Content      ..     17      18      19      20     ..

9/Series CNC Lathe. Operation and Programming Manual - page 19

Chapter 22

Single-Pass Turning Cycles

Important: Descriptions in this chapter are written assuming the control is

in the G18 plane and that plane has been defined as the ZX plane. If your

system has a different plane active, operation of these features is different.

Parameters are defined here assuming Z is the first axis in the plane, and X

is the second axis in the plane. If, for example, the XZ plane is the

currently active plane, descriptions in this document should be interpreted

accordingly (i.e., Z axis description applies for X axis and X axis

description applies to Z axis. See your system installer’s documentation

for details on the plane definitions on your system.

22.1

G20 calls either a straight or a taper cutting cycle. This cycle is a

single-pass cycle.

Single-pass O.D. and I.D.

Roughing Cycle (G20)

Use the G20 cycle to cut along the diameter of a workpiece (in this manual

that means cuts parallel to the Z axis). The G20 cycle basically consists of

the moves shown in Figure 22.1.

Figure 22.1

G20 Straight Cutting Cycle

X

Cutting feed

Rapid feed

4

3

1

2

Z

1.

Rapid approach to the part

2.

Cutting feed into the part

3.

Cutting feed out of the part

4.

Rapid return to the start point

22-2

Chapter 22

Single-Pass Turning Cycles

CAUTION: When programming the single-pass cycle, the first

move to the depth of cut is a rapid move. Make sure that the

tool does not contact the part on this initial move.

The feedrate used in the single-pass cycle is the currently active

programmed cutting feedrate. If desired, a different cutting feedrate may

be specified in the single-pass cycle block.

The rapid feedrate (for the axis in motion as assigned in AMP) is used for

the approach to the part and the return to start point.

G20 Straight O.D. and I.D. Roughing

The format for the G20 straight cutting cycle is as follows:

G20X__ Z__;

Where :

Is :

X__

is the depth of cut for the X axis. In incremental mode, specify the amount of

infeed. In absolute mode, specify the coordinate position at the desired depth of

cut. X may be programmed as either a diameter or radius value.

Z__

is the length of cut along the Z axis. In incremental, specify the amount of feed

across the part. In absolute, specify the coordinate position of the end point of the

cutting stroke.

After the G20 block is executed, the control re-executes the cycle for any

following block that commands axis motion (until the cycle is cancelled).

The value of the axis word in that block is used to replace the parameter

determined with that axis word in the original G20 block and the cycle is

re-executed using these new parameters.

22-3

Chapter 22

Single-Pass Turning Cycles

Example 22.1

Straight Cutting Cycle

G90G00X40.Z60.;

G20X28.Z25.F10.

X24.;

X20.;

G00;

Figure 22.2

Results of Example 22.1

X

25

35

Cutting feed

Rapid feed

28

24

20

Z

22-4

Chapter 22

Single-Pass Turning Cycles

G20 Taper O.D. and I.D. Roughing

A G20 block that includes an I-word generates a turning pass that produces

a taper.

Figure 22.3

G20 Taper Cutting Cycle

X

Cutting feed

Rapid feed

I

Z

The format for the G20 single-pass cycle to cut a taper is:

G20X__Z__I__;

Where :

Is :

X__

the depth of cut for the X axis at the end point of the cutting move into the part.

In incremental mode specify the amount of infeed, in absolute mode specify the

coordinate position at the desired depth of cut. X may be programmed as either

a diameter or radius value.

Z__

the length of cut along the Z axis. In incremental mode specify the amount of

feed across the part, in absolute mode specify the coordinate position of the end

point of the cutting stroke.

I__

the amount of change in the depth of cut for the X axis. I is always an

incremental radius value. Figure 22.4 shows the relationship between the sign of

the I value and the way that the cycle is performed. The control adds the value

of I to the X depth to determine the start point of the cutting pass.

22-5

Chapter 22

Single-Pass Turning Cycles

After the G20 block is executed, the control re-executes the cycle for any

following block that commands axis motion (until the cycle is cancelled).

The value of the axis word in that block is used to replace the parameter

determined with that axis word in the original G20 block and the cycle is

re-executed using these new parameters.

Figure 22.4 applies only if programming X and Z as incremental values. If

programming X and Z as absolute values, the depth of taper I is added or

subtracted (depending on its sign) to the absolute X axis position.

