Cycle 483 MEASURE TOOL (#17 / #1-05-1)
ISO programming
G483
Application
Refer to your machine manual!
To measure both the length and radius of a tool, program the touch probe cycle 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
- Measuring the tool while it is rotating and subsequently measuring the individual teeth
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 481 and 482.
Notes
- Set stopOnCheck (no. 122717) to TRUE
- You must then take steps to ensure that the NC program stops if the breakage tolerance is exceeded
- This cycle can be executed only in the FUNCTION MODE MILL machining mode.
- Before measuring a tool for the first time, enter the following data on the tool into the TOOL.T tool table: the approximate radius, the approximate length, the number of teeth, and the cutting direction.
- Cycle 483 supports neither turning tools nor dressing tools nor touch probes.
Note regarding machine parameters
- In the machine parameter probingCapability (no. 122723), the machine manufacturer defines the functionality of the cycle. This parameter allows you to permit tool length measurement with a stationary spindle and at the same time to inhibit tool radius and individual tooth measurements.
- Cylindrical tools with diamond surfaces can be measured while the spindle is stationary. To do so, in the tool table define the number of teeth CUT as 0 and adjust the machine parameter CfgTT. Refer to your machine manual.
Notes for individual tooth measurement of radius Q341=1
- Check the workpiece dimensions (for example, by using a workpiece touch probe)
- Check the workpiece optically in order to exclude broken tools
If the maximum angle of twist is exceeded, you should not carry out individual tooth measurement.
On tools with an even distribution of teeth, a maximum angle of twist can be defined as follows:
Abbreviation | Definition |
---|---|
ε | Maximum angle of twist |
h[tt] | Height of tool touch probe contact |
R | Tool radius |
x | Number of teeth of tool |
On tools with an uneven distribution of teeth, there is no calculation formula for the maximum angle of twist Check these tools optically in order to exclude breaks. You can measure wear indirectly by measuring the workpiece.
The higher the angle deviation 1 and the larger the tool radius, the more probably this behavior can occur.
- 1 Angle deviation
Cycle parameters
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.
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 TOOL CALL 12 Z | ||
12 TCH PROBE 483 MEASURE TOOL ~ | ||
| ||
| ||
|