Cycle 20 CONTOUR DATA

ISO programming

G120

Application

Use Cycle 20 to specify machining data for the subprograms describing the subcontours.

Notes

  • This cycle can be executed only 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

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.

 
Tip

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.

Example

11 CYCL DEF 20 CONTOUR DATA ~

Q1=-20

;MILLING DEPTH ~

Q2=+1

;TOOL PATH OVERLAP ~

Q3=+0.2

;ALLOWANCE FOR SIDE ~

Q4=+0.1

;ALLOWANCE FOR FLOOR ~

Q5=+0

;SURFACE COORDINATE ~

Q6=+2

;SET-UP CLEARANCE ~

Q7=+50

;CLEARANCE HEIGHT ~

Q8=+0

;ROUNDING RADIUS ~

Q9=+1

;ROTATIONAL DIRECTION