• posted
Hi,
I'm trying to understand how the various angles relate when setting up
which I've heard elsewhere- the math seems to work and suggests
(assuming I did it properly) the thread is cut a few thousanths extra,
presumably to make sure the outer edges of the threads are cut clean.
However I don't understand the purpose of the 30 degree compound
setting- is it so the cut is primarily taken by only one edge of the
tool? And second, why 30 degrees? I suspect its pretty simple
geometry that I'm overlooking- but I'm a newbie too...
Thanks,
Gregm
• posted
Most do 29 degrees which can be even more difficult to comprehend. In truth, the lathe cuts better when only one edge is doing the cutting as the bit won't work the slack back and forth while going down the cut. As such, you will get a better smoother cut for the same setup. Having the 29 degree angle also keeps the backside of the cut tight against the work with a light scraping of the surface. Note that the actual position on the metal of the thread as to where the start point is is pretty irrelevant so the cut can start at one point and gradually move around as the cut goes deeper without any problems.
-- Bob May Losing weight is easy! If you ever want to lose weight, eat and drink less. Works every time it is tried!
• posted
Try using .750 /TPI for NC/NF threads if you are using the compound for infeed with a 29 degree offset. If your material is within specs for the nominal or called bolt sizes, that will usually give you a finished thread that will take an hardware store nut.
Actually, 29 degrees (measured from perpendicular to the center line) is better than 30 because that gives some clearance between the material and the cutting edge as you move away from the point of cut.
You are right about the rest of it as far as it lightening the load on the cutter and producing cleaner threads.
• posted
Greg, I'm providing two links to another forum. If you'll take the time to read each of the threads you'll gain some very good insight to how and why you set up to chase threads. This will save you a lot of grief and agony, and is better spent time than others posting redundant information.
There's some wonderful information, including one very nice drawing that shows in clear detail what's wrong with setting your compound at the wrong angle. I highly recommend you read everything and save the information for future perusal.

At the bottom of each page you can click on another post related to the thread.
Enjoy!
Harold
• posted
information
My .02 cents
You do not have to set the compound at 29.5 (or thereabouts) degrees but you do have to understand what you are doing when you do whatever it is that you do. IE I believe that it is DoN that does all his CNC threading without using the compound, using a straight in/out cross feed movement only.
The drawing on the first link, taken together with what the man said clearly indicate that the compound was set at 30 degrees off of the axis of the part and not 30 degrees off of the axis of the cross slide.
So in his words, he started the cut with the compound which formed a very wide, shallow cut with a 30 degree left face and a 60 degree right face. Then he finished with a straight in feed with the cross slide which gave him the proper 60 degree thread form shape but sadly the cutting he had already done with the compound had already sliced off a 60 degree angle segment from the top of what should have still been there.
Bill D
• posted
Thanks! Those 2 threads are really informative. I've not done internal threads yet- you've saved me at least one newbie mistake.
Greg
• posted
Yeah, I've done a variation on that one already- I put the threading tool in a straight toolholder, pointing right down along the axis of the compound so a line drawn along the tool past its point was at 29.5 degrees relative to the work.
Gregm
• posted
DoN may thread that way, and many guys with large CNC equipment do as well. I do not endorse the method, and indeed discourage it, especially for small machines.
The proper setting of the compound of an engine lathe is critical to outcome, and reasons why are well covered by the links I posted. Plunge cutting of threads leaves the door open for improper lead or pitch and should not be considered as an alternate to proper threading unless one has a rather substantial machine which is capable of resisting the generation of a drunken thread. I have personally witnessed such a thread that was generated on an industrial rated machine, a 15" Cincinnati. If a machine of that mass is capable, I would not recommend plunge threading for any of the home shop type machines under any circumstance unless improper threads would be acceptable. As one of the links testifies, you are almost assured of just such an end result. Learn to thread by proper techniques if you desire high quality work with a minimum risk of generating scrap.
Harold
• posted
Hi Harold (Been a while.)
If I am not mistaken DoN was describing threading with his emco compact 5 CNC lathe ( heavy duty??) and I use it simply as an illustration of just one of the possible ways to skin that particular cat. I think it wise to be aware of the options that exist and not just work by rote. Of course, you have to understand what you are doing when you do whatever it is that you do.
Cheers Bill
• posted
Hi Bill--(Cal?) Yep, it's been a while. Hope you're doing fine.
I agree, it does no harm in knowing various dodges to achieving an end, but in this particular instance I'd be very wary of plunge threading. His machine would be small enough (far from heavy duty) to be easily influenced by various forces that may not be obvious to the casual observer. By not plunge threading, you eliminate the possibility that the cutting pressure can influence the carriage as it's being propelled by the screw.
