425 UNUSABLE G CODE 31!!

[guydrisc]

IT SEEMS LIKE IM GETTING CLOSER AND CLOSER TO RUNNING THIS MACHINE... I GOT THE MACHINE TO RECOGNIZE MY PROGRAMS BUT NOW I GOT THE "425 UNUSABLE G CODE 31" ALARM.. THE MANUEL SAYS G31 IS THE SKIP FUNCTION.. CAN SOMEONE GUIDE ME A LITTLE, IM NEW TO OKUMAS

[Superman]

G31 is a threading cycle on a lathe
and a "skip function" on a mill

I checked our manuals, found no real info on G31 ( may have something to do with customising an automated process / autogauging or the like ), I have not seen it used on a mill

Can you post the section for us to read ?
and explain what you want to have this G31 do, it may be that the wrong G-code has been selected ( manuals also say it cannot be used when G169 is active ).

[guydrisc]

there is no G31 in my program at all... i try to run the program and that is what the alarm says..... its wierd.. i do a G31 search in the post and nothing comes up...

[Oti]

What model is the control? I will dig through the books this weekend and see what I can find.

[guydrisc]

it is a 5020m OSP

[Superman]

Is there any library files in the machine ?
do a directory search for *.LIB

At what stage does this alarm pop-up ? what is the commanded line of code ?
The older basic Okuma's read up to 4 lines ahead, to narrow it right down, do it in single step

eg
loading the program = OK
at a "CALL" statement = alarm
or M6 = alarm

What it may be is in a file in the system area for doing a machine operation
like M6 behind the screen sequence is spindle orientate, coolant OFF, rapid retract to G30 P1, toolchange cycle. end cycle ( this is editable by a MTB - Machine Tool Buider or Okuma )

[guydrisc]

it happens in the first line of code..
$BASHPLATE.MIN%
O0001
N100 G20
N101 G0G17G40G49G80G90
N102 G30P1
N103 T4M6
N104 G0G90G54X10.0154Y-3.6748S6000M3
N105 G30P1
N106 G43H4Z1.
N107 Z.2
N108 G1Z.1F10.
N109 G2X10.072Y-3.5924Z.0917I.0283J.0412F60.
N110 X10.0154Y-3.6748Z.0835I-.0283J-.0412
N111 X10.072Y-3.5924Z.0753I.0283J.0412

blah blah

not even sure if this is right but it is what i am trying

[Superman]

Originally Posted by guydrisc it happens in the first line of code.. $BASHPLATE.MIN% O0001 N100 G20 N101 G0G17G40G49G80G90

Is this what is on the screen in the control ?

1st line
If it is, then the first line shouldn't exist ( it is only used in the upload process to name the file in the Okuma control, and is present only on the PC copy )

2nd line
:Oxxxx, FANUCs use it here for their naming info.
Oxxxx is usually a sub-routine naming address.
If it isn't used in a "CALL" statement, eg CALL O0001, then there has to be a RTS somewhere after it, similar to an M2/M30.

These sub-routines are normally placed after the M2/M30 at the end of program before the final %

I think your problem is the 2nd line
Comment out both lines in the control and run again

[skullworks]

Originally Posted by guydrisc it happens in the first line of code.. $BASHPLATE.MIN% O0001 N100 G20 N101 G0G17G40G49G80G90 N102 G30P1 N103 T4M6 N104 G0G90G54X10.0154Y-3.6748S6000M3 N105 G30P1 N106 G43H4Z1. N107 Z.2 N108 G1Z.1F10. N109 G2X10.072Y-3.5924Z.0917I.0283J.0412F60. N110 X10.0154Y-3.6748Z.0835I-.0283J-.0412 N111 X10.072Y-3.5924Z.0753I.0283J.0412 blah blah not even sure if this is right but it is what i am trying

Son - first off pitch the fanuc post you used to make the code - its useless

I'm going to take what is above and show how it should be.

O0001 - O#### is not neded
N100 G20
N101 G00G17G40G49G80G90
N102 G30P1
N103 T4M6
N104 G00G15G90G54X10.0154Y-3.6748H1S6000M3
N105 G30P1
N106 G43G56H4Z1.
N107 Z.2
N108 G01Z.1F10.
N109 G02X10.072Y-3.5924Z.0917I.0283J.0412F60.
N110 X10.0154Y-3.6748Z.0835I-.0283J-.0412
N111 X10.072Y-3.5924Z.0753I.0283J.0412

M2


Remove anything greyed - add items in blue.

So - basically all leading zeros within a G Code MAY be required ie G1 must be G01(allmost all 5020 controls)

Work coordinates are called using G15 Hxx (01-20) not g54-g59
Tool offsets are called using G56 Hxx not g43

I have no clue what you were attempting with the G30P1 - loose it.

Programs end with M2, and an M2 must be found - M30 is not used.

[Superman]

skullworks

So - basically all leading zeros within a G Code MAY be required ie G1 must be G01(allmost all 5020 controls)

Leading zeros not required M00 same as M0, F0.001 same as F.001, T01 same as T1

Work coordinates are called using G15 Hxx (01-20) not g54-g59 Tool offsets are called using G56 Hxx not g43

I'll agree here

I have no clue what you were attempting with the G30P1 - loose it.

this is okuma code, telling him to loose it, is like telling him to cut his good hand off, and saying "get used to it ". Suggest you look up your manual, these are reference return points P1 is usually the toolchange point. Don't remove it just because you don't know what it does

Programs end with M2, and an M2 must be found - M30 is not used.

BullS---M2 and M30 can be used at the end of the program

[skullworks]

OK - My bad
-" So - basically all leading zeros within a G Code MAY be required ie G1 must be G01(all most all 5020 controls) "-

Should have been:
" So - basically all leading zeros within a "G" Code MAY be required ie G1 must be G01 (all most all 5020 controls)

As to the G30P1 - I am well aware that it is used on a few specific Okuma machines as a 2nd zero return - and I can think of 2 examples where it is needed.

1) Exchanging a tool from a vertical spindle to the horizontal spindle or the other way.
2) Tool change with a pallet or 4th axis present.

On most machines I have come across the G30 position has not been defined unless addon hardware like a 4th axis or pallet changer has been added - and then it had to have been added by an authorized Okuma dealer.

As to M30 I know our newer OSPE100 and both the OSP5000 and OSP5020 machines will not allow a "program select" if the program ends with M30. - I will admit this may be unique to U.S. sold models.

For tool change on mills the M6 will take the spindle to the tool change location. On lathes the turrets must be fully up on the X axis limit to index, and this must be a programed move.

I may be a bit rusty on Okuma's since I have not touched one since Decemeber, I've been off in Mexico training a new facility in the use of the Hwacheon and Mazak lathes and the Staubli "PUMA" robots. I only have 19 year exp on OKUMA machines - still have not run any of there CNC grinders, that might be fun (not). I prefer the Dual turret LR lathes and the old MC series Vertical machines. I think the old LB-15 was one of the best hunks of iron ever made.

I prefer Mori-Seiki, but feel safer turning an operator loose on a Okuma.

[Goldorak]

Originally Posted by Superman skullworks Leading zeros not required M00 same as M0, F0.001 same as F.001, T01 same as T1 I'll agree here this is okuma code, telling him to loose it, is like telling him to cut his good hand off, and saying "get used to it ". Suggest you look up your manual, these are reference return points P1 is usually the toolchange point. Don't remove it just because you don't know what it does BullS---M2 and M30 can be used at the end of the program

you are absolutely right !

the G30P1 is include in the automatic tool change cycle, there is no need to leave it in the program