Grooving plus

Author Cutting Tool Engineering
Published
August 01, 2010 - 11:00am

Multifunction groove/turn tools stretch shops’ definition of a grooving tool.

Most shops associate “grooving” only with cutting a simple slot around the OD of a shaft. However, some grooving tools have capabilities beyond that, including turning, contouring and facing. According to toolmakers, keys to maximizing benefits from multifunction grooving tools are understanding their capabilities and having confidence in their application.

Duane Drape, national sales manager for HORN USA Inc., Franklin, Tenn., provided a nontraditional take on grooving: “Paraphrasing our owner, Lothar Horn, we define grooving as machining between two flanks or two shoulders—and one flank or shoulder doesn’t necessarily have to be there.” 

A flat-bottom hole requiring a groove at the bottom is a good example, he said. “If it couldn’t cut all the way down to the face at the bottom, it wouldn’t be able to cut the groove,” Drape said.

The same tool used for grooving the bottom of a hole can also bore/mill the hole. “When that is done on a machining center, the tool has to rotate and helically interpolate, using the same process as a thread mill,” he said. “Although it is opening the bore, it is still a grooving tool.” If the bore and the top face of that component have to be perpendicular to each other, the machinist can facemill with the same insert. 

Drape pointed out that a thread and a groove differ really only in name. “A thread is simply a helical, continuous groove.”

Multifunction grooving tools have been available for decades, and have seen extensive development over that time, according to Drape. As a result, much groove/turn tool improvement focuses on upgrading and modernizing existing technology. 

M275 - Cutter Body.tif

Courtesy of HORN USA

Multifunction grooving systems include tools engineered for application on machining centers as well as lathes. An example is the new line of M275 cutters from HORN USA. The cutters can accept grooving inserts as well as facemilling inserts and have multiple teeth to maximize metal-removal rates. 

Copy of Application-12.tif

Courtesy of Iscar Metals

When applying a grooving insert in a turning operation, a controlled degree of deflection is desirable. Without deflection, the tool edge sits flat on the part and the extended surface contact causes chatter. Conversely, when side-cutting pressures deflect the tool in a groove/turn operation, the insert tilts slightly, reducing edge contact with the workpiece. Precise control of variables can achieve tolerances as tight as ±0.0004 ".

“We are not reinventing the wheel,” he said. “For example, we continuously improve chipbreaker designs.” He pointed out that a tool cutting grooves in castings or forgings, especially on a lathe, does not cut with the full face of the insert because a casting has draft angles. Cutting with only portions of the face can complicate chip control. In response, tool manufacturers have developed chipbreaker geometries such as those on HORN’s HR (hard roughing) inserts. The design features a platform chipformer for long-chipping materials, such as low-carbon steel.

Drape’s definition of multifunction grooving tools includes those used on machining centers as well as lathes. An example from HORN is the line of M275 cutters it will introduce at IMTS. The cutters can accept grooving inserts from 1.2mm to 3.25mm wide, but can also handle facemilling inserts capable of 4.0mm DOCs. The standard cutters range in size from 31mm in diameter with four inserts to 98mm in diameter and 10 inserts. Drape said the tools are not for the general facemilling market, but for applications where a smaller tool with multiple teeth is needed to achieve high productivity. 

Preconceived Grooving

Some users may need to overcome preconceptions about multifunction grooving tools, according to Matt Schmitz, turning product manager, U.S. north central, Iscar Metals Inc., Arlington, Texas. While a traditional grooving tool usually has a dead-sharp front edge, a grooving/turning insert includes a chipformer and edge preparations on the front, left and right sides of the insert to enhance tool life, productivity and chip control, he said. Edge preparations include T-lands for machining cast iron, ground periphery and diamond polish for aluminum and more positive geometries for high-temperature work materials.

Yet despite the added geometry, many shops presume that moving a grooving insert in the Z-axis to turn or profile will magnify chip control problems. “You would think that would be one of your biggest challenges, but it’s not,” Schmitz said. “It can be difficult to break a chip in a simple plunge-grooving cut, especially in a gummy material. 

“But in a side-turning operation with a properly designed groove/turn insert, if you are taking a deep enough DOC, the chip wants to curl back toward the insert and the part and typically will break easily,” he said. “Programming can optimize each of the three cutting edges, but the programmer must ensure that only one cutting edge is engaged in the cut at a time, and be aware that, when generating radii during a plunging move, that the side edge may engage any material that has not been cleared away.”

