G50 or G92?

[protrxrptr17]

I have a 1984 Ikegai FT20-U with a Fanuc 6T-B. I've been reading the manuals, and they are kind of hard to understand. What is the difference between G92 and G50 for setting workpiece zero? Does this control have work offsets such as G54? The manual doesn't list it, but could that have been added? I am in the leaning process, so this may be a stupid question. Please forgive my ignorance.

[HuFlungDung]

Lathes may often use a different gcode system than mills, and on some controls, you can actually set (via parameter) which gcode system you intend to use.

So, mills usually use G92 as a coordinate system shift, whereas lathes will use G50 to do the same thing. The two codes are not interchangeable (within one gcode system), it will be a case of one or the other in your particular controller. You just have to find out which system is in effect

[dcoupar]

My Fanuc 6T-B manual doesn't list G54-G59, so as far as I know Work Coordinate systems weren't available on that model... so:

More than likely, your machine is set up to use Standard G-Codes (as opposed to Special G-Codes B). This means that you'll use G50 Xn Zn Sn to set your X/Z zero for each tool and maximum RPM (for CSS mode), and G92 for a simple turning cycle. You might try to MDI a G50 S500 and cycle start to see if it causes an alarm 010.

Also, you can check Parameter #7, bit 5. 0=Standard G code is used, 1=Special G code B is used.

Good luck.

[protrxrptr17]

Originally Posted by dcoupar My Fanuc 6T-B manual doesn't list G54-G59, so as far as I know Work Coordinate systems weren't available on that model... so: More than likely, your machine is set up to use Standard G-Codes (as opposed to Special G-Codes B). This means that you'll use G50 Xn Zn Sn to set your X/Z zero for each tool and maximum RPM (for CSS mode), and G92 for a simple turning cycle. You might try to MDI a G50 S500 and cycle start to see if it causes an alarm 010. Also, you can check Parameter #7, bit 5. 0=Standard G code is used, 1=Special G code B is used. Good luck.

So I should reset the zero point at every tool change or just at the beginning of the program? What if the control is setup for the special G-code? What is the difference between the two codes? Is there any advantage to using one over the other?

[dcoupar]

Yes, you'll need to program a G50 (or G98) block for each tool. If your control is set up for special G codes, use G98. My guess is, it's not, so use G50. Most (if not all) Japanese machines came over with standard G codes, if my memory serves me correctly. No advantage one over the other, just use the one that works.

[protrxrptr17]

Well, I didn't get to make any chips fly today. When I was setting my tools, something screwed up with the turret. I posted the story in the general metalworking machines section.

[tobyaxis]

Originally Posted by protrxrptr17 I have a 1984 Ikegai FT20-U with a Fanuc 6T-B. I've been reading the manuals, and they are kind of hard to understand. What is the difference between G92 and G50 for setting workpiece zero? Does this control have work offsets such as G54? The manual doesn't list it, but could that have been added? I am in the leaning process, so this may be a stupid question. Please forgive my ignorance.

G50 is used on older lathes to set the tools. The Ikegai I worked with all the tools were set from the Home Position Relative to the Work X and Z. Another way was to set a known position and program G50 X0Z0. Then write your program from there. This would usually be the axial center of the X and Face of the Z.

It is really up to you and what your comfortable with. Personally I prefer setting my tools Relative to the Home Position.

BTW G92 is a Threading Canned Cycle on a Lathe, not Work Positioning.

Threading Cycles are
G32
G76
G92

[protrxrptr17]

From what I can gather from the manual after many hours of studying is to load a turning and facing tool, take a light cut on the face and outside diameter. Zero the display, then go back to machine zero. Record the readings on a piece of paper, and then program G50 Xwhatever Zwhatever and thet will be your zero point for the entire program. Your reference tool offsets will be zero of course, and then you touch off all your other tools to set their offsets. Doesn't say you have to re-enter G50 and your zero coordinates after every tool. I looked through a couple old programs in the memory, and they didn't have a G50 at every change, so maybe I won't have to do that. There is a chart in the Fanuc manual that states G92 as special G code and special G code C. It also says workpiece coordinate shift is a basic option?? Is adding that as simple as changing a parameter or is it more complicated than that? I can see where that would be very useful, but I guess I could do it just as easily with a G50. Well I kinda got a bigger problem now. I think the rotary encoder on the turret is going out, so it may be even longer before I really get this thing going. ANybody know how to test the encoder?

[Ozemale6t9]

You have two options for using g50. You can set it once as you have just described from the manual, or you can set it for each tool. The difference is that setting once may cause tool offsets to be large numbers since the offset will be relevant to your datum tool. This can cause problems when you have to alter tool offsets due to large numbers being easy to forget if you have to enter the whole number. Setting G50 for each tool will result in all your tool offsets being zero initially, which makes it easier when resetting your offset after an insert change because you simply set it back to zero. With either method, it pays to have the program send the machine home at the start, move to your start position, then redefine G50, so if the machine gets moved manually it will pick up the correct position.

regards, Oz

[tobyaxis]

This is an old Ikegai Program for a Fanuc 6T. The starting point is set far away due to the uneven saw cut. Also this is a Safe way to start programming until you get more comfortable.

