Lathe threading math

[Harold_V]

Harold V --

I don't know if I should agree with you or argue with you.

Agree is best, and for many reasons. That's assuming that most folks don't get too caught up on the proper tool tip modifications so the threading tool complies to thread form for each pitch, which they don't. Hell, I don't do it all the time, and I know better! [img]/ubb/images/graemlins/blush.gif"%20alt="[/img]

My point is that if you cut by the formula everyone seems to be so caught up with, the pitch diameter may or may not be right. I'd suggest that anyone choosing to use the formula use it as a guide at best, never to gage thread sizes. If the minor diameter of a thread is too small, thanks to a pointed tool, the thread will still function. Whether it would pass inspection or not would be another issue. For the home shop guy, though, it's clearly not an issue, but a thread that won't fit a nut, or a mating part, certainly would be. That's the reason I suggest that threads be cut to pitch diameters, without using the major or minor diameters as reference points, and that's exactly what the formula suggests. If you use the major diameter as a starting point, and it is in error, the pitch diameter will have a corresponding error unless one compensates. That doesn't take into account the fact that the tip flat or radius is likely to not be correct. The number of mistakes I've made by using a surface as a reference point (not threading, but other operations) without further measuring tells me I'm right. The point of using the tool tip as compared to the major diameter of an external thread as the basis for cutting depth is further complicated by the angle one chooses to use on the compound. There's just too much to keep track of, only to be measuring a feature that won't tell you where the pitch diameter is anyway. Don't lose site of the fact that no go gages are truncated at the pitch line and tell no lies.

I've mentioned on more than one occasion that I cut threads for an extended period of time in a missile facility, and received my baptism by fire as a result. To insure thread form, all threading tools (this goes way back, long before inserts were available) had to be inspected by the QC department before you could make a first article, and then had to be re-inspected when they were removed from the setup for sharpening. QC inspected them with an optical comparator for angle and the appropriate flat at the point (that's all we were concerned with then, no radius) for the pitch required for the specific part being threaded. While we had both A and B gages, we often measured the threads with wires, depending on the situation at hand. The point is, if the threading tool is proper, the major diameter doesn't influence the pitch diameter, but the pitch diameter is distinctly influenced by the variations in the major diameter and/or the flat on the tool..

The bottom line on threads is that all features should be right, but when's the last time you saw anyone in the home shop worrying about the pitch diameter, the most crucial dimension of all?

Yes, John, I realize you know and understand what I'm talking about, because you said the same thing:

Your point about cutting a screwthread based on Pitch Diameter is excellent, and you are absolutely right about the effect of the toolbit-tip flat on the infeed. But Major Diameter and Pitch Diameter control is not the whole of threading; that flat (or optional radius) needs to be correctly sized and the flank angle correct in addition to the Pitch Diameter correct for the thread to be acceptable.

I maintain that a machinist or engineer who understands the fundamental geometry of screwthreads has a big advantage over the machinist or engineer whose knowledge of screwthread dimensioning is restricted to the limits and formulae in a table. If anything, the advantage of understanding fundamental screwthread geometry is greater in the home shop and in remote locations where the threading toolbit is a product of the machinist's knowledge and skill with a bench grinder.

No argument from me. Screw threads are amongst the more complex and tight tolerance of things generated in the shop, yet are treated as simple objects. The bottom line is that when machining them, measuring them by the most critical dimension, not the one easiest to measure, is the best way to go. Without checking the charts to see if I'm right, I'm pretty sure that the tolerance on pitch diameter is much more restrictive than the minor diameter, and for sure the major diameter. On the smaller threads it's not uncommon to have only a couple thou from one end to the other. That's the dimension that should be considered as critical (without disregarding thread form, for sure).

As an exercise, ask the next half-dozen machinists and mechanical engineers you encounter to describe the theoretical geometry of the Unified threadform, or if you're pinched for time, just ask them how wide/long the flat at the end of the toolbit should be theoretically.

In my 27 years of asking the latter question, I would guess that fewer than ten percent of the engineers and machinists I've asked -- all of them working in North America -- know the right answer. The correct answer is either another question: "For cutting an internal or external thread?" or is a conditional statement "For cutting an external thread the flat should be one-forth the Pitch, for an internal thread one-eighth the Pitch." (Incidentally, many current machine-shop textbooks don't answer this question correctly.)

I agree, not many know, nor understand, that of which you speak. Considering my lack of formal education, you could include me amongst them had I not had the real life experiences of which I've spoken. To make sure I know and understood proper threads when I was actively machining, I used my H28 manuals, which lack for nothing if you're willing to dig out the information.

