- Joined
- Oct 28, 2009
- Messages
- 58
- Reaction score
- 36
Pardon me, as a new contributor to this site, for plunging into the topic of using tungsten carbide inserts on small manual home lathes. This has probably been hashed over before. And let me make it clear that Im not trying to convert anybody away from HSS. If HSS does everything you ask of it, you have the most cost-effective cutters. If I had spent 10 years problem solving CNC applications with HSS, Id be writing about it instead of carbide inserts.
I agree that most tungsten carbide inserts are not suitable for small lathes. But some of them are. I'd like to contribute some of my experience to those who DO want to use tungsten carbide inserts on small lathes. They have become an integral tool in my workshop, but they are not right for everybody or for every situation. Allow me to share what I have learned, and what works for me. I think that too a large degree people have bad experiences using tungsten carbide on small manual machines because they did not know how to select the inserts with correct features. And, unfortunately for the hobbyist, economy carbide is generally not available with the right features. If you are happy with HSS, don't waste your time reading any further, for changing to carbide would be a waste of money for you. Personally, changing to carbide made my hobby a lot more fun and productive. Your mileage will vary. Being a jack-of-all-trades kind of guy, I'm not an expert in any one field, and can only claim amateur abilities in my home shop. Almost my entire career involved some aspect of using tungsten carbide. I began my career with 11 years as a product evaluation engineer for a major manufacturer of oil field rock drilling bits using tungsten carbide teeth, and finished it with 11 years as a tungsten carbide tooling sales rep for Iscar, Valenite, and Mitsubishi Carbide. I sold tungsten carbide inserts to manufacturers and machine shops in Washington, Oregon, Idaho, Montana, Wyoming, Colorado, and Utah. The most common materials used in these states are steel, stainless, aluminum and high temperature alloys, so I have very little experience with cast iron. This was the great job for a home shop machinist, for many days I couldn't tell when the hobby stopped and the work began. I always took a problem solving, applications approach to my customers, and most of them appreciated that I machined for a hobby. When I faced particularly difficult or unfamiliar materials, I commonly took scrap samples home to learn how to machine it on my own lathe. I couldn't duplicate what their CNC machines could do, and I do all of my machining dry, but what I learned with my 1.5 HP lathe could often be scaled up to their 20 HP machines. I retired about 4 years ago. I have no ties with, and receive no retirement benefits from any of my former employers.
First, my experience with HSS. My exposure to sharpening and using HSS bits is far from professional level. My grandfather was a tool room machinist, and I have inherited hundreds of HSS bit that he had ground to a wide assortment of configurations. My dad taught me to run a lathe and to sharpen HSS bits. And, believe it or not, sharpening and using HSS bits was a requirement for my BS Mechanical Engineering degree at Cal Poly, San Luis Obispo, CA, whose motto is "Learn by Doing". However, since I've learned to use tungsten carbide inserts, my enjoyment level has soared while my frustration level has dropped. I now use HSS for less than 5% of my lathe work. Chip control is much better. Surface finishes are much improved. Dimensions are more predictable. I don't have to use coolant no matter what SFM I choose to run. And I no longer wrestle when I pick up a piece of material of unknown alloy. I primarily machine steel, stainless, aluminum, brass, wood and plastic, but I've successfully machined on my lathe the toughest materials that my customers encountered: spin-cast stainlesses, titanium, nitronic, inconel, hastelloy. Indexable carbide inserts have become my first choice for turning, facing, boring, grooving, threading and partoff in all of these materials - even plastic.
Some thoughts on using tungsten carbide in a home shop- (I refer to the products of Iscar, Valenite, and Mitsubishi due to my familiarity with them - most of the other major manufacturers offer comparable products. Ask them for details.)