Schmitz said some shops are skeptical about side turning with a grooving tool because “they look at a grooving tool, get nervous and say, ‘I’m not supposed to turn with this thing!’ ” Some of the concern regards tool deflection caused by side forces that are not present in simple plunge grooving. Actually, a controlled degree of deflection is desirable. “When it comes to groove/turning, if you don’t get deflection, the tool edge sits flat on the part and is going to chatter to beat the band because there is a lot of surface contact,” he said.

Conversely, when side-cutting pressures deflect the tool in a groove/turn operation, the insert tilts slightly and tool edge contact with the workpiece is reduced. Schmitz said the deflection must be carefully controlled by managing several variables, including feed rate, cutting speed, DOC, tool overhang, insert width support and the workpiece’s cutting characteristics. When those factors are balanced and kept constant, tolerances as tight as ±0.0004 " can be achieved. Schmitz said the results are similar to that of wiper-geometry turning inserts for imparting fine surface finishes.

Although programming rough grooving/turning operations is typically straightforward, peak accuracy, especially in finishing, usually requires in-process adjustment, according to Schmitz. “For finish cuts, it’s not going to be ‘program it, hit the green button and go,’ ” he said. “You have to tweak it.” He said changing the feed rate is typically the best starting point for adjustments.

A tool operating in a deflected orientation will not produce a square shoulder, he added. “The key is to program the tool to leave the cut at a 45º angle before reaching the side of the shoulder, and then plunge the shoulder separately,” Schmitz said. “When you are plunging, you don’t have deflection.” Similarly, if a groove needs to be machined at the end of a turned section of the part, the tool should be moved in the direction opposite the feed for about 0.1mm, releasing the deflection, before the plunge grooving begins. 

According to Schmitz, Iscar’s HELI-GRIP tools are capable of external, internal and face groove/turn operations. The inserts have a double-ended, twisted body that avoids backside contact with the machined groove surface, and the tool’s geometry manages chip formation in both axial and radial directions. 

Not all grooving inserts can deflect, Schmitz noted. For example, inserts in Iscar’s PENTA tooling line have a rigid, deflection-resistant mount to provide maximum stability when shallow grooving, parting and recessing. However, the tools can perform light side turning because a concave shape on the front cutting edge reduces the amount of contact between the insert and the workpiece.

Confidence Required

Toolmakers need to educate end users on the enhanced capabilities of groove/turn tools, according to Scott Etling, manager, global threading, grooving and cutoff for Kennametal Inc., Latrobe, Pa. What often complicates the tool choice, however, is that grooving platforms are typically proprietary.

Many grooving tools are designed for certain work materials, but can still be used in other applications. Etling cited the example of tools with Kennametal’s Grooving Universal Positive (GUP) geometry, which produces low cutting forces and good chip control in stainless steels and high-temperature alloys, according to the company. Although those materials were the initial design targets for the GUP tools, he said the geometry has found wider applications in other materials and even selected cutoff operations. 

Copy of A4_GUP_Geom_Inserts_BlkA.tif

Courtesy of Kennametal

While grooving/turning tools are typically designed to maximize productivity in certain materials, some can be more broadly applied. For example, Kennametal’s Grooving Universal Positive (GUP) geometry lowers cutting forces and enhances chip control when cutting stainless steels and high-temperature alloys, and the tools are suitable for other applications as well, according to the company. 

In addition to ongoing insert geometry development, new tool bodies can improve groove/turn performance. For example, Kennametal introduced bodies with a shorter tool overhang distance (CD) than standard ones. Reducing the extension of the insert beyond the body in these short-overhang, A-4 holders increases tool rigidity and allows higher feed rates and faster turning than tools with longer overhang, according to Kennametal.

When turning with turn/groove tools, users can typically double the feed rate compared to grooving, according to Etling. “For example, if you are grooving at 0.005 ipr, you can turn at 0.010 ipr,” he said. “That would be equivalent to some of the ISO turning inserts available.” He cautioned that the relationship only represents a rule of thumb. “You’d have to look at the whole setup, including the workpiece and tool overhang. Typically, you go to a higher feed rate if you are looking for higher metal-removal rates, and apply a slower feed rate for a finishing pass.” 

A Strategic Advantage

“The combination of features multifunction [grooving] tools can create is their greatest asset,” said Ken King, COO of THINBIT/Kaiser Tool Co. Inc., Fort Wayne, Ind. “Those features include arcs, angles, chamfers, radii, grooves, face grooves and any other feature you can machine on a lathe.” 

Copy of 1groove & turn.tif

Courtesy of THINBIT/Kaiser Tool

One grooving tool can be programmed to create a variety of features. That means part geometry can be altered by simply changing a CNC program rather than mounting a new tool. 

