[TZak]

Hi Everyone

Im looking to find out if anyone can explain how to setup tools on this type of lathe. I am just learning to operate this machine and wanted to know if there are any resources for this(as the manual I have is not the greatest). Or if someone can walk me through it. I understand how to operate and setup a cnc milling machine and have built my own cnc router. But for some reason I can''t get a grasp on the lathe for setup.

Like it says in the title its a fanuc 21t controller on a 2 axis monarch lathe.

Any help would be appreciated.

Thanks

[timlkallam]

Tool seting fanuc 21

To set work shift
move the tool to to your zero point( touch off tool 1 in program)
press off set key
press right arrow soft key TWICE( the soft keys are under the screen
there are no markings on them)
on the bottom of the screen you will see (w shift) press the soft key under it you should now be in the workshift page.
Upper left hand corner of of work shift screen the is x and z
highlight the Z press 0 input ( change the number to 0)
on the bottom right of the screen there is a number z xxxxx(relative)
enter that number as a NEGATIVE number in the upper left (where you just changed it to zero )
Now that bottom right number should read zero and your workshift is set.


To set tool length offsets
index to second tool in program(example tool 2)
touch off tool
go to the geomertry screen highlight z in tool 2
push off set Measure key (this is not the same key as off set key)
press Z0
push measure (soft key under screen)

To set diameter offsets
Take a cut with the tool you want to set ,(ex tool 2 )move the tool off the work buy moving z axis.
stop spindle
measure workpiece
go to geomerty screen Highlight x tool 2
press offset measure key (this is not the same key as off set key)

type x and the diameter size (example X1.625)
press measure (soft key under screen)

[TZak]

Hi Tim

Thanks for the reply. I tried out your procedure and got my tooling set. It made sense once I started through what your wrote.

One other question. How would you set up drills and taps?

Thanks

[timlkallam]

Drills and taps are set at x0 Tram your drill holder get it exatly centered push measure key type in x0 then press measure key .

example to drill a 1 inch hole 2 inchs deep
T0101(1 INCH DRILL)
S750M3
G0X0Z.1
G1Z-2F.005
G0Z1

If your tapping in your lathe you need a tension and compresion tap holder. It lets the tap float a little because your spindle
will not stop exactly the same time as the z axis will .

Hope this helps
Tim

[TZak]

Tim

Thanks for the reply. This may be a stupid question but how do you find the centre? I understand setting X to 0. And touching off the end of the part for the other Z0. However how do you know you are exactly at the centre for the X.


Thanks

[timlkallam]

Put an indicator in the chuck tram the inside of the drill holder move x using the mpg until it is centered and that will be X0 for your drill.

[TZak]

Ok I think im getting the hang of the work shift ??? And setting tool lengths. However in the g-code what specific things do I need to make sure are in it. With the work shift do I need to call up a G54? Do I need to set the work shift for every tool or does doing the offset for each tool take care of that and the work shift is only for the touch off tool. Then use a specific g-code.

If someone can provide some simple sample code and just give a run down of it that would be great for starters.


All the best