- Joined
- Oct 28, 2009
- Messages
- 58
- Reaction score
- 42
My Thoughts on Selecting and Using Tungsten Carbide Partoff Tooling
I hope the following doesnt sound like an ad for Iscar, but it is their tooling that I know the best. I wrote it several years ago to answer a specific question, and thought it would be of benefit to this group. I want to preface my remarks by saying that I worked as a technical sales rep for Iscar from 1995 to 2001, but I no longer have ties with the company or any other. Following Iscar, I worked in the same capacities for Valenite and Mitsubishi, and I retired in 2006, so some of my knowledge about Iscar products is 10 years old now. Most of my job was spent doing technical troubleshooting on both CNC and manual machines. Partoff and grooving accounted for about 40% of my business. My personal machining has always been strictly a hobby.
Here's a little historical background of Iscar's partoff line, as best I know it, while ignoring their extensive Cut-Grip groove/turn line of tools. Iscar was just a small company until they developed and introduced the tungsten carbide partoff insert. Then the machining world changed. The first generation was the GTN style. Despite the fact that this tool design was a major improvement in partoff technology, there was room for improvement, and Iscar chose not to spend any effort defending their patent. A lot of these are still used today, and there are a number of imitators who make inserts that will fit the Iscar blades. The insert/blade interface of the GTN is a simple wedge shape. Unfortunately, the insert can move deeper into the blade's pocket under heavy cyclical loads. I have seen close-up movies graphically illustrating this. Personally, I avoid this design. The second generation was the GFN, the "F" designating a fixed stop that prevents insert movement. The third generation was the Do-Grip (pronounced dew-grip). The advantage here was that the insert was double ended, giving greater economy per cutting edge. The real innovation was their ability to mold these inserts so that the two cutting edges were twisted in relation to each other. While the edge that is in use is horizontal to the groove it is cutting, the second edge is tilted so that it does not rub along the walls of the groove. This allows the insert to cut a groove deeper than the insert's length, a limiting factor for double ended inserts that aren't twisted. (This was not possible in the thinner insert widths when the Do-Grip was introduced - check their catalog for current information.) The insert and its pocket in the steel blade both have a generally rectangular profile. The clamping finger of the blade is lifted by a wrench with a camming action. The next generation evolved into a partoff/grooving/turning tool, the Heli-Grip, which is a high productivity tool for CNC machines. It can be used on a manual machine, but not to optimum effectiveness. In the larger insert sizes, the Do-Grip and Heli-Grip inserts and blades are interchangeable, but not in the narrower sizes that can be used on our lathes. I believe that the home machinist should stick to the 2 or 3mm wide inserts. The key point about the Do-Grip/Heli-Grip insert retention system is that, even without screw-down clamping, the insert is held well enough to permit aggressive lateral turning and the resulting significant side loads. The necessary tool movements for successful grooving and turning with the same insert can be programmed into a CNC machine, but only roughly approximated on a manual machine. One disadvantage to the double-ended inserts is that if the insert cracks when using the first edge, the second edge is usually unusable. But, in that case that end of the blade is usually scrapped, too. I use both the GFN and Do-Grip/Heli-Grip styles. You can find similar tools from competitors.
While I love using tungsten carbide inserts for turning, boring, and facing on my lathe, and eagerly threw away all of my HSS partoff blades once I learned how to use partoff inserts, I have some hesitation making a broad recommendation for other hobbyists using manual lathes. The initial investment of blade, blade holder, and box of inserts is at least $300. Using a square shank tool, rather than blade style, offers initially lower entry price, but they are only single sided and don't offer the ability to shorten the amount of blade extension. And crashes WILL occur. I'm still nervous when I do it. I've crashed 2 blades within the past year. Partoff can make for an expensive hobby. Let me share some things I've learned with those who have chosen to use carbide. If HSS partoff blades work well for you, stick with it - it is a cheaper solution for the hobbyist. Pardon me for using Iscar's nomenclature - it's what I know the best. Other companies make good partoff tooling, also, but I think Iscar has taken it to a fine art, with some options that no one else offers. I also like Sandvik's tools.
