Fanuc Lathe system T codes

[KovatechCNC]

Hello all,

New to Fanuc lathe systems for lathes, more used to milling. anyhow I have discovered that by simply calling up a tool change IE: M06 T2; flags an error. read further in the manual and it would appear the T Code needs to appear as T0101, T0202; and so on.

Does anyone know why this is the case for lathes?

Similar Threads:

• Need Help!- Takisawa TS-20 CNC Lathe - Fanuc 3TF System turret problem
• Newbie- (Download)FANUC Series 30i/300i For Lathe System USER’S MANUAL
• Need Help!- 600 PC ALARAM IN FANUC 6T SYSTEM - MORISEKI SL2A LATHE
• Need Help!- Need full list of G CODES AND M CODES FOR FANUC 21I
• Fanuc SYSTEM 5/Mori lathe set-up

[the_gentlegiant]

Like you I come from a mill background recently to lathes. There is no such thing as M6 on a lathe. In fact there are so many things different about Fanuc lathes compared to mills that I strongly suggest you get some operation manuals, especially from your machine tool manufacturer and read them front to back.

Why you ask are are tools called like T0101 or T0202? Because that's how they are called. Get used to it. T0100 calls turret position one but does not call an offset with it. T0101 calls tool 1 and includes offset 1, but understand it doesn't physically move anything until you add a move command of some sort. You will see the offset reflected on the absolute position screen. That being said you might call T0100 to bring the tool into position in a safe area, and call T0101 as you move towards the workpiece. If you want to assign more then one offset to the same tool for whatever reason, it's generally accepted practice to use offset 17 for T01, offset 18 for T2 and so on. In short, add 16 to the tool number.That is if your machine has the basic 32 offsets available. So calling something like T0117 is totally acceptable, if dual offsets for the same tool is what your program needs are for the job at hand.

Get some books. Read tons, or you're going to mess that lathe up sooner then later. Fanuc Programming and Operation Manuals for your particular control are good and readily available. Programming and Operations Manuals from your machine tool manufacturer are better. Each of those books are a separate item.

[g-codeguy]

There is such a thing as M6 on lathes. On our EMAGs it calls up coolant for O.D. tools. M8 is used for both internal tools and external tools so an O.D. tool can have both M8 and M6. On our Nakamura TW-20s M6 calls up high pressure coolant and can therefore have both M6 and M8 on any tool. Otherwise the_gentlegiant is absolutely right.

Remember a machine builder can assign M-values as they see fit. Luckily the most common M-codes/G-codes are used on all lathes (that I am aware of). However, it is my experience a builder is more apt to use a different M-code than a different G-code. Manufacturers use different M-codes for opening and closing collets/chucks and for barfeeds, and for turning on spindles with coolant started with the same command. M13 for Hardinge, M63 for Daewoo, M463 for Doosan while many lathes have no such command and M8 must be used. Know your lathe.

For lazy farts like me G01 becomes G1, M01 becomes M1. Know that you can do the same thing with a tool call. T101 is the same thing as T0101 and T121 is the same thing as T0121. T100 calls up Tool 1 with no offset.