Tool # problem

[Powder Keg]

Hello,
I'm new to CNC so please bear with me. I am using an older Supermax mill with a Fanuc OM control on it. It does not have a toolchanger so I have to change then manually. The problem I'm having is that when a program calls for a tool number the program pauses. The green cycle start button stays lit, but nothing happens? If I press reset it will continue on, but, it will skip the line of code under it. Also It is not picking up the tool size in the control.

I would like to be able to use the tool # to be able to change the size of the tool so I can adjust the sizes of my tools if needed.

Any suggestions?

Thanks, Wes

[Jung]

Should use G41/G42 Dnn, G43 Hnn after M01 instead.

[dcoupar]

What happens if you press the cycle start without pressing reset? Does the program continue on?

The tool # shouldn't have any effect on the size of the tool (either length or diameter).
As Jung says, use a G43 to activate the length comp (H01 - H??) when you rapid down to your clearance plane after the tool change. To adjust for the diameter or radius, use G41 (tool left) and G42 (tool right) with an H (or D). Most of the old Fanucs used H for length AND diameter, but some used H for lenght and D for diameter. If you're stuck with just H, you'll probably go with H01 - H20 for length, and H21 - H32 for diameter.

I disagree with the M01 as Jung suggested, as you have to have the Opt. Stop switch on, or it'll go right past it. I would use M00 instead, unless the M06 is working correctly.

[Powder Keg]

Thanks guys, I'll give that a try. I use the M00 in case I forget to press the optional stop.

If I press the cycle start nothing happens. I'll mess with the G43 and G42 and see what happens.

Thanks again foe your responses, Wes

[Dan Fritz]

Since you don't have a tool changer, the T-command will not do anything, and there isn't any "finish" signal from the tool changer telling the control that the tool change is complete. Consequently, the control will just sit there waiting for a T-code finish signal that will never come. That's why you get stuck with the cycle start light on.

Why bother to use a T-command? The T-codes automatically call up tool offsets on a lathe, but not on the mill. You can just use G43 Hxxxx or G41/G42 Dxxxx to change offsets, and you can cancel an offset with G40.

When you're in the middle of a program and hit RESET, the control clears it's buffer, so one block of data gets dumped. There's only one way to avoid that: Don't hit RESET. If you use the G40/41/42/43 commands, you won't have to.

[Kakarott]

the control may identify tool no. by the offset position u give.

In my system Fanuc 6T, it is a linear tooling m/c, so it does not have turret hence it recognises the tools by the offsets only.

[Powder Keg]

So If I use length offsett No. 1 then It will look at tool one for a diameter compensation in the tool file? I'll try that.

I tried a G41 H21 with H21 set at .002" and it went from the 2'' diameter pocket that I was milling out to about 25"?

Thanks, Wes

[Jung]

Offset tool length: G43 Hxx (in Offset Setting set item xx), cancel H offset with G49.
Offset left/right (to change tool diameter) with: G41/G42 Dxx, cancel D offset with G40.

[rick_7037]

Also on Fanuc 0M I believe an M6 will still cause the machine to go home in Z and stop cycle.
always remember to cancel G49 offsets /H0 /D0 stacking them up can be catastrophic...and expensive.
no one is mentioning different offset methods...long offset method reference tool method short offset method....lots of ways to get a naked cat here....
just an observation out of boredom here. ITS FRIDAY!