Carbide Insert Threading Tools and Helix Angle for Manual Threading

I'm about to get started with carbide insert threading tools. I'll be using the tool on my Hardinge HLV-H for manual single point thread cutting.

I'm trying this out because I've been disappointed with the quality of brazed carbide threading tools (the ones coming out of CN these days are pretty rough) and the finish I can get with them. I can't find HSS threading tools for some of the threads I need to cut (or that can work close to a shoulder), and I'm hoping for better thread finish needing less work after cutting..

I cut fine pitch threads with relatively large diameters for the pitch. Always in 6061 or 7075 aluminum, 360 brass and sometimes free machining steel (C12L14, C1215).

Examples:

1.000" - 32 TPI Helix 0.58º ("C" lens mount)
1.035" - 40 TPI Helix 0.34º ("SM1" lens thread)

M28.0 x 0.75 Helix 0.50º
M30.5 x 0.50 Helix 0.30º

I've cut all of these before but I usually need to either run an adjustable die (when available) to clean up the thread, or run a CNC machined matching female thread with non-embedding lapping compound to clean up the thread.

I know the insert holder (will be using 16ER for external) has a 1.5º helix angle, and a "neutral" shim. I'm trying to get the other shims that will give me a choice of helix angles.

How closely do I need to match the angle of the insert with the helix angle of the thread I want to cut?

Thanks!

Don't they make inserts with the proper angle already built in? I don't know. For a thread that fine, I would think matching the angles, and using a dead sharp cutting tool, would be the most important thing. I finally gave up on threading with carbide, and went back to small (1/4") hand-ground HSS blanks. Having much better luck that way, nice smooth finish and I can work up to a shoulder.

I think (but others can object) that the functional helix angle for the threads you're dealing with mean that the "normal" clearance angles of the inserts themselves will give all the relief you need. So all you should need are neutral holders. At least, this should be the case with external threads, which is what it seems you're cutting.

It's when you're cutting very course threads relative to diameter that you have to worry about flank clearance to the material helix. Your threads are so "fine" that this isn't an issue.

My experience with the Carmex inserts and anvils (and I think common to all the 'laydown' style) is that you seldom get into a helix angle that requires an anvil change. I think about the only time I had to worry about it was when I was cutting a 8tpi acme on 1/2" stock, I recall having to go up one size in the anvil.

A quick and dirty is to throw a small shim under one side of the holder to tip it to the right angle.

Ed.

I think you can cut all four of those threads with the same tool, no helix adjustment needed. Will the parts be inspected?

Unless you are making many parts you might grind it your self.

Thanks for the replies so far. I'm going to be using a Carmex 16ER holder.

The parts won't be inspected except by me - they have to fit the mating part properly. I do have thread micrometers but usually I'm after a good fit without excessive play.

I'm going to be testing full profile threading inserts. Hoping that these will clean up the threads by cutting the crest. That would leave me with less deburring and lapping to do.

Try holding a wad of fine steel wool against the thread while its turning. Naturally you will want to do this safely. Low speed and great care given to your fingers.

I used to make adapters for antique lenses. Every thread imaginable and had to match up to an often well used thread. I found that cutting until I got a snug fit and then a good polish gave a nice look and fit.

You might try a similar approach, cutting to a slightly large standard and then a little polish to make a smooth finish and fit

henrya said:

Try holding a wad of fine steel wool against the thread while its turning...I used to make adapters for antique lenses.

Click to expand...

Nearly all the threads I'm turning are for optical purposes. Mostly for optical testing equipment meant to test cinematographic lenses. What kind of adapters did you make?

Thanks for the suggestion, I haven't tried that. I've used fine wet-or-dry sandpaper and Scotch-Brite.

One potential problem with steel wool for aluminum threads is that some of the steel particles shredded could get embedded in the thread and cause problems in anodizing. Ill try the fine steel wool (I have some 000) on my next fine steel or brass threads and see how that works.

The way the anvil system for laydown threading inserts is described by the manufacturers is confusing. I've resorted to reading the tech section from each of the manufacturers to get a slightly different explanation to help me have a complete understanding.

It now seems to me that the standard 1.5º angle is the insert inclination angle, and that this angle needs to be 0.5º greater than the helix angle of the thread.

So: 1.5º insert angle for helix >1º, <2º
0.5º insert angle for helix <1º

Please let me know if I'm finally on the right track...

