We have a CNC Swiss that we use to turn very small precise parts. When a part has several different diameters I notice that when one diameter is on the nominal dimension, often the others are off nominal by several tenths. Is this due to different tool pressure at the different depth of cuts? Is there a solution?

Tiny Turner

Dear Tiny,

I doubt the issue is from tool pressure. It is more likely that your turning tool center height is off. Old timers will tell you that tool center height is very important in very small turning. I’ll attempt to explain why that is so.

In the following example take a look at how being off center can affect the diameter being turned. First let’s assume that if your tool was brought to X0, the tip would be dead on the centerline of the bar.

Line “a” is how far your tool is off center. Line “b” is your programmed X-axis dimension.  Line “c” is the actual distance to the cutting edge of the tool or ½ the actual turned diameter dimension on your work.

Imagine making Line “b” longer and longer (turning progressively larger diameters) and you’ll see that Angle “A” flattens out, which in turn will make Line “c” shorter relative to Line “b.” In other words the error becomes less the larger the diameter you turn is. So when turning very small diameters it is critical to be on center.

The Pythagorean Theorem tells us that a ²+b ²=c ².  Using that information, let’s assume that your tool is 0.003” off center, and you are turning a 0.030” diameter (side a=0.003”, side “b”=0.015”). Side c therefore is equal to 0.0153” because c=√ (.003 ²+.015 ²), so your turned diameter will be 0.0306” or will be 0.0006” off of nominal size.

Now assume you are using the same tool to turn a 0.125” diameter. Running the same math we find that the turned diameter (rounded) will be 0.1251” or will be 0.0001” off of nominal size.

Since the 0.030” diameter was 0.0006” off of nominal we have a differential of 0.0005” between the two dimensions. It follows that when you offset one dimension to nominal size, the other dimension will be 0.0005” off of nominal. All of which makes it difficult to dial in the workpiece without editing the program (bad), or using two separate offsets (nearly as bad).

You can also add a macro variable to the programmed dimension. But when you think about it, all that does is provide a convenient way for the operator to edit the programmed dimension. It’s better to fix the root cause of the problem by getting the tool on center.

You can use this information to calculate how far your tool is off center and correct it with an offset assuming you have Y-axis capability. Small capacity Tsugami Swiss lathes have a feature built into the control to calculate tool height using this principle. But you can see it works best at very small diameters where Angle A and the resulting error is greater.

There can also be mechanical reasons for disparity between turned diameters. If your tool is on center check for backlash, flex in the machine/tool holder, and of course the fit of the material to the guide bushing.

Question: When you watch the Super Bowl, are you more interested in the game or the commercials?

BOB’S QUESTION:

Our client needs a thin walled brass part. My screw machine is a 1” 6-spindle Wickman. We were concerned about flaking in the threads with brass parts so I knew I had to come up with a cut thread. Our two options were thread milling and thread chasing. We couldn’t get the brass to gauge on our Johnson Gauges because of the flaking. I tried running a drill inside the part while I was thread rolling to avoid crushing of the part but it still didn’t gauge. I tried putting a thread chasing die on the machine and saw that the lead on the threads (or the pitch) was off. We had tracking problems. The thread die is 400 thousandths wide. It wasn’t tracking properly as it ran across the part.

We went through the machine and the chasing attachment looking for the cause of the problem. The attachment had just been rebuilt by a very reputable source. We did see a little play as the cams rode inside the thread chasing attachment. We eliminated the problems in the attachment but our pitch was still off. We are now going to try a thread milling attachment and a thread milling die. How can we eliminate the play in the thread? What caused it? Do you think this will solve the problem on the thin walled part?

Worn parts subject to “slopposis.”

AL’S ANSWER:

On a 1” Wickman, on the center drive shaft where the spindle speed gears are mounted, there is a coupling between the back half of the drive shaft and the front of the drive shaft. As the machines get old, and typically because people run hex material on these machines, they start to pound out the spline on the shaft and the coupling gets loose. This creates looseness or play in the machine, which I call “slopposis.” Toward the spindle end of the machine there is a drive key that engages the main spindle drive gear. That key can get pounded out and you get slopposis at that point. On each spindle there is a drive gear that engages the center drive gear. If the keyway on the spindle is pounded out that is another source of slopposis.

Thread chasing.

