[Donkey Hotey]

I've got a procedural question for the experienced lathe users here.

I just bought my first CNC lathe (TL-1). My VF-2 has the Renishaw probing system so all of my tool and work offsets are handled by the same two reference points in the machine.

Now I'm getting started with the TL-1. I put a piece of stock in the spindle, touched off each of the tools to the face and diameter and loaded them into the Tool Offset registers. G54 is zero. Everything makes sense to me so far.

I go to load the second part, I touch off the face of the part and load G54 with Z-Face-Measure. The only thing I need between the first setup and the second one is the Z difference in stock position. This also makes total sense to me.

The problem comes when I go to load a new tool (that wasn't preset on the very first setup). The face I originally used to set the tools is gone. It's been replaced by the G54 offset value that I think I'm supposed to reset with each piece of stock.

If I touch off the current part face with the tool, it does so without considering the G54 offset. If G54 is shifted by 0.5", then the tool offset is 0.5" different than the rest of the tools.

Should I just manually alter the tool offset by the work offset amount or should I be setting up the tools and offsets differently? I know it sounds like a basic question but the probing system on my mill has spoiled me.

[HuFlungDung]

Ah yes, the floating reference method! I hate that!

I kind of struggled with the same problem when I was setting up my Mitsubishi cnc lathe. After much head scratching, I came up with a logical method of setting up the machine. Some of this involved changes to certain parameters that required careful study and some trial and error to get things set correctly and logically for my own use.

When the machine homes, do you have a machine position
display? This would be the G53 coordinate system.

Now, pick one of your tools as a reference, typically, I'd suggest an OD turning tool that will never leave the turret, or that is easy to put back in exactly the same position should you ever have to remove it. Ideally, this might be T1.

Now to devise a logical method, I'd suggest that this tool shall be defined with respect to the chuck face. The tool home retracted position is normally where the turret would be parked. Some types of controllers might be set up to call this G53 Z0 at the moment homing is completed, but I'd argue that it makes more sense to redefine that parameter, rather than just giving it a value of zero. Jog and measure the Z length from T1 to the chuck face. If the tool is 16" away from the chuck face, then when the turret is homed with T1 active, the machine position should show G53 Z16.0 I have no idea if you can redefine this by parameter in the controller setup, but its worth a look to see if you can do this.

If you can get that definition correct, then the chuck face is now G53 Z0 and G54 Z is a simple measurement from the chuck face to the end of the part. This can be accomplished with a touch off, or else simply measure the part with a rule or a caliper. Typically, the G54 Z is fine tuned later on anyways, if you need to make a universal adjustment due to stock length variation.

I'd agree that the chuck face is often not a great place to touch the tools off of, so some controllers allow you to define a tool measurement position, just as though the machine were equipped with a tool eye. The tool eye must also be defined relative to the machine coordinate system, but even if you do not have that equipment on your lathe, the parameters can still be of some use.

So, if you made a 3" long cylindrical plug gauge to fit the chuck bore, and that had a shoulder to butt against the chuck face, you could use this as the tool setting reference. Define the length of the gauge as the Z parameter of the tool eye measurement position.

Whenever you have to set a new tool, use the plug gauge as a reference for Z. I suppose if you were to incorporate some kind of a magnetic base thingy, you could affix the gauge temporarily to the chuck face to touch the tools off of.

I don't know if that helps or confuses you more. If you understand the gist of my method, first thing you need to do is understand where your machine is homing now, and what the home position means. If you can, through parameter adjustment, make the home position meaningful to T1, then you have conquered most of the setup problem.

[Geof]

.....If I touch off the current part face with the tool, it does so without considering the G54 offset. If G54 is shifted by 0.5", then the tool offset is 0.5" different than the rest of the tools.....

Have a look at Setting 64 T. OFS Meas Uses Work.

When it is OFF the G54 Offset is ignored and the Z machine position is entered as the tool offset. I think this is what you want?

When it is ON the G54 offset is included so the tool offset is the machine position minus the G54 value. (Or plus, I cannot remember.)

Try both ways and you will see what it does.

[Donkey Hotey]

The TL-1 Haas is a normal 'engine lathe' layout, not a reverse layout with a turret so my 'machine home' is far right, tool post closest to the operator. It reads Z values as negative values from there.

I have considered all the things you shared (gauge bars, master touch-off faces, etc) but I had to wonder if--maybe--I missed something. It seems dumb to me but I guess this is what everybody has to go through.

