What's new
What's new

# Thread depth using 60 degree

#### benfica

##### Plastic
And I thought that I was asking a simple question...
I was just looking to get a somewhat simple answer without too much technical terms because I AM NOT a machinist but I do have a metal lathe that I use for my hobby.
Simple wording so I can put into practice.
What is the correct formula then? Does the tenon diameter makes a different in order to calculate the thread depth?

#### angelw

##### Diamond
And I thought that I was asking a simple question...
I was just looking to get a somewhat simple answer without too much technical terms because I AM NOT a machinist but I do have a metal lathe that I use for my hobby.
Simple wording so I can put into practice.
What is the correct formula then? Does the tenon diameter makes a different in order to calculate the thread depth?

Hello benifacta,

Not really. The most important diameter is the Pitch Diameter, a theoretical diameter circa halfway between the Major and Minor Diameter. Its this diameter that results in the ultimate fit of the Thread. For a male thread, both the Major and Minor diameter can be smaller than specified and that will just result in more clearance at the root and crest of the Thread Form (the reduction of the minor diameter is limited by the actual form of the Threading Tool and its nose radius}. Two common methods applied at the shop floor for measuring the Pitch Diameter is via three, best fit wires, or with a Thread Micrometer. If the Thread is measured and found to have the correct Pitch Diameter, a cut could be made to reduce the OD of the Thread (what you referred to as tenon diameter) and it will have no affect on the Pitch Diameter and fit of the Thread.

When calculating the Thread Depth, you should always use the standard Major Diameter in your calculations. If the OD is then machined smaller than the standard calls for, it will have no affect on the fit of the thread.

Regards,

Bill

Last edited:

#### G00 Proto

##### Hot Rolled
And I thought that I was asking a simple question...
I was just looking to get a somewhat simple answer without too much technical terms because I AM NOT a machinist but I do have a metal lathe that I use for my hobby.
Simple wording so I can put into practice.
What is the correct formula then? Does the tenon diameter makes a different in order to calculate the thread depth?

The other thing is, we always (???) check our cut threads and sneak up on them. In other words, if I’m cutting external threads like you are, I’ll determine the thread depth by looking up the major and minor diameters in my Machinist Handbook (or Google). Then I’ll run my program and check my threads… thread mic, three wire method, or a ring gage. 99% of the time I’ll need to make an offset because my calculation method yields a metal safe result. This new offset or empirically determined thread depth will stay consistent for the entire production run. It is (largely) independent of the actual measured tenon diameter on your part.

I would just take a reasonable number based on the “book” major and minor. Make a cut then measure or test fit. Then I’d dial in more until I got the fit I wanted. Write down that empirical number and use it as your “thread depth”.

Besides it’s wood… you give me two pieces of metal I can make something amazing. Give me two pieces of wood and I can make you a fire

Sent from my iPhone using Tapatalk

#### michiganbuck

##### Diamond
For a straight-in feed A number easy to remember is likely the best choice so .60 and .65 Could be the numbers.
For a 13 thread...Pitch (1 divided by TIP) times .60 and then .65
1/13 = .076923 x .60=.04651, then x .65=.04999. so your infeed will/should be roughly between those numbers.

You use a between amount because your cutter nose flat, the part run out, the forces on the cutter, the cutter run out, and the part deflection will change the exact amount you need to in feed at straight-in to get a correct thread. Checking for a hobby guy might be trying a nut that you checked out to be close enough to the class thread you want.
Once you get a good part you can run a series at the same feed number until your cutter gets dull and so begins to change.

Another way might be to look at a tap drill chart to see the difference between the screw diameter and the tap-drill size.
REF" for 1/2 -13 thread .500 minus .407 = .093 / 2 = about .0465.

All of the sizes are important
The major diameter can't be too big or the nut won't go, too small and it will go but is poor looking and does not give a good reference to measure your in-feed amount from.
The correct pitch, thread per inch is important or you will be making a scrap part.
The infeed of straight or 29/30* direction is important so to choose the correct infeed numbers.
How far to feed in is important because the nut may bind at the flanks (V) or at the root(bottom).
The tool bit/insert nose flat/radius is important because the correct infeed numbers will make a binding, or loose fit thread if the nose flat/radius is wrong, or not considered when figuring out numbers.
The root diameter is important because the fit will bind with the minor diameter being too big.

* Back in the 60s we had to longhand our numbers with not having calculators.
or look at a fish gauge and add our nose flat.
A thread fish might give 100 for a 13 thread so one might divide by 2 for .050 and take away the nose flat for a try.

#### michiganbuck

##### Diamond
Good to know that there are two kinds of fish gauges
Sterrett type is Straight in with showing.108 for a 12 TPI
and Lufkin is at 30* with showing .144 for a 12 TPI.
Giving double depth with a sharp point bit\insert.

Good also to note that some thread cutting inserts have a range of threads so the point flat/radius varies..with that the thread calculators or figuring thread feed numbers may show a little error to actual need.

An 8top has about.015 flat and a 30tpi has about a.004 flat.

#### michiganbuck

##### Diamond
Another important thing is the touch-off place to begin your infeed. If you turn a part to .500 for your 1/2-13 thread your touch-off place will be OK, at .500.

If you put a piece of 1/2 stock in a chuck or other holding device your touch-off place must consider the part run out. With .005 run out you may need to add that .005 to your feed calculation.

I used to skim a part to see where my skim would skim halfway around, and set zero there.

for Example: then half of the part would be about .500, and the other side of the part would be undersize, but my zero touch-off would be at .500.

Replies
14
Views
2K
Replies
2
Views
764
Replies
48
Views
2K
Replies
18
Views
2K
Replies
10
Views
1K