Lathe Tool Offsets - Tool Relationships?

[Chaz]

Hi, suppose this could apply to mill too but let's focus on lathe tool offsets for this.

I've done both both and automated offset management, so have a fairly good idea on how it all works. I would however like to understand the relationship between tools, if at all relevant.

First case, if you watch Keith's older offset video, these are set manually and the 'offset' is effectively the distance from the X home switch. Assuming the home switch is repeatable, then the offsets will always be right.

So let's say I do this method. I'm using tool 1, I cut 7mm, I measure, I get 7mm (diameter).

I swap to tool 2, I cut 6mm, I get 5.95mm. To 'fix' this, I assume I adjust the tool in the offset page, correct? Is there any relationship between tool 1 and tool 2 or is it always back to the offset to the home switch? If, for example, I keep machining and I do a test, and say on tool 1, I'm getting 6.98mm when I should have 7mm, do I adjust this in the tool offset page or do I set the Part X to 6.98mm (when at 7mm location)?

The reason I ask, is I broke / replaced an insert and when I started to check sizes, I started to tweak, but want to be sure that I dont change the wrong thing in the wrong places.

I have always assumed, maybe incorrectly, that Tool 1 is 'master / reference'. And the offsets can be set to 0, 0 on tool 1 and then tool 2 is 'offset' from tool 1. Correcting tool 1 will automatically correct the rest as they are offset from tool 1.

So when we use a probe for tool offsets, are the offsets set against tool 1 or the X home? Ill go look at the tables later again.

Thanks in advance.

[Chaz]

And in the bottom left, I can see another set of offsets. Just watched some of Uwe's vids. That looks like the 'coordinates' for the probe, correct? I assume that's measured from the homing switches?

[Chaz]

In one of Uwe's vids, he also has tool 1 as what looks to be a reference tool. The reason I say this is when you see him finetune, the offsets are like 0.006mm, so it is pretty much zero.

Franco also talks about using a fake tool which he doesnt use for cutting (mill) as reference, that he didnt like the idea at first but now prefers it. Does the same apply on a lathe? If you look at the images, it shows 'ref tool'. How do I know if the reference is this tool or the X home location? Would it be correct that this becomes the reference, if its effectively set at 0 and youve done a skim cut and told the machine the X diameter at that location?

Thanks

[suntravel]

With a skim cut setting part 0 in X, this is the distance from home to X0 with T0101

Setting X Diam on the probe with T0101 is the distance from the probe surface to X0

All other X values in the Tool Lib are the difference to T0101.

So If you change something on T0101, you have to remeasure all other tools if you set Part X and X Diam again with T0101

A way to avoid this is to have a precise ZRI home on X and use tool wear or retouch X in the tool lib for T0101 if you use another insert on T0101, but do not set X Diam again with the new insert on T0101

Uwe

[Chaz]

With a skim cut setting part 0 in X, this is the distance from home to X0 with T0101

Setting X Diam on the probe with T0101 is the distance from the probe surface to X0

All other X values in the Tool Lib are the difference to T0101.

So If you change something on T0101, you have to remeasure all other tools if you set Part X and X Diam again with T0101

A way to avoid this is to have a precise ZRI home on X and use tool wear or retouch X in the tool lib for T0101 if you use another insert on T0101, but do not set X Diam again with the new insert on T0101

Uwe

Thanks. Let me take some time to absorb that. On my Emco I have ZRI now. I need to check it again to make sure its ultra repeatable. Let's assume it is, we use that as a 'master' location and all tools are offset against that? Can that still be done with the touch probe?

[suntravel]

Sure I am doing this all time on initial set up:

Skim Cut -> Part Zero
Tool Set Up -> X Diam
Probe other tools

This works regardless of the probe position, but the stylus size must be set up ok.

Uwe

[Chaz]

Thanks. I'm using the same probe as you and also the same 10mm 'head'. One issue is that I dont have enough space to probe my boring bars. The machine envelope doesnt allow me to come in from below the 10mm 'head'. Perhaps just for that and items such as drills, Ill need to continue to do it manually.

[silver2row]

Chaz,

I have been reading about the same ideas. My current lathe has a cross slide (of course) and the cross slide is not "beefy" enough to promote deep drilling or boring. I will also need to figure out a way to do something with the tailstock outside of the cross slide.

Seth

P.S. I would have liked to not have to do it manually but I am sure there are ways. Off to read more...

[suntravel]

I do all drilling with the cross slide on my cheap benchtop lathe...

If you want to use the tailstock with CNC, make it movable with an stepper/servo..

Uwe

[Muzzer]

One issue is that I dont have enough space to probe my boring bars. The machine envelope doesnt allow me to come in from below the 10mm 'head'.

Same here. The turret on my machine would have to move some way past the axis to allow touchoff of boring bars and drills, so a chuck mounted probe can't be used, even if it didn't require the workpiece to be removed to touch off a new tool. You can still use that touch probe for tool offsets, even if it's not mounted on the axis / in the chuck. You can mount it on a mag base so it's randomly positioned away from the axis and acquire a reference position from a known or reference tool (or workpiece diameter, I forget), then touch off the others relative to it. In many ways it's the same process as used for Z probing, just a different direction.

There used to be a problem with the lathe tool probing software that caused errors for rear mounted turrets like mine but I believe it was reviewed and corrected so it now works. However, it's a while since I wasted hours of my life investigating and fighting that, trying to convince the team there was a problem and I haven't been back following the relevant update, hence I'm a bit hazy about the details.

It's worth bottoming this out, as probing is more accurate than manual methods. You will still have to skim and measure to set the reference offsets but then you should get good repeatability between tool changes.