9/Series CNC Lathe. Operation and Programming Manual

Chapter

Thread Cutting

25.0

The 9/Series control provides two methods of thread cutting:

Chapter Overview

Single-pass thread cutting

G33 and G34 blocks generate a single thread cutting pass. G33 can cut

straight, tapered, face, multistart, and multiblock threads. G34 can cut

thread passes of increasing or decreasing leads.

Automatic thread-cutting cycles

G21 and G78 provide for fully automatic thread cutting with multiple

passes at a programmed depth, including springing pass and clean-up

pass options.

This chapter describes the following topics that relate to thread cutting:

Topic:

On page:

Considerations for thread cutting

25-2

Chamfering your threads

25-4

Single pass threading mode

25-6

Single pass variable lead thread cutting

25-12

Single pass threading cycle

25-16

O.D. & I.D. multipass threading routine

25-20

If you are using a dual-processing system, you may need to use slightly

different threading methods. Refer to page 30-15 for details.

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.

25-1

Chapter 25

Thread Cutting

25.1

When performing threading operations, remember:

Considerations for Thread

Emergency Stop - Pressing the emergency stop during threading causes

Cutting

all axes to come to a rapid stop. This likely causes damage to the part or

tool and resuming the threading moves is not possible.

<CYCLE STOP> (cycle suspend) - A cycle stop does not occur if this

button is pressed during a threading pass; instead the block executes in

this manner:

If G33, or G34 threading is being executed then axis motion continues

and cycle stop is ignored.

If G78 or G21 threading is being executed, one of two possible paths is

taken by the control. If the threading retract feature has been enabled,

the control immediately chamfers out of the thread, retracts the tool and

then returns to the start point of the threading cycle. If no threading

retract is enabled then the control continues execution until it has

completed the entire pass of the threading cycle and returned to the start

point of the move.

Overrides - During the execution of any threading pass, all feedrate

overrides are fixed at 100%.

Single Block - In single block mode the entire cycle is executed for

G21. For G78 one complete sub-cycle (including the return move to the

initial point) is performed each time cycle start is pressed. When

performing single pass threading (G33 or G34) motion stops at the end

of the threading block typically resulting in a ringing of the thread.

Dry Run - Whether or not the “dry run” and spindle speed override

functions are operable during threading is determined by the system

installer’s PAL program.

Radius/Diameter Mode - The control performs threading in either

radius or diameter modes. Radius/Diameter mode only affects the

controls interpretation of the X parameter.

Start point - Due to axis acceleration and other machine dynamics, the

threading cycles should be programmed such that the axes have room to

attain speed prior to contacting the workpiece. Failure to do so may

result in the initial thread lead being incorrect.

Controlling spindle - On systems with multiple spindles, the

controlling spindle (selected with G12) is the synchronized spindle used

for thread cutting. The controlling spindle RPM, in conjunction with

the programmed thread lead (F or E), determine the threading axis

feedrate.

25-2

Chapter 25

Thread Cutting

Axis feedrates - When threading, the speed of the cutting axis is

determined by the controlling spindle speed and the thread lead through

this equation:

axis feedrate

= (S) / (F inches per revolution)

= (S) / (E threads per inch)

= (S)(E inches per thread)

Where :

Is :

the actual speed of the controlling spindle (programmed spindle speed times

the spindle speed override switch setting in percent)

threads per revolution or degree depending on the current active mode

threads per inch or inches per revolution as determined in AMP by your

system installer.

The programmer should use this equation to verify that the feedrate

resulting from the thread parameters does not exceed the maximum

allowable feedrate for the cutting axis. Otherwise an error results and

axis motion stops. This equation can also be applied to face threads and

tapered threads.

Pullout angles - During threading cycles, the control synchronizes the

moves of the X and Z axes with the spindle speed. This occasionally

may force the X axis to move quite rapidly in order to produce the

desired thread taper or pullout angles at the rates dictated by the active

spindle speed. Compounded with the fact that many machines have X

axis feedrate limits lower than those for the Z axis, the result may be

velocity limitations. This is best prevented by first executing a Feed

Check prior to actually cutting the threads and then reducing spindle

speed or changing the pullout angle where necessary.