Figure 22.4

Effect of Positive and Negative Parameters in a G20 Block

When X,Z, and I are negative

When X and Z are negative

G20 X-__ Z-__ I-__ ;

and I is positive

G20 X-__ Z-__ I+__ ;

X

X

I

Note : ˙ I ˙ £ ˙ X ˙

I

Z

Z

Cutting feed

When X and I are positive

When X is positive and

and Z is negative

Z and I are negative

Rapid feed

G20 X+__ Z-__ I+__ ;

G20 X+__ Z-__ I-__ ;

I

I

Note : ˙ I ˙ £ ˙ X ˙

X

X

Z

Z

22-6

Chapter 22

Single-Pass Turning Cycles

Example 22.2

Taper Cutting

G90G00X50.Z106.;

G20X38.Z46.I-11.F.5;

X32.;

X26.;

X20.;

Figure 22.5

Results of Example 22.2

X

46

60

11

38

32

26

20

Z

Cutting feed

Rapid feed

22-7

Chapter 22

Single-Pass Turning Cycles

22.2

G24 calls either a straight or a tapered facing cycle. This cycle is a

single-pass cycle (makes only one cutting pass over the workpiece each

Single-pass Rough Facing

time it is called).

Cycle (G24)

Use the G24 cycle to cut along the face of a workpiece (in this manual that

means it cuts along the X axis). The G24 cycle basically consists of the

moves shown in Figure 22.6.

Figure 22.6

G24 Straight Facing Cycle

1.

Rapid approach to the part

2.

Cutting feed into the part

3.

Cutting feed out of the part

4.

Rapid return to the start point

X

1

2

4

3

Z

Cutting feed

Rapid feed

CAUTION: When programming the single-pass cycle, the first

move to the depth of cut is a rapid move. Make sure that the

tool does not contact the part on this initial move.

22-8

Chapter 22

Single-Pass Turning Cycles

The feedrate used in the single-pass cycle is the currently active

programmed cutting feedrate. If desired, a different cutting feedrate may

be specified in the single-pass cycle block.

The rapid feedrate (for the axis in motion as assigned in AMP) is used for

the approach to the part and the return to start point.

G24 Straight Facing

The format for the G24 straight facing cycle is:

G24X__ Z__;

Where :

Is :

X__

the length of cut along the X axis. In incremental mode, specify the amount of feed

across the part. In absolute mode, specify the coordinate position of the end point of

the cutting stroke. X may be programmed as either a diameter or radius value.

Z__

the depth of cut for the Z axis. In incremental mode, specify the amount of infeed. In

absolute mode, specify the coordinate position at the desired depth of cut.

After the G24 block is executed, the control re-executes the cycle for any

following block that commands axis motion (until the cycle is cancelled).

The value of the axis word in that block is used to replace the parameter

determined with that axis word in the original G24 block and the cycle is

re-executed using these new parameters.

22-9

Chapter 22

Single-Pass Turning Cycles

Example 22.3

Straight Facing Cycle

G90G00X30.Z22.;

G24X10.Z15.F10.

Z13.;

Z11.;

G00;

Figure 22.7

Results of Example 22.3

Cutting feed

X

Rapid feed

15

13

11

10

Z

22-10

Chapter 22

Single-Pass Turning Cycles

G24 Tapered Facing

A G24 block that includes a K-word generates a facing pass that produces

a taper.

Figure 22.8

G24 Face Taper Cutting Cycle

X

K

Z

Cutting feed

Rapid feed

The format for the G24 single-pass cycle to cut a taper on a face is:

G24X__Z__K__;

Where :

Is :

X__

the length of cut along the X axis. In incremental mode specify the amount of

feed across the part, in absolute mode specify the coordinate position of the end

point of the cutting stroke. X maybe programmed as either a diameter or radius

value.

Z__

the depth of cut for the Z axis at the end point of the cutting move into the part.

In incremental mode specify the amount of infeed, in absolute mode specify the

coordinate position at the desired depth of cut.

K__

the amount of change in the depth of cut for the Z axis. K is always an

incremental value. Figure 22.9 shows the relationship between the sign of the K

value and the way that the cycle is performed. The control adds the value of K

to the Z depth to determine the start point of the cutting pass.

22-11

Chapter 22

Single-Pass Turning Cycles

After the G24 block is executed the control re-executes the cycle for any

following block that commands axis motion (until the cycle is cancelled).

The value of the axis word in that block is used to replace the parameter

determined with that axis word in the original G24 block and the cycle is

re-executed using these new parameters.

Figure 22.9 applies only if programming X and Z as incremental values. If

programming X and Z as absolute values, the depth of taper K is added or

subtracted (depending on its sign) to the absolute Z axis position.