I used HSS ground with plenty of clearance all around. More positive rake is your friend here as would be the ability to thread at higher speeds. But what you are doing will be tough without some auto kick out or cutting the thread from the back side and feeding out away from the shoulder. The good news for you is that the material you are cutting is prone to give a good finish when you figure out what it needs. The faster the better, governed by your reflexes to pull out in time. I like LPS Gold #1 for cutting and turning when looking for a very fine finish.

I mostly made adapters and flanges to mount antique lenses and shutters on large format cameras. Sometimes with 100 + year old glass big as an quart can on a lens board for a 11x14 camera. What you are doing is some different, but I know you are likely threading about a quarter inch section and up to a shoulder. The important for testing is that the lens be right on axis and dead square to the film or sensor plane. You probably already know that.

I think there are inserts out there somewhere with high positive addressing to the material. Thinbit could make some for you if nothing else comes up. The inserts you will find most of are really intended for high speed cnc machines. Unless you are making lots of parts HSS will work better if you keep them honed sharp as you can. Maybe every 10 parts, hone with a fine stone right on top.

Threading and Chamfering Products

Full profile ER inserts are definitely the best option for the threads you are making. Standard shim will be fine.

One thing that WILL matter, in particular in aluminium, and especially since you are threading on a manual lathe, that you get correct grade and geometry inserts for the materials you are cutting. Typical steel grade coated inserts will work very poorly in aluminium when running at the low RPM necessitated by manual threading. You are going to want ground and uncoated, ideally polished inserts for the aluminium. Brass and steel will be fine with basic coated inserts.

Do that, with some light cutting oil, using very small depths of cut, and you will have perfect threads straight off the machine with no finishing required.

I have always found a back rake and or a side cutting edge positive rake angle makes the best thread in mild steel, aluminum ND BRASS. For going in at 30* side cutting edge positive rake can be a big aid. Going straight in at the bottom of the thread the whole cutting edge is in the cutting action so there is so much cutting edge trying to cut that a final light cut is near impossible, even with having radial positive rake only. For example, if you tried to scrape vanish with a 2" wide scraper you could push down hard enough to penetrate the varnish / But with a scraper 12" wide you could not push down hard to penetrate the varnish.

Cutting a thread on a tube is even more need for the ease of cutting a positive side cutting edge gives because high cutting forces cause the tube to be pushed away and distorted. *A tube might be filled with a plug to make it more solid to resist cutting forces.

Here find a thread cutting insert. Note the top clearance is give as positive. I think giving both radial and axial clearance is important but inserts are not descriptive on that. I don't even see a threading insert with both side and back rake.
Perhaps knowledge about cutting tool geometry is being lost.
CARMEX Threading Insert, 16ERAG, External, Partial Profile 60deg - 4JHC6'|'16 ER AG60 BMA - Grainger

Wow, just about everything is poor design for threads on such as a thin tube.
https://www.mscdirect.com/browse/tn...Mill-Inserts/Threading-Inserts?navid=12107172

* Here is a positive / positive insert
60deg V-Threading - Double Ended Positive Rake – Exact Tooling 3* x 5* (5* x 5* would be better, diamond tip or HSS likely/may be better than carbide. (should be fingernail shaving sharp)

About threading tubing:

For this, don’t do it.

Start with solid bar, turn the od, cut the thread, then bore the inside and part off. This makes the set-up as rigid as possible and the solid material is less expensive than tubing.

(michiganbuck posted some good insert prospects above)

Fine threads at those diameters will have very little helix angle. Given the unusual application (in todays CNC oriented world) you should call and talk with your company of choice and see what they recommend.

Fine bronze wool may work better than the steel wool for your deburring.

Another deburring option would be to mold a thread chaser using metal filled epoxy. Devcon makes epoxy's with many different fillers, including bronze, titanium, stainless, carbide, alumina microbeads and others. As the epoxy wears away the filler would burnish the aluminum.

Consider mounting your bodies on expanding collets or boring them to size and gluing them to a sliding fit bar you can mount between centers. These will allow you to face both ends and to do external threading on both ends in the same set up. With the right set up you could do internal and external threading on one end and face and do external threading on the other, all concentric to the same axis.

henrya said:

.....For this, don’t do it.
Start with solid bar, turn the od, cut the thread, then bore the inside and part off. This makes the set-up as rigid as possible and the solid material is less expensive than tubing.

