dugard NL200Y Programming Manual

PROGRAMMING MANUAL -1-

DUGARD EAGLE NL200Y

TRAINING MANUAL

Manual Iss 1b

This document is based on information available at the time of its publication. While efforts
have been made to render accuracy to its content, the information contained herein does
not purport to cover all details or variations in hardware and software, nor to provide every
possible contingency in connection with installation, operation, programming, and
maintenance. Features maybe described herein which are not present in all hardware and
software systems.
Dugard Ltd assumes no obligation of notice to holders of this document with respect to
changes subsequently made.

Dugard Ltd makes no representation or warranty, expressed, implied or statutory with
respect to, and assumes no responsibility for the accuracy, completeness, sufficiency or
usefulness of the information in the manual.

PROGRAMMING MANUAL -2-

Machine axes.............................................................................................................................. 4

Other axes that could be encountered when programming the machine are ............................ 5

Tool offset ................................................................................................................................... 6

Entering tool offset values........................................................................................................... 6

Workpiece zero reference point..................................................................................................6

Facing..………………………………………………………………………………………………….7

Taper turning............................................................................................................................... 9

Inside turning: ........................................................................................................................... 10

Circular Interpolation................................................................................................................. 11

Incremental commands (U and W) ........................................................................................... 13

Example for operation............................................................................................................... 14

G code list ................................................................................................................................. 14

M code list................................................................................................................................. 14

Threading example using G32.................................................................................................. 14

G70 Finishing cycle................................................................................................................... 22

G71 Longitudinal roughing cycle parallel to Z-axis................................................................... 22

G72 Cross roughing cycle transversal parallel to X-axis.......................................................... 23

G73 Roughing cycle with passes parallel to profile.................................................................. 23

G74 Drilling cycle (chip break).................................................................................................. 24

G83 Drilling cycle ...................................................................................................................... 24

G84 Tapping cycle .................................................................................................................... 24

G74 Front counter boring cycle ................................................................................................ 24

G75 Longitudinal grooving cycle............................................................................................... 25

G76 Threading cycle................................................................................................................. 25

G71 Canned roughing cycle example ...................................................................................... 26

G74 and G83 fixed drilling cycles (with chip breakage) examples ........................................... 27

G74 Drilling cycle with a short retraction for chip breakage ..................................................... 27

G83 Fixed drilling cycle with retraction at the start for chip breakage and removal ................. 27

G84 Fixed rigid tapping cycle example..................................................................................... 27

G75 Fixed longitudinal grooving cycle example ....................................................................... 29

G76 Threading fixed cycle ........................................................................................................ 30

Direct drawing input (angles and round edges)........................................................................ 34

Tool radius compensation......................................................................................................... 36

Tool types.................................................................................................................................. 37

G40 G41 and G42 tool radius compensation examples…. ...................................................... 38

G71 Type I - Example of roughing and finishing cycle with direct drawing input of profile and tool

radius compensation................................................................................................................. 40

G71 Type II - Roughing cycle with displacement direction reversal on X-axis......................... 42

PROGRAMMING MANUAL -3-

G72 Example of cross roughing cycle parallel to X-axis .......................................................... 44

M98 Sub program examples .................................................................................................... 49

Bar feed examples (Hydrafeed)................................................................................................ 52

Bar feed examples (Super 80).................................................................................................. 52

C Axis and powered tooling......................................................................................................54

M codes related to C Axis functions ......................................................................................... 54

G83 Axial drilling cycle (powered tool) ..................................................................................... 55

G87 Radial drilling cycle (powered tool)................................................................................... 55

G184 Axial rigid tapping cycle (powered tool) .......................................................................... 56

G188 Radial rigid tapping cycle (powered tool) ....................................................................... 55

G83 Example of axial front drilling cycle (powered tool)…………………………………….. ..... 57

G87 Example of radial drilling cycle (powered tool)………………………………………………58
G87 Example of radial drilling cycle (using powered tool and Y-axis)………………………….59

G184 Example of axial face tapping cycle (powered tool)………………………………...........60

G188 Example of radial tapping cycle (powered tool)…………………………………………….61
G188 Example of radial tapping cycle (powered tool and Y-axis)……………………………….61

Polar interpolation G112 (G12.1)..………………………………. .............................................. .62

Tool nose radius compensation with G112 polar coordinate interpolation ............................. 64

G112 (G12.1) example of machining a square.………………………………......................... ...65

G112 (G12.1) example of machining a hexagon...................................................................... 66

Radial milling using the Y-axis and C-axis positioning example .............................................. 67

Radial helical Interpolation example………………….…………………………………………….68

G107 (G7.1) Cylindrical Interpolation ...................................................................................... 69

Tool nose radius compensation used with G107 cylindrical interpolation………………………71

G107 (G7.1) rectangle pocket example ................................................................................... 72

G107 (G7.1) rectangle pocket with corner radii example ........................................................ 74

Servo tailstock setup .............................................................................................................. 76

U Drill adaptor installation ...................................................……..………………………………78

PROGRAMMING MANUAL -4-

BASIC CONCEPTS

Machine axes

X-, Z- and B-axis and their respective positive and negative displacement directions are shown on
the above schematic diagram.

Y+ and Y- axis are not shown Y- is towards machine bed and Y+ away from the machine bed,
50mm+,50mm– to give stroke of 100mm. (machine needs to be on Y zero for turning operations).

As you can see, when workpiece zero reference point is located on workpiece end (most common
case), the positive direction is outside the workpiece, while the negative direction is on the
workpiece area to be machined (inside the workpiece).

Commonly, you will operate in the quadrant defined by X+ and Z-.

The machine will enter only in X- area for facing operations.

C-axis would be used to swivel the main spindle head in
order to position the work piece for drilling operations using
a powered tool.

C+ is in clockwise direction and C- is counter clockwise
direction.

Z- B- B+

X+

Z+

X-

C+C-

PROGRAMMING MANUAL -5-

Other axes that could be encountered when programming the
machine are

F: feed axis (related to slides) to be programmed when in operation.

In millimetres x per revolution when the head is rotating (turning)
For example:

G99 F0.3 Æ this means “03 millimetres per revolution”.

In millimetres per minute when the head is stopped (MC).
For example:

G98 F80 Æ this means “80 millimetres per minute”

T: is turret rotation.
R: is radius programming.

S: are head revolutions (cutting speed) This letter is always related to heads.

G50 S1000 Æ Rpm limit.
G97 S1000 Æ fixed rpm (for tapping and drilling).
G96 S200 Æ cutting speed (m/min) for all turning operations.

Cutting speed formula:

π×D×n

Vc=

,C: Chamfer programming.
,A: Angle programming.

Machines must be at the X home position for turret indexing.

1000

Vc×1000

n=

π×D

Vc= Cutting speed
D= Part standard diameter
n= Rpm limit.

PROGRAMMING MANUAL -6-

Tool offset

The required offset values must be entered each time tool position is changed with respect to the
aforementioned position; if tool position is not changed, entering a offset value will not be
necessary as these values are stored in the memory.

Entering tool offset values

There are two ways for entering tool correction values.

st

1

.) Supplied with presetter.

For machines with presetter, place the presetter in position and preset the tool.

nd

2

.) supplied without presetter.

For machines without presetter, turn the work piece and retract the tool without moving it out the
axis. Then measure the work piece and enter the readings in the geometry table.
To enter a value, go to the geometry table (offset value), enter the required value and press the
intermediate key; by this way the control unit will calculate the offset value.

Workpiece zero reference point

Workpiece zero is the distance that the workpiece protrudes from main chuck face.

We advise you to enter workpiece zero at the beginning of the program.
X and Y can be omitted but for safety it should be included.

G10 P0 X0. Y0. Z-80. “WORKSHIFT”

Or

G10 L2 P1 X0. Y0. Z-80. “ G54”

Facing

Program number

Metric input

Data input

O0001;

G21

G10 L2 P1 X0. Y0. Z-103

PROGRAMMING MANUAL -7-

O0001;
G21 ;
G10 L2 P1 X0. Y0. Z-103 ;
M1;

N1 G28 U0.V0.
T101
(FACING);

G50 S2000 (LIMIT R.P.M.);

G96 S200 M3;
G0 G40 G99 X45 Y0. Z0 M8;
G1 X-2 F0.25;
G0 X150 Z100 M9;
M30;

G54 Workpiece zero point

Line number

Comment

Spindle speed in

m/min

Rapid, Cancel tool

compensation and Feed

(mm/revolution)

Feed move

Rapid move to a safe
position

Program end rewind
to start of program

N1 G28U0.V0.

Position the turret on

T101;

tool 1 with offset

(FACING);
G50 S2000
G96 S200 M3;

Spindle rotation in

forward direction

G0 G40 G99 X45. Y0. Z0. M8
G1 X-2. F0.25;
G0 Z2. ;
X150. Z100. M9
M30;

Rapid move to a X and
Y home position

number 01

Limit to

2000 r.p.m.

