What's new
What's new

Custom thread size?

PepeLapiu

Aluminum
Joined
Apr 15, 2017
Okay guys. Keep in mind in your replies that I am not a machinist and I did not sleep at the Holiday Inn last night.

The 1"7/16 x 28 tpi thread would have the minor diameter of the nut threads between 1.399" and 1.405" according to the following table:

Unified Screw Threads, Standard Series

I would like to design a nut and bolt with a non-standard thread. So that the minor diameter of the internal thread sits between 1.374" and 1.380".

I figure, to do that, I need to bring the thread size down to 1.413" from the standard 1"7/16 (1.438").

So can this be done? Will I be breaking some unwritten machinist law?

And how can I write it down on my plans so that it makes sense to a machinist?

I would write up the standard thread as - 1"7/8 x 28 tpi UN
But how would I write up my non-standard new thread? 1.413" x 28 tpi UN. Is this correct?
 
Last edited:
So let me just rephrase what I am looking for.

I have a tube with a 1.370" ID. Inside the tube, will be slipped in 1.367 OD stuff.
The tube is to have internal threads at both ends.
I would like the minor diameter of the threads to be as close as possible to the actual tube ID.
The closest thread I found would be the 1"7/16 x 28 UN thread with a minor diameter of 1.400.
I want to bring it in closer to 1.370 while still keeping the same thread pitch.

How do I write this up on the plans?
 
Take your desired minor and add 2x the thread height, let's use .035" for example.

I'd call it out as a 1.45-28 thread and give your calculated major, minor and pitch diameters on the drawings. You can use the differences from the major diameter (for external) or minor(for internal) of any other 28 tpi thread for approximations of major/minor and pitch diameter.


5c collets use a 1.041-24 thread so it's not totally unheard of.
 
Take your desired minor and add 2x the thread height, let's use .035" for example.

I'd call it out as a 1.45-28 thread and give your calculated major, minor and pitch diameters on the drawings. You can use the differences from the major diameter (for external) or minor(for internal) of any other 28 tpi thread for approximations of major/minor and pitch diameter.


5c collets use a 1.041-24 thread so it's not totally unheard of.

Dude, your post is making my head spin. I'm really not very smart. I've had to make it through in life on my looks alone.

So let's have a simple exercise to see if I am off my rockets here.

Let's say I hand you a drawing of a nut. And the thread is described as 1.413" x 28.

Would you be able to make the nut thread from this information alone?
If so, what would be your calculated minor nut dia.?
 
You'd get two parts that fit together but might not be 100% correct by the book but then again you've thrown the book out the window already.

I don't have a MH around so I can't give you hard values.

I'm sure someone will chime in soon saying buy a copy of thread pal and use those numbers or maybe someone will do you a solid and run it through their copy for you.
 
I'm just going to explain my own thinking here. And you can correct or add to what I came up with.

According to the link I posted in the OP, the 1"7/16 x 28 UN uncoated thread is as follows:

External maximum major diameter: 1.4375
Internal minimum minor diameter: 1.3990

So from the above, I calculated maximum thread height at (1.4375 - 1.3990) ÷ 2 = 0.01925

So if I want the internal threads to have a minor of 1.375, I should go with a thread diameter of 1.375 + (0.01925 × 2) = 1.4135 (or rounded to 1.41).

So if I just write it down as 1.41 x 28 tpi, will that be enough for the machinist to run it?
 
You'd get two parts that fit together but might not be 100% correct by the book but then again you've thrown the book out the window already.

I don't have a MH around so I can't give you hard values.

I'm sure someone will chime in soon saying buy a copy of thread pal and use those numbers or maybe someone will do you a solid and run it through their copy for you.

I have no problems with buying software if it helps me. But that thing is likely designed for people like you. Not for someone like me who doesn't understand all that much about these things.

Hopefully someone will offer to do me a solid, as you said.
 
Well okay. I downloaded the trial version of Thread Pal. Just as I though - I understand some of it. But some of it just flies right over my head.

So if I download the full version, is anyone here willing to take me through it with baby steps?
 
