9/Series CNC Lathe. Operation and Programming Manual

Chapter 24

Compound Turning Routines

The G73 roughing routine activates the Tool Tip Radius Compensation

(TTRC) function regardless of whether it was active prior to the roughing

routine. If TTRC was not active, the roughing routine uses the tool tip

radius data of the previously programmed T-word. At the end of the

roughing routine, TTRC is cancelled unless it was active prior to the

roughing routine.

In Example 24.1, the workpiece contour blocks are blocks N11 - N14.

Example 24.1

Typical G73 Block Followed By Blocks Defining Final Contour

N005 G73 P11 Q14 U.2 W.2 D.12 F10.S210;

N010 M30;

N011 X25;

N012 X55 Z40;

N013 X65 Z35;

N014 X70 Z5;

The finish allowance words (U and W) in the G73 block are signed values

dependent on the workpiece contours. Figure 24.4 illustrates this with the

workpiece contour blocks generating the motions from point A to point C.

24-7

Chapter 24

Compound Turning Routines

G73 Tool Paths, Case 1

When the control executes a Case 1 G73 contouring path, these tool paths

are generated:

Figure 24.6

Tool Paths for Case 1 G73 Roughing Routine

Cutting feed

(start

Rapid feed

point)

Shape defined by workpiece

(I+K)/2

contour blocks

(U+W)/2

Final pass

(Optional)

In Figure 24.6:

The tool is moved from the start point parallel to the X axis, at a

feedrate F, a distance D as programmed in the G73 block.

A rough cut is made parallel to the Z axis, at a feedrate F to a point

that intersects the workpiece contour path, minus the finishing

allowance and final pass allowance (if any).

Retract from this point at a 45 degree angle, at a feedrate F, a distance

R measured parallel to the X axis. The R value may be entered as a

parameter in the G73 block. If no value for R is programmed then

the control uses the value for the retract amount set in AMP by the

system installer.

24-9

Chapter 24

Compounding Turning Routines

Figure 24.7

Tool Retraction in Case 1 G73

45°

Rapid traverse back along the X and Z axes to the coordinate that the

last rough cut started from in step 2.

Move parallel to the X axis, at a feedrate F, a distance D as

programmed in the G73 block.

Steps 2 - 5 continue to repeat until the operation is aborted or the rough

contour shape is completed. The rough contour shape is completed when

the thickness of the remaining material to be removed from the workpiece

is equal to the sum of the finishing allowance (U+W)/2 and the final pass

allowance (I+K)/2. If no final pass is to be cut (no I or K in the G73

block), skip to step 7.

The final pass is made at the feedrate programmed in your contour

block including rapid (if the contour does not contain a programmed

feedrate, then it uses the F-word in the G73 block). Only the amount

of material specified with the final pass allowance

(I+K)/2 is cut.

This cut is made parallel to the exact contour of the final workpiece,

it is not a roughing pass. After this cut is complete, the only

remaining material on the workpiece contour is the finish amount (if

any) programmed with U and W.

The control returns the cutting tool, at a rapid feedrate, to the start

point of the cycle.

24-10

Chapter 24

Compound Turning Routines

Example 24.2

Case 1 G73 Roughing Routine

N011 G00X80.Z150.;

N012 G73P14Q18U.8W.8I.6K.6D18.R7.F100;

N013 M30;

N014 X20.;

N015 Z110.;

N016 X40.Z80.;

N017 Z50.;

N018 X70.Z40.;

Figure 24.8

Results of Example 24.2

Start Point

(D)

1.4

Cutting feed

Rapid feed

40 50

110

140

In Figure 24.8, the final pass over the workpiece does not remove all

material from the final contour. A finishing pass is still required (typically

a G72) to remove the finish amounts U and W.

G73 Tool Paths, Case 2

If a pocket or multiple pockets are present in a workpiece contour, it

requires a Case 2 G73 contour turning routine.