One of the biggest challenges in the partoff operation stems from the fact that the tool is nearly as wide as the groove it cuts, making chip removal and coolant entry major problems. The cutting geometry of the insert is the key to forming the chips into a shape which is narrower than the groove. When conditions are right, these chips wind up into a watch-spring shape (when cutting ductile metals) that rides upon the top of the blade, partially in the partoff groove. When they get to be approximately the size of a quarter, they break off, and the next one forms. Except for short-chipping metals like cast iron, any other chip shape is less than optimum. The formation of "pig's tails", "rat's nest's", "6's and 9's", etc, all increase the chance of catching in the groove and leading to a crash.
I have a Birmingham 12x36. When I first started working with Iscar, I spent hours at night and weekends testing their partoff tools at different feeds and speeds, comparing the types of chips that formed. Unfortunately, the original 1.5 HP motor on this lathe wasn't up to this task. I suspect that I was lugging the motor down to a speed where the starting windings were engaging, for the starting contacts burned out. The next thing I saw was smoke curling around my legs. I replaced this motor with an American made 1.5 HP motor, which seems to have significantly more torque and has performed flawlessly. If you hear clicking sounds from your motor when parting off, it may be your starting contacts engaging. This has led me to think that 3mm (.118") is the widest practical partoff insert for a 12x36. A 2 mm or 2.2mm wide insert would have advantages with this respect. Since 3mm is the most commonly used width in industry and therefore offers the widest range of grades/chipformers/lead angles, I began to use it primarily to help me troubleshoot my customers' more challenging partoff problems.
Even on an enclosed CNC machine with a good coolant pump, it is difficult to get proper and consistent coolant flow to a partoff insert because it is buried deep within the groove. If the flow is intermittent due to obstruction by the chips, the thermal shock caused by suddenly quenching a hot insert can cause the insert to crack. Iscar addressed this my supplying blades with coolant ports beneath the insert, shooting coolant directly where the insert contacts the material. This greatly improves insert life, but I would guess that less than 10% of partoff applications use it. I choose to run my partoff tool dry, for I find this the least objectionable compromise. If you successfully use coolant, keep doing so. Since I use tungsten carbide turning inserts, I seldom use coolant except for hand applied cutting fluids for drilling and threading, and sometimes grooving aluminum. Since the partoff operation happens so quickly, I don't have enough time nor enough hands to hand apply cutting fluid and control the lathe, too. And if my lathe slings any more fluids on my wife's car, my lathe and I will both be sleeping under the stars.
Partoff requires an extremely rigid setup. Always partoff as close to the chuck as physically possible. If I can't partoff within about an inch of the chuck or collet, I'll use the bandsaw. Iscar recommends that the cutting edge of the insert be .003" above the centerline of the lathe. This allows for a slight downward flex in the setup, for if the insert goes below centerline, the workpiece tends to want to ride up over the insert, which can cause a sudden, catastrophic crash. You can try to measure this with a dial indicator and jig, but due to the complex insert geometry at the cutting lip, I think I am safe to challenge anyone to prove that they can do this accurately. Theoretically, the top of the toolblock should be at centerline of the lathe, but I never got a satisfactory answer from Iscar as to whether the insert cutting lip is made to be at the same height as the top of the toolblock, or .003" above it. (Perhaps I am being overly precise about my uncertainty.) Be sure to lock the carriage clamp. I prefer to use a partoff blade with a clamping style block so I can keep the blades' overhang to the bare minimum. Using a big block of brass, I've mounted the partoff tools on the back side of my cross-slide, but in the upright position rather than inverted. So by just reversing the spindle direction, the tool is always readily available. I use an Iscar SGTBK 32-9 block to hold a 1.25" tall blade. I may someday modify this block with an additional groove on the other side to allow the partoff blade to be held upside down, allowing the chips to fall out easier.
Using an insert with a right or left cutting angle, one can reduce, but seldom eliminate, the diameter of the nub that remains on the part, but these cutting angles also force the chip into a coil-spring shape rather than a watch-spring shape.
