[Donkey Hotey]

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.

Geof, that there is the gem of this whole thread for a nOOb like me.

[speeeeed]

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:

Hi
We just got the TL4 and I must say reading this forum has been very helpfull. Haas is lacking in the information department on this lathe and how it is controlled as with the other TL they did not go through the trouble to give it its own Manual. This Forum is a great help.
P.S. Man this thing is big
Speeeeeeeeeeeeeeeeeed(nuts)

[PBMW]

I'm not quite sure what the hubub is about offsetting tools. I have an SL10 with a probe and I have a Daewoo with a probe. When I first got the Haas, I had never owned a machine with a tool probe so I didn't use it. It was "Spensive" and I didn't want to bust it. So I just offset the thing like I've offset every lathe I've ever owned. Touch every tool to the face and call that Z zero. Done. When every tool is set to a given location, the relationship is set. When you change an insert, tweek it back in. This is the same as setting up a mill. Now that I've gotten braver...I use the probe.

[Edster]

At this moment, I can't remember the keystrokes to reset the 'User Coordinates' to zero.

use page up and down to select the user coordinates then press x or z then press origin

you probably already know this, the tl lathes are laid out like a manual lathe but the programming is the same as a slant bed with the tool upside down.

Hope it helps.

[Donkey Hotey]

use page up and down to select the user coordinates then press x or z then press origin

Thank you, but you forgot one step (I've since discovered how this works): you have to be in Hand Jog mode with the coordinates blinking before it will let you 'origin' the values. That was the step I was missing.

[Greg Benedict]

I know I'm getting into this thread kind of late, but I have just not been able to figure out offsetting on our TL-2.
I have zero CNC lathe experience. Just wanted to get that out first. But reading the manual I find I just cannot figure it out.
Offsets on the CNC mills at work I get. But when I try to go step by step through the lathe manual, no joy.
When my work bought this machine, it included training for two people, but our workload was such that I never got a chance to go. The guy that did get to the training classes is basically a SOB who won't share what he knows.
I talked to the local HFO and the online training would end up costing me nearly $800. It's unlikely I could get my company to pay for this, and complaints to the shop manager do nothing.
I guess I'm asking if anyone has taken the time to explain exactly how to use a TL-2? I'm really mostly interested in using the IPS features, but the manual says you have to set all your offsets BEFORE you can make parts with IPS. So I am basically back to where I started in the first place.
To me, at least,(and maybe I'm just a dummy) the Haas manuals are not clear enough to figure out. And they should be, considering that the machine is being marketed as a stepping stone between manual turning and CNC.

[Geof]

Here is my approach to set all the tool offsets to the end of the stock.

I do not have any values in G54.

In Handle jog with the Offsets page on tool length offsets take a skim cut off the end of the stock and without moving Z press Z Face Mesur; this enters the Z offset for that tool.

Now take a skim cut off the OD and measure the diameter, it doesn't matter what size it is you just need to know the size, and without moving X press X dia mesur; the screen will flash a little sign that says ENTER DIAM in the lower left corner. Make sure there is no number there by using Cancel if needed, and enter the diameter your measured and press Write.

You can repeat this for all the tools, with boring bars you need to run a drill in first so you can bore an ID to get the diam.

Instead of taking skim cuts with all the tools sometimes I draw with a felt pen on the surface produced with the first tool and then bring the other tools in very slowly using the 0.0001 setting in Handle jog until I machine off the felt pen ink.

There are other approaches that do make use of G54 and a reference bar and if you want to go into that later we can, but for now see if you can get sorted out with this simple approach.

[Greg Benedict]

Thanks, I'll try that on Monday. Do I need to clear all the existing offsets first?
Thanks, Greg B.

[Geof]

Thanks, I'll try that on Monday. Do I need to clear all the existing offsets first?
Thanks, Greg B.

Actually the procedure I describe will overwrite them but it is best to clear them so you don't get confused about which have been done and which have not. Press ORIGIN and Y to clear them all.

[Wiseco]

If you do some test on the machine, don't forget to write a note so other operator will know that offsets can be wrong as what Geof said don't take a work offset in consideration.

In a basic ways, tool offsets let the CPU knows where the tool nose is. So if you set all Z tool offset at the same place in example, the face of a chuck jaws, then all tools will have a same location in Z. After that, the work offset let the CPU knows where the work ZERO is for the Z for all the tools.

Don't forget the CPU is completely blind and stupid so we must tell him everything so he can do his work.

[Greg Benedict]

Thanks, Geof, Wiseco,
Those tips have got me started in the right direction. I was able to set offsets for one tool and play around with the IPS for a little while after work today.
I really appreciate the advise. I'm sure I'll have other questions soon and I hope nobody get too fed up with me.
Thanks, Greg B.

[Ringcn]

I run a Haas-TL2 and here is my SECRET to how I set my tool offsets...I set all the z offsets for all my tools using the face of the chuck. I take the tool and gently touch the face of the chuck and hit the z face measurement button while in the offsets page highlighting the correct tool number for each tool...This makes all my offsets come off the stationary chuck, so that way they never change unless of course you change the chuck or move the tool...I then set the z offset for the G54 work coordinate or whatever coordinate I'm using in my program to the distance from the face of the part to the face of the chuck. This pulls all my offsets from the face of the chuck to the face of the part. Now how do I do that? This part is kind of funky but it works if you do it right. Let's say I've touched all my tools off and have my z offsets coming off the chuck and all my x offsets are set...since I'm going to be using G54 for my program I must switch to a different active work coordinate that has 0. Values for both x and z, I use G55...to do this go to MDI clear the page if any code is there, type G55, press enter, press cycle start,you should now be in G55. Ok now you must make sure your current active tool is the same as the tool you have in the tool post. Let's say we have T6 in the tool post. Switch to Tool 6 by pressing edit, hand jog, cancel until you get to the screen with the big red words lol.. Then type T6 press turret fwd, cycle start to install T6. you should now have T6 as your current tool. now you take your tool and touch off the face of the part. Go to the offsets page and press z face measurement while highlighted over the G54 work coordinate offset. This should now be the distance between the face of your part and the face of the chuck. Double check by measuring the distance using calipers or depth mics or whatever. I guess you could even use the DRO and subtract the machine positions of the chuck and the part to get the distance. If you do not have the correct tool selected or your not using a different work coordinate that has zero values while touching off on the face of the part, you will get an incorrect offset and you can potentially eff up.. Maybe it's a little confusing at first but it's nice once you get it down. I've never tried changing the setting 64, although I'm highly interested and now am going to check it out. This is the way I figured out how to do it and it's probably not the best way but I love it.