Hey Guys,

I have a SL-10 question. I have been running a Hardinge with Fanuc controls for about 2.5 years now and we just purchased a Haas SL-10 Lathe. On the fanuc controls i use a subroutine program for a safe index point for each tool change. Here is what the code looks like...

O0001
G0G40G97G98G80
T0
X#501Z#502
M99

Pretty simple, at the begining of the program the i'm running i put in these values

#501 = 6.0
#502 = 6.0

M98P1


This makes the turrent go to that location before making a tool change. I can't get my haas to work with this programming. I'm sure that I'm doing some thing wrong. Any help would be greatly appriciated.

Thanks
Josh

This might seem like a dumb question: are you sure your control has the Macro option?

looks pretty good , what type of alarm do you get ?

Peter

Pretty sure. But then again i didn't actualy purchase the machine. What setting or parameter would it be??

looks pretty good , what type of alarm do you get ?

Peter

It does not know what the x#501 and the z#502 is

Says bad code

for 99% you dont have the macros ;-) go to parameters , one of the first pages and find that line with " macro " and see if there is an zero or one .

Peter

Ok I check and no Marco are not enabled. I will have to call Hass tomorrow morning and find out how much to turn it on. Next question....Here is the program that I am currently running. I keep getting a z axis over travel when the program is completely done and i hit cycle start for the begining of the next program.....

O01122
(--------------------------------)
(N1 - 80 DEG TURNING TOOL)
(N2 - CENTER DRILL)
(N3 - 12.0mm DRILL)
(--------------------------------)
G54 G00 X6. Z8.


N1
G54 G00 X6. Z8.
T101
S1200 M03
G00 X1.3 Z0.
G50 S2500
G96 S500 / M08
G99
G01 X-0.05 F0.006
G00 Z0.001
X1.
G01 X1.252 K-0.05
Z-0.25
G00 X1.4
G00 X6. Z8.

N2
G54 G00 X6. Z8.
T1010
G97 S1200 M03
G00 X0. Z0.2 M08
G99
G01 Z-0.3 F0.0015
G00 Z0.2
G00 X6. Z8.

N3
G54 G00 X6. Z8.
T707
G97 S750 M03
G00 X0. Z0.2 M08
G99
G83 Z-2.6 Q0.1 R0.2 F0.003
G80 G00 Z0.2
G54 G00 X6. Z2.5


M30

sorry, I can not simulate that ( I have metrics ) - but you have the place to move into Z8 ?

I had a very similar problem , but I uses W... , same effect after running the whole simulation the next run was Z overtravel , for me worked to change the W into G0 Z... but I don`t see W in your code, maybe it is an another haas bug in software.

Peter

Ok I check and no Marco are not enabled. I will have to call Hass tomorrow morning and find out how much to turn it on.

Right off their website:

Create subroutines for custom canned cycles, probing routines, operator prompting, math equations or functions, and family-of-parts machining with variables. MACRO $2,295.00

Josh,

I don't use this command myself, but our Haas Rep. suggested it to us. It is a G53 command. Way I remember it working is, you select a safe point that all tools will clear when indexing, and designate that as your G53, then in your programming you command a G53 before you do a tool index. Like I say, I've never put this to use , so get the first hand from the Machine Manual for the full procedure.

regards
Paul

Actually, that's a very good suggestion. I also use G53 for all of my toolchange locations. It's in machine coordinates and it's non-modal (meaning: it goes right back to the current work offset after you use it).

G53 G00 X-2. Z-5.

Don't forget to go back to G01 after using the rapid.

The rapids on the SL10 are so fast and the machine is so small you might just as well send it home for a tool change; G53 G00 Z0.0

I would take care using Greg's example because Z-13.0 puts you awful darn close to the chuck on the SL10.:)

Thanks for checking, Geof. I just changed it. :D

I actually just copied it out of one of my programs. I didn't remember where I parked it for toolchange. That's on my TL-1 so it was well clear of the part at that position.

The actual coordinates will vary for each part and setup. YMMV. :)

You can safely, and very very slowly, use my G53 G00 Z0.0 on a TL machine; plenty of time to brew a cup of coffee during a tool change.:)

Thanks for the input. I used the G53 G00 Z0 and it work just like I was wanting. We are a 100-2500 job shop and I am always going from machine to machine writing programs and don't always get to set them up. So i always like to make sure that everything is as clear as possible for turret tool changes.

