Understanding the TXXXX offset function on a Fanuc

[Stotty666]

Hi so recently moved jobs and I'm working on a fanuc VTL. During some of the 'training' at the new place we came across an interesting discussion topic which I am starting to think I dont understand so I'm after a bit of enlightenment.

What does a typical T0101 offset do and how is it structured. I was always under the assumption that this command in the program called the tool up and applied the geometry and wear kffsets.... but how it does it I don't understand.

There are two tables in a fanuc operating system in the offset page thos being wear and geometry.

Obviously we can use multiple offsets for e.g. T0102 or ever T3496. Tool 34 offset 96.

Right so with all that being considered what are the last two digits of the offset and how does it differentiate between the different geometries.

I thought that the first two called the tool up and applied applied geometry offset adjusting the POS data on the screen by the amounts in the geometry page and the last two digits puck up the WEAR offset which is usually under 1mm or 0.039 thou.

However I am being told that the first two only change the tool. The people teaching kr training me actually laughed in my face when I told them my understanding understanding of it.

I'm willing to admit defeat but what I don't understand is how can a tool pick up a geometry and a wear offset from the last two numbers when you can use two different combinations of geometry and wear on the same tool.

Does this make sense?

Basically TXXXX;
What does it mean and how is kt made up also how does it work.

An example I used to try and confirm my understand was same tool with different offsets e.g. a long boring bad machine a bore with a step that pushedls off due to the stick out of the part of boring bar where it pushes off the further you get down the part. Having multiple offsets on the same geometry would get around this e.g. T0101 for front of bore and T0102 for back of bore.
The only difference is the wear offset in the wear page....
How would the offset pick up the geometry if my hypothesis is incorrect?

E.g
T0101 would pick up T01geometry and apply T01 offset,
T0102 would pick up T01 geometry and apply T02 offset.
If what they were saying is true you could not use this to obtain the same outcome unless T02 has the same geometry as T01.

I feel like they don't understand this or my understanding is wrong.

The last two digits do not apply wear and geometry combined as if this was the case you couldn't differentiate between different offsets and tools the offsets would always have to be relative to the tool position.

Am I stupid?

Similar Threads:

• Need Help!- Tool Offset and Work Offset Locking on Fanuc OiMD
• Newbie- Gcode - set axis offset function
• Need Help!- Fanuc 16iMB - Z-Work Offset with "Measure"-function incl toollenght?
• Need Help!- Fixture Offset Function (CALL OO88) - Limitation
• Need help! Fanuc Work offset, Geometry offset

[Heavy_Metal]

Hi,


Your story is partially correct and so is theirs.
T0101 calls Position 01 ( Geometry ) and Wear Offset 01, let's say you have a 12 station turret with 1 Tool per holder and you want different Wear Offsets per tool
then you use T0113 - T0114 - T0115, a number higher then 12 for the Wear Offsets, it is not common to use T0102 because 02 is the (first) Wear Offset for Tool 02.
For Tool T0202 you can use T0220 - T0221 - T0222 with Wear Offset 02 - 20 - 21 - 22 etc for extra Offsets, for Tool T0303 you can use T0330 - T0331 - T0332 with
Wear Offset 03 - 30 - 31 - 32 etc.
It gets harder when you have a Half Index 12/24 tool turret to set Offsets, or a 12 station with Y-axis with double/quad tool holders with left/right Offsets and sub-spindle.
The first two numbers are for Tools but actually the last two also, e.g. a double Tool holder uses the second numbers for the Geometry for that Tool. A second Tool on holder T01 can use T0150 to call station 01 with Geometry 50.
The numbers for that Geometry you have to store in GEO 50 and use WEAR 50 for correction.
It depends on the parameter settings (FANUC) how things work properly for the tool Txxxx Geometry and Wear offsets.
regards.

[deadlykitten]

hy stoty, i will make a bit of general explanations, with examples for different machines

background can be particularized, to fit whatever machine/lathe/mill you wish

explanations will go the other way arround, ending with T, and not begining with it

for a general/simple operation, such things must be known :
... what post to index to ( will be refered as atc-pos, thus position of the tool magazine )
... where is the tool cutting edge tip ( will be refered as tool-xoy; thus coordinate for cutting edge )
for a compensation operation, is also required to know the radius ( will be refered as rad ); how turning do not use revolution tools, but asymetrical ones, it is required to know also the position of the tool nose arch in respect to arch center ( will be refered as quad;similar to trigonometric quadrants)

