[ashisroy]

Please help me to understand. I'm having hard time to understand the difference between Geometry & Work offset(G54) and their application in Fanuc Lathes.

If I touch off part face (Z) and set G54 Z0 [MEASURE] do I need to set Geometry offset Z0 [MEASURE] too? Why two different offset in same machine for same Z touch off? Please help me to understand their difference in application.

[zavateandu]

you can work in 2 ways:with G54 or without it
1.using G54 ---the G54 is the distance from the reference point of the Z axis untill the piece(the face of the turret is taken)
so if you want to set up the G54 on Z axis you must theoretical go with the face of the turret and touch the piece but in reality you have to use a gauge block 100mm and inserted between the face of the turret and piece ,move the Z untill easy touch and type z100. measure in the G54 area for Z
after this you have to measure all the tools lengths and insert the values in the table of geometry of the tools because every tool has a different lenght and also will travel diferent from the reference.
2.without using the G54
many operators are using the tool number 1 to make the Z0 ,they go and face the part a little or just touch it and than go to the page with the measure value and workshift value and type there in the measure value Z0 and in the geometry of tool number 1 will be also 0 .(no value need it there but only tool number 1)
then every tool will be measured considering the tool number 1 as reference.(you will see all the values from other tools will be with - or + because are measured considering the edge of the tool 1 as 0)

in conclusion if you work with G54 you have to use no tool for taking the 0 of the piece ,you need to set up the distance between the face of the turret and the piece and than measure all tools from number 1 to how many you have.
take tool number 1 ,go touch the piece and go in geometry and set z0 measure,tool number 2,etc

so try to separate the 2 things,using G54 or not ,this 2 methods i explained can not work together and i think is exacly what you are doing or what you do not understand.

hope i was clear enough.

[flick]

Editing this to add, I just noticed you were asking about lathes, not mills. My explanation below is still pretty much valid if you replace "table" with "chuck" and "spindle" with "turret", and ignore the reference to G43.

Cheers.

2.without using the G54
many operators are using the tool number 1 to make the Z0 ,they go and face the part a little or just touch it and than go to the page with the measure value and workshift value and type there in the measure value Z0 and in the geometry of tool number 1 will be also 0 .(no value need it there but only tool number 1)

What you are describing is the "master tool" system. It requires a value in G54.

Offsets are just values added to a Programmed Coordinate, resulting in a Machine Coordinate. Offsets are how the machine knows where along it's axes the Program Coordinates start.

The Z offsets in G54 (or G55, etc.) are combined with the Z offsets loaded for each tool with G43 to determine the total distance from Machine Zero to Program Zero.

I know of 4 distinct ways to manage how G54 (or any other Work Offset) is combined with the Geometry Offset loaded by G43.

1. The simplest way is to not use G54. The Geometry Offset for each tool is the Machine Position with the tool physically touching the workpiece at the Program Zero. In order to physically touch the workpiece at Program Zero, you may need to start by facing it.

I call this the simple method. It is distinguished by the fact that you have a just one variable reference point (the workpiece) on the table.

The major disadvantage of this method is that you must touch off ALL of your tools any time you want to change the Program Zero, such as when you run a different program.

2. The next simplest way is to set one Geometry Offset to 0. The Z value in G54 must be set to the Machine Position with that tool physically touching the workpiece at the Program Zero. As with the simple method, you must have access to the Program Zero of the physical part. All other tools are set to the difference between the Machine Position while they are touching the workpiece at Program Zero, and the value placed in the Work Offset (such as G54) by the first tool.

I call this the master tool method. It is distinguished by the fact that it uses a variable reference point (the master tool) in the spindle.

The major advantage of this system is that you only need to change one value (G54 - the Work Offset) when changing your Program Zero. A disadvantage is that if the master tool changes length for any reason, Geometry Offset for ALL the tools must be changed.

3. Another method is to use the table, or an indicator on the table, or a block on the table to set the Geometry Offsets. All Geometry Offsets are the Machine Position with the tool physically touching the table/indicator/block. The G54 Z value is the difference between the Geometry Offset of any tool, and the Machine Position when that same tool is physically touching the Program Zero of the workpiece.

I call this the touch setter method. It is distinguished by the fact that it uses a fixed reference point on the table.

The advantage of this method is that you can determine your Geometry Offsets at any time without the need for a workpiece, and the Geometry Offsets are stable as long as you have a block of the correct size to place on the table.

4. The final method is to use a fixed reference point on the spindle. The Work Offset is the distance from the spindle nose to the workpiece, and Geometry Offsets are the length of the tool sticking out of the spindle nose.

