Post By Forrest Addy
Newbie, pre-threading calculation questions.
I have never completely understood how to do the calculations before beginning to 60 degree single point thread on the lathe, as an example, trying to achieve a correct external and internal 2A & 2B thread that will not only mate with each other but will have a high probability of mating with the opposite gender of any other correctly made thread of the same size, TPI and class. In addition, I have never understood how to correctly calculate the external and internal thread depths when using different profile tools each designed to cut the same TPI. Also, how much, before beginning to cut the threads, to correctly alter the workpieces major and minor diameters between the maximums and minimums for both external and internal threads as shown in the MH book for different diameter and class of threads. Please answer questions 1,2 & 3 below in as much detail as possible, perhaps using a 1”- 8 (2A) and (2B) threads in 1-3/4” 304 round stock for examples. The compound set at 29.5 degrees.
(1) Carbide: The industry seems to offer carbide sharp V point (no flat) inserts for external and internal threading which will cut a range of TPI. They also offer full profile inserts, which are TPI specific. If one were to use the sharp “V” (no flat) insert to cut both the external & internal thread to 100% of the recommended full thread depth, would the two join together (2A and 2B) as smoothly and be as strong as if one used a full profile insert? Probably not, would one then only need to reduce the percentage to get the desired result? If so, what might that percentage be and how would one calculate the new thread depth for both the external and internal thread based on that new percentage? If not, what would need to be done?
(2) HSS: Training books seem to recommend putting a flat on the point of a HSS 60 degree external and internal threading tool. The width of the flat on the point is to be in relation to the TPI the tool is intended to cut. Does one need to change the recommended depth of thread for both the external and internal thread to allow for that flat width? If so, how would one calculate the new thread depth for each flat width for both the external and internal threads?
(3) Workpiece Major and Minor diameters in MH book: Relating below to 2A and 2B threads, how does one calculate how much to correctly alter the workpieces major and minor diameters before beginning to cut and bore the external and internal diameters and before starting to cut the threads. For each thread diameter and TPI the MH book shows a maximum and minimum diameter for both the major and minor diameters. How does one use this information to know what size to pre-cut and bore the workpieces too before threading. Does one pre-cut and bore the internal and external workpieces to the mean between the maximum and the minimum or by some formula, fixed amount or other?
Please all chime-in, these correct thread questions have vexed me for a long time perhaps to the point I’m seeing things to be more complicated than they are. Let me know, Thanks!
At one point I made some calculations and produced this table. Maybe it will answer some of your questions.
TPI=Theads Per Inch
Use your pitch micrometer or wires at the end stages to get within the specified range.
P.S. Originally, I was taught to use 0.71/TPI formula for the total infeed depth when using compound at 29-degree angle. We used HSS tools sharpened by hand. Now I, mostly, use universal threading inserts (8-48TPI) and find the 0.87/TPI is quite close to what's required (calculated from the nominal diameter).
I probably don't know the correct answer since I first ran a lathe in only in 1955, but my practice has been to cut it until it starts to look like a thread and then check with any one of a multiple of ways to check threads - like ring gauges, over wires or thread mics - the ones I own checking directly the pitch diameter.
I have never completely understood how to do the calculations before beginning to 60 degree single point thread on the lathe, as an example, trying to achieve a correct external and internal 2A & 2B thread that will not only mate with each other but will have a high probability of mating with the opposite gender of any other correctly made thread of the same size, TPI and class
Having been in a similar state of confusion I found the only way to get things straight was to spend some quality time drawing things out from the handbook data tables at a large scale so I could actually see what was happening to clearances with different fits, tolerances and so on. Eventually the penny dropped and now I can make things as per the published data. Just don't ask for a coherent explanation!
You did not mention pitch diameter. Pitch diameter plays a major role in the proper mating of the male and female thread.
The information below is for OD threads. If I get time I will write about ID threads later.
1) All the carbide inserts I have seen are NOT a sharp V point. (Except for very small threads). The inserts have a radius on the point. You have to know the radius to get the exact answer for some of your other questions. Look in the manufacturers catalogs to find the radius on the insert you are using. The radius will usually determine what range of threads it will properly make.
The threading inserts I use have the following radius and following range of threads specified:
.003" - 44 tpi to 14 tpi - OD threads
.004" - 36 tpi to 8 tpi - OD threads
.007" - 30 tpi to 6 tpi - OD threads
.014" - 11 tpi to - 4-1/2 - OD threads
Note: Making a thread with less tpi then specified above will make a function but weaker thread. Making a thread with a sharp V point will cut any functional tpi but weaker thread. Using a full profile insert uses the maximum allowed insert radius for a specific tpi and will result in a stronger thread. If you want maximum strength, roll the thread, not cut the thread.
2) A flat on the point of the tool is allowed for making a thread if it is the proper size. I do not use a flat point. The Machinery Handbook will give you enough information to calculate the proper size of the flat.
