This workflow addresses a Renishaw NC4 non-contact tool setter installed on a Doosan HP5100 with a Fanuc control. The available evidence identifies the required macro calls and variables, but it does not establish that every HP5100 uses the same integration. Confirm the machine builder's implementation before running any macro.
Confirm the NC4 integration
Obtain Renishaw programming guide H-2000-6333-0B-A and verify that programs O9760, O9768, O9860, O9861, and O9862 exist on the control. Before moving an axis, confirm that the sensor is installed, its beam is physically aligned, its signal reaches the Fanuc control, and the configuration variables in O9760 match the machine.
Back up the existing macros and variables before changing them. The evidence does not provide the O9760 variable definitions, tool-offset selection method, safe coordinates, or machine clearances; derive those details from the machine-specific installation and programming documentation.
Calibrate the spindle speed
The reported first calibration step compensates for effects such as drip neglect. Start the spindle at the speed stored in variable #139, reported as either 500 or 1000 rpm, and then call the spindle-speed calibration macro. Tool-offset selection may also be required by the machine integration.
G65 P9768Do not choose between 500 and 1000 rpm arbitrarily. Read #139 and verify its configured value before executing the macro.
Check and correct beam alignment
Load the calibration tool and jog it to the tool-setting position approximately 10 mm above the beam. Confirm clearance from both tool-setter turrets throughout the measurement span, then call the alignment macro:
G65 P9860 T<tool-length-offset> D<measurement-span>T identifies the tool-length offset and D defines how widely the routine measures across the beam. Supply tool length or radius arguments only when they differ from the values configured in the setup macro. After the cycle, read #101 for the error viewed from the top of the beam and #102 for the error viewed from the side. Adjust the tool-setter base to bring both errors as close to zero as the installation permits, then repeat the check.
Establish the reference and measure tools
- Load the calibration tool, or provide arguments that accurately describe the loaded tool.
- Run
G65 P9861 B1.for final calibration. The routine measures the calibration tool's length and diameter to establish the reference. - Run the appropriate O9862 mode for production tool measurement, then verify the resulting offset before machining.
| Macro call | Reported function |
|---|---|
G65 P9862 B1. |
Measure tool length only |
G65 P9862 B2. |
Measure tool radius or diameter only |
G65 P9862 B3. |
Measure both length and radius or diameter |
The evidence does not identify whether the machine stores radius or diameter, which offset registers it writes, or what alarm behavior applies. Verify those integration details in the programming guide and with a known calibration tool before releasing automatic tool measurement.
FAQ
Which Renishaw guide covers the NC4 Fanuc macros?
The identified programming guide is H-2000-6333-0B-A. Use it to verify O9760 setup variables, macro arguments, offsets, and machine-specific prerequisites.
What do NC4 variables #101 and #102 indicate?
After G65 P9860, #101 reports alignment error viewed from the top of the beam and #102 reports error viewed from the side. Adjust the tool-setter base and repeat the measurement to bring both values close to zero.
Which NC4 macro measures tool length and diameter?
Use G65 P9862 B3. to measure both. Use B1. for length only or B2. for radius or diameter only, subject to the machine's configured offset convention.
