I an in need of some recommendations on inserts for tool holders already on hand.  The various inserts we have leave too much to be desired for most the everyday materials and conditions we have at work.  This has left me to grind brazed carbide tools to meet the conditions, and I have become quite good at it.  But, while I want to train others to do much of what I do, I am still having to grind, and sharpen tools for them.  Suitable inserts would make it easier for me to get others to cutting metal while I do other stuff.  Haphazard trying this or that insert is not really in the budget, and is what, I think, has caused the assortment of unsuitable inserts in stock.

The first problem, is likely that the machines are old and do not have the horsepower, nor surface speed for many of the modern inserts.  For example a lathe that swings 28 inches, has only a 7.5 Hp motor, and maximum speed of 900 RPM.  Second, most of the machining is relatively dry.  Flood coolant is not going to happen.  A misting coolant is about as sophisticated as it gets.  Brushed on cutting oil is more common, but is also sparingly used.  Third, it may be due to the tool holders themselves being a bit incompatible with the realities of the conditions.

The materials that need to be bored and turned are as follows in order of frequency and quantity:
Grey Cast Iron in different hardness states but usually fairly soft,
Mechanical Tubing mostly seamless mild steel (ASTM A513 and A519) ( Note, this material is particularly difficult to get chips to break and not chatter. The final wall is often less than 1/8"),
Free Machining Steel in the form of unbored couplers,  
Pure or nearly pure Copper (DC armature commutators e.g.),
1045 Steel Shaft material normalized,
Plasma Cut Mild Steel Plate,
4140 steel bar, and DOM tubing,
Bronze ranging from just copper/tin alloys to heavily leaded to phosphorous alloys (aluminum bronze is rarely encountered),
304/303 Stainless Steel,
416 Stainless Steel,
Aluminum of various alloys, including cast.
Linen filled Micarta,
Other plastics and epoxies.  

The list of tool holders on hand are:
MWLNR-16-4W  (tool holder not boring bar)
A16MWLNR3  (Hertel Boring Bar)
RTBAP-20-3 KM4 ( Sandvik Boring Bar)
MTGNR 16 3C L4M  (tool holder)
No. TL 12 (Armstrong tool holder)
S32V-MCLNR-4 (Valenite Boring Bar)

The last thing to consider is the tolerances in which I need to work.  The final finish should be better than 32 micro inches, and the size is often well within 0.001" and often within 0.0006".  

https://www.youtube.com/watch?v=rsFFWYo8ugw


Carbide likes heat you either run it dry or flood it like a CNC does.


https://www.kennametal.com/us/en/home.html  bottom left of web page  >>>>====>  Product Support

Your material range is about like mine, no one insert grade or geometry will cover all of it well. For ferrous materials I have great results with SECO Duratomic inserts, select the geometry suited to the application such as roughing vs. finishing. Non-ferrous materials require different geometry altogether,  positive rake angles and a sharper edge with little to no edge hone. You can get trigon inserts with positive geometry but you typically only get one side of the insert so you lose 3 corners.  Also stay away from any coating on inserts used on aluminum that have any aluminum in the coating, like TiAlN or AlCrO, those are more likely to fail due to a build up of material on the edge since the aluminum will bond to those coatings at heat. Any of the geometries that work well for non-ferrous also work on the polymers and composites.

I have so many different grades and geometries in inserts it is hard to remember all of them, they each have a purpose though. None of the manufacturers are the best at everything so I have tools from many of them that represent what I have found to be the best tools for a particular application.

This is all good advice.  

OP you have several different challenges.  The SECO duratomic inserts are excellent.  They make grades for stainless and carbon steels.  They are perfectly happy to run dry within reason.

I like Mitsubishi for aluminum/plastics

Chatter on thin walled stuff is tricky but usually a smaller nose radius will help a lot.  Typical inserts are .03, if you rough with a .03 and drop down to .015 when you get to finish passes it'll be more forgiving.  It's a harmonic problem and changing rpm is the next best thing to try.  Usually slower but sometimes going faster gets you out of the bad frequency. It's all a function of how far work and tools are hanging out.

Plasma cut can be damn near laser like or cutting torch ugly. The HAZ is pretty much murder on harder grade inserts like those for stainless.  Rough that off with dead inserts or a softer grade that won't explode.  Finish with a grade appropriate to the material.

Breaking chips in gummy material may not be possible depending on conditions.  Depth of cut, surface feet, and chip load all play a part and you may have to choose between breaking chips, and some of your other requirements like finish.  Thats when setup rigidity and speed/hp matter..

Getting inserts specific to the material will help.  A carbon steel grade will cut stainless but it may not have an aggressive enough chip breaker.

Breaking chips while boring thin wall tubing has been, in my experience, one of the best ways to avoid bad finishes and control size.  When long strings of chips wrap around the tool, the following things generally happen: the tip of the tool breaks; the chips themselves scratch the newly machined surface; the chips load up and push the boring bar away, which creates a ledge, or a bump.  Small chips can be blown out during the cut and just tend to litter the shop from the chuck fan blades (also known as jaws).