I find your post somewhat confusing. First you talk about a 7/16 - 28 thread and then you talk about that thread having a minor diameter of 1.399" to 1.405". But 7/16" = 0.4375" and the minor diameter of a 7/16" thread would be less than that, not almost an inch more. You seem to be switching between 7/16" and 1 7/16". Anyway, that is what I am assuming. I am also assuming that you really want a thread that is close to but somewhat smaller than 1 7/16". This seems to square with your tube size of 1.370" ID from the second post.

Going from that tube ID and your stated range of 1.374" and 1.380" I will assume a mid value of 1.377" for the nut's ID. That will allow you to carefully enlarge the ID of your tube to that value: but that operation is another subject.

The next thing that must be considered is the class of fit. That refers to the amount of clearance between the external and internal threads. There must be some clearance or they will bind and gall and be difficult to assemble and disassemble. According to Machinist Handbook, the pitch diameters for a 1 7/16 - 28 thread with a class 2 fit (the only class shown for that thread) are:

External thread Pitch Diameter: 1.4130" - 1.4088" and the medium value is 1.4109"
Internal thread Pitch Diameter: 1.4143" - 1.4198" and the medium value is 1.4171"

The difference is 0.006" on the diameter and that is the allowance for this thread. An equal allowance should be OK for the special thread you are proposing. We can achieve this by just subtracting the difference between your thread and that nearby standard thread from both the OD of the external threads and the ID of the internal ones. You give your desired internal ID as 1.377" and that is 0.0401" smaller than the 1.4171" value. So you can subtract the same amount from the OD of the external thread to arrive at your OD: 1.4109" - 0.0401" = 1.3708". These can be rounded to 1.417" and 1.371" respectively.

So the official call out for your thread is a 1.417 - 28 UN. That is the external thread size and a good machinist should be able to make the internal thread to properly match it. But, in the real world, you should supply the extra information that will make cutting that internal thread easier. That would include the ID = 1.377" and the allowance of 0.006" on the diameter. I would put a tolerance on the external thread diameter of +0.001"/-0.002" and on the internal thread diameter of +0.002"/-0.001" The machinist making these parts can use the tolerance figures to make a gauge for the internal thread. He would/should make a go/no go gauge with external threads of 1.377" (go) and 1.379" (no go). Thus the internal thread, as measured by that gauge, would be between 1.377" and 1.379". Of course you can specify any tolerance range you wish, but you should keep in mind that 0.006" allowance. If you allow the external thread to be more than 0.003" larger or the internal thread to be more than 0.003" smaller, then you will get interference.

That is how I would look at designing and specifying this thread. As for violating any rules, the above assumes a Unified thread form. Since your diameter is not a standard one, holding to the Unified thread form is the best you can do. There are many non standard threads made in the world so don't lose any sleep over it.



Okay guys. Keep in mind in your replies that I am not a machinist and I did not sleep at the Holiday Inn last night.

The 7/16 x 28 tpi thread would have the minor diameter of the nut threads between 1.399" and 1.405" according to the following table:

Unified Screw Threads, Standard Series

I would like to design a nut and bolt with a non-standard thread. So that the minor diameter of the internal thread sits between 1.374" and 1.380".

I figure, to do that, I need to bring the thread size down to 1.413" from the standard 1"7/16 (1.438").

So can this be done? Will I be breaking some unwritten machinist law?

And how can I write it down on my plans so that it makes sense to a machinist?

I would write up the standard thread as - 1"7/8 x 28 tpi UN
But how would I write up my non-standard new thread? 1.413" x 28 tpi UN. Is this correct?
 
Certainly you can make any thread you might choose. But if it is not on a thread chart it is not a standard thread.
Standard threads are made so one can go to a reference and find the specifications of a thread.
Nobody can find your thread in any reference so it is not a standard thread.

https://mdmetric.com/tech/thddat9.htm#uc

You might search metric threads and find one close to what you wish...(Nope a 48 x 1.5 is a pitch of.059")

QT: [ 1.413" x 28 tpi UN. Is this correct? ] NO.

