Not a beginner but have not done a bunch of non-standard threading jobs. Had a guy bring me a bandsaw downfeed cylinder and wanted me to make a new top nut ( kind of an external gland nut) for this cylinder. Measured the pitch to be 24 threads per inch. Then measured the external threaded dia to be 1.39”. Not sure why this crazy size but it is what it is. Here is where I am getting confused. To create the internally threaded cap I know I have to bore to something at or less than the external thread minor diameter depending on the class fit before I start threading the cap. I’m just not sure where to start! Looked at the handbook for 24 pitch thread but just not sure how to apply all the numbers.
Follow along with the video below to see how to install our site as a web app on your home screen.
Note: This feature may not be available in some browsers.
Largest Manufacturing Technology Community on the Web
Stay Connected:
Another threading post?
- Thread starter DanBrub
- Start date
- Replies 8
- Views 1,860
How did you measure the 24tpi? Pitch gage? If it were me beings it's a bastard OD did you try a metric pitch gage also just to be sure one of those didn't fit better? Are you able to man handle the the other piece to check the nut as your making it? If no then you might need to duplicate the threaded shaft as a check piece first.
Now this may not be textbook procedure but I've done several times when in this situation. Sometimes manufacturers make shit bastard on purpose so nothing standard works.
If you're sure of the pitch, after you have the correct hole just thread the nut until you have the desired fit you want using the other piece.
I wouldn't get too shook up about all the numbers in the book and just make them fit, its bastard anyways, don't matter what thread it is as long as they screw together with a nice fit and it serve its intended purpose.
Folks may bitch about this ain't proper textbook procedure but when all I have is a bastard mating part sometimes you have no other choice.
Hopefully you find what thread it is and go from there but if not he's still going to want a nut. Hope some of this helps. Good luck!
Brent
Now this may not be textbook procedure but I've done several times when in this situation. Sometimes manufacturers make shit bastard on purpose so nothing standard works.
If you're sure of the pitch, after you have the correct hole just thread the nut until you have the desired fit you want using the other piece.
I wouldn't get too shook up about all the numbers in the book and just make them fit, its bastard anyways, don't matter what thread it is as long as they screw together with a nice fit and it serve its intended purpose.
Folks may bitch about this ain't proper textbook procedure but when all I have is a bastard mating part sometimes you have no other choice.
Hopefully you find what thread it is and go from there but if not he's still going to want a nut. Hope some of this helps. Good luck!
Brent
Last edited:
michiganbuck
Diamond
- Joined
- Jun 28, 2012
- Location
- Mt Clemens, Michigan 48035
Qt yard[ If no then you might need to duplicate the threaded shaft as a check piece first.}
I have done this with wire size the existing male at a number of place, and make a male to the largest area to make a test gauge for the nut.
Handy thread calculator..but making a test gauge is best.
UN imperial screw thread calculator
You can enter 1.39"-24 and get results ..but who would know what standard the original was made to.
I have done this with wire size the existing male at a number of place, and make a male to the largest area to make a test gauge for the nut.
Handy thread calculator..but making a test gauge is best.
UN imperial screw thread calculator
You can enter 1.39"-24 and get results ..but who would know what standard the original was made to.
rons
Diamond
- Joined
- Mar 5, 2009
- Location
- California, USA
Worked out a solution for myself by drawing a picture of a UNF thread specification and did a few sine and cosine operations. The number for D matches the machinery handbook.
With a known pitch (P) the bit travel distance (D) moving in at a 30 degree angle is:
D = 0.625 x P
The vertical height (H) is:
H = D x (cos 30) = 0.625 x P x 0.866 = 0.541 x P
---------------------------------------------------------------
I am ignoring class of fit. Which should imply that there is no voids and there is no fit at the minimum diameter, it's as tight as it gets.
The minimum diameter is to be increased by an amount determined by the class of fit.
hole bore size = 1.39 - (2 x H) = 1.39 - .045 = 1.345 (minimum diameter)
---------------------------------------------------------------
I have used this calculation mostly for external threads but it works for internals too.
With a known pitch (P) the bit travel distance (D) moving in at a 30 degree angle is:
D = 0.625 x P
The vertical height (H) is:
H = D x (cos 30) = 0.625 x P x 0.866 = 0.541 x P
---------------------------------------------------------------
I am ignoring class of fit. Which should imply that there is no voids and there is no fit at the minimum diameter, it's as tight as it gets.
The minimum diameter is to be increased by an amount determined by the class of fit.
hole bore size = 1.39 - (2 x H) = 1.39 - .045 = 1.345 (minimum diameter)
---------------------------------------------------------------
I have used this calculation mostly for external threads but it works for internals too.
Last edited:
HuFlungDung
Diamond
- Joined
- Jan 19, 2005
- Location
- Canada
A quick method I use is look up the bolt pitch on a standard drill and tap chart I have hanging on the wall. For example, 3/8 UNF is 24 tpi, so just look at what the recommended tap drill is (letter R) @.339, so just subtract to find the difference between the OD of your thread and the hole to be tapped for it.