When you chase a thread with a single point thread chasing attachment you use a multiple tooth chaser. If for some reason there is play in the machine and the lead does not repeat itself, in other words it doesn’t track in the same place every time, you will get a very sharp crest on the major diameter of the thread. If you look at the thread on a comparator it will show a very sharp crest on the major diameter of the thread and you will notice a wide area at the minor diameter of the thread. What is happening is that the chaser is not following the lead of the thread, and the chaser is shaving the sides of the thread.

You should check the lead on the thread chasing attachment. Usually what I do is mount a dial indicator on the thread chasing head manually (without the machine running). I turn the spindle one complete revolution to advance the thread chasing attachment to the lead of thread. Now lets say it’s supposed to travel .062 per revolution – if you do this three or four times, the lead should be within a tenth or two at the end of it.

The attachments do wear out, but that is probably not the case with yours because your attachment was rebuilt by a reputable source. However often people will put the thread chasing cam on the attachment and forget to put the spacer washers on. This would result in the cam flopping back and forth, which will throw the lead off.

Thread milling for a 1” Wickman.

BOB’S QUESTION:

Do you think using a thread milling attachment and a thread milling die will solve the problem?

AL’S ANSWER:

Thread milling is a completely different system than thread chasing because the lead is built into the tool itself. There is probably less chance for slopposis to affect a thread mill than to affect a thread chaser because the load is constant all the way through the cut. On a single point thread chasing attachment every time that attachment makes a pass the machine is loaded and then unloaded. So thread milling could be the way to go, especially because it’s a thin walled part. The chip load per tooth is much lower with thread milling than with thread chasing.

Al Seniw of New Lenox Machine Co., Inc. in Dwight IL. Al has been working on Wickmans for forty years and he has taught machining courses at community colleges.

Today’s Machining World Archive: June/July 2005 Vol.1, Issue 06

Dear Shop Doc,

We are turning a part made from PEEK (polyetheretherketone plastic) and need an 8 Ra surface finish on the part. We have tried carbide and a PCD insert. We can achieve around a 10 Ra finish but that is about the best we can do. Since it is a medical implant we can’t use coolant or abrasives. What process will enable the required surface finish?

Too rough

Dear Too rough,

You are on the right track using a PCD (polycrystalline diamond) for machining PEEK. The high hardness, abrasion resistance, and heat tolerance of diamond makes it an ideal tool material for machining medical grade PEEK.

However, in order to achieve very low surface finishes in soft materials like PEEK, or even metals like aluminum, you need a tool with a nearly flawless edge. Polycrystalline literally means “many crystals.” A PCD insert has a tip composed of small diamond crystals held together with a metallic binder. The random orientation of the crystals along with the metallic binder (usually containing cobalt) helps give the very hard diamond some toughness to resist fracture.

If you were to look at a micrograph of the cutting edge, you would see the diamond crystals do not provide a continuous, smooth cutting edge. In turning, each little crystal in the matrix will leave its “mark” on the turned surface. The solution is to use a monocrystalline diamond tool, which is a single piece of diamond crystal with a lapped cutting edge.

In addition to the better tool, you will need to address as many of the other variables that affect surface roughness as possible. Ideally your lathe would have a dynamically balanced integral motor spindle with ultra high precision ceramic bearings. The closer the lathe you run it on is to the ideal, the better off you’ll be. Choose the proper feed rate for the nose radius (see sidebar). Keep tool and work overhang to a minimum. Make sure your finish pass depth of cut is at least 60 percent or more of the nose radius.

Formula for Estimating Surface Roughness:
Ra= f²1,000,000/(24 r)
Ra= Surface Roughness in micro-inches
f = Feed rate in inches per revolution
r = Tool nose radius

If you are turning from bar, consider running short lengths of material and be sure to use a spindle liner that closely matches the bar diameter in order to minimize bar whip. Installing a close fitting bushing into the back of the collet can also help damp bar vibration.

Cool the work with a cold gun (vortex tube). Make sure you prevent chips from wrapping around the work. You can rig up a Shop Vac or use a compressed air gun mounted below the cutting area to draw the stringy chips away from the work.

Dan Murphy
REM Sales LLC

Dan Murphy is a regional sales manager for REM Sales LLC., a U.S. Tsugami importer. He can be reached at dmurphy@remsales.com

Dear Shop Doc,

We are trying to make a part of beryllium copper that has a .025″ square pin on one side. The length of the square pin is .140″ long, then transitions to a diameter of .035”, and then to a shoulder at .150” diameter. The problem I am having is that we have to turn the raw material down to .035″ before we polygon mill the .025″ square. We’ve done polygon milling on much larger parts but this is our first time on a small part. We are using a CNC Swiss lathe that has opposing X- and-Y-axis gang plates that are controlled separately.

