PDA

View Full Version : Confusion regarding thread depth



hwingo
11-16-2010, 01:34 AM
Hey Guys,

I’m a bit confused regarding thread depth and how large to bore a hole that’s to be threaded. I will use the following as an example.

I have a male piece that measures .970” OD at 20TPI and I need to bore a hole and thread the hole @ 20TPI so that the male piece (.970”) will screw into the bored & threaded hole. I am using the following formula to calculate thread depth:

Depth of Thread = 1 / TPI X .866
DoT = 1 / 20 X .866
DoT = .0433”
Double depth = .0866”

If I subtract .0866” from .970” the ID of the hole to be threaded is .8834”

However stamped on the Starrett 60 deg Center Gauge, is a value of .065” (double depth) for 20TPI rather than the calculated double depth of .0866. This would mean that my hole diameter would need to be .905” ID. This is a hole diameter difference of .0216”.

So which do I follow when boring the hole …. Starrett Center Gauge's stamped values or the formula? What is the reason for your choice?

Harold :confused:

Paul Alciatore
11-16-2010, 02:15 AM
The OD of a male thread is not an accurate measurement to determine the size of a female thread to match it. The male thread may have a diameter that is reduced from the nominal diameter for the thread. What you need to measure is the pitch diameter or the diameter at the 50% point of the Vee. The point where the width of the thread equals the width of the space between the threads. For a 20 TPI thread, this is the diameter where the thread and space each equal 0.025".

To measure this pitch diameter you will need either a thread micrometer or a standard mike and the proper sized wires to do the three wire measurement. The best wire size for this measurement is a wire that will contact the thread at the pitch line. But a range of wire sizes may be used for a given pitch as long as the wire contacts the threads on the straight sides of the Vee and does not bottom out or ride on the tops of the Vees. So you may use a wire that is close to the Best-size instead of the exact value.

Best-size wire = 0.57735 Χ pitch (in inches)

for 20 TPI, this comes to 0.57735 Χ 0.050 = 0.0288"
After measuring over the three wires, the following formula gives the pitch diameter:

PitchDiameter = M + 0.86603P – 3W

where M is the measured value over the three wires,
P is the pitch in inches
W is the wire diameter used

The thread micrometer method is a lot easier, but more expensive.

But you are not done. The measured pitch diameter is not necessairly the exact number to be used in cutting a matching nut because some allowance must be made for assembly. You will have to increase the measured value by a reasonable number. In the case of 20 TPI or a pitch of 0.050", allowances between 0.004" and 0.012" may be reasonable, depending on the application. In reality, if you are using a tap, you will need to look up or calculate the correct tap drill for the tap you use. Or it may be printed on the tap.

Your measured OD of 0.970" leads me to believe that the actual thread size, with a bit of an allowance for fit and perhaps a bit of the tops of the threads omitted, is actually a 1" - 20. The pitch diameter measurement would confirm this if it is close to the calculated value for this thread. A 1-20 is actually a UNEF thread (Unified Extra Fine thread) with a pitch diameter of 0.9675"

whitis
11-16-2010, 04:39 AM
The marking on your fishtail gage probably date back a century to when L.S. Starrett himself was still alive and made fishtail gages; the values on it are of little value today.

Look at this diagram while you read the rest of this post:
http://en.wikipedia.org/wiki/File:ISO_and_UTS_Thread_Dimensions.svg

First, your calculations are for sharp V threads, not unified standard threads, though they do tell you something about the imaginary V shape underlying them. Your DoT number is H; other values are based on some number of eighths of H. On an external thread, 1/8H is chopped off the crests and 1/8H to 1/4H off the root (depending on the radius of the cutter), plus you have a tip radius and clearance. The starrett number is within roundoff error of 3/4H*2 - i.e. it is based on Seller's threads. In 1864, the sharp V thread was replaced by the Seller's thread which was replaced in 1949 with the unified thread standard. Seller's threads had 1/8H chopped off both the root and the crest producing flats; Unified threads chopped off another 1/8H or more specifically specified a radius that fits somewhere between 1/8H chopped off and 1/4H chopped off (this part isn't shown well on the diagram). For your drilled hole to give 100% thread (which you would not want if using a tap) you have to allow for 1/4H (plus clearance). If you look at the diagram, 5H/8 (or 5/8*H) is the distance between the line which separates the roots and crests of the internal and external threads.

