Cycle 421 MEASURE HOLE (#17 / #1-05-1)
ISO programming
G421
Application
Touch probe cycle 421 measures the center point and diameter of a hole (or circular pocket). 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 421 MEASURE HOLE, HEIDENHAIN recommends using the more powerful Cycle 1401 CIRCLE PROBING.
Related topics
- Cycle 1401 CIRCLE PROBING
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 control derives the probing direction automatically from the programmed starting angle.
- Then, the touch probe moves along a circular arc, either at measuring height or at clearance height, to the next touch point 2 and probes again.
- The control positions the touch probe to touch point 3 and then to touch point 4 to probe two more times.
- 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 |
---|---|
Q151 | Actual value of center in reference axis |
Q152 | Actual value of center in minor axis |
Q153 | Actual value of diameter |
Q161 | Deviation at center of reference axis |
Q162 | Deviation at center of minor axis |
Q163 | Deviation from diameter |
Notes
- This cycle can be executed only in the FUNCTION MODE MILL machining mode.
- The smaller the stepping angle, the less accurately the control can calculate the hole dimensions. Minimum input value: 5°.
- 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 diameter Q262 must be between the minimum and maximum dimension (Q276/Q275).
- Parameters Q498 and Q531 have no effect in this cycle. You do not need to make any entries. These parameters have only been integrated for reasons of compatibility. If, for example, you import a program of the TNC 640 turning and milling control, you will not receive an error message.
Cycle parameters
Help graphic | Parameter |
---|---|
Q273 Center in 1st axis (nom. value)? Center of the hole in the main axis of the working plane. This value has an absolute effect. Input: –99999.9999...+99999.9999 | |
Q274 Center in 2nd axis (nom. value)? Center of the hole in the secondary axis of the working plane. This value has an absolute effect. Input: –99999.9999...+99999.9999 | |
Q262 Nominal diameter? Enter the diameter of the hole. Input: 0...99999.9999 | |
Q325 Starting angle? Angle between the main axis of the working plane and the first touch point. This value has an absolute effect. Input: –360.000...+360.000 | |
Q247 Intermediate stepping angle? Angle between two measuring points. The algebraic sign of the stepping angle determines the direction of rotation (negative = clockwise) in which the touch probe moves to the next measuring point. If you wish to probe a circular arc instead of a complete circle, then program the stepping angle to be less than 90°. This value has an incremental effect. Input: –120...+120 | |
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 | |
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 | |
Q301 Move to clearance height (0/1)? 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 | |
Q275 Maximum limit of size for hole? Maximum permissible diameter for the hole (circular pocket) Input: 0...99999.9999 | |
Q276 Minimum limit of size? Minimum permissible diameter for the hole (circular pocket) Input: 0...99999.9999 | |
Q279 Tolerance for center 1st axis? Permissible position deviation in the main axis of the working plane. Input: 0...99999.9999 | |
Q280 Tolerance for center 2nd axis? Permissible position deviation in the secondary axis of the working plane. 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 TCHPR421.TXT by default in the directory that also contains the associated NC program. 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? (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 | |
Q423 No. probe points in plane (4/3)? (optional) Define whether the control will use three or four touch points to measure the circle: 3: Use three measuring points 4: Use four measuring points (default setting) Input: 3, 4 | |
Q365 Type of traverse? Line=0/arc=1 (optional) Specify the path function to be used by the tool for moving between the measuring points if "traverse to clearance height" (Q301 = 1) is active. 0: Move in a straight line between machining operations 1: Move along a circular arc on the pitch circle diameter between machining operations Input: 0, 1 | |
Parameters Q498 and Q531 have no effect in this cycle. You do not need to make any entries. These parameters have only been integrated for reasons of compatibility. If, for example, you import a program of the TNC 640 turning and milling control, you will not receive an error message. |
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 421 MEASURE HOLE ~ | ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
|