beautypg.com

HEIDENHAIN TNC 407 (280 580) ISO Programming User Manual

Page 168

background image

5 - 3 5

TNC 426/TNC 425/TNC 415 B/TNC 407

5

Programming Tool Movements

5.5

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

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