HAAS lathe newbie with a problem

Hi,
So I received a HAAS SL10, manufactured in '08, I got it preped and powered up. This is the first time working on a Haas, I have worked on a takisawa with fanuc controller a long time ago. And I'm having a really hard time understanding whats going on with the work offset.

I followed the manual to set up a tool, tool 2. And measured x, measured z, and set z face measure on the work offset page under G54. So far so good, the tool offsets are calculated correctly. But the position panel is showing the same x and z for operator, work g54 and machine coordinates which are based on machine zero.That is the top right corner where the turret goes after power on restart.
If I change the tool all coordinates system stay the same, although the next tool has other offsets.

So my question is what do I have to do to update the g54 (or the current work offset, which happens to be G54) based on the measured tool offsets?
If anyone can help I would be indebted!
<a href="https://imgur.com/C7KkUVk"><img src="https://i.imgur.com/C7KkUVk.jpg" title="source: imgur.com" /></a>
<a href="https://imgur.com/qoDdKiq"><img src="https://i.imgur.com/qoDdKiq.jpg" title="source: imgur.com" /></a>

The machine position is simply that, where your turret is parked in relation to machine zero. When you home it out it should read 0,0.

The G54 display will read how far away you are from G54 zero. Since you have no values in G54, it will always follow the machine position.

The operator position is simply a "scratchpad" if you will. Jog your turret some where. Look at operator position.
Push MEM then go back to manual. The operator position should be 0,0

When you change tools, you are only rotating the turret, not activating anything.

Booze Daily said:

The G54 display will read how far away you are from G54 zero. Since you have no values in G54, it will always follow the machine position.

Click to expand...

ok, thank you for the reply. I understood what you wrote except the part about G54. I don’t understand why are there no values , I measured z face while on the work offset. And it did not change. And for x work offset that I really don’t understand what updates it. I thought measuring the tool would.
I am not at the machine right now. I have to try again tommorow.

There are no values because you didn't put any values in.

Typically G54 X value would be distance from machine zero to centerline of your spindle. Z value would be distance from machine zero to the face of your stock.

Done this way, all tool offsets will be relative to the centerline of the spindle and the face of the part.

What your have done is lump all that in to just the tool offset. That will work, but I don't think its a very logical way to do it.
Also, you will quickly notice that all your centerdrills, drills, taps are all going to be the same tool offset for X, namely, the distance from machine zero to center of the spindle.

Using your screenshot, if you were to set G54 X-300 Z-200, your tool offsets would be X61.918 Z18.586

You have to put a value for part face using a face or other tool.Then z face measure ever tool from that one.
I use G154 as a common.


Sent from my iPhone using Tapatalk

Boy am I glad I never had one of these easy-to-use controls.

G92 is killer.

Remember to put your G54 value in "Z" not "X" as per your picture.

Also you should be using "Tool Tip" numbers 0-4 for proper tool radius comp.
Your pick says all zeros

I figured out something. I re-did the whole measure tools and z face measure on g54 on the work offset. And put a program in MDI with a safety line, and then command T0101 which may be redundant and then a move to zero, which was set to the part face. And it did go there exactly, on centerline and just kissing the stock front. Where G54 should be. Right, now as the program ran and the tool moved the position screen showed the G54 coordinates, compensated and referenced to that point again on centerline and touching the face on z. But as the movement executes and the turret halts it goes back to that wonky way of indicating position, which is a combination of x as a position from machine home, and that z which I think is machine z minus an offset but I don't know.

Still, does HAAS work like this? Do you only get to see the tool position in G54 only while running a program. I mean, if anyone here worked on a Fanuc control you would see this as very odd.
So I tried the same with the next tool and exactly the same. I hope I'm conveying what I'm trying to do and someone points out how and what am I doing wrong. I know I probably am.


g54 weird - Album on Imgur

long story short. When Haas made their first lathe they used there mill control and all of the mill features. some people like it, some don't. you can set all of tour tools and not use g54. but most controls have what would be considered a g92 or g52 or face offset and call it whatever. my KIA KT 21 has this on a yasnac lx3 control. I'll have to turn it on and see what they call it. but anyway it's all on how you wag the dog as they say !