Figure 22.9

Effect of Positive and Negative Parameter Values in a G24 Block

(incremental X and X only)

When X and Z are

When X, Z and K

are negative

negative and K is positive

G24 X-__ Z-__ K+__ ;

G24 X-__ Z-__ K-__ ;

K

Cutting feed

X

X

Rapid feed

Note: ˙K˙£˙X˙

K

Z

Z

When X and K are positive

When X is positive and

and Z is negative

Z and K are negative

G24 X+__ Z-__ K+__ ;

G24 X+__ Z-__ K-__ ;

K

Z

Z

X

X

K

22-12

Chapter 22

Single-Pass Turning Cycles

After this G24 block is executed, the control re-executes the cycle for any

following block that contains an axis word (until the cycle is cancelled).

The value of this axis word is used to replace the parameter determined

with that axis word in the original G24 block and the cycle is re-executed

using these new parameters.

Example 22.4

Tapered Face Cutting

G90G00X43.Z55.;

G24X10.Z50.K-10.F10.;

Z45.;

Z40.;

G00;

Figure 22.10

Results of Example 22.4

X

40

10

35

30

Cutting feed

Rapid feed

10

Z

END OF CHAPTER

22-13

Chapter 23

Grooving/Cutoff Cycles

Figure 23.1

Tool Path during a G76 Face Grooving Cycle

Tool path, cutting feedrate

Tool path, rapid feedrate

No motion, for drawing clarification

X

Z

D

K+e

K

e

e

e

e

K+e

K+e

I

Z

D

X

K+e

K

e

e

e

e

K+e

K+e

Z

D

K+e

K

e

e

e

e

K+e

K+e

Z

23-2

Chapter 23

Grooving/Cutoff Cycles

Figure 23.2

Tool Path during a G77 O.D. Grooving Cycle

Tool path, cutting feedrate

Tool path, rapid feedrate

No motion, for drawing clarification

X

Z

K

I

I

I

e

e

e

I+e

I+e

I+e

X

X

X

e

e

e

I+e

I+e

I+e

e

e

e

I+e

I+e

I+e

e

e

e

D

D

D

Z

These cycles may also be used as cut off cycles. The tool infeeds into a piece

of stock, as in grooving, except that it cuts all the way through the part. Then,

instead of retracting the cutting tool straight out of the part, the tool is shifted

a predetermined direction and amount before retracting. This shifting helps

attain a good finish on the end of the part that has been cut.

23.1

The G76 Face Grooving grooving cycle is typically used to cut multiple

Face Grooving Cycle (G76)

grooves in a workpiece or as a cut off cycle. When the cycle is executed

the groove or cutoff is made by infeeding the tool into the workpiece in

steps to allow the removal of chips. The initial groove width (or width of

material removed during the infeed) is determined by the tool dimensions.

The first groove is cut from the X coordinate position of the tool prior to

the execution of the G76 block.

23-3

Chapter 23

Grooving/Cutoff Cycles

The format for this cycle is:

G76X__Z__I__K__F__D__;

Where :

Is :

X__

the location where the last groove is cut. If only one groove is to be cut do not

program X. This may be programmed as either an incremental or absolute value.

Remember that its value is also affected by diameter or radius modes (G07 and

G08).

Z__

the total depth of the groove from the Z coordinate position of the tool prior to the

execution of the G76 block. If this cycle is to be used as a cut off cycle the depth

programmed here should drive the tool through the face of the part. This value

represents the location of the bottom of the groove cut. This may be

programmed as either an incremental or absolute value.

I__

the distance between each groove. If the distance between the location of the

last groove (programmed with X) and the next to the last groove is less than the

value programmed with I, then the I value is not used to determine the position of

the last groove. The last groove is always cut at the location programmed with

X. The I parameter is always programmed as an incremental, radius value

regardless of the current mode of the control.

K__

the amount that the cutting tool infeeds into the workpiece with each step. The

step is followed by a retract of amount e (set in AMP by the system installer).

The cutting tool then infeeds into the workpiece an amount K + e, retracts an

amount e, infeeds K + e, retracts e, etc. This repeats until the total

programmed depth of the groove Z is reached. When this depth is reached the

cutting tool stops infeeding and either shifts an amount D (if programmed) or

retracts to the starting coordinate at rapid feedrate. The K-word is always

programmed as an incremental value regardless of the current mode of the

control.

F__

the desired feedrate for the grooving infeed moves. The value entered with this

parameter replaces the currently active feedrate. It is optional in the grooving

block. If F is not programmed the currently active feedrate is used.

