What's new
What's new

G76 Tapered Thread Cycle

Rogue_Machinist

Hot Rolled
Joined
Jul 26, 2011
Location
Oregon, USA
So in my shop I cut pretty much 99.9% straight thread. But I have a customer who wants 150 1/2"NPT male threads single pointed. But all the thread cycles ive tried are being a pain in the butt and I get 6 parts and the insert chips. Does anyone have a 2 line g76 I could use as a guide to set it up. Ive tried using the G32 for the taper and its pretty much worthless as it doesnt seems to wanna read on my machine. Thanx in Advance.

P.S. I thread a lot and never have issues. This thread is just giving me a fit.
 
thanx the machine I usually use only accepts g92 thread cycles. Our newer machine doesnt get much threading work. And like anything else you dont use your programming skills you forget sometimes.
 
What is the material? Maybe the first pass is too heavy and is killing inserts prematurely. Are you turning the taper before you thread?
I always use G92 cycle with NPT threads.
 
What is the material? Maybe the first pass is too heavy and is killing inserts prematurely. Are you turning the taper before you thread?
I always use G92 cycle with NPT threads.
Nope. Customer specifically gave us print yo not turn the angle. .840" diameter. And first cut is only .003". Material is 304ss. And I didnt know you could use a g92 to do a tapered thread.

Sent from my LM-V600 using Tapatalk
 
My day shit counterpart makes a bunch of these. I myself don't make them. They are for inhouse use. Butter them up with pipe dope and wrencher down. He is cutting the taper before chasing the threads. You never say but this is run on a i series Fanuc control.

Brent

N50(1/2-14 NPT)

G0G99G40G54X12.Z7.T0
T0707
G97S300M3
G0X6.Z.1
G0X1.05Z.1M8
G76P030060Q0070R0
G76X.755Z-.80R-0360P0570Q0070F.07142
G0X7.M9
G0G40X12.Z7.T0
M1

20210509_235945.jpg
20210510_000623.jpg
 
Nope. Customer specifically gave us print yo not turn the angle. .840" diameter. And first cut is only .003". Material is 304ss. And I didnt know you could use a g92 to do a tapered thread.

Sent from my LM-V600 using Tapatalk
Hello nissan300ztt,
Some people just don't have a clue. By not permitting the taper to be turned is simply making the part considerably harder to make and you would have to use a full form threading insert, or stuff around cutting the crest of the thread by cutting the taper again after the thread was cut.

You could cut the taper before screw cutting, leaving the diameter of the taper up on size and it would be impossible to tell if the thread was cut with the taper pre-cut or not.

Taper cutting with G92 uses the same type of "R" argument as G76, representing the amount of radial difference in the taper from where the tool starts in fresh air in Z at the start of the thread, to the Z finish point of the thread. Following is the syntax for cutting a taper thread with G92.

G92X__ Z__ R__ F__

Where:
X = X coordinate for thread pass at the large diameter of the taper (male thread).
Z = Z Finish Point of thread.
R = Radial amount of taper between Z start and Z finish point and will be in a minus direction when cutting a male thread.

Not cutting the Taper will make using the G76 cycle difficult. The X specified in the G76 cycle is the Minor Diameter of the Thread at the large diameter of the taper. The first pass of the threading cycle takes a specified first DOC amount. This amount would be applied at the large diameter of the taper, and at the small end of the taper, if it had been cut, by the "R" argument specified in the cycle. If the taper is not cut, the tool will start with a DOC at the start of the thread equal to the first DOC amount, plus the amount of radial taper. In Brent's example in Post #6, that DOC for the first pass would start at 0.043" at the start of the thread and wash out to 0.007" at the Z Finish point, large diameter of the thread. I would not be surprised to see the insert break on the first pass.

The same difficulty would apply with the G92, with either a lot of air cutting, or a more difficult programming project than it needs to be, by programing specific X and Z values for the first part of the taper until down to a diameter where the last part of the thread can start to be cut.


