What's new
What's new

Programming a bore for NPT internal thread

tonepaq

Plastic
Joined
Nov 3, 2022
I am trying to program a part on my lathe for an internal 1 1/2- 11.5 NPTF. I want to use an insert drill, then bore the tapered hole and then use a single point threader. How do I calculate the start point of the large side of the bored hole? I understand the angle is 1degree 47min. so once I find the finished bore size at the front of part I can just taper it down. I tried to study in the machinist handbook, but got rather confused.

Thank you for any help.
 
Use the E0 dimension and either add (OD) or subtract (ID) thread height twice for start points on pipe threads. I usually need to adjust +/- .005-.010" but that at least gets me in the ballpark. Adjust until the crests look appropriate.
 
Use the E0 dimension and either add (OD) or subtract (ID) thread height twice for start points on pipe threads. I usually need to adjust +/- .005-.010" but that at least gets me in the ballpark. Adjust until the crests look appropriate.
I do the same but adjust to leave the minimum stock while confirming the full profile insert tops the threads to ensure proper crest truncation.
 
Machinery's Handbook is your friend.
But its really not. Almost all NPT threads are theoretical dimensions. If someone made a chart of where to start the thread and where it should end as in start X and start Z to End X and End Z would be the most helpful thing I can imagine. Because the G76 cycle isnt perfect and leaves a lot to be desired. Thats just my $.02
 
But its really not. Almost all NPT threads are theoretical dimensions. If someone made a chart of where to start the thread and where it should end as in start X and start Z to End X and End Z would be the most helpful thing I can imagine. Because the G76 cycle isnt perfect and leaves a lot to be desired. Thats just my $.02
I layout the threads in Mastercam using data given in the Machinery's Handbook. Offset the line (pitch is given, if I remember correctly) in both directions half of thread height. Bore is one line, thread major diameter is the other. Draw two vertical lines based on the threading depth I want. Create circle tangent to 3 lines. Analyze. Use that value for my G76. Works okay for me. Close enough for a small offset to get on size if needed.

Haven't done it, but you could layout each pipe size at a known depth and store the values in a file. Then for different thread depths, it would be a simple math problem to figure different X-values and R-values.

I should probably do that myself as it would be quicker than bringing up the correct pipe size (already saved in MasterCam), analyzing and doing the math or drawing two more vertical lines and another circle at the new depth needed. Thanks for the idea. :)
 
I layout the threads in Mastercam using data given in the Machinery's Handbook. Offset the line (pitch is given, if I remember correctly) in both directions half of thread height. Bore is one line, thread major diameter is the other. Draw two vertical lines based on the threading depth I want. Create circle tangent to 3 lines. Analyze. Use that value for my G76. Works okay for me. Close enough for a small offset to get on size if needed.

Haven't done it, but you could layout each pipe size at a known depth and store the values in a file. Then for different thread depths, it would be a simple math problem to figure different X-values and R-values.

I should probably do that myself as it would be quicker than bringing up the correct pipe size (already saved in MasterCam), analyzing and doing the math or drawing two more vertical lines and another circle at the new depth needed. Thanks for the idea. :)
Unfortunately the shop I work for is too cheap to get me mastercam. Im using a program that doesnt write G76 code for me. Its all me and the machinist handbook. I get the parts to work. But sometimes its a lot of trial and error. once I nail it I save the program in the control and 8 or 9 back up locations. LOL. I have on my personal PC over 10,000 programs ive written for 5 different machines, because I dont want to rewrite them. LOL.
 
MasterCam is expensive. Maybe you could do some research and find a low cost CAD-CAM that your company would be willing to spring for.

I've been programming lathes since May, 1985. In 2008 I was told I had to do all my programming in MasterCam so anyone replacing me would simply need to select a different post processor to put out a program for a different lathe than whatever lathe the original program was made for. We have 26 lathes of various makes. Had 30 a few years ago.

We had MasterCam long before that (2008), but I seldom used it to make a complete program. I sometimes used MasterCam to save me time figuring endpoints, but manually wrote the programs.

I hope you have some Macro B programs written for such things as barfeeding, cut off, transferring from main spindle to sub, deep drilling, etc. that will allow you to cut-and-paste...make a few value data changes if required...to save yourself a lot of work.