Coolant on

Position tool

Feed rate per

revolution

End Point

Coolant off

PROGRAMMING MANUAL -8-

In this manual we will always refer to G codes

Comment::
These are notes included in the program.
These notes are totally optional, and it is up to the programmer to enter them or not.
These notes will be always placed in round brackets () in order to prevent the program
reading them.

T101
Here is shown that the tool to be used is in position 1 and a offset value of 01 is applied.
T0101 could be also entered, as the four mandatory characters are present, however, the
first zero is optional.

Head rotation direction:
M3 head rotation direction forward
M4 head rotation direction reverse
M5 spindle stop

type A.

If instructing the reverse from the forward direction or vice versa, the
spindle must be stopped first.
This is also valid for the sub spindle and live tools.

G0 X150 Z100
Note that tool retraction in this example is to 150 mm on X+ and 100 mm on Z+ from work
piece zero, and not from chuck face, as no order for changing the position is given to
work piece zero, which in this example is maintained in the previous position.

Line number (N10, N20...)
Line numbers are optional, and can be either entered or not.

G0 G40 G99 X45. Z0. M8
As you can see, G codes are first placed and then X, Z and M codes. Codes can be also
entered in the following manner: G0 X45. Z0.G99 G40 M8

Entering codes such as G96 and G50 in the same line is not permitted.

PROGRAMMING MANUAL -9-

Taper turning

O0002 Name of the program
G21 Metric program
G10 L2 P1 X0. Y0. Z-78 Part-zero at 78

N1 G28 U0.V0. Line number and move to X and Y home position
T101 Tool call pos 1 and offset 01
(TURN) Description
G50 S1500 Spindle turning limit: 1500 rpm
G96 S200 M3 Cutting speed (m/min), Spindle fwd direction.
G0 G40 G99 X52.5 Y0. Z2 M8 Rapid feed to point X52.5 Y0. Z2, Cancel tool nose

radius compensation, Feed per rev, Coolant on.

G1 Z-19.9 F0.25 Feed move Z-19.9 (First pass), Feed rate.
G0 X55 Z2 Rapid feed to X55 Z2
X45 Rapid feed to start point of cone in X45 Z2
G1 Z0 Feed move to X45 Z0
X52 Z-20 F.2 Machine the cone to X52 Z-20 (Second pass)
X61 Machine to X61 Z-20
G0 X150 Z100 M9 Rapid to safe position to 100mm in both axes and coolant

off

M30 End of program and back to he beginning

Pass

Pass

PROGRAMMING MANUAL -10-

Inside turning:

O0003
G21 Metric input
G10 L2 P1 X0. Y0. Z-85 Part zero at 85

N6 G28 U0.V0. Line number and move to X and Y home position
T606 Tool call (pos. 06 and offset 06)
(BORE) Description
G50 S2000 Turning speed limit: 2000 r.p.m.
G96 180 M3 Cutting speed =180 mm/rev, Spindle fwd direction.
G0 G40 G99 X44 Y0. Z2 M8 Rapid move Z2 axis to the height of the chamfer 2x45º ,

G1 Z0 F0.2 Feed move to Z0, feedrate 0.2 mm/rev
X40 Z-2 F.15 Machine chamfer with feedrate 0.15 mm/rev
Z-40 F.2 Machine the bore at ø40 with federate 0.2 mm/rev
X35 Face the inside until ø35
G0 Z5 Rapid feed to Z5
X150 Z100 M9 Rapid to safe position to X150 Z100 and coolant off
M30 End of program and back to he beginning

Cancel tool nose radius compensation, Feed per rev,
Coolant on.

PROGRAMMING MANUAL -11-

Circular Interpolation

O0004
G21 Metric input
G10 L2 P1 X0. Y0. Z-110 Part zero at 110

N3 G28 U0.V0. Line number and move to X and Y home position
T303 Tool call (pos. 03 and offset 03)
(TURN) Description
G50 S2500
G96 S220 M3
G0 G40 G99 X30 Y0. Z2 M8
G1 Z-22 F0.2 Machine to ø30 and Z-22
G2 X40 Z-27 R5 (CLOCKWISE) 5mm radius clockwise to X40 Z-27
G1 X55 Face to X55
G3 X80 Z-57 R80 (COUNTERCLOCKWISE) 80mm radius counter clockwise to X80 Z-57
G1 Z-62 Machine to Z-60
X86 Face to X86
G0 X100 Z100 M9
M30

In this example we assume that the part is rough machined.

As seen in this example, G2 is used to machine radii in clockwise direction and G3
in counterclockwise direction.
You can also see that G2 or G3 is first entered, then the end point, and finally the
radius,

G3 G2

PROGRAMMING MANUAL -12-

Circular interpolation

O0005
G21
G10 L2 P1 X0. Y0. Z-165

N4 G28 U0.V0.
T404
(TURN)
G50 S2000
G96 S200 M3
G0 G40 G99 X69.282 Y0.Z2 M8 Rapid feed to X69.292 Z2
G1 Z-20 F0.2 Machining to Z-20
G3 X69.282 Z-60 R40 Machine a 40mm radius until point X69.282 Z-

G2 X69.282 Z-100 R40 Machine a 40mm radius until point X69.282 Z-
G1 Z-105 Machining to Z-105

G0 X150. Z100. M9
M30

As you can see, for the interpolation, you must know the point from which this
interpolation will take place in order to change radius direction (in this example on
point X69.282 Z-60).

60 counter clockwise direction

100 clockwise direction

PROGRAMMING MANUAL -13-

Incremental commands (U and W)

O0006
G21
G10 L2 P1 X0. Y0. Z-96

N5 G28 U0.V0.
T505
(GROOVE)
G97 S1250 M3
G0 G40 G99 X78 Y0. Z-20 M8 Rapid feed to X78 Z-20
G1 X65 F0.1 Grooving to ø65
G4 X1 Dwell (X1=1 second dwell )
G0 X78 Rapid feed to X78
W-10. Incremental move –10mm in Z axis (W=Z)
G1 U-7. Incremental move –7mm in X axis (U=X)

G4 X1 Dwell
G0 U7 Rapid feed 7mm in X axis (U=X)
W-15 Incremental move –15mm in Z axis (W=Z)
G1 U-9 Groove incrementally –9mm in X axis (ø69)
G4 X1 Dwell

G0 U9 Rapid feed incrementally 9mm in X axis (ø78)

X150 Z100 M9

M30

Time delays are entered each time a slot is machined in order to improve the
surface finish.

PROGRAMMING MANUAL -14-

Example for operation

O0007
G21
G10 L2 P1 X0 Y0. Z-74

N1 G28 U0.V0.
T101
(TURN)
G50 S2500;
G96 S220 M3
G0 G40 G99 X35 Y0. Z0 M8
G1 X-2 F0.15
G0 X26 Z2
G1 Z0
X28 Z-1 F0.2
Z-18 F0.25
X32
G0 X150 Z100 M9
M1

N2 G28 U0.V0.
T202
(15MM DIA DRILL)
G97 S600 M3
G0 G40 G99 X0 Y0. Z3 M8
G1 Z-47 F0.1
G0 Z10 M9
X150. Z100.
M1

Tools:
T1= Outside and facing.
T2= ø15 twist drill.
T4= Bore.

External machining

Drill

PROGRAMMING MANUAL -15-

N4 G28 U0.V0.
T404
(BORE)
G50S2250
G96 S150 M3
G0 G40 G99 X22 Y0. Z3 M8
G1 Z0 F0.25
X20 Z-1 F0.15

Bore

Z-13 F0.2
X15 Z-20 F0.15
G0 Z5 M9
X150 Z150
M30

PROGRAMMING MANUAL -16-

G Code List

For full explanation of the following G codes, refer to the examples in this manual or in the Fanuc
programming manual.

