# Thread Problems Part Failure



## Latheman (Oct 5, 2015)

By part failure when closing in on final cuts, I wind up bending the part. I use a 60 deg on compound a fish tale gauge to square up. But when I get close to final few thousandths I bend the part. I center the tool on my tail stock center and I just can't seem to figure why I am bending the part. I am trying to thread 1/4-20 on 1018 crs and have just enough stick out of the chuck to get the job done. But the tool just bends the part when .005-.008 away from final depth. I would love to hear what you guys think. Please ask any question that could help me solve the problem. Also tried on a 7/16-16 and same problem.


----------



## British Steel (Oct 5, 2015)

Hi, are you taking full-width cuts with the cross slide, or advancing at 29-1/2 degrees with the topslide? a straight-in cut puts much more force into the cut as it's closing on final diameter as the full width of the thread is being cut, plus there's much less space for the swarf to curl and get out of the thread over the top of the cutting tool. If you're cutting straight in, try setting the topslide to 29-1'2 degrees (assuming a 60 degree thread) so that it only cuts on the advancing edge - this also helps keep a consistent threading feed, as the unidirectional force between work and tool keeps the leadscrew and nut engaged.

If you're unsure of the angle, for a right-hand thread cutting towards the headstock turn the topslide ANTIclockwise through almost 30 degrees, so that increasing depth of cut pushes the leading edge of the tool into the work, the trailing edge just shaves and cleans up the other flank of the thread.


----------



## higgite (Oct 5, 2015)

Besides British Steel’s questions, I will also ask what depth of cut are you taking on the pass that bends the work piece?  What is the initial diameter of the work piece before you make the first threading pass? What thread depth are you cutting to? Does your compound or cross slide scale (whichever you are using) show the actual depth of cut or does it show the reduction in diameter of the work piece?

Tom


----------



## Bill C. (Oct 5, 2015)

On small threads I prefer to use a die. Any thread over a 1/2" dia I would try to cut a thread.  Unless you have a small lathe a die is easier.


----------



## Bill Gruby (Oct 5, 2015)

Exactly how much is just enough to do the job? What is the tool position along the thread when the bend happens?

 "Billy G"


----------



## Paul in OKC (Oct 5, 2015)

That's pretty small for single pointing. Good advice above. Definitely need the compound on the angle to lesson the tool pressure. RPM plays a part as well. Slow speed will grab.


----------



## Latheman (Oct 5, 2015)

I am threading in back gears. So slow rpm

Sent from my SM-G360P using Tapatalk


----------



## Latheman (Oct 5, 2015)

British, i feed with top slide. At 29 1/2. I am feeding at a rate of .005 a cut.

Sent from my SM-G360P using Tapatalk


----------



## Latheman (Oct 5, 2015)

Tool position: about half an inch from the farthest point away from the chuck.  

Sent from my SM-G360P using Tapatalk


----------



## Latheman (Oct 5, 2015)

.2484 was that last 1/4  20 attempt

Sent from my SM-G360P using Tapatalk


----------



## jocat54 (Oct 5, 2015)

When I first learned to thread that would happen to me all the time.
Use the tailstock and a live center to support the end and hopefully all your troubles will go away---mine did. Plus you can move further away from the chuck.
I very seldom cut any threads that I don't support with the tailstock no matter what the size of the shaft is.


----------



## derf (Oct 5, 2015)

It sounds like your tool is above center.


----------



## eeler1 (Oct 5, 2015)

Could use a die for at least that last .005".  Or like said earlier, thats a small thread, just use a die for the whole thread.


----------



## Chipper5783 (Oct 6, 2015)

I'll watch this thread with interest.  I have to do almost the same job - a little stub of a 1/4" NC thread.  I've done a fair bit of single point threading, and never really had much difficulty (except one job when I had to come right upto a shoulder and no end of thread groove allowed, so it needed to be ramped out - popped the end off the tool a couple times).  Certainly the comments above are all good (especially the 29 degree).  As Jocut shared, can you leave a pin out the end of the thread (just smaller than the minor diameter of the thread), support the outer end, then cut the pin off?  Even just a bit of support will make a big difference.  Also, what cutting fluid are you using?  All fluids are not created equal (and everyone probably has their favourite).

As you get closer to being completed, repeat each pass at the same depth of cut (maybe even 3 times), until you get no more cutting at that depth (addresses spring in the set up).


----------



## T Bredehoft (Oct 6, 2015)

I hesitate to use more than .001 or .002 on the final two or three threads.   Yes, a live center will help, but .005 is a heavy cut on 1/4 20 threads.