thus is needed for the operator ( and/or for an automatic initialization mode ) to input data for:
... atc-pos : in most cases, this field is not initialized in a virtual manner, but only a real tool mounting inside a phisical pot/post occurs
... tool-xoy : there has to be a table for tool corection, that can be offset, offset+wear, offset+wear1+wear2, etc
... rad : there has to be a table for radius, radius+radius wear, etc
... quad : there has to be a table for P

futher more, previous data, has to be referenced inside the program; please notice that reference is not always directly to [ atc-pos. tool-xoy, rad, p ], but may be indirect; difference is simple :
... direct reference means that each item of this set [ atc-pos. tool-xoy, rad, p ] is being linked, thus ratio between input data field and reference fields is 4:4
... indirect reference ocurs when ratio is not 4:4

for example, on :
... lathes, rad & P are most times referenced both, toghether, thus ratio becomes 3:4
... lathes with pivot, mill-turn centers, rad & P & tool-xoy can be referenced all toghether, ratio is 2:4

so far, conclusion is that :
... input data ( during machine setup ) is a set of 4 items [ atc-pos. tool-xoy, rad, p ]
... reference data ( used in automatic mode ) is a set of 2 3 or 4 items; it can be also 1 item, but this is a particular case; more on this later, below the line below

reference data is being activated through g-code, and depending on machine type, g-code defaults can vary; examples :
... okuma mill with side magazine :
...... atc-pos is used T syntax
...... tool-xoy and rad is used G56 H* D* syntax
... okuma turret lathe :
...... atc-pos, tool-xoy , rad & P is used T syntax

on most machine T involves mainly a magazine/tool index reference, thus it will index the magazine ( side magazine or turret, etc ); thus atc-pos is nailed to T, while tool-xoy and rad is not always nailed to T

after the magazine is inposition, next thing to do is to use that tool :
... on side magazines(mills, multitask lathes) , is needed a comand to take the tool from the magazine and put it into tool-chuck/spindle
... on turret lathes, turret will revolve, and it itseld is the tool-chuck
*many have doubts on the difference between T on mils and T on lathes; but to put it into the backgournd explained so far, T is always referencing the magazine/atc-pos, while tool-xoy rad & p may or may not be referenced also by T

---

those g-codes examples show how to enable the references to input data

initial reference is milestions/critical, always done in a single manner, and requires the use of a wcs

those [ atc-pos. tool-xoy, rad, p ] are related to tool, while wcs is related to material

after this initialization occured, is possible to talk about optional/partial references

an options/partial reference will not go to the full set of [ atc-pos. tool-xoy, rad, p ], but to a subset, including single items, for example :
... is possible to change from left to right side of a grooving insert, by changing only tool-xoy;same technique can be used for drills with chamfer adapters, or to autoinitialize a corection to counter tool wear, like raise X after 5 parts ?!
... not so coomon, but is possible to change rad, from some particular reason
... is possible to reference only atc-pos, when sending turret away ( offset is no longer needed to reach a consistent home position )
*and examples can continue

as a conclusion, partial/optional refrences, thus a call to a subset of [ atc-pos. tool-xoy, rad, p ] can not occur unless the full set was previously iniitalized

for specific fanuc examples, i am sure that a fanuc person will elnghten you

---

please, so far, if you have questions, feel free to ask

in other words, a T comand is folowed by an argument, which is longer or shorter, depending on how many items of set [ atc-pos. tool-xoy, rad, p ] are being referenced

that argument, varies with cnc brand, for example Txxyyzz and Taabbb, etc may reference the full set[ atc-pos. tool-xoy, rad, p ], but 1st ones uses a ratio of 3:4 while the second uses a ratio of 2:4, even more :
... Txxyyzz :
...... xx reference to rad & P
...... yy rererence to atc-pos
...... zz reference to tool-xoy
... Taabbb :
...... aa rererence to atc-pos
...... bbb reference to rad P offset

what makes it a bit tricky is that most times, ratio is not 4:4 and is even far far away from that, when it comes to subsets; for example :
... Txxyyzz may have subsets Txxyy and Tzz
... Taabbb may not have subsets, or may have ?!

is important to undersatnd that T argument is calling initial data through a ratio that is not 4:4, and it varies with cnc brand

if it matters, is possible to program a machine without using Ts, and still make it take corections, etc

an useful aproach, is to use a custom syntax that pleases you, like you wish, then leave the particularities, for each machine, to the postprocessor / kindly

[JohnDonlan]

Hi so recently moved jobs and I'm working on a fanuc VTL. During some of the 'training' at the new place we came across an interesting discussion topic which I am starting to think I dont understand so I'm after a bit of enlightenment.