3) To start, you need to get the major diameter and the pitch diameter for the size and class of thread from the Machinery Handbook or other suitable sources. The minor diameter is specified only as a maximum, which must not be exceeded for a proper functioning thread. Use the following formula to calculate the minor diameter:
Minor diameter = Pitch diameter - (.866 * pitch) + (2 * Insert radius)
Pitch diameter = Mean value for the size and class of thread from Machinery Handbook
Pitch = 1 / tpi of threads
Insert radius = radius of insert
Example - 1.0 - 8 2A OD thread
Pitch diameter from Machinery Handbook = .9168 max + .9100 Min / 2 = 1.8268 / 2 = .9134
Pitch = 1/8 = .125
Insert radius = .007
Minor diameter = .9134 - (.866 *.125) + .014 = .9134 - .10825 + .014 = .81915
Major diameter from Machinery Handbook = (.9980 max + .9830) min / 2 = 1.981 / 2 = .9905
Height of thread = (Major diameter - Minor diameter) / 2 = (.9905 - .81915) / 2 = .085675
Use this value if your compound is set at 0 degree and your dial reads a radius value.
Double this value if your compound reads a diameter value.
Infeed length for compound set at 29.5 degree = Height of thread / Cosine 29.5 degree
= .085675 / .87036 = .0984
Use this value if your compound is set at 29.5 degree and your dial reads a radius value.
Double this value if your compound reads a diameter value.
Note: These numbers were calculated using the mean values of the pitch diameter and the major diameter. In theory, any value between the max and the min should create a functioning thread. Machining a pitch diameter and/or major diameter different from mean will require recalculating the infeed values.
All this information was based on data from the Machinery Handbook. The formulas I originally created were created using trigonometry and algebra and reducing them to their simplest form. The formulas were double check using Autocad to see if the values from Autocad matched the values from my formulas. Hopefully, I did not make any mistakes in transferring the information to this reply.
I have been using the calculations for the minor diameter for programming CNC for the last 20 years.
For Internal threads
Minor diameter = Pitch diameter + (.866 * pitch) - (2 * Insert radius)
I understand all this but have found that there is software that does all this for you.
Mine was bought here in the clasifieds (thread pal).
Best money I eaver spent.
ANSI B1.1 is THE spec on Unified 60 degree V threads. Much of the important stuff it contains is included in Machinery's Handbook and similar compilations. It all starts from the Standard Form and expands from there to all the finicky details. Chasing the details is counter-productive unless the Standard Form is studied and understood.
The despised Metric world whose Standard Form is very like the Unified Standard Form. In all these forms root and tip flats are an essential part of the form and their correct rendition in the finished product directly affect thread strenght and reliability. Careful attention should be paid to the form and symmetry of your product threads if they are to comply with the standard and perfrom to specifications.
This linked Wiki entry aint bad. It serves very well as an entry level tutorial on screw threads. There's a few faux pax but as I said, it aint bad. http://en.wikipedia.org/wiki/Screw_thread
Many folks working in the isolation of their home shops can with some justification contend they can ignore standards; what they make only has to suit and fit mating parts they make themselves. Inevitably the outside world intrudes so in theory the home shop machinist has to be at least conversant with specs and fits. Ball bearings and bearing nuts are a prime example.
As a hobbiest, I have only cut threads less than 30 times over 20 years. I have had many do overs, but I am usually successful in the end. I keep my copy of the machinist handbook close with a bookmark in the threading page. Take a scrap piece and have some fun and practice, practice, practice, it will be the best time spent learning how to do it, while getting more in touch with your machine.
Originally Posted by cash register
AMEN!! How often I've heard the dread words: "I have 30 hour making this part and I'm ready to cut the threads. Where do I start?"
I've been a machinist since the rocks were soft and any time I need to do anything I'm put of practice on (welding, threading, sex, etc) I practice on the theory I have lots of remnants to use for practice but only one part in progress. Practice in the end is the cheapest form of insurance.
Forrest, to me there is nothing more gratifying than screwing up one piece, only to make second one successfully. I count the time taken t do it as the cost to my education.
im working in a repair shop working on manual lathe and a new cnc one.
so for the external thread i usually aim for the major diameter minus 0.005 (this is within the tolerence for thread up to 6 inch or so)
after that for the depth of the cut a simple formula like this. 0.6495xTPI will give me approximativly the good depth of the thread. this is not accurate to a 0.001 so youll have to double check it with thread micrometer or wire gage but this formula is realy helping me out for the cnc lathe since its a good start and you just adjust your offset and everything will be fine for a long time.
I am in the same boat as you. In fact I have just spent the better part of the day today trying to understand the same concepts (hence finding this post thru a google search) I did run across a very helpful explanation from a member John Garner on the home shop machinist site
Internal Threading Help - Calculating bore size
His article, plus the illustration in the machinery handbook 26 ed. online here under Threads and threading has helped a few bulbs lite up
Machinery's Handbook 26th Edition
Don't let threading intimidate you - all it is, is a diameter with a 60 degree v cut in it at a specific rate of travel. Aim for minimal clearance and with some practice you should be able to get threads that fit together with almost no slop