[mflux_gamblej]

I've been reading plenty of lathe tool offset threads - however, the older fanuc 6t-b does not have G54 or G10. It has G50 and that's it.

This is a new machine to me and I'm trying to wrap my head around how to setup the tool changer with coordinate systems that don't need to be changed much part to part: e.g. if I put in a new piece that sticks out of the chuck 4" instead of 2.1", I don't want to redo all my tool offsets.

Right now (as was on machine delivery to me) all of the tool offsets are large negative numbers. for example T0101 is x: -8.7770", z: -9.5000".

I first put the machine in the ref position (turret up against the furthest x/z travels away from the axis and chuck face / most upper right position). I then set 'U' 'ORIGIN', 'W' 'ORIGIN which puts u and w both at zero.

I measured the offset for this tool by taking an OD skim and measuring the diameter (off a 1" bar), and using a z-axis setter/depth gauge (2" block with a dial indicator built in so when the dial reads zero you're exactly 2.0000" from bottom to top of that gauge) placed on the chuck jaw face. I then go to MDI mode and set x0z0 using 'G50 X 0.9945, Z2.0' After this, I put the control in ref. mode and manually jog to the reference point

At this point, the u, w reads zero because I'm back at the ref point. X and Z read X = 8.7770, Z = 10.4000. Both values are positive values. The X reads identical to the stored x offset, except positive, and the Z is a bit different because who knows what Z they were using at the time.

I then go into the OFFSET page and set this tool T0101 with my new / similar values (because that's how they were doing it before) Xoff -8.7770, Zoff -10.4000.

I do this for the tools that I will use in my program - in this case for my first simple program I only use tools 1 and 7 so I setup the offsets 1 and 7 as described above.

I then load up my program and use tool 1 to set Z (absoulte) zero. I do this by using my Z depth gauge again against the chuck jaw. (I setup the program with the chuck face as zero, stock will need to stick out about 2.5" + 0.02"). I get tool 1 against the gauge at exactly 2.0000", then I go to MDI mode and program G50 Z2.0.

All is reading well in X and Z. I put the machine back in the ref. position, then I loadup the program and hit cycle start - at which point the tool changes to tool 7 (the first tool used) by the code:

T0700
G28 U0 W0
G00 T0707

At this point, the turret procedes to rapid towards the chuck face, the tool goes exactly on centerline, but during the move, the X and Z readouts change to some seemingly random numbers (maybe subtracted the tool offset values??) and I have to mash the E-Stop to stop it from rapiding right through the chuck.


Clearly I need to rethink or learn how the tool offsets are currently setup and intented for use, and how I want to do it.

I want to use the chuck jaw as Z0 everytime and just allow some error in the placement of the stock which I face in the program to the correct size.


Any tool offset / fanuc wisdom out there? Don't start talking G54/G55, or G10 - those are not available on the 6T.


Some additional info:

the parameters for automatic coordinate shifting are set to 0000 so its not that.

Do I need to setup the z0 in a different menu screen before running the programs?


I'll be back in the shop working this out in a few hours, but any help would be very much appreciated!! :drowning:

buying a new (to me) machine is a hell of a thing, as usual. This is my first lathe, and first CNC lathe that I've ever used. I have a mill - I wish that every part could be done on my mill right now. Darn lathe is difficult! Subtract an axis, add a tool turret that can crash chuck jaws that aren't cut just right... etc., etc., etc. wow.

[txcncman]

I do not see why you are not programming like this or something similar:

G28 U0. W0. (always sent the machine to a safe position BEFORE calling tool change)
T0700 (call tool change)
G50 X0. Z0. (call work coordinate shift)
G00 T0707 (call tool offsets)

All of your X tool offsets will be set to X center line (negative values). All Z offsets will be set to desired work zero point (negative values).

If you want your Z zero tool setting point to be the chuck face, do that. Then adjust the G50 line the distance from the chuck face to the work zero point.

[fizzissist]

Your tool offsets are in relation to the G50 "start point" ( usually the machine "home" position) and the part/program zero.

Your offset value will be a -X(dia) -Z, because you're in a +X and +Z (yeah, I know, seems backwards.. I'll explain) in the home position.....

The control must know the position of EACH tool at its start point, in reference to program zero. The start point is usually the home position of the tool.

