Browse: Home / Shop Doc Blog

Shop Doc – Improving Surface Finish

By Dan Murphy on December 19, 2011

Today’s Machining World Archives June 2011 Volume 07 Issue 05

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

Posted in , , , | 2 Responses

Shop Doc – Should I rebuild my Acme?

By Dave Johnson on December 12, 2011

Dear Shop Doc,

My Acme-Gridley screw machines have been real money makers over the years, but all that production takes its toll in wear and tear on the machines. Will I be better off doing major repairs to my current Acmes, looking for deals on good used Acmes, or investing in some type of new machinery?

Which Way Should I Go

Dear Which Way,

Acme-Gridley multi-spindle automatics are well designed to be rebuilt or reconditioned, and worn machines can be returned to good running or like new condition by those qualified to perform that type of work. There are different levels of repair to choose from.

For example, you have a 1-1/4” RA6 Acme machine that needs some work. The heart of an Acme is the spindle carrier, which you might start looking at having rebuilt for around $10,000. This includes rebuilt work spindles, new precision spindle bearings, new front and rear retainers and flingers, and new spindle gears, adjusting nuts and keys. The carrier stem is also ground, and fitted to your re-bushed and bored main tool slide. At the high end of your list of options you have a complete machine rebuild, which for all practical purposes is like a new machine. That will cost in the neighborhood of $100,000 to $150,000, depending on your machine and requirements. Compare that to a price tag of $500,000 or more for a comparable new multi-spindle cam machine.

Another factor to consider is that a rebuilt Acme, when properly maintained, can be run hard for 10 years or more before it will require another rebuild. Most single-spindle CNC machines never get that old before they are obsolete or worn out. Acme-Gridley machines come in a wide variety of models, capacities, and vintages. Some machines in service today predate 1950. With sound castings most of these machines are still great candidates for rebuild or recondition, with just a few old models that are obsolete.

A concern for some shop owners today is a lack of experienced machine repair personnel to remove or re-install a spindle carrier, but most qualified rebuilders can offer contracted field service work to do this for you.

Another option popular with some shop owners is look for an inexpensive, worn, late model machine and have it rebuilt. This could be a good option because its mechanical condition is not a concern as long as the castings are in good shape. But even if a machine is examined by experienced personnel when purchasing, the condition of the spindle bearings will largely be an unknown. So it may be a better option to invest money in a machine that you already have and know.

Acmes are well suited for high production part runs, or running a family of similar parts at moderate volumes, but may not be the best choice for small lot runs unless efforts are made to reduce setup times. Attachments are available for Acmes that allow even complex parts to come off the machine complete. In some cases shops are using Acmes in tandem with single-spindle CNC machines, with the Acme blanking the part and then a robot transferring the part to one or several inexpensive CNCs to finish it off. Your production time may be longer, but in the right type of job the dramatic savings on equipment could very well make up for the additional second or two.

Bottom line, your Acmes still have a lot of life left in them, so if you have the right work for them, rebuilding and refurbishing can definitely pay off.

Posted in , | 4 Responses

Shop Doc: Trouble with Deflection on CNC Swiss

By Dan Murphy on September 6, 2011

Dear Shop Doc,

We are trying to run a variety of very small parts on a 20 mm gang tool CNC Swiss and are having trouble with deflection when cross drilling and milling. Is there a way to get the live tools closer to the guide bushing?

 Bent in Benton Harbor

 

Dear Bent,

There is no way to bring the tool closer to the guide bushing face. You can bring the guide bushing face closer to the bar by ordering an extended nose guide bushing.

An ER16 live tool spindle is usually between 14-16 mm away from the face of the guide bushing. You can decrease that distance by using an extended nose guide bushing to take up most of that space. However there are several issues to consider.

The fixed position of the live spindle is set so that the spindle has adequate clearance for the collet nut on the live tool attachment. Simply extending the nose of the bushing out means that the nut will now interfere with the face of the guide bushing, so you must do one of two things:

1)      Extend the spindle by chucking on a smaller capacity ER8 or ER11 collet chuck. You can buy an ER8 or ER11 with a 10 mm shank and a mini nut. Mount the drill chuck in the live spindle and chuck the tool in the smaller capacity drill chuck. Stick the small drill chuck out far enough so that the ER16 chuck nut doesn’t hit the bushing face.

2)      Order the extended nose to be turned to a smaller diameter. You could for example have the extension made to a 3/8” diameter by 0.300” long. Then keep the ER16 chuck nut above that diameter while cross drilling.

You will also need to shim out all of your turning tools by the same amount of the extension, as well as set your drills back by the same amount. Your machine tool builder might offer blocks that will shim the whole gang slide out by a set distance.