King said multifunction grooving tools can also simplify the formation of groove geometry, enable features of the geometry to be linked on a single tool and increase productivity. “The applications are only limited by the design of the tool or the limitations of the structural strength of the tool,” he said. 

The tools’ capabilities can help shops respond to ongoing manufacturing trends. “Long-running jobs are no longer the norm, and ‘get in and get done’ is the mentality,” King said. When a short production run ends, multifunction tools are “more versatile and can be repurposed for the next job,” he said. The tools’ adaptability also facilitates quicker turnaround when a shop’s customer needs an emergency delivery. 

In addition to creating specific part features, tools that perform more than one function can improve shop processes, including reduced cycle times due to fewer tool changes, increased open turret locations, simplified tool ordering and reduced tool inventory because the same tools can be used on multiple jobs. Because one tool can be programmed to create a variety of features, a change in part geometry can often be accomplished by simply changing a CNC program rather than mounting a new tool.

Custom tools are often required when standard tools cannot produce the desired groove form. As a result, THINBIT supplies both specials and standards with multifunction capability. Modifications to standards can include changes to tool details, including WOC and DOC, lead angle, top rake and chipbreaker configurations, and back and side clearances.

Despite the process improvement advantages of multifunctional grooving systems, many shops remain unaware of the tools’ full capabilities. “We continuously hear at trade shows, ‘Oh heck, I had to make a tool to do that myself. I wish I would have known about this,’ ” said HORN’s Drape. CTE

About the Author: Bill Kennedy, based in Latrobe, Pa., is a contributing editor for Cutting Tool Engineering. He has an extensive background as a technical writer. Contact him at (724) 537-6182 or by e-mail at billk@jwr.com.

In a problem-solving groove 

The main purpose of groove/turn tools is to create a variety of part features with one tool. However, the tools’ configuration may also allow them to solve problems other tools can’t.

Matt Schmitz of Iscar Metals said the basic design of a grooving insert and holder can facilitate chip management in some situations. For example, chip control can be challenging when boring a blind-hole, especially with smaller diameters where the boring bar and ISO insert occupy much of the space in the bore. 

“The chip wants to go in front of the tool and back around the bottom of the bore,” Schmitz said. On the other hand, a grooving insert, by design, generally extends farther from the centerline of the bar than an ISO boring insert (offering greater Tmax, or distance between the cutting edge and toolholder) and the greater clearance between the insert tip and the holder provides ample room for chip flow. 

Employing the tool in a pull-boring mode can further enhance chip evacuation, Schmitz said. In pull boring, the tool travels into the bore without cutting, is engaged at the bottom of the bore, and then is retracted or pulled towards the hole mouth. Chips are formed on the backside of the insert and coolant can evacuate the chips. 

As an example, Schmitz described an application that involved machining a coupling from 3 "-dia., ¼ "-thick, 1010 steel tubing. The lathe operation consisted of cutting ID bores in each end of the coupling and machining a smaller bore in the center, then cutting the part off the tube. Chip control was a problem in the gummy steel, and push boring the inner bore packed chips into the tube, resulting in “tools blowing up left and right,” Schmitz said. To solve the problem, a grooving bar pull bored the back counterbore and simultaneously machined a 45º ID chamfer where the part was to be cut off. When ID machining was completed, the chamfer was the basis of a clean parting-off cut. Pull boring didn’t break the chip, but “we were able to manage the chips so that when we extracted the tool, the chips fell out of the workpiece and safely came to rest on the chip conveyor,” Schmitz said.

—B. Kennedy

Contributors

HORN USA Inc.
(888) 818-4676
www.hornusa.com

Iscar Metals Inc. 
(877) 294-7227
www.iscarmetals.com

Kennametal Inc. 
(800) 446-7738
www.kennametal.com

THINBIT/Kaiser Tool Co.
(888) 844-6248
www.kaisertool.com

Related Glossary Terms

  • Rockwell hardness number ( HR)

    Rockwell hardness number ( HR)

    Number derived from the net increase in the depth of impression as the load on the indenter is increased from a fixed minor load to a major load and then returned to the minor load. The Rockwell hardness number is always quoted with a scale symbol representing the indenter, load and dial used. Rockwell A scale is used in connection with carbide cutting tools. Rockwell B and C scales are used in connection with workpiece materials.

  • alloys

    alloys

    Substances having metallic properties and being composed of two or more chemical elements of which at least one is a metal.

  • bandsaw blade ( band)

    bandsaw blade ( band)

    Endless band, normally with serrated teeth, that serves as the cutting tool for cutoff or contour band machines.

