
1Likes

Thread major and minor diameter relations by tpi...
I'm finding myself puzzled. I CAN start cutting and just test fit, but all I learn is that it fits or it doesn't. What I'm after:
I need to make a new retaining ring for the sight glass for my Van Norman. Thanks to Steve Steven, I now know that it's a parallel thread, not an NPT like the sight glasses from MSC/McMaster, etc. which are in abundance. I did some measuring today, it's .3 recessed into the gearbox, subtract the glass thickness, etc. I'm going with .25" thick. 1.5" minor diameter (peak to peak, correct me if it's not the minor diameter). Thread gauge says 20tpi. So, where I'm at:
if I take a 1/4 20 from my charts, subtract the minor diameter from the major diameter, will that be the same number as it would be for this? Are all 20tpi (let's assume the same class) going to have the same thread height? Can I take that number and add it to 1.5 and get a major diameter for single pointing the new piece?
Again, I could try, and it might work, but I would have to try and hope next time instead of knowing how to do it.
Trip

Yes. Or you could get much closer looking in Machinery's Handbook. It may list 1.50020 numbers  and for more than one class of fit.
Yes, we read that yours is larger than 1.5"

Originally Posted by johnoder
Yes. Or you could get much closer looking in Machinery's Handbook. It may list 1.50020 numbers  and for more than one class of fit.
Yes, we read that yours is larger than 1.5"
Thanks!
I tried, I really did, I spent an hour plus searching Machinery's handbook (friend gave me PDF of the 27th) but I got lost and turned around. Digital is great, but I need to save my pennies for paper, makes all the difference sometimes.
Am I looking for a chart/table/formula, specific section?
Trip

Am I looking for a chart/table/formula, specific section?
Pages and pages of thread dimensions  in bold in my 21st

Dunno if you are handy with a calculator or not....
You should work this out on paper to be sure you understand before using.
But basically, the 100% engagement for a hole (bore) for theoretical thread for the female part would be major diameter minus 2 x cos(angle/2) divided by the thread pitch for 60° threads only.
For other threads, say 55 Whitworth you have to use the tangent function. But most of the threads we deal with are 60°. Unless you go to acme, which can have different rules for addenda depending where they center.
Anyway for 100% theoretical engagment of a 20 pitch, 60° thread the equation for the amount to deduct would be 2 x cos30°/20. (=.0866")
However it is pointless to try for 100% thread engagement, so take the number above, and multiply by your preferred engagement %. If you want 75% engagement, multiply the number by .75. Then deduct it from the OD. In the example described, the amount to deduct would be .75 x .0866 = .065"
It is a little trickier to figure a plug from mic'ing the inside of threads, since you have to guess where the sharp crest would be, and estimate how much (%) engagement was included in the original. In a sense, you have to "guess" what the logical OD of the plug should have been. Then turn (thread) between centers or held in a small chuck so you can take the work off and try it when getting close.
If I was feeling bold based on the above, I'd take a WAG and try making a quick plug, maybe in easy cutting aluminum, that was 19/16" OD, creep up on the full profile thread & test along the way to see if it fit.
If you have 2, 1/220 tpi bolts, you can try grinding them each exactly in 1/2, inserting in the hole top and bottom, and mic'ing between them or using an expanding parallel and measuring over it. Add the 1/2" back on to the parallel height, and you would be within a few .001's of the target.
There's a guy from Denmark who posts on here who makes thread measuring attachments to fit onto vernier/dial/digital calipers. I have *many* OD thread mics up to 4", but nothing for ID. Have not tried his product, but it might be a useful option if you do a lot of this.
smt