You can thank modernization (CNC) for the decline in skills, which are no longer really needed. Why would a "machinist" need to know about thread form when all he does is apply the tool that he takes out of a package? Rarely does the modern day "machinist" have to sharpen a tool. Many home shop types, in an attempt to avoid the learning curve (sharpening proper cutting tools in general), are now running carbide, many on machines that clearly don't benefit by its use.

Incidentally (Mk II version), I don't think I've ever seen a 60-degree center gage with Double Depth of Thread tables containing the correct Double Depth values for the Unified threadform (developed in 1949 and incorporated into the US Federal and Military standards shortly thereafter); every one that I've noticed has listed values for the obsolescent-for-fifty-years U S Standard threadform.

That's an interesting observation. To be VERY frank, the only thing I've ever used the double depth for is in determining the length of the threading tool such that it will thread to a shoulder and provide a maximum amount of thread on the object. It's very useful in that regard. As a result, I don't really care how precise they are, for that wouldn't influence my thread. As I said, those of us that know and understand threading from the old school don't gage threads by the depth. We rely on gages or wires and measure the pitch line. That the thread tables, or the markings on a threading gage, are in minor error is of little consequence to me, and I assume for some others.

You're a rare cat, John. Hardly anyone I encounter discusses that which you just have.

Harold

[J_Tiers]

The bottom line on threads is that all features should be right, but when's the last time you saw anyone in the home shop worrying about the pitch diameter, the most crucial dimension of all?

Last time I saw it was the last time I cut a thread......

But I didn't use wires, I have some V-gages from Elisha Penniman Inc that have a set of tables of measurements for the various threads and fits. (I don't have thread wires, I probably ought to get a set. )

I usually check threads with them since otherwise I don't know what I cut or if I'm done. If it isn't particularly important I may just wing it, but I check if I want it to fit.

To wing it I usually turn to the correct OD and then cut until the crests look right, then check with gage (the nut). I know, the cutting throws up a burr, but it works for non-critical threads.

[Harold_V]

The bottom line on threads is that all features should be right, but when's the last time you saw anyone in the home shop worrying about the pitch diameter, the most crucial dimension of all?

Last time I saw it was the last time I cut a thread......

But I didn't use wires, I have some V-gages from Elisha Penniman Inc that have a set of tables of measurements for the various threads and fits. (I don't have thread wires, I probably ought to get a set. )

I usually check threads with them since otherwise I don't know what I cut or if I'm done. If it isn't particularly important I may just wing it, but I check if I want it to fit.

To wing it I usually turn to the correct OD and then cut until the crests look right, then check with gage (the nut). I know, the cutting throws up a burr, but it works for non-critical threads.

That's headed in the right direction, but we avoided the triangles for one real good reason. They are affected by thread form, whereas wires are not. It's conceivable to have a less than perfect thread angle and have to cut the thread too deeply (or even too shallow) in order for the desired measurement to come out. You effectively would be gauging the wrong part of the thread in that circumstance. That's why wires are used.

Incidentally, there's thread wires, and there's thread wires. You can buy a cheap set of wires that cover a multitude of pitches. They provide a small chart that details the wire diameter to be used for each pitch, and a constant that you add to the major diameter of the thread to be machined. The problem is it doesn't tell you where your pitch diameter really is because you have no idea what the constant represents, nor if the wire is measuring at the proper place on the thread, the theoretical pitch diameter. In some instances the wire is used for more than one pitch. They are better than nothing, however, and I have a set of them in my toolbox for emergency use. I don't have a full set of precision wires.

Proper screw thread wires are an ultra precision device, held in size to millionths, and are provided with a constant that is added to the pitch diameter you desire. That way you have a finite dimension for top and bottom tolerance, which makes it easy to know where your thread is. There is no guessing. It's been lots of years since I last bought a set, but I paid over $20 for three skinny wires when I last did. I imagine a decent set (one pitch size, or three wires) today would cost at least $40. Deltronic used to make them, as did P&W. I'm sure there were others. Van Kuren comes to mind.

By the way, I commend you. I'm not too impressed by hack methods of machining.

Harold

[Victor_R]

Gentlemen,

I've been following this discussion with some intrest as I did the plung-threading fiasco of last year. Having stayed out of that one, I just wanted to say that here that I agree with Harold about using thread wires as the most practial way of gauging external threads you are cutting. That is the way I was taught. And at the two companies I worked for, that was the only way it was done.