  • blind-hole

    blind-hole

    Hole or cavity cut in a solid shape that does not connect with other holes or exit through the workpiece.

  • boring

    boring

    Enlarging a hole that already has been drilled or cored. Generally, it is an operation of truing the previously drilled hole with a single-point, lathe-type tool. Boring is essentially internal turning, in that usually a single-point cutting tool forms the internal shape. Some tools are available with two cutting edges to balance cutting forces.

  • boring bar

    boring bar

    Essentially a cantilever beam that holds one or more cutting tools in position during a boring operation. Can be held stationary and moved axially while the workpiece revolves around it, or revolved and moved axially while the workpiece is held stationary, or a combination of these actions. Installed on milling, drilling and boring machines, as well as lathes and machining centers.

  • centers

    centers

    Cone-shaped pins that support a workpiece by one or two ends during machining. The centers fit into holes drilled in the workpiece ends. Centers that turn with the workpiece are called “live” centers; those that do not are called “dead” centers.

  • chatter

    chatter

    Condition of vibration involving the machine, workpiece and cutting tool. Once this condition arises, it is often self-sustaining until the problem is corrected. Chatter can be identified when lines or grooves appear at regular intervals in the workpiece. These lines or grooves are caused by the teeth of the cutter as they vibrate in and out of the workpiece and their spacing depends on the frequency of vibration.

  • chipbreaker

    chipbreaker

    Groove or other tool geometry that breaks chips into small fragments as they come off the workpiece. Designed to prevent chips from becoming so long that they are difficult to control, catch in turning parts and cause safety problems.

  • clearance

    clearance

    Space provided behind a tool’s land or relief to prevent rubbing and subsequent premature deterioration of the tool. See land; relief.

  • computer numerical control ( CNC)

    computer numerical control ( CNC)

    Microprocessor-based controller dedicated to a machine tool that permits the creation or modification of parts. Programmed numerical control activates the machine’s servos and spindle drives and controls the various machining operations. See DNC, direct numerical control; NC, numerical control.

  • coolant

    coolant

    Fluid that reduces temperature buildup at the tool/workpiece interface during machining. Normally takes the form of a liquid such as soluble or chemical mixtures (semisynthetic, synthetic) but can be pressurized air or other gas. Because of water’s ability to absorb great quantities of heat, it is widely used as a coolant and vehicle for various cutting compounds, with the water-to-compound ratio varying with the machining task. See cutting fluid; semisynthetic cutting fluid; soluble-oil cutting fluid; synthetic cutting fluid.

  • counterbore

    counterbore

    Tool, guided by a pilot, that expands a hole to a certain depth.

  • cutoff

    cutoff

    Step that prepares a slug, blank or other workpiece for machining or other processing by separating it from the original stock. Performed on lathes, chucking machines, automatic screw machines and other turning machines. Also performed on milling machines, machining centers with slitting saws and sawing machines with cold (circular) saws, hacksaws, bandsaws or abrasive cutoff saws. See saw, sawing machine; turning.

  • cutting speed

    cutting speed

    Tangential velocity on the surface of the tool or workpiece at the cutting interface. The formula for cutting speed (sfm) is tool diameter 5 0.26 5 spindle speed (rpm). The formula for feed per tooth (fpt) is table feed (ipm)/number of flutes/spindle speed (rpm). The formula for spindle speed (rpm) is cutting speed (sfm) 5 3.82/tool diameter. The formula for table feed (ipm) is feed per tooth (ftp) 5 number of tool flutes 5 spindle speed (rpm).

  • facemill

    facemill

    Milling cutter for cutting flat surfaces.

  • facemilling

    facemilling

    Form of milling that produces a flat surface generally at right angles to the rotating axis of a cutter having teeth or inserts both on its periphery and on its end face.

  • feed

    feed

    Rate of change of position of the tool as a whole, relative to the workpiece while cutting.

  • flat ( screw flat)

    flat ( screw flat)

    Flat surface machined into the shank of a cutting tool for enhanced holding of the tool.

  • grooving

    grooving

    Machining grooves and shallow channels. Example: grooving ball-bearing raceways. Typically performed by tools that are capable of light cuts at high feed rates. Imparts high-quality finish.

  • inner diameter ( ID)

    inner diameter ( ID)

    Dimension that defines the inside diameter of a cavity or hole. See OD, outer diameter.

