Cycle 444 PROBING IN 3-D (#17 / #1-05-1)
ISO programming
G444
Application
Refer to your machine manual.
This function must be enabled and adapted by the machine manufacturer.
Cycle 444 checks one specific point on the surface of a part. This cycle is used, for example, to measure free-form surfaces of moldmaking parts. It can be determined whether a point on the surface of the part lies in an undersize or oversize range compared to a nominal coordinate. The operator can subsequently perform further machining steps, such as reworking.
Cycle 444 probes any point in three dimensions and determines the deviation from a nominal coordinate. A normal vector, defined in parameters Q581, Q582, and Q583, is used for this purpose. The normal vector is perpendicular to an imagined surface in which the nominal coordinate is located. The normal vector points away from the surface and does not determine the probing path. It is advisable to determine the normal vector with the help of a CAD or CAM system. A tolerance range QS400 defines the permissible deviation between the actual and nominal coordinate along the normal vector. This way you define, for example, that the program is to be interrupted if an undersize is detected. Additionally, the control outputs a log and the deviations are stored in the Q parameters listed below.
Cycle run
- Starting from the current position, the touch probe traverses to a point on the normal vector that is at the following distance from the nominal coordinate: Distance = ball-tip radius + SET_UP value from the tchprobe.tp table (TNC:\table\tchprobe.tp) + Q320. Pre-positioning takes a clearance height into account.
- The touch probe then approaches the nominal coordinate. The probing distance is defined by DIST, not by the normal vector! The normal vector is only used for the correct calculation of the coordinates.
- After the control has saved the position, the touch probe is retracted and stopped. The control saves the measured coordinates of the contact point in Q parameters.
- Finally, the control retracts the touch probe by the value that you defined in parameter Q320 in the direction opposite to the probing direction.
Result parameters
The control stores the probing results in the following parameters:
Q parameter | Meaning |
---|---|
Q151 | Measured position in main axis |
Q152 | Measured position in secondary axis |
Q153 | Measured position in tool axis |
Q161 | Measured deviation in main axis |
Q162 | Measured deviation in secondary axis |
Q163 | Measured deviation in tool axis |
Q164 | Measured 3D deviation
|
Q183 | Workpiece status:
|
Log function
Once probing has finished, the control generates a log in HTML format. The log includes the results from the main, secondary, and tool axes as well as the 3D error. The control saves the log in the same folder in which the *.h file is located (as long as no path has been configured for FN 16).
The log contains the following data on the main, secondary, and tool axes:
- Actual probing direction (as a vector in the input system). The value of the vector corresponds to the configured probing path.
- Defined nominal coordinate
- If a tolerance QS400 was defined: Upper and lower dimensions are output, as well as the determined deviation along the normal vector
- Ascertained actual coordinate
- Colored display of the values (green for "good," orange for "rework," red for "scrap")
Notes
- This cycle can be executed only in the FUNCTION MODE MILL machining mode.
- In order to obtain exact results from the touch probe being used, you need to perform 3D calibration before executing Cycle 444. 3D calibration requires 3D-ToolComp.
- Cycle 444 generates a measuring log in HTML format.
- An error message is output if Cycle 8 MIRRORING, Cycle 11 SCALING FACTOR, or Cycle 26 AXIS-SPECIFIC SCALING is active before Cycle 444 is run.
- For probing, an active TCPM will be taken into account. While the TCPM is active, probing of positions is possible even if the position resulting from the Tilt working plane function is inconsistent with the current position of the rotary axes.
- If your machine is equipped with a feedback-controlled spindle, you should activate angle tracking in the touch probe table (TRACK column). This generally increases the accuracy of measurements with a 3D touch probe.
- Cycle 444 references all coordinates to the input system.
- The control writes the measured values to return parameters.
- The workpiece status good/rework/scrap is set via Q parameter Q183, independent of parameter Q309.
Notes about machine parameters
- Depending on the setting of the optional machine parameter chkTiltingAxes (no. 204600), the control will check during probing whether the position of the rotary axes matches the tilting angles (3D-ROT). If that is not the case, the control displays an error message.
- In the optional machine parameter trackAsync (no. 122503), the machine manufacturer defines whether the control orients the spindle for probing during prepositioning.
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 | |
Q294 1st measuring point in 3rd axis? Coordinate of the first touch point in the touch probe axis. This value has an absolute effect. Input: –99999.9999...+99999.9999 | |
Q581 Surface-normal in ref. axis? Enter here the surface normal in the direction of the main axis. The surface normal of a point is normally output by a CAD/CAM system. Input: –10...+10 | |
Q582 Surface-normal in minor axis? Enter here the surface normal in the direction of the secondary axis. The surface normal of a point is normally output by a CAD/CAM system. Input: –10...+10 | |
Q583 Surface-normal in tool axis? Enter here the surface normal in the direction of the tool axis. The surface normal of a point is normally output by a CAD/CAM system. Input: –10...+10 | |
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 | |
QS400 Tolerance value? Specify a tolerance band that will be monitored by the cycle. The tolerance defines the deviation permitted along the surface normal. This deviation is determined between the nominal coordinate and the actual coordinate of the workpiece. (The surface normal is defined by Q581 to Q583, and the nominal coordinate is defined by Q263, Q264, and Q294.) The tolerance value is distributed over the axes, depending on the normal vector (see examples). Examples
Input: Max. 255 characters | |
Q309 Reaction to tolerance error? 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 when tolerance is exceeded; do not output an error message 1: Interrupt program run when tolerance is exceeded and output an error message 2: If the value of the measured actual coordinate along the surface normal vector is less than the nominal coordinate, the control displays a message and interrupts the NC program run. However, there will be no error message if the value of the measured actual coordinate is greater than the nominal coordinate. Input: 0, 1, 2 |
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 444 PROBING IN 3-D ~ | ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
|