Desperately need help cutting threads

[Cec330]

I took a new job this week as an operator only to find out that the previous fella that ran this machine wiped all the programs out of the machine. I need help writing a program to cut 12 tpi I’m assuming that I’ll have to use the G32 code? I’ve never programmed a lathe before and am pretty lost. They are internal threads 1.125” deep inside of a 5.410 inside diameter. Just an example program would help a bunch. Thank you in advance for any help.

 

[Ianagos]

What controller?

Just program it up in cam software if you don’t know how to write gcode?

Im confused how someone who doesn’t know anything about a cnc lathe can end up programming one?

 

[Cec330]

It’s a hitaci seiki with a seicos j300L control. I’ve operated turning centers in the past and have edited programs but have only written one program. I don’t have no cam software. No one in this shop knows anything about this machine I was just thrown to the wolves.

 

[modelmakerblue]

It’s a hitaci seiki with a seicos j300L control. I’ve operated turning centers in the past and have edited programs but have only written one program. I don’t have no cam software. No one in this shop knows anything about this machine I was just thrown to the wolves.

Bloody hell this is ridiculous & downright dangerous!!!You need proper training & experience to run CNC & manual machines.Your so called managers need to get a grip & organise training etc.
Tony

 

[mc3608]

You don't have a programming manual for the machine?

 

[Cec330]

Tony I’ve been a machinist since 1993 it’s all I’ve ever done, I’ve operated every machine tool you can think of I’ve just never programmed a turning center. I’m just asking for help figuring out how to cut these threads.

 

[Cec330]

Yes I have a programming manual but it says nothing about how to program threading.

 

[Cec330]

Year about 1993 and model hires-turn 20J

 

[Fancuku]

I took a new job this week as an operator only to find out that the previous fella that ran this machine wiped all the programs out of the machine. I need help writing a program to cut 12 tpi I’m assuming that I’ll have to use the G32 code? I’ve never programmed a lathe before and am pretty lost. They are internal threads 1.125” deep inside of a 5.410 inside diameter. Just an example program would help a bunch. Thank you in advance for any help.

Keeping it simple

G97 S250 M3
G0 X5.1 Z0.3 M8
G92 X5.42 Z-1.125 F0.0833
X5.43
X5.44
X5.45
X5.46
X5.470
X5.477
X5.483
X5.488
X5.493
X5.497
X5.5
X5.502
X5.504
X5.505
G0 Z0.5 M9
G30 U0 W0
M1

 

[Cec330]

I stopped and talked to an old buddy of mine that programs and he told me about the G76. I’m trying to convert his fanuc program to my machines style of program.

 

[wmpy]

The G76 format for the J300L is a single line and is as follows:

G76 X Z K D F A

X= diameter of final pass
Z= ending Z position
K= height of thread
D= depth of 1st path
F= thread lead
A= angle of thread

The Fanuc G76 cycle will probably be the 2-line format and will look something like this:

G76 P010055 Q0015 R0.0015
G76 X5.505 Z-1.125 P0475 Q0150 F0.083333

The J300L version of that would look like this:

G76 X5.505 Z-1.125 K0.0475 D0.0150 F0.083333 A55

I hope this helps. I have a HT23J with J300L control. Let me know if you've got any other questions about the machine.

 

[implmex]

All I can say is WOW... I sure don't want to be anywhere near when the program first gets fired up and run.
I'm with modelmakerblue on this ...bring spare underpants when you push the green button for the first time.

Better yet, post your code here before you load it into the control.
No guarantees, but if there's an obvious mistake in your code, hopefully someone will catch it and keep you from slamming the turret into the chuck or something else equally exciting.

Whoever is OK with turning you loose on this has got big brass ones for sure.
Will he still be OK when you crash the lathe?

Good luck with it.

Cheers

Marcus
Implant Mechanix • Design & Innovation > HOME
Vancouver Wire EDM -- Wire EDM Machining

 

[Spruewell]

Are there no backup files anywhere? A pc somewhere in the shop with saved program files? It is highly unlikely that the previous operator cleaned out all the companies program files for this machine and the parts it ran (unless there was some serious bad blood). Most machines have a limited amount of memory available making it impractical (not to mention foolish) to leave all the programs on the control with no backup.

 

[EmGo]

This wonderful machine can't run standard G33 threading passes ? Thats easy to figure out and also easy to single-block. It's pretty foolproof.

 

[angelw]

I took a new job this week as an operator only to find out that the previous fella that ran this machine wiped all the programs out of the machine. I need help writing a program to cut 12 tpi I’m assuming that I’ll have to use the G32 code? I’ve never programmed a lathe before and am pretty lost. They are internal threads 1.125” deep inside of a 5.410 inside diameter. Just an example program would help a bunch. Thank you in advance for any help.