One more question then I will leave you guys alone.

How do you all setup your machine for quickly setting your Z face to the part. I always program on the lathe with the face of the part @ Z0.000. A lot of the time I can leave the same tools in the machine and use over a long time with different parts but currently I am going in and resetting the the Z Face Value each time. Is there a better way??? Just curious.

Thanks
Josh

Where you set the Z is not that important. The most important thing is to establish a method of setting the Z and then being consistant from part to part and even machine to machine. Your operators don't like surprises.

I have re-calibrated my tool-probe , and my zero is on the front of the collet, I measure the tools like always , and to determine the part Z face I take a caliper and measure the length between collet and end of the part and that number I put into the Z offset screen ( for the jobs that don`t require more accuracy ) - is that what you`re asking ?

.....How do you all setup your machine for quickly setting your Z face to the part. I always program on the lathe with the face of the part @ Z0.000. A lot of the time I can leave the same tools in the machine and use over a long time with different parts but currently I am going in and resetting the the Z Face Value each time. Is there a better way??? Just curious.

Thanks
Josh

You can set all your tools to a constant reference point and then change the work zero to move all of them to suit different parts. This is what you can do with a tool probe but you can also do it without a probe.

One way is to have a reference bar that clamps in the chuck and set all your tools to the end of that. Have the bar longer than the longest part you ever machine then you put a Z- value in G54 that is the distance from the end of the reference bar to the Z0.0 point on the part.

Some people use the face of the chuck as the reference point and really the only reason I do not is because then the Z values have to be plus (+). This introduces the possibility of error because if you make a mistake and enter a minus (-) value you go into the chuck not away; my way if you accidentally enter a plus (+) value you move away.

As JWK42 says the exact method is maybe not as important as consistency.

Geof,

Thanks for the input. Setting a zero reference point is what i want to do, but i want to set the tools off the face of the turret and then move the z plane to reference to the turret face?? Don't know if that makes sense or not. That's just how the guys at my shop understand setting the lathes up and want me to keep it that way... :) old dogs might have to learn new tricks.....

I wrote out a program today to turn a shaft and under cut behind the thread using the G71 / G70. Keep getting a alarm. Here is the code that keeps giving me a problem. Thanks in advance for all the help....


N1
G53 G00 X0 Z0
T101
S1200 M03
G00 X1.3 Z0.
G50 S3500
G96 S250 / M08
G99
G01 X-0.05 F0.006
G00 Z0.1
X1.3
G71 P100 Q200 U0.04 W0.005 D0.05 F0.008
N100 G00 X0.45
G01 Z0.001
X0.510 R-0.03
Z-0.375 K0.05
X0.62
Z-1.25
X0.506 A210.
Z-1.575 R0.05
X0.629
Z-1.980
X0.866 R-0.03
Z-2.175
X1.180 K-0.04
N200 Z-2.625
G53 G00 X0 Z0

N2
G53 G00 X0 Z0
T202
G97 S1200 M03
G00 X1.3 Z0.1
G50 S3500
G96 S300 / M08
G99
G70 P100 Q200 F0.004
G00 X1.3
Z-1.980
G01 X0.609 F0.003
G00 X1.3
Z-2.175
G01 X0.846
G00 X1.3
G53 G00 X0 Z0


Josh @ ptpmfg.com

Josh,

Are you getting an alarm that refers to non monotonic (sp?) or type 1 or type 2 G71 cycles?
If that is the case, add a Z move in your first N100 block.
When I write can cycles, I will use Z0.1 as my Z initial point. Then add Z0.05 to the first line of the N100 block.
I say this in reference to a 05/07 control. Can not speak with certainty of any control older than that.
Do know that on other machines w/ Fanuc controls we used to add a W0 (that is a number zero there) to same said block, and that would allow them to perform an undercut in the G71 cycle. Without the W0 they would cut the entire path in 1 pass.
As with any programming advise. Run it in the air first, to proof it.

Paul

I think paul has it; you need X and Z moves in your N100 line to start Type 2 roughing so you can reverse direction in the P Q block.


Setting your tools with reference to the turret face makes sense but I don't know an easy way to do it.

Paul & Geof,

After downloading the training class off of haas portal tonight I think you might be right. I'm gonna try that tomorrow morning. Haas just has a few little quirks that I'm not used to. Thanks for the help and quick reply.