Poly Gone

Dear Poly,

I know exactly what you are trying to attempt. What you’ll need to do is adjust your methodology to account for the fact that you need to turn the raw material from .250″ diameter to .035″ and polygon mill at the same time. What is happening in your current method is that after you turn the .035″ diameter, the material is no longer supported by the guide bushing. To fix your problem, you need to turn the .035″ diameter at the same time you are polygon milling.

Two actions need to be taken:
1. Tooling: In the Z-axis plane, the turning tool needs to be closer to the material than the polygon tool. The reason for this is to turn the diameter before the polygon tool starts creating the fats. I know in most Swiss machines this is already built into the tool holder geometry where the live tools are typically further away from the guide bushing compared to the turning tools. If this is not the case, then you’ll need to make some physical adjustments so that you can set the tools properly – either by shimming the polygon tool or grinding the shank on the turning tool. Then find the distance between the two tools in the Z-axis plane. As an example we’ll use .010″ as the distance between the two tools.

2. Programming: To program this you’ll need to understand how to utilize tool offsets. For the turning tool, just program it in the normal fashion where you call the tool and the offset. For example: T0101 – Tool 01 and offset 01. For the polygon tool just call up the tool position without the tool offset. For example: T0200 – Tool 02 and no offset. For the G-Code, simply add the distance between the two tools to your programming of the turning tool to get to the linear dimension of the .025″ square.

In your particular component, (using the example of .010″) you’ll want to program your turning tool to .150″ in the Z-axis to account for distance between the turning tool and the polygon tool. This will give you the net result of producing a .025″ square that is .140″ long. If you need to contour the shape of the square, then the programming gets much more complex and you’ll do just the opposite of my example. You’ll have to use the polygon tool offset and omit the turning tool offset, then control the path of the polygon tool in the program. However, you’ll still need to keep the turning tool in front of the polygon tool and account for the difference.

Happy Machining!

David Cogswell
Director, Precision Machining Operations
Bal Seal Engineering,
Medical Products Group

We have often heard the high speed machine spindle is expensive and has to be replaced at some point. Can you shed some light on the high speed spindle construction and service?

Speedster

Dear Speedster,

To understand the cost and justification of a High-Speed-Spindle, let’s look at the more common belt-driven spindle first.  A belt-driven spindle has the motor and spindle mounted separately, linked with a belt-pulley mechanism. With this simple and cost effective system, builders can also install pulley combinations that change ratios on the fly to boost both low end torque and high end rpm. However this time honored design runs into difficulties when rpm continues to push higher. Slipping, vibration, and noise from belt-pulley mechanism eventually become hard to control, so most builders cap belt-driven spindles around 12,000 to15,000 rpm. To answer the market’s demand for higher rpm, the industry’s solution is the Integral-Motor-Spindle (also known as a motorized spindle or built-in spindle).

Integral-Motor-Spindle has all three elements – motor, spindle and tooling – built into one single unit. Its motor winding surrounds the rotary shaft, completely eliminating the mechanical linkage, like belts, pulleys or gears. It can deliver low vibration speed all the way to 100,000 rpm and beyond.  But cramming all these elements into one tight unit makes an Integral-Motor-Spindle a more complex device that carries a higher price tag than that of a belt-driven spindle. Over the years, the Integral-Motor-Spindle has proven itself, becoming the spindle of choice for speed over 12,000 rpm. Practically all main-stream high-speed-spindles are Integral-Motor-Spindles. Due to its clean self-contained modular design, we have seen Integral-Motor-Spindles constantly extending their uses. They show up in some not so high-speed, heavy-duty 50-Taper CNC mills and high-end lathes and offer comparable, if not better, spindle life to that of a belt-driven spindle.

However, when it comes to High-Speed-Spindle life with speed over 20,000 rpm, there are some justified concerns. Our experience shows the spindle life is much more sensitive to how it is used, and the biggest culprit for premature failure is cutting heavier than the High-Speed-Spindle designed for.

