Fanuc 31i ... Probing under G68.2?

[dstryr]

I've been using Siemens 840d machine and 828 controls since I started doing 5th axis and I've always been able to probe results while under Cycle800.

I inquired about doing this on my new Yasda machine and the service rep didnt think it was possible. Is there a special way to do this or does renishaw not support this?

 

[Guest]

Yes it is possible, HOWEVER, you cannot probe with WSEC or TCP active.

 

I've done it - last week on a 30i-A. It's all about formatting. :

[dstryr]

What a tease....

lol

 

Any suggestions?
I guess I'm just spoiled with the Siemens control being so much superior...

 

Probing at an angled position and having it update the offset in the correct way. Lots of production parts we do need to be probed from b-90 because there is no clearance from the top to touch datums. Think aerospace brackets.

[Guest]

 

Pay all that money for a nice machine and Methods can't even help you out with a basic question. I'd be pissed. :

 

The FANUC is more powerful than you think. It's WAY more powerful than even your above average user thinks it is. It all comes down to training. Most machine tool dealers do a xxxx poor job of training their end users.

 

Anyway, you should not have to pay for your machine tool dealer's general lack of technical expertise so against my better judgement here you go;

 

%

<TWP-PROBING>

N226(Renishaw OMP400 3mm x 50mm Probe)
T1M06
M132
G00G90G55A0.0C0.0
G68.2 X0.0 Y0.0 Z0.0 I0.0 J0.0 K0.0
G53.1
X1.875Y-1.875A0.0C0.0
M131
G43Z0.9409H1
M108(PROBE ON)
POPEN
G65P9810X1.875Y-1.875Z0.0409F80.
(Probe Web - X - TOP)
G65P9812X3.25Z-.25W1.

(Probe Web - X - LOWER)
G65P9812X3.25Z-.750W1.

(Probe Web - Y - TOP)
G65P9812Y3.25Z-.250W1.

(Probe Web - Y - LOWER)
G65P9812Y3.25Z-.75W1.

G00G90
G49G53Z0.0
G69

(Probe FRONT Bore From Front)
M132
G00G90G54A-90.0C0.0
G68.2 X0.0 Y0.0 Z0.0 I-0.0 J90.0 K0.0
G53.1
X1.875Y-1.5A-90.0C0.0
M131
G43Z4.8159H1
X1.875Y-1.5Z3.8159A-90.0C0.0
G65P9823A0B120.C240D1.25W1.
M109
PCLOS
G00G90
G49G53Z0.0
G69
G49G53Z0.0M05

M30
%

 

Hope this helps.

[Guest]

Oh, if you don't want to output the cycle results to your external decvice, just remove the POPEN and PCLOS statements and remove the W1. arguments.

 

ANd obviously there's some machine specific M-Codes in there like the rotary lock/unlock and probe on/off. You should be able to figure those out.

 

HTH

 

[dstryr]

Thanks for your help .

You said "You just cant probe with W-sec or TCP active" but I dont see where you turn it off?

Is it too early and I'm missing something clearly obvious?

 

And if I'm reading correctly your probe results under the second move should update the X and Z offset and it wont try and fill in the Y value in the work cordinate?

 

 

Oh and if it makes you feel any better I helped a local buddy of mine make the decision to buy a new MX330 with the 10 pallet

[Guest]

WSEC or TCP were never activated so no need to turn them off.

 

Actually in this example, i was just measuring stuff. In order to write to offsets, I would add an S arguement. S1. Would write G54, S2. G55, so on amd so forth. S101. Would write to G54.4P1, etc...

 

The X web cycle would write to X, the Y web cycle would write to Y, etc... the cycles will only overwrite axes they are measueing and leave the othwr axes alone.

 

Do you have a Renishaw Inspection Plus manual?

[Guest]

Cool about the MX-330.

 

Thank you!

[Newbeeee™]

Cool about the MX-330.

 

Thank you!

Just looked at the MX330 video.

What a SWEEEEEET machine!

[jlw™]

Foggy, in your G68.2 your not shifting or rotating for the x web... why did you use it?