What does a typical T0101 offset do and how is it structured. I was always under the assumption that this command in the program called the tool up and applied the geometry and wear kffsets.... but how it does it I don't understand.

There are two tables in a fanuc operating system in the offset page thos being wear and geometry.

Obviously we can use multiple offsets for e.g. T0102 or ever T3496. Tool 34 offset 96.

Right so with all that being considered what are the last two digits of the offset and how does it differentiate between the different geometries.

I thought that the first two called the tool up and applied applied geometry offset adjusting the POS data on the screen by the amounts in the geometry page and the last two digits puck up the WEAR offset which is usually under 1mm or 0.039 thou.

However I am being told that the first two only change the tool. The people teaching kr training me actually laughed in my face when I told them my understanding understanding of it.

I'm willing to admit defeat but what I don't understand is how can a tool pick up a geometry and a wear offset from the last two numbers when you can use two different combinations of geometry and wear on the same tool.

Does this make sense?

Basically TXXXX;
What does it mean and how is kt made up also how does it work.

An example I used to try and confirm my understand was same tool with different offsets e.g. a long boring bad machine a bore with a step that pushedls off due to the stick out of the part of boring bar where it pushes off the further you get down the part. Having multiple offsets on the same geometry would get around this e.g. T0101 for front of bore and T0102 for back of bore.
The only difference is the wear offset in the wear page....
How would the offset pick up the geometry if my hypothesis is incorrect?

E.g
T0101 would pick up T01geometry and apply T01 offset,
T0102 would pick up T01 geometry and apply T02 offset.
If what they were saying is true you could not use this to obtain the same outcome unless T02 has the same geometry as T01.

I feel like they don't understand this or my understanding is wrong.

The last two digits do not apply wear and geometry combined as if this was the case you couldn't differentiate between different offsets and tools the offsets would always have to be relative to the tool position.

Am I stupid?

First of all let's get something straight: the stupid person is the one who does not ask the question..... But assumes. There are no "stupid" questions. Your question indicates a thirst for knowledge that will help you become a better Machinist and machine operator.... And there is absolutely nothing stupid in that. It is commendable that you even care!

Now let's get down to the understanding of the code. The first two numbers call out the tool so that the machine can find it when you want it. These CNC machines have large tool carousels and there must be a way to write it into the program so that when you want a specific tool..... The machine can find it and load it into the tool changer. The first two numbers after the T-code are for this purpose.

On any tool, as it wears down, you will have to adjust it with micro adjustments (a .0010 or .0020 or .0030 along the x or y or z axis) so that the parts will still come out within spec to the drawing. That is what the second set of numbers is for. It calls out a spot in the computer's memory (called an "offset") that tells the computer to make that tool move over a given distance in order to compensate for the wear on the tool. A typical example would be on a lathe, with the diameter needs to be cut .0015" smaller in order for the parts to remain within tolerance (because the tool has worn a bit). So that adjustment would be put into the offset represented by the last two numbers in the T-code. Thus, you are in effect adjusting for the geometry of the worn tool.

Now, let's get fancy! Suppose you had to use that tool for doing both roughing passes...... And then later on, we're doing a finishing pass. When you call that tool out each time in the program you could apply the two different offsets..... One offset for the roughing passes, and the other offset for the finishing pass. Just suppose if you want to allow more (or possibly less) material on the part after the roughing operation. You could have an offset that would allow you to make that minor adjustment.... And then you could have an offset that would allow you to fine-tune the finish pass.

You store the amount of adjustment for each offset..... In the machines controller under that offset number. For example, you could store the adjustment offset number 34 (the roughing passes) ..... And then store the adjustment offset number 56 (the finishing pass). If your tool is number 21 (let's just say), then when you call it up to do the roughing passes you would use the t-code "T2134", and the controller would apply the adjustment that you have stored in that offset to the tool. Then, when you go to do your finishing pass, you will call out the t-code "T2156"in the controller will apply the offset you have stored for the finishing pass.

Here's another example. Supposing that you have a chamfering tool that has to put a chamfer on several holes of different diameters. Now suppose that all of these holes are on the same plane (same level surface). You could apply one offset (the last two numbers of the t code) for one size diameter hole, and then apply another offset for another size diameter hole.... And so on. Your program would simply tell the chamfering tool to rapid traverse to .100" above the surface of each hole, and then feed down to the proper chamfer depth (for that diameter hole) by calling out the proper offset number for that diameter hole.

Just remember that the first two numbers of the t-code pull out the tool number in the carousel..... And the last two numbers call out the fine adjustments that you have stored in that offset for that tool. Think about it.... It will become clear soon.