CNC lathe tool and work offsets

[DareBee]

Originally Posted by HuFlungDung Darebee, I don't claim that my way is the only way You feel free to explain alternative methods.

Hey man - that wasn't a dig, just showing my ignorance in the matter - JK.
In a couple of days, weeks, months, ? I hope I can be knowledgeable enough on the subject to actually have a "Way"

You guys are helping - Thanks

[imwllc]

in x all of your tools are touched off on the spindle centerline, and when the x in the g54 is always at zero this is where it always goes for x zero, in the program when you change tools(index) the line may read: G0 T1010;- which tells it to index to tool ten and pickup offset ten, then in the next line pickup a work offset like g54 or g55. the x will be correct as long as it was taught correctly

[HuFlungDung]

Darebee,
I didn't think you were taking a dig at me. I thought maybe you did have a different method to offer

I should back up a bit and say that there are two methods of setting tool offsets on every machine, whether it be mill or lathe. The operator needs to decide if he is going to use an absolute reference point, or a relative reference point to set the tools to.

On a mill, some guys will set the tools off the top of the part. This is a relative reference point. It has drawbacks: If the next type of part is a different height, all the tools must be reset, even if they are the same tools. A-hah, they say, they will just use the G54 to take care of that. Sure. Except, they have to add in a couple more tools for the new program. The old part is gone, now what do they set the new tools off of?

On the mill, using an absolute reference plane might be a little more work, but it is worth it. Use a "standard" of some sort to set all your tools off of and stick with it. No matter what job, any old tools can be trusted to have the correct offset, as will the new tools that you have to add. There is a little bit more work involved though, because instead of leaving the G54 Z at or near zero most of the time, you actually have to measure the difference between your tool setting reference plane and the top of the part. But once that is done, you are good to go.

Lathe is similar: using the relative method, some guys will set all the tools off a given workpiece. For this method, it doesn't matter where T1, the reference tool is truly located in the machine coordinate system. The tool offsets will be the distance from the G28 position to the face of the part. Again, all the Z offsets must be reset for every part that has a different Z face position. It is possible to fudge new part Z0 positions with G54 offsets, but pretty soon with additional tools added in, you get yourself lost, because you've got too many relative offsets involved.

So, if you always set your tools Z offset off of a single known reference plane such as the chuck face, or a standard jaw height, then those offsets become portable and correct in any work coordinate system that you want to use.

I'll continue a bit later.

[HuFlungDung]

There are a few parameter options to explore in lathe that determine how you will do your tool offset measurements. These options have to be known, otherwise you may attempt to set offsets by a certain routine, and they will not be correct.

On some systems, a parameter setting will decide if the tool measurement point is (or is not) a pre-defined point in the machine's coordinate system. If the machine has a tool eye (presetting device), then the location of the sensors is defined by parameters. The sensors are so and so far from the X0Z0 of the machine G53 coordinate system. This is an absolute reference point, but in and of itself, represents an internal offset from the machine G53X0Z0. When this point is correctly set in parameters, it means that when T#1 (reference tool) touches the sensors, the offsets (in the offset table) should be zero in both X and Z.

It is not strictly necessary that the T#1 offsets actually be zero, but theoretically, they should be. Once again, we see how important it was to have the machine coordinate system set correctly relative to T#1.

The wonderful tool eye system simply allows you to then touch all the rest of your tools off the sensors, and the offset measurements are calculated and recorded by a few key presses.

Without a tool eye, most guys would rather use the manual measurement system. Many controls have a method to assist you by auto-calculating the offsets by following a given procedure. On the Mitsubishi, I can take a cut, then immediately press an axis button to store the position, then back out of the cut, and then input the actual measured diameter. The control calculates the offset automatically from an internal comparison of the stored value with the measured diameter.

Now, to do the offsets entirely manually, the same procedure can be followed, but longhand. The controls typically have several options for the displays, showing the current position in
1), the machine coordinate system,
2), in the current work coordinate system (if one is active), or
3), in the operator screen coordinate system (G52, I believe). The operator display of position is quite ambiguous, as you can zero any axis on the operator screen at any time. You just need to find the keystrokes that do it.

If T#1 reference tool is already defined correctly, you can jog it to touch any accurate surface that you have chucked, and the display in the G53 machine coordinate system should give you an accurate reading of the current diameter setting of T#1. You can even take a cut with the tool to prove it. But as luck would have it, lets say it is off by a small amount. You simply calculate the difference and enter that into the X offset for T#1.

