DIN/ISO programming | G codes from previous controls
4
HEIDENHAIN | User's Manual smart.Turn and DIN Programming | 12/2017
503
Recessing G86 – simple turning cycle
G86 machines simple radial and axial recesses with chamfers. From
the tool position, the control determines whether a radial or axial
recess, or an inside or outside recess is to be machined.
Parameters:
X: Base corner X (diameter value)
Z: Base corner Z
I: Radial recess – Ov.size / axial recess – Breadth
Radial recess
I > 0: Oversize (roughing and finishing)
I = 0: No finishing
Axial recess:
I > 0: Recess width
No input: Recess width = tool width
K: Radial recess – Breadth / axial recess – Ov.size
Radial recess
K > 0: Recess width
No input: Recess width = tool width
Axial recess
K > 0: Oversize (roughing and finishing)
K = 0: No finishing
E: Delay (default: time for one spindle revolution)
With finishing oversize: Only for finishing
Without finishing oversize: No finishing
Oversize programmed: First roughing, then finishing
G86 machines chamfers at the sides of the recess. If you do not
wish to cut the chamfers, you must position the tool at a sufficient
distance from the workpiece.
Calculate the starting position XS (diameter) as follows:
XS = XK + 2 * (1.3 – b)
XK: Contour diameter
b: Chamfer width
The tool radius compensation is active
An oversize is not taken into account
Example: G86
. . .
N1 T3 G95 F0.25 G96 S200 M3
N2 G0 X62 Z2
N3 G86 X54 Z-30 I0.2 K7 E2
Radial
N4 G14 Q0
N5 T38 G95 F0.15 G96 S200 M3
N6 G0 X120 Z1
N7 G86 X102 Z-4 I7 K0.2 E1
Axial
. . .
To Next Page
Loading...
