FAQ

What is the correct definition: cutting tool or metal cutting tool?

Historically, metals were the main materials to produce machined parts. Therefore, cutting tools were intended primarily for machining metals, and this determined their name. Today the term "metal cutting tool" is rare enough, while simply "cutting tool" is much more common; and these two definitions have become synonyms.
What is "primary motion" and "feed motion"?

In machining, the primary motion is a rectilinear or rotational motion of a cutting tool or a workpiece that provides the tool advance toward the workpiece to ensure chip removal. In a machining process, the primary motion features the maximum speed and most of the energy, which is required for machining, when compared to all other motions. The primary motion in turning, for example, is the rotation of a workpiece, while in milling, the primary motion is the rotation of a mill.

The feed motion is a rectilinear or rotational motion of a cutting tool, which adds the primary motion to complete cutting action. This motion features significantly less speed when compared to the speed of a primary motion.
What is the difference between macro- and micro geometry of a cutting edge?

Macro geometry of a cutting edge relates to the key elements of a tool cutting wedge that determine the tool cutting capabilities such as the shape of the rake face, the rake angles, the clearance angles etc. Micro geometry is a microscopic-scale condition of the edge, which is known also as the edge preparation. Depending on the edge condition, the edge can be sharp, rounded (honed), chamfered edge or combined comprising combinations of rounding and chamfering.
What is the difference between specific cutting forces that are designated as k_c and k_c1?

"k_c" relates to actual specific cutting force - the force that is needed to remove a material chip area of 1 mm² (.0016 in²), which has actual average chip thickness maintained in a machining process.
"k_c1" is commonly used for designating the specific cutting force to remove a material chip area of 1 mm² (.0016 in²) with 1 mm (.004 in) thickness.
However, in some technical data sources, the actual specific cutting force may be designated by "k_c1", and specific cutting force to remove a material chip area of 1 mm² (.0016 in²) with 1 mm (.004 in) thickness by "k_c1.1". Number "1" that follows index "c" relates to 1 mm² chip area, and addition "1.1" highlights "1 mm² chip area with 1 mm thickness".
How are cutting tools classified?
There are distinctive features to classify cutting tools.
- The machining process, for which a tool is intended (turning tools, milling tools, drilling tools etc.)
- Primary motion (rotating, non-rotating)
- The number of a tool cutting edges (single-point tools that have only one cutting edge, and multi-point tools with more than one cutting edge)
- The tool design concept (solid or one-piece, and assembled)
- The tool mounting method (bore-type tools, shank-type tools)
- Adjustment capabilities (adjustable, non-adjustable)
Which tool is considered to be standard?

The definition "standard tool" has a certain duality. On the one hand, it may mean that a tool meets the requirements of a national (international) standard. On the other hand, cutting tool manufacturers use this definition to specify their in-stock products of standard delivery.
What is the correct term, "brazed tools" or "soldered tools"?

Principally, both brazing and soldering relate to the same process: joining various materials together using a molten metal (filler) between these parts, while the filler has a lower melting point than the joined materials. The main difference between brazing and soldering is the process operating temperature, which is less for soldering, and, accordingly, the type of filler. A brazed joint usually features higher strength when compared with a soldered connection. With relation to cutting tools, using the term "brazed" is more correct.
What is "oscillation cutting"?

Oscillation cutting is a machining technique that combines the primary motion with the additional oscillatory motion of a cutting tool relative to a machined workpiece to break chips.
What is the concept of high-efficiency machining?

High-efficiency machining (HEM) is a milling method much like high-speed machining (HSM), which utilizes a large axial depth of cut and a small radial depth of cut in combination with high rotational velocity (spindle speed) of the tool. However, the radial depth of cut varies depending on the angle of tool engagement to facilitate constant chip thickness per cutting edge during tool rotation. This method assures efficient use tool use for the uniform development of wear that covers a large section of the tool's cutting edge. HEM is often referred to as "dynamic milling" and features productive rough milling operations. HEM demands appropriate capabilities of CAM and CNC to generate the required toolpath.
What is the reference system of planes?

The reference system of planes is a rectangular coordinate system with the origin in a selected point of the tool's cutting edge. This system is used to specify the angles that determine the cutting geometry of a tool.
How is the reference system for planes selected?

The reference systems for planes are defined in the following manner: - the tool-in hand system, which specifies a tool cutting geometry for design, manufacturing, and measuring process of the tool. - the tool-in-use system is used to specify the cutting geometry of the tool in use. - the machine system is intended for checking the geometry when the tool is mounted in a machine. The tool-in-hand system relates to the element of a tool that is chosen as a base (datum). The tool-in-use system is aligned with the resultant cutting motion in a machining operation. The machining system uses the direction of primary motion as reference.
What are the main mechanisms of tool wear?

The main mechanisms of tool wear are as follows: - Abrasive wear, is due to the heterogeneous metallurgical structure of the workpiece material, that features particles of different hardness. This causes the tool to be exposed to impact like abrasive machining and the removal of cutting material from the tool. - Mechanical wear is caused due to excessive mechanical load that can lead to a damaged cutting edge. - Adhesive wear occurs at specific values of cutting speeds and temperature in the cutting zone, which results in tool areas being welded with the particles of the removed material. This forms a foreign reinforced material that becomes the cutting edge and changes the cutting geometry. - Oxidation wear happens when the oxygen in the air reacts with the upper layer of the cutting material under high temperature in the cutting zone. - Diffusion wear occurs because of the tool's joint diffusion of material particles, the machined workpiece, and the formed chips. This changes the composition of the cutting material and diminishes its cutting capabilities.
What is a wedge angle?

In cutting tool geometry, the wedge angle refers to the angle between the face and the flank of a cutting tool. Depending on the plane in which this angle is measured, it can be called a normal wedge angle or a back wedge angle.
What are tool angles and working angles, and what is the difference between them?

Tool angles and working angles refer to the angles that define the position of the cutting edge, face, and flank of a cutting tool. These angles include the cutting-edge angle, rake angle, clearance angle, and so on. The difference between tool angles and working angles can be understood as follows: Tool angles determine the position of these cutting tool elements when considering the tool as a separate object. Therefore, tool angles are measured in the tool-in-hand reference system of planes. On the other hand, working angles determine the position of these elements during the cutting action of the tool, and they are measured in the tool-in-use reference system.

Milling in General

What is a cutting edge angle and what is a lead angle?

There are various international and national standards that specify the active geometry of cutting tools very precisely. The “cutting edge angle” is the angle between the main cutting edge of a milling cutter and the plane containing the direction of feed motion. "Lead angle" (or “approach angle”) is the angle complementary to the cutting edge angle, i.e. the sum of these both angles is 90°. For example, for a typical face milling cutter the cutting angle is the angle between the cutting edge and the plane, which the cutter generates. If this angle is 60°, then the lead angle will be 30°. The cutting edge angle and the lead angle are equal only for 45° milling cutters. The term "lead angle" is more commonly employed in the U.S., while "approach angle" is often used in Europe.
What is the difference between "face mill" and "shell mill"?
These two terms relate to different and complementary features of milling cutters. They are not interchangeable. Milling cutters are classified according to the following main factors:
- Machine surface type: plane, shoulder, 3D-surface, etc.
- Cutter mounting method: on mandrel or arbor, in holder, directly in spindle
- Structure: monolithic; assembled
- Cutting part material: high speed steel, tungsten carbide, ceramics, etc.)
"Face mill" characterizes a main field of application - milling flats by the cutting face of a mill. "Shell mill" refers to the design configuration of a mill: the mill has a central bore for mounting on arbor. This configuration is typical for face mills.
What is the difference between heavy and heavy-duty milling?