As you likely know, Bill, I am not CNC literate. I spent my entire machining career on manual machines and have never even turned on a CNC. I have been told by more than one person that angular feeding ( as if by compound) is a feature that one pays for over and above right angle feeds. It is for that reason that many guys plunge cut threads, so the carbide industry has introduced chasers that are much more capable of withstanding the poor cutting conditions of such a cut. It is more a consideration of economy than machining practicality. Considering the size of the majority of the CNC turning centers, and the speed at which they operate, they are far more forgiving of feeding that way. I might have a different attitude in that situation.
I mentioned a personal experience of drunken threads being generated. The machine in question would bump the carriage slightly forward as the hand wheel handle came over the top of dead center, which ruined a large Acme thread intended for the missile industry by making the lead drunken. It was one of those embarrassing moments one "enjoys" on the machine when you are well known for your high quality, yet the simplest of operations turn into a scrap job. It is for that reason that I speak out against plunge cutting. The hazards are real, and learning to use a procedure that has the potential for making scrap is not to be considered as an option. In this case working by rote (without re-inventing the wheel) is a far better choice, especially when you realize that there is no benefit to not doing it right in the first place. There are no real benefits to plunge cutting threads aside from economics of software, but the negatives are numerous.
Harold
• posted
I don't know where you are on the learning curve, but it you want a good reference for these kinds of questions and machining operations on the manual machines, pick up the Mohltrecht "Machine Shop Practice" two volume set. Great illustrations and very clear explanations of all the hows and whys.
MSC and others have those on sale from time to time for \$15-\$20 each. You put a clever guy that has never seen a machine tool in a room with all the machines and those two books and you have a good chance with winding up with a pretty good machinist.
• posted
whatever it
Hi Harold
When you say "dodges" I get the feeling that you are implying slip shod or something lesser than the way you might prescribe. I guess beauty is in the eye of the beholder. In any case I do not know how CNC software handles threading. It could do a straight plunge, or it could mathematically cause the cutter to mimic the action of the compound, with one being no more difficult for the computer to achieve then the other.
I do understand what you are saying and it is good that everyone should understand what is happening. In the same vain I do understand that when you thread the size stock that I do, on a machine as heavy as mine there is no possable chance of producing a drunken thread. If I disengage my half nut anywhere along the thread my carriage stops so fast you'd think it had disk brakes and if I had been foolish enough to leave my tip in the thread being cut, it would either, break, jam the cutter or cut a groove in the work. ( That's a pretty good indicator that the cutter engaged in the thread cannot pull the carriage anywhere.)
With your knowledge, I would bet that you could have a CNC lathe cutting parts in about two days if you had someone to run over the commands and the operation of the particular machine.
Any CNC worth it's salt can apply X and Y moves that are fine enough to mimic the operation of a compound. As you yourself are aware you can mimic a compound set at 29.5 for threading on a manual lathe, by using a compound set at 90 by simply working out how much "in feed" and how much "compound feed" it would take. I believe the ratio to replicate the 30 degree compound would be one forward on the compound to every 1.732 on the infeed. (1 to 1.732) Actually rounding to 1 : 1.75 would produce a slightly steeper angle. A little closer to the magic 29.5
withstanding
I think they do so well because the ball screws are so much more capable of setting and maintaining positional accuracy then the lead screws found in most of the old manuals.
I'll tell you Harold,, my hand wheel handle in not heavy enough to influence the movement of my carriage I was going to say: " you must have a bigger knob then mine!"
Cheers Harold Bill
numerous.
• posted
Crazy as a fart in a whirlwind, aren-cha? Years ago we used a device that went onto the lathe cross slide and cut threada automatically, by plunging straight in. Seemed to work fine,t me.
Lately, I cut threads on my Maxi, using CNC and feeding the cross slide, you guessed it straight in. Works fine for me.
Neither of these machines is heavy dty; the earlier one was a Cinnci with about 12" swing. My Maxi has 10" swing.
Can't imagine why anyone would say 'drunken treads' will result, unless setting cross slide screws up the lead screw pitch ... not likley.
The one thing that does happen is, cutting on both sides of the tool tip makes the cut a bit more apt to have rough finish. But so what? > I have personally witnessed such a thread that was
BFD ... I have personally witnessed hundreds of parts threaded with plunge on cross slide, that were aerospace perfect.
Regards, Hoyt McKagen
Best MC -
Camping/Caving -
List -
Tree huggers: try wiping your buns with a spotted owl
• posted
No one said it doesn't work, what they (that would be ME) said is the variation opens the door to failure. Maybe you don't care about quality. I do.