You can calculate and figure all you want, but in the end, you will be test fitting it, no matter what. If the original thread was cut exactly to the specs in MH, it may go a little easier, but since you have no easy way to measure the internal pitch diam, you will be operating on guesswork, no matter what. If they cut to minimum minor diam, you will have to cut under. If they cut to maximum, you'll have to leave it loose.
I say this as a guy who cuts threads pretty much every day in all kinds of sizes and pitches in hydraulic cylinders. I tried using all the formulas and such, only to have parts kick back or have to put them back in the lathe and set them up again. I fitted a piston PERFECTLY to a rod when I first started there. Brand new lock nut that came in the next day would not fit. By the time I got the locknut to spin on smoothly, the piston could about be thrown on the threads. Last time i played that little game. I now just simply won't cut a thread, internal OR external, unless I have the actual mating piece in hand.
My technique for a good starting point on something 1.5x20tpi would be to just look at the old fish and get the double depth of thread off the chart. Take your nominal diam (1.5") and subtract .005 for a clearance (1.495"). That's your major diam for the new insert. Now, subtract the 20tpi double depth of thread from that and give it another .003.005 off. That should be your minor diam with a little clearance. Feed in with the compound to half the double depth. I feed in with the compound at 60 degrees, so I add 10% for a correction and take the last five or ten thou with the cross slide straight in to finish. When the threads are good and sharp at the top, you can give it a try. If it's right, you are in business. If not, you get to reset the tool in the thread pitch and try to skim it again. If you have a QC toolpost, you could also make a long stick of thread and cut off a slice to test fit, discarding the ones that are too big until you get it right.

Maybe i read it wrong, but he seems to be measuring inside the threads in a female hole (minor dia sort of), and coming up with 1.5". Needs to know how much to _add_ to get the correct plug OD.
I probably confused the issue by showing why you come up with a given number for a given thread pitch. But once that is grasped, it is easier to add it back on.
Or maybe i completely misunderstood his post.
smt

Assuming 1.500 as the middle of the internal minor diameter size range, ThreadPal outputs the following theoretical values:
Inch Units
1.548520 UNS2A
Allowance,0.0014
Major Diameter Max,1.5471
Major Diameter Min,1.5390
Pitch Diameter Max,1.5146
Pitch Diameter Min,1.5098
Minor Diameter Max,1.4930
Minor Diameter Min (Ref),1.4773
Root Radius Max,0.0072
Root Radius Min,
Flat At Root,0.0125
Thread Height (Basic),0.0307
1.548520 UNS2B
Allowance,
Minor Diameter Min,1.494
Minor Diameter Max,1.506
Pitch Diameter Min,1.5160
Pitch Diameter Max,1.5222
Major Diameter Min,1.5485
Major Diameter Max (Ref),1.5619
Flat At Root,0.0063
Thread Height (Basic),0.0271
Pitch,0.0500
Lead,0.0500
Starts,1
Lead Angle,0.601
Included Angle,60.0000

Stephen Thomas, thank you for both posts, the first is what I was asking for, the second did sum up what I was doing. I can take a 1.5" diameter piece of stock and stick it in the hole, it touches the crests of the female thread. Thus, I know it's bigger than 1.5" but I don't know how much bigger/what size to start with, so I get the 1.5" minor dia 'sort of'.
Mike C, I do realize I'll be test fitting ultimately, but I figured if I knew how and did the math, it'd save me an iteration or two (I've got the 4 jaw mounted so I can dial it back in, then I just have to practice 'picking up a thread' which was about a 75% success rate in my previous dozen attempts, so better than average I guess.
MRainey, from the initial table add/subtract I did, those numbers look about right, thanks!
I'm all about 'getting it done' but the thing that separates bubba from the guy you want working on your stuff (in my opinion) is how many 'test parts' you have to make. I could have started and just cut away, tried, made another, etc. but knowing the proper way adds a tool to my box for future projects. Doing 'job shop' type stuff, knowing a great starting point is a huge benefit and means more profit per job, as less wasted time and materials. This and other recent projects have been an interesting experience, I feel a connection to my grandfather (passed a few years back) and at the same time make me regret not getting into this sooner so I could have shared with him. He was a machinist before and after WWII, worked his way up to foreman at AMF and then semiretired and went into machine sales. My father connected/related more to HIS grandfather and worked with wood his whole life, I feel a connection with metal (having started my career as a mechanic, then moving to weldor, and now adding machining to that, so all my father can relate is "shame you didn't get into it sooner, Grandpa would have loved it".
And as far as 'easy material, I do have a few pieces of 1.75 AL sitting on the shelf with no purpose, I think I will work with that till I get it dialed in.
Thanks all! I'll think about posting a pic when done, but I'll probably just start a thread of flames based on my choice for machine color Got 2/3 of the machine painted this weekend, I need this piece to reassemble and mount the feed box and call that part done.
Trip