Tapered Thread Lead - When cutting a tapered thread, the thread lead

(E- or F-word) is applied to the axis that travels the greatest distance

from the start to the end of the threading pass.

Infeed - Plunge infeed relies on a sharp tool made at the exact thread

angle that cuts on both sides of the tip as it is fed perpendicular to the

work on successive passes. On larger threads, this type of infeed may

cause vibration. In that case, angular infeed may be preferred. This

results in the tool being fed along the thread flank with each successive

pass, meaning only one side of the tip cuts. Figure 25.1 illustrates

plunge and angular infeed.

25-3

Chapter 25

Thread Cutting

Figure 25.1

Angular versus Plunge Infeed

Angular Infeed

Plunge Infeed

Cutting tool

The G78 threading pass allows the selection of different infeed types by

programming a P-word. If you use any of the other threading methods,

it is necessary to insert a small Z move to generate an angular feed.

Form Cut Threading - The auto threading cycles (G21 and G78)

assume a sharp triangular tool. If you use a shaped-tip tool, the tool

loading is affected. Specifically, the first cut is loaded slightly less than

successive cuts. Though generally insignificant, if this is a concern, we

suggest that the initial cut depth be compromised as necessary to ensure

that the tool is not overloaded on successive passes.

25.2

Using Thread Chamfer

Chamfering Your Threads

The thread chamfer feature, enabled in PAL, cuts a chamfer at the end of a

thread cutting pass. When the feature is activated, the control

automatically cuts a chamfer at the end of each thread cutting pass to

assure the tool is fully out of the thread before it is retracted.

This feature prevents the “ring” at the end of the thread that typically

occurs when the control stops threading motion to retract the tool. This

ring occurs when the threading axis reaches the endpoint of the thread and

decelerates before executing the retract move. Typically spindle RPM

does not compensate for this deceleration of the threading axis thus

causing a ring at the end of the thread.

Both the thread retract and thread chamfer use the same values (set in

AMP) for the pullout distance “r” and pullout angle “a” of the chamfer.

“r” is entered as the number of threads to be chamfered, “a” is entered as

the angle of the chamfer in degrees measured from the same axis as the

thread lead.

25-4

Chapter 25

Thread Cutting

Important: This feature may only be used with the G78 or G21 threading

cycle. It is ignored if a G33 or G34 threading pass is being made.

Using Thread Retract

Enabled in PAL, thread retract lets you interrupt a thread cutting operation

without damaging the thread by pressing <CYCLE STOP>. When the

operation is interrupted, the control automatically performs a retract (by

cutting a chamfer) out of the thread to prevent damage to the thread due to

ringing. Once free of the thread the control retracts the tool and returns it

to the start point. Also, program execution stops at this point.

If you attempt to interrupt the thread cutting operation without thread

retract active, the control does not interrupt the operation until the end of

the currently executing threading pass.

Thread Chamfer and Thread Retract Parameters

Both the thread retract and thread chamfer use the same values (set in

AMP) for the pullout distance “r” and pullout angle “a” of the chamfer.

“r” is entered as the number of threads to be chamfered, “a” is entered as

the angle of the chamfer in degrees measured from the same axis as the

thread lead.

Figure 25.2

Ringing occurs when retracting from thread without using thread

chamfer or thread retract.

Number of

threads

Ringing from no chamfer when cutting

for chamfer (r)

tool is retracted out of thread.

Pullout

angle (a)

Smooth exit from thread when cham-

fer is made, no ringing at end of

thread. Root depth slowly decreases.

25-5

Chapter 25

Thread Cutting

25.3

The G33 thread cutting mode can cut straight, tapered, face, and multistart

threads that have constant thread leads (use G34 to cut threads that do not

Single Pass Threading Mode

have a constant lead). The G33 thread cutting mode is a mode, not a cycle

(G33)

and does not generate any extra motion blocks. This mode synchronizes

the thread cutting tool motion with the spindle to allow programming

multiple passes over the same threads.

