Lathe: parting with ID threads.

[rfrink]

This is a new part for me. 1-1/4" OD with 1/2-20 ID threads. I'm running from bar feed in CNC turning center.

Photo is before and after chamfering in drill press.

When I cut the part off with a parting tool, it gets tossed around inside the machine because it is literally still "hanging on by a thread". Ideally, I would love this to fall gently into the parts catcher.

Secondary operation is to chamfer the ID in a drill press.

There's got to be a better solution.....a small groove tool to cut an ID groove at the parting spot? Groove before tapping?

Thoughts?

Thanks!!!

 

[ChipSplitter]

This: MINC

Just kiss the inside to about X .510 before tapping.

Otherwise you'll probably leave a burr on the thread.

 

[upm2019]

You should add a recess toll to your program using a ID grovver just program your chamfer what ever is called out The trick is to stop at the end of the part too far either way and you'll get a ring . if you do it right you'll have almost no burr and parts shold fall into parts catcher.

 

[mountie]

Single point the ID thread. Use the threading tool to cut a relief inside the bore. That'll also eliminate the deburr drill press operation.

 

[rfrink]

good info! Thank you all!!

I've got a couple tools ordered. Solid carbide grooving tools to play with.

Would you do the chamfering and grooving work before or after you tap the threads? The tool path will be the same and I can easily cut and paste it either in front of the tap, or after the tap.

My first try will be after tapping....just because.....

 

[ChipSplitter]

As a rule-of-thumb, I always chamfer/groove before threading, whether it's tapping, single-point in the lathe, or threadmilling on a mill.

If you thread beforehand, the chamfer tool has a tendency to push a burr down into the thread. BTDT. Another advantage.........there's no chance of leaving tiny chips stuck in the thread.

Your major chamfer diameter should be just bigger than the major thread diameter for internal threads (and vice versa for external).

 

[litlerob1]

Or, just use a plain Grooving Tool from the ID. Even if it's only partially through. Then come in with your pat-off Tool. Eliminate the "hanging thread".

R

 

[temporary_123]

hy rfrink, i use a custom code that removes the thread helix that is located in the cut-off zone

movement is shown in attached image, and it is done using offset 1 of a threading insert

if possible, i also use offset 2 in order to cut the front chamfer ( eliminates one turret index / may save one turret post )

it is parameterized, and works like a charm, especially for big threads, without damaging the insert; may handle a doc equal to the 1st or 2nd pass of an infeed pattern ( thus much greater then the threading finish doc ); uses mapped feeds and multiple clearances, in order to shorten the cycle time

it can be used before tapping

if used after single point threading, then is required to repeat the threading ( spring pass ), so to remove some potential internal burrs

segment [ 14 , 23 ] may be programed as long as you wish, while the minimal value should be >= length variation, thus, if, for example, length varies between 50 and 50.5, then that segment should be 0.7 ... also is important to have the segment positioned near the far end, and this can be achieved by measuring the cutting tool and the threading insert at the same time, and syncronize their Z corections through code

to shorten the setup time, is required to know the insert dimensions ( radius, offset, height )

i developed it for mass production; without it, is not possible for a go-gauge to go all the way through, thus it helps to avoid those parts that have a bad thread near the end; normally, such parts are discovered after a 2nd chamfering operation / kindly

 

[Hardplates]

I run a part almost weekly that is similar as far as parting and threads. I've always gone in and cut a small thread relief with the threading bar before cutting the threads. Literally only takes a few seconds

 

[dodgin]

hy rfrink, i use a custom code that removes the thread helix that is located in the cut-off zone

movement is shown in attached image, and it is done using offset 1 of a threading insert

if possible, i also use offset 2 in order to cut the front chamfer ( eliminates one turret index / may save one turret post )

it is parameterized, and works like a charm, especially for big threads, without damaging the insert; may handle a doc equal to the 1st or 2nd pass of an infeed pattern ( thus much greater then the threading finish doc ); uses mapped feeds and multiple clearances, in order to shorten the cycle time

it can be used before tapping

if used after single point threading, then is required to repeat the threading ( spring pass ), so to remove some potential internal burrs

segment [ 14 , 23 ] may be programed as long as you wish, while the minimal value should be >= length variation, thus, if, for example, length varies between 50 and 50.5, then that segment should be 0.7 ... also is important to have the segment positioned near the far end, and this can be achieved by measuring the cutting tool and the threading insert at the same time, and syncronize their Z corections through code

to shorten the setup time, is required to know the insert dimensions ( radius, offset, height )

i developed it for mass production; without it, is not possible for a go-gauge to go all the way through, thus it helps to avoid those parts that have a bad thread near the end; normally, such parts are discovered after a 2nd chamfering operation / kindly

What the fuck.