High-Speed-Spindle advocates smaller tools with faster and lighter cuts (High-Speed-Machining method) not only because it works for many applications – like surfacing and hard milling – but also because of the spindle limitation. First of all, once spindle bearing DN factor (speed times bore) reaches a limit, increasing max speed (N) requires decreasing bearing ID (D),  which in turn constraints the tool holder size. Typically you will find HSK63 for 24,000 rpm, HSK50 for 36,000 rpm, HSK40 for 42,000 rpm and HSK32 for 60,000 rpm. When tool holder size is reduced, so is overall tooling rigidity. Secondly, motor size is often limited by the housing available for the spindle, and with no belt/gear ratio to amplify the torque, a High-Speed-Spindle can lack low end torque for heavy cutting.  When a programmer enjoys the high speed but is inconsiderate of the rigidity and torque the High-Speed-Spindle has sacrificed, and cuts too heavy from time to time, that would cause a shortened spindle life. That’s why proper programming training with the machine delivery is critical.

Regarding the pricy image of the High-Speed-Spindle, one observation we have is that it has less to do with spindle life and more to do with its crash-resistant ability. The High-Speed-Spindle is compact and complex, and like any device of this nature, it tends to be less forgiving of mistakes. A survivable or low-cost crash for a simple belt-driven spindle might not be the case for a High-Speed-Spindle.

From service point of view, one should not try to fix a High-Speed-Spindle on the field. It’s typically a cartridge design, so switch out entirely and ship to the factory for repair. For an end user, it is important to ask the machine sales person about the spindle service program in advance, and make sure the high- speed machine or spindle OEM has a repair program in the States instead of overseas.

Jesse Xi Chen
Compumachine Inc.

Dear Shop Doc,

On our CNC lathes we occasionally have trouble with push back when using collets on bar jobs. Our collets have smooth bores and I am wondering if a serrated collet would help or if it will just create more problems.

Chuck Force

Dear Chuck Force,

Serrated collets will probably help, but first let’s consider all of the variables.

1. Bar whip—Bar whip can cause the bar to act as a lever against the collet, prying it open. You should always use a spindle liner and/or a properly sized liner set in your bar feeder to minimize bar whip.
2. Collet bore—Most collet systems have some gripping range, but the bore of the collet can only be machined to one given nominal diameter, and that diameter fits the bar the best. Avoid using a collet that’s “close enough.”
3. Chucking pressure—The hydraulic pressure to the rotary actuator can be adjusted. Follow the manufacturer’s recommendation for the operating range and adjust accordingly. In general, you need higher pressure for larger diameter bar and less pressure for small diameters.
4. Maintenance—Make sure that the sliding components of your collet chuck are clean, lubricated and slide easily. Make sure your hydraulic oil is in good condition, the level is adequate, and the system is operating in the proper temperature range.

Serrated collets work by reducing the surface area of the collet bore, thereby increasing the pressure that the contact area of the collet exerts against the work. You can calculate the surface area of the collet bore using the formula: 2 π r2 + 2 π r h. Ignoring the area removed by the slots in the collet, a 1.0” diameter collet with a 1-1/4” land has 5.5 in² of gripping surface.

If the collet closes with 1,000 pounds of force, that force is distributed over the 5.5 in² surface area of the bore, resulting in a contact pressure of 181.8 psi. If you decrease the surface area of the collet bore by machining in serrations, you increase the contact pressure by a corresponding amount. This doesn’t multiply the holding force in any way; you are still applying the same 1,000 pounds of force to the task of holding the work. By applying the force to a smaller area with greater pressure, the collet can dig into (deform) the work. Whether or not the collet permanently marks the work (plastic deformation), or the work bounces back (elastic deformation) depends on the force applied.

Another option is to have the collet coated with a textured carbide alloy coating like Carbinite (go to www.carbinite.com for more info). The principle is the same as serrations, but instead of grooves cut into the collet bore, the bore is coated with a crystalline like carbide alloy. The coating has a texture similar to sandpaper, which provides tremendous grip.

Dan Murphy
REM Sales LLC

Dan Murphy is a regional sales manager for REM Sales LLC., a U.S. Tsugami importer. He can be reached at dmurphy@remsales.com.

Dear Shop Doc,

I have problems at times with indexable boring bars when boring holes on my lathe. It seems the diameter or surface finish isn’t as good as I expect it to be, and for this job, I need to have consistent diameters due to some very close tolerances. I have tried cutting at the speed and feed parameters recommended in the tool catalogs, but most of the time the tool chatters until I slow it down. I have checked the centerline for proper alignment and believe it is set correctly. Shop Doc, I need some help quick !!!