Now, we cannot arbitrarily change the coordinates in the G53 machine coordinate system. But, we can switch to the operator position screen and zero it whenever we like. So lets zero the X axis in the operator screen while T#1 is still touching the freshly cut surface. Jog clear of the work, measure the part, and jog (handle mode) the X axis towards X0 centerline. Now, we have measured the diameter of the part, so we know where X0 should be. However, the operator display will show us moving into X- but that is ok. Move to an X- value that equals your measurement of the diameter. Zero the operator display again. Finally, T#1 is accurately located for the purposes of the operator position display, and we must remember to not zero the operator display again until the rest of the tools are set.

Begin to touch the rest of the tools off the cut surface, using a shimstock to feel the moment of the touch. Each time, note the position on the operator display, and if it does not match the actual measured diameter of the part, then either a positive or negative difference is calculated and entered into the X offset for that tool. Positive or negative is dependant on which way the new tool is offset relative to T#1. There is a 50% chance that you'll get it right if you don't know what you are doing

Watch out for yet another parameter setting in your control, that reckons the X offset amount to be either diameter or radius values. Diameter is the easiest choice, if available, because you don't have to worry about the "divide by two thing".

For your manual Z offsets, simply touch all the tools off the chuck. Again, touch T#1 first and zero the Z axis of the operator position display. Now, touch all the rest of the tools off the chuck and enter the value shown in the operator position display into the Z offsets for each tool.

Now, go back to T#1, recheck that the display is still zero when touching off the chuck face. Chuck the part, and move the tool so that it touches the face of the part. Retract in X and, if necessary, move a few thousandths in Z- to give yourself a facing amount. The Z value shown in the operator position display will be your G54 offset amount, if your machine's G53 Z0 is located at the chuck face.

[DareBee]

Nice post Hu
Thanks for taking the time to be so comprehensive.
Considering I run the VMC with all tools Z0 on the table (to expidite set up) and program my part above Z0 (as you have mentioned above) it would only stand to reason for me to datum my lathe tools similarly for ease of single part runs.

[mm4039]

Thanks for the great posts here, this has really brought me along on understanding how to properly setup my machine/tools. I think I am almost there, but not sure, so I thought I would throw my thoughts out here and let you guys tell me if I'm getting there, or still lost - partially lost...??

The item I am most confused of is how the machine coordinate system is set vs. the way I would like it to be set. I would like it set so that X0 is where my reference tool #1 is at spindle center, and Z0 is where this same tool is touched on chuck face. The machine is NOT set this way now. It is close to this, but not exact. If I am understanding correctly, I am unable to change this??

At this point the way I would go about to setup the work/tool offsets is like this -
Home machine, zero the relative displays for X,Z, with tool #1 (ref. tool) in cutting position touch that tool to the chuck face and enter the value on display for the Z offset for tool #1. For X find postion for when this tool is on spindle center and enter that value for the X offset for tool #1. Next, jog off to a safe spot and index turret to next tool and repeat the same procedure for Z, X offests. Repeat this until all of my tools are completed. When I am ready to cut parts - re-home machine and with tool #1 jog and touch face of chuck, zero the Z axis display. Jog over and touch tool to face of part - enter the value on Z axis display into the G54 Z offset. If I want clean up stock, subtract .020", .030" (whatever is needed) from the display value (the Z axis # will always be positive) and enter that value.

In this manner there will never be any X axis offsets in the work offsets, reason being the tool offsets are all set to center of spindle. The work offsets will only have Z axis offsets. The only thing I have to absolutely make sure of is to call the work offset after each tool change. This makes sense to me, so I hope I am on the right track. Please post if you see something that is wrong, or may cause me problems down the road. Again, thanks for the sharing of knowledge.

[HuFlungDung]

I don't have any manuals for your particular controller. However, someone must have programmed the reference position at some time (in parameters), so it should be adjustable, but the trick might be to find out where to tweak the settings. As I mentioned earlier, a good place to look is at the G28 settings. The G28 position is set after the machine homes, and from this position, the origin of the G53 system is inferred as being so and so far away from the G28 position.

This might be one of those parameters that won't take effect until you shut down and restart the control.

Now, as I read the rest of your method, I think the one thing you may have done "wrong" (aka different ) is that for T#1, you should set the display to zero when the T1 touches the chuck reference face. This is because you want the Z offset of T1 to be zero, and all others get set from there.

If you do it the method you described, then you might have quite a large Z offset for the T1, and this will throw you way out of position when measuring the G54 from the reference face of the chuck.

Just try it out (carefully, with rapids turned down low) and see how it pans out.