D__

the size of the incremental shift move made by the tool when the full depth of a

cut off has been reached. This parameter must be programmed even if its value

is zero when not using this cycle as a cutoff. A value other than zero is assigned

to D only if the grooving cycle is being used as a cut off cycle. It is always an

incremental value regardless of the current mode. The sign of the value

programmed with the D parameter determines the shift direction and should

move the tool away from the part. Programming this shift move helps to provide

a good finish since the cutting tool is not touching the part when it is retracted at

the rapid feedrate.

CAUTION: The shift programmed with a D parameter is

executed as a rapid move. Make sure that the cutting tool is

clear to shift at the end of the grooving cycle.

23-4

Chapter 23

Grooving/Cutoff Cycles

Figure 23.3

G76 Face Grooving Cycle Parameters

X

K

e

X inc.

I

X abs.

Z abs.

Z inc.

Z

The retraction amount e is set in AMP by the system installer.

Example 23.1

G76 Grooving Cycle

Absolute Programming

Incremental Programming

G00X7.6Z5.3;

G00X-1.8Z-1.2

G76X2.0Z3.6I-2.8K-0.8D0;

G76X-5.6Z1.7I-2.8K-0.8D0;

23-5

Chapter 23

Grooving/Cutoff Cycles

Figure 23.4

Results of G76 Grooving Cycle Example

X

9.4

7.6

K=-0.8

e

4.8

I=-2.8

2.0

Z

3.6

5.3

6.5

23.2

The G77 O.D. & I.D. grooving cycle is typically used to cut multiple

grooves in a workpiece or as a cut off cycle. When the cycle is performed

O.D. & I.D. Grooving Cycle

the groove or cutoff is cut by infeeding the tool into the workpiece in steps

(G77)

to allow the removal of chips. The initial groove width (or width of

material removed during the infeed) is determined by the tool dimensions.

The first groove is cut from the Z coordinate position of the tool prior to

the execution of the G77 block.

23-6

Chapter 23

Grooving/Cutoff Cycles

The format for this cycle is:

G77X__Z__I__K__F__D__;

Where :

Is :

Z__

the location where the last groove is cut. If only one groove is to be cut do not

program Z. This may be programmed as either an incremental or absolute value.

X__

the total depth of the groove from the X coordinate position of the tool prior to the

execution of the G77 block. If this cycle is to be used as a cut off cycle the depth

programmed here should drive the tool through the center or inside diameter of the

part. If a cut off is being made from the inside of the part, it should drive the tool

beyond the outside diameter of the part. This value represents the location of the

bottom of the groove cut. It may be programmed as either an incremental or

absolute value and is also affected by radius or diameter mode (G07 or G08).

K__

the distance between each groove. If the distance between the location of the last

groove (programmed with Z) and the next to the last groove is less than the value

programmed with K, then the K value is not used to determine the position of the

last groove. The last groove is always cut at the location programmed with Z. The

K parameter is always programmed as an incremental value regardless of the

current mode of the control.

I__

the amount that the cutting tool infeeds into the workpiece with each step. The step

is followed by a retract of amount e (set in AMP by the system installer). The

cutting tool then infeeds into the workpiece an amount I + e, retracts an amount e,

infeeds I + e, retracts e, etc. This repeats until the total programmed depth of the

groove X is reached. When this depth is reached the cutting tool stops infeeding

and either shifts an amount D (if programmed) or retracts to the starting coordinate

at rapid feedrate. The I-word is always programmed as an incremental value

regardless of the current mode of the control.

F

optional in the grooving block. If programmed the value entered with this parameter

replaces the currently active feedrate used when infeeding into the part. If F is not

programmed the currently active feedrate is used.

D__

the size of the incremental shift move made by the tool when the full depth of a cut

off has been reached. This parameter must be programmed even if its value is zero

when not using this cycle as a cutoff. A value other than zero is assigned to D only if

the grooving cycle is being used as a cut off cycle. It is always an incremental value

regardless of the current mode. The sign of the value programmed with the D

parameter determines the shift direction and should move the tool away from the

part. Programming this shift during a cutoff move helps to provide a good finish

since the cutting tool is not touching the part when it is retracted at the rapid

feedrate.

CAUTION: The shift programmed with a D parameter is

executed as a rapid move. Make sure that the cutting tool is

clear to shift at the end of the grooving cycle.

23-7

Chapter 23

Grooving/Cutoff Cycles

Figure 23.5

G77 O.D. & I.D. Grooving Cycle Parameters

X

I

e

K

X inc.

Z abs.

Z inc.

X abs.