----------



## Bill C. (Oct 6, 2015)

Check your tool bit by using a black marker or layout dye and paint the cutting edges to see if the bit may be rubbing just enough to push the part instead of cutting.  I know it is frustrating.


----------



## Latheman (Oct 6, 2015)

Oatey-16-oz-Thread-Cutting-Oil


----------



## Latheman (Oct 6, 2015)

1. Top slide set to 29 1/2 degrees feeding with topslide (Not the issue)
2. I know I'm on center (Not the issue)
3. Used fishtale gauge to set up tool (Not the issue)
4. RPM is about 180 (Might be a problem)
5. Taking .005 cuts all the way through (Might be closer to the problem)
6. Cutting oil (Probably not the issue)
7. Supporting with tailstock (Have not done, but might help)

In short it might be the two issues of taking too heavy a cut at the end and slow rpms. I will try to do everything the same and change those two things and will report back!


----------



## Bill Gruby (Oct 6, 2015)

Make your cuts no more than .003 and slow the speed to about 100 RPM. If necessary use a live center. Should solve the problem.

 "Billy G"


----------



## Latheman (Oct 6, 2015)

Jocat54 do you center drill first or just ram the center into the part?

Sent from my SM-G360P using Tapatalk


----------



## Tony Wells (Oct 6, 2015)

Is there a thread relief groove? What diameter and width?


----------



## Bill Gruby (Oct 6, 2015)

Center Drill for the Live Center. NEVER just ram the center into the stock.

"Billy G"


----------



## Latheman (Oct 6, 2015)

Just making sure. I love my live center. I won't hurt it.

Sent from my SM-G360P using Tapatalk


----------



## chips&more (Oct 6, 2015)

Single point threading ¼” crs can be too much “tool pressure” for the billet material when length from the chuck becomes 3 X diameter. The material will flex and then push away from the tool, roll on top of the threading tool and then bend. Solution: use a die, geometric die head, use a center when threading it, use a follower rest, roll the threads, or? Can you use all thread and Loctite the threaded rod into the project?...Good Luck, Dave.


----------



## British Steel (Oct 6, 2015)

Centre drill first - but before that, face the end square to get a nice central centre in it! It's a good idea (if you can) to have just a nubbin sticking out of the chuck jaws in the interests of rigidity too.


----------



## Latheman (Oct 6, 2015)

Tony Wells said:


> Is there a thread relief groove? What diameter and width?


 No I did not make a relief groove.


----------



## jocat54 (Oct 6, 2015)

I always center drill first.
It can be a pain on small diameter sometimes but worth the time to do it.
It seems I learn the hard way most of the time trying to shortcut things


----------



## Paul in OKC (Oct 7, 2015)

I wouldn't slow the rpm any myself. As for the center, yes, use it. What I do on small diameter parts is not ram it, but lock the tail stock and 'bump' the tip into the end of the part a few time to make a dimple, then put a bit of pressure on it and go. Works great.


----------



## Chipper5783 (Oct 7, 2015)

Hi Latheman,
Tonight I completed a thread similar to the one you were working on, and can share pictures (see my earlier post in this thread).  The component is ashifter pin for the table feed gear box on my mill (have to make 2).  The pins have a small knob threaded on, and previous owner snapped a couple of them off (wish he had not tossed the black plastic knobs - that is a seperate project).  The knobs thread on 1/4-20.

For this component, I had to thread up to a shoulder.  I used a groove, but I only had about 0.015" of run out (before I'd hit the shoulder - which would make a bad noise).  I threaded in the lowest gear (30 rpm) - it was actually quite easy to keep the overshoot to less than 0.003".  Once I was well into the thread (say the last 6 passes) - I'd take 0.001" DOC, followed by 0.000" check it for fit, then do another 0.001", followed by 0.000".  The cutting was quite uneventful, good surface finish, good fit.  Now to cut the support extension off and complete the rest of the pin.


----------



## Latheman (Oct 7, 2015)

Chipper! You are a great help. I appreciate all of you trying to help me. This forum has wonderful active members.


----------



## epanzella (Oct 9, 2015)

As others have said, using a live center makes a delicate job into an easy one. Even 1/4-20 threads in brass are a piece of cake with a center.


----------



## Latheman (Oct 9, 2015)

Nice pic : )


----------



## flutedchamber (Oct 12, 2015)

1.  Have a sharp tool with proper relief (both side and under the cutting edge) set at the correct height and angle (use fishtail)
2.  Support the free end of your work with a center in a proper hole.
3.  Compound, in this case set at 29.5 degrees.
4.  Small cuts, .003-.005
5.  At least on every other cut, take a pass without advancing the compound on small threads, light lathes and/or gummy material (brass/bronze)
6.  Make your last few passes at .001

This SHOULD make your problem go away.  You don't need a small lathe to cut small threads.  I cut 6-40 threads on my 17 inch swing Nardini with no trouble.