STANDAR

D G CODE

G00 01 RAPID TRAVERSE
G01 01 LINEAR INTERPOLATION
G02 01 CIRCULAR INTERPOLATION CLOCK WISE
G03 01 CIRCULAR INTERPOLATION COUNTERCLOCK WISE
G04 00 DWELL
G05 00 HIGH SPEED REMOTE BUFFER

G07.1 00 CYLINDRICAL INTERPOLATION

G10 00 PROGRAMMABLE DATA INPUT

G11 00 PROGRAMMABLE DATA INPUT CANCEL
G12.1 21 POLAR COORD INTERPOLATION MODE
G13.1 21 POLAR COORD INTERPOLATION MODE CANCEL

G17 16 XY PLANE SELECTION

G18 16 XZ PLANE SELECTION

G19 16 YZ PLANE SELECTION

G20 06 INCH INPUT

G21 06 MM INPUT

G22 09 STORED STROKE CHECK FUNCTION ON

G23 09 STORED STROKE CHECK FUNCTION OFF

G25 08 SPINDLE SPEED FLUCTUATION DETECTION OFF

G26 08 SPINDLE SPEED FLUCTUATION DETECTION ON

G27 00 REFERENCE POSITION RETURN CHECK

G28 00 REFERENCE POSITION RETURN

G30 00 2ND REFERENCE POSITION RETURN

G31 00 SKIP FUNCTION

G32 01 THREAD CUTTING

G34 01 VARIABLE LEAD THREAD CUTTING

G36 00 AUTOMATIC TOOL COMPENSATION X

G37 00 AUTOMATIC TOOL COMPENSATION Z

G40 00 TOOL NOSE RADIUS COMPENSATION CANCEL

G41 07 TOOL NOSE RADIUS COMPENSATION LEFT

G42 07 TOOL NOSE RADIUS COMPENSATION RIGHT

G50 07 MAXIMUM SPINDLE SPEED CLAMP

GROUP FUNCTION

PROGRAMMING MANUAL -17-

STANDAR
D G CODE

GROUP FUNCTION

G52 00 LOCAL COORDINATE SYSTEM SETTING
G53 00 MACHINE COORDINATE SYSTEM SETTING
G54 14 WORKPIECE COORDINATE SYSTEM 1 SELECTION
G55 14 WORKPIECE COORDINATE SYSTEM 2 SELECTION
G56 14 WORKPIECE COORDINATE SYSTEM 3 SELECTION
G57 14 WORKPIECE COORDINATE SYSTEM 4 SELECTION
G58 14 WORKPIECE COORDINATE SYSTEM 5 SELECTION
G59 14 WORKPIECE COORDINATE SYSTEM 6 SELECTION
G65 06 MACRO CALL
G66 12 MACRO CALL MODAL
G67 12 MACRO CALL MODAL CANCEL
G70 00 FINISHING CYCLE
G71 00 STOCK REMOVAL IN TURNING
G72 00 STOCK REMOVAL IN FACING
G73 00 PATTERN REPEATING
G74 00 END FACE PECK DRILLING
G75 00 OUTER DIA DRILLING CYCLE/ GROOVING CYCLE
G76 00 MULTIPLE THREADING CYCLE
G80 10 CANNED CYCLE CANCEL
G83 10 CANNED CYCLE FOR FACE DRILLING

G184 10 CANNED CYCLE FOR FACE TAPPING

G85 10 CANNED CYCLE FOR FACE BORING
G87 10 CANNED CYCLE FOR SIDE DRILLING

G188 10 CANNED CYCLE FOR SIDE TAPPING

G89 10 CANNED CYCLE FOR SIDE BORING
G90 01 OUTER DIA/ INTERNAL DIA CUTTING CYCLE
G92 01 THREAD CUTTING CYCLE
G94 01 END FACE TURNING CYCLE
G96 02 CONSTANT SURFACE SPEED
G97 02 CONSTANT SURFACE SPEED CANCEL
G98 05 FEED PER MINUTE
G99 05 FEED PER REVOLUTION

PROGRAMMING MANUAL -18-

M FUNCTIONS

M functions used in machining programs are described in this section, this is a general list for
the NL200Y and some codes may not be active due to the machine specification.
Please refer to the individual manual supplied with the machine.
These codes control functions complementary to those controlled by G codes. For instance,
coolant supply, head rotation direction, etc.

M CODE FUNCTION NOTE

M00 PROGRAM STOP
M01 OPTIONAL STOP
M02 PROGRAM END
M03 SPINDLE FORWARD
M04 SPINDLE REVERSE
M05 SPINDLE STOP
M08 COOLANT ON
M09 COOLANT OFF
M12 TAILSTOCK COOLANT / AIR BLOW ON OPTION
M13 SPINDLE FORWARD AND COOLANT ON
M14 SPINDLE REVERSE COOLANT ON
M17 MAIN SPINDLE LOCK
M18 MAIN SPINDLE UNLOCK
M19 SPINDLE ORIENTATION
M20 QUILL FORWARD
M21 QUILL BACKWARD
M22 SERVO TAILSTOCK BODY 2ND THRUST
M23 SPINDLE AIR BLOW ON
M24 SPINDLE AIR BLOW OFF
M25 BLOCK DELETE ON
M26 BLOCK DELETE OFF AND FINISH M81
M27 SUB SPINDLE LOCK OPTION
M28 SUB SPINDLE UNLOCK OPTION
M29 RIGID TAP
M30 RESET AND REWIND
M32 TURRET INDEX CW DIRECTION
M33 TURRET INDEX BY CCW DIRECTION
M34 CHIP CONVEYOR ON
M35 CHIP CONVEYOR OFF
M36 CHIP DISCARD WATER ON
M37 CHIP DISCARD WATER OFF
M38 G184 ENTRY TAP MODE
M39 G184 CANCEL TAP MODE
M41 LOW GEAR OPTION
M42 HIGH GEAR OPTION
M43 SLAVE SPINDLE SELECT
M44 C AXIS OFF
M45 C AXIS ON
M46 SECOND SPINDLE SELECT
M47 MASTER SPINDLE SELECT
M48 MAIN SPINDLE CHUCK INWARD MODE
M49 MAIN SPINDLE CHUCK OUTWARD MODE
M50 SUB SPINDLE CHUCK INWARD MODE OPTION
M51 SUB SPINDLE CHUCK OUTWARD MODE OPTION

PROGRAMMING MANUAL -19-

M52 TOOL ARM OUT OPTION
M53 TOOL ARM HOME OPTION

M55 AUTO DOOR OPEN OPTION
M56 AUTO DOOR CLOSE OPTION

M57 TURRET UNCLAMP TO FORCE
M58 SUB SPINDLE CHUCK CLOSE OPTION
M59 SUB SPINDLE CHUCK OPEN OPTION
M60 TAILSTOCK BODY CLAMP OPTION
M61 TAILSTOCK BODY UNCLAMP OPTION
M62 SERVO TAILSTOCK BODY FORWARD OPTION
M63 SERVO TAILSTOCK BODY BACKWARD OPTION
M64 SPINDLE HYDRAULIC PRESSURE LOW OPTION
M65 SPINDLE HYDRAULIC PRESSURE HIGH OPTION
M66 SPINDLE RUNNING, M68/M69 CAN EXECUTE
M67 CANCEL M66
M68 MAIN SPINDLE CHUCK OPEN
M69 MAIN SPINDLE CHUCK CLOSE
M70 PARTS CATCHER OUT
M74 PARTS CATCHER HOME
M75 SUB SPINDLE SWITCH TO SPEED CONTROL OPTION

M76

SUB SPINDLE SWITCH TO CONTOUR

CONTROL

OPTION

M77 M4= M3 AND M3=M4
M78 M77 OFF
M79 S1, S2 SYNCHRONISATION ON OPTION
M80 S1, S2 SYNCHRONISATION OFF OPTION
M81 BAR FEED PUSH
M82 BAR END CHECK
M83 BAR END CHECK CANCEL
M85 ERROR DETECT ON
M86 ERROR DETECT OFF
M87 CHAMFERING ON
M88 CHAMFERING OFF
M90 PARTS COUNTER
M98 CALL SUB PROGRAM
M99 END OF SUB PROGRAM

PROGRAMMING MANUAL -20-

THREADING

O0008
G21
G10 L2 P1 X0 Y0. Z-95

N1 G28 U0.V0.
T101
(TURN)
G50 S2500
G96 S200 M3
G0 G40 G99 X70 Y0 Z0 M8
G1 X-2 F0.25
G0 X57 Z1
G1 Z0
X59.9 Z-1.5
Z-45
X66
G0 X150 Z100 M9
M1

N2 G28 U0.V0.
T202
(SCREWCUT)
G97 S700 M3
G0 G40 G99 X60 Y0 Z6 M8
X59.4 (First pass)
G32 Z-40 F1 (F=THREAD PITCH)
G0 X62
Z6
X58.8 (Second pass)
G32 Z-40 F1
G0 X62
Z6
X58.7 (Last pass)
G32 Z-40 F1
G0 X62
X150 Z100M9
M30

G32 for threading operations, always operate at fixed rpm (G97).

When retapping threads, do not release the work piece, do not change the speed
and do not change the start point.

PROGRAMMING MANUAL -21-

PROGRAMMING MANUAL -22-

CANNED CYCLES

G70 Finishing cycle

G70 P100 Q200

PÆ Block number from which the profile operation begins.
QÆ Block number from which the profile operation ends.

At the end of each cycle sequence the machine is always positioned in the position
at which this cycle sequence was started. The tool will be commonly located in the
position used for rough machining.
The profile allows changing X and Z direction.

G71 Longitudinal roughing cycle parallel to Z-axis

G71 U3 R1
G71 P100 Q200 U0.3 W0.1 F0.25

UÆ Cut depth on radius (mm).
RÆ Retraction in radial direction from diameter to prevent touching the machined diameter
(mm).
PÆ Block number from which the profile operation begins.
QÆ Number of end block of profile.
UÆ Finishing allowance for radius on X-axis (mm).
WÆ Finishing allowance on Z-axis (mm).
FÆ Instantaneous feed (mm/revolution).

