What's new
What's new

Help with writing 1/8 NPT G76 threading cycle.

cgrim3

Cast Iron
Joined
Dec 4, 2020
Location
Baltimore
Hi all,

I needed some help programming a 1/8-27 NPT external thread on the lathe. Controller on lathe is Mitsubishi.

The thread is .3125 long. I have to go about .035" past .3125" to account for the .035" shoulder on the threading insert. I will start threading .2" in front of the part.

Also, one of the things I am confused about is which thread height to use in calculations. Do you use the "height of the sharp V thread" or "maximum height of thread" for your P value and to calculate your X? Refer to the link. For right now in the code below, I will use the "maximum height of thread".

NPT Thread Calculator

Here is what I have. Let me know if it is right or wrong.

Major Diameter of Big End: .405

Maximum height of thread = .0296

X value = .405 - (2 * .0296) = .3457

Z value = .3125 + .035 = .348

P = 296 since maximum height of thread is .0296

F = 1/27 = .03704

We know that an NPT thread is 1.7899 degrees. So to calculate R....

R = (.3125+.035+.2)tan(1.7899) = .0171

Therefore, my G76 line looks like this:

G76 X.3457 Z-.348 R-.0171 P296 F.03704

Again, I am not sure if you have to use "height of sharp v thread" or "maximum thread height" for your X calculations and P value. If anybody here knows, please chime in. Also, please tell me if my G76 line is correct or not.

For depth of each cut, # of spring passes, etc that is already in the controller settings. That info is not needed in the G code since it is already in the mits controller settings.

Angelw, you probably know this.

Thanks,

Chris
 

Booze Daily

Titanium
Joined
Sep 18, 2015
Location
Ohio
Doesn’t much matter. Just write something and adjust your tool offset til it gages.
Then adjust the program to account for the offset amt.
 

cgrim3

Cast Iron
Joined
Dec 4, 2020
Location
Baltimore
We did that in the past with NPT threads on the lathe and it worked but I just want to know if I am actually doing the G76 and P value correctly.
 

SeymourDumore

Diamond
Joined
Aug 2, 2005
Location
CT
Your G76 line looks good from here.
The R is negative as it should be for an external NPT, the minor X is probably OK @ the Z-.348.
It looks like a bit of a "stubby" thread as it should be .3924, but wotever.

The thread height is really only important for the depth calculations, which in turn effects the number of passes.
 

cgrim3

Cast Iron
Joined
Dec 4, 2020
Location
Baltimore
One of the main reasons I had a question about thread height is because somebody in a post on cnc zone was using "height of the sharp v thread" when doing NPT threads.

Also, is my R calculated correctly? You have to take into account the distance your tool is from the front of the workpiece correct?
 

SeymourDumore

Diamond
Joined
Aug 2, 2005
Location
CT
One of the main reasons I had a question about thread height is because somebody in a post on cnc zone was using "height of the sharp v thread" when doing NPT threads.

Also, is my R calculated correctly? You have to take into account the distance your tool is from the front of the workpiece correct?


Again, the thread height is affecting the incremental DOC and the # of cutting passes only.

As far as your R value, it is calculated as the incremental X-Radial distance between the X/Z-Endpoint and X/Z-Startpoint.

You have to take into account the distance your tool is from the front of the workpiece correct?

Yes, that is absolutely correct! ( I'm pretty sure you've got it figured out, just test it a bit more to let it sink in....)
 

sinha

Stainless
Joined
Sep 25, 2010
Location
india
R can be calculated more simply as L/32 where L is the total Z displacement (i.e., including initial Z clearance)

The X value in the G76 block is the level up to which the tool tip will go at the larger end. Therefore, the minimum thread height (0.02496) should be used in this calculation.
 

cgrim3

Cast Iron
Joined
Dec 4, 2020
Location
Baltimore
R can be calculated more simply as L/32 where L is the total Z displacement (i.e., including initial Z clearance)

The X value in the G76 block is the level up to which the tool tip will go at the larger end. Therefore, the minimum thread height (0.02496) should be used in this calculation.

Hi Sinha,

I appreciate your response. I ran the job and I had to adjust my offset by .005, which is about the difference between the minimum thread height and maximum height of thread. It seems you are correct. You have to use the minimum thread height
 
Last edited:

angelw

Diamond
Joined
Sep 10, 2010
Location
Victoria Australia
Hi Sinha,

I appreciate your response. I ran the job and I had to back my offset down about .005, which is about the difference between the minimum thread height and maximum height of thread. It seems you are correct. You have to use the minimum thread height

Hello cgrim3,
Theoretically that's correct, particularly where the Thread Form height is quite small, as in your example. However, there's a fudge that can be used where very coarse pitch threads, having a relatively large Thread Form height are concerned.

The algorithm used by the control to calculate each subsequent DOC is as follows:

DOC = d x SQRT(N)
Where:
d = First Thread Pass DOC
N = The Nth number of the Thread Pass (1,2,3,4,etc)

Calculation of each subsequent DOC proceeds in this manner until the specified minimum DOC is reached.

Rule of Thumb, the first pass DOC should be the greatest amount that the cutting tool and workpiece set up can safely tolerate.

On a Thread that has a large Thread Form Height, the DOC diminishes quickly and the Minimum DOC is used for much of the remainder of the Thread cutting.