One final solution that might work depending on your situation is to use larger diameter bar stock. A larger bar can provide extra rigidity if you turn up to the live tool feature, machine it, then turn. In order to work, the bar diameter must be at least 1/3 of the distance from the face of the bushing to the center of your live spindle or larger.

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

Have a technical question of your own? Email us and we’ll find a Shop Doc to answer it. Or, if you know a Shop Doc or are a Shop Doc contact us to contribute. emily@todaysmachiningworld.com, 708-535-2237

Extended nose guide bushings, courtesy of REM Sales, LLC.

Posted in , , | 2 Responses

Shop Doc: Mr. Bone Screw

By Peter Bagwell on August 24, 2011

Mr. Bone Screw

Dear Shop Doc,

I’m going to be rotary broaching a 9/64” hex in titanium. The hole is a blind hole about .160” deep. I’m worried about hydraulic pressure building up during the broaching operation. What are my options?

Mr. Bone Screw

Dear Mr. Bone Screw,

You have a few options available. But first, let’s talk about the hole. Be absolutely sure to drill it deeper than the broaching depth. You will need to leave room for chips, fluid, etc. The deeper the hole, the more room is available for swarf to get out of the way.

The first option has to do with your pilot hole. A pilot hole drilled to size will create significantly more pressure than one drilled oversize. The oversize hole allows air and fluid to escape. This larger pre-drill diameter also reduces the size of the chip while broaching. The chips are also sure to be separated. A standard 9/64” hex has a dimension across the flats of .1425”. Drilling the pilot hole about 3 percent larger, requires a drill size of .147”.

The following tooling options are all intended to reduce pressure while broaching. Most of these options are commonly available in the marketplace.

  • Spun, Ground Diameter – Eliminating the sharp corner from the broach reduces chip size and depth and strengthens the broach at the corners. Rotary broach failure is often a result of chipping at the corners.
  • Broach Pressure Relief Holes – Small holes added to the center of the broach and used in conjunction with secondary holes drilled in a cross direction allow the fluid and air to escape.
  • Broach Holder Relief Holes – A relief hole in the broach holder allows air and fluid to escape completely. Air and fluid are pushed through a center relief hole in the broach, and out of the holder through its relief hole. This option is currently available from Polygon Solutions and reduces cost of broaches requiring two vent holes.

Here are a couple tips to make sure you get the most out of your tooling. Make sure the broach is aligned with the pilot hole. This may seem obvious, but many machines can be off center by more than a few thousandths. Most broach holders have end play built into them. The broach will follow the hole. But double check it anyway; this is a common troubleshooting problem. Also, if you’re going to be broaching titanium, upgrade to a premium broach material, such as M-42 or PM T-15. These broach materials are very hard and include elements like cobalt to enhance their strength.

As you can see, all of the information here has to do with reducing the forces required while broaching and strengthening the broach. Hopefully these tips will relieve some of the pressure created when trying out a new machining operation. If you’re still uneasy, run the broach in aluminum to get a feel for the set-up.

Peter Bagwell is a Rotary Broach Product Engineer at Polygon Solutions. He is a frequent contributor to Today’s Machining World’s Shop Doc column and is also an Essential Oil enthusiast. To contact him, go to www.polygonsolutions.com.


Posted in , , | 3 Responses

Shop Doc – Polygon Milling on a Small Part

By David Cogswell on August 5, 2011

Todays Machining World Archives May 2008 Volume 04 Issue 05

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

Posted in , , , | Leave a response

Shop Doc – Justifying Use of a High-Speed-Spindle

By Jesse Xi Chen on August 2, 2011

Dear Shop Doc,

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.

Posted in , , , | 3 Responses

Shop Doc – Push Back Trouble Using Collets

By Dan Murphy on August 1, 2011

Today’s Machining World Archives January/February 2011 Volume 7 Issue 1

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.

Posted in , , , | 3 Responses

Shop Doc – High Speed Hard Milling

By Jesse Xi Chen on June 15, 2011

Dear Shop Doc,

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.

Posted in , , | 7 Responses

Shop Doc – Tangled Up in Tennessee

By Dan Murphy on June 14, 2011

Today’s Machining World Archive: April 2010 Vol. 6, Issue 03

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

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

Posted in , , , | 3 Responses

Shop Doc – Indexable Carbide Inserts for Single Point Turning

By Jim Rowe on June 1, 2011

Today’s Machining World Archives September 2007 Volume 03 Issue 09

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

Posted in , , , | 1 Response

  1. Pages:
  2. 1
  3. 2
  4. 3