For Case 2, the control cuts each pocket separately starting with the pocket

closest to the beginning of the operation. Figure 24.9 shows the tool paths

for a typical multiple pocket contour. The retract path used after each

roughing pass is different than for Case 1 roughing.

24-11

Chapter 24

Compound Turning Routines

Figure 24.10

Tool Motion in Case 2 G73

Cutting feed

Rapid feed

Start point

In Figure 24.10, these tool paths are made:

The tool is moved from the start point to first contour point at

feedrate F. This move must generate motion in both the X and Z

axes.

The control generates a rough cut towards the spindle centerline,

parallel to the workpiece contour, and offset by the finish allowance

amount and the final pass amount (if any). This rough cut continues

until the X axis value has decreased an amount D as programmed in

the G73 block.

A rough cut is made parallel to the Z axis, at a feedrate F, to a point

that intersects with the workpiece contour path minus the finish

allowance and final pass allowance (if any).

A rough cut is made away from the spindle’s centerline, parallel to

the workpiece contour, and offset by the finish allowance amount and

the final pass amount (if any). This rough cut continues, at a feedrate

F, until the X axis value has increased an amount D as programmed

in the G73 block (or until the last contour point is reached).

The tool is retracted from this point, on the X axis only, a distance R

as programmed in the G73 block (or the default distance R set in

AMP) at a feedrate F (see Figure 24.10)

A rapid traverse is made back along the X and Z axes to the Z

coordinate that the last rough cut started from (in step 3) and an X

coordinate that is D distance above the X coordinate of the last

rough cut.

24-13

Chapter 24

Compounding Turning Routines

A rough cut is made at feedrate F, into the workpiece parallel to the X

axis to the X coordinate of the last rough cut.

Steps 2 - 7 continue to repeat until the operation is aborted or the rough

contour shape is completed. The rough contour shape is completed when

the thickness of the remaining material to be removed from the contour is

equal to the sum of the finish allowance (U+W)/2 and the final pass

allowance (I+K)/2. If no final pass is to be cut, skip to step 9.

If a final pass is programmed in the G73 block (I or K values in the G73

block) it is not executed until all of the workpiece pockets have been

completely roughed out.

The final pass is made at the feedrate programmed in your contour

block including rapid moves (if no feedrate is programmed in the

contour blocks, the control uses the F-word in the G73 block). Only

the amount of material specified with the final pass allowance

(I+K)/2 is cut. This cut is made parallel to the exact contour of the

final workpiece, it is not a roughing pass. After this cut is complete,

the only remaining material on the workpiece contour is the finish

amount (if any) as programmed with U and W.

The control returns the cutting tool, at a rapid feedrate, to the start

point of the cycle.

Example 24.3

Case 2 G73 Roughing Routine

N010 G00X100.Z150.;

N011 G73P13Q20U.8W.8I.6K.6D10.R7.F100.;

N012 M30;

N013 X85.Z135.;

N014 X15.Z115.;

N015 Z82.;

N016 X45.Z72.;

N017 Z55.;

N018 X35.Z50.;

N019 Z22.;

N020 X80.Z7.;

24-14

Chapter 24

Compound Turning Routines

Figure 24.11

Results of Example 24.3

Cutting feed

Rapid feed

Start Point

100

(I+K+U+W)/2

1.4

100

120

140

24.2

The G74 rough facing routine is used to rough out the contour of a

workpiece by making repetitive cuts parallel to the X axis. A final pass

Rough Facing Routine (G74)

may be made with this routine to cut parallel to the final contour of the

workpiece. At the completion of this routine a finish allowance may also

be left on the workpiece to be removed later by a G72 finishing routine.

This routine may be used in conjunction with Tool Tip Radius

Compensation (TTRC). If TTRC is active when the routine is executed the

tool radius is taken into consideration on each consecutive pass.

