Cycle 23 FLOOR FINISHING
ISO programming
G123
Application
With Cycle 23 FLOOR FINISHING, you can finish your contour by taking the finishing allowance for the floor into account that has been programmed in Cycle 20. The tool smoothly approaches the plane to be machined (on a vertically tangential arc) if there is sufficient room. If there is not enough room, the control moves the tool to depth vertically. The tool then clears the finishing allowance remaining from rough-out.
Before programming the call of Cycle 23, you need to program further cycles:
- Cycle 14 CONTOUR or SEL CONTOUR
- Cycle 20 CONTOUR DATA
- Cycle 21 PILOT DRILLING, if applicable
- Cycle 22 ROUGH-OUT, if necessary
Related topics
- Cycle 273 OCM FINISHING FLOOR (#167 / #1-02-1)
Cycle run
- The control positions the tool to the clearance height at rapid traverse FMAX.
- The tool then moves in the tool axis at the feed rate Q11.
- The tool smoothly approaches the plane to be machined (on a vertically tangential arc) if there is sufficient room. If there is not enough room, the control moves the tool to depth vertically
- The tool clears the finishing allowance remaining from rough-out.
- Finally, the tool retracts in the tool axis to the clearance height or to the position last programmed before the cycle. This behavior depends on the machine parameter posAfterContPocket (no. 201007).
Notes
- After the end of the cycle, position the tool with all coordinates of the working plane (e.g., L X+80 Y+0 R0 FMAX)
- Make sure to program an absolute position after the cycle; do not program an incremental traversing movement
- This cycle can be executed only in the FUNCTION MODE MILL machining mode.
- The control automatically calculates the starting point for finishing. The starting point depends on the available space in the pocket.
- The approaching radius for pre-positioning to the final depth is permanently defined and independent of the plunging angle of the tool.
- If M110 is activated during operation, the feed rate for arcs compensated on the inside will be reduced accordingly.
- This cycle monitors the defined usable length LU of the tool. If the LU value is less than the DEPTH Q15, the control will display an error message.
- The cycle considers the miscellaneous functions M109 and M110. During the inside and outside machining of circular arcs the control keeps the feed rate constant at the cutting edge for inside and outside radii.
Note regarding machine parameters
- Use the machine parameter posAfterContPocket (no. 201007) to define how to move the tool after machining the contour pocket.
- PosBeforeMachining: Return to starting position
- ToolAxClearanceHeight: Position the tool axis to clearance height.
Cycle parameters
Help graphic | Parameter |
---|---|
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 | |
Q208 Feed rate for retraction? (optional) Tool traversing speed in mm/min when retracting after the machining operation. If you enter Q208 = 0, the control retracts the tool at the feed rate specified in Q12. Input: 0...99999.9999 or FMAX, FAUTO, 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.
Change the following contents as needed:
- Tools
- Cutting parameters
- Feed rates
- Clearance height or safe position
- Machine-specific positions (e.g., with M91)
- Paths of program calls
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 23 FLOOR FINISHING ~ | ||
| ||
| ||
|