HEIDENHAIN ITNC 530 - 6-2010 DIN-ISO PROGRAMMING, User Manual

Page: 297 / 618

HEIDENHAIN iTNC 530 297
9.1
1
Pr
ogr
amming Examples
N210 G00 G40 Z+250 M2 *
Retract in the tool axis, end program
N220 G98 L10 * Subprogram 10: Machining operation
N230 Q16 = Q6 - Q10 - Q108 * Account for allowance and tool, based on the cylinder radius
N240 Q20 = +1 * Set counter
N250 Q24 = +Q4 * Copy starting angle in space (Z/X plane)
N260 Q25 = ( Q5 - Q4 ) / Q13 *
Calculate angle increment
N270 G54 X+Q1 Y+Q2 Z+Q3 * Shift datum to center of cylinder (X axis)
N280 G73 G90 H+Q8 * Account for rotational position in the plane
N290 G00 G40 X+0 Y+0 * Pre-position in the plane to the cylinder center
N300 G01 Z+5 F1000 M3 * Pre-position in the tool axis
N310 G98 L1 *
N320 I+0 K+0 *
Set pole in the Z/X plane
N330 G11 R+Q16 H+Q24 FQ11 * Move to starting position on cylinder, plunge-cutting obliquely into
the material
N340 G01 G40 Y+Q7 FQ12 * Longitudinal cut in Y+ direction
N350 Q20 = +Q20 + 1 *
Update the counter
N360 Q24 = +Q24 + +Q25 *
Update solid angle
N370 D11 P01 +Q20 P02 +Q13 P03 99 * Finished? If finished, jump to end
N380 G11 R+Q16 H+Q24 FQ11 * Move in an approximated “arc” for the next longitudinal cut
N390 G01 G40 Y+0 FQ12 * Longitudinal cut in Y– direction
N400 D01 Q20 P01 +Q20 P02 +1 * Update the counter
N410 D01 Q24 P01 +Q24 P02 +Q25 *
Update solid angle
N420 D12 P01 +Q20 P02 +Q13 P03 1 * Unfinished? If not finished, return to LBL 1
N430 G98 L99 *
N440 G73 G90 H+0 * Reset the rotation
N450 G54 X+0 Y+0 Z+0 * Reset the datum shift
N460 G98 L0 *
End of subprogram
N99999999 %CYLIN G71 *