Figure 25.3

Constant Lead Threads

Parallel thread

Face thread

Tapered thread

The format for the G33 thread cutting operation is:

Parallel thread G33Z__ F__ Q__;

Tapered thread

G33X__Z__ F__ Q__;

Face thread

G33X__ F__ Q__;

25-6

Chapter 25

Thread Cutting

Where :

Is :

This parameter is the end point of the thread cutting move in the X axis. This parameter may be an incremental or absolute and radius or

diameter value. If not present there must be a Z parameter. If an X parameter is present, it indicates either a face, tapered, or lead-in

thread. When used in a G33 block without a Z parameter, a facing thread is made parallel to the X-axis at the Z axis position prior to the

G33 block. X values maybe entered as a radius or a diameter value. X may also be programmed as an incremental or absolute value.

The initial minor diameter of any straight or tapered thread is determined by the position of the X axis prior to the G33 block.

This parameter is the end point of the thread cutting move in the Z axis. This parameter may be an incremental or absolute value. If not

present there must be an X parameter. When a Z parameter is used in a G33 block without an X parameter the threading pass is made

parallel to the Z-axis at whatever X position the tool tip was at prior to the G33 block.

E F

This parameter may be entered by using either an E- or F-word. It represents the thread lead along the axis with the largest programmed

distance to travel to make the thread cut. It is mandatory when cutting any threads.

If the E-word is programmed, its value (sign ignored) is equal to the number of threads per inch or inches per thread (determined in AMP)

regardless of whether inch or metric mode is active at the time.

If the F-word is programmed, its value (sign ignored) is the thread lead in inches per revolution or millimeters per revolution, depending on

the mode in which the control is operating.

This optional parameter provides a relative value for the start offset angle of the thread. Its primary use is in cutting multistart threads.

For example, if a threading pass were made with a value of zero here, and then followed by another pass with a value of 180 then the

second cut would be started 180 degrees from the first resulting in a two start thread. If two more passes are then made, one with a

parameter value of 90 and one with a value of 270, the result would be a four-start thread.

Figure 25.4

G33 Block Parameters

X Inc.

X Abs.

1/E, E or F

Abs.

Inc.

Important: Do not re-program the G33 command in consecutive threading

blocks. Doing so will cause the control to pause axis motion (possibly

damaging the thread) while the axis re--synchronizes with the spindle.

Consecutive threading blocks in the following example are blocks N3 and

N4, and blocks N8 and N9.

25-7

Chapter 25

Thread Cutting

Example 25.2

Tapered Thread Cutting

Thread lead: .125 threads/mm (8 mm pitch)

Depth of cut: 1 mm (X direction)

Number of cutting passes: 2

N1 M03 S30;

N2 G77 G00 X20. Z4.;

N3 G33 X48. Z-47. F8;

N4 X52 Z-55;

N5 G00 X60.;

N6 Z4.;

N7 X12.;

(second pass)

N8 G33 X40. Z-47.;

N9 X52 Z-55;

N10 G00 X60.;

N11 Z4.;

Figure 25.7

Results of Tapered Thread Cutting Example 25.2

N11

-70

-55

-47

8mm

Multiple-thread cutting can be programmed by assigning a thread cutting

start shift angle using a Q-word. Omission of a Q-word indicates a shift

angle of 0 (synchronizes at the spindle marker). Entering a Q word will

offset the axis synchronization from the spindle marker position.

25-10

Chapter 25

Thread Cutting

25.4

The G34 code programs the variable lead thread cutting mode. It is

programmed almost identically to the G33 thread cutting mode with the

Single Pass Variable Lead

addition of a K-word used to program the amount of lead variation per

Thread Cutting (G34)

revolution.

Figure 25.9

Variable Lead Thread

Important: Do not re-program the G34 command in consecutive threading

blocks. Doing so will cause the control to pause axis motion (possibly

damaging the thread) while the axis re--synchronizes with the spindle.

The format for the G34 threading mode is:

Parallel thread G34Z__ F__ Q__K__;

Tapered thread

G34X__Z__ F__ Q__K__;

Face thread

G34X__ F__ Q__K__;

Where :

Is :

This parameter is the end-point of the thread cutting move in the X axis. This

parameter may be an incremental or absolute and radius or diameter value. If

not present, there must be a Z parameter. If an X parameter is present, it

indicates either a face, tapered, or lead-in thread. When used in a G34 block

without a Z parameter, a facing thread is made parallel to the X-axis at the Z axis

position prior to the G34 block.