Watch size threads...yes.  THEN you would reap the benefits of a small lathe.


----------



## epanzella (Oct 12, 2015)

_"CENTERDRILL FOR THE LIVE CENTER. NEVER JUST RAM THE CENTER INTO THE STOCK"_
Billy G


----------



## Paul in OKC (Oct 12, 2015)

I will only say that I have been a machinist for almost 40 years. It is how I make my living. Worked around some guys that are damn smarter than most of us. Once again there are those who think they are the gift to this trade. Most of them are hobby trained. Have had a few of them come into the shop, and usually quit, or get fired because they can't handle the real world of machine shop work. I run the shop I am at now and didn't get here by being a hack. 
   Once again, I did not say jam the center into the end of the part, but to bump it a few times. It WILL leave enough dimple to hold a short part. If you are machining out away from the chuck, I would not even suggest this. Close to the chuck, it works like a charm.
I have not been a member of this group very long, but as a whole there is generally good info here for the novice, and a pointer or two even for us experienced guys.  Generally the ones who think others ways are a hack usually just know enough to be dangerous.


----------



## HMF (Oct 12, 2015)

You all are welcome to disagree with regard to the right way to do something. However the disagreement may not be insulting to anyone. Remember, we can disagree without being disagreeable on this forum. Thank you


----------



## 12bolts (Oct 12, 2015)

You should be reducing your depth of cut as you progress in with the compound. The deeper the tool is in to the work then more of the tool flank is applying pressure to the work as it is cutting over a larger area.
Also, as you near the max thread depth it can be beneficial to take a zero cut with the compound, but advance in a thou with the cross slide and take a finishing cut on both flanks of the tool to clean up the thread and provide a little thread clearance.

Cheers Phil


----------



## Latheman (Oct 15, 2015)

Hey Paul. I was the one that used the word ram. But gently bumping makes perfect sense to me. I will try your method for it with save me a step of center drilling. Now I will ask you though, do you recommend on smaller dia. parts or even with larger dia. parts? Also, do you use a spring center or just a live center? Your experience is valuable to me and appreciated. But I do also know there is always more than one way to skin a cat.


----------



## Paul in OKC (Oct 15, 2015)

First off I will apologize for my rant above. Was one of those rare days I got surrounded from all sides  (thank goodness, very rare). I love to teach people this trade, thought it is not for everyone. My hope is to throw out some ideas of what works for me. It's up to you to take it or leave it, agree or disagree, and go on. Mine to do the same with yours as well.  So............
Larger parts will generally always get a center drill. Depending on how far out of the chuck they extend determines a lot. Set up rigidity, etc., etc.,...
 One reason for 'bumping' just the center in on small diameter parts is at times it will keep the center just far enough out for clearance for the tool. I use a regular live center. Again, this method I use is for short, small diameter parts that just need a bit of support, usually not more than an inch or so out of the chuck. Any more than that you need the full support of the center drilled hole. HTH.


----------



## radial1951 (Oct 15, 2015)

Paul in OKC said:


> First off I will apologize for my rant above. Was one of those rare days I got surrounded from all sides  (thank goodness, very rare). I love to teach people this trade, thought it is not for everyone. My hope is to throw out some ideas of what works for me. It's up to you to take it or leave it, agree or disagree, and go on. Mine to do the same with yours as well.  So............
> Larger parts will generally always get a center drill. Depending on how far out of the chuck they extend determines a lot. Set up rigidity, etc., etc.,...
> One reason for 'bumping' just the center in on small diameter parts is at times it will keep the center just far enough out for clearance for the tool. I use a regular live center. Again, this method I use is for short, small diameter parts that just need a bit of support, usually not more than an inch or so out of the chuck. Any more than that you need the full support of the center drilled hole. HTH.


*
Paul, same here, apologies for my comment which didn't help. A little background: I also have many decades (5) in this trade and also enjoy passing along whatever knowledge I have. In fact I was a Trade Teacher for 9 of those years.
I firmly believe the best thing to teach a novice is the proven, time-honoured, "correct" way to do something. If he decides to do it some other way, then that's his choice. And yes, we all develop our own way of achieving the end result, and others can try it or not, it's up to them. 

