Using V-point Threading Inserts on CNC Turning Center

[WakelessFoil]

We have succeeded at using G76 on our turning center to complete a single point threading cycle. The only issue is that we have been using V-point threading inserts, and we have to increase the cut depth in order to get a fitting thread profile. I believe that when we do this, it creates a poor tolerance thread fit.
Assume that we do not have access to full profile inserts, how might we accomplish getting a working and tight fitting thread? How do all the CNC guys cut external threads? Do they all just use full profile? Most of what I see online are V-point... Why?

Thanks,
Justin

 

[Philabuster]

We have succeeded at using G76 on our turning center to complete a single point threading cycle. The only issue is that we have been using V-point threading inserts, and we have to increase the cut depth in order to get a fitting thread profile. I believe that when we do this, it creates a poor tolerance thread fit.
Assume that we do not have access to full profile inserts, how might we accomplish getting a working and tight fitting thread? How do all the CNC guys cut external threads? Do they all just use full profile? Most of what I see online are V-point... Why?

Thanks,
Justin

How are you gaging the thread?

 

[Ox]

Like Phil, I don't follow the problem here?


--------------

Think Snow Eh!
Ox

 

[dave morgan]

When using a non-full profile insert I turn to the Major Diameter then run the thread tool with the wear or geometry set to cut big, measure with three wires and then adjust to arrive at the correct P.D.


Dave

 

[Cannonmn]

When using a non-full profile insert I turn to the Major Diameter then run the thread tool with the wear or geometry set to cut big, measure with three wires and then adjust to arrive at the correct P.D.


Dave

Are you doing that with CNC, and if so, is it easy to get your 2nd cut started in the right place? I’m guessing you have to remove work from lathe to do 3-wire measurement.

 

[Ox]

You never pull work to measure.
You may need to find a new way to measure, but you doo NOT pull work out!


------------------

Think Snow Eh!
Ox

 

[magno_grail]

"we have to increase the cut depth in order to get a fitting thread profile" - What do you mean by "fitting"? Are you checking with a nut or female thread of some kind? Your major diameter might be off.
Also are you talking UN thread? Cutting a flat top male for a Whitworth round valley female will cause interference in the valley unless you decrease your major diameter..

 

[dave morgan]

Cannonmn,

Yes CNC turning center and as Ox stated don't remove your piece, measure in place.





Dave

 

[Ox]

Maybe this should be in the "trick" thread (pun not intended, but ...)

If you have a bolt, stud or otherwise to compare to, you can hit your part a bit O/S, and then use any pr of calipers, stuff the tips down in the bottom of the valley's (valley's only!) of each to compare.

This not a real "measurement" but rather you are just comparing.


-----------------

Think Snow Eh!
Ox

 

[sinha]

You never pull work to measure.
You may need to find a new way to measure, but you doo NOT pull work out!


------------------

Think Snow Eh!
Ox

This is because it is not easy to re-clamp the workpiece in the exactly same axial/angular position. This will shift the thread helix.

 

[Clive603]

Time to hit the textbooks and CAD program to work out exactly how much extra in-feed you need relative to a full profile insert to accommodate the sharp point of the Vee.

Decent one page reference for the UN version of the American thread form here : - https://www.gaugestools.com/unified-screw-threads/

Basically if the thread depth (in-feed) for an infinitely sharp V pointed thread is H the depth of a full profile one is 5/8 H. The full thread is offset relative to the V point (theoretical) thread by 1/8 H so it goes 1/4 H deeper but starts at 1/8 H smaller OD.

The actuality is more complicated because your V tool isn't infinitely sharp!

I'm a manual guy and use the "zero-2-zero" threading method which effectively uses the lathe itself to caluclate the in-feed on and angled top slide. A side benefit is that it's an absolute doddle to add extra in-feed to correct for an imperfect tip shape on a hand ground tool using the first off as a test piece then adjusting the base setting to cope so all the customer parts come off dead to size.

Clive

 

[WakelessFoil]

How are you gaging the thread?

We have thread wires and a thread mic to measure pitch diameter. We also have been using a normal mic to read the major diameter. Every machinist I have talked to has defaulted to suspecting the major diameter is too large, despite several (accurate) tests suggesting otherwise.

Like Phil, I don't follow the problem here?


--------------

Think Snow Eh!
Ox

The minor diameter is too large, this offsets the pitch diameter and prevents the thread from threading in properly. The crests on the female side are trying to fit in a valley that is too shallow, causing things to get bunged up.