Sometimes the terms “heavy” and “heavy-duty” are used mistakenly as synonyms. In principle, “heavy milling” (and “heavy machining") relates to milling large-sized and heavy-weight workpieces on powerful machine tools and refers more to the dimensions and mass of a workpiece. “Heavy-duty” specifies a degree of tool loading and mainly characterizes a mode of milling.
Which cutting conditions are considered as unfavorable and which are unstable?
Unfavorable cutting conditions include:
- workpiece with skin (siliceous or slag, for example)
- significantly variable machining allowance
- considerable impact load due to non-uniform machined surface
- surface with high-abrasive inclusions
Unstable cutting conditions refer to the low stability of a complete system (machine tool, workpiece holding fixture, cutting tool, workpiece) due to:
- poor tool and workpiece holding
- high tool overhang
- non-rigid machine tools
- thin-walled workpiece
The terms "unfavorable" and "unstable" are not interchangeable.
How is average chip thickness measured?

In milling, the thickness of chips is not constant and varies during cutting, depending on several factors. The average chip thickness (hm) is a virtual parameter that characterizes mechanical load on a milling cutter and a machine tool. There are different methods for calculating hm. The most common method is to compute it in relation to the half of an angle of engagement, where the latter is the central angle that corresponds to the arc of a contact between a milling cutter and a workpiece.
What is high pressure coolant (HPC) and ultra high pressure coolant (UHPC)?

There are no strict definitions of high and ultra high pressure coolant (HPC and UHPC correspondingly). Traditionally, machine tools feature coolant supply at pressure 10-15 bar (145-217 psi). This level is now considered as low pressure.
Various modern machining centers have the option to supply coolant at rates of 70-80 bar (1000-1200 psi), which is considered as high pressure coolant. Ultra high pressure coolant relates to pressure values of 100-200 bar (1450-2900 psi) and even higher.
Some producers of CNC machine tool equipment manufacture what are known as “medium pressure” pumps; these have values of up to 50 bar (725 psi).
What are the benefits of milling with high pressure coolant (HPC)?

Heat generation is a permanent feature of machining, particularly, milling. If heat generation is intensive, the conventional low pressure coolant forms a vapor layer on the surfaces of a tool and a workpiece. This layer acts as heat sealing, producing an insulating barrier and making heat transfer harder, which significantly shortens tool life.
Pinpointed high pressure coolant penetrates the barrier and helps to overcome the problem. HPC chills chips quickly, making them hard and brittle. The chips become thinner and smaller, and they break away from the workpiece more easily. High-velocity coolant flow removes the chips. This significantly improves chip evacuation and prevents chip re-cutting.
HPC improves tool life of a cutting edge due to reducing oxidation and adhesion wear and increasing crack strength. HPC improves chip evacuation because the chips diminish in size, and the high-velocity coolant flow takes them away easily. It allows the design of cutters with smaller chip gullet, leading to a higher number of cutter teeth. Effective cooling reduces the temperature in the cutting zone, ensuring an increased width of cut.
Overall, HPC provides a good solution for increasing cutting speed and feed rate for boosting productivity.
What is the difference between milling with high pressure coolant (HPC) supply through a tool body and turning with HPC?

In turning, a tool has one cutting edge, while a milling tool features several cutting teeth. The number of coolant outlets in the milling tool is greater. An indexable extended flute cutter, where the teeth are produced by sets of replaceable inserts, will require many more outlets.
There is a specific relationship between pressure, velocity and flow rate for fluid, e.g. for coolant. In milling, HPC supply through the tool body demands appropriate characteristics of an HPC pump to ensure correct flow volume (flow rate) and not only to meet pressure requirements.
Does ISCAR provides indexable cutters for high pressure coolant milling in the standard product line?

Yes, ISCAR provides these tools in the families of milling cutters for machining titanium and high temperature superalloys (HTSA).
Why are nozzles used as coolant outlets in HPC indexable milling cutters?

There are two reasons for using nozzles as coolant outlets: technological and applicative. HPC supply through the body of a cutter requires small-diameter outlets (as well as demands regarding the shape). As manufacture of the outlets via drilling hard steel tools would encounter technological difficulties, screw-in nozzles represent a more practical option.
If a depth of cut is smaller than the maximum cutting length of an indexable extended flute milling tool, there is no need to supply coolant to the inserts that are not involved in cutting. To improve performance, you can easy unscrew the appropriate nozzles from their holes, and then close the hole by a plug or a standard set screw.
Why are a significant number of HPC milling cutters special (tailor-made)?

The main consumers of HPC milling cutters are manufacturers working with hard-to-cut materials, for example titanium alloys. In many cases, producing parts from the materials requires a high volume of metal removal. To boost productivity, manufacturers often use unique machine tools, and, to reach maximum operational rigidity, they prefer integral tools with direct adaptation to the spindle of a machine - without intermediate tooling such as arbours or holders. Specific tool diameters, cutting lengths, and overhang, as well as adaptations that vary from one manufacturer to another, demand tailor-made HPC milling cutters.
Which families are included in ISCAR’s indexable milling line?

The indexable milling line consists of cutters intended for the main types of milling operations: milling right shoulders, milling open faces, milling edges (edging) and deep shoulders, milling 3-D surfaces (profile milling), milling slots and grooves, milling chamfers, etc. Separate families of cutters have been developed to handle fast feed milling (a specific machining technique).
The logos of various ISCAR’s indexable milling families start with the wording “HELI” (a derivative from “helix”), and phrases such as “helical cutting edge” and “helical milling” are often emphasized as benefits in technical information. Why?

In the early 1990’s, ISCAR introduced the HELIMILL – a family of milling tools carrying indexable inserts with a helical cutting edge. The highly effective edge was generated by the intersection of the shaped insert top (rake) face and the helical insert side (relief) surface. The design of the HELIMILL tools formed a constant positive rake and a constant relief along all cutting lengths. This feature immediately caused a significant reduction in power consumption and ensured a smooth cut. The HELIMILL heralded a new design approach that is considered today as the acknowledged format in indexable milling, and positioned the shaped surfaces of an insert into the forefront. The wording “HELI” reflects the helical cutting edge as a significant factor in the advancement of these indexable milling families.
Does ISCAR provide indexable milling cutters for machining aluminum?

Yes. ISCAR has developed an entire comprehensive range of indexable milling cutters, designed specifically for the efficient machining of aluminum. Each family of these high-quality cutters features integral or lightweight body designs, unique principles of carbide insert clamping, structures with adjustable cartridges, various ground and polished inserts with different corner radii and, most popular in aluminum machining, inserts with polycrystalline diamond (PCD) tips. The vast majority of the cutters have inner channels for coolant supply through the body. The ISCAR HELIALU line of indexable milling tools enables efficient high speed machining (HSM) of aluminum, ensuring powerful metal removal rates (MRR).
The term “high positive” is often used when speaking about indexable milling cutters. What does it mean?