The first was Worthington Corp. (yes, the pump makers) I was at the service center where we repaired and rebuilt all of our products. Most all threading there was on pump shafts. Some small, some very large and very expensive. And the threads were for bearing lock nuts. Pump shafts are high stress items, and as such, we used radiuses on the root diameters to avoid fatigue cracks. Many times the roots were polished to remove tool marks. This applyed to shoulder radiuses also. The actual root diameter was not a big concern as long as there was proper clearence. It was the pitch diameter that mattered most. And we measured that with wires and big micrometers. We never used the lathe dials for any gauging of size. The only trouble we had with the wires was if one dropped into the chip pan and you spent ten minuets on your hands and knees looking for it. [img]/ubb/images/graemlins/frown.gif"%20alt="[/img]

Later I moved down the street to a German machine shop, General Machine & Instrument. This was a skilled job shop that did single items as well as small production runs. They also did Government contracts. It was a well equiped shop and did almost anything. There was also a QC department that verified everything just like Harold's place. And they had a thirty inch optical comparator too. It had a graticule with lines and circles and a sixty degree V in the middle. At that magnification you could see tool marks!

At GMI you were only allowed to use "Best" style of thread wires. Maybe not that brand, but that type as opposed to pee-dee wires. They come in a little plastic vile and are smaller than other types so they sit lower in the pitch diameter. I know the other types would have worked just as well as long as you adhered to their numbers, but the G-man didn't like them.

Yes it's fascinating geometry and nice to know. But I don't carry it in my head because I don't use it. If I need it, I too have a 1969 copy of Handbook H28 Screw-Thread Standards For Federal Services.

Victor

[Harold_V]

Gentlemen,

I've been following this discussion with some intrest as I did the plung-threading fiasco of last year. Having stayed out of that one, I just wanted to say that here that I agree with Harold about using thread wires as the most practial way of gauging external threads you are cutting. That is the way I was taught. And at the two companies I worked for, that was the only way it was done.

Thanks for your very nicely timed remarks, Victor.

I'm of the opinion that the information you and I have tried to convey is of little use or need to the bulk of the readers, but I have always strived to pass along the absolute best method, or perhaps the accepted method, of doing pretty much any operation. Knowing what is considered proper will always serve the reader well, and if there's some slack and a lesser procedure might serve the purpose, they can work accordingly. The tragedy is when someone learns the worst of all procedures and accepts them as gospel. That's one of the reasons I like to encourage the newbie to try to locate someone that is skilled and can pass along to them some of the tricks of the trade. All too many of the 'how to" books have been written by self proclaimed machinists that may have a flair for writing but have little knowledge of machine practice. Sadly, many of the self taught guys read these books and take what they are told as acceptable practice. Once learned, some of these things are difficult to abandon, and often yield poor results.

if one dropped into the chip pan and you spent ten minuets on your hands and knees looking for it .

Ok, time for another tip.

When ever you use thread wires, the first thing you do is clean out the chip pan. Dropping the wires is almost a guarantee. Trust me, Victor isn't the first guy to spend an afternoon on his hands and knees looking for a wire, which suddenly looks like the rest of the chips in the pan. I make it a policy to always empty the chip pan, and wipe it clean of oils. That way, anything you drop in the pan doesn't get lost.

There's an art to using thread wires, but it's easily learned, at which time using the wires is quite easy.

At GMI you were only allowed to use "Best" style of thread wires. Maybe not that brand, but that type as opposed to pee-dee wires. They come in a little plastic vile and are smaller than other types so they sit lower in the pitch diameter. I know the other types would have worked just as well as long as you adhered to their numbers, but the G-man didn't like them.

The G-man didn't like them because they didn't fit deep enough, a result of a compromise of size. The pee-dee (pitch diameter) wires are nothing more than commercial wire stock that is near a proper size. Better than nothing, but hardly proper thread wires.

As I understand it, the diameter of the wire is the precise diameter of the theoretical distance from flank to flank at the pitch diameter, so when the thread is within tolerance, that's the point that is being measured. Diameter of the wire is critical. Each pitch, therefore, has its own set of wires, unlike the cheap sets.

Not only do the proper thread wires come in a vial, but those from Deltronic also have a short, round plastic member within which you store a single wire, with each wire contained within one. The vial, in turn, comes in a nice plastic box for convenient storage. On the round plastic member there is permanently marked the actual diameter of the wire (to five places), and the constant that you add to the pitch diameter . The set I have before me as I type is for 18 pitch threads. The wire diameter is marked as .03207", and the constant that one uses is .04810".

