Need suggestions, Fanuc O-T does not recognize G83

Dave K · Dec 13, 2014

I've got an early nineties vintage lathe with a Fanuc O-T. It recognizes simple drilling code like G81, but does not recognize G83. What a pain to type out those drilling pecks long hand. What's the best solution to get around this? Make a sub? Use macro? Others? I don't have cam so I'm typing these out long hand. :cryin:

sable · Dec 13, 2014

There will prolly be a face grooving cycle which pecks .( or is that g83?)

Try G74

Dave K · Dec 13, 2014

sable said:
There will prolly be a face grooving cycle which pecks .( or is that g83?)

Try G74

No, G83 is peck drilling. Never thought of the G74. I'll try that. Thanks!

Dave K · Dec 13, 2014

Well, G74 is listed as an Auto drilling cycle. But it gives me short pecks, rather than pecks that pull completely out of the hole each peck. G75 is listed as an Auto grooving cycle, but I highly suspect it's going to do the same type of peck. It will just back up the tool to break the chip, then continue, never pulling completely above the Z plane.

706jim · Dec 13, 2014

If it helps, G74 (or is it G75?) will peck in the X axis in a similar manner which is good for grooving or parting.
Can't help with the G83 though.

Mtndew · Dec 13, 2014

Dave K said:
I've got an early nineties vintage lathe with a Fanuc O-T. It recognizes simple drilling code like G81, but does not recognize G83. What a pain to type out those drilling pecks long hand. What's the best solution to get around this? Make a sub? Use macro? Others? I don't have cam so I'm typing these out long hand.

What does your code look like where it's not seeing the G83? Maybe there's something else that it doesn't like

alphonso · Dec 13, 2014

Parameter 909.3?

Dave K · Dec 13, 2014

mtndew said:
what does your code look like where it's not seeing the g83? Maybe there's something else that it doesn't like

g83 z-1.44 r0.1 q.15 f.003;

Dave K · Dec 13, 2014

alphonso said:
Parameter 909.3?

I'll need a little expansion on that. What about that parameter?

yardbird · Dec 13, 2014

I sometimes use this on 0-T & 0i-TD both..It will do the same as G83...strange your machine won't do the G83 both mine will..

N10(MSG, 17/32 .5312 DRILL)
G0G99G40G54X14.Z10.T0
T0808

#1=.03 (FEED SHORT OF)
#2=.25 (PECK EVERY)
#3=.0 (START DRILLING AND LOCAL VARIABLE)
#4=2.67 (STOP DRILLING)
#5=.15 (RAPID BACK SHORT OF)
#6=.006 (FEED RATE)

M41
G97S185M3
G0Z.5
G0X0M8
G0Z-[#3]
#3=[#3+#2]
N200
G1Z-[#3]F[#6]
G0Z.1
G0Z-[#3-#5]
G1Z-[#3-#1]F.2
#3=[#3+#2]
IF[#3LT#4]GOTO200
G1Z-[#4]F[#6]
G0Z.5
M9
G0X10.
G0G40X14.Z10.T0
M1

Brent

Edit.. Dave It just so happens that parameter 909.3 = 1 in my Fanuc 0-T machine. I have absolutely no idea what it does but it is set to 1. alphonso doesn't say what 909.3 value should be, actually doesn't too much at all and I don't have a 0-T manual.

Below is what my G83 cycles look like you might try no decimal for the Q and add X0 but other than that I see nothing as to why it wont work on your control.

G83X0Z-2.5R.01Q2000F.005

Try the little macro drill it should stop the :cryin:

Dave K · Dec 13, 2014

yardbird said:
I sometimes use this on 0-T & 0i-TD both..It will do the same as G83...strange your machine won't do the G83 both mine will..

N10(MSG, 17/32 .5312 DRILL)
G0G99G40G54X14.Z10.T0
T0808

#1=.03 (FEED SHORT OF)
#2=.25 (PECK EVERY)
#3=.0 (START DRILLING AND LOCAL VARIABLE)
#4=2.67 (STOP DRILLING)
#5=.15 (RAPID BACK SHORT OF)
#6=.006 (FEED RATE)

M41
G97S185M3
G0Z.5
G0X0M8
G0Z-[#3]
#3=[#3+#2]
N200
G1Z-[#3]F[#6]
G0Z.1
G0Z-[#3-#5]
G1Z-[#3-#1]F.2
#3=[#3+#2]
IF[#3LT#4]GOTO200
G1Z-[#4]F[#6]
G0Z.5
M9
G0X10.
G0G40X14.Z10.T0
M1

Brent

Edit.. Dave It just so happens that parameter 909.3 = 1 in my Fanuc 0-T machine. I have absolutely no idea what it does but it is set to 1. alphonso doesn't say what 909.3 value should be, actually doesn't too much at all and I don't have a 0-T manual.

Below is what my G83 cycles look like you might try no decimal for the Q and add X0 but other than that I see nothing as to why it wont work on your control.

G83X0Z-2.5R.01Q2000F.005

Try the little macro drill it should stop the

Brent,
Thanks for the info. I'm curious. Why would you have that macro set up if your control is using the G83 just fine? Also, can you give some explanation at to what's going on with that macro? I think I understand a little bit of it, but not following it fully. And do you state this macro in the program, right in the same spot you would normally have the G83 line?

yardbird · Dec 13, 2014

Yes it goes where the G83 line goes.