- Lathe Horsepower, Drive, and Rigidity
If you have less than 1 HP, your machine is probably too small to use the same inserts tha I do. You'd probably be better off with HSS, or positive, single-sided insert holders. I agree with most of what is said in the website http://www.thegallos.com/carbide.htm. But I prefer not to use the TiN coatings or utility grade inserts on a small lathe because they don't have what I feel is a sharp enough edge. I have a Taiwanese 12" gear-driven Birmingham lathe that I inherited from my dad. It replaced an old belt-driven 12" Logan. I couldn't recommend carbide tooling for the Logan since it was worn and sloppy, and I don't think the belt would have transmitted the required power for partoff. The Taiwanese lathe came with a motor rating of 1.5 HP, but the starting windings burned out one day as I made repeated partoffs with a carbide insert partoff tool (see more below). The replacement US-made motor also has a rating of 1.5 HP, but appears to have much more power than the original, so my experiences are based upon this new motor, and this is probably a good lower horsepower limit to my recommendations here. I commonly limit my maximum DOC to .040", but if I recall correctly, I've pushed it to .070" DOC in steel without a problem. Carbide doesn't like flexible setups, or chatter, so if your machine is old and loose, you might as well stop reading this. And, as a rule of thumb, if your manual lathe is too small to hold at least 3/4" shank tooling, stick with HSS or single-sided inserts. The sharp carbide I'm recommending doesn't tolerate chatter, heavy interrupted cuts, or the unfortunate goof.
- Brazed Carbide
My comments here relate to indexable tungsten carbide inserts. Brazed tungsten carbide stick tools have their place, but they don't have any place in my shop. Inserts offer repeatablity, accurate indexability, positive geometries, chip control, coating options, accurate corner radii, no grinding, and they are not subjected to the heat from brazing - features I've never enjoyed from brazed carbide. If you want to use brazed carbide, maybe someone else here can give some pointers. I threw all of mine away years ago.
- Costs
I use 3/4" and 1" shank OD turning tools. A holder will cost about $80 to $100. The insert styles I prefer cost about $14 to $18 apiece when bought in boxes of ten. Most distributors don't sell partial boxes of inserts, but some do, so ask. MSC sells single inserts at a higher individual cost. You'll have to evaluate for yourself if you can justify the expense. In my case, I feel that if can't afford the inserts, I can't afford the hobby. I'd avoid the no-name carbide sold by the lower echelon suppliers. This is sometimes made from re-ground used carbide, unpredictable, and unlikely to come with the top-face geometries and sharp cutting edges that a small lathe needs.
- Carbide Grades
Wow - how to summarize such a broad topic in few words. In general terms, carbide grades are a compromise between toughness and heat/wear resistance. Most inserts are optimized for use in high production CNC environments, where cost savings are often found in higher feeds and speeds, which result in higher temperature. Like most materials, tungsten carbide is sensitive to high temperatures, so most industry research is in the direction of increasing heat resistance. That's not a factor for most hobbyists. When my face is 18 inches or less from a spinning chuck, I tend to keep the feeds and speeds down. I'm looking for toughness in an insert because my manual lathe doesn't have the rigidity of a CNC, and my boneheaded handle-cranking is by no means repeatable, or predictable. I prefer to have an insert wear rather than chip. The demands of industry have lead to grades specific to certain materials, but where I may be turning steel, stainless and brass all on the same day, or same hour, I want a general purpose grade. A C2 grade is a good compromise for most metals, or a C5 if you turn mostly steels. Coatings help
primarily by protecting the inserts from the heat of cutting, but it is a little talked about fact that the act of applying the coatings in hot furnaces degrades the toughness of the base carbide. Some recent advances in carbide technology have focused on minimizing that effect. In many cases the home shop machinist would be better off with an uncoated insert in order to optimize toughness and edge sharpness, and you also save a couple of bucks per insert. I'd change to a coated grade if I were experiencing built-up edge (where the material adheres to the insert), or if I did a lot of stainless steel. If I were to suggest a coating for general home use, it would be one that uses a PVD, rather than a CVD, process, due to the lower coating furnace temperatures, and the typically thinner, more lubricious coatings. The PVD process can also coat up to a sharp edge, where the CVD process requires a rounded honed edge. My favorite coating materials are TiCN (titanium carbo-nitride), and TiAlN (titanium aluminum nitride). Counter-intuitively, TiAlN is a wonderfully temperature resistant coating initially designed for use without coolant, but it also offers a high lubricity factor, which helps prevent built-up edge. To the best of my knowledge, the toughest coated insert in the industry is Iscar's IC3028 (IC328 for milling and partoff). I can't verify it, but I have been told that it's toughness, measured in Transverse Rupture Strength, while not equal to HSS, is at least in the ballpark with HSS. This has a PVD TiCN coating. The TiAlN coating version is called IC9028. The uncoated version of this is IC28 grade. This is classified as a non-ferrous grade, and is not optimized for steel but will work in steel, too. All major manufacturers offer something competitive with this, and what they have on their conversion chart that's equivalent to Iscar's grades are what you want. ( Grade numbers are added and deleted constantly. I left Iscar 10 years ago, so specifics may have changed since then, but IC 28/IC328/IC3028 have been been benchmark grades for them.) Unfortunately, the toughest grades generally aren't available with the chipformers designed for light depths of cut. Even though I call it roughing on MY lathe, .040" DOC is generally considered a finishing application, so these inserts tend to come with wear resistant grades to handle the higher SFM's commonly used in industry. So when I choose a finishing chipformer, I have to compromise and select the toughest grade available in that configuration.