24-15

Chapter 24

Compounding Turning Routines

Figure 24.12

Stock Removal in G74 Rough Facing

Tool paths determined automatically

Start point

Shape after roughing

and final pass

Workpiece finished

Finishing allowance

shape

The G74 block has a P and Q parameter that call the sequence numbers

(N-words) of the first and last blocks defining the final contour to be cut

into the workpiece. This set of blocks may be located anywhere after the

calling block (even after an end of program command), as long as the

calling block is in the same program as the set of contour defining blocks.

This means that contour blocks can not be called from a subprogram or a

macro unless the calling block is in that subprogram or macro.

The control handles two different cases of the G74 routine and

automatically recognizes them and adapts the tool path accordingly.

Case 1:

A Case 1 G74 rough facing routine is defined when the workpiece contour

has no pockets. The following constraints must be met in order to

successfully perform a Case 1 rough facing routine:

The first block of the contour program must command motion in only

the Z axis. No X axis motion is permitted in the first block of the

contour program.

The contour either continuously increases or continuously decreases in

both the X and Z axis except for the first block of the contour program.

The first contour point in the contour blocks must be closer to the

spindle centerline than the last contour point.

24-16

Chapter 24

Compound Turning Routines

Case 2:

A Case 2 G74 rough facing routine is defined when a workpiece contour

contains a pocket. The following constraints must be met in order to

successfully perform a Case 2 rough facing routine:

The first block of the contour program must contain motion in both the

X and Z axis (the move from the start point to the first contour point

must have motion in both axes).

The workpiece contour may increase or decrease along the Z axis after

the first contour block. The workpiece contour must either continuously

increase or continuously decrease along the X axis after the first contour

block.

The first contour point of the contour blocks must be farther away (or at

least equidistant) from the spindle face than the last contour point

The first and last contour blocks must define beginning and ending sides

to the contour. The first programmed endpoint must be farther away

from the spindle face than the second programmed endpoint. The last

programmed endpoint must be farther away from the spindle face than

the next to last programmed endpoint.

Figure 24.13

Workpiece Finish Contour Case 1 and Case 2 (G74)

Case 1

Case 2

Start Point

Start

point

The G74 block is programmed with the following format:

G74P__Q__U__W__I__K__D__R__F__S__T__;

24-17

Chapter 24

Compounding Turning Routines

Where :

Is :

P__

the sequence number (N-word) of the first block in the set of contour blocks that

define the final contour.

Q__

the sequence number (N-word) of the last block in the set of contour blocks that

define the final contour.

determine the finishing allowance that is left on the part when the routine is

completed. This finish allowance is typically removed later in the program when

a G72 finishing routine block is executed. The actual value of the finish

allowance is equal to the average of the U and W parameters (U+W)/2. It is not

necessary to enter both of these parameters in the calling block. If only one is

entered, the control uses half of the entered parameter value as the finish

amount. The finish allowance is optional and does not need to be programmed.

See Figure 24.15 to determine the sign of U and W. U and W are always

programmed as incremental values.

Important: This manual makes the assumption that W and U are assigned

in AMP as the incremental axis names that correspond to the Z and X axes

respectively.

Important: The value assigned to U is affected by radius/diameter mode

(G08/G09). W is not affected by radius diameter mode. If programming in

diameter mode the value of the finish allowance is really ((U/2)+W)/2.

determine the amount of stock to be removed on the final pass of the routine.

The actual amount of material removed on this final pass is equal to the average

of the I and K parameters (I+K)/2. It is not necessary to enter both of these

parameters in the calling block. If only one is entered the control uses half of the

entered parameter value. The final pass is optional and does not need to be

programmed. It is not a roughing pass and it does not remove the finish

allowance. A final pass cuts tool paths that are parallel to the workpiece finish

shape.

Important: This manual makes the assumption that I and K are assigned in

AMP as the integrand axis names that correspond to the X and Z axes

respectively.

