dugard SKT210SY Programming Manual
KIA SKT210SY
TRAINING MANUAL
PROGRAMMING MANUAL -1-
Manual Iss 1
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-
Cutting speed formula: ............................................................................................................................. 9
Vc= Cutting speed .................................................................................................................................... 9
D= Part standard diameter ....................................................................................................................... 9
n= Rpm limit. ............................................................................................................................................ 9
Machines must be at the X home position for turret indexing. .................................................................. 9
We advise you to enter workpiece zero at the beginning of the program. .............................................. 10
G10 P0 Z-80. .......................................................................................................................................... 10
How to prepare the machine for machining operations with transfer: ..................................................... 11
1st Determine workpiece zero and carry out the 1st machining stage .................................................... 11
G54 is programmed. ............................................................................................................................... 11
2nd Stop the machine and verify the dimension before doing the transfer. ............................................ 11
3nd Do the transfer and place the sub-spindle in working position. ........................................................ 11
4nd Stop the machine and determine workpiece zero before performing the 2nd machining stage G55 is
programmed. ........................................................................................................................................... 11
In this manual we will always refer to G codes type A. .......................................................................... 12
Comment:: .............................................................................................................................................. 12
These are notes included in the program. .............................................................................................. 12
These notes are totally optional, and it is up to the programmer to enter them or not. ........................... 12
These notes will be always placed in round brackets () in order to prevent the program reading them. . 12
T101 12
Here is shown that the tool to be used is in position 1 and a offset value of 01 is applied. ..................... 12
T0101 could be also entered, as the four mandatory characters are present, however, the first zero is
optional. ................................................................................................................................................... 12
Head rotation direction: .......................................................................................................................... 12
M3 head rotation direction forward ......................................................................................................... 12
M4 head rotation direction reverse ......................................................................................................... 12
M5 spindle stop ...................................................................................................................................... 12
If instructing the reverse from the forward direction or vice versa, the spindle must be stopped first. ... . 12
This is also valid for the sub spindle and live tools. ................................................................................ 12
G0 X150 Z100 ........................................................................................................................................ 12
PROGRAMMING MANUAL -3-
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. ..................................................................................................... 12
Line number (N10, N20...) ...................................................................................................................... 12
Line numbers are optional, and can be either entered or not. ................................................................. 13
G0 G40 G99 X45. Z0. M8 ....................................................................................................................... 13
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 ............................................................................................ 13
Entering codes such as G96 and G50 in the same line is not permitted. ................................................ 13
In this example we assume that the part is rough machined. ................................................................. 16
As seen in this example, G2 is used to machine radii in clockwise direction and G3 in counterclockwise
direction. .................................................................................................................................................. 16
You can also see that G2 or G3 is first entered, then the end point, and finally the radius, .................... 16
Circular interpolation ............................................................................................................................... 17
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). .............................................. 17
Time delays are entered each time a slot is machined in order to improve the ..................................... 18
surface finish. ......................................................................................................................................... 18
G Code List ............................................................................................................................................ 21
M FUNCTIONS ...................................................................................................................................... 23
THREADING .......................................................................................................................................... 25
G32 for threading operations, always operate at fixed rpm (G97). ......................................................... 26
When retapping threads, do not release the work piece, do not change the speed and do not change the
start point. ................................................................................................................................................ 26
CANNED CYCLES ................................................................................................................................. 27
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. ..... 27
The profile allows changing X and Z direction. ....................................................................................... 27
At the end of each cycle sequence the machine is always positioned in the position at which this cycle
sequence was started. ............................................................................................................................. 27
The positioning allows changing X- and Z-axis direction. ....................................................................... 27
PROGRAMMING MANUAL -4-
Same as the above one, excepting for the profile. .................................................................................. 28
IMPORTANT: Roughing cycles are without tool radius compensation. Because of this, higher allowances will
be specified for X and Z depending on tool radius. .................................................................................. 30
1. EXAMPLES OF CANNED CYCLES .................................................................................................... 31
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. 35
N5 G28 U0. V0. ...................................................................................................................................... 38
T505; 38
PROGRAMMING SIMPLIFICATION FUNCTIONS ................................................................................ 39
In theses cases, considering tool direction is most important. ................................................................ 39
The easier procedure is drawing a quadrant on the drawing and locate the degrees as shown on the above
diagram. .................................................................................................................................................. 39
All cycles end where they are started and, because of this, finishing positioning is done above the workpiece.
