[BrianSP]

Please help me to continue learning how to most efficiently use my mill.

I am quite pleased with some of the individual items I've made so far and now I am getting into fixtures and multiple workpiece positions.

Presently I set machine zero and then move to the fixture zero, touch off the tool, and G92 this position to X0Y0Z0. After this I have got the idea of the G54 etc.

Question1, on my workpiece offset screen the first offset is labeled "Shift" followed by the expected G54 etc. What is the "Shift" position used for?

Question2, I see that some people avoid using G92. Is there a better (safer, more flexible) way of entering fixture zero?

Thanks

[sinha_nsit]

WCS shift is available on lathe, but not on milling machines, as far as I know.

I also do not use G92. G54 through G59 (plus 48 additional coordinate systems, as a control option) are available for specifying different datums, in all machining sessions. Effect of G92 is temporary. You need to do it again in the next session.

[beege]

Shift or "Common" work offsets affect all of the other offsets by the amount in the shift. If you have a tooling plate with several fixtures on it, you can record the G54 -G59 offsets somewhere, and when you load the plat onto the machine, you can use the shift to fine tune the location of all the fixtures at once.

Also, look into G52 (local coordinate systems) for setting "relative" coordinate systems on that same fixture plate.

I will NEVER be using G92, since all these other options have come along later to replace the dangers of using G92.

[BrianSP]

Thanks gents,
Beege,
G52 is not included as one of my Gcode options which is why I was wondering how, and if, I could use the "shift" settings. The extended workpiece offsets are turned on in my control unit.

This is probably going to seem like a very stupid question to most people on the forum but how would I avoid using G92 in my present set up. The fixture is based on an angle plate since I am working on the ends of some aluminum square section tube mounted vertically. There is a piece of 0.5 inch ground aluminum plate permanently bolted to the angle plate to support the parts. The fixture reference is a specially machined corner of this aluminum plate. Presently I mount and align the angle plate, G92 to the reference points and then G54 etc to the individual workpiece coordinates. These are the instructions I was given by the original machine owner.

When I carry out the machine zero on start up the coordinates are set to zero. Would there be any advantage in driving to my fixture reference point and inserting the displayed coordinates into the "Shift" offset table? Apparently I can set a default work reference by parameter but this would not help me very much.

Sorry if this is a dumb question but I am trying to learn and the manual is no help since it only refers to G92.


.

[HuFlungDung]

When you power up the machine, do you home it to establish machine zero, or does it just come up as machine zero wherever it happened to be at the moment when it shut down?

There is nothing dangerous about using G92 to establish the machine coordinates, except that you must be diligent to reference to exactly the same point, time after time. If the control has no accurate homing procedure on startup, then you have no choice but to set the machine coordinates with G92 (in MDI mode). I used to run machines that had no homing procedure. It was a PITA to find and set G92 to some arbitrary fixture point, but it had to be done.

[BrianSP]

HuFlung,

This is a Kent box-way mill with Fanuc O-MD controls. I have the Fanuc yellow manuals plus a very sparse (photocopied) machine manual.

On start-up I manually drive the table to the reference position with the "Mode" selector switch set to the "ZRN" position. The table reference position sensing uses micro-switches. If G54 is set to all zero values the table reference position resets to zeros otherwise it displays the G54 position.

You can use the mill manually without referencing but I do not think it will allow you to run a program without referencing first.

[HuFlungDung]

Ok, so it sounds like it holds the G54 until you reference it. You could dispense with the G92 in that case, but then you'd need to pretend G54 is your machine coordinate system, and use G55 or higher for all your work offsets.

However, I'm not certain how accurate the reference point is when made to a microswitch. If you had a power fluc while machining something, then you'd want to know the reference position to the nearest 0.0001 so that you could find your way back. I think I'd use an edge finder against some permanently attached square corner, rather than a microswitch.

If you are comfortable with setting the machine coordinates at some defined reference with G92 in MDI, I would say to continue doing so. Just refrain from ever using G92 written within a program unless you are fully aware of what will happen if the G92 command is executed in some random position (like after aborting a program part way through).

[BrianSP]

The subject is becoming a little more clear now but I can see that I have a lot of thinking to do.

[angelw]

HuFlung,

This is a Kent box-way mill with Fanuc O-MD controls. I have the Fanuc yellow manuals plus a very sparse (photocopied) machine manual.

On start-up I manually drive the table to the reference position with the "Mode" selector switch set to the "ZRN" position. The table reference position sensing uses micro-switches. If G54 is set to all zero values the table reference position resets to zeros otherwise it displays the G54 position.

You can use the mill manually without referencing but I do not think it will allow you to run a program without referencing first.

The Reference Return position is governed by more than just the micro switches you refer to. This switch only gets you close, the exact position is gained with the axis encoder. Accordingly, this position can be relied on.

Regards,

Bill

[sinha_nsit]

Shift or "Common" work offsets affect all of the other offsets by the amount in the shift.

