nct 990T, 100T User Manual
NCT® 990T
®
NCT
Controls for Lathes
Programmer's Manual
From SW version x.060
100T
Manufactured by NCT Automation kft.
H1148 Budapest Fogarasi út 7
: Address: H1631 Bp. pf.: 26
F Phone: (+36 1) 467 63 00
F Fax:(+36 1) 363 6605
E-mail: nct@nct.hu
Home Page: www.nct.hu
Contents
1 Introduction ............................................................. 9
1.1 The Part Program ..................................................... 9
Word ............................................................... 9
Address Chain ........................................................ 9
Block .............................................................. 10
Program Number and Program Name ..................................... 10
Beginning of Program, End of Program ................................... 10
Program Format in the Memory ......................................... 10
Program Format in Communications with External Devices ................... 10
Main Program and Subprogram ......................................... 10
DNC Channel ....................................................... 11
1.2 Fundamental Terms .................................................. 12
2 Controlled Axes ......................................................... 16
2.1 Names of Axes ......................................................16
2.2 Unit and Increment System of Axes ...................................... 16
3 Preparatory Functions (G codes) ........................................... 18
4 The Interpolation ........................................................ 22
4.1 Positioning (G00) .................................................... 22
4.2 Linear Interpolation (G01) .............................................22
4.3 Circular and Spiral Interpolation (G02, G03) ............................... 24
4.4 Equal Lead Thread Cutting (G33) ....................................... 28
4.5 Variable-Lead Thread Cutting (G34) ..................................... 29
4.6 Polar Coordinate Interpolation (G12.1, G13.1) ............................. 30
4.7 Cylindrical Interpolation (G7.1) ......................................... 34
5 The Coordinate Data ..................................................... 36
5.1 Absolute and Incremental Programming (G90, G91), Operator I ................ 36
5.2 Inch/Metric Conversion (G20, G21) ...................................... 36
5.3 Specification and Value Range of Coordinate Data .......................... 37
5.4 Programming in Radius or Diameter ..................................... 38
5.5 Rotary Axis Roll-over ................................................. 39
6 The Feed ............................................................... 42
6.1 Feed in Rapid Traverse ................................................ 42
6.2 Cutting Feed Rate .................................................... 42
6.2.1 Feed per Minute (G94) and Feed per Revolution (G95) .................. 43
6.2.2 Clamping the Cutting Feed ........................................ 44
6.3 Acceleration/Deceleration. Taking F Feed into Account ...................... 45
6.4 Feed Control Functions ................................................ 47
6.4.1 Exact Stop (G09) ................................................ 47
6.4.2 Exact Stop Mode (G61) ........................................... 47
6.4.3 Continuous Cutting Mode (G64) .................................... 47
6.4.4 Override and Stop Inhibit (Tapping) Mode (G63) ...................... 47
3
6.4.5 Automatic Corner Override (G62) ................................... 48
6.4.6 Internal Circular Cutting Override ................................... 49
6.5 Automatic Deceleration at Corners ...................................... 49
6.6 Limiting Accelerations in Normal Direction along the Path in Case of Circular Arcs
.................................................................. 52
7 The Dwell (G04) ........................................................ 53
8 The Reference Point ..................................................... 54
8.1 Automatic Reference Point Return (G28) ................................. 54
8.2 Automatic Return to Reference Points 2, 3, 4 (G30) ........................ 55
8.3 Automatic Return from the Reference Point (G29) .......................... 55
9 Coordinate Systems, Plane Selection ........................................ 57
9.1 The Machine Coordinate System ........................................ 57
9.1.1 Setting the Machine Coordinate System .............................. 57
9.1.2 Positioning in the Machine Coordinate System (G53) ................... 58
9.2 Work Coordinate Systems ............................................. 58
9.2.1 Setting the Work Coordinate Systems ................................ 58
9.2.2 Selecting the Work Coordinate System ............................... 59
9.2.3 Programmed Setting of the Work Zero Point Offset ..................... 60
9.2.4 Creating a New Work Coordinate System (G92) ....................... 61
9.3 Local Coordinate System .............................................. 62
9.4 Plane Selection (G17, G18, G19) ........................................ 63
10 The Spindle Function ................................................... 65
10.1 Spindle Speed Command (Code S) ..................................... 65
10.2 Programming of Constant Surface Speed Control .......................... 65
10.2.1 Constant Surface Speed Control Command (G96, G97) ................. 66
10.2.2 Constant Surface Speed Clamp (G92) ............................... 66
10.2.3 Selecting an Axis for Constant Surface Speed Control .................. 67
10.3 Spindle Position Feedback ............................................ 67
10.4 Oriented Spindle Stop ............................................... 67
10.5 Spindle Positioning (Indexing) ......................................... 68
10.6 Spindle Speed Fluctuation Detection (G25, G26) .......................... 68
11 Tool Function ......................................................... 71
12 Miscellaneous and Auxiliary Functions .................................... 72
12.1 Miscellaneous Functions (Codes M) .................................... 72
12.2 Auxiliary Function (Codes A, B, C) ..................................... 73
12.3 Sequence of Execution of Various Functions ............................. 73
13 Part Program Configuration ............................................. 74
13.1 Sequence Number (Address N) ........................................ 74
13.2 Conditional Block Skip .............................................. 74
13.3 Main Program and Subprogram ........................................ 74