At the end of each cycle sequence the machine is always positioned in the position
at which this cycle sequence was started.
The positioning allows changing X- and Z-axis direction.

PROGRAMMING MANUAL -23-

G72 Cross roughing cycle transversal parallel to X-axis

G72 W3 R1
G72 P100 Q200 U0.25 W0.1 F0.3

WÆ Depth of cut on Z-axis (mm).
RÆ Retraction amount.
PÆ Block number from which the profile operation begins.
QÆ Number of end block of profile.
UÆ Finishing allowance for radius on X-axis (mm).
WÆ Finishing allowance on Z-axis (mm).
FÆ Instantaneous feed (mm/revolution).

Same as the above one, excepting for the profile.

G73 Roughing cycle with passes parallel to profile

G73 U9 W9 R3
G73 P100 Q200 U0.4 W0.1 F0.3

UÆ Stock allowance (for radius) unmachined on X-axis (mm).
WÆ Stock allowance on Z-axis (mm).
RÆ Number of roughing passes.
PÆ Block number from which the profile operation begins.
QÆ Number of end block of profile.
UÆ Finishing allowance for radius on X-axis (mm).
WÆ Finishing allowance on Z-axis (mm).
FÆ Instantaneous feed (mm/revolution).

PROGRAMMING MANUAL -24-

G74 Drilling cycle (chip break)

G74 R0.5
G74 Z-100 Q2500 F0.25

RÆ Retract distance (chip break).
ZÆ Final drilling depth (absolute dimensions in mm).
QÆ Cut depth per pass (Microns).
FÆ Feed rate (mm/revolution).

G83 Peck drilling cycle

G0 G80 G99 X0 Y0 Z3
G83 Z-60 Q2000 F0.2
G80

ZÆ Final drilling depth (absolute dimensions in mm).
RÆ Distance from the initial position to the start point (incremental value, not required if
already in position)
QÆ Depth of cut (Microns).
PÆ Dwell time (s) at the bottom of the hole.
FÆ Feed rate (mm/revolution).

G84 Tapping cycle

G97 S500 M3
G0 G80 G99 X0 Y0 Z6
M29S500 (RIGID TAP ON)
G84 Z-10 F1
G80

ZÆ Final tapping depth (absolute dimensions in mm).
PÆ Dwell time (s) at the bottom of the hole.
FÆ Feed rate (mm/revolution).

G74 Front counter boring cycle

G74 R0.5
G74 X50 Z-4 P3000 Q4000 F0.15

RÆ Retraction (mm) to break chips.
X (U)Æ End position on X-axis (mm).
Z (W)Æ End position in slot direction (mm).
PÆ Step over on X-axis for next pass (Microns)
QÆ Cutting depth (Microns)
FÆ Feed rate (mm/revolution).

PROGRAMMING MANUAL -25-

G75 Longitudinal grooving cycle

G75 R0.2
G75 X43 W-7.5 P4000 Q2500 F0.15

RÆ Retraction (mm) to break chips
XÆ Groove bottom diameter (mm).
WÆ Groove end point on Z-axis (mm) if Z is specified in absolute dimensions and W is the
displacement in incremental mode; from left-hand to right-hand (W+) and from right-hand to
left-hand (W-), always subtracting tool width.
PÆ Cutting depth on X-axis (Microns).
QÆ Step over on Z-axis for next pass (Microns).
FÆ Feed rate (mm/revolution).

IMPORTANT: Roughing cycles are without tool radius compensation. Because of
this, higher allowances will be specified for X and Z depending on tool radius.

G76 Threading cycle

G76 P030060 Q200 R0.05
G76 X98.773 Z-40 R0 P1227 Q400 F2

P03Æ Number of finishing passes.
P00Æ Thread run out ; distance at which thread outlet is started, in tenths of turn Example: If
thread pitch is 2 and 20 is entered: 2mm x 2 turns = 4 mm (thread runs out 4mm before the
end point).
This is normally set to 00
P60Æ Thread angle in degrees
QÆ Minimum depth of cut (Microns).
RÆ Finishing allowance (mm).
XÆ Core diameter (mm).
ZÆ Thread end point on Z-axis (absolute dimensions in mm).
RÆ Height difference on radius (mm) for taper threads (Microns).
PÆ Thread depth (Microns).
QÆ Cut depth for first pass (Microns).
FÆ Thread pitch (mm).

PROGRAMMING MANUAL -26-

1. EXAMPLES OF CANNED CYCLES

G71 Canned roughing cycle

O0071
G21
G10 L2 P1 X0 Y0. Z-130

N1 G28 U0.V0.
T101
(ROUGH TURN)
G50 S2500
G96 S200 M3
G0 G40 G99 X105 Y0 Z0 M8

G1 X-2 F0.25

G0 X105 Z1

G71 U3 R1
G71 P100 Q200 U2 W2 F0.3
N100 G0 X40
G1 Z-30
X60 Z-60
Z-80
N200 X105 Z-90
G70 P100 Q200 (FINISHING CYCLE)
G0 G40 X150 Z100 M9
M30

PROGRAMMING MANUAL -27-

G74 and G83 fixed drilling cycles (with chip breakage)

G74 Drilling cycle with a short retraction for chip breakage

O0009;
G21;
G10 L2 P1 X0 Y0. Z-75.

N8 G28 U0.V0.
T808
(DRILL)
G97 S265 M3
G0 G40 G99 X0 Y0. Z3. M8
G74 R0.5
G74 Z-60 Q20000 F0.2
G0 X150 Z100 M9
M30

G83 Fixed drilling cycle with retraction at the start for chip
breakage and removal

O0010
G21
G10 L2 P1 X0 Y0. Z-75.

N8 G28 U0.V0.
T808
(DRILL)
G97 S500 M3
G0 G80 G99 X0 Y0. Z3 M8
G83 Z-60 Q20000 F0.2
G80
G0 X150 Z100 M9
M30

PROGRAMMING MANUAL -28-

G84 Rigid Tapping Cycle

O0011
G21
G10 L2 P1 X0 Y0. Z-75.

N8 G28 U0.V0.
T808
(TAP M6)
G97 S500 M3
G0 G80 G99 X0 Y0. Z6 M8
M29S500
G84 Z-15 F1.
G80
G0 X150 Z100 M9
M30

PROGRAMMING MANUAL -29-

Fixed longitudinal grooving cycle

O0011;
G21;
G10 L2 P1 X0 Y0 Z-110.;

N7 G28 U0.V0.
T707;
(GROOVE);
G50 S1000;
G96 S110 M3;
G0 G40 G99 X80 Y0 Z-55 M8;
G75 R.5; Grooving with chip breaking
G75 X69 Z-28 P3000 Q2500 F.1; Grooving, penetrate until ø69 and until Z(W)-28,

penetration in X(P) 3mm, movement in Z(Q) 2.5mm.

G0 X150 Z100 M9;
M30;

Groove width or groove end point can be defined with a W code in this example
(W27, that is, 30 – 3 of tool), if tool is positioned on the right-hand would be (W-27).
For either Z or W, tool width must be subtracted.

PROGRAMMING MANUAL -30-

Threading fixed cycle (M60 * 2mm pitch)

O0012
G10 L2 P1 X0 Y0 Z-88

N1 G28 U0.V0.
T101
(TURN)
G50 S2000
G96 S200 M3
G0 G40 G99 X68 Y0 Z0. M8
G1 X-2 F0.25
G0 Z2
G42 X54. Z1
G1 X60 Z-2 F0.15
Z-35 F0.25
X66
G0 G40 X150 Z100 M9
M1

N9 G28 U0.V0.

T909
(SCREWCUT)
G97 S800 M3
G4X1.
G0 G40 G99 X62 Y0 Z6 M8
G76 P030060 Q200 R0.03
G76 X57.4 Z-30 P1227 Q400 F2
G0 X150 Z100 M9
M30

Application exercise for threading operations

O0013
G21
G10 L2 P1 X0 Y0 Z-100

N1 G28 U0. V0.
T101
(TURN)
G97 S200 M3
G0 G40 G99 X73 Y0. Z0. M8
G1 X-2 F0.2
G0 X61 Z2
G1 Z0
X64.9 Z-2 F0.15 (THREAD DIAMETER)
Z-35 F0.2
X70 Z-50 F0.15
X71
G0 X150 Z100 M9
M1

PROGRAMMING MANUAL -31-

PROGRAMMING MANUAL -32-

N8 G28 U0. V0.
T808
(DRILL)
G97 S300 M3
G0 G99 X0 Y0 Z3 M8
G74 R1
G74 Z-84 Q3000 F0.15
G0 X150 Z100 M9
M1

N10 G28 U0. V0.
T1010
(BORE)
G97 S150 M3
G0 G40 G99 X34 Y0 Z2 M8
G1 Z0 F0.25
X29.6 Z-2 F0.15
Z-30 F0.2
X27
G0 X150 Z100 M9
M1

N12 G28 U0. V0.
T1212
(INTERNAL SCREWCUT)
G97 S1275 M3
G4X2.
G0 G99 X28 Y0 Z6
G76 P030060 Q300 R0.05
G76 X32 Z-25 P1230 Q450 F2
G0 X150 Z100 M9

M1

N5 G28 U0. V0.
T505
(EXTERNAL SCREWCUT)
G97 S650 M3
G4 X2.
G0 G99 X67 Y0 Z6.
G76 P030060 Q300 R0.05
G76 X63.05 Z-30 P920 Q400 F1.5
G0 X130 Z25 M9
M30

PROGRAMMING MANUAL -33-

PROGRAMMING SIMPLIFICATION FUNCTIONS (DIRECT

DRAWING INPUT)

In theses cases, considering tool direction is most important.