- Insert Shape
The most commonly used insert shape and size is the double-sided 80 degree diamond, such as the CNMG432. With its 80 degree included angle, it can cut up to a 90 shoulder. Its popularity ensures that it is available in the most configurations and grades that are of interest to me, and at the most competitive costs. EVERYBODY makes CNMG's. There is valid ground to argue for a narrower angle, like a DNMG-style, if needed, but these will cost more, and offer fewer choices. I use a VNMG-style insert for profiling and reaching into tight corners. There is also a very valid argument for using single-sided "positive" inserts. They are freer cutting, and if you need the freest cut, they are the way to go. But the cost per edge is higher than a double-sided insert with the same features, and there are fewer options available if you need to address a specific application problem in the future. I can't remember any instance where the "up-sharp" double-sided "negative" inserts didn't provide a free enough cut for me, but cutting a long, slender shaft might be more of a challenge. Since I'm an amateur and more likely to chip an insert than wear it away, the double-sided, four-cornered CNMG-style is my choice if I could only have one. The third letter of the ANSI/ISO nomenclature (M in this case) denotes the tolerance class. The two
most common options are "M" and "G". It helps a home shop machinist to equate the "M" with "as molded", and the "G" with "as ground". As an insert comes out of its molding process, the cutting edge has a "hone" of .005" or more. This is well illustrated in Mitsubishi's product bulletin #B036A.
http://www.mitsubishicarbide.com/mmus/catalog/pdf/b/b036a_200710.pdf
Zoom in on the photos on page 2 where they distinguish between the "M class" and "G class" inserts. This edge hone is advantageous in most applications in order to keep the cutting edge from chipping. To get an "up-sharp" edge or tighter tolerance, the insert must be peripherally ground. Most manufacturers call these CNGG's or CNGP's. This adds several dollars to the cost of each insert, but this is a necessity for most aluminums, titanium, plastics, or wood. I use up-sharp inserts for taking depths-of-cut from .0005 to .040, even in steel. But when I recently turned cast iron for the MLA Diesel, I changed to an insert with an edge hone. For aluminum and plastic, I prefer (but seldom use) inserts that are both ground and polished. The top faces of these are polished to practically a mirror finish, which greatly helps to prevent builtup edge from forming. They are quite pricey, and are hard to justify for the small quantities I produce. When dragged by hand across the top of your thumbnail, a proper CNGG or CNGP will easily shave off some thumbnail material. A CNMG will not I save those for cast iron or heavy hogging in steel. The third digit designates the cutting tip corner radius. For a CNMG432, this is the "2", indicating a 1/32" radius. A "1" indicates a 1/64" radius. CNMG's are available with corner radii down to 1/64", but most inserts below 1/64" must be ground, so can only be made in a CNGG or CNGP style. It isn't a hard and fast rule, but it is generally recommended that the tip corner radius is the minimum depth of cut for that insert, in order to ensure that the radius is full engaged in the work. Applying this rule, the minimum DOC for a CNMG432 would be .031". Where I generally don't cut more than .040" DOC due to horsepower limitation, a CNMG431 is a much better choice for me. I won't explain the holder nomenclature here, but for manual turning (and facing) TOWARD the chuck, the proper insert holder for a CNMG or CNGP or CNGG431 is MCLNR12-4 (for 3/4" shank tooling) or MCLNR16-4 (for 1" shank tooling). These holders hold the insert at a 9 degree negative angle toward the work piece, thus giving a 9 degree front relief angle.