The wire method is the absolute method of determining pitch diameter, thus the wires must be exact. Plug gages are so calibrated, using the three wire method, along with a supermike.

Harold

[len]

what is the math formulas for figuring out the depth and amount of infeed for "Sharp V Groove" threads?

I'm afraid this thread has gotten completely out of hand and, more importantly, probably has confused the original poster more than helped.

From my reading, I think John Garner's explanation is the clearest and makes the most sense. The poster wanted geometry for a sharp V thread. Visualizing an equalateral triangle, as John suggested, then using one side as the amount of infeed with the compound set at approx. 30 degrees is easy to see and understand. The rest of the discussion, while it might be technically enlightening, only serves to confuse.

For us self-taught machinists and tinkerers, getting the job done is sometimes the biggest part. Our work doesn't have to conform to mil standards, and we will never become expert machinists, as that would take a lifetime. It would be nice to have an expert at our side to tell us what not to do, and to provide us with an unlimited number of specialized and expensive tools that we need to do the job "right", but alas, that is a pipedream. Learning from a well-written book written by an expert machinist is the closest we will come to that (and reading this forum). I am happy with this compromise, as I have a dozen other hobbies I like to devote time to.

len

[Harold_V]

I'm afraid this thread has gotten completely out of hand and, more importantly, probably has confused the original poster more than helped.

From my reading, I think John Garner's explanation is the clearest and makes the most sense. The poster wanted geometry for a sharp V thread. Visualizing an equalateral triangle, as John suggested, then using one side as the amount of infeed with the compound set at approx. 30 degrees is easy to see and understand. The! rest of the discussion, while it might be technically enlightening, only serves to confuse.

If the comments on thread measuring have served to confuse, that is most unfortunate, for the fact is that threading exclusively with the use of geometry is bound to produce threads that are not proper, but an understanding of thread measurement would allow for the correction of errors in the application of the theory.

If you'll take the time to read what has been posted and understand what has been said, it might enlighten you to the point where it would make sense. From the perspective of an engineer, where one may desire to understand what a thread is and why it works, the information gleaned from geometry is good and proper, but in the real world of application (on the machine), the information is relatively useless unless applied along with proper measurement. The harsh reality is that sharp V groove threads exist only in theory. They aren't found in the shop, so the application of the theory doesn't produce a proper thread.

So then, the use of thread wires serves as a method of measuring the application of the theory (the geometry), nothing more. What's so hard about that?

It's as simple as this, len. If you were to apply for a job in any major production facility and apply the theoretical process to threading, assuming your threads were to be subjected to inspection, you would likely not hold your job. What your theory suggests is that one should never use a micrometer to measure a diameter, for that would be confusing. It's not confusing to pick up a surface with a tool tip and from that reference point all turns should then be accomplished by the dial, with no need to ever measure to verify that the diameters are turning out as desired. Do you make components that way? If not, why not? Can you provide as much as a single reason why one would not want to measure a thread?

For us self-taught machinists and tinkerers, getting the job done is sometimes the biggest part. Our work doesn't have to conform to mil standards, and we will never become expert machinists, as that would take a lifetime. It would be nice to have an expert at our side to tell us what not to do, and to provide us with an unlimited number of specialized and expensive tools that we need to do the job "right", but alas, that is a pipedream. Learning from a well-written book written by an expert machinist is the closest we will come to that (and reading this forum). I am happy with this compromise, as I have a dozen other hobbies I like to devote time to.

Being busy and having several hobbies may or may not be a good justification for avoiding doing a job properly. What you apparently do not understand is that you are being offered, at no cost to you, the opportunity to learn a process that is accepted (you can read that as "mandatory") in industry. Whether you work in industry or not, the information is useful, for it is the basis for how we, as a society, produce components that are guaranteed interchangeable. There is little else that would prompt the trouble that the government has gone to in order to compile the information that comprises the charts, the information that came from an understanding of the geometry of threads. We apply the geometry through the use of thread wires. To the man, all of us can afford a cheap set of wires, which permit the measurement of threads, even if not perfectly.

If the book you're reading, the one you suggest came from an "expert machinist", does not detail this information, I'm afraid you don't have a well written book as you suggest, and are a victim of a person that doesn't understand machining nearly as well as he/she should.

Harold

[ferocious]

as a budding young machinist(I'm only 56) I'd like to make a few observations-

I agree everyone should learn the proper way to measure and cut threads, as Harold V suggests. Everybody should do it once just to learn.