47
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. .............................................................................. 49
M98 Repetitions of a subprogram .......................................................................................................... 53
1- Stop the spindle (S1 and/or S2) by entering the command M5 (S1) or M115 (S2) before entering M43 or
M143 command. ..................................................................................................................................... 59
2- After activating M43 C-axis on G28 C0. must be entered . .................................................................. 59
3- After activating M143 A-axis on G28 A0. must be entered. ................................................................. 59
4- Before entering command M40 and M140, the powered tool must be stopped by entering command M15.
59
59
M160, M161 and M162 commands are only used on machines equipped with a sub-spindle (S). ......... 90
M160; ............ Speed synchronisation mode on. .................................................................................... 90
M161; ............ Phase and synchronisation mode off. ............................................................................. 91
M162; ............ Phase synchronisation mode on. .................................................................................... 91
1- For transferring a workpiece from main spindle to sub-spindle, main and sub-spindle speed must be
synchronised by means of M160 command. If the workpiece is transferred without activating the
synchronisation mode, damage of the workpiece could result. ................................................................ 91
PROGRAMMING MANUAL -5-
2- For transferring an hexagonal bar, main and sub-spindle phase and speed must be synchronised by
means of M160 and M162 command, as otherwise the transfer operation will not be possible, although it is
recommended that if the part has been turned that you locate on the turned diameter so to achive any
squareness or concentricity tolerences. .................................................................................................. 91
3- M162 function can be also used for round parts, but considering that phase (and speed) synchronisation
time is longer and speed synchronisation time, using only M160 function is recommended when machining
round parts. ............................................................................................................................................. 91
Machining program. ................................................................................................................................ 92
G97 S50 M3; Main spindle rotates at 50 rpm ......................................................................................... 92
S50 M113;……………………..Sub spindle rotates at 50 rpm ................................................................. 92
M160; Synchronise spindles. .................................................................................................................. 92
M162; Synchronise spindle phase (if required). ...................................................................................... 92
Main and sub-spindle speed is synchronised to 50rpm .......................................................................... 92
M119; Sub-spindle chuck open. ............................................................................................................. 92
M151;……………………………Air blow on sub-spindle ......................................................................... 92
B-???; Sub-spindle is moved clear fo component (machine co-ordinates) ............................................. 92
G1 G98 B-??? F1500; Sub-spindle is moved over the workpiece at 1500 mm/min ................................ 92
M152; Air blow off sub-spindle. ............................................................................................................... 92
G28 B0; Sub-spindle is returned to reference point on B-axis ................................................................ 92
M161; Synchronisation mode is disabled ............................................................................................... 92
Machining program. ................................................................................................................................ 93
G97 S50 M3; Main spindle rotates at 50 rpm ......................................................................................... 93
S50 M113;………………………Sub spindle rotates at 50 rpm ............................................................... 93
M160; Synchronise spindles. .................................................................................................................. 93
M162; Synchronise spindle phase (if required). ...................................................................................... 93
Main and sub-spindle speed is synchronised to 50rpm .......................................................................... 93
M119; Sub-spindle chuck open. ............................................................................................................. 93
M151;……………………………Air blow on sub-spindle ......................................................................... 93
B-???; Sub-spindle is moved clear fo component (machine co-ordinates) ............................................. 93
G1 G98 B-??? F1500; Sub-spindle is moved over the workpiece at 1500 mm/min ................................ 93
PROGRAMMING MANUAL -6-
G28 B0; Sub-spindle is returned to reference point on B-axis ................................................................ 93
G0 X50…………………………..Move off component. ............................................................................ 93
