HEIDENHAIN TNC 407 (280 580) ISO Programming User Manual
Page 168
5 - 3 5
TNC 426/TNC 425/TNC 415 B/TNC 407
5
Programming Tool Movements
Path Contours – Polar Coordinates
Example for exercise: Tapping
Given data
Thread:
Right-handed internal thread M64 x 1.5
Pitch P:
1.5 mm
Starting angle A
S
0°
End angle A
E
:
360° = 0° at Z
E
= 0
Thread revolutions n
R
:
8
Thread overrun:
• at start of thread n
S
:
0.5
• at end of thread n
E
:
0.5
Number of cuts:
1
A =0
°
E
A =0
°
S
A = 0
°
G13
A = –180
°
Calculating the input values
• Total height h:
h = P
.
n
P = 1.5 mm
n = n
R
+ n
S
+ n
E
= 9
h = 13.5 mm
• Incremental polar coordinate angle H:
H = n
.
360°
n = 9 (see total height h)
G91 H = 360°
.
9 = 3240°
• Starting angle A
S
with thread overrun n
S
:
n
S
= 0.5
The starting angle of the helix is advanced by 180° (n = 1 corresponds
to 360°). With positive rotation this means
A
S
with n
S
= A
S
– 180° = –180°
• Starting coordinate:
Z =
P
.
(n
R
+ n
S
)
= –1.5
.
8.5 mm
= –12.75 mm
Z
S
is negative because the thread is being cut in an upward direction
towards Z
E
= 0.
Part program
%S536I G71 * ........................................... Begin the program
N10 G30 G17 X+0 Y+0 Z–20 * ................ Define the workpiece blank
N20 G31 G90 X+100 Y+100 Z+0 *
N30 G99 T11 L+0 R+5 * .......................... Define the tool
N40 T11 G17 S2500 * .............................. Call the tool
N50 G00 G40 G90 Z+100 M06 * ............. Retract and insert tool
N60 X+50 Y+30 * ...................................... Pre-position in the working plane to the center of the hole
N70 G29 * ................................................. Transfer position as pole
N80 Z–12 M03 * ....................................... Move tool to starting depth
N90 G11 G41 R+32 H–180 F100 * .......... Approach contour with radius compensation at machining feed rate
N100 G13 G91 H+3240 Z+13.5 F200 *
Helical interpolation; angle and movement in infeed axis are incremental
N110 G00 G40 G90 X+50 Y+30 * ............ Depart contour (absolute), cancel radius compensation
N120 Z+100 M02 * ................................... Retract in the infeed axis
N99999 %S536I G71 *
Part program for cutting a thread with more than 15 revolutions (also see Chapter 6)
•
•
N80 G00 G40 G90 Z–12.75 M3
N90 G11 G41 R+32 H–180 F100
N100 G26 R+20
N110 G98 L1 .............................................................. Identify beginning of program section repeat
N120 G13 G91 H+360 Z+1.5 F200 ............................ Enter thread pitch directly as an incremental Z dimension
N130 L 1,24 ................................................................ Program the number of repeats (thread revolutions)
N140 G27 R+20
•
•