Signed,
“Stop The Bore-Dumb”

Dear Bore-Dumb,

I believe we can steer you toward a solution rather quickly. The two topics that we will focus on are length to diameter ratio and tool nose radius. These topics contribute to the majority of problems in boring applications.

Indexable type boring bars are made of basically three materials—steel, heavy metal and carbide. Some manufacturers are getting quite sophisticated with these tools with dampening features and special designs, but let’s keep this simple. A 1” diameter bar hanging out of a holder 4” in length is considered to be a 4 to 1 length to diameter ratio.

Steel bars can be used in relatively shallow depth bores such as 4 to 1 ratios. Heavy metal bars can be used in bores up to a 6 to 1 ratio. Carbide bars are used for bores up to an 8 to 1 ratio. The stiffness of the bar is the key factor. The bar must be capable of hanging out that far and still be sturdy enough to not have the cutting forces affect the tool adversely while in the cut. There is a cost involved—steel is cheapest, heavy metal is slightly more expensive and carbide is the most expensive.

Tool nose radius selection is crucial regardless of what bar you use. You need to know how much material you will leave for the tool nose radius on the insert you wish to use. The correct amount of material per side will be equal to or greater than the radius of the tool. This enables the material to be engaged completely around the radius of the tool. Always try to leave more material in the hole per side than what the selected tool nose radius is. If you need to use a larger radius, leave more stock per side. This engagement stabilizes the cutting forces of the tool and provides a smooth, consistent cutting action resulting in consistent diameters and tolerances.

Also, you might want to try out the wiper insert technology available today. It allows faster feed rates and better surface fi nish due to the design of the tool nose radius and clearances following the cutting tip.

One last thing to remember—Because the tip of the tool plays a huge role in creating successful bores, the center line of the tool must be as close to the machine center line as possible. If it’s not close, some really weird pressures can occur, giving you negative results.

Good Luck.

Jim Rowe
Application Specialists / Medical Accounts
Mahar Tool Supply, Warsaw, IN

We are a mold shop specializing in cutlery molds with large cavities and tiny details, usually from 420 stainless steel hardened to 48 to 50HRC. Some corner radii are as small as 0.008”. For years, we have been using EDM machines to burn our hardened cavities and cores—a very time consuming process. I’ve heard that high-speed hard milling is the new process for mold-making. Can it really replace our EDM?

-Make Us Faster

Dear Make Us Faster,

You are right. High Speed Machining (HSM) has made a huge impact on the mold-making process in recent years. HSM is a machining process using smaller tools with high rpm and feed-rate to perform faster, lighter cuts. Surprisingly, tackling hard milling is simplified using this high-speed technique. Conventionally, cutting hardened tool steel with large tools generates a lot of heat that breaks down the end mill rapidly, making milling an impractical option. Hence the EDM (Electrical Discharge Machining) became the standard process to machine hardened steel. With HSM however, every cut is small, light and fast, minimizing thermal effects and lowering heat transfer to the end mill, so the tool will last to finish the cavity. Together with the advances in cutting tool technology, HSM Hard Milling has become a very practical alternative with major savings in time and cost.

To determine whether HSM can replace your EDM process, you must study the characteristics of your mold cavities. Obviously a 90 degree sharp internal corner can only be accomplished with EDM. For big cavities, milling is always faster than EDM. As for small features, the recommended rpm goes up proportionally as the end mill radius goes down. Small radius alone is not the issue. What makes hard milling difficult is when the end mill becomes too slim and therefore lacks strength to support its cutting. It is the ratio of the end mill diameter to neck length that is important. When hard milling with end mills under 1/4”, the rules of thumb are: a 1:3 ratio is considered stubby, 1:5 is practical, 1:8 is difficult and requires a lot of careful programming, and 1:10 probably is the limit.

Having said that, please bear in mind that HSM also compliments the EDM process. Mold cavities typically consist of free-form surfaces that are machined with ball end-mills, and the “cusp” between paths decides the final surface finish. For example, a 1/8” ball end mill with 0.003” step-over will produce a “cusp” height of 18 micro-inches. A silky smooth surface finish requires densely packed tool paths that make machining at a high rpm and feed-rate essential for cycle time reduction. This is true for both hard milling and electrode machining.