Z

Example 23.2

G77 O.D. & I.D. Grooving Cycle Used As a Cutoff Cycle

Absolute Programming

Incremental Programming

G00G90X42.Z56.;

G00G91X-36.Z-9.;

G77X19.Z21.I-8.K-14.D2.;

G77X-23.Z-35.I-8.K-14.D2.;

23-8

Chapter 23

Grooving/Cutoff Cycles

Figure 23.6

Results of G77 Used as a Cutoff Cycle Example

X

78

K distance ignored for

last groove (too close

to previous groove)

e

42

I=-8

34

19

K=-14

D=2

Z

14

21

28

42

56

65

END OF CHAPTER

23-9

Chapter

24

Compound Turning Routines

24.0

Compound turning routines are routines that make multiple passes across

the workpiece to cut a specific contour into the workpiece. A set of

Chapter Overview

blocks, called contour blocks, define the final contour shape of the

workpiece. A calling block, containing one of the following G-codes, sets

the parameters for the execution of the routine and defines what blocks are

used as the contour blocks.

Topic:

On page:

G73 O.D. and I.D. Roughing Routine (along Z-axis)

24-2

G74 Rough Facing Routine (along X-axis)

24-15

G75 Casting/Forging Roughing routine (parallel to work shape)

24-29

G72 O.D. and I.D. Finishing Routine

24-35

Important: Descriptions in this chapter are written assuming the control is

in the G18 plane and that plane has been defined as the ZX plane. If your

system has a different plane active, operation of these features is different.

Parameters are defined here assuming Z is the first axis in the plane, and X

is the second axis in the plane. If, for example, the XZ plane is the

currently active plane, descriptions in this document should be interpreted

accordingly (i.e., Z axis description applies for X axis and X axis

description applies to Z axis. Refer to your system installer’s

documentation for details on the plane definitions on your system.

If you are using a dual--processing system, refer to page 30-14 for details

about spindle control.

Important: Any rapid motions that are generated by the execution of a

compound turning routine are always performed using exponential

ACC/DEC. Refer to chapter 18. Compound turning routines ignore the

AMP parameter that determine the ACC/DEC type normally used for

rapid moves. If AMP parameters have not been configured to properly

allow rapid motions using exponential ACC/DEC, a SERVO AMPLIFIER

FAULT error may be generated during the execution of these routines.

24-1

Chapter 24

Compounding Turning Routines

24.1

The G73 contour turning routine is used to rough out the contour of a

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

O.D. and I.D. Roughing

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

Routine (G73)

workpiece. A finish allowance may 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.

Figure 24.1

Stock Removal in G73 Roughing Routine

X

Tool paths determined automatically

Start Point

Shape after roughing

and final pass

Workpiece finished

Finishing allowance

shape

Z

The G73 block has a P and a Q parameter that call out 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 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 can handle two different cases of the G73 routine. It

automatically recognizes them and adapts the tool path accordingly.

24-2

Chapter 24

Compounding Turning Routines

Figure 24.2

Workpiece Finish Contour Case 1 and Case 2 (G73)

Case 1

Case 2

X

X

Start Point

Start Point

Z

Z

The G73 block is programmed with this format:

G73P__Q__U__W__I__K__D__R__F__S__T__;

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.

U W

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 24.3 to determine the

sign of U and W. U and W are always programmed as incremental values.

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

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

24-4

Chapter 24

Compound Turning Routines

Where :

Is :

I K

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 and K are always incremental, radius

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

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 D is

programmed larger than the AMP threshold for D, the control overrides the

programmed depth and use the AMP assigned maximum depth.

R__

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

amount is an incremental, radius value measured parallel to the X axis. Case 1

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

parallel to the X axis. This does not affect the programmed value of R, as R is

always measured parallel to X. If no value for R is programmed then the control

uses the value for the retract amount set in AMP by the system installer.

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 programmed in the G73 block these words

replace any previously active modal F-, S- or T-words for the remainder of the G73

routine operation only. When the G73 routine is completed the previously active

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

24-5

Chapter 24

Compounding Turning Routines

Figure 24.3

Parameters for G73 Roughing Routine

X

Start Point

(I+K)/2

D

Shape after roughing

Shape after roughing

R

and final pass

(U+W)/2

Workpiece finished

shape

Z

In Figure 24.3, 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 (point A to B in Figure 24.3).

The contour blocks can be programmed with or without a feedrate, or with

a G00 (rapid) command The control uses the feedrate specified by the

F-word in the G73 block during all roughing portions of the routine.

During the final contour pass of the roughing cycle, the control executes

your feedrate programmed in your contour block (unless you do not use

one, then it uses the F-word in the G73 block). This final contour can even

contain rapid moves (G00).

Important: The blocks preceding the G73 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

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

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

24-6

Content      ..     17      18      19      20     ..