Cycle 20 CONTOUR DATA
ISO programming
G120
Application
Related topics
- Cycle 271 OCM CONTOUR DATA (#167 / #1-02-1)
Notes
- This cycle can only be executed in the FUNCTION MODE MILL machining mode.
- Cycle 20 is DEF-active, which means that it becomes active as soon as it is defined in the NC program.
- The machining data entered in Cycle 20 are valid for Cycles 21 to 24.
- If you are using the SL cycles in Q parameter programs, the cycle parameters Q1 to Q20 cannot be used as program parameters.
- The algebraic sign for the DEPTH cycle parameter determines the working direction. If you program DEPTH = 0, the control performs the cycle at the depth 0.
Cycle parameters
Help graphic | Parameter |
---|---|
Q1 Milling depth? Distance between workpiece surface and pocket floor. This value has an incremental effect. Input: –99999.9999...+99999.9999 | |
Q2 Path overlap factor? Q2 x tool radius = stepover factor k Input: 0.0001...1.9999 | |
Q3 Finishing allowance for side? Finishing allowance in the working plane. This value has an incremental effect. Input: –99999.9999...+99999.9999 | |
Q4 Finishing allowance for floor? Finishing allowance for the floor. This value has an incremental effect. Input: –99999.9999...+99999.9999 | |
Q5 Workpiece surface coordinate? Absolute coordinate of the top surface of the workpiece Input: –99999.9999...+99999.9999 | |
Q6 Set-up clearance? Distance between tool tip and the top surface of the workpiece. This value has an incremental effect. Input: –99999.9999...+99999.9999 | |
Q7 Clearance height? Height at which the tool cannot collide with the workpiece (for intermediate positioning and retraction at the end of the cycle). This value has an absolute effect. Input: –99999.9999...+99999.9999 | |
Q8 Inside corner radius?: Inside "corner" rounding radius; entered value is referenced to the path of the tool center and is used to calculate smoother traverse motions between the contour elements. Q8 is not a radius that is inserted between programmed elements as a separate contour element. Input: 0...99999.9999 | |
Q9 Direction of rotation? cw = -1 Machining direction for pockets Q9 = –1 up-cut milling for pocket and island Q9 = +1 climb milling for pocket and island Input: -1, 0, +1 |
11 CYCL DEF 20 CONTOUR DATA ~ | ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
|