Generally, this term relates to rake angles of an indexable milling cutter. Advances in powder metallurgy have resulted in the production of helical-cutting-edge inserts with a rake face that is “aggressively” inclined with respect to the insert cutting edge. This causes a significant increase in the positive rake angles (normal and axial) of a cutter carrying the inserts. The definition “high positive” emphasizes this feature. Note: This definition reflects the current state of the art. As the production of tools with cemented carbide inserts does not deplete its own resources, we may assume that the “high positive" of today will be considered as “normal” tomorrow.
Cemented carbide is a main cutting material for indexable inserts. ISCAR provides a rich variety of carbide grades. Where can I find basic information about the properties of a grade, recommended cutting speeds and application range?

ISCAR offers a range of electronic and printed catalogues to reference guides that contain this information and specify the structure of a grade (substrate type, coating), the application range in accordance with ISO standards and the range of cutting speeds. Contact ISCAR representatives in your region for details and assistance.
Do the indexable milling cutters have internal channels for coolant supply?

Most of the indexable milling cutters introduced recently feature an inner channel for coolant supply to each insert directly through the cutter body.
There are face shell mills that do not have these channels. If an internal coolant supply is necessary, how I can modify the mills?

In most cases, this modification is not needed. Instead, ISCAR proposes clamping screws with adjustable nozzles to provide a simple solution to the problem. The screws not only secure the shell mills on arbors but provide effective coolant supply directly in the cutting zone and improve chip evacuation. A nozzle, the movable part of the screw, allows easy adjustment of coolant supply depending on the depth of a mill countersink depth, insert sizes or application needs.
How I can guarantee applying correct torque for tightening clamping screws that secure inserts in the milling cutters?

In indexable milling lines, ISCAR provides two types of torque keys: with adjustable and fixed torque value. The first type allows the user to set torque within an available range, while the second type features a fixed torque value that is already preset. Information about which torque is necessary for tightening screws, which secure the inserts, can be found in catalogues, technical guides and leaflets. In addition, this data is now printed on the milling cutter body as a mark detail.
What is better for control productivity – varying the feed or the depth of cut within acceptable limits?

It should be noted that the question has no unambiguous answer and depends on several factors. However, in general, under the same MRR, increasing the feed coupled with reduced depth of cut is more favorable than the opposite combination (lesser feed with deeper cut) because it normally results in greater tool life.
How can I find a more efficient indexable milling cutter for my applications?

If you know the application parameters, ITA (ISCAR Tool Advisor), a computer-aided search engine, can be a very effective tool. This software is free and it may be installed even on your smartphone. If your question relates to more broad issues and considerations about selecting a suitable family of cutters, we have specific recommendations regarding priorities – please contact our representatives for assistance.
What is turn-milling?

Turn-milling is a process whereby a milling cutter machines a rotating workpiece. This method combines milling and turning techniques and has many advantages.
What are the advantages of turn-milling comparing with classical turning?
- In turning, machining non-continuous surfaces features interrupted cutting that results in unwanted impact load, poor surface finish and early tool wear. In turn-milling, the tool is a milling cutter that is intended exactly for interrupted cuts with cyclic load.
- When turning materials with long chips, chip disposal is difficult and identifying the correct chipbreaking geometry of a cutting tool is not simple. The milling cutter used in turn-milling generates a short chip that considerably improves swarf handling.
- In turning eccentric areas of rotating components (crankshafts, camshafts, etc.), off-center masses of the components cause unbalanced forces that adversely affect performance. Turn-milling with its low rotary velocity of a workpiece significantly diminishes and even prevents this negative effect.
- In turning, the rotation of heavy-weight parts, which defines the cutting speed, is limited by the characteristics of the main drive. If the drive does not allow rotation of large masses with required velocity, then the cutting speed will be far from the optimal range; and will resulut in low turning performance. Turn-milling provides a way to overcome the above difficulties effectively.
How I can calculate cutting data for turn-milling?

The calculation method is shown in the March 2017 issue of “Welcome to ISCAR’s World”, a collection of articles. The electronic version of the issue can be found also on ISCAR’s site catalogs. If necessary, please contact our local representatives in your area – they will be glad to help with this issue.
What is the difference between radial chip thinning and axial chip thinning?
Chip thinning refers to decreasing maximum chip thickness hmax compared to feed per tooth fz.
Two factors cause this decrease:
- Cutting geometry of a milling tool, specifically the tool cutting edge angle χr when it is less than 90° ("axial chip thinning"). Good examples of axial chip thinning are fast feed milling and machining 3-D surfaces at shallow depth of cut by ball nose or toroidal-shape milling tools.
- Influence of width of cut ae. If ae in peripheral milling and face milling is smaller than the radius of the milling tool, hmax becomes lower than fz. This effect is known as “radial chip thinning”. Understanding chip thinning is very important. Maintaining necessary chip thickness requires appropriate increase of feed per tooth and is a key element for correctly programmed fz.
What is a slab mill?

A slab mill is a type of a cylindrical (plain) milling cutter – a milling tool with helical cutting teeth on its cylindrical periphery. Slab mills generally feature large sizes and have a central bore for arbor mounting, mainly in horizontal milling machine tools. Slab mill length is considerably greater than its diameter. These mills are intended for machining an open surface (mostly plane) of a workpiece when the surface width is less than the mill length. Slab mills were very common in the past but today they are used quite rarely.
What is “roll-in entering” a machined workpiece in milling?

Roll-in entering (or, simply, rolling in) is a method of approaching a material in milling. In rolling in, a milling cutter enters the material by arc that causes a gradual growth of mechanical and thermal load on a cutting edge. This approach cut significantly contributes to machining stability and improves tool life. Rolling in is contrary to the traditional straight entering, when the load suddenly increases.
What are the advantages and disadvantages of clamping inserts in milling cutters by wedge?

The main advantages of clamping indexable inserts in a milling cutter by wedge are quick and easy insert replacement or changing a worn cutting edge of the insert (the insert indexing). Clamping by wedge is more common for indexable face mills, especially large-sized. These mills usually work in tough conditions and often become hot. Machine operators prefer the wedge clamping design for such mills.
However, the wedge, an additional part above the insert in the cutter structure, produces an obstacle for chip flow in the cutter chip gullet, which worsens chip evacuation and reduces cutter performance. This is a major disadvantage of wedge clamping. Intensive contact between the chips and the wedge results in the detrition wear of the latter and shortens its tool life.
How to estimate tool life for ceramic cutting tools?

Ceramic tools behave differently than carbide tools. In most cases, the end of a tool life is determined by the acceptable level of burrs and not by wear size.
What is a router?

In machining, the term "router" has several meanings. It may refer to a rotating tool for hollowing out ("routing") wood and plastic materials. "Router" refers also to a 3-axis CNC machine for cutting soft materials, such as wood, using a rotating tool. In metalworking, a "router" usually means an endmill, intended for milling aluminum at high cutting and feed speeds.
Flute or chip gullet?