You want a tough carbide grade on a manual machine, and Iscars IC328 is probably the toughest available throughout the industry. I'd much rather have an insert wear than chip - once it chips, the insert, the blade, and maybe the workpiece, are history. Except for high temperature and aerospace alloys, Iscar recommends something near 300 SFM for many materials (I don't have their current reference material at hand). But this is assuming a CNC machine with plenty of well-directed coolant. What RPM should you use on a manual machine, without coolant? Everyone is going to have a different opinion. With a 1" diameter workpiece, 300 SFM equates to 1150 RPM. And theoretically, the RPM should increase as the tool approaches the centerline. Most modern CNC lathes are capable of increasing RPM to maintain a constant SFM while parting off, up to their RPM limit. My manual lathe will stay at the originally selected RPM, so the actual SFM drops very quickly to zero as the tool approaches centerline. Iscar product managers have explained to me that using slower SFM actually puts increasingly higher loads upon the tool. This is just one more reason that partoff tools tend to crash when they have almost completed the cut. I don't know about you, but I'm too chicken to engage the crossfeed lever at 900 RPM (my closest to 1150 RPM) when my face is just 18 inches away from it. I often use 600 RPM, which in itself took a great leap of faith when I first learned to do this, being about 10 times faster, if I remember correctly, than I used with HSS partoff blades. At 600 RPM and .003" feed rate, a 1" diameter bar parts off in 17 seconds. I am curious to see what RPM other people use with their carbide partoff inserts.
I use two different chipformers for partoff - the "C" and the "J". Generally, the "J" forms a watch-spring shaped chip at a feed rate of .0015" to .003" per revolution. It has a positive top face geometry for a freer cut and lower feed rates, but is not as strong as a "C" chipformer. The "C" has a narrow lip with negative geometry before the chip flows into a positive cavity on the top face. This makes for a tougher insert, and more commonly used in industry, but requires a higher cutting force. It will generally form a watch-spring chip between .003" and .006" per rev. In most cases the "J" is better suited for our machines, but I have had instances where the "J" chattered, but the "C" did not. Thus, I have both. These inserts can be hand fed, but I prefer to use the cross-feed. Then I can precisely control the feed rate and adjust it if the chip shape is incorrect. But if you are only parting off one piece, this benefit loses its value. When I was commonly troubleshooting partoff problems over the phone, it was hard to tell if someone was hand-feeding to fast or too slow, but a power cross-feed eliminated that unknown factor.
This is all I can think of at the moment. I hope it helps some of you to decide if tungsten carbide tooling is right for you.
Bob G
I hope the following doesnt sound like an ad for Iscar, but it is their tooling that I know the best. I wrote it several years ago to answer a specific question, and thought it would be of benefit to this group. I want to preface my remarks by saying that I worked as a technical sales rep for Iscar from 1995 to 2001, but I no longer have ties with the company or any other. Following Iscar, I worked in the same capacities for Valenite and Mitsubishi, and I retired in 2006, so some of my knowledge about Iscar products is 10 years old now. Most of my job was spent doing technical troubleshooting on both CNC and manual machines. Partoff and grooving accounted for about 40% of my business. My personal machining has always been strictly a hobby.
Here's a little historical background of Iscar's partoff line, as best I know it, while ignoring their extensive Cut-Grip groove/turn line of tools. Iscar was just a small company until they developed and introduced the tungsten carbide partoff insert. Then the machining world changed. The first generation was the GTN style. Despite the fact that this tool design was a major improvement in partoff technology, there was room for improvement, and Iscar chose not to spend any effort defending their patent. A lot of these are still used today, and there are a number of imitators who make inserts that will fit the Iscar blades. The insert/blade interface of the GTN is a simple wedge shape. Unfortunately, the insert can move deeper into the blade's pocket under heavy cyclical loads. I have seen close-up movies graphically illustrating this. Personally, I avoid this design. The second generation was the GFN, the "F" designating a fixed stop that prevents insert movement. The third generation was the Do-Grip (pronounced dew-grip). The advantage here was that the insert was double ended, giving greater economy per cutting edge. The real innovation was their ability to mold these inserts so that the two cutting edges were twisted in relation to each other. While the edge that is in use is horizontal to the groove it is cutting, the second edge is tilted so that it does not rub along the walls of the groove. This allows the insert to cut a groove deeper than the insert's length, a limiting factor for double ended inserts that aren't twisted. (This was not possible in the thinner insert widths when the Do-Grip was introduced - check their catalog for current information.) The insert and its pocket in the steel blade both have a generally rectangular profile. The clamping finger of the blade is lifted by a wrench with a camming action. The next generation evolved into a partoff/grooving/turning tool, the Heli-Grip, which is a high productivity tool for CNC machines. It can be used on a manual machine, but not to optimum effectiveness. In the larger insert sizes, the Do-Grip and Heli-Grip inserts and blades are interchangeable, but not in the narrower sizes that can be used on our lathes. I believe that the home machinist should stick to the 2 or 3mm wide inserts. The key point about the Do-Grip/Heli-Grip insert retention system is that, even without screw-down clamping, the insert is held well enough to permit aggressive lateral turning and the resulting significant side loads. The necessary tool movements for successful grooving and turning with the same insert can be programmed into a CNC machine, but only roughly approximated on a manual machine. One disadvantage to the double-ended inserts is that if the insert cracks when using the first edge, the second edge is usually unusable. But, in that case that end of the blade is usually scrapped, too. I use both the GFN and Do-Grip/Heli-Grip styles. You can find similar tools from competitors.