Important: The value assigned to I is always an incremental, radius value

regardless of the current mode (radius/diameter). K is always an incremental

value and is not affected by radius/diameter mode.

Important: The system installer has the option of forcing a final pass to be

made by setting the proper AMP parameter. If this is the case the control cuts

the final pass regardless of whether I or K is programmed. When I and K are not

programmed and the system installer has forced a final pass to be made, the

control assumes I and K to be zero.

D__

the depth of cut for each pass except the final pass. No sign needs to be entered

for this parameter. The depth of cut for the final pass is determined with the I and

K parameters. D is always an incremental value regardless of the current mode.

Important: It is possible to override the programmed depth of cut (D) using

an AMP parameter. The override setting is made in increments of 1% ranging

from 0-255%. See documentation prepared by the system installer for details.

The system installer may also determine a maximum allowable value of D in

AMP. If the D value programmed is larger than the maximum allowed in AMP,

the control overrides the programmed value and use the AMP assigned

maximum value.

24-18

Chapter 24

Compound Turning Routines

Where :

Is :

R__

used to program the retract amount made after each rough facing pass. This

retract amount is an incremental, radius value measured parallel to the Z axis.

Case 1 operations retract at a 45 degree angle to the Z axis and Case 2

operations retract parallel to the Z axis. This does not affect the programmed

value of R, as R is always measured parallel to Z. If no value for R is

programmed then the control uses a value for the retract amount set in AMP by

the system installer.

Active feedrate during the routine only (see chapter 17)

Spindle speed during the routine only (see chapter 16)

Tool number and tool offset to be used during the routine only (see chapter 19)

Important: Any F-, S-, or T-words that are in the set of contour blocks are

ignored when the routine is executed. If programmed in the G74 block

these words replace any previously active modal F-, S-, or T-words for the

remainder of G74 routine operation only. When the G74 routine is

completed the previously active modal F-, S-, and T-words are reactivated.

Figure 24.14

Parameters for G74 Rough Facing

(I+K)/2

Start point

Shape after roughing

and final pass

Workpiece finished

(U+W)/2

shape

24-19

Chapter 24

Compounding Turning Routines

In Figure 24.14, the contour blocks for this routine must define all motions

that would cut the workpiece finished shape. The first block of the contour

blocks must be the tool path from the start point to the point where the

initial roughing pass begins. The first block of the contour blocks may not

be a rapid move (G00).

Important: The blocks preceding the G74 roughing block must have

positioned the cutting tool to a location above the part (start point in the

above figure) from which it can safely move to begin the roughing passes.

If cutting a Case 1 contour, the first of the contour blocks must command Z

axis motion only (no X axis motion). If cutting a Case 2 contour, the first

of the contour blocks must command both an X and Z axis motion.

The G74 roughing routine activates the Tool Tip Radius Compensation

(TTRC) function regardless of whether it was active prior to the roughing

routine. If TTRC was not active, the roughing routine uses the tool tip

radius data of the previously programmed T-word. At the end of the

roughing routine, TTRC is cancelled unless it was active prior to the

roughing routine.

In Example 24.4, the workpiece contour blocks are blocks N11 - N14.

Example 24.4

Typical G74 Block Followed by Blocks Defining Final Contour

N005 G74 P11 Q14 U.2 W.2 D1.2 F10. S210;

N010 M30;

N011 Z25;

N012 X55 Z40;

N013 X40 Z65;

N014 X30 Z75;

The finish allowance words (U and W) in the G74 block are a signed value

dependant on the workpiece contours. Figure 24.15 illustrates this with the

workpiece contour blocks generating the motions from point A to C.

24-20

Chapter 24

Compounding Turning Routines

G74 Tool Paths, Case 1

When the control executes a Case 1 G74 rough facing routine the

following tool paths are generated:

Figure 24.17

Tool Paths for Case 1 G74 Rough Facing

(I+K)

start

point

Cutting feed

Rapid feed

Shape defined by

workpiece contour

blocks

Final Pass

(optional)

(U+W)/2

In Figure 24.17:

1. The tool is moved from the start point parallel to the Z axis, at a

feedrate F, a distance D as programmed in the G73 block.