As for pipe threads, you could PM me what you need and I will lay it out in MC and give you the results. The only problem is that I would have to reset my password as I don't remember it, and can only logon from home. Therefore I wouldn't see your PM until at home. I know it isn't hard, but just haven't had the desire to reset my password. What can I say? I'm 74 and you have to expect some eccentricities. :)
 
We do a lot of NPT threads at work (internal and external). I'll take a look at the code for the finish pass for that size thread tomorrow at work.

We check our threads with the thread gage and the 3-step gage to make sure the crest is correct so our numbers will get you very close.
 
I am trying to program a part on my lathe for an internal 1 1/2- 11.5 NPTF. I want to use an insert drill, then bore the tapered hole and then use a single point threader. How do I calculate the start point of the large side of the bored hole? I understand the angle is 1degree 47min. so once I find the finished bore size at the front of part I can just taper it down. I tried to study in the machinist handbook, but got rather confused.

Thank you for any help.
Here is my boring code for 1-1/2 NPT internal:

X1.1Z.03
G85 NBOR1 D.24 U.1 W.005
NBOR1 G81
X1.93 Z.03
G1G41Z0.F.009
X1.76Z-.1
X1.711Z-.88
X1.667Z-.98
X1.276Z-1.185
X1.265Z-1.25
G40X1.15
G80

and the thread line is:
X1.55Z.5
G71Z-.78F.08696I-.0373D.026H.16U.003M32M73
G80
G0G97S300X20.Z20.M5M9

Note:
This is for an Okuma P300L control, but the basic numbers should be good for any control. On the boring pass, there a little blending at the end, but the important stuff ends at Z-.98.
Also, this is for a 6-Step, sharp V thread, between B and BT. If you are allowed to truncate the crest a bit, add .02 to the X’s.

Hope this helps.
Drake
 
Here is my boring code for 1-1/2 NPT internal:

X1.1Z.03
G85 NBOR1 D.24 U.1 W.005
NBOR1 G81
X1.93 Z.03
G1G41Z0.F.009
X1.76Z-.1
X1.711Z-.88
X1.667Z-.98
X1.276Z-1.185
X1.265Z-1.25
G40X1.15
G80

and the thread line is:
X1.55Z.5
G71Z-.78F.08696I-.0373D.026H.16U.003M32M73
G80
G0G97S300X20.Z20.M5M9

Note:
This is for an Okuma P300L control, but the basic numbers should be good for any control. On the boring pass, there a little blending at the end, but the important stuff ends at Z-.98.
Also, this is for a 6-Step, sharp V thread, between B and BT. If you are allowed to truncate the crest a bit, add .02 to the X’s.

Hope this helps.
Drake
Thank you for this. I wrote some code, have not ran it yet. Waiting for my inserts to arrive, I ordered some NTPF full profile for 11.5 lead
Here it is, comments welcome

(FINISH BORE)
N8 T0808
(1.0 BAR R.0156)
G54
M8
G99
G0 X1.8322 Z0.1
G50 S2500
G96 S656 M3
G1 Z0. F.01
X1.751 Z-0.0394 F.006
X1.7108 Z-0.6862
X1.703
Z-1.135
X1.543
G0 X1.36
Z0.1
M01

(THREAD)
(NTPF 1-1/2 11.5)
N1 T0101
G54
M8
G99
G97 S500 M3
G0 X1.5 Z0.1825
G92 X1.7729 Z-0.9419 R0.0351 F0.0869
X1.7816
X1.7903
X1.799
X1.8077
X1.8164
X1.8251
X1.8338
X1.8338
G0 X1.5 Z1.0
M9
G28 U0. W0.
M30
 
Last edited:
Just be aware that the X and I on an Okuma are based on being programmed at the front (X1.55Z.5 in the above Okuma example) while on a Fanuc it is at the rear. Therefore the I-value will be plus on a Fanuc and the X-value smaller for an internal pipe thread versus an Okuma.

X1.4703Z-.78 on a Fanuc based on vandytech's example. And I.0399 over 1.28 inches distance although I've had to fudge my I-value more than once to get the gauges to fit correctly.
 
MasterCam is expensive. Maybe you could do some research and find a low cost CAD-CAM that your company would be willing to spring for.

I've been programming lathes since May, 1985. In 2008 I was told I had to do all my programming in MasterCam so anyone replacing me would simply need to select a different post processor to put out a program for a different lathe than whatever lathe the original program was made for. We have 26 lathes of various makes. Had 30 a few years ago.

We had MasterCam long before that (2008), but I seldom used it to make a complete program. I sometimes used MasterCam to save me time figuring endpoints, but manually wrote the programs.

