ISO programming
G274
G274
With Cycle 274 OCM FINISHING SIDE, you can program finishing with the side finishing allowance programmed in Cycle 271. You can run this cycle in climb or up-cut milling.
Cycle 274 can also be used for contour milling.
Positioning logic in OCM cycles
Help graphic | Parameter |
---|---|
Q338 Infeed for finishing? Tool infeed in the spindle axis per finishing cut. Q338 = 0: Finishing with a single infeed This value has an incremental effect. Input: 0...99999.9999 | |
Q385 Finishing feed rate? Traversing speed of the tool in mm/min for side finishing Input: 0...99999.999 or FAUTO, FU, FZ | |
Q253 Feed rate for pre-positioning? Traversing speed of the tool in mm/min for approaching the starting position. This feed rate will be used below the coordinate surface, but outside the defined material. Input: 0...99999.9999 or FMAX, FAUTO, PREDEF | |
Q200 Set-up clearance? Distance between lower edge of tool and workpiece surface. This value has an incremental effect. Input: 0...99999.9999 or PREDEF | |
Q14 Finishing allowance for side? The finishing allowance for the side Q14 is left over after finishing. This allowance must be smaller than the allowance in Cycle 271. This value has an incremental effect. Input: –99999.9999...+99999.9999 | |
Q438 or QS438 Number/name of rough-out tool? Number or name of the tool that was used by the control to rough out the contour pocket. You can transfer the coarse roughing tool directly from the tool table via the action bar. In addition, you can enter the tool name via the Name in the action bar. The control automatically inserts the closing quotation mark when you exit the input field. –1: The control assumes that the tool last used is the rough-out tool (default behavior). Input: –1...+32767.9 or max. 255 characters | |
Q351 Direction? Climb=+1, Up-cut=-1 Type of milling operation. The direction of spindle rotation is taken into account. +1 = climb milling –1 = up-cut milling PREDEF: The control uses the value of a GLOBAL DEF block (If you enter 0, climb milling is performed) Input: -1, 0, +1 or PREDEF |
NC programs contained in this User's Manual are suggestions for solutions. The NC programs or individual NC blocks must be adapted before being used on a machine.
Some NC programs depend on the machine kinematics. Adapt these NC programs to your machine kinematics before the first test run.
In addition, test the NC programs using the simulation before the actual program run.
With a program test you determine whether the NC program can be used with the available software options, the active machine kinematics and the current machine configuration.
11 CYCL DEF 274 OCM FINISHING SIDE ~ | ||
| ||
| ||
| ||
| ||
| ||
| ||
|