 

[ChipSplitter]

What the fuck.

It's toxic feline, previously known as deadlykitten.



He can't get rid of those telltale words......

Here's the record of his demise: Rook question about setting a radius tool in a lathe

 

[OCTANE WORKHOLD]

View attachment 295939

This is a new part for me. 1-1/4" OD with 1/2-20 ID threads. I'm running from bar feed in CNC turning center.

Photo is before and after chamfering in drill press.

When I cut the part off with a parting tool, it gets tossed around inside the machine because it is literally still "hanging on by a thread". Ideally, I would love this to fall gently into the parts catcher.

Secondary operation is to chamfer the ID in a drill press.

There's got to be a better solution.....a small groove tool to cut an ID groove at the parting spot? Groove before tapping?

Thoughts?

Thanks!!!

Agree with everyone else about creating a small groove/chamfer on the ID.
Using a parting tool with one higher leading edge like this one helps too. The higher leading edge allows the part to stay attached as long as possible.
QD-RG-0300-0501-CO 1125

 

[dodgin]

It's toxic feline, previously known as deadlykitten.



He can't get rid of those telltale words......

Here's the record of his demise: Rook question about setting a radius tool in a lathe

I know who it is I just can't believe it's still going on.

 

[TeachMePlease]

What the fuck.

I snorted water out of my nose.

 

[ChipSplitter]

I know who it is I just can't believe it's still going on.

hy, dodgin

He's been banned several times under different names. kindly!

And he always keeps coming back for more. kindly!

Always spews the same BS, too. kindly!

kindly!
kindly!
kindly!
kindly!

The lights are flashing in my head.......

 

[Ox]

I would highly recommend a threading tool over a grooving tool any day on this!


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

Think Snow Eh!
Ox

 

[Delw]

I would highly recommend a threading tool over a grooving tool any day on this!


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

Think Snow Eh!
Ox

Ox. can I ask why? you and I and a few others been doing this a long time and I like to get other views from experience people.
Ive done it 3 ways threading tool, groove tool and a profile tool like this
Standard Profile Tools - Series 56

The profile tool I prefer as i put a 45º angle on the back side plus I use to it finish bore and debur after 1st thread set, gives a nice finish on the chamber due to having and small rad.
on brass and plastic I see no real difference but on other materials using a thread tool kinda wears the front end and tip out pretty quick depending on material.
grove tool I used to use alot but got tired of breaking them when I least expect it too generally on smaller parts then wiping out your borer and threading tool. chips packing up on a groove tool and doesnt help either. in the big machine with bores over 2" and up to 10" I use the toplocks alot, but the material is harder and you have lots of room for chip clearance.

The profile tools work well for me over the last 8-10 years on small parts(under 3/4) that Ive completely switched.

my typical program is citizen and Miyano same for the 10" chuck machine except I usually face the back side off, the 45 is there if I have the room before I hit the jaws.
c drill(if needed)
drill
chamfer/ bore/ relieve
thread
chamfer/ bore and relieve just finish pass for a clean thread
thread 2 pass's to break off burr

on most parts after cut-off the only thing I do is hit it with 320 grit sandpaper and the parts are perfect(both sides), thread gages are perfect as well as the 45 relief on both sides. not to mention its hard to tell what side was the cut off side.

 

[yardbird]

Ox. can I ask why? you and I and a few others been doing this a long time and I like to get other views from experience people.

I can't answer for him but I'll wager "its already in there" is somewhere in his reply. I use the thread bar too. I thread, chamfer the back end, the debur with another thread pass or two. I try to position the center of the thread tool even with the back cutoff face.

Before I started looking for a different way of doing this I was doing it on a smaller Cincinnati Avenger. Parting off down into 1 1/2-6 that last little bit of thread, you know the one that causes all the trouble. Part started whipping around with the rotation of the chuck and got wedged in between the hard jaw and the OD tool block on the turret. Crushed the part and stopped the chuck dead. The part smashed and absorbed most the energy so the machine made out ok. Luckily

Brent

 

[yardbird]

It's toxic feline, previously known as deadlykitten.



He can't get rid of those telltale words......

Here's the record of his demise: Rook question about setting a radius tool in a lathe

Sometimes I get the impression you've been here a lot longer than 2019. You new in 2019 or you old and reup as new in 2019

Brent

 

[ChipSplitter]

Sometimes I get the impression you've been here a lot longer than 2019. You new in 2019 or you old and reup as new in 2019

Brent

I'm new in 2019. I promise......

I had been lurking for awhile before I joined and I read the archives a lot.

So I know most of those old guys' personalities......boris, Solar, pi, adama, Mark McGrath, RJ Newbould, John Welden, smallshop, HuF...D...., and a bunch of others.