- Chipformers
Ahhh - the blessings of chipformers! To be able to make little chips in the shapes of "6"s and "9"s instead of a rats nest of entangled razors! But keep in mind that if you are machining at low feeds and depths of cut, or a tenacious material like some aluminums or stainlesses, it may still be a challenge to break the chips. Subtle differences in chipformer shape can make a big difference, and proper chipformer selection was often the hardest part of selecting the right insert for a customer. Chipformers also can give you a POSITIVE cutting edge at the material even when the insert itself is held at a negative angle by the MCLNR holder. Chipformers are not standardized between manufacturers like the insert sizes and shapes are, so every manufacturer has their own nomenclature. For the depths of cut that I use, I need a chipformer designed for finishing or super-finishing, even when I consider .040" DOC to be roughing. And even the super-finishing chipformers aren't expected to control the chips at DOC below .020". Chipformers usually have a two letter designation, and it is common for finishing chipformers to include the letter "F". I prefer to use what are known in the industry as "high positive" chipformers. For DOC below about .005-.010", I sometimes use a ground insert like a CNGG or CNGP with a finishing chipformer like Mitsubishi's "FJ" (with a positive top rake that varies from +12 to +20 degrees). When held in a 9 degree negative holder, a 20 degree positive top rake will enter the work with an 11 degree positive angle. Since these inserts have an "up-sharp" edge, they may chip if used too aggressively in interrupted cuts. They are not recommended for heavy cuts in steel, but they have worked well for me at very light passes in steel, and everything I do in aluminum. Since these inserts are commonly used for high temperature alloys like titanium, the grade choices are limited to the higher hardness end of the spectrum, but tend to be PVD coated or uncoated. I pick the toughest grade available. These are designed to work at about .002" to .010" feed, and .004"-.050" DOC. I use inserts similar to this for about 85% of my turning. If I want to feel more secure about not chipping the insert, Ill use an "as molded" insert. Examples are the Mitsubishi CNMG 431-MJ (+12 to 20 degrees), and the Iscar CNMG 431-PP (+13 degrees). The honed edges can handle steels very well, and can even handle moderate interrupted cuts. These are available in more grades than the CNGP or CNGG, and once again I'll select the toughest PVD or uncoated grade.
To summarize the key words, I mostly use the toughest uncoated or PVD coated grade available in an insert with a high positive finishing chipformer and an up-sharp grind.
Bob G
I agree that most tungsten carbide inserts are not suitable for small lathes. But some of them are. I'd like to contribute some of my experience to those who DO want to use tungsten carbide inserts on small lathes. They have become an integral tool in my workshop, but they are not right for everybody or for every situation. Allow me to share what I have learned, and what works for me. I think that too a large degree people have bad experiences using tungsten carbide on small manual machines because they did not know how to select the inserts with correct features. And, unfortunately for the hobbyist, economy carbide is generally not available with the right features. If you are happy with HSS, don't waste your time reading any further, for changing to carbide would be a waste of money for you. Personally, changing to carbide made my hobby a lot more fun and productive. Your mileage will vary. Being a jack-of-all-trades kind of guy, I'm not an expert in any one field, and can only claim amateur abilities in my home shop. Almost my entire career involved some aspect of using tungsten carbide. I began my career with 11 years as a product evaluation engineer for a major manufacturer of oil field rock drilling bits using tungsten carbide teeth, and finished it with 11 years as a tungsten carbide tooling sales rep for Iscar, Valenite, and Mitsubishi Carbide. I sold tungsten carbide inserts to manufacturers and machine shops in Washington, Oregon, Idaho, Montana, Wyoming, Colorado, and Utah. The most common materials used in these states are steel, stainless, aluminum and high temperature alloys, so I have very little experience with cast iron. This was the great job for a home shop machinist, for many days I couldn't tell when the hobby stopped and the work began. I always took a problem solving, applications approach to my customers, and most of them appreciated that I machined for a hobby. When I faced particularly difficult or unfamiliar materials, I commonly took scrap samples home to learn how to machine it on my own lathe. I couldn't duplicate what their CNC machines could do, and I do all of my machining dry, but what I learned with my 1.5 HP lathe could often be scaled up to their 20 HP machines. I retired about 4 years ago. I have no ties with, and receive no retirement benefits from any of my former employers.