V threads: DD = H*2
Seller's threads: DD = 3H/4*2
Unified threads: DD = 5H/8*2

And if you do modified flank infeed, you have a cosine correction for that, as well, to get your compound feed distance

oldtiffie
11-16-2010, 06:31 AM
Hey Guys,

I’m a bit confused regarding thread depth and how large to bore a hole that’s to be threaded. I will use the following as an example.

I have a male piece that measures .970” OD at 20TPI and I need to bore a hole and thread the hole @ 20TPI so that the male piece (.970”) will screw into the bored & threaded hole. I am using the following formula to calculate thread depth:

Depth of Thread = 1 / TPI X .866
DoT = 1 / 20 X .866
DoT = .0433”
Double depth = .0866”

If I subtract .0866” from .970” the ID of the hole to be threaded is .8834”

However stamped on the Starrett 60 deg Center Gauge, is a value of .065” (double depth) for 20TPI rather than the calculated double depth of .0866. This would mean that my hole diameter would need to be .905” ID. This is a hole diameter difference of .0216”.

So which do I follow when boring the hole …. Starrett Center Gauge's stamped values or the formula? What is the reason for your choice?

Harold :confused:

Harold.

I think that the thread you have is an under-size (outside diameter) 1"-20-UNEF thread and assuming that it is Class 2A (the "normal" fit) the outside diameter limits are 0.9986"/0.9905", the pitch diameter limits are 0.9961"/0.9616".

The details for the mating nut/female which I have assumed is a Class 2B you are making are:
- minor diameter (bore) limits: 0.946"/0.957"
- pitch diameter limits: 0.9675"/0.9734"

(See Machinery's Handbook 27 page 1745).

Keep the screwing tool point as fine as you can and just keep screw-cutting until the screw that you have is an easy fit into the hole your are screw-cutting.

Its as easy as that.

There is no need for the use of either "3-wires" or the calculations that go with them - and no need for a thread micrometer in this instance either.

Screw-threading is not rocket science but has a lot of urban myths, useless mystique and bull-$hit attached to it.

The nominal pitch diameter that many will refer you to is usually not within the tolerance zone for either the nut or the bolt. This pic should help to explain it.

http://i200.photobucket.com/albums/aa294/oldtiffie/Black_book/Black_book_Fasten_P72-73_1.jpg

JCHannum
11-16-2010, 07:14 AM
The simple formula for determining the diameter for tap drill or hole size is 1 divided by thread number subtracted from the OD. This will get you in the 70-75% thread range.

Using this, your ID works out to 0.920". If you have the male thread at hand, test fitting as final thread size approaches will give you the best fit. When threading a receiver or barrel blank, I will usually make test parts first from scrap to determine best fit.

hwingo
11-16-2010, 09:40 AM
Harold.

I think that the thread you have is an under-size (outside diameter) 1"-20-UNEF thread and assuming that it is Class 2A (the "normal" fit) the outside diameter limits are 0.9986"/0.9905", the pitch diameter limits are 0.9961"/0.9616".

The details for the mating nut/female which I have assumed is a Class 2B you are making are:
- minor diameter (bore) limits: 0.946"/0.957"
- pitch diameter limits: 0.9675"/0.9734"

(See Machinery's Handbook 27 page 1745).

Keep the screwing tool point as fine as you can and just keep screw-cutting until the screw that you have is an easy fit into the hole your are screw-cutting.

Its as easy as that.

There is no need for the use of either "3-wires" or the calculations that go with them - and no need for a thread micrometer in this instance either.

Screw-threading is not rocket science but has a lot of urban myths, useless mystique and bull-$hit attached to it.

The nominal pitch diameter that many will refer you to is usually not within the tolerance zone for either the nut or the bolt. This pic should help to explain it.


The simple formula for determining the diameter for tap drill or hole size is 1 divided by thread number subtracted from the OD. This will get you in the 70-75% thread range.

Using this, your ID works out to 0.920". If you have the male thread at hand, test fitting as final thread size approaches will give you the best fit. When threading a receiver or barrel blank, I will usually make test parts first from scrap to determine best fit
__________________
Jim H.



OldTiffie & Jim H,

Just to clear things up, and somewhat keeping with Jim H, the male piece is a bolt head for a rifle and was not designed to conform with standard size OD. I am making another rifle (from scratch) thus nothing is "conventional" ..... it simply works out the way it happens to work out.