Holy Shit!!!

Let's just start with the basics.

Since you're new on a Haas lathe and want to figure out how the offsets work ( fanuc too but I digress for now ), lets start out by clearing
all offsets. That is Tool offsets and Work offsets. Instructions how-to is on the screen. Just make sure that all tool and workoffsets are in fact zero.

For now also, lets assume that there is no toolsetter, so in the Settings page set the 64: "T Offset Measur Uses Work" to On.

Then:
1: Put a piece of stock into the chuck, clamp it.

2: Index to a tool, let's say Tool1,( turret FWD, REV is OK to use ), jog down to the part and make a face cut.
Without moving the Z axis, go to the Tool offset page, navigate to the Z offset of tool 1 and hit the "Z Face Measur" button on the panel.
This will enter a large negative value into the offset register. If you pay attention, then you realize that this value is equal to the machine ( G53 ) coordinate.
Basically, the machine knows that for tool 1 it has to travel to this distance from home to reach the part face.

3: Now with the same tool, make a clear cut on the OD. Without moving the X axis, measure the resulting diameter.
Then hit the "X Dia Mesur" button, and enter the measured value at the prompt. The resulting value will again be a large negative number in the register, though
it isn't a direct equal correlation to the machine coordinates, rather a calculated value from an internal number ( set by Haas at the factory for X0 ) and the measured diameter.

Now, you're done with Tool 1, so move onto Tool 2.

4: Jog to the face of the part you've cut with tool 1. Use a very thin shim or feeler gage or just by a real good eye, and touch the tool to the face.
On the Offset page for Tool2 - Z hit the "Z Face Mesur" button. Again machine Z coordinate will be entered.

5: Jog in X, touch the clean OD you've cut with the previous tool, and now hit the "X Dia Mesur" button. The prompt will show you the previously measured and entered number
so you can just hit Enter.
Alternatively, you can make a new clean cut with this tool, measure it and do the same button sequence but enter the newly measured value.

Do all this for all other tools.
Done, your tools are now all set up.

So, to now go to machining your part, you can install the new jaws and put in the part.
Take a tool ( ANY TOOL!!! ) that you've just picked up, jog to the face of your part, make a clean cut.
Without moving in Z, go to the G54 Z offset register and hit " Z Face Mesur"
The register will now have a much smaller number, may be negative, may be positive.
This number is very very simply the signed distance between the current machine coordinate and the Tool Z offset value. Nothing more, nothing less.

Tool Z offset = arbitary ( once fixed ) point in Z measured from machine home.
Work Z offset = distance from arbitary ( once fixed ) point and new part Z zero.
Programmed Z position = Tool Z offset + G54 Z offset + Programmed Z position.
If you graph it out on a piece of paper you can easily figure out how it works.

Try this first, try to wrap your head around it and feel free to come back with more questions.

Now to some of the posters...

No, there is no G92 on a Haas lathe. Well, there is but it's a freakin' thread cutting cycle.

Yes, the control appears to be a mill control at first glance, but other than the color and the screen that's where the similarities end.
The software inside has nothing to do with mills, not unlike how Fanuc works BTW.
In fact I'd say the Haas lathe control may be more Fanuc like than some real Fanuc controls and iterations.

On a Haas, indexing the turret into position also activates the correct Tool offset and tool wear offset.

G54 X value should always be 0 ( in virtually all but very very special cases ).
The spindle center line never changes, so the workoffset X is always 0 ( again, special exceptions exists )
IOW you ARE NOT telling the machine where it's spindle center line is, the machine already knows where it is.
What you ARE telling the machine is how long to travel to put the respective tool's tip there.

And, before someone attempts to bring up some idiocy about a "Master Tool" or "Boss Tool" or "Setup Tool" , please, just Don't!
There ain't no such thing!
Any tool in the turret which has been properly picked up previously is a proper and appropriate tool to use for successive new setups and programs.

TudorLuca said:

But as the movement executes and the turret halts it goes back to that wonky way of indicating position, which is a combination of x as a position from machine home, and that z which I think is machine z minus an offset but I don't know.

