[monaro mike]

Hi to fanuc fanatics
I always use G92 to program absolute coordinates on my 1987 leadwell mcvo oma, but when inserting these numbers after G92 they must be opposite to the actual movement to establish zero point .
For example :move mc to x200. y -150. z-250.
Program must read G92 x-200. y150. z250.
Thereafter all subsequent commands use positive and minus in the correct positions, its no big deal ...but annoying and if it can be changed easily then can someone please tell me how ?
I suspect its something set up by machine tool builder and not fanuc

cheers from Mike

[beege]

Perhaps you could move there first, then Zero your coordinate system from there.

G00X200.Y-150.
Z-250.
G92X0Y0Z0

This might also help to conceptualize why this is the way it is. When you call a G92, you are describing to the control where "right now" is. So, if X is +200. away, then "right now" you are at X-200.

Helps?

By The Way, I strongly recommend moving away from using G92 anywhere. Just asking for trouble, in my book! Learn about G54-G59, G10.

[Andre' B]

This might also help to conceptualize why this is the way it is. When you call a G92, you are describing to the control where "right now" is. So, if X is +200. away, then "right now" you are at X-200.

Helps?

By The Way, I strongly recommend moving away from using G92 anywhere. Just asking for trouble, in my book! Learn about G54-G59, G10.

Beat me.

Stated another way the X,Y values you put on the G92 line are the directed XY distances from where you want zero to be to where the spindle is currently sitting.

And yes if the control has the G54-59 work offsets, use them and forget that G92 ever existed.

[monaro mike]

Hi again,
I think i did,nt provide enough info , on my m/c x axis homing direction is minus (table to right > ) y axis positive (table towards operator ) and of cause z axis positive (UP).
I was always taught to use G92 not G54-59 more on that later, so after homing m/c i manually move axises to clock up a face or hole on part to
establish work position coord. (absolute zero), easy, then i note on the position page ...machine posn. from home , e.g x200. y-150. z-250, i use
these no.s for G92 .....but it has to be written in program as G92 x-200. y150.
z250. ( the opposite to the actual movement direction ) so i assume its just
a odd thing about this m/c .
I think we where told to stay away from G54-59 because of the potential devastation that could be caused if you input a G54 instead G55 etc. and also
every time you call up a new program, you have to remember to input new coord. into the G54-59 register unless you only ever have 6 programs .
With G92 the absolute zero points are already there in the program , provided you posn. the part correctly....there,s little room error .
I,d appreciate others opinions on this subject.

thanks

[Mike Stevenson]

My opinion is this:

1. G92 = newbie

2. G54-G59 = knowledgeable

You said, "stay away from G54-59 because of the potential devastation?"

Where on god's green earth did you hear that one?

G92 can be just as devastating as G54-G59 if is set wrong.

[monaro mike]

I hear what your saying , Mike Stevenson !
The guy who initially showed me how to program this m/c was well respected
in the industry (albeit a long time ago ) and there was,nt much he did,nt know
not unlike yourself no doubt , i figure he may have thought that G92 setting was somehow safer for newbe,s at the time , and ive always used it when operating fanuc control machines .
Most of my time has been on mazak machines ( lathes) 100ms and older quickturns so ive been spoilt with conversational programming etc .
Now that i have bought this machining centre i,m trying to get a better understanding of fanuc methods etc .....so if i ask a couple of dumb questions occasionally ...i,ll get over it !

cheers from Mike

[Dan Fritz]

G92 was the only way to set a coordinate system back in the 70s and 80s. The mulitple coordinate systems of G54-G59 were introduced on the Fanuc system 6M-B around '81 or so. A lot of "old timers" like me still like to use G92 out of habit.

It really doesn't matter which method you use. You're just establishing a zero for your program, so why argue over method? I will say that G54-59 is best if you want to jump from one coordinate system to another in the middle of a program, or if you have several established reference points on the table that you use for "zero" with different fixtures or different tools. Also, G54-59 is great if you're using a pallet shuttle.

I always used G92 in the old days, and it worked great. My routine was to zero-return the machine, move out to a known position on my part, then use G92. These first blocks of the program would use block-deletes (/), so when I powered up the machine and ran the first part, I could turn on the BDT switch and run parts without that zero-return move. Something like this:

/G00G91X-1.Y-1.Z-1.
/G28Z0
/G28X0Y0
/X--.----Y--.----Z--.---- (move to my part zero)
/G92X0Y0Z0
G90
(the rest of your program)
M30

The first block would move an inch in the opposite direction from zero-return, just in case the machine was at the zero-return position when I last powered down. Just make sure that you're not within an inch of anything when you cycle start with BDT turned off.

The G91 with the G28 is essential, because G28 is really a zero-return BY WAY OF AN INTERMEDIATE POINT. If you're in G91, that intermediate point is always the same position as where you already are (an incremental move of zero), so no unexpected moves occur.

[jamesweed]

I to was taught to use G92 back in the day. When we got my new mill, the MB taught me to use G54. The G92 was cool cause I could just call it in my program. The G54 you had to go to the offset page to enter it in. Didn't like that so I wrote a macro(O9010) that is called with a custom Gcode(G70) so I can use it just like the ole' G92. I dont know if you have macros enabled, but here it is...