[Guest]

Because I want XYZ zero, to ALWAYS be XYZ 0 no matter what orientation pr rotation.

[jlw™]

but but but... you don't have to call it from the top.

[dstryr]

That is what I was getting to...

 

I program everything off COR. So if I want to measure a bore at B-90 then the probe results for the hole being off in XY would not go into XY. They would either be Y or Z because in reality the part is off location at b0c0

[dstryr]

but but but... you don't have to call it from the top.

Yes. Should always call it at 0,0 rotation because what happens if there is a fixture offset ?

 

[dstryr]

 

Pay all that money for a nice machine and Methods can't even help you out with a basic question. I'd be pissed. :

 

The FANUC is more powerful than you think. It's WAY more powerful than even your above average user thinks it is. It all comes down to training. Most machine tool dealers do a xxxx poor job of training their end users.

 

Anyway, you should not have to pay for your machine tool dealer's general lack of technical expertise so against my better judgement here you go;

 

%

<TWP-PROBING>

N226(Renishaw OMP400 3mm x 50mm Probe)

T1M06

M132

G00G90G55A0.0C0.0

G68.2 X0.0 Y0.0 Z0.0 I0.0 J0.0 K0.0

G53.1

X1.875Y-1.875A0.0C0.0

M131

G43Z0.9409H1

M108(PROBE ON)

POPEN

G65P9810X1.875Y-1.875Z0.0409F80.

(Probe Web - X - TOP)

G65P9812X3.25Z-.25W1.

(Probe Web - X - LOWER)

G65P9812X3.25Z-.750W1.

(Probe Web - Y - TOP)

G65P9812Y3.25Z-.250W1.

(Probe Web - Y - LOWER)

G65P9812Y3.25Z-.75W1.

G00G90

G49G53Z0.0

G69

(Probe FRONT Bore From Front)

M132

G00G90G54A-90.0C0.0

G68.2 X0.0 Y0.0 Z0.0 I-0.0 J90.0 K0.0

G53.1

X1.875Y-1.5A-90.0C0.0

M131

G43Z4.8159H1

X1.875Y-1.5Z3.8159A-90.0C0.0

G65P9823A0B120.C240D1.25W1.

M109

PCLOS

G00G90

G49G53Z0.0

G69

G49G53Z0.0M05

M30

%

 

Hope this helps.

 

This result... should update X and Z offset... and not XY. What does it do in reality?

[Guest]

Programming from COR.... COMPLETELY old school and COMPLETELY unnecessary. Program from part datums and use the fuction as it was intended.

[jlw™]

That's the whole reason why I use it.  I rarely mess with G54.4 any more.  Any way, you don't need it at B0C0 so why call it from "TOP"?

[dstryr]

Programming from COR.... COMPLETELY old school and COMPLETELY unnecessary. Program from part datums and use the fuction as it was intended

How is this old school and uncessary?

Let me give an example from my Grob.

 

Lets say I have a part with a big flange. Datum surfaces are under the flange.

I can program the machine off x0y0z0a0b0 for every job.

 

Then critical job comes up where you need to probe the datums. I cycle800 to a0b0, probe in Z on one wall set my Z offset. Retract Cycle800 to a0b90 probe in Z and set the X offset.

 

How does changing where my program comes off change this?

[jlw™]

G68.2 will let you "move" your "offset" to another location while staying "associated" to original offset.  So that, if you roll A90. and come from a face not on Z0. you can shift it so that it is now Z0. and then the code is some what more readable for the operator.  It also handles deviation vector all on it's own so that you have no need for G54.4.  And you can set the part any where on the table.  It is unbelievably better for tombstone programming.

 

Have you ever used "Rotate Offsets" on an old Acramatic 2100 to handle tombstone work?  Sorta like that but infinitely better.

[Guest]

That's the whole reason why I use it. I rarely mess with G54.4 any more. Any way, you don't need it at B0C0 so why call it from "TOP"?

This file was a training/example file for a test part I used to for setting/adjusting the #19700-#19705 parameters. I called it top so the operator looking at the code/machine understood what was going.