Newbie- G54 ?

[dave6]

Here is a program I am trying to run on my Meldas L3 lathe. I have done the MDI G54 entry for program zero 6" out from the chuck face to set up program zero. All my tool offsets are set correctly I believe. Every time I try to run this program it wants to start working 1" into the chuck (not good). Changing the G54 number setting makes no difference. Is G54 assumed or should it be called up in the program somewhere. Also is there anything in the file that would mess up G54 program zero? Can you suggest a FOOL proof way of setting this up or changing the file. This is my first program on this machine after a year of overhauling it.(the program is made from a pps that is also new and under development).
Thanks Dave

[Caprirs]

That G92 is setting a local zero. Remove that and see what happens. G54 is default but it never hurts to put it explicitly in the program.


O0010 ( Lathe Tool Bushing )
N5 G20
N10 G00 G40 G97 Z2.0 X1.0 T0000 M09
N15 T0101
N20 G92 S4500
N25 G94 G96 F5.0 S164 M03
N30 X1.6128 Z0.1645
N35 G72 U0.05
N40 G72 P45 Q75 U0.0 W0.0

[dave6]

Thanks for the response....I will give this a try on Friday.

[HuFlungDung]

G92 S4500 is okay because that sets the spindle 'clamp speed', provided that you have set it correctly for the chuck and work at hand.

I would also say to put the G54 in the program.

Of course, you need to know unequivocally where machine zero is, before you know where you are shifting the coordinate system to with the G54.

The location where the machine homes to, may or may not be machine zero, as it is likely possible, through parameters, to assign values to the home position when homing is completed.

Command G00 G53 Z0 T0 and see where that sends the tool to. Do this without a part in the chuck, and run at slow rapid override in case a collision looks inevitable. Once you know that position, then G54 Z is relative to that point.

How you set your tool length offsets may also have some bearing on tool position.

[dave6]

I will try what you suggested to find zero. From looking at the parameters I think the zero will be at the machine home position for both Z and X . What is (G92) spindle clamp speed? Running the code block by block watching the G54 number, the G54 stays the same until line N30 then the number in the G54 changes a difference of about 8" before making a move and of course distance to go changes about the same.

[HuFlungDung]

G92 S spindle clamp speed is a safety command used to keep from over-revving the spindle based on the characteristics of the job at hand. Although there is a maximum spindle speed set in parameters, it is not always safe to even go that fast.

I like to insert the spindle clamp speed after every tool change, in case I start mid program and the control needs to be reminded what max rpm is for this job.

G53 Z0 is most meaningful if it corresponds to some constant but accessible point of reference on the machine. I set my lathe up so that G53 Z0 is at the chuck face, but that is just me I never remove the chuck (it is a self-contained power chuck).

So once I chuck up the first part, I can simply measure with a tape measure from the chuck face to the end of the part, and enter that amount as the G54Z value. I tweak it from there, if sometimes the stock is a bit short, or too long.

[dave6]

I would like to have my ref. point set up as the face of the chuck also. So you use a G53 (say -12") ? for that then G54 is the distance from G53 to the part end as a positive #?

[Geof]

Originally Posted by HuFlungDung G92 S spindle clamp speed is a safety command....

I am confused; I thought G50 was spindle clamp on nearly every lathe.

I do know on a Haas lathe G92 is a threading cycle.

[stevo1]

Dave,
In order to get the tool to be 0 at the spindle chuck you have to change your 1st reference position parameters. I don't know what kind of control you have so I am not sure what parameters to look up.

Once you have this parameter you have to put the distance from chuck face to machine orgin in this parameter. Now when you program as Huflung has said G53Z0 or you can just Z0 and it will want to bring the tool to the chuck face. These numbers are usually in metric @ a 3 decimal place but you don't use the decimal when inputting. So if you wanted to put in 300.53 mm you have to type 300530 input. If you type 30053 it will read it as 30.053mm.

Huflung is 100% correct many people set up there machine in different ways but I set up all my machines as this procedure. Your tool's are always offset so all you have to do is put your part height in G54-G59 and specifiy that in the program. Now when saying G0G54Z0 the tool goes to the top of the part.

Almost forgot. You will have to change the soft overtravel limits. The machine now has a new home so you have to build your overtravels around that. I usually go 2.54mm past the home position parameters. You also have to power cycle the machine to have the 1st reference parameters take effect.

Stevo

[HuFlungDung]

Originally Posted by Geof I am confused; I thought G50 was spindle clamp on nearly every lathe. I do know on a Haas lathe G92 is a threading cycle.

Yes, it could be either way. The Mitsubishi has an option to select Gcode system 2 or system 3, which transposes certain gcodes.
When I see a command like:
G92 S4500
that tells me that the programmer expected system 3, as otherwise that command makes no sense.

[HuFlungDung]

Dave6,
Does your machine have a tool eye on it for setting tool offsets? This is just an inquiry as to how complicated resetting machine zero might become.

When you power up and home the machine now, what do you see on the G53 position display? And where is your reference tool tip in relation to the chuck face and spindle centerline at that moment (tape measure). This might give us somewhere to start as to what your expected settings should be in the parameters. For a reference tool, I would recommend an OD turning tool in the turret homed position. This tool would be one that you are unlikely to ever remove from the turret.

[dave6]

OK I tried a bunch of suggestions and this is what I have come up with so far. When I delete the line asking for the first tool everything seams to go to a reasonable position. So I think my set up for my tool data or tool offsets are wrong to begin with, I will have to look at those again. G53 is machine zero home position which is the top right hand side on my slant bed lathe. My machine does not have a tool eye for tool setting. My machine is set to use G code system 2. Stevo1 my control is a Mitsubishi Meldas L3 and I will look for those parameters, they may be set for a collet chuck and I have a three jaw which protrudes more. So you say its a machine parameter that sets G53? I am familiar with the travel and over travel parameters, but these dont set zero do they?