ISO programming
G124
G124
Cycle 24 SIDE FINISHING allows you to finish your contour by taking the side finishing allowance into account that has been programmed in Cycle 20. You can run this cycle in climb or up-cut milling mode.
The starting point calculated by the control also depends on the machining sequence. If you select the finishing cycle with the GOTO key and then start the NC program, the starting point can be at a different location from where it would be if you execute the NC program in the defined sequence.
Help graphic | Parameter |
---|---|
Q9 Direction of rotation? cw = -1 Machining direction: +1: Counterclockwise –1: Clockwise Input: –1, +1 | |
Q10 Plunging depth? Tool infeed per cut. This value has an incremental effect. Input: –99999.9999...+99999.9999 | |
Q11 Feed rate for plunging? Tool traversing speed in mm/min during plunging Input: 0...99999.9999 or FAUTO, FU, FZ | |
Q12 Feed rate for roughing? Traversing feed rate in the working plane Input: 0...99999.9999 or FAUTO, FU, FZ | |
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 20. 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 are able to 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. Q438 = –1: The control assumes that the tool last used is the rough-out tool (default behavior) Q438 = 0: If there was no coarse-roughing, enter the number of a tool with the radius 0. This is usually the tool numbered 0. Input: –1...+32767.9 or 255 characters |
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 24 SIDE FINISHING ~ | ||
| ||
| ||
| ||
| ||
| ||
|