[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]

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]

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]

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]

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]

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]

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

[txcncman]

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

Right as usual. I get jumped on a lot for being rough on questioners. But in my defense, most of the questioners have done little to research any answers on their own. They jump on CNCzone knowing some idiot like myself will at least try to help them out. This guy proved it when he would not even go look up the thread data in Machinery's Handbook. I doubt he even owns a copy. But I went ahead and did his homework for him. Out of every 10 questioners, there are 1 or 2 that are legitimately trying to be better machinists. Those 1 or 2 are the only ones I care about.

[fordav11]

I usually just do a search. if I find info I point them to it.... saves typing.
otherwise if I find nothing useful I'll get the info from the memory bank in my skull, hoping that the info is still there and the battery hasn't gone flat.

[cncwhiz]

Right as usual. I get jumped on a lot for being rough on questioners. But in my defense, most of the questioners have done little to research any answers on their own. They jump on CNCzone knowing some idiot like myself will at least try to help them out. This guy proved it when he would not even go look up the thread data in Machinery's Handbook. I doubt he even owns a copy. But I went ahead and did his homework for him. Out of every 10 questioners, there are 1 or 2 that are legitimately trying to be better machinists. Those 1 or 2 are the only ones I care about.

Dude,
Your a tool. All I was looking for was a threading cycle for a friends shop. If you read my post you would have seen that I am not a lathe guy. I would blow you away for anything milling. txcncman; your way cool helping me out on this issue. I will take this posting to the lathe shop and give it to my friend. For all the guys that help me thank you very much. for you big talking hobby shop guys that trow rocks at other people have a nice day. I have been a member of this forum for years, I dont come here as much as I uesd to. bone heads like this guy are a good reason.

[dcoupar]

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.

I assumed that CNC Zone was a "volunteer" effort... silly me.

I suggest we take up a collection so you can be compensated for your time spent here. I know that the advice you gave to me earlier this week in the CNC Tooling Forum was invaluable.

There are many folks here like Bill (angelw), SteveO, and others too numerous to mention that go to extreme lengths to be helpful. Never once have I seen any of these guys (or gals) complain about how much time they spent to provide a solution, or that "I don't paid for it." (I assume you meant that you don't GET paid for it.)

Obviously your time is much too valuable to be wasted here, especially on the 8 or 9 out of 10 that you DON'T care about. You probably should pre-qualify the OP's to be sure they are worthy of your help.

Dave

[txcncman]

I assumed that CNC Zone was a "volunteer" effort... silly me.

I suggest we take up a collection so you can be compensated for your time spent here. I know that the advice you gave to me earlier this week in the CNC Tooling Forum was invaluable.

There are many folks here like Bill (angelw), SteveO, and others too numerous to mention that go to extreme lengths to be helpful. Never once have I seen any of these guys (or gals) complain about how much time they spent to provide a solution, or that "I don't paid for it." (I assume you meant that you don't GET paid for it.)

Obviously your time is much too valuable to be wasted here, especially on the 8 or 9 out of 10 that you DON'T care about. You probably should pre-qualify the OP's to be sure they are worthy of your help.

Dave

Did you follow me here to this thread to post something about G76 threading cycles? Just because I do not put much stock into people that call themselves "engineer" does not mean I do not have at least some useful information to share. I think I will lay off for a few weeks and sit back and watch how many questions get answered in a timely manner. Hope you have a great week.

[cncwhiz]

Did you follow me here to this thread to post something about G76 threading cycles? Just because I do not put much stock into people that call themselves "engineer" does not mean I do not have at least some useful information to share. I think I will lay off for a few weeks and sit back and watch how many questions get answered in a timely manner. Hope you have a great week.

First off, if you are referring to me I am not an engineer. I am the guy that fixes their mistakes, I'm a machinist/ programmer. As far as you help, if you died tomrrow someone else will step up and be a god like you think you are and awnser the questions that needed awnsers. Have a great few weeks, heck take a month...

[dcoupar]

First off, if you are referring to me I am not an engineer. I am the guy that fixes their mistakes, I'm a machinist/ programmer. As far as you help, if you died tomrrow someone else will step up and be a god like you think you are and awnser the questions that needed awnsers. Have a great few weeks, heck take a month...

cncwhiz: I believe he was referring to me. My title is Application Engineer. I was a machinist/programmer/field-service tech before I became an Application Engineer, but he took exception to the "Engineer" part.

txcncman: No, I didn't follow you here. I hang out here quite a bit, trying to help when I can.

I'm sure you have oodles of useful information to share. We'll miss your sunny disposition while you "lay off".

Trust me, I will have a great week. Thanks for the kind wishes.

[cncwhiz]

cncwhiz: I believe he was referring to me. My title is Application Engineer. I was a machinist/programmer/field-service tech before I became an Application Engineer, but he took exception to the "Engineer" part.

txcncman: No, I didn't follow you here. I hang out here quite a bit, trying to help when I can.

I'm sure you have oodles of useful information to share. We'll miss your sunny disposition while you "lay off".

Trust me, I will have a great week. Thanks for the kind wishes.

Whats up with that guy? I think he has a god complex.