13.3.1 Calling the Subprogram .......................................... 74
13.3.2 Return from a Subprogram ....................................... 75
4
13.3.3 Jump within the Main Program .................................... 77
14 The Tool Compensation ................................................. 78
14.1 Reference to Tool Offset .............................................. 78
14.2 Modification of Tool Offset Values from the Program (G10) . ................ 82
14.3 Taking the Tool Length Offset into Account .............................. 82
14.4 Tool Nose Radius Compensation (G38, G39, G40, G41, G42) . . . ............. 84
14.4.1 Start up of Tool Nose Radius Compensation .......................... 88
14.4.2 Rules of Tool Nose Radius Compensation in Offset Mode . . . ............ 92
14.4.3 Canceling of Offset Mode ........................................ 95
14.4.4 Change of Offset Direction While in the Offset Mode .................. 98
14.4.5 Programming Vector Hold (G38) ................................. 100
14.4.6 Programming Corner Arcs (G39) .................................. 100
14.4.7 General Information on Tool Nose Radius Compensation .............. 102
14.4.8 Interferences in Tool Nose Radius Compensation ..................... 107
15 Special Transformations ................................................ 112
15.1 Mirror Image for Double Turret (G68) .................................. 112
15.2 Scaling (G50, G51) ................................................. 113
15.3 Programmable Mirror Image (G50.1, G51.1) ............................. 113
16 Automatic Geometric Calculations ....................................... 115
16.1 Programming Chamfer and Corner Round ............................... 115
16.2 Specifying Straight Line with Angle .................................... 116
16.3 Intersection Calculations in the Selected Plane ........................... 118
16.3.1 Linear-linear Intersection ........................................ 118
16.3.2 Linear-circular Intersection ...................................... 120
16.3.3 Circular-linear Intersection....................................... 122
16.3.4 Circular-circular Intersection ..................................... 124
16.3.5 Chaining of Intersection Calculations .............................. 126
17 Canned Cycles for Turning ............................................. 127
17.1 Single Cycles ..................................................... 127
17.1.1 Cutting Cycle (G77) ............................................ 127
17.1.2 Thread Cutting Cycle (G78) ...................................... 129
17.1.3 End Face Cutting Cycle (G79) .................................... 131
17.1.4 Single Cycle Application ........................................ 133
17.2 Multiple Repetitive Cycles ........................................... 134
17.2.1 Stock Removal in Turning (G71) .................................. 134
17.2.2 Stock Removal in Facing (G72) ................................... 139
17.2.3 Pattern Repeating Cycle (G73) .................................... 141
17.2.4 Finishing Cycle (G70) .......................................... 143
17.2.5 End Face Peck Drilling Cycle (G74) ............................... 144
17.2.6 Outer Diameter/Internal Diameter Drilling Cycle (G75) ................ 146
17.2.7 Multiple Thread Cutting Cycle (G76) .............................. 148
18 Canned Cycles for Drilling .............................................. 154
18.1 Detailed Description of Canned Cycles ................................. 160
18.1.1 High Speed Peck Drilling Cycle (G83.1) ............................ 160
5
18.1.2 Counter Tapping Cycle (G84.1) .................................. 161
18.1.3 Fine Boring Cycle (G86.1) ...................................... 162
18.1.4 Canned Cycle for Drilling Cancel (G80) ............................ 163
18.1.5 Drilling, Spot Boring Cycle (G81) ................................ 163
18.1.6 Drilling, Counter Boring Cycle (G82) .............................. 164
18.1.7 Peck Drilling Cycle (G83) ....................................... 165
18.1.8 Tapping Cycle (G84) ........................................... 166
18.1.9 Rigid (Clockwise and Counter-clockwise) Tap Cycles (G84.2, G84.3) .... 167
18.1.10 Boring Cycle (G85) ........................................... 170
18.1.11 Boring Cycle Tool Retraction with Rapid Traverse (G86) . ............ 171
18.1.12 Boring Cycle/Back Boring Cycle (G87) ........................... 172
18.1.13 Boring Cycle (Manual Operation on the Bottom Point) (G88) .......... 174
18.1.14 Boring Cycle (Dwell on the Bottom Point, Retraction with Feed) (G89) . . 175
18.2 Notes to the Use of Canned Cycles for Drilling ........................... 175
19 Polygonal Turning .................................................... 177
19.1 Principle of Polygonal Turning ....................................... 177
19.2 Programming Polygonal Turning (G51.2, G50.2) ......................... 178
20 Measurement Functions ................................................ 180
20.1 Skip Function (G31) ................................................ 180
20.2 Automatic Tool Length Measurement (G36, G37) ........................ 181
21 Safety Functions ...................................................... 183
21.1 Programmable Stroke Check (G22, G23) ............................... 183
21.2 Parametric Overtravel Positions ....................................... 184
21.3 Stroke Check Before Movement ...................................... 184
22 Custom Macro ........................................................ 186
22.1 The Simple Macro Call (G65) ........................................ 186
22.2 The Macro Modal Call .............................................. 187
22.2.1 Macro Modal Call in Every Motion Command (G66) ................. 187
22.2.2 Macro Modal Call From Each Block (G66.1) ........................ 188
22.3 Custom Macro Call Using G Code .................................... 189
22.4 Custom Macro Call Using M Code .................................... 189
22.5 Subprogram Call with M Code ....................................... 190
22.6 Subprogram Call with T Code ........................................ 191
22.7 Subprogram Call with S Code ........................................ 191
22.8 Subprogram Call with A, B, C Codes .................................. 191
22.9 Differences Between the Call of a Subprogram and the Call of a Macro ....... 192
22.9.1 Multiple Calls ................................................ 192
22.10 Format of Custom Macro Body ...................................... 193