In milling cutter terminology, both words designate a chip space or a chip pocket – the shaped area of a milling cutter body that is intended for the flow of chips that are formed as a result of cutting. This space must be sufficient to enable a free, unrestricted chip flow. The term "chip gullet" is generally used to specify the chip space of indexable milling cutters, whereas "flute" is mainly applied to a solid mill design, where it means a helical groove that ensures chip flow and produces a sharp cutting edge or a mill tooth by one of its edges.
Chip breaker or chip former?

A chip breaker is an area of a tool rake face that is specially shaped for breaking or controlling (forming) the produced chip. The term "chip breaker" is commonly used in turning operations, where breaking a long chip is one of the key success factors. In milling, the term "chip former" is generally used, as milling is an interrupted, "chip breaking" cutting process that focuses on chip forming.
Which depth of cut percentage is recommended with respect to the insert cutting edge length?

In process planning, depth of cut is defined depending on operation, machine tool characteristics, rigidity and other factors.
ISCAR catalogs specify the maximum depth of cut for each insert. Maximum depth of cut refers to the maximal length of the insert cutting edge that can machine.
This value must not be exceeded. In most cases, inserts are operated at cutting depths of no more than 2/3 of the specified maximum.
What is "chip load"?

The term "chip load" is often used as a synonym for the term "feed per tooth". This term is more common for the North American market. However, the correct synonym for "chip load" is "chip thickness". In shop talk "chip load" relates usually even to maximum chip thickness.
In North American countries the term "feed rate" is often used instead of the ISO definition "feed speed". While on this subject, manufacturers can refer to "feed speed" as "table feed". The original term "table feed" refers to a classical milling machine, from previous generations, where feed motion was created by movements of the machine table.
What is the difference between "wiper flat" and "wiper insert"?

A wiper flat is a small minor edge on a regular indexable insert in milling cutters to improve the quality of a machined surface. It is often referred to as a “wiper”.
A wiper insert is a specially designed insert where the wiper flat is significantly larger than for a standard insert. When mounted in a milling cutter, the wiper insert protrudes 0.05…0.07 mm axially relative to a regular insert. A wiper insert "smooths down" the machined surface, noticeably improving surface finish.
What is "stepover" and what is "stepdown"?

In multi-pass milling, "stepover" and "stepdown" refer to the distance between two adjacent passes. "Stepover" relates to this distance when, after finishing a pass, the milling cutter moves sideward and then performs the next pass. By contrast, if at the end of a pass the milling cutter moves downward to start the next part, the distance is called "stepdown". Sometimes "stepover" and "stepdown" are referred to as "sidestep" and "downstep" correspondingly although this is less common.
What is the difference between "gang milling" and "straddle milling"?

Straddle milling is a type of gang milling.
In gang milling, an assembled tool comprising two or more milling cutters mounted in the same arbor, machines several workpiece surfaces simultaneously. In straddle milling, two or more side-and-face milling cutters, mounted in one arbor, machine parallel planes of a workpiece. The planes are perpendicular to the arbor axis and feature an exact distance (distances) between them. To ensure the necessary accuracy of the distance (distances), the milling cutters are spaced apart with the use of bushings and spacers.
What is an "on-edge" insert?

This term is used sometimes as another name for a tangentially clamped insert. When mounted in a cutter, the insert is placed "edgeways" ("on -edge"), and the largest cross-section of the insert is under the working cutting edge.
What is the difference between rough milling and finish milling?

Rough milling focuses on high metal removal rates while finish milling assures precise accuracy on the milled surface.
As a rule, finish milling features significantly smaller machining allowances when compared with rough milling.
What are the main types of edge conditions for indexable inserts?

The cutting edge of an indexable insert may be sharp, rounded or chamfered. These are the basic types of edge conditions, also referred to as "edge preparation".
In addition to the above, there are combined edge conditions such as chamfered and rounded, double-chamfered, and double-chamfered and rounded.
A rounded edge can also be referred to as a "honed edge".
What are the advantages and disadvantages of wedge clamping indexable inserts?

The wedge clamping principle, which is an alternative to a screw clamping concept, provides a more durable insert structure; there is no need for a central bore. A wedge clamp ensures quick and easy indexing and is very important when the insert is extremely hot due to heavy machining conditions.
The wedge clamping method is most suitable for machining materials that produce short chips (i.e., cast iron).
When should I replace insert clamping screws that secure indexable inserts in the body of a milling cutter?

An insert clamping screw requires thorough visual examination before using a milling cutter. The threads and head of the screw, as well as the socket for a key, should all be in good operating condition, and therefore, demand special attention. If these screw elements are damaged, or the screw is bent, the screw must be replaced immediately.
When tightening a screw, apply the correct tightening torque and use the right key to prolong the wear life of the screw. Also, do not forget ISCAR’s recommendations for the application of an anti-seize lubricant when replacing an insert or its indexing. Following these obvious, but sometimes forgotten rules will increase the screw life.
How to determine when to replace an insert (change its cutting edge), a solid tool or an exchangeable head?
The correct answers are: At the end of the tool life or upon reaching the wear limit. The life period of a tool or the wear limit for a cutting tool depends on various designs, operational and administrative factors.
At the same time, during a machining operation, there are certain signs that can indicate the need to replace inserts, tools, or heads.
- Noticeable increase of power consumption (spindle load)
- Increased vibration and noise
- Worsening of machining accuracy and a need for frequent additional tool dimensional adjusting
- Reduced surface finish
- Occurred burrs
- A visual inspection of a cutting edge shows considerable flank wear, extensive edge chipping, cracks etc.
For more detailed data on how to define a tool’s life in a specific case, we recommend contacting an ISCAR technical representative.
What is the principal difference between a "triangular" and "trigon" indexable insert?

To be exact, both triangular and trigon relate to the same shape of a polygon – a triangle. A triangular insert features a triangular shape. In a trigon insert, the side of a polygon comprises two-line segments that have the same length and form an obtuse angle.
From a geometrical point of view, a convex isotoxal hexagon is an accurate definition for the trigon insert shape. Under certain assumptions, this shape may also be referred to as a truncated triangle. However, neither of these names are commonly used, instead, trigon is the most known term today.
To conclude: the trigon shape of an indexable insert relates to the form of a convex isotoxal hexagon.
What is the main design feature of a TANGFIN indexable face mill for superb finish of a machined surface?

A TANGFIN face mill is based on a step-cutter-concept: the inserts are positioned in gradual locations on the mill in both radial and axial directions. This design causes each insert to cut only a small portion of the material in both radial and axial directions. The high surface quality is attained thanks to a very rigid clamping of the inserts together with the long and straight insert minor cutting edges. A final surface texture is provided by the axially protruding insert that serves as a wiper insert.
Hence, the combination of the step-cutter robust design and the long wiper cutting edge, which is produced by the axially protruding insert, results in impressive surface finish parameters.
Within its range of products, ISCAR has a few families of small-sized milling cutters carrying miniature indexable inserts. What is the main field of their application, and what advantages can these cutters provide?