2. A rough cut is made parallel to the X axis, at a feedrate F to a point

that intersects the workpiece contour path, minus the finishing

allowance and final pass allowance (if any).

3. Retract from this point at a 45 degree angle, at a feedrate F, a distance

R measured parallel to the Z axis. The R value may be entered as a

parameter in the G74 block. If no value for R is programmed then the

control uses the value for the retract amount set in AMP by the

system installer.

24-22

Chapter 24

Compound Turning Routines

Figure 24.18

Tool Retraction in Case 1 G74

45°

4. Rapid traverse back along the X and Z axes to the coordinate that the

last rough cut started from (in step 2).

5. Move parallel to the Z axis, at a feedrate F, a distance D as

programmed in the G74 block.

Steps 2 - 5 continue to repeat until the operation is aborted or the rough

contour shape is completed. The rough contour shape is completed when

the thickness of the remaining material to be removed from the workpiece

is equal to the sum of the finishing allowance (U+W)/2 and the final pass

allowance (I+K)/2. If no final pass is to be made skip to step 7.

6. The final pass is made at the feedrate programmed in your contour

block including any rapid moves (if no feedrate is programmed in the

contour blocks the control uses the F-word programmed in the G74

block). Only the amount of material specified with the final pass

allowance (I+K)/2 is cut. This cut is made parallel to the exact

contour of the final workpiece, it is not a roughing pass. After this

cut is complete, the only remaining material on the workpiece contour

is the finish amount (if any) programmed with U and W.

7. The control returns the cutting tool, at a rapid feedrate, to the start

point of the cycle.

24-23

Chapter 24

Compound Turning Routines

G74 Tool Paths, Case 2

If a pocket or multiple pockets are present in a workpiece face, it requires a

Case 2 G74 rough facing routine.

For Case 2, the control cuts each pocket separately, starting with the pocket

closest to the beginning of the operation. Figure 24.20 shows the tool

paths for a typical multiple pocket contour. The retract path used after

each roughing pass is different than for Case 1 rough facing.

Figure 24.20

Tool Paths for Case 2 G74 Rough Facing Routine (with pockets)

Start Point

Cutting feed

Rapid feed

(U+W+I+K)/2

Important: Figure 24.20 does not show the optional final pass being

made. This is for drawing clarity.

In Figure 24.20, after the roughing passes of one pocket have been

completed, the control does not perform a normal retract move out of the

pocket. Instead the control follows the part contour out of the pocket and

then proceeds on to the next pocket or finishes the routine.

24-25

Chapter 24

Compounding Turning Routines

Figure 24.21

Tool Motion in Case 2 G74

Start point

Cutting feed

Rapid feed

In Figure 24.21, these tool paths are made:

1. The tool is moved from the start point to the first contour point at

feedrate F. This move must generate motion in both the X and Z

axes.

2. The control generates a rough cut towards the spindle face, parallel to

the workpiece contour, and offset by the finish allowance amount and

the final pass amount (if any). This rough cut continues until the Z

axis value has decreased an amount D as programmed in the G74

block.

3. A rough cut is made parallel to the X axis, at a feedrate F, to a point

that intersects with the workpiece contour path minus the finish

allowance and final pass allowance (if any).

4. A rough cut is made away form the spindle face, parallel to the

workpiece contour, and offset by the finish allowance amount and the

final pass amount (if any). This rough cut continues, at a feedrate F,

until the Z axis value has increased an amount D as programmed in

the G74 block.

5. The tool is retracted from this point, on the Z axis only, a distance R

as programmed in the G74 block (or the default distance R set in

AMP) at a feedrate F (see Figure 24.21).

