the short block Acc/Dec clamp can be

disabled by programming a G36.1. In this mode, the control assumes that

no rapid decelerations are required and allows axis velocities to go higher

than they otherwise would. Activate G36.1 mode only when:

no sudden changes in programmed feedrate within consecutive short

motion blocks exists (this includes requesting a feedhold or cycle stop)

no drastic change in programmed direction is present within the short

blocks

If any of these conditions are not met during the G36.1 mode, the control

can overshoot positions since the axes do not have time to decelerate. For

example, consider the following position and velocity plots if a drastic

change in direction is requested after the move from Z5.0 to Z5.1 when in

G36.1 mode (see Figure 18.13) . The position Z5.1 is overshot and the

axis would have to reverse direction to reach proper position.

Figure 18.13

Drastic Change in Direction while in Short Block Mode (G36.1)

Z-axis overshoots endpoint of

move because of drastic change

Series of short

in programmed direction.

move blocks.

Series of short

move blocks.

Programmed Feedrate

X1.9

Deceleration

Z-axis is traveling too

fast to stop when end

Acceleration

of move is reached.

X1.8

Z4.8

Z4.9

Z5.0

Z5.1

Z4.8

Z4.9

Z5.0

Z5.1

DISTANCE

12164-I

CAUTION: The programmer must consider the direction and

feedrate transitions from block to block when the short block

Acc/Dec check is disabled (G36.1 mode). If the transition

exceeds the deceleration ramp of the axis, damage to the part or

equipment can occur.

18-21

Chapter 18

Programming Feedrates

G36 and G36.1 are modal. The control should only be in short block

check disable mode (G36.1) when executing a series of fast short blocks

that contain only slight changes in direction and velocity. What constitutes

a slight change in direction and velocity depends on the Acc/Dec ramp

configured for your machine.

G36 -- Short Block Acc/Dec clamp Enable

G36.1 -- Short Block Acc/Dec clamp Disabled

G36 is the default mode, and it is established at power-up, E-STOP reset,

and end of program (M02, M30, or M99). The recommended method of

programming G36 and G36.1 is to program a relatively long entry and exit

move into and out of the mode.

The entry move should be a long move, in the general direction of the

first short move, and at the same feedrate as the first short move. This

entry move should be long enough for the axes to reach programmed

speed. Program the G36.1 code in this entry block

The exit move should be a long move, in the general direction of the

last short move, and at the same feedrate as the last short move. This

exit move should be long enough for the axes to decelerate properly

without overshooting their end points. Program the G36 code in this

exit block

Figure 18.14 shows the recommended entry and exit moves for short block

Acc/Dec clamp disable mode.

Figure 18.14

Entry and Exit Move to/from Short Block

Long Entry move.

Long Exit move.

This block contains a

This block contains

G36.1 command

a G36 command

Series of short move blocks

12165-I

END OF CHAPTER

18-22

Chapter

Dual Axis Operation

19.0

The Dual Axes feature lets the part programmer simultaneously control

multiple axes while programming commands for only one. It differs from

Chapter Overview

the split axis feature of the 9/Series control in that the split axis feature is

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

This chapter reviews the following major dual axis operations:

Topic:

On page:

Parking a dual axis

19-3

Homing a dual axis

19-4

Programming a dual axis

19-5

Offset management

19-7

The dual axes feature is especially useful for lathes with dual turrets and

other machines running with parallel cutting tools. Figure 19.1 shows a

typical configuration for dual axes.

Implementation of the dual axis feature can require significant PAL

modification as well as proper AMP configuration. The dual axis feature

is an option. Refer to your system installer’s documentation to see if the

dual axis option has been purchased for your machine.

19-1

Chapter 19

Dual Axis Operation

Figure 19.1

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 can support two dual axis groups. A dual axis group

consists of two or more axes coupled through AMP and commanded by a

master axis name. The master axis name is used by the part programmer

or operator when commanding the dual axis group in part programs or for

jog moves.

Each axis that makes up a dual group is controlled by a separate

positioning command from the servo module. This dual group command

is based on the move generated by the control when the master axis is

commanded to a position.

All axes that make up a dual group reach end-points at the same time. This

requires that all axes that make up a dual axis group share the same

feedrate parameters, acc/dec ramps, and other axes specific data for the

group.

This section requires that you understand these terms:

Master Axis -- A master axis is the name used to command the axes in a

dual group.

Dual Group -- A dual group is a set of axes that are coupled together in

AMP and commanded by a single master axis name.

19-2

9/Series CNC Lathe. Operation and Programming Manual - page 15