The easier procedure is drawing a quadrant on the drawing and locate the
degrees as shown on the above diagram.

PROGRAMMING MANUAL -34-

Direct programming of profile (angles and round edges)

PROGRAMMING MANUAL -35-

O0014
G21
G10 L2 P1 X0 Y0 Z-120

N3 G28 U0.V0.
T303
G50 S2200
G96 S230 M3
G0 G40 G99 X0 Y0 Z3. M8
G1 Z0 F0.15 (P1)
,A90 ,R6 (FIRST ANGLE)
,A165 X50 Z-25 (SECOND ANGLE) A165 comes from 180°-15°=165°
,A180 Z-49.
,A90 X75. ,C1
Z-60
,A150 ,R50 A150 comes from 180°-30°=150°
,A110 X185 Z-100 A110 comes from 180°-70°=110°
,A90 X200 ,C2
,A180 Z-150. (P2)
G0 X250 Z100 M9
M30

PROGRAMMING MANUAL -36-

Tool radius compensation

st

1

) Type of toolÆ (Control) T (Offsets table).

st

2

) Radius inserts of toolÆ (Control) R (Offsets table).

st

3

) Workpiece position with respect to tool Æ (Part program) G41 or G42.

<EXTERNAL>

<INTERNAL>

Tool types

PROGRAMMING MANUAL -37-

Milling cutters are assigned with type “0” or “9” for interpolations.

PROGRAMMING MANUAL -38-

G40 G41 and G42 tool radius compensation

Tools

T1 = EXTERNAL
T8= TWIST DRILL ø38
T10 = INTERNAL

O0015 (TOOL RADIUS COMPENSATION G40, G41, G42)
G21
G10 L2 P1 X0 Y0 Z-95.

N1 G28 U0.V0.
T101
(TURN)
G50 S2200
G96 S200 M3
G0 G40 G99 X110 Y0 Z0 M8
G1 X-2 F0.25
G0 X100 Z2
G1 Z-17
G0 X102 Z3
G42 X95 Z1 (ACTIVES COMPENSATION RIGHT)
G1 Z0 F0.1
X97 Z-1 F0.15
Z-15 F0.2
,A150 X102.
,A180 Z-45
X106.
G0 G40 X150 Z100 M9 (CANCEL TOOL COMPENSATION)
M1

N8 G28 U0.V0.
T808
(DRILL 38MM DIA)
G97 S165 M3
G0 G99 X0 Y0 Z3 M8
G74 R1
G74 Z-80 Q25000 F0.25
G0 X150 Z100 M9
M1

N10 G28 U0.V0.
T1010
(BORE)
G50 S2000
G96 S150 M3
G0 G40 G99 X45 Y0 Z2 M8
G1 Z-6 F0.2
X41 Z-35
Z-38.9
G0 X37 Z2
G41 X50 Z1 (ACTIVES COMPENSATION LEFT)
G1 X46 Z-1 F0.15
Z-6
X42 Z-35
Z-39
X37
G40 X35(CANCEL TOOL COMPENSATION)
G0 Z10. M9
X150 Z100
M30

PROGRAMMING MANUAL -39-

PROGRAMMING MANUAL -40-

G71 Type I - Example of roughing and finishing cycle with direct
definition of profile and tool radius compensation

PROGRAMMING MANUAL -41-

O0016 (Example of roughing cycle G71 Type I);

G21
G10 L2 P1 X0 Y0 Z-115.

N1 G28 U0.V0.
T101
(ROUGH TURN)
G50 S2500
G96 S200 M3
G0 G40 G99 X115 Y0 Z2 M8
G1 X-2 F0.25
G0 Z2. (POSITIONING, STARTOF CYCLE)
X111 (POSITIONING, STARTOF CYCLE)
G71 U3 R1 (ROUGHING CYCLE)
G71 P100 Q200 U0.3 W0.1 F0.25
N100 G0 X52 (START OF PROFILE)
G42 X54. Z1.
G1 X60. Z-2 F0.15
Z-22
,A170. ,R20
,A140. X95 Z-50. ,R5.
,A180.
,A135. X110 Z-64
N200 G40 X111 (END POINT OF PROFILE)
G0 X150 Z100 M9
M1

N3 G28 U0.V0.
T303
(FINISH TURN)
G50 S2500
G96 S230 M3
G0 G40 G99 X62 Y0 Z0 M8
G1 X-1 F0.15
G0 Z2
X111. (POSITIONING START OF CYCLE)
G70 P100 Q200 (FINISHING CYCLE)
G0 X150 Z100 M9
M1

N5 G28 U0.V0.
T505
(SCREWCUT)
G97 S750 M3
G4X1.
G0 G99 X62 Y0 Z6 M8
G76 P030055 Q050 R0.05
G76 X57.641 Z-19. P1179 Q450 F1.814
G0 X150 Z100 M9
M30

All cycles end where they are started and, because of this, finishing positioning is
done above the workpiece.

PROGRAMMING MANUAL -42-

G71 Type II - Roughing cycle with displacement direction reversal on
X-axis

O0017 (Example of roughing cycle G71 Type II)
G21
G10 L2 P1 X0 Y0 Z-115

N1 G28 U0.V0.
T101
(ROUGH TURN)
G50 S2250
G96 S200 M3
G0 G40 G99 X95 Y0 Z0.1 M8
G1 X-2 F0.2
G0 Z2.
X92
G71 U2.5 R1
G71 P100 Q200 U1.2 W0.1 F0.2
N100 G0 X60 Z1.
G1 G42 Z0 F0.15
G3 X76 Z-39 R40
G1 Z-57
X90 Z-65
N200 G0 G40 X92
X150 Z100 M9
M1

N3 G28 U0.V0.
T303
(FINISH TURN)
G50 S2750
G96 S220 M3
G0 G40 G99 X65 Z0 M8
G1 X-2 F0.15
G0 Z2.
X92
G70 P100 Q200
X150 Z100 M9
M30

For control units with capability for machining profiles with X-axis direction
reversal, the first block for defining the profile must state the movement of the two
axes.

PROGRAMMING MANUAL -43-

PROGRAMMING MANUAL -44-

G72 Example of cross roughing cycle parallel to X-axis

TOOLS:

T1 = EXTERNAL ROUGHING
T2 = EXTERNAL FINISHING
T6 = INTERNAL ROUGHING
T10 = INTERNAL FINISHING

ROUGHING CYCLE APPLICATION

00018 (Example of roughing cycle G72);

G21
G10 L2 P1 X0 Y0 Z-115.

N1 G28 U0.V0.
T101
(ROUGH TURN)
G50 S2200
G96 S200 M3
G0 G40 G99 X95 Y0 Z0.1 M8
G1 X18 F0.25
G0 X92 Z2
G72 W2.5 R1
G72 P100 Q200 U0.3 W0.15 F0.25
N100 G0 G41 Z-15
G1 X90
X88 Z-1;4
X55 ,R4
Z-1.5
N200 X50. Z1
G0 X150 Z100 M9
M1

N6 G28 U0.V0.
T606
(ROUGH BORE);
G50 S2250
G96 S150 M3
G0 G40 G99 X18 Y0 Z2 M8
G71 U2.5 R1
G71 P300 Q400 U-0.3 W0.1 F0.2
N300 G0 X45
G41 X43. Z1
G1 X38 Z-1.5 F0.1
,A180 ,R15
,A195. X25 Z-30
X22
X20 Z-31
N400 G40 X18.
G0 X150 Z100 M9
M1

N10 G28 U0.V0.
T1010
(FINISH BORE)
G50 S1750
G96 S180 M3
G0 G40 G99 X18 Y0 Z2 M8
G70 P300 Q400
G0 X150 Z100 M9
M1

PROGRAMMING MANUAL -45-

PROGRAMMING MANUAL -46-

N3 G28 U0.V0.
T303
(FINISH TURN)
G50 S2250
G96 S230 M3
G0 G40 G99 X57 Y0 Z0 M8
G1 X35. F0.1
G0 X92 Z2
G70 P100 Q200
G0 G40 X150 Z100 M9
M30

M98 Repetitions of a subprogram

SUBPROGRAM REPETITION APPLICATION

00019 (Repeating of subprogram M98);
G21;
G10 L2 P1 X0 Y0 Z-150.