G28 U0………………………….Move turret home in X-axis. ................................................................... 93
G28 W0…………………………Move turret home in Z-axis. ................................................................... 93
M161; Synchronisation mode is disabled ............................................................................................... 93
G28 U0.: Turret home position in X ........................................................................................................ 94
M115: Sub-spindle is stopped ................................................................................................................ 94
G4 X0.5: Dwell for half a second ............................................................................................................ 94
M73; Parts catcher forward. ................................................................................................................... 94
Workpiece collector operates independently from turret position. .......................................................... 94
The B-axis co-ordinate value will be the G30 position, at which the workpiece is released from the sub-
spindle, without causing any interference with workpiece collector, turret, etc. ........................................ 94
G4 X0.5; Dwell for half a second ............................................................................................................ 94
M119; Open jaws on sub-spindle. .......................................................................................................... 94
G4 X3.; Dwell for three seconds to allow the part to be ejected fully. ..................................................... 94
M74; Parts catcher back. ........................................................................................................................ 94
G28 B0.; Sub spindle home. ................................................................................................................... 94
G4 X1.; Dwell for one second. ................................................................................................................ 94
G83 Example of face front drilling cycle (powered tool main spindle)…………………………………59
G83 Example of face front drilling (powered tool sub spindle)…………………………………………………..60
G87 Example of side drilling cycle (powered tool main spindle)………………………………………………..61
G87 Example of side drilling cycle (using main spindle and Y-axis)…………………………………………..62
G87 Example of side drilling cycle (powered tool sub spindle )………………………………………………...63
G184 Example of front face drilling cycle (powered tool main spindle)………………………………………...64
G185 Example of back face tapping cycle (powered tool sub spindle)………………………………………..65
G188 Example of side tapping cycle (powered tool main spindle)…………………………………………… ..66
G188 Example of side tapping cycle (powered tool main spindle using Y-axis)…………………………… ..67
Cylindrical interpolation………………………………………………………………………………………………68
Tool nose radius copensation and circular interpolation used with G112 polar coordinate interpolation….70
Example of machining a square using polar milling………………………………………………………………71
Example of machining a hexagon using polar milling…………………………………………………………….72
PROGRAMMING MANUAL -7-
Milling using the Y-axis and C-axis…………………………………………………………………………………73
Milling usng the Y-axis and A-axis………………………………………………………………………………….76
Helical Interpolation using the Z-axis and Y-axis………………………………………………………………….79
Cylindrical Interpolation G107………………………………………………………………………………………..80
Tool nose radius compensation and circular interpolation used with G107 cylindrical interpolation…………82
Rectangle engrave example (cylindrical interpolation)…………………………………………………………….83
Rectangle with corner radii example (cylindrical interpolation)…………………………………………………..84
Part transfer (Billet)…………………………………………………………………………………………….........87
Part transfer (with part off).…………………………………………………………………………………….........87
Sub Spindle example…………………………..……………………………………………………………………..89
Part eject…………………………..……………………………………………………………………………........90
Machine axes
BASIC CONCEPTS
X+
Z- B- B+
Z+
X-
C+
C-
A+
A-
PROGRAMMING MANUAL -8-
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,
40mm+,40mm– to give stroke of 80mm. (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.
You may also operate X+ Z+ quadrant when the workpiece is clamped on the subhead.
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.
A-axis would be used to swivel the sub-spindle head in
order to position the work piece for drilling operations using a powered
tool.
A+ is in clockwise direction and A- is counter clockwise direction.
PROGRAMMING MANUAL -9-
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 this means “03 millimetres per revolution”.
In millimetres per minute when the head is stopped (MC).
For example:
G98 F80 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 Rpm limit.
G97 S1000 fixed rpm (for tapping and drilling).
G96 S200 cutting speed (m/min) for all turning operations.
,C: Chamfer programming.
,A: Angle programming.
Tool offset
Cutting speed formula:
Dn
Vc=
1000
Vc1000
n=
D
Machines must be at the X home position for turret indexing.
Vc= Cutting speed
D= Part standard diameter
n= Rpm limit.
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.
1st.) Supplied with presetter.
PROGRAMMING MANUAL -10-
For machines with presetter, place the presetter in position and preset the tool.
2nd.) 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 workpiece protruding length from main chuck face.
We advise you to enter workpiece zero at the beginning of the program.
Single spindle machine format
G10 P0 Z-80.
Sub spindle machine format
In the following example we explain how a value of 80 is entered for the first stage G54 (machining
the workpiece on the main spindle), while a value of 460 is entered for the second stage G55
(machining the workpiece on the sub-spindle).
