Haas OL-1 Live Tooling

[Jorge-D-Fuentes]

Good morning, all.

The company I work purchased an additional Haas OL-1 Lathe with the optional Live Tooling, and they want to see it in action.

I'm trying to set it up to do some holes on the workpiece (on the C Axis), but the example on Pg 167 of the manual... I don't quite understand it.

The Example shows the following:

%
O00800
N1 T101 (Radial 1/4-20 Tap)
G99 (Necessary for this cycle)
G00 Z0.5
X2.5
Z-0.7
S500 (rpm should look like this, cw direction)**
M19PXX (Orient spindle at desired location)
M14 (lock spindle up)
G195 X1.7 F0.05 (thread down to X1.7)
G28 U0
G28 W0
M135 (Stop live tooling spindle)
M15 (unlock spindle brake)
M30
%

I can see this bit of code doing one hole... but I don't understand how this makes more than one hole (though it probably has something to do with that Reset Axis G28's hanging out right before the M135).

From what I can understand from this code, it's doing the following:

%
O00800
N1 T101 (picking tool, first line number)
G99 (setting the spin to RPM mode)
G00 Z0.5 (rapid horizontal)
X2.5 (rapid vertical)
Z-0.7 (rapid horizontal -left- from previous Z point)
S500 (setting the rotational spin speed)
M19PXX (M19 rotates spindle, PXX, where XX is a degree, orients the thing to a particular degree, so P90 rotates 1/4 around, P270 rotates 3/4 around, etc.)
M14 (Prevents the spindle from turning, I'm guessing while the drilling on the contour happens)
G195 X1.7 F0.05 (Live Tool drills into OD of 1.7 at a rate of 0.05... and back?)
G28 U0 (Resets incremental axis of X?)
G28 W0 (No idea, probably resets incremental axis of Z? The manual's parameters for this example only show the variables F R U X and Z)
M135 (turns drill off... although I didn't see a previous code that turned it on...)
M15 (unlocks the spindle brake, so I guess the thing can spin again)
M30 (Program ends... but I didn't see it loop back and do another hole...)
%

I was told by someone here that the OL-1 is one of a few lathes that has live tooling available, and the online help on drilling will be difficult since most of what I will find is for Milling machines.

I just want to have a canned cycle (if possible.. is there one?) that'll drill a number of holes I specify in the OD of a workpiece, by rotating, then drilling, then rotating, etc. I didn't think it would be difficult, but the example is tripping me up.

Am I forgetting something?

I'm sorry if anything above got posted before. I used the search function and couldn't find anything 'cept one thread that didn't really shed any more light on the subject.

[Geof]

It is not any consolation I suppose but that example makes no sense to me either. I am not near manuals at present but I will pull out what I have later.

[stefan2108]

O00800
N1 T101 (picking tool, first line number)
G99 (setting the spin to RPM mode)
G00 Z0.5 (rapid horizontal)
X2.5 (rapid vertical)
Z-0.7 (rapid horizontal -left- from previous Z point)
S500 (setting the rotational spin speed)
M19PXX (M19 rotates spindle, PXX, where XX is a degree, orients the thing to a particular degree, so P90 rotates 1/4 around, P270 rotates 3/4 around, etc.)
M14 (Prevents the spindle from turning, I'm guessing while the drilling on the contour happens)
G195 X1.7 F0.05 (Live Tool drills into OD of 1.7 at a rate of 0.05... and back?)
G28 U0 (Resets incremental axis of X?)
G28 W0 (No idea, probably resets incremental axis of Z? The manual's parameters for this example only show the variables F R U X and Z)
M135 (turns drill off... although I didn't see a previous code that turned it on...)
M15 (unlocks the spindle brake, so I guess the thing can spin again)
M30 (Program ends... but I didn't see it loop back and do another hole...)


The G28 U0 is machine home in x and G28W0 is machine home in Z
After your G195 cycle (in which you also need a reference point return (R) you need to unclamp the spindle with M15. Then rotate to your next position and clamp spindle again. then you run another G195 cycle.

Stefan 2108

[Jorge-D-Fuentes]

Ahhh, I think I see.
Another thing that was tripping me up is that they put two asterisks in the example after S500 (I guess to add emphasis, or for some footnote somewhere... which I didn't find), as well as adding a note on top of the page to the parameters of G195:

G195 Live Tool Radial Tapping (Diameter) Group 00)
F Feed Rate in inches(mm) per minute
R Position of the R plane (this part here I didn't understand)
*U X-Axis incremental distance
*X X-axis motion command
*Z Position of bottom of hole (or this part, I thought Z was a horizontal movement placement)

Afterwards it has the same thing but for G196 (Reverse Live Tool VECTOR Tapping (Diameter) (Group 00))

Then it has a little note (but no asterisk for it) saying "These G Codes perform live tooling radial or vector tapping on a lathe; they do not permit an "R" plane.

This trips me up further since the latest reply mentions this "Reference Point Return (R)". So is the manual wrong and they do need an R plane? Or do they mean that only the asterisked Parameters do not need one?

Anyway, at least I now know that if I want four holes, I'm gonna have to write four snippits of code with the same info, and eight if I need 8, and 16 if I need 16... I was hoping that, like a canned cycle, one could program it to perform a DOWHILE or something... which I suppose can be done with a little programming knowhow... *sigh*

EDIT (Update): Ran the example using MDI... with some changes to the X's and the Z's.

The spindle does lock, but after it locks, it doesn't want to rotate the 90 degrees that I asked it for. It looks like it wants to move but the brake is stopping it.