Originally Posted by stephen thomas
Dunno if you are handy with a calculator or not....
You should work this out on paper to be sure you understand before using.
But basically, the 100% engagement for a hole (bore) for theoretical thread for the female part would be major diameter minus 2 x cos(angle/2) divided by the thread pitch for 60° threads only.
For other threads, say 55 Whitworth you have to use the tangent function. But most of the threads we deal with are 60°. Unless you go to acme, which can have different rules for addenda depending where they center.
Anyway for 100% theoretical engagment of a 20 pitch, 60° thread the equation for the amount to deduct would be 2 x cos30°/20. (=.0866")
However it is pointless to try for 100% thread engagement, so take the number above, and multiply by your preferred engagement %. If you want 75% engagement, multiply the number by .75. Then deduct it from the OD. In the example described, the amount to deduct would be .75 x .0866 = .065"
It is a little trickier to figure a plug from mic'ing the inside of threads, since you have to guess where the sharp crest would be, and estimate how much (%) engagement was included in the original. In a sense, you have to "guess" what the logical OD of the plug should have been. Then turn (thread) between centers or held in a small chuck so you can take the work off and try it when getting close.
If I was feeling bold based on the above, I'd take a WAG and try making a quick plug, maybe in easy cutting aluminum, that was 19/16" OD, creep up on the full profile thread & test along the way to see if it fit.
If you have 2, 1/220 tpi bolts, you can try grinding them each exactly in 1/2, inserting in the hole top and bottom, and mic'ing between them or using an expanding parallel and measuring over it. Add the 1/2" back on to the parallel height, and you would be within a few .001's of the target.
There's a guy from Denmark who posts on here who makes thread measuring attachments to fit onto vernier/dial/digital calipers. I have *many* OD thread mics up to 4", but nothing for ID. Have not tried his product, but it might be a useful option if you do a lot of this.
smt
I'm "the guy from Denmark"
I make thread measurement inserts for measuring both external and internal thread pitch diameter. Click on my name and you can see my home page. For what it's worth (my prices are in Euro (€) and €1 is $1.30 at the moment. Just email or PM me if you have any questions.
Gordon

Originally Posted by Gordon B. Clarke
I'm "the guy from Denmark"
I make thread measurement inserts for measuring both external and internal thread pitch diameter. Click on my name and you can see my home page. For what it's worth (my prices are in Euro (€) and €1 is $1.30 at the moment. Just email or PM me if you have any questions.
Gordon
Hi Gordon, was wondering where you were
Which product am I after, I took a quick look but had to run to a meeting. Wasn't sure which link specifically.
No different than dealing with England shipping/customswise, is it?

"Maybe i read it wrong, but he seems to be measuring inside the threads in a female hole (minor dia sort of), and coming up with 1.5". Needs to know how much to _add_ to get the correct plug OD."
Read my post backwards, lol. Seriously, reverse the math to get an OD from the given ID. Just take the measured ID, add double depth of thread plus .005.008 for clearance. Turn the slug to that diam and then start threading. You'll be VERY close to a proper fit when the crest of the thread gets almost sharp.

Originally Posted by Trip59
Hi Gordon, was wondering where you were
Which product am I after, I took a quick look but had to run to a meeting. Wasn't sure which link specifically.
No different than dealing with England shipping/customswise, is it?
You're not the only one wondering where I was and why I've been "silent" the last 3 weeks LOL. My wife and I were on vacation in Texas the last 3 weeks enjoying Texan hospitality
PM or email me on the thread types and sizes you are interested in and I'll give you some suggestions/advice.
I've never had any customs problems with sending to the USA or any other country.
Gordon

Originally Posted by Mike C.
"Maybe i read it wrong, but he seems to be measuring inside the threads in a female hole (minor dia sort of), and coming up with 1.5". Needs to know how much to _add_ to get the correct plug OD."
Read my post backwards, lol. Seriously, reverse the math to get an OD from the given ID. Just take the measured ID, add double depth of thread plus .005.008 for clearance. Turn the slug to that diam and then start threading. You'll be VERY close to a proper fit when the crest of the thread gets almost sharp.
There's the little problem that the tolerance on a thread bore diameter is about twice that of the thread pitch diameter and over 50% that of the OD tolerance on most threads. Pussying around might give a fit but probably not a good one.
Gordon

