ISO programming
G220
G220
This cycle enables you to define a point pattern as a full or pitch circle. It can be used for a previously defined machining cycle.
Sequence:
If you run this cycle in Program Run / Single Block mode, the control stops between the individual points of a point pattern.
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).
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.
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 |