My worry is that every time I take a wispy touch-off cut to find a tool face, I lose some accuracy. Stack it up between a few tools, add in a work offset and I could be 0.003-0.005" out before I ever hit cycle start. Many of my parts are going to get second and third operations in the mill. The tolerance stackup is what I fear.

I originally had the idea to buy an LED edge finder for a mill and mount it in one of the lathe tool holders to use as a master tool length (exactly as you described).

And exactly as you described, there really is no reliable 'work' position to use. I have a 6-jaw, 3-jaw and a 5C system. Any one of them could be in the machine at a given time so the only reference I would have is the spindle face (that I obviously can't reach with the tooling in place). Maybe I can carefully measure the distance for each and write them down for future offsets.

Now the tool presetter arm in the Haas turning centers makes sense. I wonder if I could fabricate a similar pivoting arm with another LED edgefinder or height gauge that wouldn't interfere with the rest of the machine.

Thanks for taking the time to reply. I was worried that I was heading in the wrong direction or doing it the hard way.

[Donkey Hotey]

When it is ON the G54 offset is included so the tool offset is the machine position minus the G54 value.

Thanks for that. I think that's exactly what I was looking for. Yes, I want it to compensate for G54. If I faced off a bar with a tool of known length (establishing a new Z-zero face) I want to be able to touch off a new tool of unknown length to that Z face and have it relative to all the rest of the tools.

I'll try that out in a few hours. If it works, a Z-height LED presetter could be put into any chuck or collet. A master tool length could be used to establish the presetter's face as G54, then all the tools could be precicely set.

This is very good. Thanks guys, I'll let you know what I find out.

[SeymourDumore]

Donkey

On the Lathe without the toolsetter, you have to turn ON Setting 64 T. OFS Meas Uses Work as Geof has suggested.
In that case as soon as you use a known tool and set the Z0 on G54, you once again have a reference point to which to set your tools.
Actually quite painless once you get used to it. The only problem is when you have to replace a non-inserted tool in the middle of the program, at which time you need some inventive workaround.

[Donkey Hotey]

Yup, it all makes sense now, guys. Setting 64 was the trick.

I'm not really complaining since I'm sure other brands are similar but Haas could really do a much better job on their user and training documentation. They simply describe what settings do but don't give any examples of why you'd want to change them.

If Haas described Toilet Paper it would say:

Setting TP--Toilet Paper
Turning this option 'on' enables the user to use toilet paper. Toilet paper is paper used near a toilet (TP software version 6.7.1b or later)

[Geof]

.....I'm not really complaining since I'm sure other brands are similar but Haas could really do a much better job on their user and training documentation. They simply describe what settings do but don't give any examples of why you'd want to change them....

Never was a truer word spoken, or written. But I do have to be fair and admiot it is very, very difficult to write documentation. I have done it for our products and get about fifty-fifty criticism and compliment.

[Donkey Hotey]

The only reason that I'm critical of Haas is that they have the sales volume and the infrastructure to produce truly stellar manuals. It would help their marketing as well. I'm no dummy with this stuff but I still find it mildly challenging. I can't imagine what the average speed-shop guy does when he only 'barely gets' computers. I know the HFO is supposed to pick up at that point but what if you live an area with a bad HFO? Or a great rep who just isn't qualified to do end-user training?

I spent 7 years teaching CAD systems and eventually branched into Mac & PC basics, Word, Excel, PowerPoint and Project. Among all of them, few manuals were written very well. When I had the opportunity to write manuals, I tried to give the 'clinical' explanation, then give a real-world example of how to apply it.

I have the factory supplied manuals for my 9-day old TL-1. When reading, I'm never really sure which is the control documentation and which is the user training manual. I do know but so much of the training manual belongs in the control manual that I find myself swapping back and forth.

And the Intuitive Programming System is sorely lacking in documentation. Most of what I know about it, I learned from watching their sales video on the machine. If I didn't already know something about the control, I'd still be lost.

When setting tool offsets in the IPS mode, you 'Turret FWD' to select the next tool. At that point the register blinks at you but won't allow you to touch off the tool--it just continues blinking. I think I've figured out that I'm supposed to press Cycle Start to tell it I've loaded the tool (not Write/Enter or anything else). Cycle Start is NOT the intuitive thing to do when the tool is parked against the stock or the chuck face and nothing in the prompts tells me what to do.

