GEOMETRIC INSPECTION WITH RENISHAW PROBE AND CNC FANUC

[info]

Good morning,
I would like to perform the geometric inspection for example of your attached "probe sample part" file, but my Fanuc post downloaded from your site is not working.
I would like to understand how to modify it in order to make it effective.
In attachment file and post processor that I use
Best regards

[AchimN]

There is a specific version of the fanuc posts which has support for inspection:

https://cam.autodesk.com/hsmposts?p=fanuc_inspection

[info]

Good morning @AchimN ,
I downloaded the recommended post processor, but still can't write the program as you see in the attachment.
the cycles I tried are the ones inside the red cloud.
Thank you, kind regards

[AchimN]

The post processor is complaining that following properties needs to be defined:

[Richard.stubley · Accepted solution]

@info,

We intentionally leave these blank and error if they have not been filled in, you can imagine how bad things can get if we don't turn the probe on correctly and try to probe. 

What you need to define is:

Probe on command, standard renishaw default is P9832. So try G65 P9832 to call this sub program in MDI with the probe in the spindle.

If your probe turns on then you know thats correct.

Probe off command, standard default is P9833

However you may also know M codes for your machine that you can use just as well as these sub program calls.

The next 3 are macro variables that are for your calibration data. 

you are looking for a 3 values normally aground macro variable #500.

The calibrated radi will be just less than the actual radi (Default #501)

The eccentricity (run-out in X) will be close to 0 (Default #502)

The eccentricity (run-out in X) will also be close to 0 (Default#503)

If you can send me a image of your macro variables at around 500 then I will be able to tell you what they are.

[info]

Hi @Richard.stubley   ,
the probe power on command is exactly G65 P9832 and the power off command is exactly G65 P9833.
variables #500 ... I have them on #700 as you can see from the picture.
cordial greetings

[info]

then this is a Mitsubishi cnc (almost equal to fanuc) for example the other normal probing cycles I use them also on a Fanuc 31i machine and they work on both.

[Richard.stubley]

@info , perfect well done for finding those.

So you will need to put 700 as the calibrated radi (this will then take the average of 700 and 701)

702 will be X eccentricity.

703 will be Y eccentricity.

FYI, if you havent already you will need to know where your DPRNT sends the data to.

The Fanuc has 2 output channels, 20 and 21. if Parameter 110 bit 0 is a 0, you are using parameter 20, if its a 1 you are using 21. Now the value of 20 or 21 lets you know where the file is being written to, 0 serial connection, 5 data server, 4 memory card, 9 FTP, 15 Ethernet, 17 USB.

[info]

the data is written on the USB stick, the problem is that the PCLOS command must not be written before the POPEN otherwise it freezes

[Richard.stubley]

@info,

That is interesting, we put that in because most controllers cant POPEN if the port is already open so we make sure we close it first. A very easy post mod though. You will just have to make sure that if you ever stop a program before it finishes you will have to PCLOS in MDI.

Also make sure you have the measure federate correctly specified in Fusion, this needs to be the same Feedrate that the Renishaw cycles use, the easiest way to find it is just use one of their cycles to probe something and look at the feedrate when the probe touches. If renishaw is using 2 touch probing then get the feedrate of the second touch. 

And finally as the feedrate is so important, ensure you always probe at 100%. Renishaw actually override your feedrate to set it at 100%, we don't do this to allow you to run the first few cycles slowly, but you always need to run at 100% to get good reliable results. 

Please let me know how you get on with this, we are always looking for feedback on our inspection functions. 

[info]

Good morning @Richard.stubley ,
thank you for your availability and punctuality.
I have now performed a simple probing cycle as you see the attachment and also the error it gives me.
greetings

[info]

This is the file with the touch probe

[Richard.stubley]

@info could you please turn commissioning mode off in the post properties and give it another go. Thank you.

[info]

I did the test as you so kindly requested and now you give it to me here.

[Richard.stubley]

I Think this may be the difference between the Mitsubushi and Fanuc tool length tables.

Does your machine have both length and wear in the tool table or just length?

Could you type this into MDI then check the value of #1

#1=#[2000 + #4111]

M0

I think this will be what we need to sort. 

[info]

I also ran this test.
as you imagined it would alert me.
I'm also sending you the tool correction table where I have both diameter wear and tool length check.
I hope that's clear enough.

[Richard.stubley]

@info, Ok what we are trying to do here is find the tool length of the active tool in the spindle. It look like one or more of the Macros are different to what we have in the generic fanuc. So lets break them down to find out which ones are the issue.

#1=#4111

M0

#2=#2000

M0

#3=#2001

M0

#4=#2002

M0

If you could run each of those individually please and let me know which ones, if any work.

[info]

@Richard.stubley , 

Perfect, I analyzed them all and the only macro that gives me the error is the #2=#2000

[Richard.stubley]

Sorry. could you also let me know the value it give back for each of them aswell.

[info]

@Richard.stubley 

that's how kindly requested:
#1=#4111=0.000
#2=#2000=
#3=#2001=207.384
#4=#2002=219.005