N5 G28 U0.V0.
T505
(GROOVING)
G50 S1750
G96 S100 M3
G0 G40 G99 X74 Y0 Z-59 M8
M98 P1000 (CALLING TO SUBPROGRAM 01000)
G0 Z-42

M98 P1000

PROGRAMMING MANUAL -47-

PROGRAMMING MANUAL -48-

SUBPROGRAM FOR A SLOT:

The subprogram is called by means of command P followed by a number. This

number consists of four or more characters.

If the number consists of four characters, it indicates the identification number of
subprogram to be called.

If the number consists of more than four characters, the first four characters, from
right to left, indicate the identification number of subprogram to be called. Next
characters indicate the number of repetitions of subprogram to be called.

G0 Z-25
X44
M98 P1000
G0 Z-10
M98 P1000
G0 X200 Z200 M9
M30

01000 (SUBPROGRAM FOR THE SLOT)
G1 U-12 F0.1
G4 X1
G0 U12
W-1
G1 U-4
U-2 W1
G0 U6
W1
G1 U-4
U-2 W-1
G0 U6
M99 (END OF SUBPROGRAM)

M98 Repetition of parts of a program

PROGRAMMING MANUAL -49-

PROGRAMMING MANUAL -50-

PARTS OF A PROGRAM REPETITION APPLICATION:

00020 (REPEATING OF PARTS OF A PROGRAM)
G21
G10 L2 P1 X0 Y0 Z-150.

N4 G28 U0.V0.
T404
(GROOVING)
G50S1750
G96 S90 M3
G0 G40 G99 X46 Y0 Z0 M8
M98 P21001 (REPEATS TWO TIMES 1001)
G0 X200 Z200 M9
M30

SUBPROGRAM FOR A SLOT:
O1001 (SUBPROGRAM FOR GROOVING)

W-10
G1 X30 F0.1
G4 X1
G0 X36
M99

As described above, a subprogram or part of a subprogram is repeatedly called by means of a

command P followed by several numerical characters. In this example, the subprogram is

repeatedly called by means of “P21001”.

This command consists of three parts:

“P” Æ calling a subprogram.
“2” Æ number of subprogram repetitions.
“1001”Æ number consisting of four characters and directly referring to the subprogram.

The maximum number of repetitions for a subprogram in a single call is

9999.

PROGRAMMING MANUAL -51-

OTHER EXAMPLE OF SUBPROGRAM EXECUTION REPETITION

PROGRAM:

O0021 (EXAMPLE OF M98)
G21
G10 L2 P1 X0 Y0 Z-130

M98 P30002 (REPEATS 3 TIMES THE SUBPROGRAM 0002)
G0 X150 Z150 M9

M30

SUBPROGRAM
00002 (SUBPROGRAM)

N1 G28 U0.V0.

T101

G50 S1500
G96 S150 M3
G0 G40 G99 X36 Y0 Z-10
G1 X30. F0.08

G0 X36.

G10 P0 W10

M99

PROGRAMMING MANUAL -52-

Bar feed examples (Hydrafeed)

The program example below is for reference, some modifications may be required due to
variations in the machine software and customer requirements

O5000 (BAR FEED DEMO)
G21
G10 L2 P1 X0. Y0 Z-165.

N12 G28 U0.V0.
T1212
(STOP)
#110=50(COMPONENT LENGTH)
M98 P8888
M1

O8888(BAR FEED) O8889 (LOAD NEW BAR)
(#110=COMPONENT LENGTH AS POSITIVE) G0 Z50.
G28U0.V0.M9 G28 U0. V0.
M5 M63 (PARTS CATCHER UP)
G0G40G98M10(PUSH) M69 (CHUCK OPEN)

Z50. M85 (EJECT)
X0.
/ M98 P8889 G4 X1.

G1Z-#110F2500. G4 X1.
M69 (CHUCK OPEN) G1 G98 Z-#110 F2500.

G4X2. M85 (LOAD NEW BAR)
Z0.5 F3500. M68 (CHUCK CLOSE)
M68 (CHUCK CLOSE) G99
M11 (STOP PUSH) M99
G04 X2.
G0 Z50.
G28U0.V0.
M99

M64 (PARTS CATCHER DOWN
G0 X0.

PROGRAMMING MANUAL -53-

Bar feed examples (Super 80)

The program example below is for reference, some modifications may be required due to variations in the
machine software and customer requirements, also this example assumes that #3708.0=1 spindle arrival
signal is set.

O5000 (BAR FEED DEMO)
G21
G10 L2 P1 X0. Y0 Z-165.

N12 G28 U0.V0.
T1212
(STOP)
M98 P8888
M1

O8888(EAGLE NL200Y SUPER 80) O8889(EAGLE NL200Y SUPER 80 LOAD NEW BAR)

M68(CHUCK CLOSE)

G0X150.Z50. G0 Z50.
X0.M25(SKIP ON) G28 U0.
Z10. M70(PARTS CATCHER UP)
G97S0M3 M69(CHUCK OPEN)
G1G98Z0.5F2500. M82(END OF BAR CHECK ON)
M66 M81 (EJECT)
M69(CHUCK OPEN) G4X2.
M82(END OF BAR CHECK ON) M74(PARTS CATCHER HOME)
G0 X0.
M83
G4 X1.
M82
/M98P8889 G1 G98 Z0.5 F2500.

M99

M81
G4X2.
M68(CHUCK CLOSE)
M67
G4X2.
M83
G0G99Z50.
G28U0M26
M99

PROGRAMMING MANUAL -54-

C Axis powered tooling

This section describes the procedures used to program Y type machines controlled by the C
Axis

1- Stop the spindle by entering the command M5 before entering M45

command.

2- After activating M45 C-axis on G28 H0. must be entered .

3- Before entering command M44, the powered tool must be stopped by

entering command M5.

C axis would be used to swivel the head in order to
position the work piece for drilling operations using a
powered tool.

C + is in clockwise direction and C - is counter clockwise
direction.

C+C-

M codes related to C axis functions

M3 Mill spindle forward direction
M4 Mill spindle reverse direction

M5 Mill spindle stop
M17 C-axis brake on
M18 C-axis brake off
M44 C-Axis disconnect
M45 C-Axis connect

PROGRAMMING MANUAL -55-

G83 Front drilling cycle (Z-axis powered tool)

(chip breakage with retraction to the start point)

G0 G80 G98 C90 X30 Y0 Z3
G83 Z-30 H90 K4 Q2000 M17 F100
G80

XÆ hole position

ZÆ Final drilling depth (absolute dimensions in mm)

HÆ distance between two holes in degrees.
KÆ number of holes.
QÆ Depth of cut (microns).

PÆ Dwell time (s) at the bottom of the hole.

FÆ Feed rate (mm/min).

M17Æ brake on (the brake will automatically unclamp before indexing within the cycle,

this is also optional).

See program example on page 57

G87 Radial drilling cycle (X-axis powered tool)
(chip breakage with retraction to the start point)

G0 G80 G98 X50 Y0 Z-20
G87 X30 H90 K4 Q2000 M17 F100
G80

XÆ Final drilling depth (absolute dimensions in mm)
HÆ distance between two holes in degrees.
KÆ number of holes.
QÆ Depth of cut (microns).
FÆ Feed rate (mm/min).
M17Æ brake on (the brake will automatically unclamp before indexing within the
cycle, this is optional).

See program example on page 58

PROGRAMMING MANUAL -56-

G184 Axial rigid tapping cycle (Z-axis powered tool)

G0 G80 G98 X30 Y0 Z6
G184 C30 Z-20 Q0.5 F1.5

CÆ C-axis angle
QÆ Dwell at bottom of hole (optional)
XÆ X hole position (optional)
YÆ Y hole position (optional)
ZÆ Final tap depth

FÆ Thread pitch
MÆ Brake (optional)

If the optional dwell is omitted then no dwell is performed within the tapping cycle.
If the X and Y is omitted from the tapping cycle then the X and Y positioning prior
to the tapping cycle is assumed. Also if the brake is not required then this is also
omitted, use of the brake does increase the cycle time.

See program example on page 60

G188 Radial rigid tapping cycle (X-axis powered tool)

G0 G80 G98 X50 Y0 Z-20
G188 C30 X30 Q0.5 F1.5

CÆ C-axis angle
QÆ Dwell at bottom of hole (optional)
XÆ Final tap depth
YÆ Y position (optional)
ZÆ Z position (optional)

FÆ Thread pitch
MÆ Brake (optional)

If the optional dwell is omitted then no dwell is performed within the tapping cycle.
If the Y and Z is omitted from the tapping cycle then the Y and Z positioning prior
to the tapping cycle is assumed. Also if the brake is not required then this is also
omitted, use of the brake does increase the cycle time.

