ISO programming
G483
G483
Refer to your machine manual!
To measure both the length and radius of a tool, program the touch probe cycle 33 or 483 (Differences between Cycles 30 to 33 and Cycles 480 to 483). This cycle is particularly suitable for the first measurement of tools, as it saves time when compared with individual measurement of length and radius. Input parameters allow you to select which of the two following methods will be used to measure the tool:
Measuring the tool while it is rotating:
The control measures the tool in a fixed programmed sequence. First, if possible, it measures the tool length, and then the tool radius.
Measuring the individual teeth:
The control measures the tool in a fixed programmed sequence. First it measures the tool radius, then the tool length. The sequence of measurement is the same as for touch probe cycles 31 and 32 as well as 481 and 482.
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 length and the measured tool radius are written to columns L and R of the TOOL.T tool table, and the tool compensation is set to DL = 0 and DR = 0. If there is already a value in TOOL.T, it will be overwritten. 1: The measured tool length and the measured tool radius are compared to the tool length L and tool radius R in TOOL.T. The control calculates the deviation from the stored value and enters them into TOOL.T as the delta values DL and DR. The deviation is also available in the Q parameters Q115 and Q116. If the delta value is greater than the permissible tool length or tool radius tolerance for wear or break detection, the control will lock the tool (status L in TOOL.T). 2: The measured tool length and the measured tool radius are compared to the tool length L and tool radius R in TOOL.T. The control calculates the deviation from the stored values and writes it to the Q parameter Q115 or Q116. Nothing is entered under L, R, or DL, 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 483 MEASURE TOOL ~ | ||
| ||
| ||
|
Cycle 33 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 (LTOL or/and RTOL exceeded) 2.0: Tool is broken (LBREAK or/and 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 33.0 MEASURE TOOL |
13 TCH PROBE 33.1 CHECK:0 |
14 TCH PROBE 33.2 HEIGHT:+120 |
15 TCH PROBE 33.3 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 33.0 MEASURE TOOL |
13 TCH PROBE 33.1 CHECK:1 Q5 |
14 TCH PROBE 33.2 HEIGHT:+120 |
15 TCH PROBE 33.3 PROBING THE TEETH:1 |