The initial minor diameter of any straight or tapered thread is determined by the

position of the X axis prior to the G34 block.

This parameter is the end-point of the thread cutting move in the Z axis. This

parameter may be an incremental or absolute value. If not present, there must

be an X parameter. When a Z parameter is used in a G34 block without an X

parameter, the threading pass is made parallel to the Z-axis at whatever X

position the tool tip was at prior to the G34 block.

25-12

Chapter 25

Thread Cutting

Where :

Is :

E F

This parameter may be entered by using either an E- or F-word. It represents the

thread lead along the axis with the largest programmed distance to travel to

make the thread cut. It is mandatory when cutting any threads.

If the E-word is programmed, its value (sign ignored) is equal to the number of

threads per inch or inches per thread (determined in AMP) regardless of whether

inch or metric mode is active at the time.

If the F-word is programmed, its value (sign ignored) is the thread lead in inches

per revolution or millimeters per revolution, depending on the mode in which the

control is operating.

In a G34 block, E or F indicates the initial thread lead used at the start of the

threading pass.

This optional parameter provides a relative value for the start offset angle of the

thread. Its primary use is in cutting multistart threads. For example, if a

threading pass were made with a value of zero here, and then followed by

another pass with a value of 180°,then the second cut would be started 180°

from the first resulting in a two-start thread. If two more passes are then made

(one with an a parameter value of 90°and one with a value of 270°), the result

would be a four-start thread.

Program the difference in the thread lead per spindle revolution (inch/rev/rev or

mm/rev/rev). The amount of K is added to the thread lead (E or F) after each

thread is cut. K may be programmed as a positive (increasing thread lead) or a

negative (decreasing thread lead) value.

The lead changes continuously during the move. At any point during the

move, you can calculate the lead with this formula:

instantaneous lead = F + (K * number of revs since the start)

Figure 25.10

Instantaneous Lead

Lead

K * Revs

Distance

Revolutions

The actions of the G34 variable lead threading operation are identical to

the G33 threading operation with the exception of the variable thread lead.

See the G33 threading section for details and examples of single-pass

threading blocks that cut parallel, tapered, or face threads.

25-13

Chapter 25

Thread Cutting

25.5

The G21 single pass threading cycle can be programmed to cut parallel or

tapered fixed lead threads (variable lead threads may only be cut using a

Single Pass Threading Cycle

G34 block). This threading cycle performs a predetermined series of

(G21)

machining steps designated by a single program block.

The two chamfering features (threading retract and threading chamfer)

described on page 25-4 can also be used with this threading cycle. The

parameter to enable these and determine their angle and length is set in

AMP. The thread chamfer feature must also be enabled through PAL.

This threading cycle repeats automatically after every block that contains

axis words until the cycle is cancelled. These axis words generate rapid

moves. A G21 single pass threading cycle is canceled by programming

any other G-code in modal group 1 (this includes G00, G01, etc.).

The conditions to be satisfied to execute this thread cutting cycle are

described on page 25-2, thread cutting considerations.

Before programming the G21 threading cycle, the cutting tool must be

positioned away from the part at a location that allows the control to

execute the cycle correctly.

Straight Thread Cutting

This format is for programming a single pass straight threading cycle:

G21 X__ Z__ {F__};E

Where :

Is :

This parameter is the start-point of the thread cutting move in the X axis. This

parameter may be an incremental or absolute and radius or diameter value. This

is the depth that the X axis moves to before starting the thread cutting pass. This

value may be replaced in any block following the G21 block while the G21 cycle

is active. X may also be programmed as an incremental or absolute value.

This parameter is the end-point of the thread cutting pass in the Z axis. This

parameter may be an incremental or absolute value. Z parameters are always

entered as a radius values regardless of the current mode.

E F

This parameter may be entered by using either an E- or F-word. It represents the

thread lead along the axis with the largest programmed distance to travel to

make the thread cut. It is mandatory when cutting any threads.

If the E-word is programmed, its value (sign ignored) is equal to the number of

threads per inch or inches per thread (determined in AMP) regardless of whether

inch or metric mode is active at the time.

