[JWB_Machining]

Hey,

I'm having a problem that i really need to resolve. I have a 2 foot long 3/4" Diam piece of Steel Stock. I turned down an inch of it to .490" with a .125" Radius. I then used a 1/2" - 20 TPI Die to thread the turned down inch. When i go to screw it in to the fixture it's going into the threads are off center so you can see the bar isn't spinning on it's center axis. I've made three of these so far and all of them are off center. Does anyone have any advice as to how I can make these threads perfect? I would thread mill them but I can't because the bar is so long. thanks for any input.

[Geof]

That is very common using a die because it is tricky getting centralized forces on the handles of the die, especially if the part is held in a lathe and you are leaning over trying to hold it.

If you try the lazy man's trick of resting one arm of the die holder on the saddle and turning the chuck it will almost certainly run off.

The most precise approach is to thread cut them; what type of lathe are you using CNC or manual?

If you cannot thread cut another approach is to turn a pilot on the end of the threaded section down to the ID of the die. This acts as a guide to start the die on center and parallel and you then machine it off after the thread is done.

And practise your technique for balanced rotation of the die.

[JWB_Machining]

I'm using a TL-1, but I posted earlier regarding threading on a lathe. When I only have triangle inserts with a nose radius as fine as 1/64th how many TPI can I get using that because when i hold the insert up to a .5" Diam rod with 20 TPI the insert does not fit in the entire grove of the thread. Could my problem also be that my chuck isn't holding the part true?

You know what I'm saying? If i take the bar stock and chuck it but it's center axis isn't in line with the axis of rotation of my machine then the section I turn down won't be in line with my piece of stock so that could be what's causing the problem, couldn't it?

[Geof]

If your chuck is not holding the part true the turned section will be off center. You can easily check this by turning it, rotating the stock 180 degrees in the chuck and see if it still runs true; it probably will to with a few thou. If it does not make sure the end of the material hidden up the spindle is running true when you grip it; often this part of the bar sags down as you tighten the chuck and can throw things off.

You should really get more inserts. The universal style are good for a range of pitches but it sounds like you have one for a range above 20tpi.

You can also get full profile, or 'topping' inserts which are made for a specific pitch; these make a much nicer thread.

[JWB_Machining]

Ok a Few questions here...

I'm gonna go turn down a piece of stock switch around n see if the part i was previously gripping on runs true. But if it does not, how do I make sure the length hidden up the spindle is running true? it's hidden in my head stock so i can't really measure it or think of a way of correcting any possible sagging due to the bar's weight. And What's the best way to fix my 3 jaw chuck so that when I grip round stock the center of it is in line with the machines axis of rotation?

I do have Diamond and 35 degree inserts n some other types but I have Equilateral Triangle inserts that I assume are what I need for threading because threads are 60 degrees. The nose Radii I have are 1/16 1/32 and 1/64 but I feel they're limited in how many TPI I can get with them and how small of a diameter i can thread. I was looking the other day for more triangle inserts to purchase but nothing struck me as any better for threading. Any chance you can link me to these Topping inserts or any type of insert you think would work for sometihng like 20 TPI because aorund here 1/4 20 and 1/2 20 are pretty common so I'd like to be able to make those on my lathe.

[Geof]

Regarding linking you to topping inserts I could hold the Iscar catalogue up in front of my computer. I guess go to Iscar.com and serch for full profile threading inserts.


To keep your bar running true inside the spindle one method is to machine a piece of aluminum to a good fit inside the spindle and bore a cone shaped hole in the end. Then you push this in from the far end of the spindle up against your bar stock and the cone centers any diameter; an inside out center as it where.

If the chuck is indeed not running true the first step is to take it off and make sure everything is clean before replacing it. Of course if it is a set-tru chuck you just grip a good piece of material in the chuck and true it to that.

If it is not a set-tru but can bolt onto the spindle nose in any of three (or more) positions try each position dy dialing a precise piece of round bar in the chuck; you may find one is better than the others.

Then if it is still out of true either live with it or consider trying to grind the jaws. It is more or less essential to rule out all other reasons for inaccuracy such as dirt, incorrect installation, or mounting position before grinding it true otherwise you will simply embody your own inaccuracy in the chuck.

[JWB_Machining]

I can almost so it through my monitor haha. I'll definitely look into that.

I look at the threads on a comparator and they were obviously being cut deeper on one side then the other towards the bottom so I'm assuming the die is bad. I'm a get a hold of another one and try that.

[JDenyer232]

I can almost so it through my monitor haha. I'll definitely look into that.

I look at the threads on a comparator and they were obviously being cut deeper on one side then the other towards the bottom so I'm assuming the die is bad. I'm a get a hold of another one and try that.

For thread cutting we use on edge threading inserts as they have a very tiny radius, it sounds like you are trying to use a turning insert for threading purposes. I use the on edge system for various threads from 5tpi-56tpi. I use a full profile laydown style insert for common threads like 4-40 or 1/4-20 etc. Full profile inserts as Geof said make very nice threads because they clean up the top of the thread when they make a pass. Go to msc website or equivalent tooling distributor and search for on edge tool holders and insert, also laydown systems are nice when combined with full profile inserts. Hope this helps.

[One of Many]

I can almost so it through my monitor haha. I'll definitely look into that.

I look at the threads on a comparator and they were obviously being cut deeper on one side then the other towards the bottom so I'm assuming the die is bad. I'm a get a hold of another one and try that.

It isn't the die. It's a flaw in the procedure. More along the line of do not use a die to hand cut OD threads you expect concentric.

You should have cut the threads at the same time(as a subsequent step in the same operation) as turning the OD. That would have only taken a tool change and a bit more programming. Yes, I would find the cause of the chuck runout. The fallback is to use soft jaws and bore them on center at the diameter of the stock. The sad news is the eccentric parts you already have turned will need to be indicated in by hit & miss or a set-tru chuck that can be moved to true the part on center.

As a general rule, the root or cutter tip should be pitch/8 so that either internal or external threads cut with the same cutter will mesh without interference. Full form threads are typically pitch/4 on the minor diameter and pitch/8 on the major diameter.

At 20tpi, which is .05 pitch/8=.00625 at the tangent point of the cutter nose radius. With full form cutter, the cutter nose would be .0125 at the tangents. So, you can see where a 60deg turning cutter with a .015 radius will actually be roughly 2x to wide to cut the thread full depth.

DC

[JWB_Machining]

I was talking with this Guy here and he thinks I may have undercut the stock too much. Let's say I cut the stock down to .485" could that possibly be why the Die ran deeper on one side? Makes Sense to me but I'm still learning.

[JWB_Machining]

I was talking with this Guy here and he thinks I may have undercut the stock too much. Let's say I cut the stock down to .485" could that possibly be why the Die ran deeper on one side? Makes Sense to me but I'm still learning.

[Delw]

heres an easy way. if you have to use a die.
get a 5c collet holder for your mill, block it up so you have have clearance.
get a collet that holds the die lock the die in
get a 3/4 r8 collet chuck it in the hand mill. shove your part in the collet.
(make sure everything is indicated to center)
turn you mill on
feed the part into the die and use lots of OIL.
gives you a perfect thread every time. I have done 3b class threads down to 4-40 with adjustable dies.
I ony do it that way if the thread is to long to single point.


Delw