What's new
What's new

Probing cycles on Fanuc - manual guide i vs renishaw inspection plus

Mike RzMachine

Cast Iron
Joined
Feb 4, 2007
Location
Utah
I'm installing an OMP40-2 spindle probe on my robodrill this week and wanted to get people's feedback on using the manual guide i probing functions built in vs buying inspection plus from renishaw (~$1100).

The main functions I want to use the probe for are fairly conventional,
1. setting fixture offsets in xyz as a separate step before running programs - i'd like to be able to do this easily through the control
2. setting fixture offsets within a program relative to existing part features - i'd like to set up my HSMWorks/Fusion postprocessor to generate the code to run these

It looks like I need to change my post processor to accommodate either approach. Currently, my post processor outputs the following, which seems to be macro numbers prior to inspection plus:

(PROBE1)
N25 T1 M06
(RENISHAW OMP40-2)
N30 G54
N40 G00 X0.0469 Y-0.372
N45 G43 Z15.4131 H01
N50 G65 P9832
N55 G65 P9810 Z9.4131 F50.
N60 G65 P9814 D2.0472 Z9.0556 Q0.35 R0.315 S4.
N65 G65 P9810 Z9.4131
N70 G00 Z15.4131
N75 G65 P9833

Inspection plus advises to initiate everything from P9901. Do the underlying macro numbers still match up with those called in the g-code above?

Also, has anyone used "Set and Inspect" from a tablet? do you like it? shown here: How to set a work offset quickly and easily using Set and Inspect on a Fanuc controller - YouTube

I'm trying to minimize manual data entry because I transpose numbers all the time. Set and inspect is included as a windows tablet app with inspection plus. Fanuc manuals are terse and cryptic, renishaw has excellent support, so maybe the cost difference gets absorbed very quickly in time saved.

Thanks,
Mike
 
I'm installing an OMP40-2 spindle probe on my robodrill this week and wanted to get people's feedback on using the manual guide i probing functions built in vs buying inspection plus from renishaw (~$1100).

The main functions I want to use the probe for are fairly conventional,
1. setting fixture offsets in xyz as a separate step before running programs - i'd like to be able to do this easily through the control
2. setting fixture offsets within a program relative to existing part features - i'd like to set up my HSMWorks/Fusion postprocessor to generate the code to run these

It looks like I need to change my post processor to accommodate either approach. Currently, my post processor outputs the following, which seems to be macro numbers prior to inspection plus:

(PROBE1)
N25 T1 M06
(RENISHAW OMP40-2)
N30 G54
N40 G00 X0.0469 Y-0.372
N45 G43 Z15.4131 H01
N50 G65 P9832
N55 G65 P9810 Z9.4131 F50.
N60 G65 P9814 D2.0472 Z9.0556 Q0.35 R0.315 S4.
N65 G65 P9810 Z9.4131
N70 G00 Z15.4131
N75 G65 P9833

Inspection plus advises to initiate everything from P9901. Do the underlying macro numbers still match up with those called in the g-code above?

Also, has anyone used "Set and Inspect" from a tablet? do you like it? shown here: How to set a work offset quickly and easily using Set and Inspect on a Fanuc controller - YouTube

I'm trying to minimize manual data entry because I transpose numbers all the time. Set and inspect is included as a windows tablet app with inspection plus. Fanuc manuals are terse and cryptic, renishaw has excellent support, so maybe the cost difference gets absorbed very quickly in time saved.

Thanks,
Mike
The O9901 is common command of Renishaw's GO PROBE. It is application program which operates the Inspection Plus. I personally hate these application programs, which by definition should facilitate the programming, but in fact are extremely not intuitive and force you to remember countless number of parameters which follow the O9901 command to perform measuring tasks.
Few years ago I had here discussion with undercover Renishaw guy, who claimed that he is getting Inspection Plus for free. I never had such luck.

Stefan
 
Manual guide i does probing?

I would like to know more.

I wouldnt use go-probe from within a program. The code you show is my preferred way.

Go probe is ok for setup, beats an indicator and edgefinder. But as Probe says above. You will have to have a paper cheat sheet or your smartphone with the go-probe app do do anything more than single surface hits and bores.Unless you are Johnny Mnemonic . And dont forget a decimal point or you are typing it all again. Its M1. A1. S101. not M1

The Go-probe macros comes with insp +.

If you are buying all the hardware at retail, I would want the inspection plus gratis.
 
My understanding is that renishaw stopped selling the older macros. They used to list a more basic package but now inspection+ is the most basic package they offered to me. I would actually prefer the older macro set but I don't know what that product was called.

On the manual guide I probing cycles, this video shows what it supports. For a 4 point round boss measurement, my control inserts G2023 with most of the same parameters that the renishaw macros take. I'll likely start with these cycles but I think the older renishaw package would be the most time efficient to work with my existing post processor (and knowledge base).
Fanuc probing video:
https://youtu.be/OiEH4mIfKgI

Thanks
Mike
 
the old macros were on a folder on the disc, The wizard wouldnt spit them out.

I think the "older" I was looking for back then was the old cal routines. without the m and k stuff
 
Renishaw clarified some details with me on inspection plus. The current macro package supports all of the legacy macro calls. Go probe functions as a layer above those to execute all of the sequencing required to switch on and off the probe and maybe simplifies stringing measurements together to set XY then Z with fewer lines of code.
 
I'm now up and running with inspection plus and the spindle probe. All works well.

One question I have for people familiar with fanuc 31i controls and maybe robodrills; The renishaw macros are populating data into #100-#150 variables, but some setting on my control is clearing those variables when the control returns from the macros, I think cleared during execution of M99.

I'm finding parameter 6001 bit 6 and 6037 affect this, but I'm not clear on how to interpret the parameter manual. Is there any downside to configuring the common variables to retain value after reset/m30? They are all initialized or overwritten in the renishaw macro's as far as I can tell. I'm going to dig in to find all of my current 6xxx parameter settings later today.

Thanks,
Mike
 
I'm now up and running with inspection plus and the spindle probe. All works well.

One question I have for people familiar with fanuc 31i controls and maybe robodrills; The renishaw macros are populating data into #100-#150 variables, but some setting on my control is clearing those variables when the control returns from the macros, I think cleared during execution of M99.

I'm finding parameter 6001 bit 6 and 6037 affect this, but I'm not clear on how to interpret the parameter manual. Is there any downside to configuring the common variables to retain value after reset/m30? They are all initialized or overwritten in the renishaw macro's as far as I can tell. I'm going to dig in to find all of my current 6xxx parameter settings later today.

Thanks,
Mike

Parameter 6001 bit 6, set to 1 and your #100-#199 not cleared on reset. As far as the GO Probe, it’s no different then the EZ set. Just different arguments. Either way unless it’s integrated into the GUI of the control your stuck having a cheat sheet of some sort with the cycles. I would put templates in your manual guide I or If you have the Hmi 31i you can save the templates to your favorite tab in the MDI screen.
 








 
Back
Top