I call this the offline method, because Geometry Offsets are usually determined with a fixture and height gauge outside the machine. G54 is still set by touching any tool to the workpiece at Program Zero and calculating the difference between the Geometry Offset and the current Machine Position. The advantage of this method is that Geometry Offsets of a tool are valid for any machine in the shop.

The offline method is not for a hobbyists or beginners. The simple method is a good way to get making chips quickly for beginners. Hopefully you will see the limitations of the simple method and move on to the master tool or touch setter methods eventually.

[sinha_nsit]

If need to use just one tool, then G54 alone is sufficient. Set it with the tool you would be using.
But, if you change the tool, the cutting point of the next tool would not not match with that of the first tool, because all tools are geometrically different. In such a case, you will have to use geometry offset. The term geometry offset originates from the fact that it takes care of difference in geometry.

[ashisroy]

zavateandu, flick and sinha_nsit.... Great advice! Thanks a lot for explaining in details ! I liked the number 2 method - using G54 and use one tool as reference! Appreciate the detail concept - that is what i was looking for !

[sinha_nsit]

In the master tool method, if the length of the tool changes because of some reason, its offset may be corrected by its geometry offset. If we do not change work offsets, offset of all other tools would remain correct.

[flick]

In the master tool method, if the length of the tool changes because of some reason, its offset may be corrected by its geometry offset. If we do not change work offsets, offset of all other tools would remain correct.

It's tempting to think this, because the master tool geometry is established with the work offset. The problem is that every other tool is also affected by the work offset. So if you correct the work offset for the master tool, the other tools will remain out of sync with it.

Example: In a program that just faces a shaft and machines a snap ring groove, the tool used for facing is the master tool. As the master tool wears, the parts become longer, and the snap ring groove ends up farther from the face. If you move the work offset (-Z direction, to the left) to correct the length of the shafts, the snap ring groove will also move (to the left), and will still be too far from the face (but now it is also too close to the other end of the shaft). In order to compensate for this you would have to add to the grooving tool (and all other tools) whatever amount you subtracted from the work offset.

I acknowledge that for many applications these variations are small enough to disregard. The amount of variation can also be reduced by careful selection of the master tool - for example a CNMG insert tends to be positioned very consistently, and usually remains in the turret for every job whereas a drill in a collet holder can stick out almost any length, and may be removed for some jobs. The master tool method is very popular for the lathe, and many shops are quite satisfied with it. But it's drawbacks can still be problematic for some applications: think of a machining center equipped with a large magazine. Imagine having to adjust 200 tools just because your face mill was damaged and needs to be replaced! You've basically blown the whole morning, just to keep your offsets in sync.

The touch setter and offline methods which use fixed references are much more stable than the simple method or the master tool method which use variable references. The master tool method is still a BIG improvement on the simple method, but my favourite method for both mill and lathe is the touch setter method, because it uses a fixed reference without all the extra tooling need for the offline method.

[sinha_nsit]

Even if the master tool on a milling machine needs to be replaced, its offset can be corrected by its length offset, without changing work offsets. Then all other tools would remain unaffected. Of course, the new tool would not be strictly the master tool, but it does not matter.
I prefer the master tool method for manual offset setting. It is simple, if MEASUR key is available.

[flick]

Oh, I misread your previous post - only saw "work offset" and missed that your first reference to offsets was "geometry offset". Yes, you're right of course on both points: adjusting the master tool geometry offset would be an expedient solution to the problem, and it would no longer really be the master tool. I would caution that making ad hoc adjustments like this can lead to even more problems down the line... if you face a piece of stock with the new master/not master tool and set your work offset, the measure function may or may not take the tool offset into account. If it doesn't, then touching another tool off that surface would be inaccurate.

It's clear that you can make it work if you're savvy about offsets, but I wouldn't recommend using the master tool system in this way for a beginner.

[sinha_nsit]

Once set, there is normally no need to redefine work offsets. Geometry and wear offsets are there for making adjustments. These can be defined and redefined any number of times, without affecting other tools. Or, maybe, I am missing some point.

[flick]

Of course you must change the work offset when the job changes.

At that point, you would normally face the new workpiece or touch the face of the new workpiece with the master tool, and use it to set the work offset. But if the master tool geometry has been adjusted, the work offset may be incorrect, depending on how the measure button works on your particular machine.

If you then install a new tool in the magazine, and set it's geometry based on the new workpiece, it will be out of sync with the other tools.

[sinha_nsit]

That is correct and is the limitation of the master tool method.
If the difference between the old and the new master tool is exactly known, then the geometry offsets of other tools may be manipulated but chances of mistakes can be there.