First, my experience with HSS. My exposure to sharpening and using HSS bits is far from professional level. My grandfather was a tool room machinist, and I have inherited hundreds of HSS bit that he had ground to a wide assortment of configurations. My dad taught me to run a lathe and to sharpen HSS bits. And, believe it or not, sharpening and using HSS bits was a requirement for my BS Mechanical Engineering degree at Cal Poly, San Luis Obispo, CA, whose motto is "Learn by Doing". However, since I've learned to use tungsten carbide inserts, my enjoyment level has soared while my frustration level has dropped. I now use HSS for less than 5% of my lathe work. Chip control is much better. Surface finishes are much improved. Dimensions are more predictable. I don't have to use coolant no matter what SFM I choose to run. And I no longer wrestle when I pick up a piece of material of unknown alloy. I primarily machine steel, stainless, aluminum, brass, wood and plastic, but I've successfully machined on my lathe the toughest materials that my customers encountered: spin-cast stainlesses, titanium, nitronic, inconel, hastelloy. Indexable carbide inserts have become my first choice for turning, facing, boring, grooving, threading and partoff in all of these materials - even plastic.
Some thoughts on using tungsten carbide in a home shop- (I refer to the products of Iscar, Valenite, and Mitsubishi due to my familiarity with them - most of the other major manufacturers offer comparable products. Ask them for details.)
- Lathe Horsepower, Drive, and Rigidity
If you have less than 1 HP, your machine is probably too small to use the same inserts tha I do. You'd probably be better off with HSS, or positive, single-sided insert holders. I agree with most of what is said in the website http://www.thegallos.com/carbide.htm. But I prefer not to use the TiN coatings or utility grade inserts on a small lathe because they don't have what I feel is a sharp enough edge. I have a Taiwanese 12" gear-driven Birmingham lathe that I inherited from my dad. It replaced an old belt-driven 12" Logan. I couldn't recommend carbide tooling for the Logan since it was worn and sloppy, and I don't think the belt would have transmitted the required power for partoff. The Taiwanese lathe came with a motor rating of 1.5 HP, but the starting windings burned out one day as I made repeated partoffs with a carbide insert partoff tool (see more below). The replacement US-made motor also has a rating of 1.5 HP, but appears to have much more power than the original, so my experiences are based upon this new motor, and this is probably a good lower horsepower limit to my recommendations here. I commonly limit my maximum DOC to .040", but if I recall correctly, I've pushed it to .070" DOC in steel without a problem. Carbide doesn't like flexible setups, or chatter, so if your machine is old and loose, you might as well stop reading this. And, as a rule of thumb, if your manual lathe is too small to hold at least 3/4" shank tooling, stick with HSS or single-sided inserts. The sharp carbide I'm recommending doesn't tolerate chatter, heavy interrupted cuts, or the unfortunate goof.
- Brazed Carbide
My comments here relate to indexable tungsten carbide inserts. Brazed tungsten carbide stick tools have their place, but they don't have any place in my shop. Inserts offer repeatablity, accurate indexability, positive geometries, chip control, coating options, accurate corner radii, no grinding, and they are not subjected to the heat from brazing - features I've never enjoyed from brazed carbide. If you want to use brazed carbide, maybe someone else here can give some pointers. I threw all of mine away years ago.
- Costs
I use 3/4" and 1" shank OD turning tools. A holder will cost about $80 to $100. The insert styles I prefer cost about $14 to $18 apiece when bought in boxes of ten. Most distributors don't sell partial boxes of inserts, but some do, so ask. MSC sells single inserts at a higher individual cost. You'll have to evaluate for yourself if you can justify the expense. In my case, I feel that if can't afford the inserts, I can't afford the hobby. I'd avoid the no-name carbide sold by the lower echelon suppliers. This is sometimes made from re-ground used carbide, unpredictable, and unlikely to come with the top-face geometries and sharp cutting edges that a small lathe needs.
