Cycle 411 PRESET OUTS. RECTAN (#17 / #1-05-1)
ISO programming
G411
Application
Touch probe cycle 411 finds the center of a rectangular stud and defines this position as the datum. If desired, the control can also write the center point coordinates to a datum table or the preset table.
Instead of Cycle 411 PRESET OUTS. RECTAN, HEIDENHAIN recommends using the more powerful Cycle 1403 RECTANGLE PROBING.
Related topics
- Cycle 1403 RECTANGLE 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).
- Then the touch probe moves either paraxially 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.
- The control returns the touch probe to the clearance height.
- Depending on the cycle parameters Q303 and Q305, the control processes the determined preset, (see Fundamentals of touch probe cycles 408 to 419 for preset setting).
- Then the control saves the actual values in the Q parameters listed below.
- If desired, the control subsequently determines the preset in the touch probe axis in a separate probing operation.
Q parameter | Meaning |
---|---|
Q151 | Actual value of center in reference axis |
Q152 | Actual value of center in minor axis |
Q154 | Actual value of side length in the reference axis |
Q155 | Actual value of side length in the minor axis |
Notes
- Do not activate the following cycles before the use of touch probe cycles:
- Cycle 7 DATUM SHIFT
- Cycle 8 MIRRORING
- Cycle 10 ROTATION
- Cycle 11 SCALING FACTOR
- Cycle 26 AXIS-SPECIFIC SCALING
- Reset any coordinate transformations beforehand.
- Before the cycle definition, you must have programmed a tool call to define the touch probe axis.
- 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.
Cycle parameters
Help graphic | Parameter |
---|---|
Q321 Center in 1st axis? Center of the stud in the main axis of the working plane. This value has an absolute effect. Input: –99999.9999...+9999.9999 | |
Q322 Center in 2nd axis? Center of the stud in the secondary axis of the working plane. This value has an absolute effect. Input: –99999.9999...+99999.9999 | |
Q323 First side length? Length of stud parallel to the main axis of the working plane. This value has an incremental effect. Input: 0...99999.9999 | |
Q324 Second side length? Length of stud parallel to the secondary axis of the working plane. This value has an incremental effect. Input: 0...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 | |
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 | |
Q305 Number in table? Enter the row number from the preset table / datum table in which the control saves the center coordinates. Depending on Q303, the control writes the entry to the preset table or datum table. If Q303=1, the control will write the data to the preset table. If Q303=0, then the control describes the datum table. The datum is not automatically activated. Input: 0...99999 | |
Q331 New preset in reference axis? Coordinate in the main axis at which the control will set the calculated stud center. Default setting = 0. This value has an absolute effect. Input: –99999.9999...+99999.9999 | |
Q332 New preset in minor axis? Coordinate in the secondary axis at which the control will set the calculated stud center. Default setting = 0. This value has an absolute effect. Input: –99999.9999...+99999.9999 | |
Q303 Meas. value transfer (0,1)? Define whether the calculated preset will be saved in the datum table or in the preset table: -1: Do not use. Is entered by the control when old NC programs are loaded see Application 0: Write the calculated preset to the active datum table. The reference system is the active workpiece coordinate system. 1: Write the calculated preset to the preset table. Input: -1, 0, +1 | |
Q381 Probe in TS axis? (0/1) (optional) Define whether the control will also set the preset in the touch probe axis: 0: Do not set the preset in the touch probe axis 1: Set the preset in the touch probe axis Input: 0, 1 | |
Q382 Probe TS axis: Coord. 1st axis? (optional) Coordinate of the touch point in the main axis of the working plane; the preset will be set at this point in the touch probe axis. Only effective if Q381 = 1. This value has an absolute effect. Input: –99999.9999...+99999.9999 | |
Q383 Probe TS axis: Coord. 2nd axis? (optional) Coordinate of the touch point in the secondary axis of the working plane; the preset will be set at this point in the touch probe axis. Only effective if Q381 = 1. This value has an absolute effect. Input: –99999.9999...+99999.9999 | |
Q384 Probe TS axis: Coord. 3rd axis? (optional) Coordinate of the touch point in the touch probe axis; the preset will be set at this point in the touch probe axis. Only effective if Q381 = 1. This value has an absolute effect. Input: –99999.9999...+99999.9999 | |
Q333 New preset in TS axis? (optional) Coordinate in the touch probe axis at which the control will set the preset. Default setting = 0. This value has an absolute effect. Input: –99999.9999...+99999.9999 |
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 411 PRESET OUTS. RECTAN ~ | ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
|