ISO programming
G277
G277
Cycle 277 OCM CHAMFERING enables you to deburr edges of complex contours that you roughed out using OCM cycles.
This cycle considers adjacent contours and boundaries that you called before with Cycle 271 OCM CONTOUR DATA or the 12xx standard geometric elements.
Positioning logic in OCM cycles
Adapting the feed rate for circular paths with M109
Help graphic | Parameter |
---|---|
Q353 Depth of tool tip? Distance between theoretical tool tip and workpiece surface coordinate. This value has an incremental effect. Input: –999.9999...–0.0001 | |
Q359 Width of chamfer (-/+)? Width or depth of chamfer: -: Depth of chamfer +: Width of chamfer This value has an incremental effect. Input: –999.9999...+999.9999 | |
Q207 Feed rate for milling? Traversing speed of the tool in mm/min for milling Input: 0...99999.999 or FAUTO, FU, FZ | |
Q253 Feed rate for pre-positioning? Traversing speed of the tool in mm/min for positioning Input: 0...99999.9999 or FMAX, FAUTO, PREDEF | |
Q200 Set-up clearance? Distance between tool tip and workpiece surface. This value has an incremental effect. Input: 0...99999.9999 or PREDEF | |
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 | |
Q354 Angle of chamfer? Angle of the chamfer 0: The chamfer angle is half the defined T-ANGLE from the tool table > 0: The chamfer angle is compared to the value of T-ANGLE from the tool table. If these two values do not match, the control will display an error message. Input: 0...89 |
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 277 OCM CHAMFERING ~ | ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
|