22.11 Variables of the Programming Language ............................... 194
22.11.1 Identification of a Variable ..................................... 194
22.11.2 Referring to a Variable ........................................ 194
22.11.3 Vacant Variables ............................................. 195
22.11.4 Numerical Format of Variables .................................. 195
22.12 Types of Variables ................................................ 196
22.12.1 Local Variables .............................................. 196
6
22.12.2 Common Variables ........................................... 196
22.12.3 System Variables ............................................. 197
22.13 Instructions of the Programming Language ............................. 206
22.13.1 Definition, Substitution ........................................ 206
22.13.2 Arithmetic Operations and Functions ............................. 206
22.13.3 Logical Operations ............................................ 210
22.13.4 Unconditional Divergence ...................................... 210
22.13.5 Conditional Divergence ........................................ 210
22.13.6 Conditional Instruction ......................................... 210
22.13.7 Iteration .................................................... 211
22.13.8 Data Output Commands ........................................ 213
22.14 NC and Macro Instructions .......................................... 217
22.15 Execution of NC and Macro Instructions in Time ........................ 217
22.16 Displaying Macros and Subprograms in Automatic Mode .................. 218
22.17 Using the STOP Button While a Macro Instruction is Being Executed ........ 218
Notes ................................................................... 219
Index in Alphabetical Order ............................................... 220
October 15, 2004
7
© Copyright NCT October 15, 2004
The Publisher reserves all rights for contents
of this Manual. No reprinting, even in extracts, is permissible unless our written consent is obtained.
The text of this Manual has been compiled
and checked with utmost care, yet we assume no liability for possible errors or spurious data and for consequential losses or damages.
8
1 Introduction
1 Introduction
1.1 The Part Program
The Part Program is a set of instructions that can be interpreted by the control system in order to
control the operation of the machine.
The Part Program consists of blocks which, in turn, comprise words.
Word: Address and Data
Each word is made up of two parts - an address and a data. The address has one or more characters, the data is a numerical value (an integer or decimal value). Some addresses may be given a
sign or operator I.
Address Chain:
Address Meaning Value limits
O program number 0001 - 9999
/ optional block 1 - 9
N block number 1 - 99999
G preparatory function *
X, Y, Z, U, V ,W length coordinates I, -, *
A, B, C, H angular coordinates, auxiliary functions I, -, *
R circle radius, auxiliary data I, -, *
I, J, K circle center coordinates, auxiliary coordinate -, *
E auxiliary coordinate -, *
F feed rate *
S spindle speed *
M miscellaneous function 1 - 999
T tool number 1 - 9999
L repetition number 1 - 9999
P auxiliary data, dwell time -, *
Q auxiliary data -, *
,C distance of chamfer -, *
,R radius of fillet -, *
,A angle of straight line -, *
( comment *
At an address marked with a * in the Value Limits column, the data may have a decimal value
as well.
At an address marked with I and –, an incremental operator or a sign can be assigned, respectiv-
ely.
The positive sign + is not indicated and not stored.
9
1 Introduction
Block
A block is made up of words.
The blocks are separated by characters s (Line Feed) in the memory. The use of a block number
is not mandatory in the blocks. To distinguish the end of block from the beginning of another
block on the screen, each new block begins in a new line, with a character > placed in front of it,
in the case of a block longer than a line, the words in each new line are begun with an indent of
one character.
Program Number and Program Name
The program number and the program name are used for the identification of a program. The use
of program number is mandatory that of a program name is not.
The address of a program number is O. It must be followed by exactly four digits.
The program name is any arbitrary character sequence (string) put between opening "(" and clo-
sing brackets ")". It may have max. 16 characters.
The program number and the program name are separated by characters s (Line Feed) from the
other program blocks in the memory.
In the course of editing, the program number and the program name will be displayed invariably
in the first line.
There may be not two programs of a given program number in the backing store.
Beginning of Program, End of Program
Each program begins and ends with characters %. In the course of part program editing the program-terminating character is placed invariably behind the last block in order to ensure that the
terminated locks will be preserved even in the event of a power failure during editing.
Program Format in the Memory
The program stored in the memory is a set of ASCII characters.
The format of the program is
%O1234(PROGRAM NAME)s/1N12345G1X0Y...sG2Z5...s....s
...s
...s
N1G40...M2s
%
In the above sequence of characters,
s is character "Line Feed",
% is the beginning (and end) of the program.
Program Format in Communications with External Devices
The above program is applicable also in communications with an external device.
Main Program and Subprogram
The part programs may be divided into two main groups -
main programs, and
subprograms.
The procedure of machining a part is described in the main program. If, in the course of machining repeated patterns have to be machined at different places, it is not necessary to write those
program-sections over and over again in the main program, instead, a subprogram has to be organized, which can be called from any place (even from another subprogram). The user can return
from the subprogram to the calling program.
10
1 Introduction
DNC Channel
A program contained in an external unit (e.g., in a computer) can also be executed without storing
it in the control's memory. Now the control will read the program, instead of the memory, from
the external data medium through the RS232C interface. That link is referred to as "DNC channel". This method is particularly useful for the execution of programs too large to be contained
in the control's memory.
The DNC channel is a protocol-controlled data transfer channel as shown below.