Hello Cec330,
Your control can use a Multi-repetitive Threading Cycle G76 in the following format:

G76 X_ _ Z_ _ K_ _ D_ _ F_ _ A_ _ P_ _

Where:
X = X Coordinate of Minor Dia. when cutting and External Thread. Major Diameter when cutting an Internal Thread.
Z = Z Finish Coordinate
K = Thread Height (Radius Value)
D = DOC for the first Threading Pass (Radius Value)
F = Lead of Thread
A = Included Angel of Thread Form (Included Angel of Threading Insert)
P = Cutting Pattern (P1 to P4)

The Cutting Pattern most commonly used is specified by P1 (Constant Cutting Amount - Single Cutting Edge). If the "P" address is omitted, P1 is assumed by the control.

When cutting an Internal Thread, the Major Diameter is specified by the X address and the Thread Height by the K address. Given these two values, the control calculates the coordinate of the Minor Diameter, with the First Pass and all subsequent DOC being applied from that calculated diameter.

In your example, you have specified the Minor Diameter and Thread Pitch (Lead). On the assumption that it a 60deg. Thread Form, the Major Diameter is 5.5".

To cut an External Thread, you initially park the Threading Tool at a diameter larger than the Major Diameter, and for an Internal Thread, at a diameter smaller than Minor Diameter of the Thread. Provided the X and K values have been correctly specified, the control determines whether an Internal or External Thread is being cut by comparing the specified X value in the G76 Cycle and the current position of the Threading Tool in X.

Constant RPM spindle speed should be specified and not Constant Surface Speed. If a not too difficult to cut steel is the material being used, a reasonable starting CSS would be circa 490SFM and at a Major Diameter of 5.5", that equates to 340RMP.

Because the tool must accelerate from Zero to a Z axis Slide Velocity equaling the Thread Lead x Spindle RPM, each time a Threading Pass is Started, the tool should be parked at a Z coordinate far enough away form the start of the Thread, so that the correct Slide Velocity is reached before starting to cut. If not, then the lead of the first part of the Thread will be incorrect. The greater the Slide Velocity, the greater distance required for the correct Slide Velocity to be reached. There is a formula for calculating the minimum distance required, but with a Spindle Speed of 340 RPM and a Thread Lead of 0.0833" a 0.25" standoff in Z will be plenty.

So, putting all the above together, a G76 Block something like the following will get you close:

G76 X5.5 Z1.125 K0.0496 D0200 F0.08333 A60 P1

Incorporated into the program, it may look something like the following for your control:

N2 G28 U0.0
G28 W0.0
T0100 G97 S340 M03
G00 Z0.25 T0101 M08
G00 X5.3
G76 X5.5 Z1.125 K0.0496 D0200 F0.08333 A60 P1 (P1 could be omitted)
G28 U0.0 M09
G28 W0.0
M01

Regards,

Bill

 

[Mtndew]

Man, if it were me, I'd be looking for another place of employment. It says a lot about the company and how much they want to grow when nobody in the higher-ups know how to do a simple lathe program.
I feel for ya, it doesn't sound like a great place to work.

 

[dieselpilot]

All I can say is WOW... I sure don't want to be anywhere near when the program first gets fired up and run.

Doesn't anyone dry run, single block with feeds turned way down anymore? Or does everyone just simulate and send it now?

Man, if it were me, I'd be looking for another place of employment. It says a lot about the company and how much they want to grow when nobody in the higher-ups know how to do a simple lathe program.
I feel for ya, it doesn't sound like a great place to work.

The guy that left and wiped the programs had the same idea. Isn't that straight up theft?

 

[Mtndew]

The guy that left and wiped the programs had the same idea. Isn't that straight up theft?

I don't know about theft, but it's definitely a petty,dick move by that guy. And it sucks to be tossed into the position that you're in right now. Fortunately a thread program is easy enough.
angelw gave you some good tips above, he's knows his shit and has probably forgotten more about Fanuc style programming than I have learned over the last 35 years.

 

[michiganbuck]

Better to hire someone to write a few programs that less skilled might work off from.

Often there is a retired guy who might come in for dirt low wages or reasonable just for something to do.

 

[triumph406]

I'd use a large z axis offset, away from the chuck, and if it was my first rodeo I'd put a piece of delrin in the chuck and run that so as to avoid damaging the tool.

---------------

The first time I thread milled I tried it on a piece of delrin first, didn't want to crash the thread mill into solid metal, or otherwise f'up.