Cycle 427 MEASURE COORDINATE
ISO programming
G427
Application
Touch probe cycle 427 measures a coordinate in a selectable axis and saves the value in a Q parameter. If you define the corresponding tolerance values in the cycle, the control makes a nominal-to-actual value comparison and saves the deviation values in Q parameters.
Instead of Cycle 427 MEASURE COORDINATE, HEIDENHAIN recommends using the more powerful Cycle 1400 POSITION PROBING.
Related topics
- Cycle 1400 POSITION PROBING
Cycle run
- The control positions the touch probe to the pre-position of the first touch point 1, using positioning logic.
- Then the control positions the touch probe to the specified touch point 1 in the working plane and measures the actual value in the selected axis.
- Finally, the control returns the touch probe to the clearance height and saves the measured coordinate in the following Q parameters:
Q parameter | Meaning |
---|---|
Q160 | Measured coordinate |
Q168 | Deviation of the measured coordinate |
Notes
- This cycle can be executed only in the FUNCTION MODE MILL machining mode.
- If an axis of the active working plane is defined as the measuring axis (Q272 = 1 or 2), the control will perform a tool radius compensation. The control determines the direction of compensation from the defined traversing direction (Q267).
- If the touch probe axis is defined as the measuring axis (Q272 = 3), the control will perform a tool length compensation.
- 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 measuring height Q261 must be between the minimum and maximum dimension (Q276/Q275).
- If parameter Q330 references a milling tool, the information in parameters Q498 and Q531 has no effect
- If parameter Q330 references a turning tool, the following applies:
- Parameters Q498 and Q531 must have values in them.
- The information in parameters Q498 and Q531, for example from Cycle 800, has to match this information.
- If the control corrects the position of the turning tool, the corresponding values in rows DZL and DXL, respectively, will be corrected.
- The control also monitors the breakage tolerance, which is defined in column LBREAK.
Cycle parameters
Help graphic | Parameter |
---|---|
Q263 1st measuring point in 1st axis? Coordinate of the first touch point in the main axis of the working plane. This value has an absolute effect. Input: –99999.9999...+99999.9999 | |
Q264 1st measuring point in 2nd axis? Coordinate of the first touch point in the secondary axis of the working plane. This value has an absolute effect. Input: –99999.9999...+99999.9999 | |
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 | |
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 | |
Q272 Meas. axis (1/2/3, 1=ref. axis)? Axis in which the measurement will be made: 1: Main axis = measuring axis 2: Secondary axis = measuring axis 3: Touch probe axis = measuring axis Input: 1, 2, 3 | |
Q267 Trav. direction 1 (+1=+ / -1=-)? Direction in which the touch probe will approach the workpiece: –1: Negative traverse direction +1: Positive traverse direction Input: –1, +1 | |
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 | |
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 TCHPR427.TXT in the folder that also contains the associated NC program. 2: Interrupt the program run and display the measuring log on the control screen.Resume the NC program run with NC Start. Input: 0, 1, 2 | |
Q288 Maximum limit of size? (optional) Maximum permissible value Input: –99999.9999...+99999.9999 | |
Q289 Minimum limit of size? (optional) Minimum permissible value Input: –99999.9999...+99999.9999 | |
Q309 PGM stop if tolerance exceeded? (optional) 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? (optional) 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 | |
Q498 Reverse tool (0=no/1=yes)? (optional) Only relevant if you have entered a turning tool in parameter Q330 before. For proper monitoring of the turning tool, the control requires the exact machining situation. Therefore, enter the following: 1: Turning tool is mirrored (rotated by 180°) by, for example, Cycle 800 and parameter Reverse the tool Q498 = 1 0: Turning tool corresponds to the description in the turning tool table (toolturn.trn); no modification by, for example , Cycle 800 and parameter Reverse the tool Q498 = 0 Input: 0, 1 | |
Q531 Angle of incidence? (optional) Only relevant if you have entered a turning tool in parameter Q330 before. Enter the angle of incidence (inclination angle) between turning tool and workpiece during machining (e.g., from Cycle 800, Angle of incidence? Q531). Input: -180...+180 |
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 427 MEASURE COORDINATE ~ | ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
|