These families feature a diameter range that is traditionally connected with solid carbide endmills. However, in milling with shallow depths of cut, only a part of the cutting length is used, which makes applying a solid carbide endmill inefficient in many cases, especially in rough machining operations. In contrast, cutters with miniature indexable inserts are not only intended for such applications but ensure rational utilization of cemented carbide due to the indexing capability of an insert. Hence, the small-sized indexable milling cutters provide a reasonable, cost-effective alternative to solid carbide endmills, mostly in rough cuts.
What is the difference between semi-roughing and semi-finishing in milling?

The difference can be blurred and may often be considered synonyms. However, in some cases when milling a surface requires more than one operation, these operations are specified as rough milling, semi-rough milling, semi finish milling, finish milling, fine milling or simply roughing, semi roughing, semi finishing, finishing.
Incidentally, the same situation may be observed not only in milling but also in other types of machining, such as turning.
What is an integral collet?

Generally, an integral collet is a tool with a tapered shank for direct mounting in ER collet chucks. When compared to a typical spring collet clamp, the integral collet provides better accuracy and higher rigidity.
Do ISCAR's integral collets have internal coolant channels?

In general, yes, for example, ISCAR's integral collet families with MULTI-MASTER adaptation.
What is abreast milling?

Abreast milling is the method of simultaneous milling of several parts that are positioned in a row parallel to the milling cutter axis.
What is the pitch of a milling tool?

The pitch is the distance between the two nearest-neighboring teeth of a milling tool measured between the same points of the teeth's cutting edges. The pitch shows the tooth density of a tool, in accordance with the milling tools which differ from the tools with a coarse, fine, and extra fine pitch. Parallel to coarse-fine-extra fine pitch rating, alternative grading such as: coarse-regular-fine, normal-close-extra close and others, exists. In addition, extra-fine pitch tools are also referred to as high-density cutters.
What is the main application of indexable shell mills with a titanium body?

Titanium-body indexable shell mills are intended mostly for long-reach machining applications. To improve results and to achieve an excellent surface finish, it is recommended to mount the milling cutter on tool holders with an anti-vibration mechanism, such ISCAR's WHISPER LINE adaptors.
Which factors should be considered when determining the feed speed for milling by use of interpolation?

When determining the feed for milling by interpolation, it is important to consider that the feed speeds (feed rates) of the cutting edge and the mill axis are different. This is unlike straight-line milling. In milling by use of helical and circular interpolation, the programmed feed speed in most CNC machines refers specifically to the axis of the cutter. When milling inside surfaces by interpolation, the feed speed of the mill axis is slower than that of the cutting edge. Conversely, when milling outside surfaces by interpolation, the feed speed of the mill axis is faster than that of the cutting edge. It is necessary to consider the above difference in feed speeds when setting the cutting data.
What is a "no mismatch" 90°-indexable milling tool?

In machining square shoulders, the height of the shoulder can exceed the maximum depth of cut that is determined by the cutting length of an indexable insert mounted on a given tool. In such cases, multiple passes are required for shoulder milling. "No mismatch" refers to the ability of a precise indexable milling tool to ensure a true 90° shoulder profile without a noticeable border, step, or burr between the passes. This feature is essential for accurate square shoulder milling.
What is string milling?

String milling is the milling method where a mill sequentially machines several workpieces that are arranged closely in the feed direction, resembling a string.
What is a sprocket cutter?

A sprocket cutter is a type of form milling cutter specifically designed for machining sprockets of roller chain wheels. It may also be referred to as a sprocket-wheel cutter or chain sprocket cutter.
What is a step milling cutter?

A step milling cutter is a type of mill with teeth that are equally displaced relative to each other in either the axial or radial direction. If the teeth are used by use of indexable inserts, the cutter is referred to as an indexable step milling cutter.

Profile Milling

What is the difference between profile milling, milling contoured surfaces and form milling?

Generally, these definitions mean the same thing and relate to milling 3-D surfaces. Such kind of machining is often named in shop talk as simply profiling.
Which industrial sectors are characterized by a great number of profile milling operations?

First, it is the Die and Mold industry, then Aerospace but almost every branch requires profile milling tools in a varying degree, too.
Which types of tools are the most popular for profile milling?

In rough milling for “pre-shaping” further 3-D surfaces, process planners use different tools and even general-duty 90° milling cutters. Fast Feed milling cutters* are very efficient means for high-efficiency roughing. However, most of profile milling operations relate to toroidal and ball nose milling cutters because they ensure correct generation of a needed shape in every direction.

* refer to the appropriate section in FAQ session
Are inserts with chip splitting action in ISCAR’s profile milling products?

Yes. Moreover, exactly from MILLSHRED, a family of indexable milling cutters with round inserts, the serrated cutting edge of ISCAR milling inserts was started its way.
What is the effective cutting diameter of a profile milling tool?

In profile milling, due to the shaped, non-straight form of the tool, a cutting diameter is a function of a depth of cut; and it is not the same for different areas of the tool cutting edge that is involved in milling. The effective diameter is the largest true cutting diameter: maximum of the cutting diameters of these areas. In calculating cutting data, it is very important to consider the effective diameter, because the real cutting speed relates to the effective diameter, while the spindle speed refers to the nominal diameter of a tool.
Which types of profile milling tools ISCAR provides?
ISCAR line of profile milling tools comprises Fast Feed*, toroidal, and ball nose cutters in the following design configurations:
- tools with indexable inserts
- solid carbide endmills
- replaceable milling heads with MULTI-MASTER* adaptation
* refer to the appropriate section in FAQ session
What is restmilling?

Productive milling proposes applying more durable and rigid tools for high metal removal rate. In many cases the form and the dimensions of the tools do not allow for a cut in some area; for example, the corners of a die cavity. The remainder of the material in the areas is removed by restmilling – a method under a technological process where a tool of smaller diameter cuts the areas with residual stock.
Does ISCAR recommend the use of “plungers” for profile milling?

Yes, in cases of large overhang we recommend the use of cutters/plungers on the Z axis, as this will result in a more productive milling operation with less vibration in profiling/roughing. The depth of cut for plungers with overhang is higher than ap for conventional systems, obtaining a higher metal removal rate. ISCAR offers a variety of plungers and, to achieve important lengths, we recommend use of the ITS modular system.
What is ISCAR's "rule of 12" for ball nose cutters?

"The rule of 12" is a rule of thumb that may be useful for quick estimation of the relation between a depth of cut and a width of cut (a stepover) when milling ISO P materials (soft and pre-hardened steel, ferritic and martensitic stainless steel) by ball nose cutters. In accordance with the rule, if a depth of cut is the half of a cutter diameter (D/2), a recommended width of cut (a stepover) should be no more than D/6; for the depth of cut D/3 the maximal width of cut should be D/4 etc.
It is not difficult to see that 2×6=3×4=12.
In face milling, a recommended width of cut is often given as a ratio to a tool diameter. When using a mill with round inserts, which tool diameter should I consider?

