Thread: Fanuc 6T Post

Hi

I have a fanuc 6T control on a Nakumara TMC4. I purchased Mastercam recently and they provided me a generic post however it does not match my machine.
So I am wondering if somebody may have some examples of the G-code format. I do have a manual but it dates back to 1980

This much i know its a single line I did manage to find this one in the past and it works

G71 P (?) Q (?)U.05 W.005 D1500 F.015

Originally Posted by cookie54

Hi

I have a fanuc 6T control on a Nakumara TMC4. I purchased Mastercam recently and they provided me a generic post however it does not match my machine.
So I am wondering if somebody may have some examples of the G-code format. I do have a manual but it dates back to 1980

This much i know its a single line I did manage to find this one in the past and it works

G71 P (?) Q (?)U.05 W.005 D1500 F.015

The 1980 manual is correct for the 6T. 6, 10, 11, 12, and many 15 use the single line cycles. Some 15, and most 16, 18, 21, 32, 31, 30, and 0 use the two line cycles.

You'll probably need to have them cook up a post as the older controls have been out of production for so long.

I have Mastercam, but I purchased it used 12 years ago.

"I purchased mastercam for me 6T..." Doesn't seem right. Why? You had to've paid more for the software than the machine, right?

Lathe code is pretty simple. If mastercam is spitting out wrong code I can't imagine tweaking it by hand is so hard?

You could always, just not use canned roughing. Until you figure it out.

Originally Posted by GENERALDISARRAY

You could always, just not use canned roughing. Until you figure it out.

I never used canned cycles in my 6T because I was never able to make it work.

Originally Posted by wheelieking71

I never used canned cycles in my 6T because I was never able to make it work.

Really?
I had an old 6T-B and the one line canned cycles worked ok. Same as my 10's and 11's.

No type 2 roughing with the 6T but other than that the canned cycles work pretty much the same. Two line G76 is different.

Brent

Originally Posted by yardbird

No type 2 roughing with the 6T but other than that the canned cycles work pretty much the same. Two line G76 is different.

Brent

Hello Brent,
Type II was available with the 6T Model B.

Regards,

Bill

Hi DouglasJRizzo & Wheelieking

Your right about the post i will get one to fit my machine. The generic on spits out

3 axis instead of 2 only

It doesn't make the G50 X0.0 Z0.0 to work with G28 U0.0 W0.0

I would like it to do a M5 before it goes to G0G28U0.0 W0.0 if not the spingle ramps up in full RPM till it hits machine 0 then it shuts off
I tried a threading cycle and for some reason it throws a A58 in the threading cycle instead of a A60 the machine faulted again the manual requires A60

If I idle the machine in M41 spindle low range (Warm Up) Start the program that needs to be in M42 the machine wont shift and wont run but i can shift with the control panel. Does this machine have to be running for a gearbox change from low to high?

regards
Eric

Originally Posted by cookie54

Hi DouglasJRizzo & Wheelieking

Your right about the post i will get one to fit my machine. The generic on spits out

3 axis instead of 2 only

It doesn't make the G50 X0.0 Z0.0 to work with G28 U0.0 W0.0

I would like it to do a M5 before it goes to G0G28U0.0 W0.0 if not the spingle ramps up in full RPM till it hits machine 0 then it shuts off
I tried a threading cycle and for some reason it throws a A58 in the threading cycle instead of a A60 the machine faulted again the manual requires A60

If I idle the machine in M41 spindle low range (Warm Up) Start the program that needs to be in M42 the machine wont shift and wont run but i can shift with the control panel. Does this machine have to be running for a gearbox change from low to high?

regards
Eric

Hello Eric,
With regards to the threading cycle, I assume G76, are you saying that the machine actually alarms when A58 is specified, or do you mean that the A58 is the error? It may be your interpretation that the manual requires A60, but I doubt that the manual actually says that. Specifying A58 for the included angle of a 60deg Threading Tool is quite legal with the 6T control, even with the model A; the allowable angles are Zero to 120degs in increments of 1deg. The control only knows the included angle of the tool by what is specified by address A in the program and as long as an angle between Zero and 120degs is specified (in increments of 1deg.) then there should be no issue.

