Threading Formula

E

egapelr

Registered
Registered
Joined
Aug 25, 2016
Messages
4
I write this note with the hope that you veteran machinists will be able to enlighten this hapless newbie. Newbie only as it pertains to lathe work and certainly not to my age. I refer to the calculations required to cut threads on my Atlas 10 inch lathe. Lets assume that I want to cut 16 TPI on a 3/8 inch rod. The tables found in the "Manual of Lathe Operations" provides the following information. Major diameter = 0.375, Minor diameter = 0.2938, Pitch = 1/16 = 0.0625, Single Depth of Thread = 0.0406. Assuming the compound is set at 30 degrees then the manual states that the depth of compound feed should be 0.054 for a Vee Form Tool.

I have read in other letters/publications that the measure of the depth of the compound slide travel is easily calculated by multiplying the pitch by Cos(30) which is 0.866. This in fact seems to work but I am befuddled by the math. Although its been a long time since I studied trigonometry I still understand the Pythagorean Theorem where the square of the two sides adjacent to the right angle of a triangle will equal the square of the hypotenuse which in this instance is the distance traveled by the compound slide. Another means of calculating the hypotenuse is to use the accepted formula Cosine(30) = Adjacent Side/Hypotenuse. This formula is found in math manuals and the Machinery's Handbook. If the pitch is adjacent to the 30 degree angle of the compound then Cos(30) = Pitch/Hypotenuse. Simplifying the formula then the Hypotenuse = Pitch/0.866. The answer by this method is 0.072. Note that the Pitch is divided by 0.866 and not multiplied as suggested by others.

Obviously the "Manual of Lathe Operations" has the correct values but I am stumped as to why I get a value of 0.072 using the Cosine formula and the square of the adjacent sides. Mathematically I am unable to understand how a value of 0.054 is obtained. I appreciate and thank everyone who will take the time to educate me.
 
I think you would find that doing it by math is quite impractical; If you want to cut threads, all you need to do is cut the part to OD size and feed in with the compound at 30 deg. and take succeeding cuts until the thread nearly comes up sharp, then try for fit with a nut; I usually run a tap through a nut that I use for a gage to make sure that there are no burrs in the threads; when the thread fits the nut, I take a mill file and take a slight pass over the threads to remove any burrs, then another pass with the tool without any infeed to remove any burrs set out by the file. If the thread is an odd one, and I have a tap for it I make a gage to try the thread with; if it is relativly large diameter, I rough out the thread with the lathe and an internal threading tool, and finish it with the tap; if I don't have a tap, I make a plug gage to 3 wire size or thread mike, and use that to make the ring gage.
One other thing about compound depth is that it would only work with a sharp vee thread, which is not a desirable thing to use due to the sharp point is not durable in terms of tool wear; the tools do not hold up well. I use several tools for threading with different width flats on the points, one may be nearly sharp for fine threads, but I would at least stone a tiny flat on its point.
 
egapelr said:
I write this note with the hope that you veteran machinists will be able to enlighten this hapless newbie. Newbie only as it pertains to lathe work and certainly not to my age. I refer to the calculations required to cut threads on my Atlas 10 inch lathe. Lets assume that I want to cut 16 TPI on a 3/8 inch rod. The tables found in the "Manual of Lathe Operations" provides the following information. Major diameter = 0.375, Minor diameter = 0.2938, Pitch = 1/16 = 0.0625, Single Depth of Thread = 0.0406. Assuming the compound is set at 30 degrees then the manual states that the depth of compound feed should be 0.054 for a Vee Form Tool.