The correct way to decide is by calculating the width of cut with the effective diameter of the mill with round inserts – the largest of the tool diameters that’s involved in cutting.
This diameter is a function of the depth of cut, or by using the cutting diameter of a face mill for such a calculation. In accordance with standard ISO 6462, the cutting diameter is defined by the point that is produced by the intersection of the major cutting edge and the machined plane. This is the smallest tool diameter involved in cutting, while the cutting diameter is one of the main milling dimensions. This is also specified in the ISCAR catalog.
Here are some rules for quick estimating the cutting diameter:
If a face mill carries an even number of round inserts, the cutting diameter may be considered accurate enough as the distance between the centers of two opposite inserts. In other words, it is the mill’s maximum diameter minus the insert diameter.
If the cutter has an uneven number of inserts, the cutting diameter is approximately equal to the doubled distance from the mill axis to an insert center.
Using the maximum mill diameter as a base for calculating the width of cut is acceptable only when the depth of cut is close to the insert radius. In any other case, this calculation may cause intensive insert wear.
What is a form milling cutter?

A form milling cutter is a general name for milling cutters that are intended for generating curve-based (complex) surfaces.
What is ISCAR's product range for barrel-shaped (circle segment) milling cutters?

ISCAR's barrel-shaped milling cutter products comprise solid carbide endmills, MULTI-MASTER exchangeable carbide heads, and single-insert indexable endmills. According to the cutting profile, the shape of these cutters can be divided into pure barrel, oval, tapered, lens, and combined.

Solid Endmills

Does ISCAR provide solid carbide endmills for machining all groups of engineering materials?

ISCAR’s SOLIDMILL line consists of various families of solid carbide endmills that are intended for machining different materials: steel, stainless steel, cast iron, etc. The line offers a rich variety of tools covering all application groups under ISO classifications P, M, K, N, S and H.
Which types of solid carbide endmills does ISCAR offer as standard products?

ISCAR’s standard solid carbide endmill products include 90° endmills, ball nose cutters, and tools for high feed (fast feed) milling, chamfering, and deburring. ISCAR also offers families of endmills designed specifically for high speed machining that apply trochoidal milling techniques.
What are the advantages of the trochoidal milling method?

Usually, trochoidal milling is applied to machining slots and pockets. In trochoidal milling, a fast-rotating tool moves along an arc and “slices” a thin but wide layer of material. When the layer is removed, the cutter advances deeper into the material radially and then repeats the slicing. This method ensures uniform tool engagement and stable average chip thickness. The tool experiences constant load, causing uniform wear and predictable tool life. The small thickness of sliced material significantly reduces heat impact on the tool and ensures an increase in the number of tool teeth. This method results in a very high metal removal rate with considerably decreased power consumption and improved tool life.
What is a "trochoid"?

"Trochoid", or "trochoidal curve", is a general name for a curve described by a fixed point on a circle as it rolls along a straight line or curves without slipping.
What is the secret of CHATTERFREE geometry?

CHATTERFREE represents a design utilized in several ISCAR solid carbide endmill families. The main CHATTERFREE features are unequal angular pitch of cutter teeth and variable helix angle. This concept results in substantially reducing or even eliminating vibrations during cutting, which significantly improves performance and tool life.
What is a variable helix?

The term "variable helix" refers to the helix angle in vibration-free designs of solid carbide endmills (SCEM), as are found in ISCAR CHATTERFREE products. A typical SCEM features helical teeth and the helix angle determines the cutting edge inclination of a tooth. In traditionally designed endmills, the helix angle is the same for all flutes, but it varies in vibration-free configurations.
The term “variable helix” is commonly understood to represent two design features: 1) Combining flutes with unequal helix angles where the angles are constant along every flute.
2) Helix angle varies along the flute.
However, the term “variable helix” is correct only in relation to design feature 2 and the term “different helix” should be used to specify design feature 1.
Why are FINISHRED endmills often referred to as “Two in One”?

FINISHRED endmills feature four flutes, two serrated teeth and two continuous teeth. This facilitates the integration of two cutting geometries into a single tool: rough (serrated teeth with chip splitting action) and finish (continuous teeth), so gaining the “two in one” appellation. By running at rough machining parameters, semi-finish or even finish surface quality can be achieved. One such tool can replace two rough and finish endmills, reducing cutting time and power consumption while increasing productivity.
Does ISCAR provide instructions for regrinding solid carbide endmills?

Yes. All catalogues, as well as relevant technical leaflets and brochures, contain instructions for regrinding solid carbide endmills, and ISCAR local representatives are available to advise on this issue.
What is a length series?

Solid carbide endmills of the same type and the same diameter often vary in overall length within a family. According to the length gradation, there are short, medium and long series. Additional series such as extra-short or extra-long can also be applied. As a general rule, short-length endmills ensure highest strength and rigidity whereas extra-long solid carbide endmills are intended for long-reach applications.
What is a slot drill?

“Slot drill” is a name of an endmill that can cut straight down. Slot drills have at least one center cutting tooth and are used mainly to form key slots. Slot drills are typically two-flute mills, but they can have three and even four flutes.
ISCAR ball nose solid carbide endmills have two or four flutes (teeth). How should the correct number of flutes for a ball nose endmill be chosen?

The all-purpose four flute ball nose solid carbide endmills provide a universal and robust production solution for various applications, especially for semi-finish and finish operations. Two flute endmills have a larger chip gullet, which makes them more suitable for rough machining as they ensure better chip evacuation. Two flute tools are also considered to be a workable method for fine finishing due to a lower accumulated error, which depends on the number of teeth. When milling with shallow depth of cut, calculating feed per tooth should take into consideration only 2 effective teeth; as the advantages of a multi-flute design are diminished.
Does the ISCAR solid carbide endmill line include miniature endmills?

ISCAR solid carbide endmill lines include endmills with diameters of tenths of mm. For example, the standard ball nose endmills, which are intended for processing ribs for hard materials, start from a minimal diameter of 0.1 mm.
Does ISCAR produce solid ceramic endmills? Where is their application most effective?

ISCAR's product range includes a family of solid ceramic endmills. They are mainly applied to machining high temperature superalloys, heat resistant stainless steel, cast iron and graphite.
What are the applications for ISCAR's lens- and oval-shape solid carbide endmills and MULTI-MASTER exchangeable heads? (Related to MULTI-MASTER - 466)

The lens- and oval-shape solid carbide endmills and MULTI-MASTER exchangeable heads are designed for 5-axis semi-finish and finish milling complex surfaces, especially in aerospace, medical and die & mold industries.
Is it possible to regrind ISCAR's lens- and oval-shape solid carbide endmills?

The lens- and oval-shape solid carbide endmills features a complicated cutting shape and therefore they are not intended for regrinding.

MULTI-MASTER

How is a head mounted into a shank?

A head has two surfaces: a short taper and a rear non-cutting face that determines the head location in a shank. The taper ensures high concentricity and the face – a face contact. The thread is intended for securing the head. Therefore the rear (tail) part of the head has two areas: tapered and threaded.
During mounting, the head is initially rotated by hand and then is tightened by means of a key. The head has flats for applying a key.
What are the advantages of the face contact?