Trip 
Measuring the inside diameter of an internal screwthread doesn't tell you the Minor Diameter of the screwthread, but may provide a reasonable approximation of that screwthread's Tap Drill Size, and adding the measured screwthread Pitch to the inside diameter may provide a reasonable estimate of the screwthread's Major Diameter.
I wrote this essay more than a decade ago, to explain the fundamental geometry of today's most common screwthreads, and have posted it on this and a number of other bulletin boards since then:
A sound understanding of screwthread geometry makes it MUCH easier to understand threadcutting.
I wrote the following essay to explain the geometry of the most common screwthreads; it's long, but I think it'll be worth the time for you sit down with a pencil and pad of paper and make sketches as you read through it:
There are three different forms of screwthreads that have been in widespread use in the industrialized world in the last century or so that we should talk about here, and probably several dozen more forms that I'll tactlessly ignore. All three of these threadforms  the Sellers (aka Franklin Institute, National, American National, and US Standard), the Unified, and the ISO Metric  are descended from an earlier form, the "60 degree Sharp V".
The 60 degree Sharp V threadform has been obsolete since the 1800s, but it provides a good place to begin our discussion.
Let’s start by imagining a bolt with a 60 degree Sharp V thread. Now imagine that we cut that bolt lengthwise, so that the plane of the cut contains the central axis of the screwthread, and then look closely at the profile of the thread in the plane of the sectioning cut.
If we were having this discussion over a cup of coffee in the breakroom, I'd be drawing sketches to show you what I'm trying to explain. Since we aren't, though, you might want to get out a pencil and paper and try to make your own sketches while I talk.
The Sharp V screwthread profile looks like a row of equilateral triangles, each with one side resting on a straight edge with their points pushed together. All sides of these triangles are the same length, so the “points” of successive triangle away from the straight edge are separated by the length of the triangle side . . . we'll call this distance The Pitch of the screwthread.
There is another row of these little triangles on the opposite side of the sectioned bolt, offset along the length of the bolt by a half Pitch, with their notonstraightedge points pointing in the opposite direction from the first row's notonstraightedge points.
Following so far? Ok, now lightly draw two parallel lines, one connecting the awayfromstraightedge triangle points on one side of the bolt and the other connecting the awayfromstraightedge triangle points on the other side of the bolt. These two line are separated by the Major Diameter of the screwthread.
The onstraightedge sides of the two rows of triangles are separated by the Minor Diameter of the screwthread. The awayfromstraightedge points of each row of triangles are off of the straightedge by the Single Depth of Thread, which is The Pitch x Cosine 30 degrees.
The Double Depth of Thread is twice the Single Depth of Thread, 2 x The Pitch x Cosine 30 degrees. The Double Depth of Thread is also the difference between the Major Diameter and Minor Diameter.
If you were going to cut this thread on a lathe using a singlepoint toolbit with the compound rest slewed to feed along the flank of the screwthread, and assuming that you zero the compound when the sharp point of the toolbit just touches the alreadycuttoMajorDiameter workpiece, you'd have a complete threadform when you'd fed the tool into the workpiece by a distance equal to The Pitch. After all, all three sides of each triangle are the same length.
While the geometry of the 60 degree Sharp V screwthread is nice and simple, it has practical problems. The sharp point on the toolbit breaks or wears very quickly, the sharp ridges at the Major Diameter of bolts and Minor Diameter of nuts get banged up very easily, and the sharp grooves at the Minor Diameter of the bolts are "stress risers" weakening the bolt. By the 1860s the American industrialist and machine tool builder William Sellers proposed a modified version of the earlier threadform, one with 1/8 Pitch flats at both the Major Diameter and Minor Diameter, as a new standard.
This new threadform, the Sellers threadform, was fairly well accepted, but it didn't actually become the official US Standard threadform until well into the first half of the 20th century.
