Programming Aid
Address Letters
Contour cycles:
Program structure for machining sequences with several tools:
.
.
List of contour subprograms G37 P01 . . .
Define / call drill
Contour cycle: Pilot drilling G56 P01 . . .
Pre-positioning, cycle call
Define / call rough mill
Contour cycle: Rough-out G57 P01 . . .
Pre-positioning, cycle call
Define / call finish mill
Contour cycle: Contour milling G58 P01 . . .
Pre-positioning, cycle call
End of main program, return jump M02
Contour subprograms G98
Radius compensation of the contour subprograms:
Contour Sequence of the programmed Radius
Inside Clockwise (CW) G42 (RR)
(Pocket) Counterclockwise (CCW) G41 (RL)
Outside Clockwise (CW) G41 (RL)
(Island) Counterclockwise (CCW) G42 (RR)
Coordinate transformations:
Coordinate transformations Activation Cancellation
Datum shift G54 X+20 Y+30 Z+10 G54 X+0 Y+0 Z+0
Mirror image G28 X G28
Rotation G73 H+45 G73 H+0
Scaling factor G72 F0.8 G72 F1
contour elements compensation
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
G98 L0
.
.
.
Q Parameter Definitions
D Function
00 Assign
01 Addition
02 Subtraction
03 Multiplication
04 Division
05 Square root
06 Sine
07 Cosine
D Function
08 Root sum of squares c = a2+b
09 If equal, jump to label number
10 If not equal, jump to label number
11 If greater than, jump to label number
12 If smaller than, jump to label number
13 Angle (from c • sin α and c • cos α)
14 Error number
15 Print
19 Assign values for the PLC
2
Add. Function
% Begin program
% Call program with G39
A Rotate around the X axis
B Rotate around the Y axis
C Rotate around the Z axis
D Q parameter definitions
F Feed rate
F Dwell time with G04
F Scaling factor with G72
G G functions
H Polar angle
H Rotation angle with G73
I X coordinate of
circle center/pole
J Y coordinate of
circle center/pole
K Z coordinate of
circle center/pole
L Assign a label number
with G98
L Jump to a label number
L Tool length with G99
M M functions
Add. Function
N Block number
P Cycle parameter
in fixed cycles
P Value or Q parameter
in Q parameter definitions
Q Parameter Q
R Polar radius
R Circle radius with G02/G03/G05
R Rounding radius with
G25/G26/G27
R Tool radius with G99
S Spindle speed
S Oriented spindle stop with G36
T Tool definition with G99
T Tool call
T Next tool with G51
U Axis parallel to the X axis
V Axis parallel to the Y axis
W Axis parallel to the Z axis
X X axis
Y Y axis
Z Z axis
* End of block
Sequence of Program Steps: Milling
PGM
Select program name
Program 234 in mm % 234 G71
Define workpiece blank G30 G17 X+0 Y+0 Z–40
Define tool G99 T1 L+0 R+5
Call tool T0 G17
Tool change position G00 G40 G90 Z+100 M06
Call tool T1 G17 S1000
Starting position, near the workpiece X–20 Y–20 M03
Working depth Z–20
1st contour point, with radius compensation (RL) G01 G41 X+0 Y+0 F200
Smooth approach G26 R15
Straight line Y+100
Chamfer G24 R20
Straight line X+100
Corner rounding G25 R20
Straight line Y+25
Circle center I+100 J+0
Circle, incremental values G03 G91 X–25 Y–25
Last contour point, absolute values G01 G90 X+0 Y+0
Smooth departure G27 R15
End position, near the workpiece G00 G40 X–20 Y–20
Retract tool, return to beginning of program Z+100 M02
NR
G31 G90 X+100 Y+100 Z+0
TNC 360
ISO-Programming
Operating Modes
Machine operating modes:
Manual The axes are moved with the machine axis direction
Handwheel The axes are moved with the electronic handwheel or
Positioning The axes are moved to or by a programmed distance
with manual with the selected radius compensation, feed rate and
data input M function (single-axis movement). The block is not
Program run After starting the program with the machine START
Full sequence button, the program is automatically executed to program
Program run Each block must be started separately with the machine
Single block START button.
Programming:
Programming Part programs can be entered, checked and changed, and
and Editing read in and out the control memory through an RS-232-C/
Test The TNC checks part programs for logical programming
Graphical test run:
GRAPHICS Part programs can be graphically simulated in the display
MOD
buttons. The position display can be set to the desired
display type.
by a programmed jog increment with the machine axis
direction buttons.
stored in the TNC memory.
end or to a program stop.