Controller:
Equipment:
<
BEL > DC1 NAK/ACK DC3
ACK > BLOCK
<
The above mnemonics have the following meanings (and their ASCII codes):
BEL (7): The control requests the sender to establish the communication. The control is-
sues L again unless ACK is returned in a definite length of time.
ACK (6): Acknowledgment.
NAK (21): Spurious data transfer (e.g. hardware trouble in the line or BCC error). The
transfer of BLOCK has to be repeated.
DC1 (17): Transfer of the next BLOCK has to be started.
DC3 (19): Interruption of communication.
BLOCK:
– Basically an NC block (including the terminating character s) and the check-
sum thereof (BCC) stored in 7 bits as the last byte of the block (bit 7, the
uppermost one, of BCC is invariably 0). No SPACE (32) or some other
character of lower ASCII code may be contained in the block.
– EOF (26) (End Of File), a signal is transferred by the Equipment ("sender") to
interrupt the communication.
For the DNC mode, set the second physical channel (only that one is applicable as a DNC channel) for 8-bit even-parity mode.
A main program executed from the DNC channel may have a linear sequence only. This does not
apply to subprogram or macro (if any have been called) however, they must be contained in the
memory of control. In the event of a departure from the linear sequence in the main program (GOTO, DO WHILE), the control will return error message 3058 NOT IN DNC. If the control detects
a BLOCK error and returns NAK, the BLOCK has to be repeated.
11
1 Introduction
1.2 Fundamental Terms
The Interpolation
The control system can move the tool along straight lines
and arcs in the course of machining. These activities will
be hereafter referred to as "interpolation".
Tool movement along a straight line:
Program:
G01 Z__
X__ Z__
Tool movement along an arc:
Fig. 1.2-1
Program:
G02 X__ Z__ R__
Fig. 1.2-2
Preparatory Functions (G codes)
The type of activity to be performed by a block is described with the use of preparatory functions
(also referred to as G codes). E.g., code G01 introduces a linear interpolation.
Feed
The term "feed" refers to the speed of the tool relative to
the workpiece during the process of cutting. The desired
feed can be specified in the program at address F and with
a numerical value. For example F2 means 2 mm/rev.
12
Fig. 1.2-3
1 Introduction
Reference Point
The reference point is a fixed point on the machine-tool. After power-on of the machine, the
slides have to be moved to the reference point. Afterwards the control system will be able to interpret data of absolute coordinates as well.
Coordinate System
The dimensions indicated in the part drawing are measured
from a given point of the part. That point is the origin of
the workpiece coordinate system. Those dimensional data
have to be written at the coordinate address in the part program. E.g., X150 Z–100 means a coordinate point of 340
and –100 mm in the coordinate system of the workpiece in
the direction X and Z respectively.
The coordinate system in which the control interprets the
positions, is different from the coordinate system of the
workpiece. For the control system to make a correct workpiece, the zero point offsets of the two coordinate systems
have to be set. This can be achieved, e.g., by moving the
tool tip to a point of a known position of the part and set-
Fig. 1.2-4
ting the coordinate system of the control to that value.
Absolute Coordinate Specification
When absolute coordinates are specified, the tool travels a
distance measured from the origin of the coordinate system, i.e., to a point whose position has been specified by
the coordinates.
The code of absolute data specification is G90.
The block
G90 X200 Z150
will move the tool to a point of the above position, irrespective of its position before the command has been issued.
Fig. 1.2-5
13
1 Introduction
Incremental Coordinate Specification
In the case of an incremental data specification, the control
system will interpret the coordinate data in such a way that
the tool will travel a distance measured from its instantaneous position:
U–50 W–125
The code of incremental data specification is G91. Code
G91 refers to all coordinate values.
The specification above is equivalent to the block below:
G91 X–50 Z-125
It will move the tool over the above distance from its previous position.
Fig. 1.2-6
Diameter Programming
The coordinate X may be specified both in diameter or in radius depending on parameter.
Modal Functions
Some codes are effective until another code or value is specified. These are modal codes. E.g.,
in program detail
N15 G90 G1 X20 Z30 F0.2
N16 X30
N17 Z100
the code of G90 (absolute data specification) and the value of F (Feed), specified in block N15,
will be modal in blocks N16 and N17. Thus it is not necessary to specify those functions in each
block followed.
One-shot (Non-modal) Functions
Some codes or values are effective only in the block in which they are specified. These are oneshot functions.
Spindle Speed Command
The spindle speed can be specified at address S. It is also termed as "S function". Instruction
S1500 tells the spindle to rotate at a speed of 1500 rpm.
Constant Surface Speed Control
The control changes the spindle speed according to the diameter machined the way that the speed
of the tool tip relative to the surface of the workpiece to be constant. This function is the constant
surface speed control.
Tool Function
In the course of machining different tools have to be employed for the various cutting operations.
The tools are differentiated by numbers. Reference can be made to the tools with code T. The first
two digits of the T code refer to the tool number (that is in which position in turret it can be
found), while the second two digits refer to the code of offset compensation. Instruction
T0212
in the program means that tool No. 2 has to be changed and the offset compensation group No.
12 is to be applied.
14
1 Introduction
Miscellaneous Functions
A number of switching operations have to be carried out in the course of machining. For example,
starting the spindle, turning on the coolant. Those operations can be performed with M (miscellaneous) functions. E.g., in the series of instructions
M3 M8
M3 means “rotate the spindle clockwise”, M8 means "turn on the coolant".