Maybe when you understand threading the way I do it will make sense. Mean time, your comments have little value, exposing your lack of understanding of the real problems of threading when threads will be inspected by proper means. Whether threads are so inspected or not is no reason to use procedures that have the potential for failure. I do not endorse poor machining practice. I have no concern about practices that you see fit in your shop, assuming you have one.
The "so what" is the sacrifice of tool life, poor chip flow, and the potential for drunken threads, which appears to be a concept beyond your ability to comprehend.
off the last teensy bit with a spring pass cleans that up just fine.
And once established, assuming they have error in pitch due to poor machining practice, they will clean up "just fine" and be wrong. Again, when you have an understanding of that which I have spoken about, you might see it differently. On the other hand, perhaps you just plain don't give a damn. I was not afforded that luxury, I had to satisfy a myriad of inspection procedures and had no alternative but to learn to do it right, or lose my job. I get the distinct impression that you think you know a lot more about machining than your peers that went before you. Your comments prove to me you don't.
I can only guess that if you stand in a garage you also think you're a car? BFD, indeed. I made clear mention of the fact that threading by plunging on CNC machines has the potential to yield different results, often very acceptable. That does not mean that an engine lathe, especially a small one, will achieve like results. You do a disservice to those that are trying to learn to chase threads when you make light of proper procedure. You may bullshit them, but you aren't teaching me anything except that you are not knowledgeable. No more so than when you told me that you can drill a hole 12" deep and stay on location. You might, and you might not. That's the point. You'd do readers a service by telling the potential for failure instead of making it sound like it's a given. It isn't.
I don't take unnecessary chances when I machine. I earned a reputation as a highly skilled tool maker and machinist, a result of learning proper procedures and applying them. Plunge threading opens the door for error that would otherwise not be possible. Maybe some day you'll understand that the way I do. Maybe not. Should I have the opportunity to visit your shop and you're threading that way, I'll keep my mouth shut. I'll expect the same in return should you visit my shop (assuming the day comes when I have it back in operation, anyway. Damned house building project!).
Don't know about you, but I'm finished discussing this issue with you. You'll not hear any more from me on the subject. In the future I'll simply consider the source. Damned trolls.
Harold
• posted
I followed your advice to practice pulling the tool at the right moment to stop the thread- or at least I tried to, and it does make a lot of difference. My stopping "point" is more like a notch, but it decreases pleasantly from the full thread depth up to the OD of the stock. Previously I was just cutting the feed and letting the tool run round the stock before pulling out.
I also sucessfully tried the "dry" cuts for finish which helped, though I couldn't get a really nice polish (I had to burnish a bit on the wire wheel for that). Which is no doubt a consequence of the Home Despot grade HRS and Newbie grade tool edge & cutting angle.
Greg
• posted
Arrogant bastid, aren'tcha? You remind me of a religious fundamentalist, who KNOWS he's right each and every time.
And nothing in theory or example can change your mind. Fact is, sucker, I do understand threads, but certainly not the way you do ... evidently my intuitions and practice go much deeper.
When the thread being cut drives the carriage instead of the other way round, you may have a point. I never saw that happen though and so far you're the only one who says it might. At least one other person here agrees with me. If you do have a problem like that, my suggestion is 1) use a tool with more bottom relief, or 2) find another job.
Ya see, only fools continue to argue against reality. I don't care if you believe me or not, but fact is, I cut plenty of threads by plunging and it always worked out fine. IOW, your contentions aren't supported by any realities in my world. So go find another dead horse to beat.
Pure arrogance. I do understand what you mean. You just aren't giving credit to what I've frequently observed.
My shit always passed too.
In fact it's quite the opposite.
As noted, we also used a Snap-Tap setup that plunged straight in. Worked fine!
It worked on a 12" Cinnci.
I didn't tell you that, but someone online here DID drill 1 mm holes about 300 diameters and managed to make the start from each end meet in the middle. But I suppose you think that's impossible too.
Why don't you start RIGHT NOW?
Regards, Hoyt McKagen
Best MC -
Camping/Caving -
List -
Tree huggers: try wiping your buns with a spotted owl
• posted
>
>
You're very welcome, Greg.
Don't expect too much from mild steel where finish is concerned, particularly hot rolled. If you want real pretty threads, you'll have to use free machining stock, something like 12L14 or 11L17, each of which have lead added to improve machining characteristics. Bad thing is these materials don't lend themselves to being welded, so you have to choose wisely, depending on how you'll use the pieces you make.
There are other materials that thread and machine quite well, too. Stressproof machines very nicely, and you'll find that 303 S or 303 Se stainless is a pure pleasure, threads beautifully, and is nice to machine in general. You'll get on to it with some experience and know what to expect from each one.
