HEIDENHAIN MANUALPLUS 620 User Manual

246 ISO Programming
4.17 Contour-Based Turning Cycles
4.17 Contour-Based Turning Cycles
Working with contour-based cycles
Possibilities of transferring the contour to be machined to the cycle:
 Transferring the contour reference in the start block number and the
end block number. The contour area is machined in the direction
from “NS” to “NE”.
 Transferring the contour reference via the name of the auxiliary
contour (ID). The complete auxiliary contour is machined in the
direction of contour definition.
 Describing the contour with G80 in the block directly after the cycle
(see “Cycle end / Simple contour G80” on page 265).
 Describing the contour with G0, G1, G2 and G3 blocks directly after
the cycle. The contour is concluded by G80 without parameters.
Possibilities of defining the workpiece blank for calculating the number
of cutting passes:
 Defining a global workpiece blank in the WORKPIECE BLANK program
section. Regeneration of the workpiece blank is automatically
active. The cycle uses the specified workpiece blank.
 If no workpiece blank is defined, the cycle calculates the blank from
the contour to be machined and the position of the tool during cycle
call. Contour follow-up is not active.
Finding the block references:
U Place cursor in NS or NE input field
U Press the soft key
Select the contour element:
U Use the horizontal arrow keys to select the contour
element
U Use the vertical arrow keys to switch between
contours (also face contours, etc.).
Switch between NS and NE:
U Press the NS soft key
U Press the NE soft key
U Press the soft key to confirm the block number and
return to the dialog.
Cutting limits in X, Z
The tool position before the cycle call determines the effect of a
cutting limit. The MANUALplus machines the area to the right or to the
left of the cutting limit, depending on which side the tool has been
positioned before the cycle is called.
Example: Contour-based cycles
. . .
N1 G810 NS7 NE12 P3[block reference]
N2 ...
N3 G810 ID“007“ P3[name of auxiliary
contour]
N4 ...
N5 G810 ID“007“ NS9 NE7 P3[combination]
N6 ...
N7 G810 P3[predefined contour description]
N8 G80 XS60 ZS-2 XE90 ZE-50 AC10 WC10 BS3
BE-2 RC5 EC0
N9...
N10 G810 P3[direct contour description]
N11 G0 X50 Z0
N12 G1 Z-62 BR4
N13 G1 X85 AN80 BR-2
N14 G1 Zi-5
N15 G80
N16 ...
. . .
A cutting limit restricts the contour area that can be
machined; it does not apply to the paths for approach and
departure.

HEIDENHAIN MANUALPLUS 620 Specifications

General

Brand	HEIDENHAIN
Model	MANUALPLUS 620
Category	Control Systems
Language	English