- Carbide Grades
Wow - how to summarize such a broad topic in few words. In general terms, carbide grades are a compromise between toughness and heat/wear resistance. Most inserts are optimized for use in high production CNC environments, where cost savings are often found in higher feeds and speeds, which result in higher temperature. Like most materials, tungsten carbide is sensitive to high temperatures, so most industry research is in the direction of increasing heat resistance. That's not a factor for most hobbyists. When my face is 18 inches or less from a spinning chuck, I tend to keep the feeds and speeds down. I'm looking for toughness in an insert because my manual lathe doesn't have the rigidity of a CNC, and my boneheaded handle-cranking is by no means repeatable, or predictable. I prefer to have an insert wear rather than chip. The demands of industry have lead to grades specific to certain materials, but where I may be turning steel, stainless and brass all on the same day, or same hour, I want a general purpose grade. A C2 grade is a good compromise for most metals, or a C5 if you turn mostly steels. Coatings help
primarily by protecting the inserts from the heat of cutting, but it is a little talked about fact that the act of applying the coatings in hot furnaces degrades the toughness of the base carbide. Some recent advances in carbide technology have focused on minimizing that effect. In many cases the home shop machinist would be better off with an uncoated insert in order to optimize toughness and edge sharpness, and you also save a couple of bucks per insert. I'd change to a coated grade if I were experiencing built-up edge (where the material adheres to the insert), or if I did a lot of stainless steel. If I were to suggest a coating for general home use, it would be one that uses a PVD, rather than a CVD, process, due to the lower coating furnace temperatures, and the typically thinner, more lubricious coatings. The PVD process can also coat up to a sharp edge, where the CVD process requires a rounded honed edge. My favorite coating materials are TiCN (titanium carbo-nitride), and TiAlN (titanium aluminum nitride). Counter-intuitively, TiAlN is a wonderfully temperature resistant coating initially designed for use without coolant, but it also offers a high lubricity factor, which helps prevent built-up edge. To the best of my knowledge, the toughest coated insert in the industry is Iscar's IC3028 (IC328 for milling and partoff). I can't verify it, but I have been told that it's toughness, measured in Transverse Rupture Strength, while not equal to HSS, is at least in the ballpark with HSS. This has a PVD TiCN coating. The TiAlN coating version is called IC9028. The uncoated version of this is IC28 grade. This is classified as a non-ferrous grade, and is not optimized for steel but will work in steel, too. All major manufacturers offer something competitive with this, and what they have on their conversion chart that's equivalent to Iscar's grades are what you want. ( Grade numbers are added and deleted constantly. I left Iscar 10 years ago, so specifics may have changed since then, but IC 28/IC328/IC3028 have been been benchmark grades for them.) Unfortunately, the toughest grades generally aren't available with the chipformers designed for light depths of cut. Even though I call it roughing on MY lathe, .040" DOC is generally considered a finishing application, so these inserts tend to come with wear resistant grades to handle the higher SFM's commonly used in industry. So when I choose a finishing chipformer, I have to compromise and select the toughest grade available in that configuration.
- Insert Shape
The most commonly used insert shape and size is the double-sided 80 degree diamond, such as the CNMG432. With its 80 degree included angle, it can cut up to a 90 shoulder. Its popularity ensures that it is available in the most configurations and grades that are of interest to me, and at the most competitive costs. EVERYBODY makes CNMG's. There is valid ground to argue for a narrower angle, like a DNMG-style, if needed, but these will cost more, and offer fewer choices. I use a VNMG-style insert for profiling and reaching into tight corners. There is also a very valid argument for using single-sided "positive" inserts. They are freer cutting, and if you need the freest cut, they are the way to go. But the cost per edge is higher than a double-sided insert with the same features, and there are fewer options available if you need to address a specific application problem in the future. I can't remember any instance where the "up-sharp" double-sided "negative" inserts didn't provide a free enough cut for me, but cutting a long, slender shaft might be more of a challenge. Since I'm an amateur and more likely to chip an insert than wear it away, the double-sided, four-cornered CNMG-style is my choice if I could only have one. The third letter of the ANSI/ISO nomenclature (M in this case) denotes the tolerance class. The two
most common options are "M" and "G". It helps a home shop machinist to equate the "M" with "as molded", and the "G" with "as ground". As an insert comes out of its molding process, the cutting edge has a "hone" of .005" or more. This is well illustrated in Mitsubishi's product bulletin #B036A.
