Table of Contents
Advertisement
CYLINDER SURFACE Slot milling (Cycle 28, DIN/ISO: G128, software
Please note while programming:
This cycle performs an inclined 5-axis machining
operation. To run this cycle, the first machine axis
below the machine table must be a rotary axis. In
addition, it must be possible to position the tool
perpendicular to the cylinder surface.
Define the approaching behavior in ConfigDatum,
CfgGeoCycle, apprDepCylWall
CircleTangential:
Tangential approach and departure
LineNormal: The movement to the contour
starting point is not performed on a tangential
path, but on a straight line
In the first NC block of the contour program, always
program both cylinder surface coordinates.
The algebraic sign for the cycle parameter DEPTH
determines the working direction. If you program
DEPTH=0, the cycle will not be executed.
This cycle requires a center-cut end mill (ISO 1641).
The cylinder must be set up centered on the rotary
table. Set the reference point to the center of the
rotary table.
The spindle axis must be perpendicular to the rotary
table axis when the cycle is called.
This cycle can also be used in a tilted working plane.
The set-up clearance must be greater than the tool
radius.
The machining time can increase if the contour
consists of many non-tangential contour elements.
When you use local QL Q parameters in a contour
subprogram you must also assign or calculate these
in the contour subprogram.
After the end of the cycle, do not use incremental
positioning for the tool. Rather, program an absolute
position.
In the parameter CfgGeoCycle, displaySpindleErr, on/
off, define whether the TNC should output an error
message (on) or not (off) if spindle rotation is not
active when the cycle is called. The function needs
to be adapted by your machine manufacturer.
HEIDENHAIN | TNC 320 | User's manual for cycle programming | 9/2016
8.3
option 1)
223
8
Advertisement
Table of Contents