I refer to it as EXTERNAL WCS.
WCS shift is in addition to it, available only on a lathe.

[stevo1]

As Beege stated "shift" and "common" are going to adjust all of your coordinates without having to set each one. As an example if you were to machine a part that is exactly 2" tall and you wanted this to be Z0 you could put 2" in your G54 and this would be zero when G54 is specified. This holds true if you put 2" in the Z of G55, G56, G57, G58 and G59. What "common" does is if you were to put .1 in the Z of the common "ALL" of the coordinates of G54-G59 would be treated as 2.1"

IMO if you have G54-G59 you have no need to do any shifting with G92. Find what you want as part X0Y0Z0 and set it in any one of G54-G59 and go. As Hu stated if you use G92 you can lose yourself very quickly if you do not reference back to the same position.

Stevo

[sinha_nsit]

Another example of External WCS (I will stick to the term I use):
You may have a "compound" fixture which holds six workpieces at six different places, all needed to be machined with their own WCS, G54 through G59.
If you place the fixture on some other place on the worktable, you need to modify only External WCS, with respect to a known reference point on the fixture, since the relative positions of all WCSs remain fixed with respect to this reference point.

[gbowne1]

I have not needed to shift with G92.

Generally I'm pretty careful where I put G54 and G55. Well, I generally use vise fixtures, so I'm pretty confined at times but I keep track of my part X0Y0Z0 along with all the other references, including the homes, ref positions, offsets for each job.

As in my situation, generally workpieces/stock are the same size so I am pretty safe.

The switches do get you pretty close. I keep careful setup notes so I record a lot of data thats probably not needed. But I have it in case I lose some data or forget where I'm at during a job or when setting up.

I've been doing as described in the other offset thread I posted in.

[BrianSP]

Great information

So, to use a simple example, I have one of the electrical contact set-up sensors with a 0.2 inch diameter probe. Therefore, whenever I use this probe I have to adjust the zero work reference setting by 0.1 inch in X and Y to find true zero. The way I do this now means physically moving the probe, making darn sure the axis selection is correct to avoid a crash, and then I use G92 to set zero. Using "shift" I could just touch off on the X and Y faces, call this zero for G92, and then adjust the position with the "shift" offset and avoid the possibility of a stupid crash with the probe.
I could even use a "shift" offset that was nowhere near the workpiece as long as relationship is known.

Thanks Gentlemen, this could be useful and it adds another item to my CNC knowledge.

[angelw]

Great information

So, to use a simple example, I have one of the electrical contact set-up sensors with a 0.2 inch diameter probe. Therefore, whenever I use this probe I have to adjust the zero work reference setting by 0.1 inch in X and Y to find true zero. The way I do this now means physically moving the probe, making darn sure the axis selection is correct to avoid a crash, and then I use G92 to set zero. Using "shift" I could just touch off on the X and Y faces, call this zero for G92, and then adjust the position with the "shift" offset and avoid the possibility of a stupid crash with the probe.
I could even use a "shift" offset that was nowhere near the workpiece as long as relationship is known.

Thanks Gentlemen, this could be useful and it adds another item to my CNC knowledge.

The stupid crash is more likely to come from the fact that you're using G92 than anything else. Even if you use a "shift" offset for the probe radius, you still have to apply it in the correct direction, so you gain nothing by using it, as apposed to applying the probe radius to the G92 coordinate set.

All previous discussion in this thread has been along the lines of using an EXTERNAL WCS to apply a global shift to all work offsets G54 to G59. This is useful when various work offsets are being used in a program, where if you shift one, you need to shift them all. If your program is using only one work offset, or G92 only, there is no point in applying an EXTERNAL WCS to correct the position; you simply edit the work offset or G92 that's being used.

If you apply the G92 from the Reference Return position, and you use G28 to ensure that the slides are at that location prior to the G92 being called, then the G92 is relatively safe (but not completely). The danger is if you don't use such a precautionary approach, and therefore the G92 can be executed when the slides are at a position other than where they should be when the G92 is executed.

For example:
The program has to be halted because a cutting inset failed. The spindle is moved to a convenient location to be able to change the insert, and because this location is visually close to the tool change, or program start position, in the heat of the moment the program is restarted. Using G92, the work coordinates will be out by what ever the position error was when changing the insert. You now have a potential crash on your hands, or at best, a ruined part because the feature is now being machined in the wrong spot.

In contrast to the above, no matter where the slides are when the G54 to G59 is executed, the control knows exactly where the spindle is relative to the workpiece zero. The values for the G54 to G59 are obtained in exactly the same way as for G92, but your fixed reference point is the Reference Return position. The only difference being is that the slides don't necessarily have to start from that point, whereas the slides MUST be at the same known reference before the G92 is executed. In my opinion, if the machine has the workpiece coordinate system G54 to G59 option, its tantamount to having a dog and barking yourself, not to use it.

Regards,

Bill

[stevo1]

Bill.....I could not agree more. Well explained.

Stevo