HEIDENHAIN CNC Pilot 4290 V7.1 - Manual (Page 232)

232
4.21 Simple T
u
rn
ing Cy
cles
Simple face roughing G82
G82 roughs the contour area defined by the current tool position and
X, Z. If you wish to machine an oblique cut, you can define the angle
with I and K.
The CNC PILOT uses the position of the target point to distinguish
between external and internal machining. The number of cutting
passes is calculated so that an abrasive cut is avoided and the
calculated infeed distance is <= K.
Cycle run
1 Calculates the number of cutting passes.
2 Approaches workpiece for first pass from starting point on
paraxial path.
3 Moves at feed rate to target point Z.
4 Depending on algebraic sign of I:
„ <0: Machines contour outline
„ I>0: Retracts by 1 mm at 45°
5 Returns at rapid traverse and approaches for next pass.
6 Repeats 3 to 5 until target point X has been reached.
7 Move to:
„ X: Last retraction coordinate
„ Z: Starting point of cycle
Example: G82
. . .
N1 T3 G95 F0.25 G96 S200 M3
N2 G0 X120 Z2
N3 G82 X20 Z-15 I4 K4 Q0
N4 G0 X120 Z-15
N5 G82 X50 Z-26 I2 K-4 Q1
N6 G0 X120 Z-26
N7 G82 X80 Z-45 K4 Q1
. . .
Parameters
X Target point contour (diameter)
Z Target point contour
I Offset in X direction (default: 0)
K Maximum infeed
„ K<0: With machining contour outline
„ K>0: Without machining contour outline
Q G function for infeed (default: 0)
„ 0: Infeed with G0 (rapid traverse)
„ 1: Infeed with G1 (feed rate)
„ Programming X, Z: Absolute, incremental or modal
„ The tool radius compensation is not active.
„ Safety clearance after each pass: 1 mm
„ A G57 oversize
„ Is calculated with algebraic sign (oversizes are
therefore impossible for inside contour machining)
„ Remains effective after cycle end
„ A G58 oversize is not taken into account.