%
O9010(SET WORK COORD.)
#3003=1
IF[#7GT#0]GOTO10
IF[#19EQ#0]GOTO3
IF[#19EQ0]GOTO1
#19=ABS[#19]
IF[#8EQ#0]GOTO99
G22Z[#5023+[-#19]]
F1
GOTO2
N99G22X[#5021+.001]Z[#5023+[-#19]]I2.5000
F2
GOTO2
N1G22X0.000Z0.000I0.000
F0
N2#33=0
N3IF[#24NE0]GOTO4
#5221=#5021
#33=1
N4IF[#25NE0]GOTO5
#5222=#5022
#33=2
N5IF[#26NE0]GOTO6
#5223=#5023
#33=3
N6IF[#1NE0]GOTO7
#5224=#5024
#33=4
N7IF[#33NE#0]GOTO8
#5221=#5021
#5223=#5023
#5224=#5024
N8G54
M#13
#3003=0
M99
N10
#3000=1(NOGO4U)
%

So now instead of programming a G92XZYB or whatever, I can call it with a G70XZYB. just as handy and more with the times. This macro is long cause I call set my zeros different ways and use it to set my stroke check.

[HuFlungDung]

Mike Manaro,
What other Gcode will that machine recognize? Does it permit commands in the machine coordinate system (G53) as well as the work shifts G54-G59?

I'm not sure why, if you move to the work datum, that you would want anything other than G92 X0 Y0 unless the control is keeping track of where the work home is relative to the machine home.

If the machine is parked at machine home and you want the work datum elsewhere, then, IMO you use coordinates with G92 X and Y to designate that the work home is not at the present location but is elsewhere. In this case, the signs should not need inversion.

If possible, I prefer to use a G53 line before a G92 line because this forces the machine to move to a known position in the machine coordinate system before the coordinate system is shifted by the G92. This can help prevent crashes after a program is aborted but the operator must always start at the beginning of the program to ensure that the G53 is read. Either that, or start from machine home.

[monaro mike]

Great response guys,
First Dan Fritz,
Glad to hear a guru like yourself used G92 in the 1980s which is
when i started, i was interested in your method of accident prevention at start of your programs.
My programs all start with this sub:
05000.
M98P9000.

G91.
G28 ZO.
G28 XO YO.
G90.
M99.

G92 X......Y......Z.......(at this point +@- signs had to be opposite )
GO XO YO ZO.
rest of program
M30.

Now ive tryed it the way you and Beege and the Huflung describe it
05000.
M98 P9000.
G0 X......Y......Z......( +@-signs match actual moves now)
G92 XO YO ZO.
rest of program
M30.
Now no problem! also Dan my "87 OMA control has G54-G59....must be one of the first to have this option.
To Jamesweed, macros are enabled on my m/c, bit of a mouthful that one you
sent, still trying to get my head around it ! thanks
To Huflung, tried G53 and control does,nt have it ,

Thanks to all

[CarbideBob]

G92 is just preset readout. No different than the preset button on a DRO on mill or comparator.

You are at zero ref position and put in G92 X-200. The machine must now move 200 in the plus direction to get to zero.

Many older controls don't support G54 or it is an option so this is your oly way of moving the zero.

Gets real confusing if you do a G92 while not at the zero ref position.
I use both methods and may sometimes have multiple G92s in a program. Useful if you have more repeating patterns than you have coordinate systems or tools with more than one cutting point. G54-G59 is easier to understand.
Bob

[jamesweed]

hey monroe mike,
that macro example i used is ran on a custom made mill that is used to mill feedscrews. so it may be a little strange for a mc. its programmed to set all axises but y to zero if no arguments are called.
ex...G70;
or i can set one axis at a time if i want by using a argument. ex...G70X0Z0;
also i use this same program to set stroke check2. so thats why its a mouthful. i just wanted you to see that using G54 can be as easy as G92
good day,
Jim

[ALLtra Mach]

Mike,
your machine is not doing anything unusual.
G92 denotes your present position.
So if where you are is, for example, .2 above Z0, then you are G92 Z.2, if below, you are G92 -.2.
Basically tells the machine, my current position is this far from programming zero point.

[harshal]

CNC G92 threading cycle for fanuc program (metric threading)
July 29, 2018 - FANUC G92 THREADING CYCLE [T]

G92 threading code is used in "G-code system A"




O1571
N10 M06 T02 02 ;
N20 G50 S1500 ;
N30 M03 G97 S200 ;
N40 M08 ;
N50 G00 X50 Z2 ;
N60 G92 X49.07 Z-20 F1.5 ;
N70 X48.77
N80 X48.47
N90 X48.17
N100 G28 U0 W0 ;
N110 M05 M09 M30 ;
More examples..........!!!!
DESCRIPTION OF MAIN PROGRAM :-
Calculation :- Depth of thread = 0.6134 X Pitch
= 0.9201
Crest = major dia - 0.9201
= 49.07
Root = Major dia - 2 x Depth of thread
= 50 - 2 x 0.9201
= 48.16 (root)
Each cut is 150 microns =0.15mm , it means total reduce 0.30 mm and cutting upto root 48.16 mm
First cut is 49.07 mm (Crest)
Second cut is 49.07-0.3 = 48.77
Third cut is 48.77-0.3 = 48.47
Final cut is 48.47 -0.3 = 48.17 (~ 48.16)(root)
*************************all dimension in mm ***********************************
01571 - Name of main program
N10- Tool change command , select tool no 2
N20- Maximum spindle speed command , speed is 1500 rpm
N30- Spindle ON clockwise , constant spindle speed , speed is 200 rpm
N40- Coolant ON
N50- Rapid action command , where X50 and Z2 .
N60- Threading cycle command , where X49.07( crest )(First cut) and Z-20 , feed rate is 1.5 ( it is always is equal to pitch )
N70- Second cut is 48.77 in X axis
N80- Third cut is 48.47 in X axis
N90 - Final cut is 48.17 in X axis (root)
N100 - Reference position command , where X0 and Z0 ;
N110 - Spindle OFF , coolant OFF , main prog. end

my link is
http://www.hdknowledge.com/2018/07/c...c-program.html