While I love using tungsten carbide inserts for turning, boring, and facing on my lathe, and eagerly threw away all of my HSS partoff blades once I learned how to use partoff inserts, I have some hesitation making a broad recommendation for other hobbyists using manual lathes. The initial investment of blade, blade holder, and box of inserts is at least $300. Using a square shank tool, rather than blade style, offers initially lower entry price, but they are only single sided and don't offer the ability to shorten the amount of blade extension. And crashes WILL occur. I'm still nervous when I do it. I've crashed 2 blades within the past year. Partoff can make for an expensive hobby. Let me share some things I've learned with those who have chosen to use carbide. If HSS partoff blades work well for you, stick with it - it is a cheaper solution for the hobbyist. Pardon me for using Iscar's nomenclature - it's what I know the best. Other companies make good partoff tooling, also, but I think Iscar has taken it to a fine art, with some options that no one else offers. I also like Sandvik's tools.
One of the biggest challenges in the partoff operation stems from the fact that the tool is nearly as wide as the groove it cuts, making chip removal and coolant entry major problems. The cutting geometry of the insert is the key to forming the chips into a shape which is narrower than the groove. When conditions are right, these chips wind up into a watch-spring shape (when cutting ductile metals) that rides upon the top of the blade, partially in the partoff groove. When they get to be approximately the size of a quarter, they break off, and the next one forms. Except for short-chipping metals like cast iron, any other chip shape is less than optimum. The formation of "pig's tails", "rat's nest's", "6's and 9's", etc, all increase the chance of catching in the groove and leading to a crash.
I have a Birmingham 12x36. When I first started working with Iscar, I spent hours at night and weekends testing their partoff tools at different feeds and speeds, comparing the types of chips that formed. Unfortunately, the original 1.5 HP motor on this lathe wasn't up to this task. I suspect that I was lugging the motor down to a speed where the starting windings were engaging, for the starting contacts burned out. The next thing I saw was smoke curling around my legs. I replaced this motor with an American made 1.5 HP motor, which seems to have significantly more torque and has performed flawlessly. If you hear clicking sounds from your motor when parting off, it may be your starting contacts engaging. This has led me to think that 3mm (.118") is the widest practical partoff insert for a 12x36. A 2 mm or 2.2mm wide insert would have advantages with this respect. Since 3mm is the most commonly used width in industry and therefore offers the widest range of grades/chipformers/lead angles, I began to use it primarily to help me troubleshoot my customers' more challenging partoff problems.
Even on an enclosed CNC machine with a good coolant pump, it is difficult to get proper and consistent coolant flow to a partoff insert because it is buried deep within the groove. If the flow is intermittent due to obstruction by the chips, the thermal shock caused by suddenly quenching a hot insert can cause the insert to crack. Iscar addressed this my supplying blades with coolant ports beneath the insert, shooting coolant directly where the insert contacts the material. This greatly improves insert life, but I would guess that less than 10% of partoff applications use it. I choose to run my partoff tool dry, for I find this the least objectionable compromise. If you successfully use coolant, keep doing so. Since I use tungsten carbide turning inserts, I seldom use coolant except for hand applied cutting fluids for drilling and threading, and sometimes grooving aluminum. Since the partoff operation happens so quickly, I don't have enough time nor enough hands to hand apply cutting fluid and control the lathe, too. And if my lathe slings any more fluids on my wife's car, my lathe and I will both be sleeping under the stars.