The reason is I ran a Leblond and the deep hole drilling cycle sucked. I used it mostly on that machine

I like it because when drilling very long holes the macro rapids short of the bottom (variable #5 .15) feeds to (variable #1 .03) then starts drilling again.

Do you use N numbers for every line? What i posed is exactly what is in my program when using it.

I have drilled holes on our Fanuc o-t many times with it.

Brent

Dave K · Dec 13, 2014

yardbird said:
Yes it goes where the G83 line goes.

The reason is I ran a Leblond and the deep hole drilling cycle sucked. I used it mostly on that machine

I like it because when drilling very long holes the macro rapids short of the bottom (variable #5 .15) feeds to (variable #1 .03) then starts drilling again.

Do you use N numbers for every line? What i posed is exactly what is in my program when using it.

I have drilled holes on our Fanuc o-t many times with it.

Brent

I don't use N words in every line. I'm using canned cycles for the turning so there's only N words within that canned cycle.

yardbird · Dec 13, 2014

#1=.03 (FEED SHORT OF)
#2=.25 (PECK EVERY)
#3=.0 (START DRILLING AND LOCAL VARIABLE)
#4=2.67 (STOP DRILLING)
#5=.15 (RAPID BACK SHORT OF)
#6=.006 (FEED RATE)

Starts drilling at Z0
pecks evey .25
stops at 2.67
rapids back short of the bottom by .15
feeds to .03 of the bottom
feed of .006

you can alter all them ^^^ variables to suit you needs on any particular part.

Dave trust me on this one. Load up what I posted and out in the air watch it run. Then just start playing with it.

You can also start drilling at a 1" in the part but variable #3 is still a positive number. Pretty sweet really. From N10 to M1 is exactly what I'd have in my program.

Ok so typically you dont get to N200 then correct, I dont. N200 is being used in the macro that would cause a potential problem. Be aware of that..

Brent

Dave K · Dec 13, 2014

yardbird said:
#1=.03 (FEED SHORT OF)
#2=.25 (PECK EVERY)
#3=.0 (START DRILLING AND LOCAL VARIABLE)
#4=2.67 (STOP DRILLING)
#5=.15 (RAPID BACK SHORT OF)
#6=.006 (FEED RATE)

Starts drilling at Z0
pecks evey .25
stops at 2.67
rapids back short of the bottom by .15
feeds to .03 of the bottom
feed of .006

you can alter all them ^^^ variables to suit you needs on any particular part.

Dave trust me on this one. Load up what I posted and out in the air watch it run. Then just start playing with it.

You can also start drilling at a 1" in the part but variable #3 is still a positive number. Pretty sweet really. From N10 to M1 is exactly what I'd have in my program.

Ok so typically you dont get to N200 then correct, I dont. N200 is being used in the macro that would cause a potential problem. Be aware of that..

Brent

Ok, got it! This looks pretty cool. I'll give this a try in the morning. Thanks for the help!!

ZachN · Dec 14, 2014

I have a fanuc OT control as well. We use the G74 all the time. But we have never found a code that works to do a full retract... Can't remember if we have tried a g83 or not. I'll give it a try.
But when we need a full retract I have a blank program saved with something like the following:

G0 Z.050
G74 Z-1.0
G0 Z.050
Z-.950
G74 Z-2.0
G0 Z.050
Z-1.950
G74 Z-3
Ect
Ect

I have it saved with maybe 20 repeats on my laptop. Just open it, edit the lines I need, delete the rest of them. And hit SAVE AS to give it a different name. Then my sample file is still there and I have my new program.

I'm going to follow this thread and test out G84 as well.

Zach

yardbird · Dec 14, 2014

Zach G84 is rigid tap..typo probably. Don't you need a peck amount in the G74 line? What you have would work but when your 7 or 8 inches in a hole you need to peck more than every inch. If you cant get the G83 to work, try what I've posted in my first post.

I've drilled holes with that little macro on a Cincinnati Milacron with Acromatic 850s control, LeBlond Makino with a Mark Century 2000 control, Johnford TC-50 with Fanuc 0-T control and Doosan Puma 300 & 240 with 0i-TD control they all ran this macro drill cycle. Each control was different but the logic remained the same. I've had it quite some time.

Load up what I've posted move the G54 out to something safe, watch it run..

Brent

yardbird · Dec 14, 2014

Pretty sure this doesn't need said but saying it anyways. Change any no brainers you see that you will be specific to your machine, the Fanuc 0-T here is a Johnford TC-50 some MTB differ on some shit. Dont know if your machine has a high and low gear range, might need to take the M41 out maybe. Let me know how things go..

One more thing.. its going to rapid to Z zero and start the drilling cycle there, center dirll provides some cush, take this into account if not center drilling first.

Good luck Dave.. Its late been a long day.. :Yawn:

Brent

screensnot · Dec 14, 2014

Dave K said:
g83 z-1.44 r0.1 q.15 f.003;

Try Q1500 instead.

Dave K · Dec 14, 2014

Ha! I'm screwed I think. I can't even type a # sign into my control. It exists on the same button as the "end of block" button, but it only toggles to ; / and ,. The # sign never shows up.

Need suggestions, Fanuc O-T does not recognize G83

Diamond

Titanium

Diamond

Diamond

Titanium

Diamond

Titanium

Diamond

Diamond

Titanium

Diamond

Titanium

Diamond

Titanium

Diamond

Aluminum

Titanium

Titanium

Hot Rolled

Diamond

Similar threads