See program example on page 61

PROGRAMMING MANUAL -57-

G83 Example of drilling cycle with Z-axis powered tool

O0022

G21

G10 L2 P1 X0 Y0 Z-100

N6 G28 U0. V0.

T606

(AXIAL 6MM DIA DRILL)

M5

M45

G28 H0

G97 S2500 M3

G0 G80 G98 X90 Y0 Z2 M8

G83 Z-10 K4 H90 F100

G80

M5

M44

G0 X150 Z150 M9

M1

ALTERNATIVE PROGRAM

This fixed drilling cycle can be programmed in the apparently more logic and simple

sequence, ie, 0º - 90º - 180º - 270º. This cycle would be as follows:

O0023

G21

G10 L2 P1 X0 Y0 Z-100

N6 G28 U0. V0.

T606

(AXIAL 6MM DIA DRILL)

M5

M45

G28 H0

G97 S2500 M3

G0 G80 G98 X90.Z2M8

G83 Z-10. Q2000 F100.

C90. Q2000

C180. Q2000

C270. Q2000

G80

M5

M44

G0 X150 Z150 M9

M1

PROGRAMMING MANUAL -58-

G87 Example of radial drilling cycle with X-axis

powered tool

3 HOLES SPACED 120º

O0024

G21

G10 L2 P1 X0 Y0 Z-100

N8 G28 U0 V0.

T808

(RADIAL 4MM DIA DRILL)

M5

M45

G28 H0

G97 S3500 M3

G0 G80 G98 X122. Y0 Z-15. M8

G87 X96.Q3000 F350.

C120.Q1000

C240.Q1000

G80

M5

M44

G0 X150.Z150.M9

M1

PROGRAMMING MANUAL -59-

G87 Example program of radial drilling cycle with X-axis
powered tool and using Y-axis positioning.

O0025
G21
G10 L2 P1 X0 Y0 Z-100

N8 G28 U0. V0.
T808
(RADIAL 4MM DIA DRILL)
M5
M45
G28 H0
G97 S3500 M3
G0 G80 G98 X122.Y-10 C0 Z-15. M8
G87 X96 Y-10 Q3000 F350
Z-20. Y-10. Q1000
Z-20. Y10. Q1000
Z-10. Y10. Q1000
G80
M5
M44
G0 X150.Z150.M9
M1

PROGRAMMING MANUAL -60-

G184 Example program of a tapping cycle with Z-axis powered
tool

O0026 (AXIAL TAPPING)
G21
G10 L2 P1 X0 Y0 Z-100

N10G28 U0 V0
T1010
M5
M45
G28 H0
G97 S800 M3
G0 G80 G98 X90 Y0 Z6 M8
G184 C0 Z-10 Q1. F1.
G184 C90 Z-10 Q1. F1.
G184 C180 Z-10 Q1. F1.
G184 C270 Z-10 Q1. F1.
M5
M44
G0 X150.Z150. M9
M30

PROGRAMMING MANUAL -61-

G188 Example program of side tapping cycle with X-axis
powered tool

O0026 (RADIAL TAP)
G21
G10 L2 P1 X0 Y0 Z-100

N12 G28 U0. V0.
T1212
M5
M45
G28 H0
G97 S800 M3
G0 G80 G98 X122 Y0 Z-10 M8
G188 C0 X96 Q1. F1.
G188 C90 X96 Q1. F1.
G188 C180 X96 Q1. F1.
G188 C270 X96 Q1. F1.
M5
M44
G0 X150. Z150. M9
M30

G188 Example program of side tapping cycle with X-axis
powered tool using Y axis positioning

O0027
G21
G10 L2 P1 X0 Y0 Z-100

N12 G28 U0. V0.
T1212
M5
M45
G28 H0
G97 S800 M3
G0 G80 G98 X122 Y10 Z-25 M8
G188 C0 X96 Y10 Q1 F1.
G188 C90 X96 Y-10 Q1 F1.
G188 C180 X96. Y10 Z-10 Q1 F1.
G188C270 X96. Y-10 Z-25.Q1 F1.
M5
M44
G0 X150. Z150. M9
M30

PROGRAMMING MANUAL -62-

G112 or G12.1 Polar coordinate interpolation

Polar coordinate interpolation is used when it is desired to perform milling operations on the
face of the work piece, which require synchronous movement of the spindle and live tooling
mounted on the turret.
When polar coordinate interpolation is commanded by the G112 or G12.1, the control interprets
several pieces of data to determine the direction and speed at which the axes must be moved
to reach the commanded end point.
The drawing below shows the coordinate system used with polar coordinate interpolation.
The programmed end points are laid out as coordinates on this plane.
Note the signs for X and C. The following program examples illustrate the use of this system.

1. The following G codes may be used when G112 is active: G1, G2, G3, G40,
G41, G42, G65, and G98.

2. G0 positioning is not allowed when G112 is active.

3. When using G2 or G3, the arc radius is specified using the R word.

4. M45 C axis mode must be active before commanding polar coordinate
interpolation.

5. The spindle should be oriented to C0 degrees before commanding polar
coordinate interpolation.

6. If machining in the X axis only, do not activate polar coordinate interpolation.

7. The unit of command for the C axis, when polar coordinate interpolation is used,
is MM or inches, not degrees.

8. When using cutter compensation during polar coordinate interpolation, the same
basic TNRC rules apply as with normal lathe programming. However, the
following rules must also be observed:-

PROGRAMMING MANUAL -63-

The tool radius and the quadrant must be loaded into the geometry offset file.
For polar coordinate interpolation, the X tool offset represents the centre of the
cutter and the tool tip location (Quadrant) will be set to 9.

9. The TNRC start up block (G41 or G42 line) must be programmed after the polar
coordinate interpolation command (G112 line) has been activated. For polar
coordinate interpolation, the X axis move must be equal to at least two times
the tool radius entered in the tool offset file. Program the G40 (TNRC cancel)
command before the block containing the G113 or G13.1 (cancel polar
coordinate interpolation).

10. Program restart and block restart are not allowed when G112 is active.

11. Specify the feedrate as millimetres per minute.

12. X values are diameters and C values are radii

PROGRAMMING MANUAL -64-

Tool nose radius compensation with G112 polar coordinate
interpolation

The drawings below show the combination of tool nose radius and circular interpolation codes
used with polar coordinate interpolation.
The shaded area in each drawing represents the finished part contour.

G41 Part right (cutter left) G42 Part left (cutter right)
G2 Clockwise arc G3 Counter-clockwise arc

G42 Part left (cutter right) G41 Part right (cutter left)
G2 Clockwise arc G3 Counter-clockwise arc

PROGRAMMING MANUAL -65-

Example of machining a rectangle with powered tool using C
Axis

O0028
G21
G10 L2 P1 X0 Y0 Z-100

N6 G28 U0. V0.
T606
(AXIAL MILL)
M5
M45
G28 H0
G97 S1500 M3
G0 G40 G98 X80. Y0 Z2 M8
G1 Z-5. F2500.
G112
G42 X50.F500.
C20.
X-50.
C-20.
X50.
C0.
G1 G40 X80.F1500.
G113
G0 Z10.M9
M5
M44
G0 X150 Z150 M9
M1

PROGRAMMING MANUAL -66-

Example of machining a Hexagon with powered tool using C
Axis

Use the following formula to calculate the following hexagon.
Data known: Across flats and angle

A= 50/2
Cos30

B= 30Tan*50/2 =14.433

O0029
G21
G10 L2 P1 X0 Y0 Z-100

N6 G28 U0. V0.

T606
(AXIAL MILL)
M5
M45
G28 H0
G97 S1500 M3
G0 G40 G98 X80. Y0. Z2.
G1 Z-0.25 F2500.
G112
G42 X50.F500.
C14.433
X0. C28.867
X-50. C14.433
C-14.433
X0. C-28.867
X50. C-14.433
C0.
G40 X80.F1500.
G113
G0 Z10.M9
M5
M44
G0 X150 Z150 M9
M30

= 28.867

PROGRAMMING MANUAL -67-

Example of machining a square with powered tool using the Y
axis and C Axis for positioning

O0030
G21
G10 L2 P1 X0 Y0 Z-100

N5 G28 U0. V0.
(RADIAL MILL)
T505
M5
M45
G28 H0.
G97 S2500 M3
G0 G40 G98 X52.Y30.Z-10.M8
M17
X39.
G1 Y-30. F400
G0 X52.
Y30.
M18
C90. (SECOND FLAT)
M17
X39.
G1 Y-30.
G0 X52.
Y30.
M18
C180. (THIRD FLAT)
M17
X39.
G1 Y-30.
G0 X52.
Y30.
M18
C270. (FOURTH FLAT)
M17
X39.
G1 Y-30.
G0 X52.M9
Y0.
G28 U.0 V0.
M5
M44
M30

PROGRAMMING MANUAL -68-

Example of helically interpolating a 20mm diameter hole off
of centre line with a powered tool

O0031
G21
G10 L2 P1 X0 Y0 Z-100

N5 G28 U0. V0.
(RADIAL MILL)
T505
M5
M45
G28 H0.
G97 S2000 M3
G0 G40 G98 G19 X52.Y20.Z-60.M8
M17
G0 X50.
G1 G41 Z-70. F400
G3 X46 K10.
G3 X42 K10.
G3 X38 K10.
G3 K10.
G1 G40 Z-60.
G0 X52.
M18
M5
M44
G0 G18 X150. Y0. Z100.
M30

PROGRAMMING MANUAL -69-

|G107 or G7.1 Cylindrical Interpolation

Cylindrical interpolation is used to perform contoured milling operations on the outside diameter
of the workpiece. The Z and C words are used to specify the end points of the moves.
When using cylindrical interpolation, the C word is programmed in degrees.
C is also used to specify the radius of the part in the G107 or G7.1 block which activates
cylindrical interpolation.
The X word is used to program the depth of cut.