If you draw a picture of the outline of the part and the program zero along with the tool in its home position, you'll see that the tool is in a very positive X position, and it's also in a very positive Z position, relative to the program zero. In order to move the tool towards the program zero, it has to move in -Z. 'Zat make sense now?

Hope this helps a little.
Keep your hand on that big red button!!

[mflux_gamblej]

I do not see why you are not programming like this or something similar:

G28 U0. W0. (always sent the machine to a safe position BEFORE calling tool change)
T0700 (call tool change)
G50 X0. Z0. (call work coordinate shift)
G00 T0707 (call tool offsets)

All of your X tool offsets will be set to X center line (negative values). All Z offsets will be set to desired work zero point (negative values).

If you want your Z zero tool setting point to be the chuck face, do that. Then adjust the G50 line the distance from the chuck face to the work zero point.

Here is a program that was running on the machine for the last owner (there were 5 programs in memory, each g-code is similar to this). I've added some comments explaining the codes to myself a couple of days ago.

Notably, G50 is set here to clamp the max spindle speed - but no G50 x0 y0 is programmed. I'm pretty sure that they were using mastercam based on the look of this code.

-------------------------
%
:6034
(Z0 IS FACE OF PART)

N1
G97 S2500 M3
T0800 ("L" DRILL .29)
G0 X0. Z.15 T0808 M8 (M8 is coolant ON)
G1 Z.02 F.02
G1 Z-.8 F.004
G0 Z.15 M9
G28 U0. W0. (automatic return to ref point before tool change)
T0800
M1
N2
G50 S4000 (G50 followed by spindle speed, sets max spindle speed = to given value)
G97 S2634 M3 (M3 is spindle on, CCW [forward direction])
T0900 (1/4" B.B.,ROUGH)
G0 X.29 Z.15 T0909 M8
G1 Z.02 F.005

X.31
Z-.7 F.003
G0 X.3
Z.02
X.33
G1 Z-.7
G0 X.3
Z.02
X.34
G1 Z-.3195 F.002
G2 X.3179 Z-.3958 I.1215 K-.0565
G1 X.3325 Z-.4445
Z-.706
X.29
G0 Z.02
G1 X.39
Z-.1421
G2 X.3783 Z-.1654 I.062 K-.028
G1 X.3591 Z-.3023
G2 X.34 Z-.3195 I.1119 K-.0737
G0 Z.02
G1 X.44
Z-.0899
X.3913 Z-.1407
G0 Z.02
G1 X.49
Z-.0378
X.44 Z-.0899
G0 Z.02
G1 X.54
Z0
G2 X.518 Z-.011 K-.011
G1 Z-.03
X.505
G2 X.4942 Z-.0334 K-.006
G1 X.49 Z-.0378
G0 Z.02
G1 X.59
Z0.
X.54
G0 Z.02
G1 X.627
Z0.
X.59
G0 Z.02
Z0.
X.61
G0 Z0.15 M9
G28 W0U0
T0900
M1
N3
G50 S2000
G97 S1000 M3
T0200 (.0625 I.D. GROOVER)
M8
G0 X.528 Z.1 T0202
G1 G99 Z.02 F.005
Z-.03 F.001
X.503
X.401 Z-.1374
G2 X.3893 Z-.1597 I.0565 K-.0268
G1 X.369 Z-.2983
G2 X.325 Z-.37 I.106 K-.0717
G1 Z-.4325
G2X.3425 Z-.479 I.128
G1 Z-.7
G0 X.32
Z-.6375
G1 X.3418
X.3425 Z-.6475
G2 X.3625 Z-.6575 I.01
G1 X.453 F.00025
Z-.66 F.001
G0 X.32
Z.15 M9 (M9 is coolant OFF)
G28 W0. U0. (automatic return to ref point before tool change)
T0200
M1
N4
G50 S2000
G97 S1000 M3
T1200 (VNMG-331)
(GROOVE MARK ON FACE)
G0 X.7 Z.15 T1212 M8
G1 G99 Z.05 F.01 (set feedrate type to Feed per Revolution)
Z-.01 F.002
G4 P500 (Dwell for 0.5 seconds)
G1 Z.05 F.01
G0 Z.15 M9
M5 (M5 stops the spindle)
G28 W0. U0. (automatic return to ref point before tool change)
T1200
T0600
/M12 (M12 is 'end of cycle' the / means that it is optional depending on whether the option switch on the control is on or off)
M30
%
------------------------------------

[mflux_gamblej]

Your tool offsets are in relation to the G50 "start point" ( usually the machine "home" position) and the part/program zero.