Its quite a common practice to specify an angle that is a few degrees less than the actual included angle of the Threading Tool, particularly on coarse pitched threads that will have a corresponding large thread height. The reason being is that when the actual included angle of the Threading Tool is specified, all of the cutting will be done with the leading edge of the insert and it can result is a slightly stepped and poor finish on the trailing flank of the thread form. By specifying an included angle slightly less than the actual Threading Tool, most of the cutting will be done by the leading edge of the tool and a slight amount by the trailing edge.

It would be better if you were to Post examples of your code so that the Forum members can give you more informed answers.

Regards,

Bill

Originally Posted by cookie54

Hi DouglasJRizzo & Wheelieking

Your right about the post i will get one to fit my machine. The generic on spits out

3 axis instead of 2 only

Have you tried

LATHE 2-AXIS SLANT BED.mcam-lmd

Hi Everybody,

In regards to my threading program here is the code for discussion

M42
N5T0100
(OD THREAD RIGHT)
(MAX - Z-.036 MIN - Z-.8925)
G98
G97S200M03
G0X1.5125Z-.036M08T0101
G76X1.2352Z-.8925I0.K0387D0150A60F.0714
M09
G50X0.Z0.
G0G28U0.W0.
T0100
M05
M01

(BORE ID)
G0G28U0.W0.
G50X0.Z0.
M42
N6T0800


With the A58 angle the machine would Index the turret and go to the position of starting the thread cycle and then block and give a program alarm 060 Program

By changing the A58 to A60 the lathe would cycle through.

The A 58 came from MasterCam it was set up in the Parameters. 29 degree lead angle. I attached the a copy of the manual

I got my Post modified now.

Originally Posted by cookie54

Hi Everybody,

In regards to my threading program here is the code for discussion

M42
N5T0100
(OD THREAD RIGHT)
(MAX - Z-.036 MIN - Z-.8925)
G98
G97S200M03
G0X1.5125Z-.036M08T0101
G76X1.2352Z-.8925I0.K0387D0150A60F.0714
M09
G50X0.Z0.
G0G28U0.W0.
T0100
M05
M01

(BORE ID)
G0G28U0.W0.
G50X0.Z0.
M42
N6T0800


With the A58 angle the machine would Index the turret and go to the position of starting the thread cycle and then block and give a program alarm 060 Program

By changing the A58 to A60 the lathe would cycle through.

The A 58 came from MasterCam it was set up in the Parameters. 29 degree lead angle. I attached the a copy of the manual

Hello Eric,
That's an unusual alarm number to be raised for an issue relating to the included angle of the thread form specified, because p/s060 is normally raised for the following reason:

"Commanded sequence number was not found in the sequence number search."

See the extract from Fanuc 6T manual following:



So I think this is an issue peculiar to your machine.



Regards,

Bill

Hi Bill,

Sorry for the mistake I provided the wrong error code

Went back and double checked the machine and found that it is actually 062 Program

Regards,
Eric

Originally Posted by cookie54

Hi Bill,

Sorry for the mistake I provided the wrong error code

Went back and double checked the machine and found that it is actually 062 Program

Regards,
Eric

Hello Eric,
That makes more sense. I suspect that your control is quite an early build of the 6T Model A control. When in memory mode, do you see a whole page of code (when you have the program page selected), or just the current and pending Block? If not a whole page, then the control is a Model A. Another telltale of the Model B, if the plate has not been lost, is a Yellow Fanuc plaque attached to the front of the control; the plaque of the Model A is white.

Actually, I thought the FS5T control was able to use any angle, in increments of 1deg, between Zero and 120deg, but it can only use the angles 0, 29, 30, 55, 60 and 80, the same as listed in your manual. There was a lot of carry forward from the FS5T control, including the same, seven segment LED display and no CTR screen for the very early FS6T controls. For the reason give in my earlier Post, it's still a common practice to specify an angle of 55degs, when cutting a Thread using a tool with an included angle of 60deg.

Regards,

Bill

Originally Posted by cookie54

I have a fanuc 6T control on a Nakumara TMC4. I purchased Mastercam recently and they provided me a generic post however it does not match my machine.

So.... why don't you call them and get it sorted out?

Hi Bill

The machine produces the whole page on the screen and there is also a white plate at the bottom of the control panel.

It has a Model number starting with A02B- 00 It was made in November 1980

Regards
Eric