24-26

Chapter 24

Compound Turning Routines

6. A rapid traverse is made back along the X and Z axes to the X

coordinate that the last rough cut started from (in step 3) and a Z

coordinate that is D distance above the Z coordinate of the last rough

cut.

7. A rough cut is made at feedrate F, into the workpiece parallel to the Z

axis to the Z coordinate of the last rough cut.

Steps 2 - 7 continue to repeat until the operation is aborted or the contour

shape is completed. The contour shape is completed when the thickness of

the material remaining to be removed from the contour is equal to the sum

of the finish allowance (U+W)/2 and the final pass allowance (I+K)/2. If

no final pass is to be cut, skip to step 9.

If a final pass is programmed in the G74 block (I or K values in the G74

block) it is not executed until all of the workpiece pockets have been

completely roughed out.

8. The final pass is made at the feedrate programmed in your contour

block including any rapid moves (if no feedrate is programmed in the

contour blocks, the control uses the F-word programmed in the G74

block). Only the amount of material specified with the final pass

allowance (I+K)/2 is cut. This cut is made parallel to the exact

contour of the final workpiece, it is not a roughing pass. After this

cut is complete, the only material remaining on the workpiece contour

is the finish amount (if any) as programmed with U and W.

9. The control returns the cutting tool, at a rapid feedrate, to the start

point of the cycle.

Example 24.6

Case 2 G74 Rough Facing Routine

N011 G00X128.Z120.;

N012 G74P14Q21U.6W.6I.8K.8D10.R7.F10.S60;

N013 M30;

N014 X120.Z110.;

N015 X100.Z30.;

N016 X80.;

N017 X70.Z70.;

N018 X60.;

N019 X50.Z50.;

N020 X30.;

N021 X20.Z107.;

24-27

Chapter 24

Compound Turning Routines

24.3

In the G75 casting/forging roughing routine (also called pattern repeating

routine), the control generates multiple cuts, each parallel to the workpiece

Casting/Forging Roughing

final shape. Each cut is offset from the other an amount determined by the

Routine (G75)

I, K and D parameters.

Through this process, a shape similar to the finished contour is obtained

when the routine is completed. At the completion of this routine a finish

allowance is usually left on the workpiece to be removed later by a G72

finishing routine.

Figure 24.23

Pattern Repeating Routine

Cutting feed

Rapid feed

(start point)

Note: Tool paths not to scale.

Shape defined by

workpiece contour blocks

Finishing pass

The calling block references the sequence numbers (N-words) of the first

and last blocks of the contour blocks defining the final contour of the

workpiece. This set of blocks may be located anywhere after the calling

block (even after an end of program command), as long as the calling

block is in the same program as the set of contour defining blocks.

Contour blocks cannot be in a subprogram or a macro unless the calling

block is in that subprogram or macro.

24-29

Chapter 24

Compounding Turning Routines

The G75 block is programmed with this format:

G75 P__

Q__ I__ K__ U__ W__ D__ F__ S__ T__;

Where :

Is :

P__

The sequence number of the first block in the set of contour blocks that defines the

finished workpiece shape.

Q__

The sequence number of the last block in the set of contour blocks that defines the

finished workpiece shape.

Finish allowance. These parameters determine the finishing allowance that is left on

the part when the routine is completed. This finish allowance is typically removed

later in the program when a G72 finishing routine block is executed. The actual value

of the finish allowance is equal to the average of the U and W parameters ((U+W)/2).

It is not necessary to enter both of these parameters in the calling block. If only one

is entered, the control uses half of the entered parameter value as the finish amount.

The finish allowance is optional and does not need to be programmed. See

Figure 24.25 to determine the sign of U and W. U and W are always programmed as

incremental values.

Important: This manual makes the assumption that W and U are assigned in

AMP as the incremental axis names that correspond to the Z and X axes

respectively.

