[mbam]

When I fire up my Cincinatti Hawk lathe (Fanuc 21t) the start positopn is about 17" on the X and 25" on the Z

I'm scared to death of crashing this thing so I want to completly understand every thing my cam program is doing.

Looking at the code the first lines are

G18 G20 G40 G80 G90
G00 G28 U0. W0.

The way I understand it G28 is going to send the machine to X & Z 0 which will promptly crash it.

So why is this there? And on a similar topic how do I move the turret to a safe position for tool change? I see that my post might need some editing.

[ShovelheadMark]

Never dealt with a Cincinatti ... but G28 is turret home u0. and w0. is kinda silly because it tells the machine to move incrementally 0.0 , but back to the G28 , that should actually be the safest place for a tool change ... but as I said never dealt with a Cinc only Haas lathe.

EDIT: I forgot G18 G20 G40 G80 G90 is what is refered to as a safty line
G18 = xz plane
G20 = inch dimensioning
G40 = Cancel cutter comp
G80 = Cancel canned cycles
G90 = Absolute positioning

[mbam]

Hmmm....
Yes I would have thought the first thing to do would be to move it to a safe position. And I assumed that is what it would do, but then I started to do a reality check. BTW - this CNC lathe stuff is all new to me, I have not cut a single piece yet.

Here are a series of pictures at startup. The first is after power on, the second is after the "homing" routine (offset 2 happens to be in effect). This puts the turret as far from the chuck as possible. Then the third picture is with the tool as shown in #4

Just looking at the pic it looks like U0 W0 will put the tool tip at the centerline and right on the chuck. And that would mean it is using the tool and work offsets.

I can't get any more grey hair but I do have some more I can lose.

[dcoupar]

It appears as if your machine is set up with G-Code system A, in which case G90 is a "Canned Cycle", not Absolute.

With Fanuc in G-Code System A you can program absolute (X Z) or incremental (U W) or a combination (X W / U Z):

G28 U0 W0 (to send both X and Z axes directly to their home position)
G28 U0 W2. (to move Z+2.0 THEN X and Z directly to home)
G28 X6. Z3. (to move X to 6.0 and Z to 3.0 THEN X and Z directly to home)
G28 X0 Z0 (to move X and Z to absolute 0 THEN X and Z directly to home) > this is not recommended.

You'll notice that in Single Block that G28 requires 2 cycle starts: the first will execute the intermediate move, the 2nd will execute the move to home position.

[ShovelheadMark]

Oops .. forgot about the 'other' system , been dealing with mills mostly , I stand corrected

[mbam]

So am i right that G28 W0 U0 will put the tool tip at the centerline and right on the chuck in this case?

[ShovelheadMark]

Nope it should send the tool all they way home. machine home not workoffset home .

EDIT: If you are really unsure turn your feeds , rapids and spindle way ... way down , put your finger on the e-stop button and let 'er rip... but that's just me

[mbam]

Wouldn't that put Z0 at the reference point on the spindle? That's the part I don't understand, not exactly a place to send the turret.

Yes - I need to see how far down they will go, and start at the Z max lol
I have done that more times than I can count, but on a much slower machine!

[ShovelheadMark]

Hahaha , yes I do prefer mills them lathes can move awfully quick and the worpiece moves very quick . Again I am only trained on a Haas lathe , the G28 command will send the turret all the way to the right back as far as it possible goes and ( at least on the one I trained ) that is the safest place to do a tool change. But try this put the machine in MDI ( manual data input ) and type
G18 G20 G40 G80 G90
G00 G28 U0. W0.
then hit start .
there is no toolchange in these lines and no spindle command so it should be very safe to see where the turret ends up. ( I do operate a lot by trial and error and that's usually what I do when I am unsure )


EDIT: darn I always think of something after I hit submit , do not confuse G28 with G54 if that is what you are referring to when you say Z0. , your G54 Z0. is where your part 0. is the G28 is where the machine has its 'Home' or 0. position.

[mbam]

Ok - sounds like a plan, I will report back in the AM - Thanks!

[ShovelheadMark]

Great I gotto run too , besides the network here at college is so damn slow today it drives me nuts ( more then I already am )

[dcoupar]

So am i right that G28 W0 U0 will put the tool tip at the centerline and right on the chuck in this case?

I think maybe you're confusing Part (Absolute) Zero and Machine Zero (Home).

G28 U0 W0 moves X and Z to directly to Machine Zero <-- use this to move turret to safe index point.
G28 X0 Z0 moves X and Z to Part Zero THEN to Machine Zero <-- DON'T use this

[mbam]

Ok, got it figured out. The thing that confused me were the explanations I read previously that referred to machine 0 (home) , it is not actually 0. It is the machine reference position. Which in this case is about 17" on the X and 25" on the Z

On my machine the readout that shows machine position is actually 0 at the spindle centerline and a point on the spindle.

dcoupar your comment and the readout on the display is what started me thinking. It didn't make sense to me as for sure going to 0 per the display was going to crash it.

So sure enough I put my big boy pants on this AM and did a G28 W0 X0 and it went right to the startup/reference position.

How can I tell if it is a format A? I did a G90 all by itself and nothing happened. Would I expect an error if it was looking for more parameters?

I see my post processor put a G0 on the same line as the G28. No need for it, correct?

[ShovelheadMark]

Glad you got it figured. If I remember right a G00 would be a good thing if your previous move was a metered ( G01 G02 G03 ) move otherwise it will veeeery long to get to machine home .

[dcoupar]

Parameter 3401 bits 7 & 6 (leftmost 2 digits): setting both = 0 selects G-Code System A
As for the G0 on the G28 block, I'd leave it... it's certainly not hurting anything.

[mbam]

dcoupar, I finally have a program loaded and ready to run.

Yes it is clear I have G-Code System A. And the G90 produces an error. So is System A something I want? My manual says B&C are options (and I don't know if I have them). If A is my only choice do I use something else for setting absolute?

Boy - what I would give to have someone visit and get this running for me

[ShovelheadMark]

Again I hope I am not talking out of my rear ... on the Haas if you program x and y you are automatically in absolute in order to use incremental you substitude U for X and W for Y and the machine will move in incremental mode.

[mbam]

Thanks, I kind of thought that was it. It made sense if there was no absolute switch. I just need to modify my post-processor and then figure out the next issue

I am getting an error on a G96 line. We had a bunch of thunderstorms come through today so I shut the machine down. Back at it in the AM.

I am so ready to run this thing finally!

[ShovelheadMark]

Best of luck to you !