I wrote the following (in MDI, sans the % sign):
%
G99
T101
G00 Z0.5
X1.000
S500
M19 P90
M14
G195 X0.75 F0.05
M15
S500
M19 P180
M14
G195 X0.75 F0.05
G28 U0
G28 W0
M15
M30
%

I'm pretending that my T101 is my live tooling tool, but in reality it's not, it's just another tool, but for the purposes of testing (and the fact that they've not purchased drillbits for the livespindle) it works.

Okay, the spindle does lock up, but won't turn the 90 degrees I want when I call for the M19. It looks like it wants to start up, but the brake clamping stops it. This happens again when I call for it to rotate 180. The G195 does happen twice like I ask it too.

Maybe we don't have a spindle/chuck capable of it? I don't think my superiors would do that... Weird.

[stefan2108]

you need to add a dwell G4 P(value) in order to give the brake time to open before rotation

[Jorge-D-Fuentes]

Thanks for the tip, that helped out a bit. I'm very grateful for all your responses, guys.

I got the M19 to 'somewhat' do what I wanted, but as it turns out, it wasn't necessary, because...

...I was on the phone with Haas for a while yesterday afternoon, and they have a feature on the OL-1 whereby the C Axis works on it if it's engaged. After jumping through a few hoops or so, it turns out that there is an

M154

that turns the spindle into a C-Axis drive, allowing me to command the rotational axis using C coordinates, such as

C45.

for 45 degrees from the origin.

This feature is cleverly hidden so that there's nearly no clues to its usage in the manual in the example for the Radial Live Tooling example (instead, that example uses the M19 PXX code, which... seems to be a pain to use given the circumstances).

The C-Axis is an optional feature on the Haas, and thus, there seems to be nothing even mentioning C coordinates at all in the (generic) manual, from what the guy on the phone said (he said it in nicer terms though). It's one of those 'hidden' things that you'd only know about by actually calling Haas and asking.

The only clue I had at first was the G/M-Code sheet that's laminated and placed inside the drawer for the OL-1. That's the only thing that mentions "C Axis Engage". The book has one tiny blurb (found after spotting that) at the very end of the "G Codes & M Codes" section, that says:

M154 C-Axis Engage/M155 C-Axis Disengage (optional)
This M Code is used to engage or disengage the optional C-Axis motor

all the way at the very end in pg175.

That's when I decided to call 'em. This was late yesterday though.

I guess if the C-Axis wasn't there, one would use the M19...?

ANYway, here's the new code that does what I want:

G99; (RPM Mode)
T101; (Tool Change)
G00 Z0.5; (Rapid)
X1.0; (Rapid);
;
M154; (C Axis engage)
C45.; (rotate 45 degrees. Note the period)
M14; (lock spindle)
G04 P4.; (4-second dwell as recommended. Spindle appears to vibrate a bit from the braking for about...oh... 2 seconds or so)
G195 X0.75 F0.01; (drilling cycle)
M15; (unlock spindle)
G04 P1.; (1-second dwell as recommended)
; (repeat previous seven blocks as below, changing the degree)
M154; (C Axis engage)
C90.; (rotate 90 degrees this time)
M14; (lock spindle)
G04 P4.; (4-second dwell)
G195 X0.75 F0.01; (drilling cycle)
M15; (unlock spindle)
G04 P1.; (1-second dwell as recommended)
;
(repeat the seven blocks ad nauseam, the only change is the degree)
;
M155; (C-Axis disengage)
G28 U0; (Home X)
G28 W0; (Home Z)
M30; (Program End & Rewind)

One thing of note is, I'm not all that fond of the C-Axis's rotational speed as it goes from one degree to the other. It's very very fast! :O Adding S values to the M codes doesn't change anything, it still servoes to 45, 90, etc. degrees very very fast! I've got to look for a parameter or a setting in the machine to slow it down. As an experiment, I decided to go all the way to 270 degrees from zero, and the thing gave me a nasty sound when it reached its destination.

I didn't like that at all. I'd like to slow down the spindle C-Axis.

I also don't like that you have to keep re-enabling the C-Axis. Every time you do that, it resets back to C Origin before turning to the angle needed (and at 'ludicrous speed', too). Tried running without the M154 (just putting it on top) and as soon as the drilling was done and I needed to turn again it gave me a "C axis not engaged" alarm. :\

[stefan2108]

we´ve also been able to decipher our manual with direct help from HAAS.
It seems that when using a flatening cycle the slowest spindle rpm is 3. this can only be achieved by specifying the S value directly on the flat cycle block otherwise it will default value of 6.For example G77J0.625I0R0.25K2S3.
greetings from germany

[Jorge-D-Fuentes]

That was a good idea to try out.
Unfortunately, it did not work for me, it still turns at a speed too fast for its own good.

If I wanted 8 holes on this, by the time you get to hole 5 it starts making that sound. I suppose I could tell it to rotate in the other direction, but that's not a 'true' solution. :\

Sounds like if I didn't hit the clutch while changing gears. I'd like to avoid that noise, as it sounds like stuff could be getting messed up in that spindle.

[theemudracer]

I belive the G99 is Feed per revolution. G98 is Feed per inch.

I think there is alot of simularities between Haas and Fanuc.

[stefan2108]

what if you add a g01 & a F command to your c (angle) command
G01 C90. F.05
?

[Jorge-D-Fuentes]

Ooh, interesting thought.
I'll try out using a G01 sometime later.

PS- Yeah I wrote the wrong description. Sorry 'bout that. ^^;;
Manual calls for G99 though.

[Jorge-D-Fuentes]

Update:

Adding an F to the G01 C the control spits out the error "Spindle not turning".

It seems you cannot make a C movement without locking out/resetting the X/Z movement/viceversa. It's very weird.

Basically, if I make a movement in the X/Z axis, I have to reset the C axis. Or at least, it seems that way.

EDIT- Sorry, I didn't realize I was the last post. I should've used "Edit", not "Reply". X_x Apologies.