I hope you have some Macro B programs written for such things as barfeeding, cut off, transferring from main spindle to sub, deep drilling, etc. that will allow you to cut-and-paste...make a few value data changes if required...to save yourself a lot of work.

As for pipe threads, you could PM me what you need and I will lay it out in MC and give you the results. The only problem is that I would have to reset my password as I don't remember it, and can only logon from home. Therefore I wouldn't see your PM until at home. I know it isn't hard, but just haven't had the desire to reset my password. What can I say? I'm 74 and you have to expect some eccentricities. :)
I use ShopCAM for most CNC Lathe programs. And just hand write the threading cycles. We have BobCAD which is fine but my boss wont spring for another seat. Our owner is old and doesnt believe in fixing or upgrading stuff until it is absolutely necessary to do. Which is currently where I am at with our one machine. And I showed both my boss and super visor what the machine does and theyre like well..............turn the spindle up. Like thats not the answer.
 
Just be aware that the X and I on an Okuma are based on being programmed at the front (X1.55Z.5 in the above Okuma example) while on a Fanuc it is at the rear. Therefore the I-value will be plus on a Fanuc and the X-value smaller for an internal pipe thread versus an Okuma.

X1.4703Z-.78 on a Fanuc based on vandytech's example. And I.0399 over 1.28 inches distance although I've had to fudge my I-value more than once to get the gauges to fit correctly.
Here is my boring code for 1-1/2 NPT internal:

X1.1Z.03
G85 NBOR1 D.24 U.1 W.005
NBOR1 G81
X1.93 Z.03
G1G41Z0.F.009
X1.76Z-.1
X1.711Z-.88
X1.667Z-.98
X1.276Z-1.185
X1.265Z-1.25
G40X1.15
G80

and the thread line is:
X1.55Z.5
G71Z-.78F.08696I-.0373D.026H.16U.003M32M73
G80
G0G97S300X20.Z20.M5M9

Note:
This is for an Okuma P300L control, but the basic numbers should be good for any control. On the boring pass, there a little blending at the end, but the important stuff ends at Z-.98.
Also, this is for a 6-Step, sharp V thread, between B and BT. If you are allowed to truncate the crest a bit, add .02 to the X’s.

Hope this helps.
Drake
Correction to the thread line…

G71 X1.847Z-.78F.08696B60 I-.0373D.026H.16U.003M32M73

I missed the X dia.
 
I use .016 for 1/64R and .031 for 1/32R. No G41/G42. Two websites gave 1-23/32 inch for drill size. Four websites gave 1-47/64 inch drill size. I drew the 1-1/2 NPT per Machinery's Handbook. Below are finish bore passes for both drill sizes and for both 1/64R and 1/32R inserts.

The G76 cycle for a Fanuc control is at the end. I measured the radius of a 16ER 11.5NPT insert to layout the end point. Unusual that the X-value came out at an even thousandth.

T0202G97S965M3 (FINISH BORE .016R)
X1.98Z.5M8
G50S2500
G96S500
Z.03
G1X1.948Z.01F.02
Z0F.005
G2X1.9183Z-.0061R.021F.002
G1X1.7479Z-.0914F.003
X1.7344Z-.3083F.004
Z-?
X1.7F.01

T0202G97S950M3 (FINISH BORE .031R)
X2.01Z.5M8
G50S2500
G96S500
Z.03
G1X1.978Z.01F.02
Z0F.005
G2X1.9271Z-.0105R.036F.002
G1X1.7483Z-.1F.004
X1.7344Z-.3231F.006
Z-?
X1.7F.01

T0202G97S965M3 (FINISH BORE .016R)
X1.98Z.5M8
G50S2500
G96S500
Z.03
G1X1.948Z.01F.02
Z0F.005
G2X1.9183Z-.0061R.021F.002
G1X1.7479Z-.0914F.003
X1.719Z-.5557F.004
Z-?
X1.68F.01


T0202G97S950M3 (FINISH BORE .031R)
X2.01Z.5M8
G50S2500
G96S500
Z.03
G1X1.978Z.01F.02
Z0F.005
G2X1.9271Z-.0105R.036F.002
G1X1.7483Z-.1F.004
X1.719Z-.5704F.006
Z-?
X1.68F.01

Thread cycle

X1.68Z.5
G76P000129Q30R.002
G76X1.851Z-.78P696Q120R.0399F.08696
 
Last edited:








 
Back
Top