If the F-word is programmed, its value (sign ignored) is the thread lead in inches

per revolution or millimeters per revolution, depending on the mode in which the

control is operating.

25-16

Chapter 25

Thread Cutting

When this cycle is executed:

The cutting tool rapids to the depth programmed with the X-word.

The thread cutting pass is made to the position programmed with the

Z-word using a feedrate that generates the required lead programmed

with the E- or F-word. If the Thread Chamfering feature was enabled

before the cycle began executing, the control performs a chamfer just

before reaching the programmed Z position.

The cutting tool is retracted away from the part at a rapid feedrate to

where the X axis was positioned prior to the G21 block.

The cutting tool is returned along the Z axis at a rapid feedrate to

where the Z axis was positioned prior to the G21 block.

Program execution continues on to the next block.

G21 works like most fixed cycles in that it automatically repeats after

every rapid move until canceled. Following passes need only contain a

new value for the infeed (X value). The other parameters programmed in

the G21 block remain in effect.

Example 25.5

G21 Straight Thread Cutting Cycle

G00X10.Z10.;

Rapid to the start point of the thread cutting cycle. This should be

a point that allows a straight, rapid, X move to the depth that the

thread is cut to.

S500.M03;

Starts the spindle turning at 500 RPM in the clockwise direction.

G21X4.8Z5.F.5;

This block makes a thread cutting pass with a lead of .5 and

return the cutting tool to the start point of the thread cutting cycle

(X10 Z10).

X4.5;

This block repeats the G21 thread cutting block using a new

depth of cut to 4.5.

X4.3;

This block repeats the G21 thread cutting block using a new

depth of cut to 4.3.

G00;

This block cancels the G21 thread cutting mode.

25-17

Chapter 25

Thread Cutting

Figure 25.12

Results of G21 Straight Thread Cutting Example

10.0

0.5 lead

4.8

4.3

5.0

10.0

Taper Thread Cutting

This format is for programming a single pass tapered threading cycle:

G21X__Z__I__ F__ ;

Where :

Is :

This parameter is the end point of the thread cutting move in the X axis. This parameter may be an incremental or absolute and radius

or diameter value. This is the depth that the X axis moves to before starting the thread cutting pass. This value may be replaced in any

block following the G21 block while the G21 mode is active.

This parameter is the end point of the thread cutting pass in the Z axis. This parameter may be an incremental or absolute value.

Z parameters are always entered as radius values.

E F

This parameter may be entered by using either an E- or F-word. It represents the thread lead along the axis with the largest

programmed distance to travel to make the thread cut. It is mandatory when cutting any threads.

If the E-word is programmed, its value (sign ignored) is equal to the number of threads per inch or inches per thread (determined in

AMP) regardless of whether inch or metric mode is active at the time.

If the F-word is programmed, its value (sign ignored) is the thread lead in inches per revolution or millimeters per revolution, depending

on the mode in which the control is operating.

This is the change in radius of the thread (on the X axis) that the threading pass makes as it reaches the end point of the thread cutting

pass. The end point is the X position programmed with the X-word. I is an incremental, signed distance (+ or -) added to the X

parameter to determine the start point of the threading pass on the X axis. If a chamfer is being cut at the end of the thread cutting

pass, it does not affect the value programmed here. This parameter should be entered as if no chamfer was being cut. I parameters are

always entered as radius values regardless of the current mode. I is always an incremental value regardless of the current mode.

25-18

Chapter 25

Thread Cutting

Figure 25.13

G21 Taper Thread Cutting Parameters

X Inc.

X Abs.

Abs.

Inc

When this cycle is executed:

The cutting tool rapids to the depth programmed with the X-word

added to the I value.

The thread cutting pass is made to the position programmed with the

X- and Z-words using a feedrate that generates the required lead

programmed with the F- or E-word. As the tool moves along this

threading pass, the taper distance programmed with the I parameter is

interpolated along the X axis.

Important: If the Thread Chamfering feature was enabled before the cycle

began execution, the control performs a chamfer before reaching the

programmed Z position. The chamfer angle and length of are set in AMP.

