Thread depth using 60 degree

[benfica]

Hello,

I am in the need to cut live threads in wood. I have read so many things about correct depth calculations and I needed to know what is the correct approach and calculations.
Heads up! I am terrible in math but I can use a calculator
Please try to explain really clear so I can put it in practice. Any other advice is much appreciated.
I have a router mounted on my BXA tool post with a 60 degree cutter and I am cutting V threads in wood (I made a video that showed to a friend how I did it).

The formulas I was given and saw on line were the following:

This link:
UN imperial screw thread calculator

.650/tpi = thread depth (I feel that this depth is not enough)

1/tpi = 0.xxxxxx
0.xxxxxx x .866 = thread depth (closer to where I need to be I think)

So what is true and what is not? I feel that this formula is closer to where I need to be. Thoughts?

 

[706jim]

Thread depth for a sharp V thread form is 0.866P

For American National 0.6495P

I'm guessing your router bit has a sharp point.

If so D = 0.866P

Hope this helps.

 

[benfica]

Thread depth for a sharp V thread form is 0.866P

For American National 0.6495P

I'm guessing your router bit has a sharp point.

If so D = 0.866P

Hope this helps.

Every little bit helps Jim.

Thanks a bunch.

 

[Bobw]

Nominal thread diameter minus pitch diameter.

Of course if you have a rad on the end of your tool, you'll
need to go a little deeper. Cut it once, measure the PD, adjust,
and cut again.

 

[benfica]

Nominal thread diameter minus pitch diameter.

Bob,

Would you be able to give me an example?
Lets say the screw is 1/2" and I want 13tpi, what is the calculation formula?

 

[Bobw]

Bob,

Would you be able to give me an example?
Lets say the screw is 1/2" and I want 13tpi, what is the calculation formula?

1/2-13 Pitch Diameter .4485-.4435.. Averages to .446".

So. .500 - .446 = .054 thread depth..

On my threading cycle, even though I may have turned it to .495, I will still use .500"
to keep everything simple and consistent. You could use .495, but then your
thread depth changes, and now you are doing more math and creating confusion.

KISS principal.

If you are running a big nose rad on your tool, like with a J thread, obviously,
you have to go a little deeper.. But Major minus PD gets you really close if not
dead on first shot.

 

[G00 Proto]

1/2-13 Pitch Diameter .4485-.4435.. Averages to .446".

So. .500 - .446 = .054 thread depth..

On my threading cycle, even though I may have turned it to .495, I will still use .500"
to keep everything simple and consistent. You could use .495, but then your
thread depth changes, and now you are doing more math and creating confusion.

KISS principal.

If you are running a big nose rad on your tool, like with a J thread, obviously,
you have to go a little deeper.. But Major minus PD gets you really close if not
dead on first shot.

Since I don’t do much lathe work, I have some gaps in my knowledge base. I always use (major diameter-minor diameter)/2…. am I wrong or just two ways to skin a cat?


Sent from my iPhone using Tapatalk

 

[angelw]

Since I don’t do much lathe work, I have some gaps in my knowledge base. I always use (major diameter-minor diameter)/2…. am I wrong or just two ways to skin a cat?

Just another way.

The calculation listed in the OP's opening Post (.650/tpi), for all intensive purposes, nets the same result as Bob's, but without first needing to know the Pitch Diameter. The PD is the most important dimension of a Thread, in my opinion, but it depends on the method of measuring the Thread as to whether the PD is required to make the part. If measuring the Thread using 3 wires, or a Thread Micrometer, then for sure the PD is required. If using a mating part, or a GO/NO GO gauge, then not so important.


Regards,

Bill

 

[michiganbuck]

Here is an old pdf on straight in
https://www.mitsubishicarbide.com/a...1/5783/tec_threading_depth_external_en-us.pdf

Many references suggest P x .64952(650) and p x .866. (@30) and x .125 X for the nose flat.


But it is ballpark because the starting point must include any run out you have in the part and the size of your nose flat..

I used to tickle a few short turnings and when my turn evidence was half round the part, I would set my zero...then when a few thousandths still to go I would check my thread size.

The ops setup likely has a little whip in the treadmill so that should be considered perhaps .005 or so away.

I Have a decent straight in, and at 30* chart that I made, guess I should publish it and sell it on eBay for $2.. each.

 

[michiganbuck]

Here is an interesting thread depth video

I haven't checked it out yet but will gt back to it

About Thread Depth - YouTube

 

[sinha]

The use of the term "minor diameter" can be confusing.
Core diameter for external threads, and bore diameter for internal threads, are better terms.

