Question about carbide cutters

H

Henry V

Guest
I have been using full profile carbide threading cutters to cut barrel threads. The last two barrels I cut were too tight to screw on the action. It seems that the minor thread diameter was too large. To me this indicates that the insert was worn and did not cut deep enough. However, inspection of the cutting point shows no visible wear. The gold coating on the tip of the insert looks new. Am I missing something or do I just need new cutters?
Thanks.
 
Couple of questions:

First, is the full profile cutter the correct one for the thread pitch?

Second, what is the OD of the threads?

Fitch
 
OK, I'll play the ignorant farm-boy here. My answer - take another light cut or two until they fit. :cool:

Am I missing something?:confused:

You should concentrate your efforts on a precise shoulder fit and not worry so much about thread fit. Of the 15 +/- threads, how many of them do you think actually make full contact?? Answer - not very many.:rolleyes:

Ray
 
Last edited by a moderator:
The job is getting the correct fit.

Greetings,
When I true an action I use a full profile internal insert and when I thread the barrel shank I use a full profile external insert. The beauty of full profile inserts is that the root and crest of the tread will remain correct regardless of the major on minor diameters.

Internally I chase the thread until it cleans up all of the way around. I feed straight out with the cross slide and record the amount of material removed.

Externally I add the amount of material removed from the receiver to the nominal size of the barrel shank plus an additional two or three thousandths. I then cut the external thread until I get the fit I want. You can continue to remove material from the part by cutting the thread deeper without changing the profile until you reduce the diameter so much that you need to change the shim in the in the toolholder to correct the lead angle.

It works for me.
Nic.
 
Henry,

The major diameter is probably what is giving you trouble. For a nominal 1.0625 tenon, I turn to 1.056 to 1.058. It's the pitch diameter that does the job, not the major or minor diameter. Turning 6 to 8 tho' undersize leaves a small flat on top of the threads that doesn't hurt a thing.

The pitch diameter is what thread wires measure, which is the "standard" for measuring threads.
 
Cheechako said:
OK, I'll play the ignorant farm-boy here. My answer - take another light cut or two until they fit. :cool:

Am I missing something?:confused:

You should concentrate your efforts on a precise shoulder fit and not worry so much about thread fit. Of the 15 +/- threads, how many of them do you think actually make full contact?? Answer - not very many.:rolleyes:

Ray
Click to expand...
Ray, I'm witchyew. I keep going in on the compound until the receiver screws on just as I want it to do.
 
Pitch Dia.

What Wayne is saying is correct,We cut hundreds of threads a year on precision aircraft parts,we would have all of our top notch inserts ground with a .005 to .010 tip radius to relive stress on the parts,we used the three wire method to inspect the parts.
 
Measuring external threads with three wires is cheap, accurate and easy to do. If you can't afford a pitch mic, buy some wires and use them.
I like to hold them in a piece of modeling clay but have also held them in a gum eraser.
Whatever works....
 
Some thoughts regarding carbide insert tooling.

First lets do a comparison. lets look at a carbide insert and a HSS piece of tool stock ground to cut threads.

What is the first thing a guy notices about the cutting surfaces?

HSS is sharp where's carbide is not (typically)

Now why is that?

HSS actually cuts.

Carbide inserts on the other hand work a little differently. In a highschool graduate/laymans/lazy guy explanation the insert gets the material almost to a molten state. It depends on pressure and surface speed to work properly. The high hardness and the radius's on the surfaces help mitigate the heat buildup. This discussion spawns into yet another debate over the use of intermittent coolant. The engineers from the tooling companies will tell you that the thermal shock causes rapid breakdown when using a misting coolant system. I've been told you go one of two ways. Dry or with flood coolant.

The part to pay attention to all this is the surface speed and pressure. Most often these inserts are designed for production CNC equipment programmed to run at speeds/feeds much higher than 99.9% of us are comfortable with on manual turning machines. I can cut a barrel thread at over 1200 rpm on a hardinge tool room lathe but not many of us have these machines and it takes some practice to keep the insert out of the shoulder.

