Programming Examples - HEIDENHAIN TNC 620 User Manual

8.13

Programming examples

Example: Ellipse
Program sequence
The contour of the ellipse is approximated by many
short lines (defined in Q7). The more calculation
steps you define for the lines, the smoother the curve
becomes.
The milling direction is determined with the starting
angle and end angle in the plane :
Machining direction is clockwise:
Starting angle > end angle
Machining direction is counterclockwise:
Starting angle < end angle
The tool radius is not taken into account.
0 BEGIN PGM ELLIPSE MM
1 FN 0: Q1 = +50
2 FN 0: Q2 = +50
3 FN 0: Q3 = +50
4 FN 0: Q4 = +30
5 FN 0: Q5 = +0
6 FN 0: Q6 = +360
7 FN 0: Q7 = +40
8 FN 0: Q8 = +0
9 FN 0: Q9 = +5
10 FN 0: Q10 = +100
11 FN 0: Q11 = +350
12 FN 0: Q12 = +2
13 BLK FORM 0.1 Z X+0 Y+0 Z-20
14 BLK FORM 0.2 X+100 Y+100 Z+0
15 TOOL CALL 1 Z S4000
16 L Z+250 R0 FMAX
17 CALL LBL 10
18 L Z+100 R0 FMAX M2
19 LBL 10
20 CYCL DEF 7.0 DATUM SHIFT
21 CYCL DEF 7.1 X+Q1
22 CYCL DEF 7.2 Y+Q2
23 CYCL DEF 10.0 ROTATION
24 CYCL DEF 10.1 ROT+Q8
25 Q35 = (Q6 -Q5) / Q7
26 Q36 = Q5
27 Q37 = 0
TNC 620 | User's Manual
HEIDENHAIN Conversational Programming | 5/2013
Programming examples 8.13
Center in X axis
Center in Y axis
Semiaxis in X
Semiaxis in Y
Starting angle in the plane
End angle in the plane
Number of calculation steps
Rotational position of the ellipse
Milling depth
Feed rate for plunging
Feed rate for milling
Set-up clearance for pre-positioning
Definition of workpiece blank
Tool call
Retract the tool
Call machining operation
Retract the tool, end program
Subprogram 10: Machining operation
Shift datum to center of ellipse
Account for rotational position in the plane
Calculate angle increment
Copy starting angle
Set counter
8
303