  • lathe

    lathe

    Turning machine capable of sawing, milling, grinding, gear-cutting, drilling, reaming, boring, threading, facing, chamfering, grooving, knurling, spinning, parting, necking, taper-cutting, and cam- and eccentric-cutting, as well as step- and straight-turning. Comes in a variety of forms, ranging from manual to semiautomatic to fully automatic, with major types being engine lathes, turning and contouring lathes, turret lathes and numerical-control lathes. The engine lathe consists of a headstock and spindle, tailstock, bed, carriage (complete with apron) and cross slides. Features include gear- (speed) and feed-selector levers, toolpost, compound rest, lead screw and reversing lead screw, threading dial and rapid-traverse lever. Special lathe types include through-the-spindle, camshaft and crankshaft, brake drum and rotor, spinning and gun-barrel machines. Toolroom and bench lathes are used for precision work; the former for tool-and-die work and similar tasks, the latter for small workpieces (instruments, watches), normally without a power feed. Models are typically designated according to their “swing,” or the largest-diameter workpiece that can be rotated; bed length, or the distance between centers; and horsepower generated. See turning machine.

  • lead angle

    lead angle

    Angle between the side-cutting edge and the projected side of the tool shank or holder, which leads the cutting tool into the workpiece.

  • machining center

    machining center

    CNC machine tool capable of drilling, reaming, tapping, milling and boring. Normally comes with an automatic toolchanger. See automatic toolchanger.

  • milling machine ( mill)

    milling machine ( mill)

    Runs endmills and arbor-mounted milling cutters. Features include a head with a spindle that drives the cutters; a column, knee and table that provide motion in the three Cartesian axes; and a base that supports the components and houses the cutting-fluid pump and reservoir. The work is mounted on the table and fed into the rotating cutter or endmill to accomplish the milling steps; vertical milling machines also feed endmills into the work by means of a spindle-mounted quill. Models range from small manual machines to big bed-type and duplex mills. All take one of three basic forms: vertical, horizontal or convertible horizontal/vertical. Vertical machines may be knee-type (the table is mounted on a knee that can be elevated) or bed-type (the table is securely supported and only moves horizontally). In general, horizontal machines are bigger and more powerful, while vertical machines are lighter but more versatile and easier to set up and operate.

  • outer diameter ( OD)

    outer diameter ( OD)

    Dimension that defines the exterior diameter of a cylindrical or round part. See ID, inner diameter.

  • parting

    parting

    When used in lathe or screw-machine operations, this process separates a completed part from chuck-held or collet-fed stock by means of a very narrow, flat-end cutting, or parting, tool.

  • rake

    rake

    Angle of inclination between the face of the cutting tool and the workpiece. If the face of the tool lies in a plane through the axis of the workpiece, the tool is said to have a neutral, or zero, rake. If the inclination of the tool face makes the cutting edge more acute than when the rake angle is zero, the rake is positive. If the inclination of the tool face makes the cutting edge less acute or more blunt than when the rake angle is zero, the rake is negative.

  • recessing

    recessing

    A turning operation in which a groove is produced on the periphery or inside a hole of a workpiece. The grooving tool moves at right angles to the axis of rotation.

  • stainless steels

    stainless steels

    Stainless steels possess high strength, heat resistance, excellent workability and erosion resistance. Four general classes have been developed to cover a range of mechanical and physical properties for particular applications. The four classes are: the austenitic types of the chromium-nickel-manganese 200 series and the chromium-nickel 300 series; the martensitic types of the chromium, hardenable 400 series; the chromium, nonhardenable 400-series ferritic types; and the precipitation-hardening type of chromium-nickel alloys with additional elements that are hardenable by solution treating and aging.

  • threading

    threading

    Process of both external (e.g., thread milling) and internal (e.g., tapping, thread milling) cutting, turning and rolling of threads into particular material. Standardized specifications are available to determine the desired results of the threading process. Numerous thread-series designations are written for specific applications. Threading often is performed on a lathe. Specifications such as thread height are critical in determining the strength of the threads. The material used is taken into consideration in determining the expected results of any particular application for that threaded piece. In external threading, a calculated depth is required as well as a particular angle to the cut. To perform internal threading, the exact diameter to bore the hole is critical before threading. The threads are distinguished from one another by the amount of tolerance and/or allowance that is specified. See turning.

  • turning

    turning

    Workpiece is held in a chuck, mounted on a face plate or secured between centers and rotated while a cutting tool, normally a single-point tool, is fed into it along its periphery or across its end or face. Takes the form of straight turning (cutting along the periphery of the workpiece); taper turning (creating a taper); step turning (turning different-size diameters on the same work); chamfering (beveling an edge or shoulder); facing (cutting on an end); turning threads (usually external but can be internal); roughing (high-volume metal removal); and finishing (final light cuts). Performed on lathes, turning centers, chucking machines, automatic screw machines and similar machines.