There is no shortcut to proficient Turning (definitely NOT Lathing...see another thread), especially screw cutting. For a novice, the best place to start is to get a book and read it. I still refer to the South Bend book "How To Run A Lathe". It is THE classic amateur's lathe handbook, but there are others also. The section on threading is excellent, and tells you how it _should_ be done. Then it needs practice and the more the better. And by all means, experiment and learn...

I assume Latheman has solved his problem by now!


----------



## Paul in OKC (Oct 15, 2015)

Agreed, radial. I have taught at a vo-tech for  short time, and the first thing was to teach them the correct way to do a job safely. Some were more proficient than others, and once they grasped things some could handle other ways to go about a project. Others, well, lathing was the term some never lost .


----------



## Wreck™Wreck (Oct 16, 2015)

Think that you have problems (-:
I finished turning all of the OD and ID diameters of 64 parts today. Monday I will begin the internal threading, 24 parts 2"-4 TPI Acme, 12 are RH and 12 LH, followed by 40 parts 1 1/2"-4 TPI Acme 20 RH and 20 LH all in 1018 steel.

Before leaving at 3:00 today I turned a 2-4 TPI LH Acme male gauge plug in aluminum to get a handle on the thread depth required for these Vardex inserts, measured it over wires, (had to tweak it 3 times) then made a test nut in aluminum using the same thread depth and it screwed onto the GP Acme threaded rods by hand, a bit tight as I was right at the pitch diameter listed in the tables, adding .002 to .005 to the depth will make it just right.

This is the plug, Monday should prove to be a rather trying day, I have roughly 21 hours to finish all of the parts, wish me luck.


----------



## Paul in OKC (Oct 16, 2015)

Fun stuff! Had to do a 1 3/4-5 TPI full acme rod about 18" long a couple of times. Building a 'C' vise for pipe. Then had to do about a 5" long nut for it! The nut was welded to the frame afterwards. That stuff is fun to me!


----------



## 4GSR (Oct 18, 2015)

Paul in OKC said:


> Fun stuff! Had to do a 1 3/4-5 TPI full acme rod about 18" long a couple of times. Building a 'C' vise for pipe. Then had to do about a 5" long nut for it! The nut was welded to the frame afterwards. That stuff is fun to me!



Very familiar with C-style pipe vises.  One's I've dealt with over the years has a 2"-4 Acme thread on them.  The latest one's I've had to deal with have a M55x4 Trapezoid thread!  Glad I didn't have to cut them.  Just had to disposition them as good or scrap.


----------



## Wreck™Wreck (Oct 20, 2015)

Paul in OKC said:


> Fun stuff! Had to do a 1 3/4-5 TPI full acme rod about 18" long a couple of times. Building a 'C' vise for pipe. Then had to do about a 5" long nut for it! The nut was welded to the frame afterwards. That stuff is fun to me!


The LH threading did not work at all, these tools have the helix angle built into them, which is diameter specific as well, the LH tool should arrive tomorrow. using a RH tool to make a LH thread had the helix angle 180° apart, this cannot possibly work, well..
Also, each part took 125 threading passes or 4000 passes for 32 parts, good thing that I used a CNC lathe or I would be typing this from prison right about now.


----------



## Paul in OKC (Oct 21, 2015)

Never had trouble using RH inserts for LH threads, but always been a 'V' thread, or stub acme. Not had to do a full acme LH, could see where that depth might give ya fits!


----------



## Wreck™Wreck (Oct 21, 2015)

The inserts are laydown triangle and are symmetrical, the holder has 3+° of angle, when ran left handed that's 3° in the wrong direction, an insert with enough relief on both sides in a holder with zero angle would work both ways. 
The helix angle for a 1 1/2-4 thread is 3.06°


----------



## Latheman (Nov 8, 2015)

Made headway. 

Sent from my N9518 using Tapatalk


----------



## Latheman (Nov 11, 2015)

Ok so what worked for me? 
1. I used a live center. Made all the difference. 
2. I tried both approaches live center and bumping (Not ramming lol) I will say both worked flawlessly without any issues. So I would say gimme six of one and half a dozen of the other. On bigger threads 1/2 up I will center drill more than likely, but as Paul said just bumping my center into the part to make a dimple and lock it down, worked just as good as center drilling.
3. Lighten up. What I mean is at the point I was within .015 I started with .003 cut. Then within .006 I just would take .002 to depth. Each pass followed with a spring pass. Worked great there. 
4.  Patience. I know I want to send the tool in .060 and the part winds up threaded in the first pass, but it just won't work. : ) 

Thanks to all who helped. I shall continue on my learning way.


----------