Your offset value will be a -X(dia) -Z, because you're in a +X and +Z (yeah, I know, seems backwards.. I'll explain) in the home position.....

The control must know the position of EACH tool at its start point, in reference to program zero. The start point is usually the home position of the tool.

If you draw a picture of the outline of the part and the program zero along with the tool in its home position, you'll see that the tool is in a very positive X position, and it's also in a very positive Z position, relative to the program zero. In order to move the tool towards the program zero, it has to move in -Z. 'Zat make sense now?

Hope this helps a little.
Keep your hand on that big red button!!

Yep, your description makes perfect sense. Because I set the offset equal to the x and z distance from the chuck face, The tool wants to take this offset out of the position if it is given absolute z 0 x 0 at the home position.

what i don't understand is when the machine wants to move to the tool offset position (which would be inside the stock, at the chuck face and lathe axis) which will definately crash! Additionally, I believe that I tried setting g50 x0 z0 at home last night and it didn't work. I'm sure that your description is the correct setup, but I'm not sure of:
- the code
- when to call g50 (multiple times I assume / every tool change?)
- if you look below at the previous owner's code this isn't the case
- why the tool moves to the tool offset (which will always crash or unescessarily move to the tip of the stock if set there)

Here is MY code from last night - it makes a chess pawn (obvious 1st program ):

------
%
O0001
(PROGRAM NAME - PAWN 01)

G20

G28 U0. W0.
T0700
T0707
G97 S785 M03
G0 X.9731 Z2.6707
G50 S3600
G96 S200
G99 G1 X.8317 Z2.6 F.005
Z.7167
X.8347 Z.7141

///// do some moving around//////

X1.0485 Z.4557
T0700
G28 U0. W0. M05
M01
G28 U0. W0.
T0100
T0101
G97 S898 M03
G0 X.8505 Z1.1453
G50 S3600
G96 S200
G1 X.6394 F.002
G4 P.5
G0 X.8505
Z1.2175
G1 X.6419 F.0025
G4 P.5
G1 X.6708 Z1.2031
G0 X.8505
Z1.073
G1 X.5793
G4 P.5
G0 X.8505
Z1.2898
G1 X.6019
G4 P.5
G0 X.8505
Z1.3061
G1 X.4236
G4 P.5
G0 X.8505
Z1.3281
G1 X.4236
G4 P.5
G1 X.4525 Z1.3137
G0 X.8505
Z1.0579
G1 X.4236
G4 P.5
G0 X.8505
Z1.0359
G1 X.4236
G4 P.5
G1 X.4525 Z1.0504
G0 X.8505
G96 S3000
Z1.4363
X.7858
G1 X.6444 Z1.3656 F.002
X.5831 Z1.3359
G3 X.5692 Z1.3331 I-.0069 K.0071
G1 X.4136
Z1.3011
X.5597
G3 X.5748 Z1.2977 K-.01
G1 X.627 Z1.2678
G3 X.6319 Z1.2613 I-.0076 K-.0066
G1 Z1.1815
G0 X.7285
Z.9267
G1 X.587 Z.9974
X.5343 Z1.0275
G2 X.5193 Z1.0309 I-.0075 K-.0066
G1 X.4136
Z1.0629
X.5329
G2 X.5459 Z1.0653 K.01
G1 X.6158 Z1.0952
G2 X.6227 Z1.102 I-.0065 K.0076
G1 X.6242 Z1.1113
X.6295 Z1.1464
X.6319 Z1.1629
Z1.1815
G0 X.7858
G96 S200
X1.3
Z.382
G1 X1.1 F.0025
X-.02
X.18
G0 X1.1
T0100
G28 U0. W0. M05
M30
%

[mflux_gamblej]

In their code they're calling the tool offset, along with the rapid back to the workpiece.

G0 Z.15 M9
G28 U0. W0. (automatic return to ref point before tool change)
T0800
M1
N2
G50 S4000 (G50 followed by spindle speed, sets max spindle speed = to given value)
G97 S2634 M3 (M3 is spindle on, CCW [forward direction])
T0900 (1/4" B.B.,ROUGH)
G0 X.29 Z.15 T0909 M8
G1 Z.02 F.005

In my code I have been calling the tool offset, then spindle speed, then rapid back to workpiece.

