Siemens SINUMERIK 828D User Manual

Programming technology functions (cycles)
9.3 Contour turning
Turning
Operating Manual, 01/2015, 6FC5398-8CP40-5BA2
393
5.
Press the "Accept" softkey.
The input window for the starting
point of the contour appears.
Enter the individual contour elements (see Section "Creating contour
elements").
Parameter
Description
Unit
Z
Starting point Z (abs)
mm
X
Starting point X ∅ (abs)
mm
Transition to con-
tour start
Type of transition
• Radius
• Chamfer
FS=0 or R=0: No transition element
R
Transition to following element – radius
mm
FS
Transition to following element – chamfer
mm
Direction in front
of the contour
Direction of the contour element towards the starting point:
• In the negative direction of the horizontal axis
• In the positive direction of the horizontal axis
• In the negative direction of the vertical axis
• In the positive direction of the vertical axis
Additional com-
mands
You can enter additional commands in the form of G code for each contour element.
You can enter the additional commands (max. 40 characters) in the extended parame-
ter screens ("All parameters" softkey). The softkey is always available at the starting
point, it only has to be pressed when entering additional contour elements.
You can program feedrates and M commands, for example, using additional G code
commands. However, carefully ensure that the additional commands do not collide with
the generated G code of the contour and are compatible with the machining type re-
quired. Therefore, do not use any G code commands of group 1 (G0, G1, G2, G3), no
coordinates in the plane and no G code commands that have to be programmed in a
separate block.
The contour is finished in continuous-path mode (G64). As a result, contour transitions
such as corners, chamfers or radii may not be machined precisely.
If you wish to avoid this, then it is possible to use additional commands when program-
ming.
Example: For a contour, first program the straight X parallel and then enter "G9" (non-
modal exact stop) for the additional command parameter. Then program the Z-parallel
straight line. The corner will be machined exactly, as the feedrate at the end of the X-
parallel straight line is briefly zero.
Note:
The additional commands are only effective for finishing!

Siemens SINUMERIK 828D Specifications

General

Brand	Siemens
Model	SINUMERIK 828D
Category	Control Systems
Language	English