One other tip. The side of your threading tool that actually does the cutting is prone to dragging on the thread you're generating because of the helix angle. If you have excessive tearing on one face, a little more relief angle on that side of the tool may be in order. It's very pronounced on coarse threads, hardly noticeable on fine ones. You can usually see signs of dragging on the tool, so look closely at the tool under the cutting edge to see if you see scuff marks.
Mean time, be sure to keep your threading tool very sharp, on center, and lubricate the cut well with proper cutting oil for the material at hand. That's the best you can do.
Harold
• posted
Well ... my CNC machine does not *have* a compound, so there is no real choice. I have no access to the internal algorithms used for the threading, so I don't know whether the lathe actually makes a diagonal move for each successive pass, though given the size of the memory, I suspect that it does not.
However -- note that the major problem which you have mentioned before -- a "drunken thread" -- comes from backlash in the leadscrew and its mounting.
My lathe, and any *real* CNC lathe, should have ballscrews, which are essentially backlash free, and the bearings at the end of the leadscrew should be paired ball or roller bearing assemblies tuned to eliminate end-play. This should eliminate the main contributor to the "drunken thread" phenomenon.
I can't stop the CNC machine in the middle of a cut to examine the chips, to see whether the cut is balanced or mostly from one side.
However -- with my 12x24" Clausing -- a manual machine, I *do* utilize the compound.
Agreed -- for any manual threading. The manual machine -- even if it starts life with little backlash, will almost certainly develop it as it wears.
Enjoy, DoN.
• posted
[ ... ]
It is *far* from heavy duty. It has a total swing of 5", and I can (barely) lift it -- with its electronics, (which add considerably to the weight) -- from the bench by myself. I can't go very far with it -- just enough to swing around and place it on an alternate surface at about the same height. :-)
However -- (as mentioned elsewhere in this thread), it does not *have* a compound -- so the option of feeding at an angle does not exist -- unless it is emulated in the (rather minimal) software. Nor does it have a handwheel, so the weight of the crank handle going over center is a non-problem. What it *does* have is ball screws -- zero-backlash, very low friction, and mounted in a bearing which eliminates thrust backlash in either direction. So the control of position is quite
So -- I am *stuck* (with that lathe) with whatever way the makers designed into it for threading. I use it frequently -- for metric threads, and for threading up to a shoulder, as it does not depend on my reaction times. Though I do thread to near a shoulder, with a run-out groove pre-cut, on the manual lathe. The CNC *does* have a proper backing out of the tool at the end of each pass, so the thread ends with a groove getting shallower until it no longer exists on that machine -- no need for a run-out groove there.
Enjoy, DoN.
• posted
snip--------
Thanks for the description,DoN. That helps confirm my suspicion (I'm not CNC literate, as I've stated) and leaves only the problem of chip loading to be addressed. You can probably tell from the chip generated if the machine cuts both sides equally. I often plunge cut my last few passes to clean up threads, especially in 303 stainless. When you have a sharp tool and lubricate well, the chip comes off looking like a thread, thin 60 degree chip, equally generated from each face of the thread.
One of the problems associated with plunge threading is the tool tip pressure generated by the chips meeting at the center as they come off the machine. Carbide used to fail at the tip almost routinely under that condition, so plunge threading was almost a guaranteed failure. With the advent of superior carbide and higher speed threading due to CNC controls, I get the distinct impression that the operation is now far more successful. Turning at higher speeds, the chip has much better flowing characteristics.
It pays. You can get away using other methods, but occasionally it bites you on the butt. Why take chances, I say!
On the machine I ran that gave me grief, the wear of the machine, which wasn't really excessive, and consistent wiping and oiling, had made the carriage so easy to move that it could be done with a finger tip. Makes for nice handling and good feel, but it also allowed the hand wheel handle to bump the carriage as it came across top dead center due to the slight back lash in the handle assembly. It was not perfectly balanced, obviously. This happened to me at my place of employment, before I started my own shop. I was dumbfounded to find I had made scrap. Funny thing was I was watching the handle jump as it went across center, but couldn't imagine it was bumping the carriage. Talk about young and foolish! I was cutting a coarse Acme thread, fairly large diameter, perhaps only a two pitch. Don't really recall the part, just the failure.
Once you've made the first pass, there's no chance it will ever correct itself under those conditions. That's the chief reason to keep the compound set in the right direction, so the chip load itself pushes against the lead screw. When plunge cutting, the carriage may or may not be loaded, and is subject to the drunken condition.
Thanks again, DoN.
Harold

PolyTech Forum website is not affiliated with any of the manufacturers or service providers discussed here. All logos and trade names are the property of their respective owners.