X1.0485 Z.4557
T0700
G28 U0. W0. M05
M01
G28 U0. W0.
T0100
T0101
G97 S898 M03
G0 X.8505 Z1.1453
G50 S3600
G96 S200
G1 X.6394 F.002

According to the Fanuc 6T manual, when you call a tool offset as either T0101 or G00 T0101 they do the same thing - rapid to the tool offset position.

Additionally, in the manuals the tooling offsets are described as small numbers - the distance from a standard tool to the other tools for example. In this case, rapiding to the tool offset wouldn't be a problem.

I am assuming then that the other style where you call the rapid to near the workpiece along with the tool offset will be executed simulatneously resulting in a non-crash. I will go try this instead.

[txcncman]

In this case, G50 X Z sets the machine coordinate zero shift relative to the turret position. Normally it is employed by returning the turret to home position (G0 G28 U0. W0.) the commanding the shift to be X0. Z0. Then the tool offsets will work as described before. If you set the tools off the chuck face and your part zero was 4" out, you could command the move to home position and then a shift of G50 X0. Z4. This would then bring all the tools out 4" from the chuck face to match the part zero. Some machines you have to do the G28 move first and then G50. Other lathes just work off G54 (commanded or not - or G55, etc.).

[mflux_gamblej]

Since the offsets are the distance from the zero (chuck jaw in Z, lathe axis in X) to the home position, you must set the absolute zero at the home position before running a program.

Interestingly this must be done using G50 in MDI mode:
- set dial to MDI
- press COMMD
- press Page --> (to get to the next command page)
- press G50, input, Z0, input, X0, input, Start

Now the position is stored. This is always from the home position, since the tool offsets are defined as described.

What I observed is that you cannot set the zero's using the ORIGIN button. It seems that the origin button only changes what the DRO/display reads - but DOES NOT actually tell the machine the work absolute zero:

- Press POS
- Press Page --> (until it displays X, Z)
- Press X ORIGIN (DRO reads X 0.0000)
- Press X ORIGIN (DRO reads Z 0.0000)

So, I had set the machine's absolute to X 0 Z 0 using the origin button at the home position, and using G50 at the home position. When you run the a program in full auto mode, the absolute DRO reads out all negative numbers (not what the program says).

It seems that you want to setup your ORIGIN at the chuck / axis zeros, but setup the G50 x and z zeros in MDI mode when at the home position.

In my case, U and W readouts and positions aren't of concern to me yet since I don't output relative movement g-codes to use in the program?? I did set them 0 0 at the home position, but using the ORIGIN not using G50 U W


The code (of course) needs to be as the previous owner's code shows - calling G28 U0 W0 to go home, cancel the previous tool offset e.g.
T0700
call the next tool, T0100,
start moving to the part + activate new tool offset, G0 X(#.####), Z(#.####) T0101

I've got a couple more subtleties to work out in the code, but I cut my pawns last night!!! One in Delrin, and another in 6061

[mflux_gamblej]

Here's a video of some of the toolpath: https://www.youtube.com/watch?v=jyDb7IpXeCM

I've got some learning to do about depth of cut, surface speeds, tooling, and cleaning up my codes - but there's no denying that CNC lathes are pretty badass!

[txcncman]

Good job. If you do not want the part dropping off in the chip pan, program the cut off to stop at about X0.090 and then you usually can twist and break the part off by hand. I would also recommend pecking the cut off to give you some chip control. Other than that, get rid of some of the air cutting and you will be good to go.

[mflux_gamblej]

Good job. If you do not want the part dropping off in the chip pan, program the cut off to stop at about X0.090 and then you usually can twist and break the part off by hand. I would also recommend pecking the cut off to give you some chip control. Other than that, get rid of some of the air cutting and you will be good to go.

I'll definately check out pecking the cutoff. For the air cutting - I had already roughed that part with the coolant on/door shut. So the air cutting isn't as bad as it looked.

Thanks for your help man - sometimes you just need someone with experience to tell you to shut the f* up and go do it. Tool offsets are a pain if you don't know what you're doin'