HEIDENHAIN TNC 620 User Manual page 380

9
Programming Q parameters
9.12 Programming examples
Example: Concave cylinder machined with spherical
cutter
Program run
This program functions only with a spherical cutter.
The tool length refers to the sphere center.
The contour of the cylinder is approximated by many
short line segments (defined in Q13). The more
line segments you define, the smoother the curve
becomes.
The cylinder is milled in longitudinal cuts (here: parallel
to the Y axis).
The milling direction is determined with the starting
angle and end angle in space:
Machining direction clockwise:
Starting angle > end angle
Machining direction counterclockwise:
Starting angle < end angle
The tool radius is compensated automatically
%CYLIN G71 *
N10 D00 Q1 P01 +50*
N20 D00 Q2 P01 +0*
N30 D00 Q3 P01 +0*
N40 D00 Q4 P01 +90*
N50 D00 Q5 P01 +270*
N60 D00 Q6 P01 +40*
N70 D00 Q7 P01 +100*
N80 D00 Q8 P01 +0*
N90 D00 Q10 P01 +5*
N100 D00 Q11 P01 +250*
N110 D00 Q12 P01 +400*
N120 D00 Q13 P01 +90*
N130 G30 G17 X+0 Y+0 Z-50*
N140 G31 G90 X+100 Y+100 Z+0*
N150 T1 G17 S4000*
N160 G00 G40 G90 Z+250*
N170 L10.0*
N180 D00 Q10 P01 +0*
N190 L10.0*
N200 G00 G40 Z+250 M2*
N210 G98 L10*
N220 Q16 = Q6 - Q10 - Q108
N230 D00 Q20 P01 +1*
N240 D00 Q24 P01 +Q4*
N250 Q25 = ( Q5 - Q4 ) / Q13
N260 G54 X+Q1 Y+Q2 Z+Q3*
380
Center in X axis
Center in Y axis
Center in Z axis
Starting angle in space (Z/X plane)
End angle in space (Z/X plane)
Cylinder radius
Length of the cylinder
Rotational position in the X/Y plane
Allowance for cylinder radius
Feed rate for plunging
Feed rate for milling
Number of cuts
Workpiece blank definition
Tool call
Retract the tool
Call machining operation
Reset allowance
Call machining operation
Retract the tool, end program
Subprogram 10: Machining operation
Account for allowance and tool, based on the cylinder radius
Set counter
Copy starting angle in space (Z/X plane)
Calculate angle increment
Shift datum to center of cylinder (X axis)
HEIDENHAIN | TNC 620 | ISO Programming User's Manual | 9/2016