What's new
What's new

G code, tool numbers?

Higgins909

Aluminum
Joined
Nov 19, 2018
I've only done basics with G code on Haas mills. and even more basic on a Mazak Mill. (didn't know how to call tooling in the rush I was in so I worked around it) This Mitsubishi LT-350 lathe with Navi is a bit different. On the Haas it's just T1 T2 T12 T20 T32 etc. On lathe I've seen T0101 and T303 T909 T707. I don't understand it that well. There is also some sort of tool registration that makes it more difficult to understand. (So not only the tool number, but the tool registration number) I was trying to call tool 3 in the turret with T203 and it kept on giving me tool 2 on the turret, which is a C drill. This was a tool number in the tool file, so I assumed it was being used. After fiddling with it for a while it was found that T303 would give me the right tool. I just don't understand what the numbers mean in the T code. What is the first 0 in T0101 mean? What if I just went T101? What if I put in T111 or T100 or T110? Does each number place have a specific meaning? For now I think everything repeats it's first number in the 3rd number spot. I'm not sure about any tooling 10 and over. (12 tool turret)

The first number in a 3 digit T code seems to correspond with the tool, but what do the others mean?

Thanks,
Higgins909
 
It's for multiple tool offsets for a single physical location. Say you have two boring bars in a two-station holder, on the same physical turret location.
Or maybe an offset for an insert drill being used for drilling, and an offset for using it as a boring bar.
So you've got basically T <2 digit hardware offset> <2 digit software offset>
http://www.mdtooling.com/images/Mori_turret_54_tools.jpg
On that machine, you'd have 12 actual tool locations and up to 6 offsets for each. You might run T0101, T0121, T0131, etc. You've gotta find the system that works for you.


On a mill you call an M6 T# then call a G43 H#. Same thing, physical location and software offset. Maybe you have multiple saws on an arbor, or you have run out of tool pockets and you want to use T20 (which you leave empty) and then have 5 other tools you manually change that have a software offset recorded in your machine. You might call T20, then H21/22/etc

Most of the time you're going to have a matching T# and offset #, but it can be useful to have different ones for various reasons.
 
On a lathe, the first two digits after the letter T are for the tool number, the third and fourth digits for the tool offset. T0101 means change to tool 1 and use the tool 1 offset.

When you used T203, you told the machine to change to tool 2 but use the offset from tool 3. Good thing you didn't send it because it would have been a disaster :D
M6 command is not needed on lathes.

On a mill T01 means tool 1 and you have to use G43 with the appropriate tool height offset which in this case it would be H1, so M6 T1 G43 H1.
 
The first two are the tool position number, which you can see with your eyes, and the second two are the offset number, which you can see on the “offset” page. Well, I should say I think the “last and second to last” are the offset (usually 0-99) and the “first of three or first two of four” are the tool number. So T222 is tool 2 offset 22, just like T0222 would be. T2222 is tool 22 offset 22. And T2202 would be tool 22 offset 2. I believe is it good practice to use all four places in the “T” word, even if the first digit is “0”.

They are often congruent (i.e. “T0101, T2727, etc) but they don’t have to be. It just depends on how your offsets are assigned. Sometimes you may be machining numerous features with the same TOOL but use more than one OFFSET to get those various features within spec. So one feature may use, say, T0202 and then another feature T0222.
 
On a lathe, the first two digits after the letter T are for the tool number, the third and fourth digits for the tool offset. ......

The first two are the tool position number, which you can see with your eyes, and the second two are the offset number, which you can see on the “offset” page. ......

Not all Fanuc equipped machines will behave the same. By parameter setting, the high order T address (first 2 digits after T) call the tool and can call the tool geometry offset while the low order digits (last 2 digits of the T address) call the wear offset. The machine builder or user can set this to their preference.
 
Not all Fanuc equipped machines will behave the same. By parameter setting, the high order T address (first 2 digits after T) call the tool and can call the tool geometry offset while the low order digits (last 2 digits of the T address) call the wear offset. The machine builder or user can set this to their preference.

This is another reason why one should use the offset number same as the tool number. This becomes independent of parameter setting.
 
One really simple solution is to READ the programming manual for the machine. As Vancbiker said, not all machines are the same and not all tool call parameters are set to the same function even with the same control.
 
Not all Fanuc equipped machines will behave the same. By parameter setting, the high order T address (first 2 digits after T) call the tool and can call the tool geometry offset while the low order digits (last 2 digits of the T address) call the wear offset. The machine builder or user can set this to their preference.

Example of what that looks like, please. I've never seen that. I don't think?

I guess by your description, the format would appear identical, but not do the same things.

R
 
Not all Fanuc equipped machines will behave the same. By parameter setting, the high order T address (first 2 digits after T) call the tool and can call the tool geometry offset while the low order digits (last 2 digits of the T address) call the wear offset. The machine builder or user can set this to their preference.

are you talking about the old 10t like on a citizen?

uses T1500 to call up turret 1 tool 15, then on 1st move uses T15 to call up wear offset.
 
Example of what that looks like, please. I've never seen that. I don't think?

In the line T0101, the 01 immediately following the T indexes the turret and activates the geometry offset in register 1. The last 01 would activate the wear offset.

Couple of reasons it can be nice is it simplifies use of multiple offsets.

When you use multiple offsets (ie. T0101 and T0141) to separately control sizes on different features with the same tool it eliminates the need to set geometry values (and keep them matched) in register 01 and 41. Just set the geometry in register 01 and tweak the wear in 01 and 41.

Some builders of machines with measurement devices will link the cursor on the offset page to the turret position selected when the measurement function is being used. This eliminates the operator from having to scroll the cursor to the register to be set and eliminates the need as above for manual entry of matching geometry values in the alternate register.

are you talking about the old 10t like on a citizen?

uses T1500 to call up turret 1 tool 15, then on 1st move uses T15 to call up wear offset.

Many versions of controls. 10T,11T,15T,16T/18T, 16iT,18iT, all have this ability. For example, on a 16T/18T series parameter 5002 bit 1 determines this behavior.
 
Last edited:
I misunderstood. I personally don't use the wear offsets, so it just didn't click for me.

R

Yes, I should have mentioned earlier.... This parameter is only applicable to machines configured with both wear and geometry offset registers. Not all builders spec that option from Fanuc.

As with so many aspects of the Fanuc controls, the machine builder has a huge amount of responsibility or latitude in how the control behaves on their machines. Plus in many cases the end user or their tech can often set machines from different builders to behave similar to each other.
 
Not all Fanuc equipped machines will behave the same. By parameter setting, the high order T address (first 2 digits after T) call the tool and can call the tool geometry offset while the low order digits (last 2 digits of the T address) call the wear offset. The machine builder or user can set this to their preference.

Why would one prefer that? I am curious to know because it makes no sense to me to have it that way.
 








 
Back
Top