[30tooo]

Would someone be kind enough to furnish me with the G76 coding to produce 1/2" British standard taper pipe thread please . I can produce a parallel thread using 2 line G76 coding but i do not understand how to do taper threading with this format . Thank you .

[fordav11]

G00 X0.600 Z0.2
G76 X... Z... I... K... D... F... A...

X and Z = end point of the thread
I = taper in X
K = depth of thread (see thread specification drawings)
D = depth of cut (typically ~ 0.005" to 0.010")
F = pitch. (you need the TPI). If thread is 4 TPI pitch = 0.250")
A = thread angle so A = 55

You can get most of the other values from a thread hand book or similar.
If no one else adds the numbers I'll look them up myself in a few hours.

[30tooo]

That looks good thank you . I have never used a single line g76 code before . Even so , it would still be nice to have the "actual" numbers for this particular thread . The control is an OT being used on an Akebono lathe . It is all set up in metric as well . It's the start position and taper values I do not understand .
My fanuc book is not at all to helpful at explaining things in a basic enough fashion .

Thanks for the response .

[fordav11]

ok here's the answer with all the numbers. Tapered threads are not so simple. A thread chart will only give you the OD and TPI and taper per foot or whatever length the engineer pulled out of his ass that day. You need to do some work to get all of the numbers.

1/2" BSPT
Specification says 14TPI = 1/14 = 0.0714" pitch (i.e. Feed Rate)
Specification says BSPT thread depth = 0.64 x pitch. Thread depth = 0.0457
Specification says 1/2" BSPT major diameter (i.e. OD) = 0.825".
Specification says BSPT taper ratio = 1:16. That means 1" taper in X (on diameter) for every 16 inches along in Z. For our trig we use 0.5 for the X taper since we must do the calcs on radius.
0.5 / 16 = 0.03125
Arctan 0.03125 = 1.7899 degrees decimal for the taper.

This example will cut to Z-1.0 but our cutting length is 1.200" because we are starting 0.200" in front of the part.

If you want more or less in Z you will need to re-calculate I.
I is minus for OD threads and positive for ID threads.

To calculate I, the taper is 1.7899 degrees so
I = tan 1.7899 x 1.2 (thread cutting length) x2 (to give a diameter value)
= 0.03125 x 1.2 x 2
= 0.0750"

To calculate X simply take the major diameter and subtract 2x thread depth.
0.825 - (2x 0.0457) = 0.7336

If your control needs 1 line for G76 then use this one...


G00 X1.00 Z0.2
G76 X0.7336 Z-1.0 I-0.075 K0.0457 D0.010 F0.0174 A55


If your control needs 2 lines for G76 then use this one...


G00 X1.00 Z0.2
G76 P030055 Q100 R0.002
G76 X0.7336 Z-1.0 R-0.075 P457 Q100 F0.0174


On the 1st line P = number of finish passes (first 2 digits), threading chamfer amount (second 2 digits) and thread angle (third 2 digits)
Q = depth of roughing cuts (no decimal point allowed)
R = finishing allowance

On the 2nd line P = Depth of Thread and Q = Depth of first cut (no decimal point allowed for P or Q)
R = Taper amount in X. I don't remember if the sign is relevant. I don't have a series 16/18/21 manual handy to check it. I never use the 2 line method because I set all of the machines we have to 1 line by setting parameter 0001 bit 1 (FCV) to 1 so it uses just one line :-D
You can check it on the machine. Run the thread above the part (offset +1.0") and see which way the X axis moves. If it moves the wrong way remove the minus sign.

All sizes are in inches but you can convert the numbers to metric and it will work fine.

NOTE! All of the specification info was found on the internet by searching but ideally you should get this info from the Machinery Handbook or similar official source.

The standard disclaimer applies. Please remember that YOU are in control of YOUR machine and YOUR programs.
I advise you to do your own research and verify this is correct before cutting your threads.

All of my tapered threading experience is with API, IF, BECO, Metzke, Remet and other pain in the ass proprietary mining type threads that have proper drawings with toleranced stand-offs and precision ground guages. I've never actually cut any rough tapered thread like a BSPT thread on a CNC lathe. However I guarantee my theory is 100% correct but the numbers above I offer no guarantee on

[30tooo]

Well !