Still, does HAAS work like this? Do you only get to see the tool position in G54 only while running a program. I mean, if anyone here worked on a Fanuc control you would see this as very odd.


g54 weird - Album on Imgur

Click to expand...

Unfortunately, yes, Haas does work that way.
Truly stupid if you ask me because deep down it knows EXACTLY where in the currently active work coordinate system it is, but
for some unexplainable reason Haas refuses to change.
One of their representative has explicitly said so on this forum in the past, that they have considered it and then decided not to implement it.

KenFoulks said:

I agree as an operator and machinist that having this feature would be nice. Yes, some manufacturers have done it. We may or may not introduce this feature in the future. I disagree with your claim that we overlooked this feature, we looked at it and decided against it every time. As far as simple, keeping some commands active outside a program does not sound like something we are going to introduce.

Click to expand...

You can prove this on your own by putting an M00 at the end of that MDI program.
The control will travel to the X0 Y0 coordinates and then stops for the M00.
In this case the G54 will still show the correct X0 Y0.
Hit the green again, program rewinds and it'll revert to the G53 coords.
Why?
Fucked if I know!

SeymourDumore said:

No, there is no G92 on a Haas lathe. Well, there is but it's a freakin' thread cutting cycle.

Click to expand...

That's nasty !

Nice explanation, thank you. Made me glad I don't own one

EmanuelGoldstein said:

That's nasty !

Nice explanation, thank you. Made me glad I don't own one

Click to expand...

Writing off the whole machine because no G92 huh?

Don't know about the UK, but I would say 75% of modern (take that for what you will) machines in the US are using G54-G55 and so on for coordinates. Along with G53 for machine coords, and G52 for global offsets (as examples). I think using G92 is *dubious*, unless your machine does not support G54, but I would say those are getting fewer and fewer...

Mike1974 said:

Writing off the whole machine because no G92 huh?

Click to expand...

Well, that and the non-standard use of G92 would turn me off, yes. As a veteran of the browser wars, I hate to see standards tromped on.

I would say 75% of modern (take that for what you will) machines in the US are using G54-G55 and so on for coordinates. Along with G53 for machine coords, and G52 for global offsets (as examples).

Click to expand...

That's because you don't have any real controls left, just that upside-down and backwards Jap stuff .... and you think it's normal

I think using G92 is *dubious*, unless your machine does not support G54, but I would say those are getting fewer and fewer...

Click to expand...

Yup, the good stuff is dying out, replaced by feeble junk

Not to beat on Haas especially but I could not find a lathe to buy these days ... maybe that's good, instead of liking your machines you just buy the cheapest one you can get and aim your nose at making money.

On a midsize lathe, I don't care for linear ways and zoop-zoop light cuts. Box ways and lotsa beef. If we're dreaming, I'd take a Cincy 10cc or 10cu with the swingup, and a Producer or GA or (since they are still alive) Dynapath. (Put the whole thing on an fpga tho, cuz hardware breakdowns were no fun.) And resolvers and a full control panel with heavy-duty Sylvania buttons, and switches ! And Square D electrics, with the wiring all done in a neat geometric layout.

Oh well. Good thing I don't gotta run this "modern" stuff after all

p.s. G92 kicks ass over these silly Jap methods. Yes I know Haas is not Jap but it may as well be. OP would not be having this confusion with a sensible control.

Compare this to Seymour's description:

All your tools are qualified. You do that when you get them, they are a set length in X and you can measure the Z offset on a surface plate and engrave it on the toolholder. There's your basic tool offsets.

Put the tools in the turret and transfer over the Z offsets. X is already qualified to 0.

Bore your jaws. Run the turret up close and use a 1-2-3 block and a piece of paper or whatever to set the face of the turret 3, 2, or 1 inches away from the locating feature in the jaws with your differential resolver.

That's your Z 0. (Actually 3, you have to subtract the thickness of the 1-2-3 block. You could use the turret face instead but that is hard on the hand.)

Look at the program, where's the start point ? Subtract the 3" of the 1-2-3 block and go that far. Home X. That's your G92 program start point.

Done. Pretty simple and fast. But it depends on a part being drawn in positive numbers, from the left hand end. Oh, like the blueprint !