V.24 data interface.
errors such as exceeding the axis traverse limits, doubleprogrammed axes, etc.
modes plan view, projection in three planes and 3D view.
The graphical test run is executed in the "full sequence"
and "single block" modes of operation and is started with
with the START key.
G Functions
G Functions
M Functions
Tool movement
G00 Linear interpolation, Cartesian coordinates, at rapid traverse
G01 Linear interpolation, Cartesian coordinates
G02 Circular interpolation, Cartesian coordinates, clockwise
G03 Circular interpolation, Cartesian coordinates, counterclockwise
G05 Circular interpolation, Cart. coordinates, no direction of rotation defined
G06 Circular interpolation, Cartesian coordinates, tangential connection
∗G07 Single axis positioning block
G10 Linear interpolation, polar coordinates, at rapid traverse
G11 Linear interpolation, polar coordinates
G12 Circular interpolation, polar coordinates, clockwise
G13 Circular interpolation, polar coordinates, counterclockwise
G15 Circular interpolation, polar coordinates, no direction of rotation defined
G16 Circular interpolation, polar coordinates, tangential connection
Chamfer / Corner rounding / Approaching and departing a contour
∗G24 Chamfer with chamfer length R
∗G25 Corner rounding with radius R
∗G26 Smooth (tangential) approach of a contour with radius R
∗G27 Smooth (tangential) departure from a contour with radius R
Tool definition
∗G99 With tool number T, length L, radius R
Tool radius compensation
G40 No tool radius compensation
G41 Tool radius compensation, tool traverse to the left of the contour
G42 Tool radius compensation, tool traverse to the right of the contour
G43 Single axis compensation for G07, lengthening of the tool path
G44 Single axis compensation for G07, shortening of the tool path
Definition of the workpiece blank for graphic display
G30 (G17/G18/G19) MIN point
G31 (G90/G91) MAX point
Simple fixed cycles
G83 Pecking
G84 Tapping with a floating tap holder
G85 Rigid tapping
G74 Slot milling
G75 Rectangular pocket milling, clockwise
G76 Rectangular pocket milling, counterclockwise
G77 Circular pocket milling, clockwise
G78 Circular pocket milling, counterclockwise
SL Cycles
G37 Contour geometry, definition of subcontour subprogram numbers
G56 Pilot drilling
G57 Rough-out
G58 Contour milling (finishing), clockwise
G59 Contour milling (finishing), counterclockwise
∗) Function effective blockwise
Cycles for coordinate transformations
G54 Datum shift in a part program
G28 Mirror image of a contour
G73 Rotation of the coordinate system
G72 Scaling factor, increasing or reducing the size of a contour
Other cycles
∗ G04 Dwell time with F seconds
G36 Oriented spindle stop
∗ G39 Program call
Selecting the working plane
G17 Plane X/Y, tool axis Z
G18 Plane Z/X, tool axis Y
G19 Plane Y/Z, tool axis X
G20 Tool axis IV
Definition of positions
G90 Absolute workpiece positions
G91 Incremental workpiece positions
Unit of measurement
G70 Unit of measurement: Inches (defined at beginning of program)
G71 Unit of measurement: Millimeters (defined at beginning of program)
Other G functions
G29 Define the last programmed position as a pole (circle center)
G38 Stop program run
∗ G51 Tool pre-selection (with central tool memory)
G55 Programmable touch probe function
∗ G79 Cycle call
∗ G98 Assign a label number
∗) Function effective blockwise
M00 Stop program run / Spindle stop / Coolant off
M02 Stop program run / Spindle stop / Coolant off
Clear the status display (depending on machine parameter)
Return jump to block 1
M03 Spindle on clockwise
M04 Spindle on counterclockwise
M05 Spindle stop
M06 Tool change
Spindle stop / stop program run (depending on machine parameter)
M08 Coolant on
M09 Coolant off
M13 Spindle on clockwise / Coolant on
M14 Spindle on counterclockwise / Coolant on
M30 Same function as M02
M89 Vacant miscellaneous function, or
Cycle call, modally effective
M99 Cycle call, effective blockwise
M90 Constant path speed at inside corners and
corners without radius compensation
M91 Coordinates in the positioning block are referenced to the
machine datum
M92 Coordinates in the positioning block are referenced to a
position defined by the machine tool builder
M93 Reserved
M94 Limit display of rotary axis to value under 360°
M95 Reserved
M96 Reserved
M97 Radius compensation at outside corners: point of intersection
instead of transition arc
M98 End of radius compensation, effective blockwise
Loading...