Tool Length Compensation
In the course of machining, tools of different
length are employed for the various operations.
On the other hand, a given operation also has
to be performed with tools of different lengths
in series production (e.g., when the tool
breaks). In order to make the motions described in the part program independent of the
length of the tool, the various tool lengths must
be set in control system. If the program is intended to move the tip of the tool to the specified point, the value of the particular length data has to be called. This is feasible at the second two digits of the T code. Henceforth the
control will move the tip of the tool to the spe-
Fig. 1.2-7
cified point.
Tool Nose Radius Compensation
When machining a workpiece and the tool does not move
parallel to one of the axes exact size can be achieved only
if not the tool tip is moved on the programmed path but the
tool nose center parallel to it and with the distance of r. Radius compensation has to be introduced in order to write
the actual contour data of the part in the program, instead
of the path covered by the tool tip . The values of radius
compensations have to be set in control system. Hereinafter
reference can be made to tool nose radius compensations
at address T in the program.
Fig. 1.2-8
15
2 Controlled Axes
2 Controlled Axes
Number of Axes (in basic configuration) 2 axes
In expanded configuration 6 additional axes (8 axes altogether)
Number of axes to be moved simultaneously 8 axes (with linear interpolation)
2.1 Names of Axes
The names of controlled axes can be defined in the parameter memory. Each address can be assigned to one of the physical axes.
In the basic configuration, the names of
axes: X and Z.
The names of additional (expansion) axes
depend on their respective types.
Possible names of expansion axes performing linear motions are: Y, U, V and W.
When U, V, W axes are parallel to the
main axes X,Y and Z, their name will be
U,V and W, respectively.
Axes performing rotational motions are
termed A, B and C. The rotational axes
whose axle of rotation parallel to X, Y and
Z directions are termed A, B and C, respectively.
The name of the spindle axis in case of
polar or cylindrical coordinate interpolation is used: C.
In case U, V or W axis cannot be found in
the machine at the above addresses incremental movements can be specified for the
axes X, Y, Z respectively. Address H can
be used for specifying incremental movement for C.
Fig. 2.1-1
2.2 Unit and Increment System of Axes
The coordinate data can be specified in 8 digits. They can have signs, too. The positive sign + is
omitted.
The data of input length coordinates can be specified in mm or inches. They are the units of input
measures. The desired one can be selected from the program.
The path-measuring device provided on the machine can measure the position in mm or in inches.
It will determine the output unit of measures, which has to be specified by the control system as
a parameter. The two units of measures may not be combined among axes on a given machine.
In the case of different input and output units of measures, the control system will automatically
16
2 Controlled Axes
perform the conversion.
The rotational axes are always provided with degrees as units of measure.
The input increment system of the control is regarded as the smallest unit to be entered. It can
be selected as parameter. There are three increment systems available IS-A, IS-B and IS-C. The
increment systems may not be combined for the axes on a given machine.
Having processed the input data, the control system will provide new path data for moving the
axes. Their resolution is always twice the particular input increment system. It is termed the
output increment system of the control.
Thus the input increment system of the control is determined by the resolution of the encoder.
Increment system Min. unit to be entered Max. unit to be entered
0.01 mm 999999.99 mm
IS-A
IS-B
IS-C
0.001 inch 99999.999 inch
0.01 degree 999999.99 degree
0.001 mm 99999.999 mm
0.0001 inch 9999.9999 inch
0.001 degree 99999.999 degree
0.0001 mm 9999.9999 mm
0.00001 inch 999.99999 inch
0.0001 degree 9999.9999 degree
Coordinate data of X axis can also be interpreted by the control in diameter, provided parameter
4762 DIAM is 1. In this case the value limits defined in the above table are interpreted in diameter with their value remaining so.
17
3 Preparatory Functions (G codes)
3 Preparatory Functions (G codes)
The type of command in the given block will be determined by address G and the number following it.
The Table below contains the G codes interpreted by the control system, the groups and functions
thereof.