Josh

Ok Guys,

It worked perfectly after adding a Z0.05 in the PXXX block. But when it performed the rough cut on the back cut angle and the finish cut it left me with two different steps??? Here is the program that I used to cut both rough and finish. Also I attached a picture of the part.

N1
G53 G00 X0 Z0
T202
S1200 M03
G00 X1.3 Z0.
G50 S3500
G96 S250 / M08
G99
G01 X-0.05 F0.006
G00 Z0.2
X1.3
G71 P100 Q200 U0.04 W0.005 D0.04 F0.008
N100 G00 X0.45 Z0.01
G01 Z0.001
X0.51 R-0.03
Z-0.375
X0.62 K-0.05
Z-1.25
X0.506 A210.
Z-1.575 R0.05
X0.629 R0.015
Z-1.98
X0.866 R-0.03
Z-2.175
X1.18 K-0.04
Z-2.625
N200 X1.3
G53 G00 X0 Z0

N2
G53 G00 X0 Z0
T202
G97 S1200 M03
G00 X1.3 Z0.2
G50 S3500
G96 S300 / M08
G99
G70 P100 Q200 F0.004
G00 X1.3
Z-1.98
G01 X0.609 F0.003
G00 X1.3
Z-2.175
G01 X0.846
G00 X1.3
G53 G00 X0 Z0


Thanks

Josh

Simple things first, same profile tool, tool offsets correct?

Also you should take out the W0.005, when you are doing an undercut which means the back edge of the tool is cutting, the W value means it can take too much off the back during roughing, and your U is larger than necessary I think.

Geof,

Took out the W0.005 and cut another part. Still did it?? Any other suggestions. I am using the same 55 Deg tool for the roughing and finishing.

Josh

Are you in a panic for this?

The reason I ask is that I can run it through my Simulator or even on my TL2 but not for a few hours. First order of the day is mixing a bunch of concrete for a statue base I am making. And if I am still capable of moving after that...then I can fire up the machines.

Well, I am tring to get it setup today for a little bit of a production run. I have contacted my Haas HFO and they are working on it also for me. In the mean time I have changed the program and using my cam software to cut it. Just was wondering what I was doing wrong. Have fun with that Concrete though. It's a hot one here today!!!

If you get a chance to work on it later and find something out please let me know.

Thanks
Josh

Two problems, one your's one Haas's, but first a question; do you use Graphics to check your programs, especially by zooming in to see the detail of the toolpath? I suspect you do not because you would probably have found both.

I renumbered your program so I could refer to line numbers.

Line N19 which is supposed to give a chamfer does not chamfer during the G71 the tool just plunges straight in, but it does the chamfer during the final run through the P, Q block and during the G70. I do not use the automatic chamfering so I would never get something like this.

Line 21 which does the radius should be a negative value, your radius goes the wrong way.

%
O00000
N1
N2 G53 G00 X0 Z0
N3 T202
N4 S1200 M03
N5 G00 X1.3 Z0.
N6 G50 S3500
N7 G96 S250 / M08
N8 G99
N9 G01 X-0.05 F0.006
N10 G00 Z0.2
N11 X1.3
N12 G71 P13 Q27 U0.04 W0.005 D0.04 F0.008
N13 G00 X0.45 Z0.01
N14 G01 Z0.001
N15 X0.51 R-0.03
N16 Z-0.375
N17 X0.62 K-0.05
N18 Z-1.25
N19 X0.506 A210. Chamfer is ignored by G71
N20 Z-1.575 R0.05
N21 X0.629 R0.015 R value should be -0.015
N22 Z-1.98
N23 X0.866 R-0.03
N24 Z-2.175
N25 X1.18 K-0.04
N26 Z-2.625
N27 X1.3
N28 G53 G00 X0 Z0
N29
N30
N31 G53 G00 X0 Z0
N32 T202
N33 G97 S1200 M03
N34 G00 X1.3 Z0.2
N35 G50 S3500
N36 G96 S300 / M08
N37 G99
N38 G70 P13 Q27 F0.004
N39 G00 X1.3
N40 Z-1.98
N41 G01 X0.609 F0.003
N42 G00 X1.3
N43 Z-2.175
N44 G01 X0.846
N45 G00 X1.3
N46 G53 G00 X0 Z0
N47 M30
%