 

[sinha]

For metric (60 deg) threads,
Depth of thread = 0.61344 x Pitch of thread
Core diameter = OD - (2 x Depth of thread)
Bore diameter = OD - Pitch of thread
Root diameter = Bore diameter + (2 x Depth of thread)

 

[Screwmachine]

Threads are measured on the thread flanks for a reason. All threads have some sort of truncation of the crest and root, even if "sharp" on both, how sharp is sharp?

 

[G00 Proto]

Okay, I’ll use an example…. I frequently program threads either with a thread mill on the mill or single point on the lathe. One of my cam systems uses the minor diameter for external threads and the major diameter for internal threads. The other system requests a thread depth. It doesn’t matter which system I use, and whether it is single point or thread mill… I always end up doing an X (lathe) or cutter comp (mill) offset. It’s always metal safe, and I do it often enough that I can usually guess what it’s going to be… so where is my error? Root flat, deflection, math, general incompetence…

I don’t really lose any sleep about it, since it’s always metal safe, but now I’m curious.


Sent from my iPhone using Tapatalk

 

[angelw]

Okay, I’ll use an example…. I frequently program threads either with a thread mill on the mill or single point on the lathe. One of my cam systems uses the minor diameter for external threads and the major diameter for internal threads. The other system requests a thread depth. It doesn’t matter which system I use, and whether it is single point or thread mill… I always end up doing an X (lathe) or cutter comp (mill) offset. It’s always metal safe, and I do it often enough that I can usually guess what it’s going to be… so where is my error? Root flat, deflection, math, general incompetence…

I don’t really lose any sleep about it, since it’s always metal safe, but now I’m curious.


Sent from my iPhone using Tapatalk

Hello G00 Proto,
If its a generic cutter, whether its a single point threading tool for a lathe, or thread mill, that typically has a very small radius at the point, smaller than the Thread Form radius or flat at the root, then it will always cut metal safe; the tool needs to cut deeper so that the Pitch Diameter is correct.

Regards,

Bill

 

[michiganbuck]

With a tool bit or thread mill too pointy and with touching the part OD and traveling the correct amount straight or at 29/30 the thread is likely to be too tight, having point nose flat too big and the thread will be loose (sloppy), even though the travel feed amount and major and minor diameters are correct.

A thread micrometer or a 3 wires check may tell the thread is correct at the flanks(V) but if the tool bit/insert nose flat is too big the external (male) thread will/may bind a nut at the root and not work (not be to spec.).

The very least check is trying a known good nut on a male thread..that won't make it to thread spec but at least one will know that it will go.

If a thread micrometer is too pointy and bottoms out at the root it may not give a correct inspection of the thread.

 

[TheBigLebowski]

I wrote a routine to figure out the correct depths for OD UN(C/F) threads a while back, this is what came up with. If I recall correctly this calculates the depth for a "Perfect" thread - In reality you will need to go a little bit deeper depending on what class of thread you want.

This calculates the Theoretical thread height. If you touch off the od and cut this deep you will create scrap - OD Threads dont have sharp crests!
(setq THX_H (* THREAD_PITCH 0.866025404)) ;VV height - theoretical Height for a given pitch at 60 degrees

To calculate the correct depth based on the Theorectical major diameter
If the tool has a nose radius...
(setq THX_H_DEPTH (- (* THX_H 0.875) TNR))
;if the tool has a TNR and is touched off the OD - its closer to its final depth than a sharp tool - this
movement is 1:1 on a 60 angle
Otherwise for a tool with just a sharp point..
(setq THX_H_DEPTH (* THX_H 0.875)


So lets say you are cutting 1/2-13 threads
Theoretical major diameter is 0.500
pitch is 0.07692
Theoretical thread height is 0.066617 but...
if touching off the od with a sharp tool you would cut 0.05829 Deep
If your tool had a nose radius you subtract it from that value
so if it has a 0.002" nose radius - you would cut 0.05629 deep instead.


EDIT....

This picture helps explain more clearly

 

[706jim]

FWIW the published three wire measurement formula will give you the value for the top limit of a class 3A thread pitch diameter.

To use this method to make anything but a class 3A thread will then require adjusting the value for "M" slightly downwards to compensate for the smaller pitch diameters of class 1 and 2 threads.

For anyone wishing to experiment with this method or perhaps check "M" with existing threads, consider using number drills in place of the less common precision wire sets.

 

[G00 Proto]

The longer I’m in this industry (~25 years) the more I realize how little I know

Self -acknowledged gaps:
-a true understanding of threads and thread specs.
-heat treating
-cutter geometry
-women


Sent from my iPhone using Tapatalk

 

[Vancbiker]

3 of those 4 can be figured out.