ISO programming
G1430
G1430
Touch probe cycle 1430 allows a position to be probed with an L-shaped stylus. The control can probe undercuts due to the shape of the stylus. You can apply the result of the probing procedure to the active rows of the preset table.
In the main axis and secondary axis, the touch probe is oriented in accordance with the calibration angle. In the tool axis, the touch probe is oriented in accordance with the programmed spindle angle and the calibration angle.
If, prior to this cycle, you program Cycle 1493 EXTRUSION PROBING, then the control repeats the touch points in the selected direction and at the defined length along a straight line.
Q parameter | Meaning |
---|---|
Q950 to Q952 | Measured position in the main axis, auxiliary axis and tool axis |
Q980 to Q982 | Measured deviation of the position in the main axis, auxiliary axis and tool axis |
Q183 |
|
Q970 | If you have programmed Cycle 1493 EXTRUSION PROBING: Maximum deviation based on the nominal position of the first touch point |
Help graphic | Parameter |
---|---|
Q1100 1st noml. position of ref. axis? Absolute nominal position of the first touch point in the main axis of the working plane Input: –99999.9999...+99999.9999 or ?, -, + or @
| |
Q1101 1st noml. position of minor axis? Absolute nominal position of the first touch point in the secondary axis of the working plane Input: –99999.9999...+9999.9999 or optional input (see Q1100) | |
Q1102 1st nominal position tool axis? Absolute nominal position of the first touch point in the tool axis Input: –99999.9999...+9999.9999 or optional input (see Q1100) | |
Q372 Probe direction (–3 to +3)? Axis defining the direction of probing. The algebraic sign lets you define whether the control moves in the positive or negative direction. Input: –3, -2, -1, +1, +2, +3 | |
Q336 Angle for spindle orientation? Angle at which the control orients the tool prior to the probing procedure. This angle takes effect only during probing in the tool axis (Q372 = +/– 3). This value has an absolute effect. Input: 0...360 | |
Q1118 Distance of radial approach? Distance to the nominal position at which the touch probe is pre-positioned in the machining plane and to which it retracts after probing. If Q372= +/–1: Distance is in the direction opposite to the probing direction. If Q372= +/– 2: Distance is in the direction opposite to the probing direction. If Q372= +/–3: Distance is in the direction opposite to the angle of the spindle Q336. This value has an incremental effect. Input: 0...9999.9999 | |
Q320 Set-up clearance? Additional distance between touch point and ball tip. Q320 is active in addition to the SET_UP column in the touch probe table. This value has an incremental effect. Input: 0...99999.9999 or PREDEF | |
Q260 Clearance height? Coordinate in the tool axis at which no collision between touch probe and workpiece (fixtures) can occur. This value has an absolute effect. Input: –99999.9999...+99999.9999 or PREDEF | |
Q1125 Traverse to clearance height? Positioning behavior between the touch points: –1: Do not move to the clearance height. 0, 1, 2: Move to the clearance height before and after the touch point. Pre-positioning occurs at FMAX_PROBE. Input: –1, 0, +1, +2 | |
Q309 Reaction to tolerance error? Reaction when tolerance is exceeded: 0: Do not interrupt program run when tolerance is exceeded. The control does not open a window with the results. 1: Interrupt program run when tolerance is exceeded. The control opens a window with the results. 2: The control does not open a window if rework is necessary. The control opens a window with results and interrupts the program if the actual position is at scrap level. Input: 0, 1, 2 | |
Q1120 Transfer position? Define which touch point will be used to correct the active preset: 0: No correction 1: Correction based on the 1st touch point. The control corrects the active preset by the amount of deviation between the nominal and actual position of the 1st touch point. 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 TCH PROBE 1430 PROBE POSITION OF UNDERCUT ~ | ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
|