Cycle 1493 EXTRUSION PROBING (#17 / #1-05-1)
ISO programming
G1493
Application
Cycle 1493 allows you to repeat the touch points of specific touch probe cycles along a straight line. In the cycle, you define the direction and the length of the extrusion, as well as the number of extrusion points.
The repetitions allow you, for example, to perform multiple measurements at different heights and to determine deviations based on the deflection of the tool. You can also use the extrusion to increase the accuracy during probing. Multiple measuring points help you ascertain contamination on the workpiece or rough surfaces.
In order to activate the repetition of specific touch points, you need to define Cycle 1493 before the touch probe cycle. Depending on the definition, this cycle will remain active for only the next cycle or for the entire NC program. The control interprets the extrusion in the input coordinate system I-CS.
The following cycles are capable of performing extrusions:
- PROBING IN PLANE (Cycle 1420, ISO: G1420) (#17 / #1-05-1), see Cycle 1420 PROBING IN PLANE (#17 / #1-05-1)
- PROBING ON EDGE (Cycle 1410, ISO: G1410) (#17 / #1-05-1), see Cycle 1410 PROBING ON EDGE (#17 / #1-05-1)
- PROBING TWO CIRCLES (Cycle 1411, ISO: G1411) (#17 / #1-05-1), see Cycle 1411 PROBING TWO CIRCLES (#17 / #1-05-1)
- INCLINED EDGE PROBING (Cycle 1412, ISO: G1412) (#17 / #1-05-1), see Cycle 1412 INCLINED EDGE PROBING (#17 / #1-05-1)
- INTERSECTION PROBING (Cycle 1416, ISO: G1416) (#17 / #1-05-1), see Cycle 1416 INTERSECTION PROBING (#17 / #1-05-1)
- POSITION PROBING (Cycle 1400, ISO: G1400) (#17 / #1-05-1), see Cycle 1400 POSITION PROBING (#17 / #1-05-1)
- CIRCLE PROBING (Cycle 1401, ISO: G1401) (#17 / #1-05-1), see Cycle 1401 CIRCLE PROBING (#17 / #1-05-1)
- PROBE SLOT/RIDGE (Cycle 1404, ISO: G1404) (#17 / #1-05-1), see Cycle 1404 PROBE SLOT/RIDGE (#17 / #1-05-1)
- PROBE POSITION OF UNDERCUT (Cycle 1430, ISO: G1430) (#17 / #1-05-1), see Cycle 1430 PROBE POSITION OF UNDERCUT (#17 / #1-05-1)
- PROBE SLOT/RIDGE UNDERCUT (Cycle 1434, ISO: G1434) (#17 / #1-05-1), see Cycle 1434 PROBE SLOT/RIDGE UNDERCUT (#17 / #1-05-1)
Result parameter Q
The control saves the results of the touch probe cycle in the following Q parameters:
Q parameter | Meaning |
---|---|
Q970 | Maximum deviation of the first touch point position |
Q971 | Maximum deviation of the second touch point position |
Q972 | Maximum deviation of the third touch point position |
Q973 | Maximum deviation of diameter 1 |
Q974 | Maximum deviation of diameter 2 |
Q975 | Maximum deviation of the width |
Result parameter QS
The control saves the individual results of all measuring points of an extrusion in the QS parameters QS97x. The result is ten characters long. The results are separated from each other by a space.
Example: QS970 = 0.12345678 -0.1234567 -0.1134567 0.11234567
QS parameter | Meaning |
---|---|
QS970 | Deviation of the position of the first probed object of an extrusion |
QS971 | Deviation of the position of the second probed object of an extrusion |
QS972 | Deviation of the position of the third probed object of an extrusion |
QS973 | Deviations of diameter 1 |
QS974 | Deviations of diameter 2 |
QS975 | Deviations of the width |
You can convert the individual results in the NC program, using string processing into numerical values and use them in evaluations, for example.
Example:
A touch probe cycle produces the following results within QS parameter QS970:
QS970 = 0.12345678 -0.1234567
The example below shows how to convert the results produced into numerical values.