http://www.mitsubishicarbide.com/mmus/catalog/pdf/b/b036a_200710.pdf
Zoom in on the photos on page 2 where they distinguish between the "M class" and "G class" inserts. This edge hone is advantageous in most applications in order to keep the cutting edge from chipping. To get an "up-sharp" edge or tighter tolerance, the insert must be peripherally ground. Most manufacturers call these CNGG's or CNGP's. This adds several dollars to the cost of each insert, but this is a necessity for most aluminums, titanium, plastics, or wood. I use up-sharp inserts for taking depths-of-cut from .0005 to .040, even in steel. But when I recently turned cast iron for the MLA Diesel, I changed to an insert with an edge hone. For aluminum and plastic, I prefer (but seldom use) inserts that are both ground and polished. The top faces of these are polished to practically a mirror finish, which greatly helps to prevent builtup edge from forming. They are quite pricey, and are hard to justify for the small quantities I produce. When dragged by hand across the top of your thumbnail, a proper CNGG or CNGP will easily shave off some thumbnail material. A CNMG will not I save those for cast iron or heavy hogging in steel. The third digit designates the cutting tip corner radius. For a CNMG432, this is the "2", indicating a 1/32" radius. A "1" indicates a 1/64" radius. CNMG's are available with corner radii down to 1/64", but most inserts below 1/64" must be ground, so can only be made in a CNGG or CNGP style. It isn't a hard and fast rule, but it is generally recommended that the tip corner radius is the minimum depth of cut for that insert, in order to ensure that the radius is full engaged in the work. Applying this rule, the minimum DOC for a CNMG432 would be .031". Where I generally don't cut more than .040" DOC due to horsepower limitation, a CNMG431 is a much better choice for me. I won't explain the holder nomenclature here, but for manual turning (and facing) TOWARD the chuck, the proper insert holder for a CNMG or CNGP or CNGG431 is MCLNR12-4 (for 3/4" shank tooling) or MCLNR16-4 (for 1" shank tooling). These holders hold the insert at a 9 degree negative angle toward the work piece, thus giving a 9 degree front relief angle.
- Chipformers
Ahhh - the blessings of chipformers! To be able to make little chips in the shapes of "6"s and "9"s instead of a rats nest of entangled razors! But keep in mind that if you are machining at low feeds and depths of cut, or a tenacious material like some aluminums or stainlesses, it may still be a challenge to break the chips. Subtle differences in chipformer shape can make a big difference, and proper chipformer selection was often the hardest part of selecting the right insert for a customer. Chipformers also can give you a POSITIVE cutting edge at the material even when the insert itself is held at a negative angle by the MCLNR holder. Chipformers are not standardized between manufacturers like the insert sizes and shapes are, so every manufacturer has their own nomenclature. For the depths of cut that I use, I need a chipformer designed for finishing or super-finishing, even when I consider .040" DOC to be roughing. And even the super-finishing chipformers aren't expected to control the chips at DOC below .020". Chipformers usually have a two letter designation, and it is common for finishing chipformers to include the letter "F". I prefer to use what are known in the industry as "high positive" chipformers. For DOC below about .005-.010", I sometimes use a ground insert like a CNGG or CNGP with a finishing chipformer like Mitsubishi's "FJ" (with a positive top rake that varies from +12 to +20 degrees). When held in a 9 degree negative holder, a 20 degree positive top rake will enter the work with an 11 degree positive angle. Since these inserts have an "up-sharp" edge, they may chip if used too aggressively in interrupted cuts. They are not recommended for heavy cuts in steel, but they have worked well for me at very light passes in steel, and everything I do in aluminum. Since these inserts are commonly used for high temperature alloys like titanium, the grade choices are limited to the higher hardness end of the spectrum, but tend to be PVD coated or uncoated. I pick the toughest grade available. These are designed to work at about .002" to .010" feed, and .004"-.050" DOC. I use inserts similar to this for about 85% of my turning. If I want to feel more secure about not chipping the insert, Ill use an "as molded" insert. Examples are the Mitsubishi CNMG 431-MJ (+12 to 20 degrees), and the Iscar CNMG 431-PP (+13 degrees). The honed edges can handle steels very well, and can even handle moderate interrupted cuts. These are available in more grades than the CNGP or CNGG, and once again I'll select the toughest PVD or uncoated grade.
To summarize the key words, I mostly use the toughest uncoated or PVD coated grade available in an insert with a high positive finishing chipformer and an up-sharp grind.
Bob G