1. The following G codes may be used when G107 is active: G1, G2, G3, G40, G41,
G42, G65, and G98.

2. G0 positioning is not allowed when G107 is active.

3. When using G2 or G3, the arc radius is specified using the R word.

4. M45 C axis mode must be active before commanding cylindrical interpolation.

5. The spindle should be oriented to C0 degrees before commanding cylindrical
interpolation. The formula for calculating the value of the C word is shown in the
following program example.

6. If machining in the X axis only, do not activate cylindrical interpolation.

7. The H word is used to program incremental C axis moves.

8. Machine lock mode MAY NOT BE USED when G107 is active.

PROGRAMMING MANUAL -70-

9. The unit of command for the C axis, when cylindrical interpolation is used,

degrees, not MM or INCHES.

10. When using cutter compensation during cylindrical interpolation, the same

basic TNRC rules apply as with normal lathe programming. However, the
following rules must also be observed.
The tool radius and the quadrant must be loaded into the geometry offset file.
For cylindrical interpolation, the Z tool offset represents the centre of the cutter
and the tool tip location (Quadrant) will be set to 9.

11. The TNRC start up block (G41 or G42 line) must be programmed after

the cylindrical interpolation command (G107 line) has been activated. For
cylindrical interpolation, the Z axis move must be equal to at least the tool
radius entered in the tool offset file. Program the G40 (TNRC cancel)
command before the block containing the G107 C0 (cancel cylindrical
interpolation).

12. Program restart and block restart are not allowed when G107 is active.

13. Specify the feedrate as millimetres per minute.

PROGRAMMING MANUAL -71-

Tool nose radius compensation and circular interpolation used
with G107 cylindrical interpolation

The drawings below show the combination of tool nose radius and circular interpolation codes
used with cylindrical interpolation.
The part circumference is viewed laying flat with the part face (Z0) at the base.

G41 Part Right (Cutter Left) G42 Part Left (Cutter Right)

G2 Clockwise G3 Counter Clockwise

G42 Part Left (Cutter Right) G41 Part Right (Cutter Left)
G2 Clockwise G3 Counter Clockwise

PROGRAMMING MANUAL -72-

Rectangle Example (Cylindrical Interpolation)

Calculation formula

Circumference = 38 x π =119.396mm

Degrees = mm x 360
circumference

= 9 x 360

119.396

= 27.14 degrees

eg.9mm

O0032
G21
G10 L2 P1 X0 Y0 Z-100

N4 G28 U0.V0.
T404
(RADIAL MILL)
M5
M45
G28 H0
G97 S3500 M3
G0 G40 G98 X40.Z2.
G1 Z-14. F2500.
G107 C19. G19
X37.F90.
Z-32.
C-27.14
Z-14.
C0.
X40.F1500.
G107 C0.
M5
M44
G0 X150 Z150 M9
M30

PROGRAMMING MANUAL -73-

PROGRAMMING MANUAL -74-

Rectangle with Corner Radii Example (Cylindrical Interpolation)

4MM Pocket depth
Tool compensation not used.

Calculation formula

Circumference = 36 x π =113.11mm

Degrees = mm x 360
circumference

= 8 x 360

113.11

= 25.46 degrees

eg.9mm

PROGRAMMING MANUAL -75-

O0033
G21
G10 L2 P1 X0 Y0 Z-100

N8 G28 U0. V0.
T808
(RADIAL 6MM DIA SLOT DRILL)
M5
M45
G28 H0
G97 S3500 M3
G0 G40 G98 X38.Z2.
G1 Z-14. F2500.
G107 C18. G19
X28.F100.
Z-22.
G2 C-9.55 Z-25. R3.
G1 C-15.91
G2 C-25.46 Z-22. R3.
G1 Z-15.
G2 C-15.91 Z-12. R3.
G1 C-9.55
G2 C0. Z-15. R3.
X38. F1500.
G107 C0.
M5
M44
G0 X150. Z150. M9
M30

PROGRAMMING MANUAL -76-

Servo tailstock setup

The tailstock on the NL200Y is servo driven and is the “B” axis. It has the facility to be
positioned and have the desired thrust set using a custom page on the control.
Pressing the “CUSTOM” button on the control panel will bring up this page

The following parameters will need to be set

#1 THRUST

This sets the initial pressure that the tailstock applies.

#2 THRUST

This sets a secondary pressure if required

ERROR

This is a positional tolerance in microns for the “hold coord”

DEC COORD

This is the position where the tailstock will rapid too.

HOLD COORD

This is the position that the tailstock will feed to and apply the required thrust as previously set.

BACK COORD

This is the retraction position for the tailstock. These parameters will need to be set before
using the tailstock. To operate the tailstock you will first need to set your thrust and positional
parameters. Using the curser buttons cursor to the parameter to the parameter to change.
The thrust parameters are set by using the soft keys at the bottom of the screen F2 to F5.
By pressing these buttons you can dial in your required thrusts.

PROGRAMMING MANUAL -77-

Servo tailstock initial setup

• To set the tailstock position initially bring the tailstock up to the job using the hand wheel until

it is a safe distance away from the part then press “DEC COORD”

• Now move the tailstock forward until the centre engages the part then press “HOLD
COORD”

• The “BACK COORD” can then be set to a retract position that will allow the finished part to

be removed.

• To change the other figures you can either input them directly or use F1 Measure. Pressing
F1 Measure will input the position that the tailstock is currently in.

• Once these parameters are set you can then control the tailstock in the program.

M62 will rapid the tailstock to the “DEC COORD” then it will feed to the “HOLD COORD” and

apply the set pressure.

• M22 will set the #2 THRUST (optional)

• M63 will retract the tailstock to the “BACK COORD”

PROGRAMMING MANUAL -78-

U Drill adaptor installation

The NL200Y is equipped with a servo tailstock and is the “B” axis.
It has the facility to be used as a fully programmable driven axis enabling the use of U-drills.
The machine is supplied with two tailstock adaptors one with a morse taper for use with a
centre and one with a parallel shank to suit U-drills. The taper adaptor comes pre-fitted to the
tailstock.
The following instructions are how to fit the adaptor for the U-drill.

Using manual jog or the hand wheel bring the tailstock forward to enable full access to both
ends of the tailstock.

1. Using a 6mm allen key loosen and remove the M8 cap head screws holding the morse taper
adaptor to the tailstock body.

Using two longer M8 bolts insert them into the two threaded ejector holes on the front of the
adaptor plate. Gradually tighten these two screws until the front of the adaptor separates from
the tailstock body. Once this is done you can then remove the adaptor by pulling the adaptor
forwards out of the tailstock body.

2. Now you will need to remove the rear part of the morse taper adaptor. Using a suitable
spanner undo the coolant delivery pipe. Then using an allen key remove the three cap head
screws that secure the rear adaptor plate. You can now remove the rear adaptor plate by
pulling it out gently parallel to the body housing. Now that these two parts have been removed
put them in a safe place for when they are required again.

PROGRAMMING MANUAL -79-

3. The U-drill adaptor consists of three parts, The U-drill holder that goes into the front of the tailstock,
the rear coolant pipe support plate and the coolant pipe. Apply a small amount of grease to the U­drill holder and then insert it into the front of the tailstock body. This needs to be done gently as the

diameters are a precision fit. Do not

When it is in all the way, index the adaptor until the two flats are aligned with the two flats on the
tailstock body. Insert cap screws and tighten. This is the front part complete.

4. The rear plate screws on to the back of the tailstock body using three cap screws.

use a hammer to fit this part!

5. The coolant pipe inserts through the rear coolant pipe support plate. This is then screwed into the
back of the U-drill to provide through tool coolant. The adjuster nut is then tightened up to the
coolant pipe support plate.

PROGRAMMING MANUAL -80-

6. To connect the coolant delivery pipe drive the tailstock all of the way back to home then
remove the rear door to allow access to the pipefitting.

7. The coolant delivery pipe can then be connected to the coolant pipe and tightened with a
suitable spanner.

The installation of the U-drill holder is now complete.

To change back to the morse taper holder is a reversal of these instructions.