Important: The value assigned to U is affected by radius/diameter mode

(G08/G09). W is not affected by radius diameter mode. If programming in diameter

mode the value of the finish allowance is really ((U/2)+W)/2.

These parameters determine the incremental distance between the first and last pass

of the routine. This distance is equal to the average of the I and K parameters

((I+K)/2). The location of the last pass is determined by the contour blocks and the

finish amount ((U+W)/2), if any is programmed. I and K must be programmed. They

are neither positive nor negative.

Important: This total incremental distance should be less than one tool radius if

cutter compensation is on when this cycle is executed.

Important: This manual makes the assumption that K and I are assigned in

AMP as the integrand axis names that correspond to the Z and X axes respectively.

Important: The values assigned to I and K are always an incremental, radius

value regardless of the current mode (radius/diameter or absolute/incremental).

D__

Number of passes. The integer value entered with this parameter determines how

many passes are made to reach the final pass. The depth of each pass is

determined by dividing (I+K)/2 by D-1. The value entered with D must be an integer.

F__

Active feedrate during the routine only (see chapter 17)

S__

Spindle speed during the routine only (see chapter 16)

T__

Tool number and tool offset to be used during the routine only (see chapter 19)

Important: Any F-, S-, or T-words that are in the set of contour blocks are

ignored when the routine is executed. If these words are to be changed

from their current value, it is necessary to program an F-, S-, or T-word in

the G75 block. If programmed in the G75 block these words replace any

previously active modal F-, S-, or T-words for the remainder of G75

routine operation only. When the G75 routine is completed the previously

active modal F-, S-, and T-words are reactivated.

24-30

Chapter 24

Compound Turning Routines

Figure 24.24

Pattern Repeating Routine Parameters

Cutting feed

Rapid feed

(start point)

Note: Tool paths not to scale.

Shape defined by

workpiece contour blocks

(I+K)/2

Finishing pass

(U+W)/2

In Figure 24.24, the contour blocks for this routine must define all motions

that would cut the workpiece finished shape and the tool path that connects

the start point of the routine to the first block of the workpiece finished

shape. The first block of the contour blocks must be the tool path from the

start point to the first block of the workpiece finished shape. It is assumed

that some other blocks have positioned the cutting tool to a position above

the part (start point in the above figure).

The arc and pocket in the example above get smaller and smaller as the

passes get farther away from the final contour. If you specify passes very

far from the final contour, the cutting tool can be too large to cut the

resulting arc or pocket. When this occurs the control generates the error

message “INVALID CYCLE PROFILE”. Resolve this problem by making

the distance from the final pass to the first pass smaller. This cycle was not

designed to remove large amounts of material. Its intended design is to

perform cleanup passes on castings or forgings. If you must remove large

amounts of material you should use one of the roughing/facing routines

discussed earlier in this chapter.

24-31

Chapter 24

Compounding Turning Routines

Prevent this invalid cycle profile error by keeping the right portion of the

following equation less than the radius of any arcs in your cycle profile.

R² p(I+U)2 + (K+W)2

+ (tool radius)

The same basic equation can apply to other contours. If the length of a

block in the contour is less than the right portion of the above equation,

you can get an “INVALID CYCLE PROFILE” error depending on your

part contour. For contours with pockets, the width of the pocket must be at

least twice the value of the right hand portion of the above equation. In

general this error is a result of removing metal too far from the original

part profile (I, K, U, or W too large) and reducing this distance typically

resolves the error condition.

The workpiece contour blocks can be at any location within the same

program containing the G75 block (even after an end of program block).

They can not be resident in a subprogram or macro that is called by the

program containing the G75 block. Contour blocks can be either circular

or linear blocks. Any F-, S-, or T-words that are programmed in this set of

contour blocks are ignored when they are executed as workpiece contour

blocks in the G75 mode.

In Example 24.7, the workpiece contour blocks are blocks N11 - N14.