So let's modify those sketches. The general spacing and angles stay the same, but the new profiles have flats instead of sharp points at the Major Diameter and samesize flats instead of sharp grooves at the Minor Diameter. Both flats need to be 1/8 Pitch long, which reduces the length of the angled flanks AS MEASURED ALONG THE AXIS OF THE SCREWTHREAD to (Pitch  1/8 Pitch at the Minor Diamter  1/8 Pitch at the Major Diameter) = 6/8 Pitch = 3/4 Pitch.
The length of the flank is reduced by the same ratio, and the other Pitchdependent calculations are adjusted accordingly.
Flank length (alongflank infeed using slewedtofeedalongflank compound rest) for Sellers threadform = 3/4 Pitch.
Single Depth of Sellers Screwthread = 3/4 Pitch x Cosine 30 degrees.
Double Depth of Sellers Screwthread = 2 x 3/4 Pitch x Cosine 30 Degrees.
The Sellers threadform served the US's needs well enough until World War II, when the difference between the United States' and the British Standard threadforms created major logistical headaches . . . British equipment could only be repaired with Britishstandard hardware while US equipment could only be repaired with USstandard hardware.
Once WWII had been won, the US, Great Britain, and Canada (which, interestingly enough, had fifty years of experience struggling to supply the appropriate British Standard and US Standard hardware when and where needed) put their collective heads together to develop a single standard that all three nations would use. To "share the pain" of forsaking a traditional standard screwthread, a new threadform was developed that both the US and Britain would need to learn to use. This new threadform was called the "Unified" threadform, and it incorporates the easiertotool 60degree angle with flats at the Major and Minor Diameters of the Sellers screwthread, but with different proportions.
A decade later, the fundamental geometry of the Unified threadform was incorporated into what could be considered a metric version of the Unified form intended to replace the various European national standard threadforms. Since the International Standards Organization developed and promoted the new metric standard, it was christened the ISO Metric threadform.
The major difference between the Sellers and Unified threadforms is that the length of the flat at the Minor Diameter of the Sellers threadform was doubled to 1/4 Pitch for the Unified threadform. The flat at the Major Diameter of the Unified and ISO Metric threadforms is the same as the Major Diameter flat of the Sellers threadform, 1/8 Pitch.
So, for both the Unified and ISO Metric threadform the axial length of the flanks is reduced still further to (Pitch  1/4 Pitch at Minor Diamter  1/8 Pitch at Major Diameter) = 5/8 Pitch.
Flank length (alongflank infeed using slewedtofeedalongflank compound rest) of Unified and ISO Metric threadforms = 5/8 Pitch.
Single Depth of Unified and ISO Metric threadforms = 5/8 Pitch x Cosine 30 degrees.
Double Depth of Unified and ISO Metric threadforms = 2 x 5/8 Pitch x Cosine 30 degrees.
Minor Diameter = Major Diameter  Double Depth of Thread.
Well, that's the basic geometry of these screwthreads.
As you've already pointed out, the dimensions of real hardware are properly perturbed by allowances and tolerances. External screwthreads cannot be larger than the dimensions derived from the basic geometry, and internal screwthreads cannot be smaller than the dimensions derived from the basic geometry if the external and internal screwthreads are to fit together. The alongflank infeed calculated from the basic geometry assumes that the Major Diameter of the tobeexternallythreaded workpiece is right at the basic Major Diameter AND the flat on the toolbit is the proper width (1/4 Pitch for Unified and ISO Metric threadforms, 1/8 Pitch for the Sellers threadform) . . . or that the Minor Diameter bored into the tobeinternallythreaded workpiece is right at the basic Minor Diameter AND the flat on the tip of the toolbit is the proper 1/8 Pitch width (any of the three threadforms we've talked about).
As for the charts . . . even though the Unified threadform replaced the Sellers threadform as the official US standard threadform a half century ago, many of the tables in various "reference works" have been carried forward from edition to edition with values appropriate to the Sellers threadform.
I realize that my posting is longwinded, but I hope it's clear enough for you to follow. If not, post back and I'll try to answer your questions.