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 QS0 = SUBSTR ( SRC_QS970 BEG0 LEN10 ) | ; Read out the first result from QS970 |
12 QL1 = TONUMB ( SRC_QS0 ) | ; Convert alphanumeric value from QS0 to a numerical value and assign it to QL0 |
13 QS0 = SUBSTR ( SRC_QS970 BEG11 LEN10 ) | ; Read out the second result from QS970 |
14 QL2 = TONUMB ( SRC_QS0 ) | ; Convert alphanumeric value from QS0 to a numerical value and assign it to QL2 |
Log function
Once probing has finished, the control generates a log file in HTML format. The log file contains the results of the 3D deviation in graphical and tabular form. The control saves the log file in the same folder in which the NC program is located.
The log file contains the following data in the main axis, secondary axis and tool axis depending on the selected cycle (e.g., circle center point and diameter):
- Actual probing direction (as a vector in the input system). The value of the vector corresponds to the configured probing path
- Defined nominal coordinate
- Upper and lower dimensions, as well as the determined deviation along the normal vector
- Measured actual coordinate
- Color coding of the values:
- Green: Good
- Orange: Rework
- Red: Scrap
- Extrusion points:
The horizontal axis represents the direction for the extrusion. The blue points are the individual measuring points. The red lines indicate the lower limit and the upper limit of the dimensions. If a value violates a specified tolerance, the control will show the area in red color in the graphic.
Notes
- This cycle can be executed only in the FUNCTION MODE MILL machining mode.
- If Q1145 > 0 and Q1146 = 0, then the control will perform the number of extrusion points at the same position.
- If you use Cycle 14011401 CIRCLE PROBING or Cycle 1411 PROBING TWO CIRCLES to perform an extrusion, the direction for the extrusion must be Q1140=+3; otherwise, the control will output an error message.
- If you use Cycle 1404 PROBE SLOT/RIDGE to perform an extrusion, the direction for the extrusion in the main axis must be Q1140=+1, or in the tool axis it must be Q1140=+3; otherwise, the control will output an error message.
- When defining the TRANSFER POSITION Q1120>0 within a touch probe cycle, the control will correct the preset by the mean of deviations. The control calculates this mean from all measured extrusion points of the probing object according to the programmed TRANSFER POSITION Q1120.
Example:
- Nominal position of touch point 1: 2.35 mm
- Results: QS970 = 2.30000000 2.35000000 2.40000000 2.50000000
Mean: 2.387500000 mm
The preset is corrected by the mean from the nominal position, in this case by 0.0375 mm.
Cycle parameters
Help graphic | Parameter |
---|---|
Q1140 Direction for extrusion (1-3)? 1: Extrusion in the direction of the main axis 2: Extrusion in the direction of the secondary axis 3: Extrusion in the direction of the tool axis Input: 1, 2, 3 | |
Q1145 Number of extrusion points? Number of measuring points that the cycle repeats over the length of the extrusion Q1146. Input: 1...99 | |
Q1146 Length of extrusion? Length over which the measuring points are repeated. Input: –99...+99 | |
Q1149 Extrusion: Modal duration? Effect of the cycle: 0: The extrusion is effective for only the next cycle. 1: The extrusion is effective until the end of the NC program. 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 1493 EXTRUSION PROBING ~ | ||
| ||
| ||
| ||
|
Example
With this example you can ascertain a form deviation, such as can occur when the tool is deflected. To do so you must first define Cycle 1493 EXTRUSION PROBING and specify whether it applies to just the subsequent cycle or for the entire program. After this cycle you can program any Cycle 14xx. This enables you to ascertain form deviations on various objects and actively intervene in the process (e.g., exchange tools).
Program sequence
- Cycle 1493 EXTRUSION PROBING
- Q1140=+1: Extrusion in the direction of the main axis
- Q1145=+4: Number of extrusion points
- Q1149=+0: The extrusion is effective for only the next cycle
- Cycle 1410 POSITION PROBING
- Q372=+2: Probing direction in minor axis
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.
0 BEGIN PGM TOUCHPROBE MM | |||
1 TOOL CALL 600 Z | |||
2 TCH PROBE 1493 EXTRUSION PROBING ~ | |||
| |||
| |||
| |||
| |||
3 TCH PROBE 1400 POSITION PROBING ~ | |||
| |||
| |||
| |||
| |||
| |||
| |||
| |||
| |||
| |||
4 CALL PGM 35 | ; Call the part program | ||
5 END PGM TOUCHPROBE MM |