Chatter, too, seems go go away with well behaved chips and a well shaped tool.  Sometimes I have had to wrap the tube in rubber, or when turning the O.D. stuff a length of thin horse stall matting into the tube.  

I was rather hoping for suggestions on which chip breaker styles folks have found to be useful in the sizes and shapes I have tools for.

Another thing that may narrow choices (and might make some selections non-existent) is my finish cuts are generally 0.010 to 0.007 deep.  This is especially true when machining a cast iron repair sleeve in a motor end bracket.  The brand of sleeve we use only has 0.060 or so on diameter material to take out.  I have to do this in three or four passes, depending on how the machine and tool is behaving that day.

I'd get the Iscar or whoever you like guy in there to get you a package together. There's so made grades and so many situations, it's hard to say "just buy this."

Unless it's OD grooving, then you buy Iscar Penta in IC-908.

I run mostly CNMG inserts for OD turning and larger boring jobs.  Seco MF4 breakers on stainless 304-316 work well. They will handle pretty much anything in steel, if I had to use one grade/breaker for steel that would be it. For carbon steels I use the M3 breaker. TP2501 and TM2501 grades.  It all just depends on whether SECO offers those in your required geometry.

I use same holders for aluminum but the insert is specific to non ferrous. It has a huge positive rake and aggressive breaker. Mitsubishi CNGG .008 nose radius...I can't remember the breaker or grade but I don't think they offer many options.

Yep anything that will change the harmonic of the setup, dampen it will help.  rubber is perfect.  Changing up the nose radius and speed help prevent harmonics, sometimes you just can't so what you're doing is the next step.

I hear what you're saying about chip control, rats nests always cause issues.

One thing I didn't mention, and you may not have enough speed (how big are these parts anyway?) is using CBN for cast iron and diamond for copper.    Both require higher surface speeds but the results are pretty impressive. Excellent finishes.  It all depends on the machine and setup stability.  Both are $$ and don't tolerate abuse well.   If they aren't abused they tend to last forever.  Probably not the right tools for the less skilled operators.

I don't see any issue with a .007 finish cut, lots of materials and tools will finish better with a little deeper cut like that.  But it all comes down to the machine, setup and parameters.  There isn't any one answer, you just have to get the basics as good as possible, pick an appropriate tool and experiment with parameters.

I have these little ID groove bars, indexable, gotta be the smallest bar before they go to solids.  I need them for making o-ring grooves, they cost like $250 and they are so fragile. The inserts are $20 something each and are tiny.

One errant chip seems to rip the ends right off them, I have a box of dead ones that must have cost 5k.

I swear they make them fragile on purpose.

Iscar can bite me. 908 is a good grade though.

My parts vary in size.  All the way from about 1" (sometimes smaller but rarely) to 38" O.Ds. (I have a lathe that will swing 42" in the gap.) Inside bores are generally 1.5" and up to 12"  Occasionally smaller or larger, but not often.  

I so have a feeling that in many cases the RPM is going to be a bit of a problem. The other is lack of horsepower for the high speeds.  I have nearly stopped the machines when making heavy cuts with highspeed steel tools.  The faster RPM required of carbide, would certainly not work.

One thing of note, I tend to grind the brazed carbide tools like I would for Highspeed steel, and even at 3 times the normal highspeed steel surface speeds, I still only get light straw chips.  I have to get to 4.5 times that before I can be sure to get blue chips.  With the inserts I've tried, blue chips occur at about 2.5 time highspeed steel speeds.  Plus, there is noticeable loading of the motor. (Same material, same machine, same set-up, same day.)

Makes sense, hss type grinds are sharp, carbide doesn't like to do sharp. It's too brittle, so a lot of carbide inserts tend to have little relief angle and a very stout cutting edge.

More of a grip it and rip it style cutting.  It needs more torque and causes more heat, but they last longer and in 30 seconds or less you can index the insert and typically repeat within a thou or so.

They do make positive inserts, ccmt is a common one.  Typically they aren't double sided so you don't get as much life out of them, but they are effectively sharper and take less torque. They also lower the cutting forces so they will behave more like a ground brazed tool.

Sharper positive inserts aren't really roughing tools, they just don't hold up.  So you may have to find one tool for roughing and switch to a hand ground or positive insert for finishing.

As for speeds, on the smaller stuff you might not have enough rpm, but as you get out around 8 or 10 inches 900 rpms is getting into serious surface feet for everything except aluminum maybe.

Inserts will work at lower speeds just fine, but you might not get the absolute best finish or chip breaking.

You may find that the machines are happier at higher RPMs. Low speed requires torque, you could find that higher speeds with a lesser depth of cut actually works better and gets the job done in the same amount of time.

I have lathes with sub spindles that typically have about half as much power as the main spindle. I play the rpm/depth of cut game all the time.

There are so many choices and options you just need to experiment to find what works.  Ideally a local tooling rep would give you some samples and things to try.  Worse case hit MSC and order one or two of an insert and try it..