Renishaw NC4 Laser Tool Setter with Installation and Training

[gavintwopies]

HI all,

just thought id give this a go this is the 3rd company ive worked for now that have a doosan hp5100 which have the NC4 renishaw laser height setter built into it as standard, yet not none of the operators or programmers know how to get it working and as ive never been working somewhere when the machines been installed ive never been there to catch the trainin or get any notes on how to use it, i have however used the ealier touch probes on the older doosans and mori seiki machines.

also i just cant find any videos or info online either.

Similar Threads:

• OTB with Renishaw tool setter help request
• Renishaw tool setter repair
• Leveling Renishaw OTS (tool setter)
• OTS Renishaw Tool setter help, Actually using it?
• OTS Renishaw Tool setter help

[PNaedele]

I just got one of these sensors back up and running after years of being disabled.

Renishaw does have a few installation manuals online that should help with physical setup. NC4 non-contact tool setter

If you can find the Programming guide, H-2000-6333-0B-A, it will take you through the setup variables O9760, and calibration steps.

So I'm assuming that the sensor is properly installed and aligned and the signal is connected and working on your control (Fanuc) and that the setup variables contained in program O9760 are correct for your machine configuration.

The first step in calibration is to calibrate the spindle speed for things like drip neglect. The programming guide says to start the spindle at the speed as set by #139 (500 or 1000 rpm) and run G65P9768 (you may have to select tool offset).

The second step is to check alignment of the beam. It says to load the calibration tool in the spindle and jog it to the tool setting position about 10mm above the beam. This will check the beam position from the top and sides at several points along the beam and just be careful that the tool doesn't crash into the toolsetter turrets during this. The format is G65 P9860 T(tool length offset number) D(span of how wide across the beam you want to measure). There is also tool length and radius arguments you can pass if they differ from what's in the setup variable macro.

After that's done macro variables #101 and #102 will tell you the alignment error. #101 is error looking from the top of the beam and #102 is from the side. The goal is to get these as close to zero as possible by adjusting the tool setter base, then your beam is properly aligned and parallel to whatever axis it's supposed to be.

There's another method to check this by using a tool with an offset pin, but I don't have experience with this.

Now for the actual calibration. You need the calibration tool loaded, or feed it arguments that accurately represent the tool you have loaded.

G65 P9861 B1.

B1. is for the final calibration. It will measure the length and diameter of the tool and that will be the reference.

Normal tool length setting is in this format:

G65P9862B1. for length only, G65P9862B2. for radius/diameter only. G65P9862B3. for both.

Tons of other options for measuring tools too. If you have the programming guide this is all explained in detail.