Click to expand...

Why in such easy to cut material?
In lens mount thread surface finish is king.
One can get away with murder in the thread form and PD but it has to glass smooth and the lockup 90 wall has to be spot on nice.
This is so way different than cutting a threaded shaft for a nut.
Bob

CarbideBob said:

Why in such easy to cut material?
In lens mount thread surface finish is king.
One can get away with murder in the thread form and PD but it has to glass smooth and the lockup 90 wall has to be spot on nice.
This is so way different than cutting a threaded shaft for a nut.
Bob

Click to expand...

Because the end result will likely have threads both ends and the part may only be 1/2 long and perhaps only 1/8 thick. Having the part rigid and planning the last operation to be the part off and drop onto a dowel rod. Done. No messin’ around with funny work holding methods or distortion of the part.

Why solid and not tube? I’m wrong. Just checked prices and at the OPs requirement tube is much cheaper. I used to buy 4-6” diameter material and solid was often cheaper and easier to get.

michiganbuck said:

I have always found a back rake and or a side cutting edge positive rake angle makes the best thread in mild steel, aluminum ND BRASS. For going in at 30* side cutting edge positive rake can be a big aid. Going straight in at the bottom of the thread the whole cutting edge is in the cutting action so there is so much cutting edge trying to cut that a final light cut is near impossible, even with having radial positive rake only. For example, if you tried to scrape vanish with a 2" wide scraper you could push down hard enough to penetrate the varnish / But with a scraper 12" wide you could not push down hard to penetrate the varnish.

Cutting a thread on a tube is even more need for the ease of cutting a positive side cutting edge gives because high cutting forces cause the tube to be pushed away and distorted. *A tube might be filled with a plug to make it more solid to resist cutting forces.

Here find a thread cutting insert. Note the top clearance is give as positive. I think giving both radial and axial clearance is important but inserts are not descriptive on that. I don't even see a threading insert with both side and back rake.
Perhaps knowledge about cutting tool geometry is being lost.
CARMEX Threading Insert, 16ERAG, External, Partial Profile 60deg - 4JHC6'|'16 ER AG60 BMA - Grainger

Wow, just about everything is poor design for threads on such as a thin tube.
https://www.mscdirect.com/browse/tn...Mill-Inserts/Threading-Inserts?navid=12107172

* Here is a positive / positive insert
60deg V-Threading - Double Ended Positive Rake – Exact Tooling 3* x 5* (5* x 5* would be better, diamond tip or HSS likely/may be better than carbide. (should be fingernail shaving sharp)

Click to expand...

what is the 3° on the last insert?

cratex (or equivalent) works well for conditioning threads.

Perhaps this little machine shop description at the bottom of my post shows side and back rake better. These are the angles of the tool bit top face that faces the part in the direction (s) that the force is applied to the part. . One top face angle is toward the lathe spindle rotation, and the other to the side or to the travel of the tool bit as it travels toward the headstock. These top of the tool bit/inset fave are important to how the material is taken from the part. with more/increased positive angle a free-flowing material like mild steel and aluminum comes off the part with less force required. This reduction of forces reduces the tendency of the part pushing away. deflecting, causing a machine or part chatter, along with reducing the removed material to be compacted or pushed together onto itself allowing a much better surface finish on the part.

The top face angles are called top and side rake angles also called axial and radial angles ar attitudes. These two angles may be positive, negative, or neutral. Neutral being no angle or right angle towards the part center to the part. Negative is the top face faces angle tilts downward.

The use of
Positive top and side rake angles to such as turning threads on a tobe tube will give a much better surface finish.

Much of the need for after turning/threading repair may be due to the part material compacting onto /into itself because of not having the material free-flowing that a positive top face rake angles would provide...along with inserting a plug to the ID of the part to make it more solid. to the cutting forces.

Turning a thread should be just another turning operation and so should achieve the same very good surface finish that you should expect as simply turning the OD of a part. perhaps along with a thread crest ridge. The thread crest ridge should be filed or honed prior to the last finish cut pass.

A good example of forces applied might be to whittle a piece of wood with the knife angle positive, neutral and negative the the the wood surface.

From this, you see that for aluminum and mild steel a greater, more positive rale angle is suggested.
https://littlemachineshop.com/images/gallery/instructions/grindingtoolbits.pdf