G10 L2 P1 X0. Z-80. ;
G10 L2 P2 X0. Z-460. ;
Zero 1st phase
G10 L2 P1 Z-80
Zero 2nd phase
G10 L2 P2 Z-460
PROGRAMMING MANUAL -11-
How to prepare the machine for machining operations with transfer:
1st Determine workpiece zero and carry out the 1st machining stage
G54 is programmed.
2nd Stop the machine and verify the dimension before doing the transfer.
3nd Do the transfer and place the sub-spindle in working position.
4nd Stop the machine and determine workpiece zero before performing the 2
machining stage G55 is programmed.
nd
Facing
Program number
O0001;
G21 ;
G10 L2 P1 X0. Z103 ;
M1;
N1 G28 U0. ;
T101
(FACING);
G50 S2000 (LIMIT R.P.M.);
G96 S200 M3;
G0 G40 G54 G99 X45 Y0. Z0 M8;
G1 X-2 F0.25;
G0 X150 Z100 M9;
M30;
Metric input
Data input
O0001;
G21;
Workpiece zero 103
PROGRAMMING MANUAL -12-
G10 L2 P1 X0. Z103;
Line number
Comment
Spindle speed in
Rapid, Cancel tool
compensation and Feed
(mm/revolution)
Feed move
Rapid move to a safe
position
Program end rewind
to start of program
m/min
Move to X and Y
home position
N1 G28 U0.V0.
T101;
(FACING);
G50 S2000
G96 S200 M3;
Spindle rotation in
forward direction
G0 G40 G99 G54 X45. Z0. M8;
G1 X-2. F0.25;
G0 Z2. ;
X150. Z100. M9
M30;
Coolant off
Position the turret on
tool 1 with offset
number 01
Limit to
2000 r.p.m.
Coolant on
Selected work offset & Position tool
Feed rate per
revolution
End Point
In this manual we will always refer to G codes type A.
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
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...)
PROGRAMMING MANUAL -13-
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 -14-
Taper turning
O0002; Name of the program
G21; Metric program
G10 L2 P1 X0. Z78; Part-zero at 78
N1 G28 U0.V0. Line number and move to X and Y home position
T101; Tool call (pos. 01 and offset 01)
(TURN); Description
G50 S1500; Spindle turning limit: 1500 rpm
G96 S200 M3; Cutting speed (m/min), Spindle fwd direction.
G0 G40 G54 G99 X52.5 Z2 M8; Rapid feed to point X52.5 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
Inside turning:
PROGRAMMING MANUAL -15-
O0003;
G21; Metric input
G10 L2 P1 X0. Z85; 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 G54 G99 X44 Z2 M8; Rapid move Z2 axis to the height of the chamfer 2x45º ,
Cancel tool nose radius compensation, Feed per rev,
Coolant on.
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
PROGRAMMING MANUAL -16-
Circular Interpolation
G3G2
O0004;
G21; Metric input
G10 L2 P1 X0. Z110; 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 G54 G99 X30 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,
Circular interpolation
PROGRAMMING MANUAL -17-
O0005;
G21;
G10 L2 P1 X0. Z165;
N4 G28 U0.V0.
T404;
(TURN);
G50 S2000;
G96 S200 M3;
G0 G40 G54 G99 X69.282 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-
60 counter clockwise direction
G2 X69.282 Z-100 R40; Machine a 40mm radius until point X69.282 Z-
100 clockwise direction
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).
PROGRAMMING MANUAL -18-
Incremental commands (U and W)
O0006;
G21;
G10 L2 P1 X0. Z96:
N5 G28 U0.V0.
T505;
(GROOVE);
G97 S1250 M3;
G0 G40 G54 G99 X78 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.
Example for operation
PROGRAMMING MANUAL -19-
Tools:
T1= Outside and facing.
T2= ø15 twist drill.
T4= Bore.
O0007;
G21;
G10 L2 P1 X0 Z74;
N1 G28 U0.V0.
T101;
(TURN);
G50 S2500;
G96 S220 M3;
G0 G40 G54 G99 X35 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 G54 G99 X0 Z3 M8;
G1 Z-47 F0.1;
G0 Z10 M9;
X150. Z100.;
M1;
External machining
Drill
PROGRAMMING MANUAL -20-
N4 G28 U0.V0.