It's a shame because even though I can do the raw programming, the IPS screens are really, really nice for basic facing and turning operations.

To get myself familiar with the machine and the IPS software, I made two threaded, knurled rings to replace the broken plastic switch retainers on my old lathe. They were my very first parts from the machine.

I had the first one off in about 30 minutes (including tool offset setup) and the second (going through all the motions again) took 15 minutes. All I can say is 'wow'. The threading was easier than I expected and I didn't open the manual once. I was impressed with the whole machine. The only glitches were when I changed the threading tool on the second part (causing the problem I had with work offsets) and the IPS version of the work offset screen (solved by doing it in the 'normal' offset screen).

I'm sure there is much more to the IPS that I'm missing and even Haas doesn't advertise all the changes in the latest version. The video on their website shows a very early version. It looks like the original version only used machine coordinates and lacked many of the on-screen prompts that the latest version has.

Anyway, thanks again for the help, guys. End of my diatribe.

[Wiseco]

Just to give my 2 cents, what's Haas is all about? CNC machines manufacturer or an educational company? They sell machines. People who bought CNC machines should have a CNC base. When you buy a car, do they show you how to drive them? No so I think Haas are there to sell machines but the thing is their machines are cheap so many poeple who doesn't know how to drive buy them and THAT'S a problem for their reputation I think when newbie people told Haas doesn't have support for learning.

Set your tools the right manner and the rest will be easy. One of the manner would be to set your tool as it would be with a probe. Touch off every tools at the same place on the machine. For me it's the frontmost jaw face offset with a 1/4 hss tool steel stock for the Z. When I use another chuck ( 4 independant jaws chuck) I set all my tools on another range of tool number. I mean if all my tools were set from 1-10 with my 3 jaw chuck, all my tools would be 21-30 for my 4 ind. jaws chuck.

[SeymourDumore]

Wiseco

With all due respect, I cannot for the life of me think of one good reason to pick your tools off to a chuck jaw. Mill is a different story, but lathe? Specially when Haas makes it a breeze to pick your tools without a toolsetter.
Not sure about current manuals with the TL-s, but all I've used for the SL-s was the manual and no training whatsoever. The SL was my very first CNC lathe and I've never even pushed the green button on one either before then.
The manual has a description of how tool offsets and work offsets are derived, and that apparently was enough to set my parts and tools up the very first day. Their settings and parameters are also relatively descriptive in the manual, specially when compared to a Fanuc manual. Not that it has more words, but rather they are in English, written by an english speaking technical guy. I sometimes get the feeling that all Japanese manuals are first written for an audience of science PHD-s, then given to seamstresses for translation into the appropriate language.

[Wiseco]

Seymour, it work very well for me. The thing is to touch off everytools at the same place for setting offsets and stock should not be involved in that. That was my point.

[Donkey Hotey]

I wasn't suggesting that Haas is in business to educate, however, they are responsible for telling you how their control works.

Example:
In my previous post, I mentioned how you have to tell the control to 'load a new tool' for offsets. I thought It was 'Turret Fwd' then 'Cycle Start'. It turned out I was wrong.

To change tool numbers while in IPS mode (for tool offset recording) you have to:

1. Press Turret Fwd
2. Press Next Tool
3. Press Cycle Start

The problem is that at this point the control simply says 'Running' and it's beeping incessantly at you. You have to press Cycle Start a second time to make it stop beeping and take the command (not documented anywhere that I've seen so far). Everything else in the control is 'Write/Enter' but this one wants 'Cycle Start' to change tool numbers on the display.

On the technical side, I understand why it works this way but that's no help to the new user and it doesn't make logical sense unless you already have experience with the Haas control (the very thing they were trying to avoid by coming up with the slick IPS screens).

The manual they supply for the TL-1 is actually the SL series manual so everything is written for the user who actually has a turrett. The Toolroom series user has to rely on the 'supplement' manual which--sadly--does not have that information in it.

Think about the things that Haas puts into the 'Control Tips' document. There is no reason that should be buried in there. It should be in the contents of a well documented manual for the machine or in a well documented Control manual:

"Here's a manual that describes the machine, here's a manual that describes some ways to use it and here's a 'tips' manual of things we forgot to put in the other two, here's a supplement for you beginners with a completely different machine who will be left on your own to figure it out."

