HEIDENHAIN TNC 620 User Manual page 378

9
Programming Q parameters
9.12 Programming examples
9.12 Programming examples
Example: Ellipse
Program run
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
%ELLIPSE G71 *
N10 D00 Q1 P01 +50*
N20 D00 Q2 P01 +50*
N30 D00 Q3 P01 +50*
N40 D00 Q4 P01 +30*
N50 D00 Q5 P01 +0*
N60 D00 Q6 P01 +360*
N70 D00 Q7 P01 +40*
N80 D00 Q8 P01 +30*
N90 D00 Q9 P01 +5*
N100 D00 Q10 P01 +100*
N110 D00 Q11 P01 +350*
N120 D00 Q12 P01 +2*
N130 G30 G17 X+0 Y+0 Z-20*
N140 G31 G90 X+100 Y+100 Z+0*
N150 T1 G17 S4000*
N160 G00 G40 G90 Z+250*
N170 L10.0*
N180 G00 Z+250 M2*
N190 G98 L10*
N200 G54 X+Q1 Y+Q2*
N210 G73 G90 H+Q8*
N220 Q35 = ( Q6 - Q5 ) / Q7
N230 D00 Q36 P01 +Q5*
N240 D00 Q37 P01 +0*
N250 Q21 = Q3 * COS Q36
N260 Q22 = Q4 * SIN Q36
378
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
Workpiece blank definition
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
Calculate X coordinate for starting point
Calculate Y coordinate for starting point
HEIDENHAIN | TNC 620 | ISO Programming User's Manual | 9/2016