I have read in other letters/publications that the measure of the depth of the compound slide travel is easily calculated by multiplying the pitch by Cos(30) which is 0.866. This in fact seems to work but I am befuddled by the math. Although its been a long time since I studied trigonometry I still understand the Pythagorean Theorem where the square of the two sides adjacent to the right angle of a triangle will equal the square of the hypotenuse which in this instance is the distance traveled by the compound slide. Another means of calculating the hypotenuse is to use the accepted formula Cosine(30) = Adjacent Side/Hypotenuse. This formula is found in math manuals and the Machinery's Handbook. If the pitch is adjacent to the 30 degree angle of the compound then Cos(30) = Pitch/Hypotenuse. Simplifying the formula then the Hypotenuse = Pitch/0.866. The answer by this method is 0.072. Note that the Pitch is divided by 0.866 and not multiplied as suggested by others.

Obviously the "Manual of Lathe Operations" has the correct values but I am stumped as to why I get a value of 0.072 using the Cosine formula and the square of the adjacent sides. Mathematically I am unable to understand how a value of 0.054 is obtained. I appreciate and thank everyone who will take the time to educate me.
Click to expand...
I created an Excel spreadsheet which calculates the depth of cut for the compound set at 29.5º. It is in a post #7 in this thread. https://www.hobby-machinist.com/threads/math-help-needed-for-threading.66801/#post-557625
 
egapelr,

First, as the fine print in the table says, the 0.054 is for a compound angle of 29 degrees, not 30. Second, the OD of the 3/8"-24 male thread is less than 0.375 by an amount that with a Vee-form threading tool will make a Unified thread form on only the OD so that it will fit a nut made as either Unified or Vee-form without metal to metal contact. I didn't try to find where in Part 7 it gives what the OD should be (if it's even still in there) but pick up any 3/8"-24 US or UK made bolt and put your calipers on it and you will find that its OD is less than 0.375". Or to put it another way, the actual source of the 0.054 is shrouded by the fog of history.

Robert D.
 
Set compound at 29.5 degrees, Not 30, you will get a better thread by cutting on one face at a time and not both side of the V at the same time, done it this way for 50 years, GO to Youtube and type in "Joe Pie" watch his videos on single point threading, Joe understands threads. Then get some Al and go to the lathe and make threads all day long for practice and understanding.
 
Many thanks to all of you practical machinists that have responded to my query about threading. I agree with all of you with regards to the 29 degree angle of the compound and the need to more or less ignore the math and rely on the end results. That being said no one provided the answer that I was looking for which was how the distance of feed for the compound is determined. I found that the answer involves simple trigonometry. The length of travel of the compound is actually the hypotenuse of a right-angle triangle with the angle of the compound next to the x-axis set at 29 degrees. Depending on the type of tool used (N.F. or Vee form) the table lists the single depth of thread for each tool. The formula to determine the hypotenuse is Cosine (Angle) = Adjacent side/Hypotenuse. The Cosine of 29 degrees is 0.875. The formula simplified is then;

Hypotenuse = Adjacent side/ 0.875. The adjacent side in this instance is the single depth of cut for either type of cutter used.

Try this and you will get the exact answers as published in the table. I'm not sure where the formula Cosine(angle) X Pitch originates but I suspect that it works somewhat due to the close relationship between the depth of cut to the pitch.

If you determine the distance your compound will travel along the x-axis when set at 29 degrees then you can then extrapolate the amount the compound dial needs to rotate to achieve the desired depth of cut.

All this may seem like overkill to most of you but I just needed to satisfy myself that the numbers listed in the tables had some scientific merit. Sorry if I seem a bit anal about this and I can assure you that my threading still needs a lot of practice despite this dubious knowledge.

Thanks again to all of you
 
Yes, you have the math correct. I have cut threads based on compound feed calculation. Nevertheless, I find when threading that having a "go gauge" is essential. It may just be a nut or bolt. I ideally it is the mating part. There are so many variables when threading like the spring in the tool or the work that hitting a really tight thread is hard to do with just using the compound advancing by the numbers. I am not sure I can set my compound to within 1 deg! The fit of the gauge often determines whether I take that extra spring cut or not.
Robert
 
You must log in or register to reply here.
Back
Top