As I wrote, I'm a happy customer but if they're marketing the Toolroom machines to people with no CNC experience, there is still a huge documentation gap to getting them up and running. By the time an inexperienced user knows enough about work and tool offsets and the basic control to get them running in IPS, they didn't need IPS to begin with.

I find IPS easy and friendly only because I've been through their three day class and because I already own a Haas mill. The IPS screens should have their own manuals: one for the lathe and one for the mill.

At this moment, I can't remember the keystrokes to reset the 'User Coordinates' to zero. I'd say that's a pretty basic (and useful) thing to know. I know I've seen it but I haven't got a clue where to find it in the documentation. That's what I'm talking about.

I'm not upset. I love my machines. I just think there is room for improvement in the docs. They are doing their own product a huge disservice by not thoroughly and logically documenting all of the great features built into their control.

[SeymourDumore]

Wiseco

Not sure if I'd trust the Z-location of the jaws remaining the same after remove and replace.
If it works though... then OK.

[Donkey Hotey]

I dunno' guys, this is my new plan for offsets:

1. Put a pin gauge or old endmill stem into the unused end of one the tool blocks. This will become the 'master tool' Z length for all future tool measurements.
2. Put an LED edge finder in the spindle whenever I need to touch off new tools.
3. Touch the 'master tool' to the edge finder and establish a G54 'Z' work offset.
4. Load and touch off any new tools to the edge finder (making it a pseudo presetter). If I'm careful to adjust the spindle runout, it could be used for rough diameter touch-offs too (though I prefer a sample cut).

As long as the 'master tool' never changes length, the presetter position will self-compensate by the work offset.

Thanks to all for clearing this up for me.

[SeymourDumore]

Donkey

Yup, that is a workeable idea, as long as you have a manual chuck.
With hydraulic chucks that need re-boring or jaw moving to accept the led indicator, it is not so great.
Not to mention of re-picking the Z after a toolbreak.

[Wiseco]

It will work if your carefull but you have 2 useless moves and one tool block enslaved(maybe not). As I said, if you touch off in Z all your tools on the same place (chuck face in example) it will do the job.

Everytime I set a new tool, I do it like the manner I said in a previous post for the Z and for the X I simply touch off the tool on the stock that I have, press X dia mesur, entered the dia of the stock and add 0.015 in the X wear offset (if it's an OD tool) to leave me something to compensate on the first turned of my new tool. And that' it! no need of an edge finder, or anything else, just something to touch off that is constant which is the chuck face or in my case one of the frontmost jaw face offset by a 1/4 hss toolstock. Useless to say that eveytime I do that, I have a stock clamp in my chuck since I need something to touch off anyway for the X tool offset.

Sure this manner will not be accurate as hell, but as you make the first part with your new tools set, you adjust them and that's all.

But hey, all roads lead to Rome!

Can someone who have done a CNC course give us what is teach in school for setting tools? Just curious.

[Geof]

....Sure this manner will not be accurate as hell, but as you make the first part with your new tools set, you adjust them and that's all.

But hey, all roads lead to Rome!.....

I am glad somebody else made the 'not as accurate as hell' comment. This is my approach; touch off on the end of the stock and get pretty darn close. If two tools have to be very accurately referenced to each other just adjust things to suit using either wear or tweak the offset.

Regarding using the chuck jaws or face I will make my standard comment; choose a location that is further out than your longest part. This means that the G54 will be a minus value.

If you choose a location shorter than the longest part the G54 has to be a plus value.

Both are equivalent; the tool goes to the correct place but there is a difference: If the value should be a plus and you accidently put in a minus the tool goes into the chuck. If the value should be a minus and you put in a plus the tool stays way back clear of the chuck.

I always try to have the situation where an error does not cause loud noises.

[big_mak]

Donkey,

Perhaps you have never read a Fanuc or Yaskawa manual. Try it, and you will see that the Haas manual is a godsend compared to these. I've read manuals from fanuc for 3000c to 18I and man they never realy improved over the years.

[Wiseco]

...
Both are equivalent; the tool goes to the correct place but there is a difference: If the value should be a plus and you accidently put in a minus the tool goes into the chuck. If the value should be a minus and you put in a plus the tool stays way back clear of the chuck.

As value you mean the work offset value I guess. I try to never entered a value there by hand, I try to allways use the Z Face measur button to avoid error. And if I would entered a value in minus, most of the time the controller will tell me that I'm out of Z travel range. But that's one good manner that I will consider.