Fanuc Probing Macro

[Mick]

Hi there,

 

We have two Toyodas (well, three actually), one FH100B, and two FA1050S's (in a FMS).

 

We're running probing cycles to centre the G54 work co-ordinate on castings.

 

However, we quite often get a "no touch" on the FMS machines running the same probing macro, because the "air stroke distance value", which from memory (I am typing this at home) is variable #505, or a similar number.

 

Not being familiar with Fanuc macro's, can someone tell me if these variable values are stored in the controller so I can view their current value? If so, in what section of the controller are they stored? (The controller on the FMS machines is a Fanuc 31i)

[Lars Christensen]

To my knowledge Fanuc have never made a probe. Are you sure it is not like a Marposs or Renishaw probe? in that case, it is there macro that is loaded into the control, and most likely them that can tell you what variable number they have the "air stroke distance value" assigned to. Of course if someone here have same make of probe and machine they might be able to retrieve it, but I have always got great help from the probe builders, like Renishaw with these kind of questions.

In regards to where they are getting stored in the control can be difficult to track down without tracing through the program itself or having the actual programmer in a headlock, because when macro programing you can input values one variable (like #505), retrieve them through another sub-macro program and restore them under another variable(Renishaw is famous for this).

[Mick]

It is a Renishaw probe. Sorry, I didn't make that clear.

 

It is a Renishaw probe on a Toyoda machining cente.

[Guest CNC Apps Guy 1]

#500 variables stay resident in the control until either cleared manually or through programs. They do not change unless written to.

 

Normally, the default setting stuff resides in O9760 (at least that's how our Renishaw guy sets it up).

 

HTH

[Mick]

So it is possible to view what the current #500 variables are set at? I'm assuming these are a kind of "user variable"?

 

We didn't have a Renishaw guy set ours up. It was set up at the Toyoda factory afaik :/

[Tim Johnson]

If you're using original Renishaw programs you can't set the overtravel value thru the control. It will need to be set in the program. Renishaw uses the value "Q" (#17) for the overtravel with a default of 10mm if "Q" is not set (shown) on the G65P9814 block. If you want the overtravel set to 3/4" add in that block Q.75

[Guest CNC Apps Guy 1]

YOu can view User Variables. Offset/Setting, ► (right arrow soft key), MACRO, brings you to the variables.

[Psychomill]

quote:

---

We didn't have a Renishaw guy set ours up. It was set up at the Toyoda factory afaik :/

---

Even so, it's probably still running Renishaw's Inspection Plus macros. Toyoda should've given you a programming book for it. But, as Tim said, generally these macros use a "Q" value for overtravel distance you can write in (with 10mm being the default XY skip distance and 4mm in Z).

[Tinhman]

shoud be the same with my machine Toyoda FA630

#500 Maximum distance probe will travel in a feed mode

#501 Touch sensor feedrate

#504 clearance distance of probe in x & y axes for all O.D probing

#505 Distance probe will stop (in x,y & z axis infeed)away from the datum plane prior to the final yet slower feed define in #500. #500 & #505

work in conjunction. Common practice is to set #505 to 33% of #500 value.

It is from my book.

Hope it help

[Mick]

Thanks for the info everyone.

 

I found in the controller where the macro values are stored (thanks CNC Apps Guy ).

 

Are these variable values stored in the probing macros? ie, if I was to change one of the the values in the controller, when I ran a probing cycle currently in a programme, would it reset those variables (if programmed in the current programme)?

 

Sorry for all the questions. I'm very new to probing :/

[Psychomill]

Tinhman,

 

Many installs will have common variables identified to be able to show what the settings are/will be for current cycles. Are you saying that by changing #500 numbers your probing will act differently? I can view those as well on my Toyodas (among many other machines) but changing them doesn't affect the actual running cycle since the local variables being set on the actual macro call line (or system default which is a written variable) will overwrite them (which is what Mick is wondering about).

 

 

 

(this is based on actual Inspection Plus installations. I have seen "custom" software written that acts the way you describe)

[iowajim62]

quote:

---

Are these variable values stored in the probing macros? ie, if I was to change one of the the values in the controller, when I ran a probing cycle currently in a programme, would it reset those variables (if programmed in the current programme)?

---

Yes, you should find the variable you need to adjust in O9724(Setting Macro).

Not all machines keep the macros under original file names/numbers but if they are you will find that O97xx programs are for calibrating the probe and O98xx programs are for measuring.

[Mick]

What I meant, was that if I change the variable on the table in the controller (offset/settings -> Right Arrow, then Macro, and then change the #505 to the required value), this would change the way the touch setter macro behaves?

 

Or do I have to change the value in the setting macro?

[iowajim62]

quote:

---

Or do I have to change the value in the setting macro?

---

Yes change it in the macro itself. Everytime you run the probe these macro programs are running in the background prior to actually touching off on the part/workpiece. If you go to single block you can watch the programs change back and forth but it takes forever pushing the "green" button a billion times HTH

[Mick]

Heh, thats what I was afraid of. Our controller doesn't have a O9724 programme, so I guess I'll have to go through the programmes to find the right one.

[Tinhman]

I may misunderstand something but i never changed my macro setting. I only changed the variable value in my machine control.

Default number in my machine set to

#500 .039

#504 .012

#505 .012

but when i machine castings, i changed it to

#500 .300

#504 .100

#505 .100

by doing that i do not get the alarm probe " no touch or touch early" very often.

Just hope it help

[Tinhman]

Sorry to clarify, my control is 15M and 16i

[Mick]

" no touch or touch early"

 

Yes, that is the problem we encounter. On our old Toyoda, the #505 is set to 3mm, and we dont have a problem, but on the new Toyodas, the #505 is 1mm, and we get the no touch or touch early error.

[Psychomill]

So Toyoda may have stuff of their own written and judging by Tinhman's actions it appears that it's adjustable by changing #5xx numbers/values.

 

I'd say just try changing the #505 value and see if it sticks and corrects your problem. Make notes of your changes so in case something isn't looking right, you can get back to it. The skip signal should keep you protected.

 

My Toyoda's have the Renishaw programs installed so I don't adjust in this manner...

[Tinhman]

Well, Mick, you could try this if you want (I NEVER try it before) and i think it will works for both machine. But you should making sure #600,#604 and #605 have not asign for anything.

 

Code

---------------------------------

 

N120T120(PROBE)

M6

T20

M1

G0G49G90G54B0.M11

M10

G0G90G54X0.Y0.M19

G43H120Z3.M50

#600=#500

#604=#504

#605=#505

#500=.300(or your metric number)

#504=.100(or your metric number)

#505=.100(or your metric number)

(AUTOMATIC OUTER DIAMETER CENTERING)

G65P8806X0.Y0.Z.1R7.0454S5.W54.B1.

#500=#600

#504=#604

#505=#605

M5

G0Z3.

G91G28Z0M19

G49G90

M1

------------------------------

 

Just hope it help

[Rick Henrickson The Boeing Co.]

there has to be macro programs you may have to switch you parameters to edit the O8000's or O9000"s but that is easy and make sure to protect them when you are done editing.