Cycle 425 MEASURE INSIDE WIDTH (#17 / #1-05-1)
ISO programming
G425
Application
Touch probe cycle 425 measures the position and width of a slot (or pocket). If you define the corresponding tolerance values in the cycle, the control makes a nominal-to-actual value comparison and saves the deviation value in a Q parameter.
Instead of Cycle 425 MEASURE INSIDE WIDTH, HEIDENHAIN recommends using the more powerful Cycle 1404 PROBE SLOT/RIDGE.
Related topics
- Cycle 1404 PROBE SLOT/RIDGE
Cycle run
- The control positions the touch probe to the pre-position of the first touch point 1, using positioning logic.
- Next, the touch probe moves to the entered measuring height and probes the first touch point at the probing feed rate (F column). The first probing is always in the positive direction of the programmed axis.
- If you enter an offset for the second measurement, the control then moves the touch probe (if required, at clearance height) to the next touch point 2 and probes that point. If the nominal length is large, the control moves the touch probe to the second touch point at rapid traverse. If you do not enter an offset, the control measures the width in the exact opposite direction.
- Finally, the control returns the touch probe to the clearance height and saves the actual values and deviations in the following Q parameters:
Q parameter | Meaning |
---|---|
Q156 | Actual value of measured length |
Q157 | Actual value of the centerline |
Q166 | Deviation of the measured length |
Notes
- This cycle can be executed only in the FUNCTION MODE MILL machining mode.
- The control will reset an active basic rotation at the beginning of the cycle.
Notes on programming
- Before defining this cycle, you must have programmed a tool call to define the touch probe axis.
- The nominal length Q311 must be between the minimum and maximum dimension (Q276/Q275).
Cycle parameters
Help graphic | Parameter |
---|---|
Q328 Starting point in 1st axis? Starting point for probing in the main axis of the working plane. This value has an absolute effect. Input: –99999.9999...+99999.9999 | |
Q329 Starting point in 2nd axis? Starting point for probing in the secondary axis of the working plane. This value has an absolute effect. Input: –99999.9999...+99999.9999 | |
Q310 Offset for 2nd measuremnt (+/-)? Distance by which the touch probe is offset before the second measurement. If you enter 0, the control does not offset the touch probe. This value has an incremental effect. Input: –99999.9999...+99999.9999 | |
Q272 Measuring axis (1=1st / 2=2nd)? Axis in the working plane in which the measurement will be performed: 1: Main axis = measuring axis 2: Secondary axis = measuring axis Input: 1, 2 | |
Q261 Measuring height in probe axis? Coordinate of the ball tip center in the touch probe axis in which the measurement will be performed. This value has an absolute effect. Input: –99999.9999...+99999.9999 | |
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 | |
Q311 Nominal length? Nominal value of the length to be measured Input: 0...99999.9999 | |
Q288 Maximum limit of size? Maximum permissible length Input: 0...99999.9999 | |
Q289 Minimum limit of size? Minimum permissible length Input: 0...99999.9999 | |
Q281 Measuring log (0/1/2)? Define whether the control will create a measuring log: 0: Do not create a measuring log 1: Create a measuring log: The control will save the log file named TCHPR425.TXT in the folder that also contains the .h file 2: Interrupt program run and display the measuring log on the control screen. Resume the NC program run with NC Start. Input: 0, 1, 2 | |
Q309 PGM stop if tolerance exceeded? Define whether in the event of a violation of tolerance limits the control will interrupt program run and output an error message: 0: Do not interrupt program run; no error message 1: Interrupt program run and output an error message Input: 0, 1 | |
Q330 Tool for monitoring? Define whether the control should perform tool monitoring: 0: Monitoring not active > 0: Number or name of the tool used for machining. Via selection in the action bar, you have the option of applying a tool directly from the tool table. Input: 0...99999.9 or max. 255 characters | |
Q320 Set-up clearance? (optional) Additional distance between touch point and ball tip. Q320 is added to SET_UP (touch probe table), and is only active when the preset is probed in the touch probe axis. This value has an incremental effect. Input: 0...99999.9999 or PREDEF | |
Q301 Move to clearance height (0/1)? (optional) Define how the touch probe will move between the measuring points: 0: Move to measuring height between measuring points 1: Move to clearance height between measuring points 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 TCH PROBE 425 MEASURE INSIDE WIDTH ~ | ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
|