When you are considering HSM for your shop, please be aware of the upfront costs associated. A true high speed machine costs more than a conventional CNC machining center. They typically have bridge construction and are equipped with high-speed motor spindles with anywhere from 20,000 rpm to 50,000 rpm. Other critical features to look into include advanced CNC with look-forward capabilities, large storage, Ethernet connection and thermal control. Last but not least, it is the human factor, from process planning and tooling selection, to programming and setup that separates the men from the boys in HSM implementation.

-Jesse Xi Chen
Jesse Xi Chen Compumachine Inc.

Dear Shop Doc,

We are running a long aluminum part on our CNC Swiss and have problems with the long stringy chips building up in the machine and getting wrapped around the part. We’ve tried every “aluminum” insert under the sun and have 2,000 psi coolant, but nothing works. Please help!

Tangled Up in Tennessee

Dear Tangled,

There is a new chip control technology for aluminum that I’ve found to be very effective. It’s a PCD (polycrystalline diamond) insert that has a 3D chipbreaker. Up until now, manufacturers have been unable to produce 3D chipbreakers in the ultra-hard polycrystalline diamond material. A new process has been developed that uses a laser to etch a variety of 3D chipbreaker shapes into the PCD. The inserts are made by Becker Diamont.

They have a video on YouTube that can be found at: www.youtube.com/watch?v=gLRJdMDvbpY. A brochure can be downloaded at: www.ranitool.com/ChipBreaker-ranilowres.pdf.

On a Swiss I’ve found that it’s the feed rate that is critical to getting the chip to break. In general, a larger depth of cut requires a slightly higher feed rate. On a fixed headstock lathe, you can also vary the depth of cut and the feed rate for optimum results.

Other possible solutions include milling a flat or narrow slot along the length of the cut before turning. I prefer to use a narrow slotting saw to cut an off-center slot along the turn length. A narrow slot has less chance of generating an out-of-round condition on the turned diameters. Milling the slot off of the centerline of the work prevents the slot from hitting the turning insert squarely. The slot being off center along with the rotation of the work causes the slot to hit the insert and travel by it on an angle. This eliminates any pounding caused by the interruption while providing enough interruption to break the chip.

Problems with grooving and cutoff tools can often be solved by using a peck cycle like G75, which is like a peck drilling cycle, but from the cross axis rather than along the Z-axis.

Ultimately these other options add cycle time while the PCD insert will likely reduce cycle time and improve uptime.

You will pay more for PCD, but it almost always costs less than a polished carbide insert due to the vastly improved tool life.

Another added benefit is that once you start breaking the chips up, you won’t have to empty out the chip bin nearly as often. Those long wiry chips create big air pockets that take up a lot of space.

Dan Murphy
Tsugami REM Sales

Dear Shop Doc,

We are frequently utilizing indexable carbide inserts for single point turning processes in our shop. It appears that most of these inserts are available in M (molded) or G (ground) tolerances. Can you tell me the benefits of one over the other? Also, how will I see the performance advantages from the more expensive G inserts?

Weighing In

Dear Weighing In,
Let’s first briefly touch base on how an insert is made. Several powders which make up the substrate of the carbide are molded into the shape desired. The next step is to “sinter” or basically bake it. This sintering process actually shrinks the insert to the size desired, with a tolerance for its thickness and inscribed circle dimensions.

At this “molded” point, all that is left is to prep the cutting edges, then inserts are ready to make chips. There isn’t any other cost involved other than packaging. Some of these molded inserts will be coated, which is one more step that adds to the cost. A subsequent grinding operation can take place on the edges, and or top and bottom of the inserts. This will ensure each insert will be held to a given tolerance.

A great reason to use ground inserts is that once you establish the centerline of a turning insert, the next insert should be sitting at the same height. Incorrect centerline height is one of the most common causes of poor tool life in turning applications.

Also, as you index the insert from cutting edge to cutting edge, you should be able to reset any wear offsets (on a CNC machine) or back off any adjustments to the starting position that the last tip of the insert started at, and begin with a good part or dimension that this tool is cutting. Each manufacturer states their tolerance on their insert. Typically it is the third letter in their insert nomenclature

In some cases, to maximize machining effectiveness when cutting materials such as aluminum or titanium, a slicing or shearing action is exactly what is preferred. This is obtained by further grinding a sharper cutting edge on the insert.

Jim Rowe
Mahar Tool Supply