"we have to increase the cut depth in order to get a fitting thread profile" - What do you mean by "fitting"? Are you checking with a nut or female thread of some kind? Your major diameter might be off.
Also are you talking UN thread? Cutting a flat top male for a Whitworth round valley female will cause interference in the valley unless you decrease your major diameter..

It was not threading in and our pitch diameter was off. Like I said before the major diameter was not too large, in fact it was cut down to the minimum allowable diameter per the charts. Yes these are both UNC threads, both male and female have noticeably flat crests.

 

[awander]

We have thread wires and a thread mic to measure pitch diameter. We also have been using a normal mic to read the major diameter. Every machinist I have talked to has defaulted to suspecting the major diameter is too large, despite several (accurate) tests suggesting otherwise.

The minor diameter is too large, this offsets the pitch diameter and prevents the thread from threading in properly. The crests on the female side are trying to fit in a valley that is too shallow, causing things to get bunged up.

It was not threading in and our pitch diameter was off. Like I said before the major diameter was not too large, in fact it was cut down to the minimum allowable diameter per the charts. Yes these are both UNC threads, both male and female have noticeably flat crests.

I think you mean to say, "the minor diameter comes to a sharp point because we are using V inserts, and this means that the pitch diameter is not correct."

As stated above, you do need to cut deeper, by a factor of 1.4. In other words, if the formulas tell you to cut 1mm deep with a correctly-flatted tool, you would need to cut 1.4mm deep with the sharp tool.

 

[michiganbuck]

I'm, not the CNC guy but if you want to go the root diameter from the height of the insert/bit the nose flat or radius changes everything. If the insert is from the same box/same run number then likely to repeat..but first try the infeed has to be gauged/measured

 

[Ox]

I've threaded a part'r two in my day, and I'm not quite sure exactly what it is that your issue is, but suffice to say that I always end up "deeper" than the book says to git it to fit.


--------------------

Think Snow Eh!
Ox

 

[gcodeguy]

I've threaded a part'r two in my day, and I'm not quite sure exactly what it is that your issue is, but suffice to say that I always end up "deeper" than the book says to git it to fit.


--------------------

Think Snow Eh!
Ox

Yeah. Pretty sure the Machinery's Handbook gives the MAX diameter for the root of an O.D. thread.

OP, I'm another that doesn't understand your problem. The pitch diameter determines fit. You have a pitch mic. The only time the insert radius has an affect on fit is when it gets too large. The no-go gauge will go while the go-gauge won't when that happens. You don't even have to look at the insert to know it is time for a new corner. If you only have a pitch mic and wires, then I can see you getting into trouble at some point.

Once I get the thread where I want it, I use an optical comparator to measure root diameter, and change my X-value to that and the P-thread height in the program to reflect the actual thread height. (I'm using canned threading cycles. Mostly G76 cuz we mostly have Fanuc controls.) Sometimes you have to lie, but that is for another post.

 

[Cole2534]

I've threaded a part'r two in my day, and I'm not quite sure exactly what it is that your issue is, but suffice to say that I always end up "deeper" than the book says to git it to fit.


--------------------

Think Snow Eh!
Ox

Me too. On a manual or a CNC.

Cheap trick- 2 wire measurement. Put 2 wires at 12 o clock and measure to the thread crest with a depth mic. It >should< get you to the correct PD after a little math and is much easier to execute in the machine.

 

[706jim]

I've mentioned this before, but when using three wires the "M" value gives you the maximum pitch diameter for a class three thread. Drew it out on the computer to check. So if you are trying for any reasonable class two fit, "M" has to be reduced accordingly.

 

[michiganbuck]

If you have a threading single-point insert that can turn various threads perhaps from 9 to 36 threads per inch then the nose flat/radius must fit the smallest thread, about .003 for the 36 thread. So to get a wire size that same insert will go deeper to turn a 9 (TPI) thread whose root flat may be about .014

I guess the .oo3 nose insert likely will need to go about .0095 deeper to make the 9-thread wire size.

With this nose flat/radius variance (of the insert), the infeed from major diameter to root diameter will not be the thread-chart or calculated amount to make the V correct to the target wire size unless you calculate the infeed using the actual nose flat/radius of the insert ..

 

[Ox]

I have to overfeed even with cresters.


----------------------

Think Snow Eh!
Ox