First of all, the face contact considerably increases the stiffness of an assembled tool comprising a shank and a head and its ability to withstand impact loading so common in milling. This factor allows for stable cutting, minimizes vibrations, and reduces power consumption.
Secondly, the face contact ensures high repeatability of the head overhang with respect to the shank. As a result, there is no need for an additional adjustment after replacing the head - no setup time – and an operator can change the head without removing the shank from a machine tool spindle.
What does “the initial gap” mean?

When tightening a head, an operator starts by rotating the head by hand. The head then stops at some point and a small gap remains between the contact faces of the head and the shank. From this moment, further head tightening is possible only with the use of the key. Tightening of the head causes elastic deformation of the adjoining contact area of the shank section, in a radial direction. The above-mentioned gap is called "initial" and it is an important feature of the MULTI-MASTER connection. The gap value is several tenths of a millimeter, depending on the thread size.
Why does the MULTI-MASTER thread have a special profile?

The MULTI-MASTER heads are produced from tungsten carbide. Although this is an extremely hard and heat-resistant material, it has lowered impact strength against, for example, high speed steel (HSS). Therefore, in designing a threaded tungsten carbide part, minimizing stress concentrators is one of the main problems to be solved.
Additionally, the MULTI-MASTER thread connection has relatively small dimensions: the nominal diameters of the threads lay approximately within 4-15 mm. These sizes and the necessity to meet the strength requirements for the operational loads, can possibly limit the height of the thread profile.
The above points make it problematic to use the standard threads and strongly dictate a special thread shape that will comply with specifications of the connection. That is why ISCAR designed the special-profile thread, which has been designated as “T-thread”.
What types of MULTI-MASTER heads does ISCAR offer?
- End milling heads of various shapes – 90°, 45°, 60°, etc.
- Profile milling heads having ball nose, toroidal, concave radii and other shapes
- Heads for high-feed milling
- Slot and groove milling heads for milling grooves for retaining or O-rings, T-slots, etc.
- Thread milling heads
- Center and spot drilling heads
- Engraving heads
The milling heads have various numbers of teeth (flutes), helix angles, and degrees of accuracy, as well as cutting geometry for effective machining of various engineering materials.
What is an economy-type end milling head?

There are two types of MULTI-MASTER end milling heads.
The first type of MULTI-MASTER end milling head is the same as the ISCAR standard solid carbide endmills but differs in overall and cutting edge lengths. A major advantage of this type of end milling heads is that there is a large variety to choose from (practically all the standard line of the solid mills). In finishing and milling hard materials, increasing the number of flutes makes cutting more stable and productive. The heads of the first type are produced from stepped cylindrical blanks by grinding.
The second type of MULTI-MASTER end milling heads is the economy version; it is shaped beforehand by pressing and sintering with a small oversize. Further grinding defines the final shape of a head and its accuracy. The heads of this type have a high-strength tooth that makes it possible to substantially increase the feed per tooth in comparison with the heads of the first type. Pressing technology enables production of different complicated shapes; although making these from the stepped blanks is problematic. The economy-type heads have only two teeth.
Why do the MULTI-MASTER keys have two openings?

Due to the design features of the heads, one of the openings, similar to openings of ordinary engineering wrenches, is intended for the multi-flute heads of the first type of MULTI-MASTER end milling head (see above) and the appropriate cylindrical blanks. The second shaped opening is designed for the economy-type heads.
Does the MULTI-MASTER family include hole making tools?

The Multi-Master family includes heads with a point angle of 60°, 80°, 90°, 100°, 120° and 145 unintended for chamfering only. The heads are suitable for spot drilling, countersinking supplemented by center drilling heads.
Is a center drilling head that is made from solid carbide, really a reasonable solution? There are various low-cost double-sided standard combined center drills and countersinks produced from HSS.

When compared to the above-mentioned HSS combined drills and countersinks, the center drilling heads allow for a considerable increase in tool life. The heads are operated under higher cutting data and thus lead to higher productivity. Therefore, we advise checking the current production cost and then making a decision, taking all relevant factors into account.
What is the accuracy of the heads?

The nominal diameter of the normal accuracy end milling heads has the following tolerance limits: e8 for multi-flute heads produced from blanks and h9 for the economy- type heads. The precise heads for finish profiling are made with tolerance limits for diameter h7 and the heads for milling aluminum – h6. The diametric tolerance for the cylindrical cutting area of the heads for chamfering, spot drilling and countersinking is h10.
What is the repeatability tolerance of MULTI-MASTER heads?

As mentioned in the answer to question 2, one of the main advantages of the face contact is high repeatability, which ensures closed tolerance for the head overhang with respect to the contact face of a shank. The overhang limits are ±0.01 mm for the majority of the end milling heads.
Does ISCAR offer MULTI-MASTER heads intended for milling hardened steel?

Yes. These heads are made from a high-strength and wear-resistant submicron carbide grade; and they have tight dimensional tolerances.
What are the main types of shanks and for which purpose should they be used?

The shanks are available in different versions: smooth cylindrical and with a neck. The neck can be straight or conical.
The smooth shanks and the shanks with a straight neck, called Type A shanks in MULTI-MASTER’s designation system, are general purpose shanks and are used for a variety of applications. There is also a reinforced version, intended mainly for milling keyways or high-feed milling (HFM). It is distinguished by flats on a shank body that make it suitable for clamping in Weldon-type adapters.
Type B is a reinforced shank with a relatively short conical neck which has a taper angle of 5° on the side. It is characterized by increased strength of the durable body that defines its main application: heavy-duty machining.
For long-reach machining at high overhang, the Type D shank with a long conical neck can offer a good solution. It has a taper angle of 1° on the side and is designed primarily for milling deep pockets and cavities, high steep walls, etc. This shank should not be used in heavy-load conditions.
For short-reach applications, the MULTI-MASTER family offers shanks with a collet adaptation. These are mounted directly into a collet chuck instead of the spring collet. The direct mounting increases rigidity and accuracy, and reduces the overall overhang relative to the datum face of a machine tool spindle.
The MULTI-MASTER family also includes smooth steel cylindrical shanks of considerable overall length (at least 10 diameters of the shank). These are intended primarily for producing specially tailored tools of various configurations by additional machining of the shanks in order to form the required shape. Such machining can be performed even directly by the customer. In fact, they are the blanks with an internal T-thread. For the convenience of additional machining operations (turning, sometimes external grinding, etc.), the shanks are provided with a center hole in the rear face.
The MULTI-MASTER family contains a variety of extensions and reducers for connecting with other ISCAR systems of modular tooling (for example, FLEXFIT).
From what materials are the shanks made? How should the correct material be chosen?

The shanks are produced from the following materials: steel, tungsten carbide and heavy metal (an alloy containing 90% and more of tungsten).
In the context of functionality, a steel shank is the most versatile. Due to the considerable stiffness of tungsten carbide, a carbide shank is intended primarily for finishing and semi-finishing, machining at high overhang and milling internal circumferential grooves. In case of unstable cutting, applying a heavy metal shank can give good results because of the vibration-proof properties of heavy metal. However, heavy metal shanks are not recommended for heavy-duty machining.
Are the MULTI-MASTER tools suitable for coolant supply directly through the tool body?