G code
G00
G01
Group
*
*
Positioning 22
Linear interpolation 22
Function
Page
01
G02 Circular interpolation, clockwise (CW) 24
G03 Circular interpolation, counter-clockwise (CCW) 24
G04
Dwell 53
G05.1 Multi-buffer mode on
G07.1 Cylindrical interpolation 34
00
G09 Exact stop (in the given block) 47
G10 Data setting (programmed)
60, 78,
82
G11 Programmed data setting cancel
G12.1
Polar coordinate interpolation on 30
26
G13.1 Polarc coordinate interpolation off 30
G17
G18
*
*
Selection of X
02
Selection of ZpXp plane 63
plane 63
pYp
G19 Selection of YpZp plane 63
G20
Inch input 36
06
G21 Metric input 36
G22
*
Programable stroke check function on 183
04
G23 Programable stroke check function off 183
G25
*
Spindle speed fluctuation detection off 68
08
G26 Spindle speed fluctuation detection on 68
G28
Programmed reference-point return 54
G29 Return from reference point 55
00
G30 Return to the 1st, 2nd, 3rd and 4th reference point 55
G31 Skip function 180
G33
Thread cutting 28
01
G34 Variable-lead thread cutting 29
G36
Automatic tool-length measurement X 181
G37 Automatic tool-length measurement Z 181
00
G38 Tool nose radius compensation vector hold 100
G39 Tool nose radius compensation corner arc 100
18
3 Preparatory Functions (G codes)
G code
*
G40
G41 Tool nose radius compensation left
Group
Tool nose radius compensation cancel
07
G42 Tool nose radius compensation right
G50
*
Scaling cancel 113
Function
Page
84
84, 84,
88
84, 84,
88
11
G51 Scaling 113
G50.1
*
Programable mirror image cancel 113
18
G51.1 Programable mirror image 113
G51.2
Polygonal turning on 178
20
G50.2 Polygonal turning off 178
G52
Local coordinate system setting 62
00
G53 Positioning in the machine coordinate system 58
G54
*
Work coordinate system 1 selection 59
G55 Work coordinate system 2 selection 59
G56 Work coordinate system 3 selection 59
14
G57 Work coordinate system 4 selection 59
G58 Work coordinate system 5 selection 59
G59 Work coordinate system 6 selection 59
G61
Exact stop mode 47
G62 Automatic corner override mode 48
15
G63 Override inhibit 47
*
G64
Continuous cutting 47
G65 Simple macro call 186
G66 Macro modal call (A) in every motion command 187
G66.1 Macro modal (B) call from each block 188
G67 Macro modal call (A/B) cancel 187
G68
G69
*
Mirror image for double turret on 112
16
Mirror image for double turret off 112
G70 00 Finishing cycle 143
G71 Stock removal in turning cycle 134
G72 Stock removal in facing cycle 139
G73 Pattern repeating cycle 141
G74 End face peck drilling cycle 144
G75 Outer diameter/internal diameter drilling cycle 146
G76 Multiple thread cutting cycle 148
G77 01 Cutting cycle 127
G78 Thread cutting cycle 129
19
3 Preparatory Functions (G codes)
G code
Group
Function
Page
G79 End face turning cycle 131
*
G80
09 Canned cycle for drilling cancel 163
G81 Drilling, spot boring cycle, 163
G82 Drilling, counter boring cycle 164
G83 Peck drilling cycle 165
G83.1 High Speed Peck Drilling Cycle 160
G84 Tapping cycle 166
G84.1 Counter tapping cycle 161
G84.2 Rigid tap cycle 167
G84.3 Rigid counter tap cycle 167
G85 Boring cycle 170
G86 Boring Cycle Tool Retraction with Rapid Traverse 171
G86.1 Fine boring cycle 162
G87 Boring Cycle/Back Boring Cycle 172
G88 Boring Cycle (Manual Operation on the Bottom Point) 174
G89 Boring Cycle (Dwell on the Bottom Point, Retraction with Feed) 175
G90
G91
*
*
Absolute command 36
03
Incremental command 36
G92 00 Work coordinates change/maximum spindle speed setting 61
G94
G95
G96
G97
G98
*
*
*
*
Feed per minute 43
05
Feed per revolution 43
Constant surface speed control 66
13
Constant surface speed control cancel 66
Canned cycle initial level return 155
10
G99 Canned cycle R point level return 155
L Notes:
– The * marked G codes in a group represent the state assumed by the control system after
power-on.
– If several codes are marked with * in a group, a parameter can be set to select the effective one
after power-on. They are : G00, G01; G17, G18; G43, G44, G49; G90, G91; G94, G95.
– At the time of power-on, the particular one of G20 and G21 will be effective, that has been set
at the time of power-off.
– Default interpretation of command G05.1 after power-on can be specified with the MULBUF
parameter.
– G codes in group 00 are not modal ones; the rest are so.
– More than one G code can be written in a block with the restriction that only one of the same
function group may used.
– Reference to an illegal G code or specification of several G codes belonging to the same group
20
3 Preparatory Functions (G codes)
within a particular block will produce error message 3005 ILLEGAL G CODE.
21
4 The Interpolation
4 The Interpolation
4.1 Positioning (G00)
The series of instructions
G00 v
refers to a positioning in the current coordinate system.
It moves to the coordinate v. Designation v (vector) refers here (and hereinafter) to all controlled
axes used on the machine-tool. (They may be X, Y, Z, U, V, W, A, B, C) E.g.:
G00 X(U)__ Z(W)__
where X, Z refer to absolute movement, while U, W refer to incremental one (provided U, W are
not selected for axis).
The positioning is accomplished along a straight line involving the simultaneous movements of
all axes specified in the block. The coordinates may be absolute or incremental data.
The speed of positioning cannot be commanded
in the program because it is accomplished with
different values for each axis, set by the builder of
machine-tool as a parameter. When several axes
are being moved at a time, the vectorial resultant
of speed is computed by the control system in
such a way that positioning is completed in a minimum interval of time, and the speed will not exceed anywhere the rapid traverse parameter set for
each axis.
In executing the G00 instruction, the control system performs acceleration and declaration in starting and ending the movements, respectively. On
completion of the movement, the control will check the "in position" signal when parameter POS-
CHECK in the field of parameters is 1, or will not do so when the parameter is set to 0. It will
wait for the "in position" signal for 5 seconds, unless the signal arrives, the control will return the
1020 POSITION ERROR message. The maximum acceptable deviation from the position can be
specified in parameter INPOS.
Being a modal code, G00 remains effective until it is re-written by another interpolation command. After power-on, G00 or G01 is effective, depending on the value set in parameter group
CODES.
Fig. 4.1-1
4.2 Linear Interpolation (G01)
The series of instructions
G01 v F
will select a linear interpolation mode. The data written for v may be absolute or incremental
values, interpreted in the current coordinate system. The speed of motion (the feed) can be programmed at address F.