The cutting tool is retracted away from the part at a rapid feedrate to

the X axis position prior to the G21 block.

25-19

Chapter 25

Thread Cutting

The cutting tool is returned along the Z axis at a rapid feedrate to the

Z axis position prior to the G21 block.

Program execution continues on to the next block.

G21 is modal. Following passes need to contain only a new value for the

infeed (X value). The other parameters programmed in the G21 block

remains in effect.

25.6

The G78 multipass threading routine can be programmed to cut parallel,

face, or tapered fixed lead threads (variable lead threads may only be cut

O.D. & I.D. Multipass

using a G34 block). This routine performs a predetermined series of

Threading Routine (G78)

threading steps designated by a single program block. The G78 block

contains all of the necessary information to cut the complete thread. When

executed, the routine makes multiple passes over the thread until the

programmed root depth is reached. The control automatically generates all

threading passes necessary to reach the programmed root depth.

In effect, with the exception of the different infeed types, the multipass

threading routine is executed as if many G21 single pass threading cycles

were being executed. The key difference between the two features (aside

from infeed types) is that the multiple pass cycle only requires one block to

do the job of many single pass threading blocks. The G78 multipass

threading routine is a non-modal G-code (unlike G21). This routine is

executed only when a block contains a G78.

A finishing pass is also available with the multipass threading routine.

The size of the finishing pass, and whether a finishing pass is performed at

all, is determined by the system installer in AMP. If a finishing pass is

made, it is typically to improve final thread finish by removing a

significantly smaller amount of material with the last pass executing across

the thread by the G78 routine.

The two different chamfering features (threading retract and threading

chamfer) described in section 25.1 may also be used with this multipass

thread cutting routine. The parameters to enable these and to determine

their angle and length are set in AMP. The thread chamfer feature must

also be enabled through PAL.

The conditions to be satisfied to execute this thread cutting routine are

described in section 25.1, thread cutting considerations.

25-20

Chapter 25

Thread Cutting

Programming Multipass Thread Cutting

Before programming the G78 threading routine, the cutting tool must be

positioned to the point from which the routine is to be executed. This point

is the end-point of each complete cycle of the threading routine’s

execution.

Use this format to program a multipass thread cutting routine:

G78X__Z__K__D__ F__ A__P__I__;

Where :

Is :

This parameter is the coordinate value of the root (depth) of the thread. If

programming a tapered thread, it is the coordinate value to be attained at the end

of the last threading pass (assume there is no chamfer cut at the end of the

pass). X values may be entered as a radius or a diameter value. X may also be

programmed as an incremental or absolute value.

This parameter is the Z coordinate value of the end of the thread cutting pass. Z

parameters are always entered as a radius value regardless of the current mode.

Z may also be programmed as an incremental or absolute value.

This parameter is an unsigned value (always programmed as positive). It

programs the distance from the thread root (as determined by the X parameter to

the top of the thread. K is always programmed as a radius value.

This parameter programs the depth of cut (designated in radius) for the first pass.

It is an unsigned value (always programmed as positive). The depth of following

passes is determined by this value and the type of infeed selected with the P

parameter.

This parameter programs the angle of the tool tip. It must be entered as an

integer value from 0 to 120 (corresponding to 0-120 degrees). Not programming

a value for A is the same as A0. A0 would be the same as a plunge type infeed.

The value entered here determines the angle that the infeed moves makes,

which also determines the final thread angle. See the tool infeed section that

follows for details.

This parameter determines the tool infeed. It must be entered as an integer

value from one to four. See the tool infeed section that follows for details.

E,F:

This parameter may be entered by using either E or F for the thread lead

(as in G33).

If the E-word is programmed, its value (always unsigned) is equal to the number

of threads per inch or inches per thread (determined in AMP) regardless of

whether inch or metric mode is active at the time.

If the F-word is programmed, its value (always unsigned) is the thread lead in

inches per revolution or millimeters per revolution, depending on the mode in

which the control is operating.