I and many others have used carbide inserts for years on manual machines with good/great/exceptional results. Be that as it may its still a challenge to produce a bright shiny thread on a manual machine with these inserts. HSS steel on the other hand often does provided the tool bit is ground properly. The difference is that the HSS cuts well at the lower surface speed where's the carbide is only just getting started. It depends on the surface speed to load properly and develop the shearing action through heat. Running properly, the bulk of the heat goes out in the chip (blue chipping) and not in the substrate. HSS (even cobalt) would look like Chernobyl if this were attempted.

There are inserts out there that have sharp edges and I'd encourage you to look at them for what your doing. Typically they are non coated because the coating doesn't like sharp edges. It depends on a radius so that it has an even film thickness. A sharp edge will cause rapid breakdown of coatings. Kennametal makes some good ones. I don't recall the insert number right now.

Last is an example and I'm sure I'm not alone on this. Your at your machine and the thread is "almost there". You just need a spring pass or two to get a nice silky fit on the receiver. You go that one last pass and to your horror the receiver feels like the way H/S girlfriends do after prom. Insert tooling with radius'd edges seems to be more prone to doing this than the sharp stuff. That's been my experience anyway. Making sure your compound is at 29 degrees also helps since it reduces tool pressure a bit.

As mentioned, just squeak another pass. I used to take all the time to measure threads over wires or with a mic when fitting them to actions (Nesika receivers) In the end I just wrote programs on the CNC using variable macros and subroutines to get to the thread fit in a more efficient manner. The main advantage being the much higher surface speeds when turning threads. It was written in such a way to rough the thread out and then progressively get closer with .0005" passes with programmed stops between each pass to allow the operator to check the fit. (that and being able to use canned cycles that mitigate chatter by staggering the cutting depths.)

Hope this helped.

Chad
 
Last edited by a moderator:
NesikaChad said:
I and many others have used carbide inserts for years on manual machines with good/great/exceptional results. Be that as it may its still a challenge to produce a bright shiny thread on a manual machine with these inserts. HSS steel on the other hand often does provided the tool bit is ground properly. The difference is that the HSS cuts well at the lower surface speed where's the carbide is only just getting started. It depends on the surface speed to load properly and develop the shearing action through heat. Running properly, the bulk of the heat goes out in the chip (blue chipping) and not in the substrate. HSS (even cobalt) would look like Chernobyl if this were attempted.
Click to expand...
Not that I'm very experienced yet, but the other night while turning an old truck axle that is very hard I found that the carbide worked better producing a smoother finish when the speed was up to a minimum of 700rpm on my manual SB lathe. If I slowed down the speed the cutter would rip more than cut leaving an uneven finish and dulling the bit faster. Blue chipping is the only way these carbide bits would cut and leave the best finish with dark cutting oil. Wife complained about the smoke and fumes because of the heat.

Not the best material to cut, but a valuable lesson learned to me about carbide and HSS. I'm now convinced from others and my experience that unless you can do threading at high speeds with carbide bits, you will get a nicer finish at slow speeds [my preference] with HSS.

The only other factor I don't know yet is if it makes any difference with threading 416 or 4140 barrel steel as I don't have enough stock laying around to make comparative tests using carbide and HSS bits at the same slow backgear 38rpm speed to compare, but I will take the advise of NesikaChad here.
 
Last edited by a moderator:
Carbide Cutters

Nesika Chad has given an excellent explanation of the characteristics of carbide inserts. Kennametal uncoated inserts are available in a number of grades and styles. I have found that the K68 grade of uncoated inserts cut well at slower speeds and are tough enough for interrupted cuts, such as when turning split bolt sleeves. If you can run a bit faster, the KC730 grade of coated inserts are about as sharp as you can expect in a TiN coated insert, but are not as tough.

Quality hand sharpened cobalt steel tools are probably best for slow speed machining and for the best finish, but for convenience, I still use carbide most of the time.