The feed programmed at address F will be accomplished invariably along the programmed path.
Its axial components:
22
Feed along the axis X is
Feed along the axis Z is
where x, z are the displacements programmed along
the respective axes, L is the vectorial length of programmed displacement:
Fig. 4.2-1
G01 X192 Z120 F0.15
The feed along a rotational axis is interpreted in units of
degrees per minute (°/min):
G01 C270 F120
In the above block, F120 means 120deg/minute.
If the motion of a linear and a rotary axis is combined
through linear interpolation, the feed components will be
distributed according to the above formula. E.g. in block
4 The Interpolation
G91 G01 Z100 C45 F120
Fig. 4.2-2
feed components in Z and B directions are:
Feed along axis Z: mm/min
Feed along axis C: °/min
Being a modal code, G01 is effective until rewritten by another interpolation command. After
power-on, G00 or G01 is effective, depending on the parameter value set in group CODES of the
parameter field.
23
4 The Interpolation
4.3 Circular and Spiral Interpolation (G02, G03)
The series of instructions specify circular interpolation.
A circular interpolation is accomplished in the plane selected by commands G17, G18, G19 in
clockwise or counter-clockwise direction (with G02 or G03, respectively).
Fig. 4.3-1
The above figure shows clockwise (G02) and
counter clockwise (G03) circular directions in
plane G18 when the plane is viewed in the positive-to-negative direction of axis Y. If the
plane is viewed in the negative-to-positive direction of axis Y the interpretation of circular
directions is reversed owing to tool turret arrangements.
Fig. 4.3-2
24
4 The Interpolation
Here and hereinafter, the meanings of Xp, Yp, and Zp are:
Xp: Axis X or its parallel axis,
Yp: Axis Y or its parallel axis,
Zp: Axis Z or its parallel axis.
The values of Xp, Yp, and Zp are the end-point coordinates of the circle in the given coordinate
system, specified as absolute or incremental data.
Further data of the circle may be specified in one of two different ways.
Case 1
At address R where R is the radius of the circle. Now
the control will automatically calculate the coordinates
of the circle center from the start point coordinates (the
point where the control is in the instant of the circle
block being entered), the end point coordinates (values
defined at addresses Xp, Yp, Zp) and from the programmed circle radius R. Since two different circles of radius
R can be drawn between the start and the end points for
a given direction of circumventing (G02 or G03), the
control will interpolate an arc smaller or larger than
180° when the radius of the circle is specified as a positive or a negative number, respectively. For example:
Fig. 4.3-3
Arc section 1: G02 X80 Z50 R40
Arc section 2: G02 X80 Z50 R-40
Arc section 3: G03 X80 Z50 R40
Arc section 4: G03 X80 Z50 R-40
Case 2
The circle center is specified at address I, J, K for the Xp, Yp and Zp axes. The values specified
at addresses I, J, K are interpreted always incrementally by the control system, so that the vector
defined by the values of I, J, K points from the start point to the center of the circle. Value I must
always be specified in radius even if X coordinate is set to diameter. For example:
With G17: G03 X10 Y70 I-50 J-20 (X programmed in radius)
With G18: G03 X70 Z10 I-20 K-50 (X programmed in radius)
With G19: G03 Y10 Z70 J-50 K-20
Fig. 4.3-4
25
4 The Interpolation
The feed along the path can be programmed at address F,
pointing in the direction of the circle tangent, and being
constant all along the path.
L Notes:
– I0, J0, K0 may be omitted, e.g.
G03 X0 Z100 I-100
– When each of Xp, Yp and Zp is omitted, or the end point
coordinate coincides with the start point coordinate, then:
a. If the coordinates of the circle center are pro-
grammed at addresses, I, J, K the control
will interpolate a complete circle of 360°.
E.g.:
G03 I-100,
Fig. 4.3-5
b. If radius R is programmed, the control returns error 3012 ERRONEOUS CIRCLE DEF.
R.
– When the circle block
a. does not contain radius (R) or I, J, K either,
b. or reference is made to address I, J, K outside the selected plane, the control returns
3014 ERRONEOUS CIRCLE DEF. error. E.g. G03 X0 Y100, or (G18) G02 X0
Z100 J-100.
– The control returns error message 3011 RADIUS DIFFERENCE whenever the difference bet-
ween the start-point and end-point radii of the circle defined in block G02, G03 exceeds
the value defined in parameter RADDIF.
Whenever the difference of radii is
smaller than the value specified in
the above parameter, the control
will move the tool along a spiral
path in which the radius is varying
linearly with the central angle.
The angular velocity, not the one
tangential to the path will be constant in the interpolation of a circle
arc of a varying radius.
Fig. 4.3-6
The program detail below is an example of how a spiral interpolation (circle of varying radius) can be specified by
the use of addresses I, K.
G90 G0 X0 Z50
G3 Z-20 K-50
Fig. 4.3-7
26
If the specified circle radius is smaller than half the distance of straight line inter-connecting the start point with the
end point, the control will regard the specified radius of the
circle as the start-point radius, and will interpolate a circle
of a varying radius (spiral), whose center point is located
on the straight line connecting the start point with the end
point, at distance R from the start point.