O0086
(IKEGAI FANUC 6T)
(TURBINE SPLINE 27SPL)
(GM 200 TH200R4)
(MATERIAL=4140)
(PILOT=1.375D)
(ID=.814D)
(OAL=)
(BLANK=)
(DRWNG=SPLINEA.CAD)
(OP#1)
(DATE 2/10/03 PGMR TJD)
(DATE REV 2/10/04 TJD)
(T1=CNMG432 VALINITE SV330 T3)
(T2= DRILL .75D COB STUB 135SPT)
(T3=DNMG431 SECO FF1 CM T3)
(T4=B-BAR 1/2 CCMT21.51F2 TP1000 T2)
(SECO CARBOLOY)
(JAWS=400 PRESS=200)
(CYCLE TIME=MS)

G0 G40 G97 G99 M5
G28 U0 W0 M9
G50 S2000 M39
M1

N1(REMOVE SKIN/R-FACE/TURN)
G28 U0 W0
T0100
G50 X(RP) Z(RP) M8
G96 S700 M3
G0 G42 X3.99 Z.3 T0101
G1 Z-1.3 F.01
X4.05 F.015
G0 G40 X4.1 Z.2
G72 P10 Q15 W.005 D400 F.008
N10 G0 G41 Z0
N15 G1 X0 F.004

G0 G40 X4.0 Z.1
G71 P20 Q25 U.02 W.002 D850 F.01
N20 G0 G42 X1.0
G1 Z0 F.0025
X1.325 F.003
G3 X1.375 Z-.025 R.025 F.0025
G1 Z-.75 F.004
X2.75 F.0035
X3.975 Z-.9141 F.0025
G1 Z-1.08 F.004
N25 X4.1 F.0035

G0 G40 Z.1 M9
G0 X(RP) Z(RP) T0100
G28 U0 W0
G97
M1

N2(DRILL)
G28 U0 W0
T0200
G50 X(RP) Z(RP) M8
G97 S400 M3
G0 X0 Z.2 T0202
G1 Z-2.25 F.0075
Z.05 F.2

G0 G40 Z.1 M9
G0 X(RP) Z(RP) T0200
G28 U0 W0
G97
M1

N3(F-FACE/TURN/U-CUT)
G28 U0 W0
T0300
G96 S900 M3
G0 G41 X1.5 Z0 T0303
G1 X.625 F.004
Z.05 F.015

G0 G40 X4.1 Z.1
G70 P20 Q25
G0 G40 Z.1

(U-CUT)
G1 X1.3755 Z-.725 F.05
Z-.7555 F.0025
G4 U1.0
G1 Z-.75 F.003
X2.8 F.0035

G0 G40 Z.1 M9
G0 X(RP) Z(RP) T0300
G28 U0 W0 M5
G97
M1

N4(R-BORE )
G28 U0 W0
T0400
G50 X(RP) Z(RP) M8
G96 S400 M3
G0 G40 X.75 Z.1 T0404
G71 P40 Q45 U-.02 W.002 D320 F.0075
N40 G0 G41 X1.214
G1 X.814 Z-.1 F.003
Z-1.3 F.005
N45 X.75

G0 G40 Z.1 M9
G0 X(RP) Z(RP) T0400
G28 U0 W0
G97
M1

N5(F-BORE)
G28 U0 W0
T0404
G50 X(RP) Z(RP) M8
G96 S650 M3
G0 G40 X.75 Z.1 T0404
G70 P40 Q45

G0 G40 Z.1 M9
G0 X(RP) Z(RP) T0400
G28 U0 W0
G97
T0

M30

[protrxrptr17]

Thanks for the program. I can definitely use that to format my own programs. The programs that are already in the machine don't really make much sense to me. I don't think they really follow the basic order.

[tobyaxis]

Originally Posted by protrxrptr17 Thanks for the program. I can definitely use that to format my own programs. The programs that are already in the machine don't really make much sense to me. I don't think they really follow the basic order.

To put it bluntly Fanuc Books SUCK. Try this one. It can be found on Amazon.com and explains everything in ENGLISH.

http://www.amazon.com/Computer-Numer...e=UTF8&s=books

This is by far the Best for Learning Lathe and Mill G-Code Programming.

Tool Stations 1,3,5,7,9,11 are all O.D Turning Threading, and Grooving

Tool Stations 2,4,6,8,10,12 are all I.D. Drilling, Boring, I.D. Grooving and Threading.

Post the Program You have and I'll walk you through it.