Then get busy and learn the short cuts, such as setting up the tool post to feed the correct cutting depth, in order to get the job at hand done as quickly and easily as is compatible with what needs to be done. i.e. turning a short thread to hold on a hand wheel with a hardware store nut certainly does not require thread guage wires and supermikes. But cutting missile parts or highly loaded pump shafts probably does. Match the tools and technique to the job at hand!

[Jacin]

Match the tools and technique to the job at hand!

The only "problem" with that logic is that WHEN the time comes for one of us amateurs to "step up to the plate" and produce some "industrial quality" results - will we be able to? Sure most of us rarely NEED the type of accuracy that Harold and others are so adament we strive for, BUT the way I see it that it IT IS MORE IMPORTANT FOR US AMATEUR'S learn these practices for the simple reason that we DON'T have the luxury of honing our skills everyday. Given this if "we" embrace shoddy practices from the "get go" then what hopes do we really have that when we HAVE to produce the accuracy needed.

Learn the basics - learn the RIGHT way - leave the short cuts for the experts.

But I suppose it all boils down to "different strokes for different folks"

Some people see No Problem outfitting their shop full of Harbor Fright materials. Me personally I BUY the BEST I CAN AFFORD. That way when I am STUCK between a rock and a hard spot - I can at least count on my tools. I see machining as no different - I strive for perfection and while I don't ever achieve it I can hang my hat up and think I've done a job I can be proud of. Those who settle for less - well - welcome to being average. In today's unstabil job market - just average - ain't gonna let me sleep too good.

To the origional poster - let's hope "we" didn't confuse him -but it's UP TO HIM to ask for clarity - if he needs it. Personally I almost always prefer the COMPLETE answer - I can at least be assured of sucess THAT way.

Give me a fish - I eat for a day.....Teach me to fish - I eat a lifetime.

And FWIW I have (almost) without exception measured my threads at home - yep even for the piddly bracket. Frankly, I NEED the practice!!!

Your mileage may vary.

[J_Tiers]

Well, I don't think there is a simple answer other than measuring.

For one thing, it is perfectly obvious to me that infeed alone is totally meaningless.

1) unless you know exactly what the OD is, infeed has NO REFERENCE, and so indicates no size.

2) Infeed does not account for spring, nor for screw error, nor for errors due to less than perfect form, off-center height etc. obviously the latter shouldn't happen, but spring means you don't know your infeed is the same as the actual cut.

Essentially, infeed is "open loop".

Per wires....

As I understand the thread wires, each TPI / Pitch must have a specific wire size, or it will not contact at the pitch line (which would actually be at an angle to a diameter across the wire, btw, due to the V angle).

A small set of "fits all" wires is probably only minimally better than the triangles, as it too will assume good form if it contacts off the P-D.

Speaking of the triangles vs wires: It seems that the wires might also lie, as a thread might be perfect at the pitch diameter, and wrong elsewhere (for instance a "bulgy" V wouldn't interfere elsewhere) . Then the wire might contact at right height and indicate right pitch diameter but the thread could still be off.

It seems that th thread must be inspected both for pitch diameter and for basic form in order to be known correct within tolerance. A gage should pick up most such problems, but I think even it needs a form inspection, unless it has really comprehensive go and no-go criteria. Might take a couple gages, but just one look on an optical comparator to verify form (and maybe even P-D.)


A last thought, if you didn't have your handy table, it should be possible to re-generate it. Any given size of wire in a V will sit in a predictable place, and thus can be calculated. if I recall, the calculation is a bit onerous though. I calculated a related thing, (chord of circle to volume/area remaining) and it wasn't nice to do.

So any wire of known size that fits close to correctly COULD be used in a pinch if you do the math. I'll hazard a guess that Marv Klotz has a program for it........

[Harold_V]

as a budding young machinist(I'm only 56) I'd like to make a few observations-

I agree everyone should learn the proper way to measure and cut threads, as Harold V suggests. Everybody should do it once just to learn.

Then get busy and learn the short cuts, such as setting up the tool post to feed the correct cutting depth, in order to get the job at hand done as quickly and easily as is compatible with what needs to be done.

I gather, from your comments, that you drive the freeway at a given speed just one time, at which point you toss your speedometer and drive your vehicle blindly from that day forward, secure in the knowledge that you already know how fast to drive.