That is what I call a complete and fantastic reply . I'm sorry I have not got back sooner , but either way I am very grateful for the immense amount of effort you have put in . Superb .

Thank you .

[damapasco]

dear sir
its very useful
but i dont know where you have take the first number and can you tell me the compelete formula please ?
see betwin red stars please
best regards

ok here's the answer with all the numbers. Tapered threads are not so simple. A thread chart will only give you the OD and TPI and taper per foot or whatever length the engineer pulled out of his ass that day. You need to do some work to get all of the numbers.

*********1/2" BSPT
Specification says 14TPI = 1/14 = 0.0714" pitch (i.e. Feed Rate)
Specification says BSPT thread depth = 0.64 x pitch. Thread depth = 0.0457
Specification says 1/2" BSPT major diameter (i.e. OD) = 0.825".
Specification says BSPT taper ratio = 1:16. That means 1" taper in X (on diameter) for every 16 inches along in Z. For our trig we use 0.5 for the X taper since we must do the calcs on radius.
0.5 / 16 = 0.03125
Arctan 0.03125 = 1.7899 degrees decimal for the taper.

This example will cut to Z-1.0 but our cutting length is 1.200" because we are starting 0.200" in front of the part.

If you want more or less in Z you will need to re-calculate I.
I is minus for OD threads and positive for ID threads.

To calculate I, the taper is 1.7899 degrees so
I = tan 1.7899 x 1.2 (thread cutting length) x2 (to give a diameter value)
= 0.03125 x 1.2 x 2
= 0.0750"

To calculate X simply take the major diameter and subtract 2x thread depth.
0.825 - (2x 0.0457) = 0.7336**************

If your control needs 1 line for G76 then use this one...


G00 X1.00 Z0.2
G76 X0.7336 Z-1.0 I-0.075 K0.0457 D0.010 F0.0174 A55


If your control needs 2 lines for G76 then use this one...


G00 X1.00 Z0.2
G76 P030055 Q100 R0.002
G76 X0.7336 Z-1.0 R-0.075 P457 Q100 F0.0174


On the 1st line P = number of finish passes (first 2 digits), threading chamfer amount (second 2 digits) and thread angle (third 2 digits)
Q = depth of roughing cuts (no decimal point allowed)
R = finishing allowance

On the 2nd line P = Depth of Thread and Q = Depth of first cut (no decimal point allowed for P or Q)
R = Taper amount in X. I don't remember if the sign is relevant. I don't have a series 16/18/21 manual handy to check it. I never use the 2 line method because I set all of the machines we have to 1 line by setting parameter 0001 bit 1 (FCV) to 1 so it uses just one line :-D
You can check it on the machine. Run the thread above the part (offset +1.0") and see which way the X axis moves. If it moves the wrong way remove the minus sign.

All sizes are in inches but you can convert the numbers to metric and it will work fine.

NOTE! All of the specification info was found on the internet by searching but ideally you should get this info from the Machinery Handbook or similar official source.

The standard disclaimer applies. Please remember that YOU are in control of YOUR machine and YOUR programs.
I advise you to do your own research and verify this is correct before cutting your threads.

All of my tapered threading experience is with API, IF, BECO, Metzke, Remet and other pain in the ass proprietary mining type threads that have proper drawings with toleranced stand-offs and precision ground guages. I've never actually cut any rough tapered thread like a BSPT thread on a CNC lathe. However I guarantee my theory is 100% correct but the numbers above I offer no guarantee on

[damapasco]

dear sir
would you please more explain about the follow numbers :

((((1/2" BSPT
Specification says 14TPI = 1/14 = 0.0714" pitch (i.e. Feed Rate)
Specification says BSPT thread depth = 0.64 x pitch. Thread depth = 0.0457
Specification says 1/2" BSPT major diameter (i.e. OD) = 0.825".
Specification says BSPT taper ratio = 1:16. That means 1" taper in X (on diameter) for every 16 inches along in Z. For our trig we use 0.5 for the X taper since we must do the calcs on radius.
0.5 / 16 = 0.03125
Arctan 0.03125 = 1.7899 degrees decimal for the taper.