Scott Roeder
 
One must shop wisely for inserts

There are several manufactures that make positive rake carbide inserts and you need to use them in the correct tool holder. These positive rake inserts are available in both coated and uncoated in several grades. If you try to use negative rake carbide inserts at too few SFPM and/or too slow of a feed you will have poor results. If you nail the SFPM and feed speed but do not have a ridged set-up in a ridged machine you will have poor results. If you try to use a negative rake insert in a positive rake holder you will have a mess because of insufficient nose relief.

For threading I like and use Kennametal Lay-down Full Profile inserts. These have plenty of positive rake and nose relief to work well at “human” speeds and by changing the shim you can correct the helix angle for any pitch diameter.

For turning I like and use Interstate 60 degree triangular single sided inserts ground with chip breakers and positive rake. These inserts provide you with a selection of nose radiuses and have plenty of nose relief. The tool holders are available in several different configurations depending on application.

For cutting muzzle crowns I like and use only Cobalt High Speed Steel hollow ground and honed by hand. I grind these like a 60 degree threading tool except I put in a ton of nose relief, about 10 degrees of positive rake and about a .020 radius on the nose.

Individual results may vary,
Nic.
 
One way to get the cutting speed up is to turn the barrel thread upsidedown and backwards. You are feeding away from the shoulder. (assuming the barrel is in the headstock) Easier to start at speed in the groove then to stop there. You mount the cutter upside down and run the lathe in reverse, and feed laft to right. This is also a good way to control threading on and internal threading job. Only on the internal job you want the cutter against the inside backwall so you can see it.
 
There is a problem ...

... with that method. You must have a thread relief at the shoulder for an external thread and if you are one to set back your barrel then you must deal with that down the road. Another problem is that you have zip and pip for error when engaging the half nut and zero chance for taking up the entire amount of backlash before the cutter starts cutting the thread. Internally as in a receiver you will cause a weak point right at the end of the barrel shank with that thread relief. Some actions are already thin enough without exacerbating the situation with a thread relief. All of the force is retained by the area between the end of the threads in the receiver between the locking lug abutments and the end of the barrel shank. This is the thinnest section of the receiver, if you cut a thread relief at the end of the threads you will reduce the strength of the receiver and create a stress riser to speed failure along.

A properly cut external thread will tail out at the end from the root diameter to the major diameter; an internal thread will be the opposite. Neither will have a radial groove perpendicular to the axis to make a weak point and stress riser. The helix angle of the thread will spread out the force along the axis of the thread unless you cut a thread relief where it will focus this force.

Again Individual results may vary,
Nic.
 
Henry
Cheapest way is to switch to a partial profile insert and the plus side is you can cut more than one thread pitch. I am a manual lathe user. I wanted this set up for the internal indexed cutter because of the interrupted threads from base screw holes and other cuts in receivers I work on. It is a PITA to break a tip on a hand ground internal thread set up and have to set up again after regrinding the tip. Look in the catalogs for your holder and get the partial profile insert.
BV
 
Last edited by a moderator:
Niccolo, There are some, maybe many, who cut stopped threads up to a shoulder without a groove. I personally find that it isn't worth the trouble. I don't like to design things so close that a groove the depth of the threads is going to compromise the strength of the project. However, the upside down and backwards method is an easy way to cut nice threads at a higher tool speed up to a shoulder, anybody can do it, even mere mortals out there maybe trying this for the first time.
 
papapaul said:
Niccolo, There are some, maybe many, who cut stopped threads up to a shoulder without a groove. I personally find that it isn't worth the trouble. I don't like to design things so close that a groove the depth of the threads is going to compromise the strength of the project. However, the upside down and backwards method is an easy way to cut nice threads at a higher tool speed up to a shoulder, anybody can do it, even mere mortals out there maybe trying this for the first time.
Click to expand...
I think I am going to try it. Let me see if I have this straight.

For external threads, install the tool pointing toward you and position it around on the back side of the work. Make sure the cutting tip is at the center line of the work. Move the tool in at the shoulder (thread relief). Then start the lathe in reverse, and engage the half nut at the appropriate number. Is this right?

For internal threads the only difference would be that the threading tool would be facing away from you on the back side of the internal hole. Is this right?
 
You must log in or register to reply here.
Back
Top