Cycle 220 POLAR PATTERN
ISO programming
G220
Application
Related topics
- Defining a full circle with PATTERN DEF
- Defining a circle segment with PATTERN DEF
Cycle run
- The control moves the tool at rapid traverse from its current position to the starting point for the first machining operation.
Sequence:
- Move to 2nd set-up clearance (spindle axis)
- Approach the starting point in the working plane
- Move to set-up clearance above the workpiece surface (spindle axis)
- From this position, the control executes the last defined fixed machining cycle.
- The tool then approaches the starting point for the next machining operation on a straight lineor a circular arc. The tool stops at the set-up clearance (or the 2nd set-up clearance).
- This procedure (steps 1 to 3) will be repeated until all machining operations have been completed.
If you run this cycle in Program Run / Single Block mode, the control stops between the individual points of a point pattern.
Notes
Cycle 220 POLAR PATTERN can be hidden with the optional machine parameter hidePattern (no. 128905).
- Cycle 220 is DEF-active. In addition, Cycle 220 automatically calls the last defined machining cycle.
Note on programming
- If you combine one of the machining cycles 200 to 209 or 251 to 267 with Cycle 220 or Cycle 221, the set-up clearance, the workpiece surface, and the 2nd set-up clearance from Cycle 220 or 221 are effective. This applies within the NC program until the affected parameters are overwritten again.
Example: If Cycle 200 is defined in an NC program with Q203=0 and you then program Cycle 220 with Q203=-5, then the subsequent calls with CYCL CALL and M99 will use Q203=-5. Cycles 220 and 221 overwrite the above-mentioned parameters of CALL-active machining cycles (if the same input parameters have been programmed in both cycles).
Cycle parameters
Help graphic | Parameter |
---|---|
Q216 Center in 1st axis? Pitch circle center in the main axis of the working plane. This value has an absolute effect. Input: –99999.9999...+99999.9999 | |
Q217 Center in 2nd axis? Pitch circle center in the secondary axis of the working plane. This value has an absolute effect. Input: –99999.9999...+99999.9999 | |
Q244 Pitch circle diameter? Diameter of circle Input: 0...99999.9999 | |
Q245 Starting angle? Angle between the main axis of the working plane and the starting point for the first machining operation on the pitch circle. This value has an absolute effect. Input: –360.000...+360.000 | |
Q246 Stopping angle? Angle between the main axis of the working plane and the starting point for the last machining operation on the pitch circle (does not apply to complete circles). Do not enter the same value for the stopping angle and starting angle. If you specify a stopping angle greater than the starting angle, machining will be carried out counterclockwise; otherwise, machining will be clockwise. This value has an absolute effect. Input: –360.000...+360.000 | |
Q247 Intermediate stepping angle? Angle between two machining operations on a pitch circle. If you enter an angle step of 0, the control will calculate the angle step from the starting and stopping angles and the number of pattern repetitions. If you enter a value other than 0, the control will not take the stopping angle into account. The sign for the angle step determines the working direction (negative = clockwise). This value has an incremental effect. Input: –360.000...+360.000 | |
Q241 Number of repetitions? Number of machining operations on a pitch circle Input: 1...99999 | |
Q200 Set-up clearance? Distance between tool tip and workpiece surface. This value has an incremental effect. Input: 0...99999.9999 or PREDEF | |
Q203 Workpiece surface coordinate? Coordinate on the workpiece surface referenced to the active datum. This value has an absolute effect. Input: –99999.9999...+99999.9999 | |
Q204 2nd set-up clearance? Distance in the tool axis between tool and workpiece (fixtures) at which no collision can occur. This value has an incremental effect. Input: 0...99999.9999 or PREDEF | |
Q301 Move to clearance height (0/1)? Specify how the tool moves between machining processes: 0: Move to the set-up clearance between operations 1: Move to the 2nd set-up clearance between operations Input: 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.
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 220 POLAR PATTERN ~ | ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
12 CYCL CALL |