Regards,

Bill
 
So I was put back on this job today and ended up email the engineer in charge of this job and explained the situation and they said cutting the taper was fine. LOL. I need to get out my programming books again its been a long time since I used some of these thread canned cycles. Thanx for all the input.
 
My day shit counterpart makes a bunch of these. I myself don't make them. They are for inhouse use. Butter them up with pipe dope and wrencher down. He is cutting the taper before chasing the threads. You never say but this is run on a i series Fanuc control.

Brent

N50(1/2-14 NPT)

G0G99G40G54X12.Z7.T0
T0707
G97S300M3
G0X6.Z.1
G0X1.05Z.1M8
G76P030060Q0070R0
G76X.755Z-.80R-0360P0570Q0070F.07142
G0X7.M9
G0G40X12.Z7.T0
M1

View attachment 320802
View attachment 320803

That program worked great. Thanks for the information. Engineer was very happy with the outcome.
 
So in my shop I cut pretty much 99.9% straight thread. But I have a customer who wants 150 1/2"NPT male threads single pointed. But all the thread cycles ive tried are being a pain in the butt and I get 6 parts and the insert chips. Does anyone have a 2 line g76 I could use as a guide to set it up. Ive tried using the G32 for the taper and its pretty much worthless as it doesnt seems to wanna read on my machine. Thanx in Advance.

P.S. I thread a lot and never have issues. This thread is just giving me a fit.

Understand the frustration. Tapered threads they only need to be done right either on lathe or mill with threaders which is my preferred method on them.


Dang insert? You could use more passes most likely. Material and quality of insert are known variables too the simple variety. Also you might rough thread it then finish thread it with a another threader. That way the chipped insert can actually keep being used. I think it is best to salve that problem completely.

At the least pace your threading inserts and check for the chipped insert before removing the part. That way you can back off and clean up the threads likely where the chipped tooth left material.

Don’t do things dirty allow some good machining practices. At least you can determine the rate at which that insert stops giving you good threads and change it before it chips at least.
 
G76 can cut tapered - insert an "R" value in the line with the taper amount. "R-" will taper upwards towards the rear, "R+" will taper downwards.
 
Yeah I know just wasnt sure the actual values for the 1/2" NPT. I got it sorted.

Hello nissan300ztt,
The easiest algorithm to use in calculating the R value to use in the G76 Cycle is:

R = Z x 0.03125

Where:
Z = Total Z move of the tool
0.03125 = Radial Constant for diameter taper of 1:16

Regards,

Bill
 
Hello nissan300ztt,
The easiest algorithm to use in calculating the R value to use in the G76 Cycle is:

R = Z x 0.03125

Where:
Z = Total Z move of the tool
0.03125 = Radial Constant for diameter taper of 1:16

Regards,

Bill

I use Z/32 which is easier to remember.
 
I noticed yesterday (test cutting NC-50 pipe thread) that if you're using "60" (flank cutting) as opposed to 00 (plunge cutting) in the first G76 line (eg P010060), it messes with your taper angle! I dry ran it and calculated the angle (took pictures of the "distance to go" values while it was threading).
It's easy to calculate. What the machine does is: It moves over the Z-start position to start from the top of the one side of the flank. So you just have to use the thread depth value (P-value in second G76 line) and calculate: tan(30) (flank angle) X thread depth (P-value) X tan(4.764) (thread taper angle)
I made a Google sheet (you can copy it to use/edit it) that calculates the correct R-value for the second G76 line (negative value for OD thread).
https://docs.google.com/spreadsheets/d/12EknKs2dvL48GFfXVQhzTETzxx4SXRX78neDTQQwiM8
 

Attachments

  • Screenshot_20230805-094341.png
    Screenshot_20230805-094341.png
    351.1 KB · Views: 8
Last edited:
If you are not using a full profile insert it is more difficult to keep the root and crest truncation in tolerance. And if you are not turning the taper to size and not usimg a full profile insert the crest truncation will never be correct.

I turn the taper leaving a few thousandths for topping. This is not necessary but the topping threading insert lasts longer because it takes less stock. 45 chamfer the leading edge to just below the minor dia will help too.
 








 
Back
Top