This is the change in radius of the thread (on the X axis) that the threading pass

makes as it reaches the end-point of the thread cutting pass. The end-point is

the X position programmed with the X-word. I is an incremental, signed distance

(+ or -) added to the X parameter to determine the start-point of the threading

pass on the X axis. If a chamfer is being cut at the end of the thread cutting

pass, it does not affect the value programmed here. This parameter should be

entered as if no chamfer were being cut. I is always an incremental value

regardless of the current mode. This parameter is always entered as a radius

value regardless of the current mode.

25-21

Chapter 25

Thread Cutting

If a straight thread is desired:

enter a value of zero for this parameter

do not program the I-word in the block

The control performs threading in either radius or diameter mode. Be

aware that X values entered as a radius or a diameter value when entered.

Z, I, K, and D, parameters are always entered as radius values regardless of

the current mode. X and Z may also be programmed as incremental or

absolute values. K, D, and I are always programmed as incremental values

regardless of the current mode.

Figure 25.14 illustrates these parameters.

Figure 25.14

Multipass Thread Cutting Parameters

X inc.

Pullout angle

1/E or 1/F

X abs.

Finishing

allowance

Z abs.

Z inc.

25-22

Chapter 25

Thread Cutting

Tool Infeed

This multipass threading routine provides 4 different types of cutting tool

infeed determined by a P-word in the threading block. These different

infeeds are provided to allow operation with different types of cutting tools

and materials. These different infeed types all move the end-point of the

cutting tool when infeeding an amount referenced from the infeed

reference point.

P1 - Constant cutting volume, angular infeed along thread face. A

constant amount of material is removed in each pass (except possibly the

last few passes). The last few passes may reach the minimum infeed

amount set in AMP by the system installer. If the depth of cut is smaller

than the minimum depth of cut set in AMP, it is increased to equal that

minimum depth of cut. Only one edge of the cutting tool removes

material.

P2 - Constant cutting volume, zigzag infeed. With this parameter, the

control alternates the cutting edge of the tool after every pass. The amount

of material that is removed is constant every two passes.

Important: If the user programs one pass, the control halves the

programmed depth and makes two passes. Because of this, the number of

passes programmed must always be even; and the depth of the pass cannot

be too small. If it is too small, the cutting tool may only burnish the part,

instead of cutting it.

To prevent burnishing, the system installer can program in AMP a

minimum depth of cut. If the user then enters a depth of cut smaller than

the minimum depth of cut in AMP, the entered value is disregarded, and

the value in AMP replaces it.

P3 - Constant depth of cut, angular infeed along thread face. This method

is the same as P1, except that the cutting depth is kept constant with each

pass, and there is no minimum infeed applied. Only one edge of the

cutting tool removes material.

P4 - Constant depth of cut, zigzag infeed. This method is the same as P2

except that the cutting depth is kept constant for each pass, and there is no

minimum infeed applied. Each edge of the cutting tool removes material

on alternate passes.

25-23

Chapter 25

Thread Cutting

Figure 25.15

Multipass Thread Cutting Infeed Parameters

Infeed Reference

Single edge

Point

Double edge

cutting

Cutting

tool

D÷2÷2

D(÷2+÷4)

D(÷4+÷6)

D÷2

D÷3

D÷4

D÷6

Finishing

allowance

Infeed Reference

Single edge cutting

Point

Cutting

Double edge

Cutting

tool

cutting

tool

Infeed Reference

Point

D’

Finishing

allowance

D’is the remaining material to reach

D’is the remaining material

K -- finish allowance. Note 2 equal

to reach K -- finish allowance.

passes are made equal to half D’

25-24

Chapter

Drilling Cycles

26.0

This chapter covers the G-word data blocks in the drilling cycle group.

The operations of the drilling cycles are explained on these pages:

Chapter Overview

Topic:

Page:

Drilling cycles

26-1

Positioning and Hole Machining Axes

26-4

Parameters

26-7

Drilling Cycle Operations

26-8

Altering Drilling Cycle Operating Parameters

26-38

Fixed Drilling Cycle Examples

26-40

WARNING: The cycles described in this chapter can be used

with live tooling. This application however requires proper

PAL control of the spindle, especially in cycles that perform

spindle orients or change the spindle rotation direction. Failure

to do this can result in injury to personal or damage to

equipment.