JCByrd24
Aluminum
- Joined
- Jan 24, 2009
- Location
- Maine, USA
I just went through this recently and learned once you add in standard fit you get to a very easy formula:
Target bore = Nominal diameter - Pitch
Your 0.541P is basically reduced slightly so the threads don't interfere, to nominally 0.5P on each side, which is 1P on the diameter.
I checked this against fit tolerance tables and this formula works if you hit it within a few thou. Same checking against HuFlungDung's method.
Target bore = Nominal diameter - Pitch
Your 0.541P is basically reduced slightly so the threads don't interfere, to nominally 0.5P on each side, which is 1P on the diameter.
I checked this against fit tolerance tables and this formula works if you hit it within a few thou. Same checking against HuFlungDung's method.
AlfaGTA
Diamond
- Joined
- Dec 13, 2002
- Location
- Benicia California USA
Tap drill size to give 75% thread depth:
Diameter of male thread or tap Minus .974/Threads per inch= drill size or in your case your bored hole.
Cheers Ross
Diameter of male thread or tap Minus .974/Threads per inch= drill size or in your case your bored hole.
Cheers Ross
EPAIII
Diamond
- Joined
- Nov 23, 2003
- Location
- Beaumont, TX, USA
You have an external thread with a known pitch (24 TPI) and an approximate OD (1.39"). You may have measured the actual OD to ten decimal places, but it is still only APPROXIMATE as it relates to the theoretical OD of your actual thread which may be larger or smaller (most likely larger).
Threads may be specified by the OD, but measuring the OD is NOT a dependable way to ensure a fit. The problem is most threads have truncated peaks and there is no good way to measure or estimate the actual percentage of this truncation. For a standard thread form it is a nominal 1/8th of the height of the sharp edged thread form BUT this is only a nominal value and even the standard allows for a large variation. There are many reasons which may cause this number to be different from that nominal value. And, as I said, there is no good way to directly measure it.
This is why we have thread wires and thread micrometers. They measure the pitch diameter of the thread and that is the real basis of the calculation that you need to do. I suggest that you read the procedure and the math for the three wire method and use it to find the pitch diameter. Then use the standard thread formulae to calculate the ID you need for a mating, female thread.
After boring the needed ID, I would single point cut the threads with an appropriate tool (proper angle and flat at the tip), checking the fit as the cut progresses.
If you guess at the ID, try to guess on the small size as you can always cut more off, but putting it back on is difficult. Not many lathes can do that trick. The problem with using an unknown ID is that you can cut the threads too deep if you cut a sharp peak down below the original level of that bore. Then the pitch diameter WILL be too large and you WILL have a very loose fit.
That flat on the ID MUST be correct when you make any trial fits to see if the thread is cut deep enough. If it is not correct, then a sharp Vee at that point will interfere with the fit and cause you to cut the female thread too deep. Just ask me how I know.
Threads may be specified by the OD, but measuring the OD is NOT a dependable way to ensure a fit. The problem is most threads have truncated peaks and there is no good way to measure or estimate the actual percentage of this truncation. For a standard thread form it is a nominal 1/8th of the height of the sharp edged thread form BUT this is only a nominal value and even the standard allows for a large variation. There are many reasons which may cause this number to be different from that nominal value. And, as I said, there is no good way to directly measure it.
This is why we have thread wires and thread micrometers. They measure the pitch diameter of the thread and that is the real basis of the calculation that you need to do. I suggest that you read the procedure and the math for the three wire method and use it to find the pitch diameter. Then use the standard thread formulae to calculate the ID you need for a mating, female thread.
After boring the needed ID, I would single point cut the threads with an appropriate tool (proper angle and flat at the tip), checking the fit as the cut progresses.
If you guess at the ID, try to guess on the small size as you can always cut more off, but putting it back on is difficult. Not many lathes can do that trick. The problem with using an unknown ID is that you can cut the threads too deep if you cut a sharp peak down below the original level of that bore. Then the pitch diameter WILL be too large and you WILL have a very loose fit.
That flat on the ID MUST be correct when you make any trial fits to see if the thread is cut deep enough. If it is not correct, then a sharp Vee at that point will interfere with the fit and cause you to cut the female thread too deep. Just ask me how I know.
Many thanks to everyone who weighed in on this it has helped me immensely. I first went back and verified the pitch and while it was close to 1.0mm the 24/inch was a better fit. The fact that this cylinder is off an older US built saw before metric became normal helped convince me. The three-wire measurements didn’t confirm but I looked at the threads under magnification and the crest flat is twice as wide as root. Regardless I used the link Michiganbuck provided (wish I had known that link years ago) and started with the low end of the min internal dia. Then followed yardbirds recommendations to just keep turning until the two parts threaded together. In the end the fit is really good so I have achieved the end goal. I’ve made some notes on all your replies and it will surely come in handy in the future.