Lets say that the first DOC of 0.5mm is what the insert and setup can safely handle. This amount will be applied to the Major Diameter calculated by the control and the second DOC will increase by 0.207mm, becoming progressively smaller as the Threading Operation progresses.

If the Thread Height is increased by 0.5mm and a 1.0mm DOC used as the First Pass DOC, the control will calculate a Major Diameter that is greater than actual by 0.5mm on Radius. The First Threading pass of 1.0mm will be applied to the larger Major Diameter, with 0.5mm being applied through fresh air and the remaining 0.5mm applied to the actual Major Diameter. Accordingly, the actual First Pass DOC applied is the same as the first example, where 0.5mm was specified for the First Pass DOC. The difference is that subsequent DOC will be greater than in the first example. In the case of the 1.0mm First Pass DOC and larger Major Diameter, the increase in the DOC for the second Thread Pass will be 0.414mm.

Regards,

Bill
 
Last edited:

zerok666

Plastic
Joined
Jun 8, 2019
The P value we use at work is pitch x .8. This is what is listed inside the Machinist Handbook and have not had an issue with it. The taper can be easily calculated by multiplying your total z distance move (including your start location) by .0625, also listed inside the Machinist Handbook.
 

angelw

Diamond
Joined
Sep 10, 2010
Location
Victoria Australia
That is correct

Actually, that's not correct. R used in the G76 Cycle for specifying the taper is an incremental, radial value. Total Z multiplied by 0.0625 will result in the total taper in diameter. Accordingly, the correct algorithm is:
R=Total Z x 0.0625 / 2

The OP's use of tan(1.7899) in his calculation is correct, as it equates to a radial value, but could have simplified it by substituting the constant of 0.03125 (the result of tan(1.7899)).
 
Last edited:

cgrim3

Cast Iron
Joined
Dec 4, 2020
Location
Baltimore
I appreciate everybody's help on this. We ran the job awhile ago and it turned out good. I guess from now on we will use the minimum thread height for calculation on npt threads like what Sinha said above.

Biggest thing is you have to get your tool comp right while turning the taper of the thread and the chamfer of the front of the thread before you actually start cutting the thread.

It may be just me, but I have found that there isn't a lot of good info out there about how to single point NPT threads on a cnc lathe. Just my experience but I may be wrong
 

sinha

Stainless
Joined
Sep 25, 2010
Location
india
I appreciate everybody's help on this. We ran the job awhile ago and it turned out good. I guess from now on we will use the minimum thread height for calculation on npt threads like what Sinha said above.

Biggest thing is you have to get your tool comp right while turning the taper of the thread and the chamfer of the front of the thread before you actually start cutting the thread.

It may be just me, but I have found that there isn't a lot of good info out there about how to single point NPT threads on a cnc lathe. Just my experience but I may be wrong

You are right. Systematic information on NPT thread is not readily available,
But, I think, you have given enough information, with a sample calculation. You have also given the link for a thread calculator. Good enough!
The only thing that is not clear is whether the pipe should have an initial taper turning before threading. If yes, how much?
 

cgrim3

Cast Iron
Joined
Dec 4, 2020
Location
Baltimore
You are right. Systematic information on NPT thread is not readily available,
But, I think, you have given enough information, with a sample calculation. You have also given the link for a thread calculator. Good enough!
The only thing that is not clear is whether the pipe should have an initial taper turning before threading. If yes, how much?


Yes, the part should have an initial taper before single point threading. Here is how I do it. Others may do it differently but this what we have found works:

Typically, the customer tells you how long the thread should be. For my case, the thread was .3125" long. We know for a 1/8 NPT that the major diameter of the big end of the thread is .405". We also know that the taper of the thread is 1.7899 degrees (per side). With this information, I actually model the thread in fusion 360. The front of the thread should have a chamfer on there, so I throw on a .030" 45 degree chamfer. I then write a CAM program for turning the taper in fusion 360 with the proper insert with the proper nose radius tool I will be using. I get my numbers from fusion (which accounts for nose radius) and then I manually (by hand) create a G71 and G70 turning cycle for the thread with the info from fusion. Then I proceed to single pointing the thread after the taper has been turned.

You can bypass the fusion 360 step by using g42 tool nose comp but you don't get as much control doing this IMO and the control can do weird things. Regardless, I model the thread in CAD to see what the starting OD is of the thread because adding the .030" chamfer there can make calculating that starting OD of the tapered thread tricky.

I hope this was clear and concise.

Chris
 

nissan300ztt

Hot Rolled
Joined
Jul 26, 2011
Location
Taylor
I appreciate everybody's help on this. We ran the job awhile ago and it turned out good. I guess from now on we will use the minimum thread height for calculation on npt threads like what Sinha said above.

Biggest thing is you have to get your tool comp right while turning the taper of the thread and the chamfer of the front of the thread before you actually start cutting the thread.

It may be just me, but I have found that there isn't a lot of good info out there about how to single point NPT threads on a cnc lathe. Just my experience but I may be wrong

youre correct or even proper dimensions for npt threads. its almost scary that here I am in 2022 and still nothing. or cnc machines dont come pre programmed with certain thread cycles in them.
 








 
Top