That's exactly what you're proposing where chasing threads is concerned, and that doesn't work. When you have a better understanding of thread form and tolerance in the variable features, it will help you understand why. It's all a function of the fact that threads are discussed in the terms of a sharp V, but they are not machined as such. Without the use of an optical comparator, I suggest to you that you can't judge the depth close enough to be effective, assuming you have the slightest interest in producing a thread that is within respectable limits.

There's one other point I'd like to discuss with you. There are no "short cuts" to machining. Certainly disregarding dimensions couldn't be one of them if there were any, especially with threads. If you would like to learn to run machines, nothing will serve you better than learning and understanding the basics. The short cuts, such as they are, come from experience, from the ability to apply that which you have learned, effectively. Holding your mouth "just so" while you're cranking your handles will yield nothing more than a tired mouth. Ignoring proper procedures usually yields junk work.

i.e. turning a short thread to hold on a hand wheel with a hardware store nut certainly does not require thread guage wires and supermikes. But cutting missile parts or highly loaded pump shafts probably does. Match the tools and technique to the job at hand!

The information that has been provided is intended to help those that have no clue, how threads are properly measured, which would allow them to apply the concept at their level, so they don't produce parts that don't function as hoped. You do that every time you cut a thread and use a nut (ring gage). Why wouldn't you want to do the same thing when cutting a thread for an object that you can't fit to the part while it's in the machine? It matters not where this theoretical part goes, it might be for your old rusty lawnmower. You still want it to fit! That's what thread wires do for you, they measure the part so you know that it will fit when it is removed from the lathe.

I can't speak for you, but I can put a chased thread back in a lathe and pick up the thread and remove more when I find it doesn't fit, should that happen. I can do it all day long and do it without scrapping the part. I can do it because I am a machinist, one that knows and understands the process, one that first ran a lathe at the tender age of 13, and have lived a life that is 8 years longer than yours. Here you have an opportunity to learn a procedure that would permit you to avoid having to put that thread back in the machine, which can be taxing, at best. If you're wise you'll read and understand everything that has been posted in that regard, and keep it in mind for the job in the future when you desperately need it.

If you choose to disregard this information and reduce it to a level of no importance, should you run into a wall and need help, why would you expect me, or any of the others that already know and understand proper procedures, to bail you out?

These processes are not those of the missile industry, they are the recognized processes used in machine shops, some of which do work for the missile industry. I trust you get my drift.

Harold

[Doug_C]

Everybody should do it once just to learn.

Then get busy and learn the short cuts, such as setting up the tool post to feed the correct cutting depth, in order to get the job at hand done as quickly and easily as is compatible with what needs to be done. i.e. turning a short thread to hold on a hand wheel with a hardware store nut certainly does not require thread guage wires and supermikes. But cutting missile parts or highly loaded pump shafts probably does. Match the tools and technique to the job at hand!

The whole point of spending time on this board for those of us with experience, is to be helpful and offer guidance to those with little to no experience in doing operations with the least amount of risk. Legitimate short cuts need to be learned from doing it correctly in a skilled fashion.

If you only learn to do it right once. You rarely gain any skill to know the difference why it should be done that way or comprehend what shortcuts can leave undesirable results. Sort of like driving in the dark with no lights and then put on some sunglasses.

I'd bet even Harold's tolerances have lightened up with no one looking over his shoulder. But he has the know how and is trying to be helpful in the bigger picture. I'd be right along side his description in passing along important details that the inexperienced would obviously miss. I'd at least suggest you don't discount it now. You may very well need it at some time. Those bad habit shortcuts formed may get in the way then though.

With Len's statement of the original poster getting confused? I think what creates the confusion is the mis-information that a good thread can be cut the first time without knowing the true dimension of point A to get to the desired dimension of point C. Guiding anyone around point B because it is way to involved to be of much use, clouds the whole explanation.

For that matter a triangle file can be used to cut a thread. We could even put a stop on it to know how far it should cut. Only the totally naive would take us up on that kind of guidance.

Relying on a constant formula for infeed is not much different and MAY get you close. The unknowns in the mix MAY not allow this to work as expected. Glowing results are based on removing questionable elements of prediction. Not throwing it all to chance.

To be realistic in offering SKILL that has been hard earned on the road to success is given pretty freely here. Sometime we even take a request and turn it into more information than the poster bargained for. Going off an a tangent seems unavoidable at times we misunderstand the real area of help requested.

Since the postings here are not private. I think it is has much greater potential to offer not just the originating poster an answer, but to inform others who may have more in mind than just short order focus.

The simplest answer would be, just use a die! [img]/ubb/images/graemlins/grin.gif"%20alt="[/img]

DC