Siemens SINUMERIK 840D sl Operating Manual page 440

Programming technological functions (cycles)
10.3 Contour milling
For machining in the opposite direction, contours must not consist of more than 170 contour
elements (incl. chamfers/radii). Special aspects (except for feed values) of free G code input
are ignored during path milling in the opposite direction to the contour.
Note
Activating G40
We recommend that you activate G40 before the cycle call.
Programming of arbitrary contours
The machining of arbitrary open or closed contours is generally programmed as follows:
1. Enter contour
You build up the contour gradually from a series of different contour elements.
Define the contour in a subprogram or in the machining program, e.g. after the end of
program (M02 or M30).
2. Contour call (CYCLE62)
You select the contour to be machined.
3. Path milling (roughing)
The contour is machined taking into account various approach and retract strategies.
4. Path milling (finishing)
If you programmed a finishing allowance for roughing, the contour is machined again.
5. Path milling (chamfering)
If you have planned edge breaking, chamfer the workpiece with a special tool.
Path milling on right or left of the contour
A programmed contour can be machined with the cutter radius compensation to the right or
left. You can also select various modes and strategies of approach and retraction from the
contour.
Approach/retraction mode
The tool can approach or retract from the contour along a quadrant, semi-circle or straight line.
● With a quadrant or semi-circle, you must specify the radius of the cutter center point path.
● With a straight line, you must specify the distance between the cutter outer edge and the
contour starting or end point.
You can also program a mixture of modes, e.g. approach along quadrant, retract along semi-
circle.
440
Operating Manual, 05/2017, A5E40868956
Milling