26.1

Drilling cycles, sometimes referred to as canned cycles or auto cycles,

repeat a series of basic machining operations, such as boring, drilling, or

Drilling Cycles

tapping. These operations, designated by a single-block command, usually

consist of a fixed series of steps that are dependent on the type of

machining application.

For this chapter, as well as this manual, assume that the Z axis is the hole

machining axis. The hole machining axis is established by the system

installer.

If you are using a dual-processing system, refer to chapter 30 for more

details about drilling fixed cycles for your system.

The control provides the drilling cycles shown in Table 26.A.

26-1

Chapter 26

Drilling Cycles

Table 26.A

Drilling Cycles

G-code

Application

Tool Movement

Operation At Hole Bottom

Retraction Movement

G80

Cancel Or End Fixed Cycle

N/A

G81

Drilling Cycle,

Feed

Retract

Rapid Traverse

No Dwell/Rapid Out

G82

Drilling Cycle,

Feed

Dwell / Retract

Rapid Traverse

Dwell/Rapid Out

G83

Deep Hole Drilling Cycle

Intermittent Feed

Retract

Rapid Traverse

G83.1

Deep Hole Peck

Intermittent Feed

Retract

Rapid Traverse

Drilling Cycle with Dwell

G84

Right-Hand Tapping Cycle

Feed

Spindle or Live Tool Reversed / Retract

Feed

G84.1

Left-Hand Tapping Cycle

Feed

Spindle or Live Tool Reversed / Retract

Feed

G84.2

Right-Hand Solid-Tapping Cycle

Feed

Spindle or Live Tool Reversed / Retract

Feed

G84.3

Left-Hand Solid-Tapping Cycle

Feed

Spindle or Live Tool Reversed / Retract

Feed

G85

Boring Cycle,

Feed

Retract

Feed

No Dwell/Feed Out

G86

Boring Cycle,

Feed

Spindle or Live Tool Stop / Retract

Rapid Traverse

Tool Stop/Rapid Out

G86.1

Boring Cycle,

Feed

Orient Spindle or Live Tool Stop / Retract

Rapid Traverse

Tool Shift

G87

Back Boring Cycle

Feed

Oriented Spindle or Live Tool Stop / Retract

Rapid Traverse

G88

Boring Cycle

Feed

Dwell / Retract

Manual/Rapid Traverse

Spindle or Live Tool Stop / Retract

Spindle or Live Tool Stop/

Manually Out

G89

Boring Cycle,

Feed

Dwell/Retract

Feed

Dwell/Feed Out

26-2

Chapter 26

Drilling Cycles

26.2

This section assumes that the programmer can determine the hole

machining axis using the plane select G-codes (G17, G18, G19). Refer to

Positioning and Hole

the system installer’s documentation to make sure that a specific axis has

Machining Axes

not been selected in AMP to be the hole machining axis.

G-codes G17, G18, or G19 determine the plane, the hole machining axis,

and the positioning axes. The two axes that define the selected plane are

used as positioning axes. The axis perpendicular to the plane is the hole

machining axis.

Table 26.B assumes a specific plane definition. Refer to the system

installer’s documentation for the plane definitions on your system.

Table 26.B

Plane Selection vs Machining Axis

Plane

Hole Machining Axis

Positioning Axes

XU (G17)

Z axis or its parallel axis

X and U axes or their parallel axes

ZX (G18)

U axis or its parallel axis

Z and X axes or their parallel axes

UZ (G19)

X axis or its parallel axis

U and Z axes or their parallel axes

Example 27.1 shows you how to change the hole machining axis to a

parallel axis. Prior to changing the hole machining axis, a G80 should be

executed to cancel any active milling mode.

Example 27.1

Altering the Machining Axis to a Parallel Axis

Program Block

Comment

The W axis is parallel to the Z axis.

G17;

XU plane active

G81X ___ U ___ ;

Drilling cycle, Z is the hole

machining axis

G80;

Cancel drilling fixed cycle

mode

G81X ___ U ___ W ___;

Drilling cycle, W is the hole

machining axis

The plane selection codes (G17, G18, and G19) can be included in the

drilling fixed cycle block, or can be programmed in a previous block.

26-4

9/Series CNC Lathe. Operation and Programming Manual - page 21