T404;
(BORE);
G50S2250
G96 S150 M3;
G0 G40 G54 G99 X22 Z3 M8;
G1 Z0 F0.25;
X20 Z-1 F0.15;
Z-13 F0.2;
X15 Z-20 F0.15;
G0 Z5 M9;
X150 Z150;
M30;
Bore
G Code List
For full explanation of the following G codes, refer to the examples in this manual or in the Fanuc
programming manual.
PROGRAMMING MANUAL -21-
STANDARD
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 -22-
STANDARD
G CODE
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
G84 10 CANNED CYCLE FOR FACE TAPPING
G85 10 CANNED CYCLE FOR FACE BORING
G87 10 CANNED CYCLE FOR SIDE DRILLING
G88 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
GROUP FUNCTION
PROGRAMMING MANUAL -23-
M FUNCTIONS
M functions used in machining programs are described in this section, this is a general list for the Kia range,
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
M10 BAR FEEDING ON OPTION
M11 BAR FEEDING OFF OPTION
M12 COUNTER OPTION
M13 MILL SPINDLE FORWARD
M14 MILL SPINDLE REVERSE
M15 MILL SPINDLE STOP
M18 SPINDLE ORIENTATION OFF OPTION
M19 SPINDLE ORIENTATION ON OPTION
M21 ERROR DETECT ON
M22 ERROR DETECT OFF
M23 CHAMFERING ON
M24 CHAMFERING OFF
M30 RESET AND REWIND OPTION
M31 COUNT UP CHECK OPTION
M36 AUTO POWER OFF ENABLE OPTION
M37 AUTO POWER OFF DISABLE OPTION
M38 CENTRE AIR BLOW ON OPTION
M39 CENTRE AIR BLOW OFF OPTION
M40 C-AXIS OFF OR LOW GEAR OPTION
M41 AUTO Q-SETTER ARM DOWN OPTION
M42 AUTO Q-SETTER ARM UP OPTION
M40 C-AXIS OFF OR LOW GEAR OPTION
M43 C-AXIS ON OR HIGH GEAR OPTION
M46 SPINDLE OVERRIDE ENABLE
M47 SPINDLE OVERRIDE DISABLE
M48 FEED OVERRIDE ENABLE
M49 FEED OVERRIDE DISABLE
M51 MAIN SPINDLE AIR BLOW ON OPTION
M52 MAIN SPINDLE AIR BLOW OFF OPTION
M54
M55
M61 AUTO DOOR OPEN OPTION
M62 AUTO DOOR CLOSE OPTION
CONSTANT SPINDLE SPEED CONTROL (MAIN
SPINDLE)
CONSTANT SPINDLE SPEED CONTROL (SUB
SPINDLE)
PROGRAMMING MANUAL -24-
M63 PARTS CATCHER UP OPTION
M64 PARTS CATCHER DOWN OPTION
M66 LOW CHUCK PRESSURE OPTION
M67 HIGH CHUCK PRESSURE OPTION
M68 CHUCK CLOSE
M69 CHUCK OPEN
M70 CALL LIGHT ON
M73 SUB SPINDLE PARTS CATCHER UP
M74 SUB SPINDLE PARTS CATCHER DOWN
M75 CHIP CONVEYOR ON
M76 CHIP CONVEYOR OFF
M81 ROBOT SERVICE REQUEST 1 OPTION
M82 ROBOT SERVICE REQUEST 2 OPTION
M85 NEW BAR FEEDER LOADING OPTION
M90 C-AXIS BRAKE ON (HIGH)
M91 C-AXIS BRAKE OFF (LOW)
M98 SUB PROGRAM CALL
M99 END OF SUB PROGRAM
M108 SUB SPINDLE COOLANT ON
M109 SUB SPINDLE COOLANT OFF
M113 SUB SPINDLE FORWARD
M114 SUB SPINDLE REVERSE
M115 SUB SPINDLE STOP
M116 SUB SPINDLE ORIENTATION ON
M117 SUB SPINDLE ORIENTATION OFF
M118 SUB SPINDLE CHUCK CLAMP
M119 SUB SPINDLE CHUCK UNCLAMP
M114 SUB SPINDLE REVERSE
M115 SUB SPINDLE STOP
M116 SUB SPINDLE ORIENTATION ON
M117 SUB SPINDLE ORIENTATION OFF
M118 SUB SPINDLE CHUCK CLAMP
M119 SUB SPINDLE CHUCK UNCLAMP
M140 A-AXIS OFF
M141 EXTERNAL M CODE 1 OFF
M142 EXTERNAL M CODE 2 ON
M143 A-AXIS ON
M144 EXTERNAL M CODE 3 ON
M145 EXTERNAL M CODE 3 OFF
M146 EXTERNAL M CODE 4 ON
M147 EXTERNAL M CODE 4 OFF
M151 SUB SPINDLE AIR BLOW ON
M152 SUB SPINDLE AIR BLOW OFF
M160 S1, S2 SYNCHRONISATION ON
M161 S1, S2 SYNCHRONISATION OFF
M162 S1, S2 PHASE SYNCHRONISATION ON
THREADING
PROGRAMMING MANUAL -25-
O0008;
G21;
G10 L2 P1 Z95;
N1 G28 U0.V0.