G0 G90 X0 Z0
G2 X60 Z40 R10
In the following sample blocks X coordinate is in diameter
and U and W are assumed not to be selected for axis:
G2 G90 X100 Z40 R41.2
or G2 G90 X100 Z40 I40 J10
or G2 G91 X60 Z30 R41.2
or G2 (G90) U60 W30 R41.2
or G2 (G90) XI60 ZI30 R41.2
or G2 G91 X60 Z30 I40 J10
or G2 (G90) U60 W30 I40 J10
or G2 (G90) XI60 ZI30 I40 J10
4 The Interpolation
Fig. 4.3-8
Fig. 4.3-9
27
4 The Interpolation
4.4 Equal Lead Thread Cutting (G33)
The instruction
G33 v F Q
G33 v E Q
will define a straight or taper thread cutting of equal lead.
The coordinates of maximum two axes can be written for vector v. The control will cut a tapered
thread if two coordinated data are assigned to
vector v. The control will take the lead into
consideration along the long axis.
If "<45°, i.e. Z>X, the programmed lead will
be taken into account along axis Z,
if ">45°, i.e. X>Z, the control will take the
programmed lead along axis X.
The lead can be defined in one of two 2 ways.
– If the lead is specified at address F, the data
will be interpreted in mm/rev or
inch/rev. Accordingly, F2.5 has to be
programmed if a thread of 2.5 mm lead
Fig. 4.4-1
is to be cut.
– If the pitch is specified at address E, the control will cut an inch thread. Address E is interpre-
ted as number of ridges per inch. If, e.g., E3 is programmed, the control will cut a thread
a"=25.4/3=8.4667mm lead.
The shift angle of the thread start is specified at address Q expressed in degrees from the zero
pulse of the spindle encoder. A multiple thread can be cut by an adequate programming of the
value of Q, i.e., the control can be programmed here for the particular angular displacements of
the spindle, at which the various threads are to be cut. If, e.g., a double thread is to be cut, the first
and the second starts will be commenced from Q0 (no special programming is needed) and from
Q180, respectively.
G33 is a modal function. If several thread-cutting blocks are programmed in succession,
threads can be cut in any arbitrary surface limited by straight lines.
Fig. 4.4-2
The control is synchronized to the zero pulse of the spindle encoder in the first block, no synchronization will be performed in the subsequent blocks resulting in a continuous thread in each section of lines. Hence the programmed shift angle of the thread start (Q) will also be taken into account in the first block.
28
4 The Interpolation
An example of programming a thread-cutting:
G0 G90 X50 Z40
U-30
G33 U10 W38 F2
G0 U20
W-38
In the example above X is specified in diameter.
L Notes:
– The control returns error message 3020 DATA DEFINI-
TION ERROR G33 if more than two coordinates
are specified at a time in the thread-cutting block,
Fig. 4.4-3
or if both addresses F and E are specified simultaneously.
– Error message 3022 DIVIDE BY 0 IN G33 is produced when 0 is specified for address E in the
thread-cutting block.
– An encoder has to be mounted on the spindle for the execution of command G33.
– In the course of command G33 being executed, the control will take the feed and spindle over-
ride values automatically to be 100%; the effect of the stop key will only prevail after the
block has been executed.
– On account of the following error of the servo system, overrun and run out allowances have
to be provided for the tool in addition to the part at the beginning and end of the thread
in order to obtain a constant lead all along the part.
– In the course of thread-cutting the feed (in mm/minute) may not exceed the value selected in
the group of parameters FEEDMAX.
– In the course of thread-cutting the speed (r.p.m) of the spindle may not exceed the maximum
speed permissible for the spindle encoder mechanically and electrically (the maximum
output frequency).
4.5 Variable-Lead Thread Cutting (G34)
Command
G34 v F Q K
cuts straight or tapered threads of variablelead. The interpretation of input data v, F, Q
corresponds to those written for function G33.
The interpretation of K:
K: Increase or decrease of thread lead
Fig. 4.5-1
per spindle revolution.
The value of K ranges from 0.001 mm/rev (0.0001 inch/rev) to 500 mm/rev (10 inch/rev).
29
4.6 Polar Coordinate Interpolation (G12.1, G13.1)
4.6 Polar Coordinate Interpolation (G12.1, G13.1)
Polar coordinate interpolation is a control operation method, in case of which the work described
in a Cartesian coordinate system moves its contour path by moving a linear and a rotary axis.
Command
G12.1
switches polar coordinate interpolation mode on. The path of the milling tool can be described
in the succeeding part program in a Cartesian coordinate system in the usual way by programming
linear and circular interpolation, by taking the tool radius compensation into account. The com-
mand must be issued in a separate block and no other command can be written beside.
Command
G13.1
switches polar coordinate interpolation mode off. The command must be issued in a separate
block and no other command can be written beside. It always registers state G13.1 after power-on
or reset.
Plane selection
A plane determining the address of the linear and the rotary axis to be applied must be selected
before switching polar coordinate interpolation on.
Fig. 4.6-1
Command
G17 X_ C_
selects axis X for linear axis, while as for the rotary axis it is axis C. The virtual axis is indicated
with C’ on the diagram, the programming of which is implemented by defining length measures.
With the help of commands
G18 Z_ B_
G19 Y_ A_
further linear and rotary axes can be selected together in the above mentioned way.
Work zero point offset in the course of polar coordinate interpolation
In case of using polar coordinate interpolation the origin of the applied work coordinate system
must be chosen so that it coincides with the rotation axis of the circular axis.
Position of the axes when polar coordinate interpolation is switched on
Before switching polar coordinate interpolation on (command G12.1) make sure that the circular
axis position is 0. The linear axis position can either be negative or positive but it cannot be 0.
30
Loading...