ISO programming
G482
G482
Refer to your machine manual!
If you want to measure the tool radius, program the touch probe cycle 32 or 482 (Differences between Cycles 30 to 33 and Cycles 480 to 483). Input parameters allow you to select which of the two following methods will be used to measure the tool radius:
The control pre-positions the tool to be measured to a position at the side of the touch probe head. The distance from the face of the milling tool to the upper edge of the touch probe head is defined in offsetToolAxis (no. 122707). The control probes the tool radially while it is rotating. If you have programmed a subsequent measurement of individual teeth, the control will measure the radius of each tooth with the aid of oriented spindle stops.
Note the following sequence for setting up grinding tools
Help graphic | Parameter |
---|---|
Q340 Tool measurement mode (0-2)? Define whether and how the measured data will be entered in the tool table. 0: The measured tool radius is written to column R of the TOOL.T tool table, and the tool compensation is set to DR = 0. If there is already a value in TOOL.T, it will be overwritten. 1: The measured tool radius is compared to the tool radius R from TOOL.T. The control calculates the deviation from the stored value and enters it into TOOL.T as the delta value DR. The deviation is also available in the Q parameter Q116. If the delta value is greater than the permissible tool radius tolerance for wear or break detection, the control will lock the tool (status L in TOOL.T). 2: The measured tool radius is compared to the tool radius from TOOL.T. The control calculates the deviation from the stored value and writes it to Q parameter Q116. Nothing is entered under R or DR in the tool table. Input: 0, 1, 2 | |
Q260 Clearance height? Enter the position in the spindle axis at which there is no danger of collision with the workpiece or fixtures. The clearance height is referenced to the active workpiece preset. If you enter such a small clearance height that the tool tip would lie below the top of the probe contact, the control automatically positions the tool above the top of the probe contact (safety zone from safetyDistStylus). Input: –99999.9999...+99999.9999 | |
Q341 Probe the teeth? 0=no/1=yes Define whether the control will measure the individual teeth (maximum of 20 teeth) 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.
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 TOOL CALL 12 Z | ||
12 TCH PROBE 482 CAL. TOOL RADIUS ~ | ||
| ||
| ||
|
Cycle 32 includes an additional parameter:
Help graphic | Parameter |
---|---|
Parameter number for result? Parameter number in which the control stores the status of the measurement: 0.0: Tool is within the tolerance 1.0: Tool is worn (RTOL exceeded) 2.0: Tool is broken (RBREAK exceeded). If you do not wish to use the result of measurement within the NC program, answer the dialog prompt with NO ENT Input: 0...1999 |
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.
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 TOOL CALL 12 Z |
12 TCH PROBE 32.0 CAL. TOOL RADIUS |
13 TCH PROBE 32.1 CHECK:0 |
14 TCH PROBE 32.2 HEIGHT:+120 |
15 TCH PROBE 32.3 PROBING THE TEETH:0 |
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.
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 TOOL CALL 12 Z |
12 TCH PROBE 32.0 CAL. TOOL RADIUS |
13 TCH PROBE 32.1 CHECK:1 Q5 |
14 TCH PROBE 32.2 HEIGHT:+120 |
15 TCH PROBE 32.3 PROBING THE TEETH:1 |