Originally Posted by John Garner
Trip 
Measuring the inside diameter of an internal screwthread doesn't tell you the Minor Diameter of the screwthread, but may provide a reasonable approximation of that screwthread's Tap Drill Size, and adding the measured screwthread Pitch to the inside diameter may provide a reasonable estimate of the screwthread's Major Diameter.
I realize that my posting is longwinded, but I hope it's clear enough for you to follow. If not, post back and I'll try to answer your questions.
This might help illustrate some of your points.
http://www.fms.dk/1.09.pdf
Gordon

Originally Posted by John Garner
Trip 
Measuring the inside diameter of an internal screwthread doesn't tell you the Minor Diameter of the screwthread, but may provide a reasonable approximation of that screwthread's Tap Drill Size, and adding the measured screwthread Pitch to the inside diameter may provide a reasonable estimate of the screwthread's Major Diameter.
I realize that my posting is longwinded, but I hope it's clear enough for you to follow. If not, post back and I'll try to answer your questions.
This might help illustrate some of your points.
http://www.fms.dk/1.09.pdf
Gordon

Originally Posted by Gordon B. Clarke
You're not the only one wondering where I was and why I've been "silent" the last 3 weeks LOL. My wife and I were on vacation in Texas the last 3 weeks enjoying Texan hospitality
PM or email me on the thread types and sizes you are interested in and I'll give you some suggestions/advice.
I've never had any customs problems with sending to the USA or any other country.
Gordon
Figured it must be something like that. I'll send you a message, thanks!
John, thank you for sharing that, great read and well written. Again, I could go with 'try it and see' but I have a passion for learning. I've read this twice now and will definitely be reading it again.
One thing to add, and I do appreciate the info presented, some of the outcome is skewed due to the dates you mentioned... I'm dealing with threads from 1939 (which may be made by the same tooling from years earlier). Looks like I'll have to do a bit more figuring and measuring to account for the differences. I wasn't fully aware of the actual form changes, I mean, I know about the designation changes, SAE, UNC, UNF, so on and so forth, the Whitworth headache, etc. but I honestly didn't know the origin of some of the changes nor the timeframes involved. Before this machine, everything I worked on or owned had a post 1950 manufacture date, not much to factor in on the previous used forms.
That said, will this cause a distinct difference, or do the varying tolerances/classes mitigate that to some extent. I've run modern taps to clean up the holes, didn't seem to have any issues, but those were all relatively standard. This is kind of an odd size/pitch and isn't something I'd have or would want to buy a tap for (or die for) so it will indeed be singlepointed. How critical is the 1/41/8 differences between the two forms, enough to regrind a tool to match, or at 20tpi is the difference minimal enough to BS through?
Again, can do the tryit, but I'm trying to learn all that I can to move forward, I can't afford a true career shift or to return to school to switch careers, so this is a second career and has to be done a certain way.

"There's the little problem that the tolerance on a thread bore diameter is about twice that of the thread pitch diameter and over 50% that of the OD tolerance on most threads. Pussying around might give a fit but probably not a good one."
Assuming everything is exactly to spec, which anyone who works making machinery repair parts will quickly learn it is usually NOT. My clearance was an example, I did not have a thread depth chart on hand in the living room. Needless to say, it's not rocket science and for the OPs particular task (holding a piece of clear plastic against about 1" of oil pressure head), this has taken longer to read than it would have taken to make the part, gold plate it and have the machine up and functional. There's a time and place for uber precision and there's a time to make parts that work.

Originally Posted by Mike C.
"There's the little problem that the tolerance on a thread bore diameter is about twice that of the thread pitch diameter and over 50% that of the OD tolerance on most threads. Pussying around might give a fit but probably not a good one."
Assuming everything is exactly to spec, which anyone who works making machinery repair parts will quickly learn it is usually NOT. My clearance was an example, I did not have a thread depth chart on hand in the living room. Needless to say, it's not rocket science and for the OPs particular task (holding a piece of clear plastic against about 1" of oil pressure head), this has taken longer to read than it would have taken to make the part, gold plate it and have the machine up and functional. There's a time and place for uber precision and there's a time to make parts that work.
Indeed Mike... using it as a learning opportunity as well. This time it's something I could probably just squeeze a bunch of RTV into and call it a day, but if I learn the specifics now, on my own project, when something pops up next, I'll have the knowledge to move forward.
Posting Permissions
 You may not post new threads
 You may not post replies
 You may not post attachments
 You may not edit your posts

Forum Rules

Bookmarks