T101;
(TURN);
G50 S2500;
G96 S200 M3;
G0 G40 G54 G99 X70 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;
PROGRAMMING MANUAL -26-
N2 G28 U0.V0.
T202;
(SCREWCUT);
G97 S700 M3;
G0 G40 G54 G99 X60 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.
CANNED CYCLES
G70 Finishing cycle
G70 P100 Q200
P Block number from which the profile operation begins.
Q 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
PROGRAMMING MANUAL -27-
G71 U3 R1
G71 P100 Q200 U0.3 W0.1 F0.25
U Cut depth on radius (mm).
R Retraction in radial direction from diameter to prevent touching the machined diameter (mm).
P Block number from which the profile operation begins.
Q Number of end block of profile.
U Finishing allowance for radius on X-axis (mm).
W Finishing allowance on Z-axis (mm).
F 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 -28-
G72 Cross roughing cycle transversal parallel to X-axis
G72 W3 R1
G72 P100 Q200 U0.25 W0.1 F0.3
W Depth of cut on Z-axis (mm).
R Retraction amount.
P Block number from which the profile operation begins.
Q Number of end block of profile.
U Finishing allowance for radius on X-axis (mm).
W Finishing allowance on Z-axis (mm).
F 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
U Stock allowance (for radius) unmachined on X-axis (mm).
W Stock allowance on Z-axis (mm).
R Number of roughing passes.
P Block number from which the profile operation begins.
Q Number of end block of profile.
U Finishing allowance for radius on X-axis (mm).
W Finishing allowance on Z-axis (mm).
F Instantaneous feed (mm/revolution).
G74 Drilling cycle (chip break)
G74 R0.5
G74 Z-100 Q2500 F0.25
R Retract distance (chip break).
Z Final drilling depth (absolute dimensions in mm).
Q Cut depth per pass (Microns).
F Feed rate (mm/revolution).
G83 Peck drilling cycle
G0 G80 G99 X0 Z3
G83 Z-60 Q2000 F0.2
G80
Z Final drilling depth (absolute dimensions in mm).
R Distance from the initial position to the start point (incremental value, not required if
already in position)
Q Depth of cut (Microns).
P Dwell time (s) at the bottom of the hole.
F Feed rate (mm/revolution).
PROGRAMMING MANUAL -29-
G84 Tapping cycle
Please note that if not using a LM or MS machine, then M122 and M123 can be omitted
G97 S500 M3
G0 G80 G99 X0 Z6
M122 (MAIN SPINDLE RIGID TAP ON)
M129S500 (RIGID TAP ON)
G84 Z-10 F1
G80
M128 (RIGID TAP OFF)
M123 (MAIN SPINDLE RIGID TAP OFF)
Z Final tapping depth (absolute dimensions in mm).
P Dwell time (s) at the bottom of the hole.
F Feed rate (mm/revolution).
G74 Front counter boring cycle
G74 R0.5
G74 X50 Z-4 P3000 Q4000 F0.15
R Retraction (mm) to break chips.
X (U) End position on X-axis (mm).
Z (W) End position in slot direction (mm).
P Step over on X-axis for next pass (Microns)
Q Cutting depth (Microns)
F Feed rate (mm/revolution).
Loading...