While I was working on the receiver, a buddy decided to surprise me by making the bolt-head .... and he did a fine job. I had ordered a piece of 4130 Chromemoly tubing 1.250 OD by .750 ID. So the shank he cut and threaded is .970. This leaves me with determining how large I am to bore the ID before I start threading.

Tiffie, I understand "keep cutting threads until the piece fits" but I was hoping to get a close estimate of ID size so that I didn't have to spend too much unnecessary time threading until the piece fits.

I think that Jim H has gotten close to what I need. Though there appears to be some inconsistency between the end of the thread and the shoulder remaining, believe it or not the minor diameter ranges between .920 and .915. With that in mind I probably should make the ID .915, call it good, and start threading until it fits. That would work for me.

Harold

Carld
11-16-2010, 11:48 AM
I think you need to go for a class 3 fit for a gun barrel/receiver or any major gun part. The math should get you to a close minor diameter for the bore giving a 75-80% thread engagement, at least I would prefer that for a gun. You will still have to cut to fit when doing the internal thread to match the male thread. There is no way around that for a class fit.

Larry Swearingen
11-16-2010, 02:15 PM
Harold,
How do you plan on threading the ID of that receiver ?
It's a lot easier to match a Male thread to an existing
female thread.
I'd scrap the bolt your buddy made and get a tap to
thread that receiver. Then lathe turn the bolt to fit.

Larry S
Fort Wayne, IN

Carld
11-16-2010, 03:40 PM
That's not true. As long as I have one threaded part, male or female, I can make the other part to a class fit in as much as I can make the thread fit as tight as I want it or as loose as I want it and he can do the same.

His concern is that he has the right size ID or bore to get the thread depth he desires. Cutting the thread to the desired fit is easy after that.

hwingo
11-16-2010, 10:54 PM
I think you need to go for a class 3 fit for a gun barrel/receiver or any major gun part. The math should get you to a close minor diameter for the bore giving a 75-80% thread engagement, at least I would prefer that for a gun. You will still have to cut to fit when doing the internal thread to match the male thread. There is no way around that for a class fit.

Carld, don't need a Class 3 fit especially for the barrel to receiver. For years, we have used switch-barrel-rifles in competition. Barrels screw in by hand and lock via a snap of the wrist. When it's time to change from light varmint to heavy varmint (and sometimes unlimited events with super heavy barrels) we simply unscrew the barrel and switch to another. No big thing.

Keeping with this thread, my attention is not on barrel to receiver fit, rather, how to determine the correct size I will need when boring the bolt body to accept the threaded bolt head.

To veer off topic, the union between the bolt head and bolt body does not need to be a class 3 fit for many reasons. In fact, many large caliber bolt action rifles are made with a floating bolt head that's only loosely pinned to the bolt body. Lock-up occurs when the locking lugs on the bolt head rotate (via turning the bolt body) and engage the locking lugs inside the receiver. Other than that, the bolt body only server to open and close the bolt head (chambering and extraction) and it serve as a carrier for the firing pin, bolt shroud, and cocking mechanism.

Harold

Carld
11-16-2010, 11:00 PM
Well, in that case several methods have already been given. I would also recommend using the formula in the Machinery Handbook or many other books that cover threading. In fact there may be several online calculators to use.

I just use one of the many Machinery Handbooks or others to find a formula.

From your last post it seems the fit don't really matter so close would be good enough apparently.

hwingo
11-16-2010, 11:22 PM
Harold,
How do you plan on threading the ID of that receiver ?
It's a lot easier to match a Male thread to an existing
female thread.
I'd scrap the bolt your buddy made and get a tap to
thread that receiver. Then lathe turn the bolt to fit.

Larry S
Fort Wayne, IN

Once again, the threads on a receiver has nothing to do with a bolt head. The bolt head does not screw into a receiver, rather, a barrel screws into the receiver. The bolt head screws into a bolt body which slides back and forth within the receiver's ways when chambering a shell or extracting a shell.

However, to answer you question regarding how I will thread the ID of a receiver, ..... it's easy. Simply chuck the receiver in the lathe, center the receiver, bore, and then thread. It would be most difficult, if not cost prohibitive, to get a tap for my receiver. The ID (not OD) of my receiver is 2.0" (two inches) and 1.850" deep X 16TPI. It's far easier to simply cut the threads on a lathe. But again, we are not talking about threading a receiver and matching the barrel to the receiver ..... that was a done a long time ago.

Harold