Example 24.7

Typical G75 Block Followed By Blocks Defining Final Contour

N005 G75P11Q14I2.W2.D3.F10.S210;

N010 M30.;

N011 X24.;

N012 X55.Z40.;

N013 X65.Z35.;

N014 X70.Z5.;

The control generates multiple passes each offset from the other by an

amount equal to the total material to be removed (I+K/2) divided by the

number of passes (D) minus 1. The tool paths repeat until (D) tool paths

have been made across the part. Each tool path is shifted sequentially by

the distance obtained in this division to generate roughing paths. If a

finishing allowance (U, W) was programmed in the block, it is left uncut.

After the completion of the roughing routine, the cutting tool returns to the

routines starting point.

24-32

Chapter 24

Compound Turning Routines

The G75 routine can be programmed while the tool tip radius

compensation mode (G41 or G42) is active. If tool tip radius

compensation is active prior to the G75 block it remains active throughout

the execution of the routine.

The G75 roughing routine activates the Tool Tip Radius Compensation

(TTRC) function regardless of whether it was active prior to the roughing

routine. If TTRC was active, the roughing routine uses the previously

programmed T-word to compensate for the tool tip radius. At the end of

the roughing routine, TTRC is cancelled unless it was active prior to the

roughing routine.

The finish allowance words (U and W) in the G75 block are signed values

dependant on the workpiece contours. Figure 24.25 illustrates this with the

workpiece contour program generating the blocks from point A to C.

Figure 24.25

Effect of Positive and Negative Finish Allowance Parameters

U(+), W(+)

U(+). W(-)

U(-), W(+)

U(-), W(-)

The control generates multiple passes each offset from the other by an

amount equal to the total material to be removed (I and K) divided by the

number of passes (D) minus 1. These tool paths repeat until (D) tool paths

have been made across the part. At completion of the last path the tool

returns to the start point of the routine.

24-33

Chapter 24

Compound Turning Routines

24.4

The G72 finish routine is normally executed after the completion of a

contouring routine (G73, G74 or G75). With the G73, G74, and G75

O.D. and I.D. Finishing

routines a finish allowance is left on the workpiece if a U- and/or K-word

Routine (G72)

is specified in the routine. The G72 routine is used to remove this finish

allowance and cut the workpiece to within the specified tolerance of the

actual workpiece finished shape.

The calling block references sequence numbers of the first and last blocks

of the contour blocks defining the final contour of the workpiece. This set

of blocks may be located anywhere after the calling block (even after an

end of program command), as long as the calling block is in the same

program as the set of contour defining blocks. This means that contour

blocks can not be called from a subprogram or a macro unless the calling

block is in that subprogram or macro. This routine actually executes the

set of contour defining blocks as entered in the program.

The G72 finishing routine is usually performed at a lower feedrate to

produce the desired finish results that are not necessary using the other

rough contouring routines for rapid removal of material.

The program format for this finishing routine is indicated below:

G72 P__ Q__;

Where :

Is :

P__

The sequence number of the first block in the set of contour blocks that defines

the finished workpiece shape.

Q__

The sequence number of the last block in the set of contour blocks that defines

the finished workpiece shape.

In the G72 finishing routine, the contour of the finished workpiece can be

described by a set of linear and/or circular blocks bounded by the sequence

numbers specified with parameters P and Q. It is assumed that some other

blocks have positioned the cutting tool to some position above the part.

This position should be the start point of the workpiece contour blocks.

The workpiece contour blocks may be at any location within the same

program containing the G72 block (even after an end of program M02 or

M30). They may not be resident in a subprogram or macro that is called

by the program containing the G72 block.

The control recognizes F-, S-, or T-words programmed in this set of

contour blocks and uses these values for the routines execution. These

values are not ignored as in the G73, G74, and G75 routines (F-words are

used in the G73, G74, and G75 routines).

24-35

9/Series CNC Lathe. Operation and Programming Manual - page 20