Partoff requires an extremely rigid setup. Always partoff as close to the chuck as physically possible. If I can't partoff within about an inch of the chuck or collet, I'll use the bandsaw. Iscar recommends that the cutting edge of the insert be .003" above the centerline of the lathe. This allows for a slight downward flex in the setup, for if the insert goes below centerline, the workpiece tends to want to ride up over the insert, which can cause a sudden, catastrophic crash. You can try to measure this with a dial indicator and jig, but due to the complex insert geometry at the cutting lip, I think I am safe to challenge anyone to prove that they can do this accurately. Theoretically, the top of the toolblock should be at centerline of the lathe, but I never got a satisfactory answer from Iscar as to whether the insert cutting lip is made to be at the same height as the top of the toolblock, or .003" above it. (Perhaps I am being overly precise about my uncertainty.) Be sure to lock the carriage clamp. I prefer to use a partoff blade with a clamping style block so I can keep the blades' overhang to the bare minimum. Using a big block of brass, I've mounted the partoff tools on the back side of my cross-slide, but in the upright position rather than inverted. So by just reversing the spindle direction, the tool is always readily available. I use an Iscar SGTBK 32-9 block to hold a 1.25" tall blade. I may someday modify this block with an additional groove on the other side to allow the partoff blade to be held upside down, allowing the chips to fall out easier.
Using an insert with a right or left cutting angle, one can reduce, but seldom eliminate, the diameter of the nub that remains on the part, but these cutting angles also force the chip into a coil-spring shape rather than a watch-spring shape.
You want a tough carbide grade on a manual machine, and Iscars IC328 is probably the toughest available throughout the industry. I'd much rather have an insert wear than chip - once it chips, the insert, the blade, and maybe the workpiece, are history. Except for high temperature and aerospace alloys, Iscar recommends something near 300 SFM for many materials (I don't have their current reference material at hand). But this is assuming a CNC machine with plenty of well-directed coolant. What RPM should you use on a manual machine, without coolant? Everyone is going to have a different opinion. With a 1" diameter workpiece, 300 SFM equates to 1150 RPM. And theoretically, the RPM should increase as the tool approaches the centerline. Most modern CNC lathes are capable of increasing RPM to maintain a constant SFM while parting off, up to their RPM limit. My manual lathe will stay at the originally selected RPM, so the actual SFM drops very quickly to zero as the tool approaches centerline. Iscar product managers have explained to me that using slower SFM actually puts increasingly higher loads upon the tool. This is just one more reason that partoff tools tend to crash when they have almost completed the cut. I don't know about you, but I'm too chicken to engage the crossfeed lever at 900 RPM (my closest to 1150 RPM) when my face is just 18 inches away from it. I often use 600 RPM, which in itself took a great leap of faith when I first learned to do this, being about 10 times faster, if I remember correctly, than I used with HSS partoff blades. At 600 RPM and .003" feed rate, a 1" diameter bar parts off in 17 seconds. I am curious to see what RPM other people use with their carbide partoff inserts.
I use two different chipformers for partoff - the "C" and the "J". Generally, the "J" forms a watch-spring shaped chip at a feed rate of .0015" to .003" per revolution. It has a positive top face geometry for a freer cut and lower feed rates, but is not as strong as a "C" chipformer. The "C" has a narrow lip with negative geometry before the chip flows into a positive cavity on the top face. This makes for a tougher insert, and more commonly used in industry, but requires a higher cutting force. It will generally form a watch-spring chip between .003" and .006" per rev. In most cases the "J" is better suited for our machines, but I have had instances where the "J" chattered, but the "C" did not. Thus, I have both. These inserts can be hand fed, but I prefer to use the cross-feed. Then I can precisely control the feed rate and adjust it if the chip shape is incorrect. But if you are only parting off one piece, this benefit loses its value. When I was commonly troubleshooting partoff problems over the phone, it was hard to tell if someone was hand-feeding to fast or too slow, but a power cross-feed eliminated that unknown factor.
This is all I can think of at the moment. I hope it helps some of you to decide if tungsten carbide tooling is right for you.
Bob G
![DreamPlan Home Design and Landscaping Software Free for Windows [PC Download]](https://m.media-amazon.com/images/I/51kvZH2dVLL._SL500_.jpg)
