1/4 NPT threading cycle (G76)

[cncwhiz]

I am looking for a canned cycle for a fanuc OT control on a femco lathe. I am a mill programmer and I have not been on a lathe in a long time. Im pretty sure that I can use a "G76" cycle to cut a 1/4 NPT thread. The depth in Z is only .375. Does someone have a cycle they can send me ? Could yo also explain the cycle so I can see how to control the cycle?

Thanks
Terry

[txcncman]

ID or OD thread?

http://www.visinia.com/cnc-programmi...lathe-machine/

[cncwhiz]

Originally Posted by txcncman ID or OD thread? CNC Blog | Tapered Threading with Fanuc G76 Cycle on CNC Lathe Machine - CNC Blog

They are OD threads. Do you have one for 1/4 NPT?

[txcncman]

No, I do not have one already written. Do you have Machinery's Handbook? What is the starting diameter? What is the thread length? What is the finish diameter? What is the pitch? What is the lead? How much depth of cut do you want to start with? How much depth of cut would you like to have on the final pass? What the the height of a single thread depth from crest to root?

[cncwhiz]

Originally Posted by txcncman No, I do not have one already written. Do you have Machinery's Handbook? What is the starting diameter? What is the thread length? What is the finish diameter? What is the pitch? What is the lead? How much depth of cut do you want to start with? How much depth of cut would you like to have on the final pass? What the the height of a single thread depth from crest to root?

I dont have that information off hand but is this the information that I need to have for this cycle? I you are anyone else explain the necessary format for this cycle?

[txcncman]

My plan was to explain where to put in the numbers once you get them. I was not going to totally stop what I was doing and go look up thread specs for you.

[cncwhiz]

Originally Posted by txcncman My plan was to explain where to put in the numbers once you get them. I was not going to totally stop what I was doing and go look up thread specs for you.

I am not looking for someone else to figure it out for me. I am just looking for either a completed canned cycle for this thread or detailed info on how to build the cycle.

[angelw]

Originally Posted by cncwhiz I am not looking for someone else to figure it out for me. I am just looking for either a completed canned cycle for this thread or detailed info on how to build the cycle.

txcncman has already given you this information with the links he provided. However, following is another explanation. All you have to do is get the values for the thread you want to cut and fill in the blanks.

Regards,

Bill

G76P00_00_00 Q _ R _;
G76X (u) _ Z(W) _ R _ P _ Q _ F _ ;
The the first G76 block is specified as follows, where:
First 2 characters = Repetitive count in finishing (1 to 99). This designation is modal and is not changed until the other value is designated. Also this value can be specified by the parameter No. 5142, and the parameter is changed by the program command.

Second 2 characters = Chamfering amount
When the thread lead is expressed by L, the value of L can be set from
0.0L to 9.9L in 0.1L increment (2–digit number from 00 to 90).
This designation is modal and is not changed until the other value is
designated. Also this value can be specified by the parameter No.
5130, and the parameter is changed by the program command.

Third 2 characters = Angle of tool tip
One of six kinds of angle, 80°, 60°, 55°, 30°, 29°, and 0°, can be selected, and specified by 2–digit number.
This designation is modal and is not changed until the other value is designated. Also this value can be specified by the parameter No. 5143, and the parameter is changed by the program command.
(Example)
When:
1. Finish repeats = 2,
2. Chamfer amount r= 1.2 x Lead
3. Included angle of thread (Angle of tool tip) = 60°

The first G72 block P address is specify as follows.
P02 12 60

Q of first G76 block = Minimum cutting depth (specified by the radius value).
When the cutting depth of one cycle operation (Δd –Δd –1) becomes smaller than this limit, the cutting depth is clamped at this value. This designation is modal and is not changed until the other value is designated. Also this value can be specified by parameter No.
5140, and the parameter is changed by the program command.

R of first G76 block = Finishing allowance
This designation is modal and is not changed until the other value is designated. Also this value can be specified by parameter No.5141, and the parameter is changed by the program command.

The second G76 block is specified as follows, where:
X(U) = Minor (root) diameter of external thread, major (crest) diameter of internal thread. U is incremental equivalent of absolute X

Z(W) = Finish Z coordinate of thread. W is incremental equivalent of absolute Z

R = Difference of thread radius. If R = 0, parallel thread will be cut. In an External tapered thread X will equal the Root diameter at the major diameter of the taper. R will be specified as the radial difference between of the taper calculated from where the tool starts clear of the workpiece to the end Z coordinate. In this case the R will be a negative value.

P = Height of thread. This value is specified by the radius value.

Q = Depth of cut in 1st cut (radius value)

F = Lead of thread

[txcncman]

Not in any particular order for 1/4-18 NPT:

Height of sharp V thread 0.04811 (Height of truncated thread 0.04444/0.03833)

Lead of course is 18

Pitch is 1 / 18 = 0.0556

Length is 0.5946

Large diameter is 0.540 (Size of pipe)

Taper is 3/4" per foot measured on diameter (This sets a ratio of 0.750 / 12. = 0.0625)

0.0625 X 0.5946 = 0.0372 (The small diameter of the taper will be 0.0372 smaller than the large diameter). The difference in radius will be 1/2.

0.540 - 0.0372 = 0.5028 for the small diameter

The root diameter will be the large diameter minus 2 times the thread height. I always use sharp V thread height in calculations.

0.540 - ( 2 X 0.0481 ) = 0.4438

I will set the first threading pass for 0.012" and the amount for the finish pass at 0.001".

Earlier I forgot got the minimum cutting depth. This does not effect the finish pass. I will set that to 0.005".

P's and Q's are set in ten-thousandths. (i.e. P1 = 0.0001", P0500 = 0.050")

Now, to fill in the blanks:

G76 P010060 Q0050 R0.001;
G76 X0.4066 Z-0.5946 R-0.0186 P0481 Q0120 F0.0556;

Hope that helps. This took about 30 minutes of my time to type all this out and make sure it was correct. I don't paid for it.

[angelw]

Originally Posted by txcncman G76 P010060 Q0050 R0.001; G76 X0.4066 Z-0.5946 R-0.0186 P0481 Q0120 F0.0556;

1. The X address is specified as the root diameter at the large end of the tapered thread, X 0.4438
and
2. the R value to specify the radial difference in small and large diameter, is calculated from where the threading tool starts in Z clear of the workpiece. Assuming in your example the end of the workpiece is Z Zero, then the formula for calculating "R" would be as follows:

Where:
R = Radial difference between large and small end of thread
ZC = Clearance of tool in Z from start of thread = 0.2"

R = (0.0625 X (0.5946 + ZC))/2
R = (0.0625 X (0.5946 + 0.2))/2
R = 0.0248

G76 P010060 Q0050 R0.001;
G76 X0.4438 Z-0.5946 R-0.0248 P0481 Q0120 F0.0556


Regards,

Bill

[sinha_nsit]

Thread using g76 - Practical Machinist - Largest Manufacturing Technology Forum on the Web

[fordav11]

Originally Posted by txcncman Hope that helps. This took about 30 minutes of my time to type all this out and make sure it was correct. I don't paid for it.

hehe! for all the gory details you should have just pasted this link.....
http://www.cnczone.com/forums/fanuc/...ed_please.html

could have saved yourself 30 minutes


actually the OP should have done a search. there's many many posts on how G76 works. could have saved us all 30 minutes