HEIDENHAIN TNC 360 ISO-Programmierung - Manual

Machine operating modes:
Manual The axes are moved with the machine axis direction
buttons. The position display can be set to the desired
display type.
Handwheel The axes are moved with the electronic handwheel or
by a programmed jog increment with the machine axis
direction buttons.
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
stored in the TNC memory.
Program run After starting the program with the machine START
Full sequence button, the program is automatically executed to program
end or to a program stop.
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/
V.24 data interface.
Test The TNC checks part programs for logical programming
errors such as exceeding the axis traverse limits, double-
programmed axes, etc.
Graphical test run:
GRAPHICS Part programs can be graphically simulated in the display
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.
D Function
00 Assign
01 Addition
02 Subtraction
03 Multiplication
04 Division
05 Square root
06 Sine
07 Cosine
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
G98 L0
Address Letters
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
Programming Aid
..
.
..
.
..
.
..
.
Sequence of Program Steps: Milling
Q Parameter Definitions
Radius compensation of the contour subprograms:
Contour Sequence of the programmed Radius
contour elements compensation
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
Select program name
Program 234 in mm % 234 G71
Define workpiece blank G30 G17 X+0 Y+0 Z–40
G31 G90 X+100 Y+100 Z+0
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
Operating Modes
TNC 360
ISO-Programming
..
.
..
.
..
.
..
.
..
.
PGM
NR
MOD
D Function
08 Root sum of squares c = a 2 +b 2
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