Still your tread can be easily made.. you just need to specif the specs so the manufacturing shop knows what you want.

EPA111 did the engineering for your non standard thread.. Most manufacturing shops would not wish to do all that extra work and/or take a chance for a reject part..
 
I find your post somewhat confusing. First you talk about a 7/16 - 28 thread and then you talk about that thread having a minor diameter of 1.399" to 1.405". But 7/16" = 0.4375" and the minor diameter of a 7/16" thread would be less than that, not almost an inch more. You seem to be switching between 7/16" and 1 7/16".

That was just a typo. I meant 1.4375, not 0.4375.

Will correct that later and soak in all that you have written later. On my way to work right now.

Looks impressive. Thanx
 
A few thoughts...

Is there a reason you are married to 28tpi?? 1-7/16 - 16 lands
the minor right where you need it.

On the tubing with a 1.37 ID.. Is this a one off, or is this *hopefully* going
to be a recurring thing? Tubing is notoriously shitty at having a consistant ID..
If my tiny little brain remembers correctly your ID is set by wall thickness, which
has a tolerance of ±10%. That little fact has bitten me in the ass more than once.

As for a non-standard thread.. Big deal, any machinist won't have a problem with that..
Or at least they shouldn't.

My suggestion.. Especially if its a one off... Have your machinist make both parts,
with a tolerance of "make it work".. "make it work" tolerances cost a LOT less than
some obscure thread call out. A LOT le$$.. "Make it work" jobs are fun, and generally
stress free... Oddball thread call outs where you have to bust out the wires, that costs.
 
Why do you want a non standard thread? How many of these will be made. what happens in a year or fifty when someone some where in the world loses a part a needs a new one?
Bill D
 
A few thoughts...

Is there a reason you are married to 28tpi?? 1-7/16 - 16 lands
the minor right where you need it.

The tube has an OD of 1.5". Other guys put on 1"7/16 x 20 thread on it which brings the thread within 1/32" from the OD. So I decided to increase the tpi and decrease the diameter to bring the major ID in further away
from the OD.

Honestly, putting a 1"7/16 thread on a 1.5" tube feels ridiculously insane to me. I don't know how other guys have been getting away with it.

On the tubing with a 1.37 ID.. Is this a one off, or is this *hopefully* going
to be a recurring thing? Tubing is notoriously shitty at having a consistant ID..
If my tiny little brain remembers correctly your ID is set by wall thickness, which
has a tolerance of ±10%. That little fact has bitten me in the ass more than once.

Tube OD is 1.5" (+/-0.005) and wall thickness of 1.78" (+/-10%). So the ID will actually be machined up to a consistent 1.370".

Edit: tube OD is 38mm (+/-0.127mm)and wall thickness is 1.78mm (+/-10%)

As for a non-standard thread.. Big deal, any machinist won't have a problem with that..
Or at least they shouldn't.

My suggestion.. Especially if its a one off... Have your machinist make both parts,
with a tolerance of "make it work".. "make it work" tolerances cost a LOT less than
some obscure thread call out. A LOT le$$.. "Make it work" jobs are fun, and generally
stress free... Oddball thread call outs where you have to bust out the wires, that costs.

So you are saying I should just tell him the thread is 1.413" x 28 tpi UN class 2, and make it fit? That will be enough for him to do it?
 
Why do you want a non standard thread? How many of these will be made. what happens in a year or fifty when someone some where in the world loses a part a needs a new one?
Bill D

The tube has very small wall thickness. The best fitting standard thread is just too close to cutting into the OD of the tube. See my previous post to that effect.
 
My concern is the tolerance of the available tube (the bore in this case)
Your supplier has a tolerance listed, what is it for the bore ?
 
My concern is the tolerance of the available tube (the bore in this case)
Your supplier has a tolerance listed, what is it for the bore ?
I mixed up my numbers. There tube manufacturer claimed OD is 38mm (+/-0.127mm) and wall of 1.78mm (+/-10%).

I need a consistent ID with a tolerance of +/-0.002". So I figured machining it to 1.370" would do it. Agreed?
 








 
Back
Top