This example will cut to Z-1.0 but our cutting length is 1.200" because we are starting 0.200" in front of the part.

If you want more or less in Z you will need to re-calculate I.
I is minus for OD threads and positive for ID threads.

To calculate I, the taper is 1.7899 degrees so
I = tan 1.7899 x 1.2 (thread cutting length) x2 (to give a diameter value)
= 0.03125 x 1.2 x 2
= 0.0750"

To calculate X simply take the major diameter and subtract 2x thread depth.
0.825 - (2x 0.0457) = 0.7336

If your control needs 1 line for G76 then use this one...)))))))))

ok here's the answer with all the numbers. Tapered threads are not so simple. A thread chart will only give you the OD and TPI and taper per foot or whatever length the engineer pulled out of his ass that day. You need to do some work to get all of the numbers.

1/2" BSPT
Specification says 14TPI = 1/14 = 0.0714" pitch (i.e. Feed Rate)
Specification says BSPT thread depth = 0.64 x pitch. Thread depth = 0.0457
Specification says 1/2" BSPT major diameter (i.e. OD) = 0.825".
Specification says BSPT taper ratio = 1:16. That means 1" taper in X (on diameter) for every 16 inches along in Z. For our trig we use 0.5 for the X taper since we must do the calcs on radius.
0.5 / 16 = 0.03125
Arctan 0.03125 = 1.7899 degrees decimal for the taper.

This example will cut to Z-1.0 but our cutting length is 1.200" because we are starting 0.200" in front of the part.

If you want more or less in Z you will need to re-calculate I.
I is minus for OD threads and positive for ID threads.

To calculate I, the taper is 1.7899 degrees so
I = tan 1.7899 x 1.2 (thread cutting length) x2 (to give a diameter value)
= 0.03125 x 1.2 x 2
= 0.0750"

To calculate X simply take the major diameter and subtract 2x thread depth.
0.825 - (2x 0.0457) = 0.7336

If your control needs 1 line for G76 then use this one...


G00 X1.00 Z0.2
G76 X0.7336 Z-1.0 I-0.075 K0.0457 D0.010 F0.0174 A55


If your control needs 2 lines for G76 then use this one...


G00 X1.00 Z0.2
G76 P030055 Q100 R0.002
G76 X0.7336 Z-1.0 R-0.075 P457 Q100 F0.0174


On the 1st line P = number of finish passes (first 2 digits), threading chamfer amount (second 2 digits) and thread angle (third 2 digits)
Q = depth of roughing cuts (no decimal point allowed)
R = finishing allowance

On the 2nd line P = Depth of Thread and Q = Depth of first cut (no decimal point allowed for P or Q)
R = Taper amount in X. I don't remember if the sign is relevant. I don't have a series 16/18/21 manual handy to check it. I never use the 2 line method because I set all of the machines we have to 1 line by setting parameter 0001 bit 1 (FCV) to 1 so it uses just one line :-D
You can check it on the machine. Run the thread above the part (offset +1.0") and see which way the X axis moves. If it moves the wrong way remove the minus sign.

All sizes are in inches but you can convert the numbers to metric and it will work fine.

NOTE! All of the specification info was found on the internet by searching but ideally you should get this info from the Machinery Handbook or similar official source.

The standard disclaimer applies. Please remember that YOU are in control of YOUR machine and YOUR programs.
I advise you to do your own research and verify this is correct before cutting your threads.

All of my tapered threading experience is with API, IF, BECO, Metzke, Remet and other pain in the ass proprietary mining type threads that have proper drawings with toleranced stand-offs and precision ground guages. I've never actually cut any rough tapered thread like a BSPT thread on a CNC lathe. However I guarantee my theory is 100% correct but the numbers above I offer no guarantee on

[sinha_nsit]

Refer to some handbook for thread dimensions.
For tapered pipe threads (NPT or BSPT), take R = L/32 in the second block of G76. L is the total axial travel of the tool.
For external threads, R would be negative if machining is being done towards the chuck (right-to-left).
If you ask specific questions, you would get better answers. Reading the Fanuc manual or some book would be helpful.