Yes, there is a design of the shanks with holes for internal coolant supply.
Can the MULTI-MASTER shanks be held in heat shrink chucks and collets?

The carbide or heavy metal shanks are suitable for toolholding by the heat shrink method. As for the steel shanks, clamping them into heat shrink chucks and collets is not recommended.
Is it necessary to lubricate T-threads when mounting the heads into a shank?

No. Do not apply lubricants to the MULTI-MASTER T-thread connection!
Are the MULTI-MASTER connection design and thread compatible with other tool brands?

No. ISCAR’s unique design is patented and other systems that appeared later are not compatible.
Does ISCAR provide blank MULTI-MASTER heads that are intended for final forming by the customer?

The MULTI-MASTER family includes semi-finished uncoated carbide blank heads, designed for manufacturing various special cutting profiles by additional grinding at customer facilities. The blank heads have a T-thread for MULTI-MASTER adaptation and a cylindrical portion intended for grinding by the customer.
Does ISCAR provide a key with adjustable tightening torque for MULTI-MASTER heads?

Yes. The MULTI-MASTER product range includes an assembled key, comprising an adjustable torque handle with a set of interchangeable wrenches and TORX-tipped bits, designed for secure and accurate tightening of MULTI-MASTER heads. This key is an optional product and should be ordered separately.
What are the applications for ISCAR's lens- and oval-shape solid carbide endmills and MULTI-MASTER exchangeable heads?

The lens- and oval-shape solid carbide endmills and MULTI-MASTER exchangeable heads are designed for 5-axis semi-finish and finish milling complex surfaces, especially in aerospace, medical and die & mold industries.
What is the maximum rotational velocity for a MULTI-MASTER milling tool?

A MULTI-MASTER tool is an assembly comprising of a shank and an exchangeable milling head. The maximum rotational velocity values (in rpm) for each shank can be found in ISCAR’s catalogs and guides. To estimate the maximum rotational velocity for an assembly when a specific milling head is attached to a shank, the maximum rpm value (taken from the catalog) should be divided by the number of flutes of the milling head.
Apart from keeping the maximum rotational velocity restriction, the entire tool assembly (milling head, shank, and adapter/tool holder) must be properly balanced.
Which of the MULTI-MASTER milling heads are considered long-flute?

Usually, these are the heads where the length of a cutting edge is at least half as much as the head diameter.
There is a variety of Multi-Master heads MM HCD for chamfering, countersinking, and spot drilling that have different point angles. What is the reason for this variety?

In the Multi-Master standard product line, heads MM HCD have a point angle of 60°, 80°, 90°, 100° and 120°. Such a variety relates mainly to the requirements of different standards for chamfers and countersinks for fasteners. For example, metric countersunk screws require a 90° countersink, but American National countersunk screws require 80° and aerospace rivets 100°. A typical chamfer features a 45° chamfer angle, although, 30° and 60° chamfers are also common. This multiformity of required generated profiles defines the functional capabilities of the heads and explains their variety.
What is the main field of application for the ISCAR MULTI-MASTER exchangeable flat bottom drilling head?

The application range of these heads is not limited to making relatively short holes with a flat bottom (in-depth of up to 1.2 of the hole diameter). The MULTI-MASTER exchangeable flat bottom drilling head ensures efficient drilling on slanted and curved surfaces, directly on solid material without center- or pre-drilling, making it possible to produce half holes, counterboring and spot facing.
Is it necessary to reduce the feed rate when drilling slanted surfaces with the MULTI-MASTER exchangeable flat bottom drilling head?

Yes. When drilling slanted surfaces, the feed rate should be adjusted according to the angle of a surface inclination as recommended in the corresponding ISCAR guides. It can be roughly estimated that the feed reduction is 30-50% of a common value, depending on the angle of inclination.
Does ISCAR produce MULTI-MASTER tools for direct mounting onto a machine spindle?

Yes, ISCAR produces MULTI-MASTER tools with tapered shanks for mounting in spindles with various adaptations. For example: 7:24 taper (DIN 69871), HSK taper (DIN 69893), polygonal taper (ISO 26623-1) etc.

Fast Feed Milling

For which type of fast feed milling cutters does ISCAR manufacture tools?

ISCAR’s line of fast feed milling cutters comprises tools carrying indexable inserts, Multi-Master tools and solid carbide end mills.
Which milling operation is more effective for applying FF milling cutters?

The most effective applications for FF milling cutters are rough milling planes, pockets and cavities.
What is the meaning of the “Triple F” or "FFF" that is often mentioned in ISCAR technical editions and presentations?

"FFF" refers to fast feed face milling or fast feed facing. Rough milling planes is one of most the efficient and widespread applications for FF cutters. The operation usually relates to face milling, so the FFF acronym refers usually to fast feed face milling. FFF can also mean fast feed facing, as milling plane operations are often known as facing.
Fast feed milling is considered as a high-efficiency metal removal technique when machined workpieces are made from steel or cast iron. Can FF milling cutters be applied to machining difficult-to-cut materials like titanium or high temperature alloys?

FF milling cutters may be used in machining difficult-to-cut materials. The cutting geometry in this case differs from the geometry of general-duty FF milling tools that are intended for steel and cast iron. In addition, feed per tooth is significantly smaller compared to machining steel and cast iron; however it is much higher than the feed values that are recommended for traditional methods.
What are MF milling tools?

MF means “moderate feed”: moderate comparing with “fast” in FF milling but faster than the standard in traditional milling. The MF method is intended for increasing productivity when using slow high-power machines, milling heavy workpieces, etc.
The LOGIQ campaign introduced new families of indexable FF milling cutters with a diameter range typically covered by solid carbide endmills. Can these new cutters successfully compete with the solid carbide design concept?

Yes. The design of the cutters ensures a multi-teeth tool configuration. Let’s consider the NAN3FEED mill family as an example. They have 2 and 3 teeth for nominal diameters 8 and 10 mm (.315 and .394”) correspondingly. In a cutter carrying replaceable inserts, only the insert - a small part of the cutter - is made from cemented carbide. This means that the indexable design consumes far less of this expensive material than a solid carbide solution. The NAN3FEED insert with its 3 cutting edges ensures triple edge indexing, which is also cost-effectiveness. As the insert is small, it is placed simply in a pocket via a key with a magnetic boss on the key handle. The economical efficiency and ease of use make the family competitive with solid carbide tools.
Are fast feed cutters recommended for milling operations in turning or multi-task machines?

Yes. In general, these are small to medium diameter cutters and the turning operation is fast. The use of fast feed cutters results in improving the milling operation, reducing the machining time and minimizing damages to the machine head. MULTI-MASTER is an excellent option for turn-milling machines.
What is a radius for programming in fast feed milling cutters?

In CNC programming, a fast feed cutter is often specified as a 90°mill with a corner radius. This imaginary radius, which is called as "radius for programming", is an important data because it defines the maximal thickness of a cusp (scallop) and deviations from the theoretical profile of a surface that is generated by such a specification.
ISCAR has a wide range of high feed (fast feed) milling cutters. How can I select an optimal milling cutter for my application?

Basic information about ISCAR's high feed (fast feed) milling cutters, and recommendations for their selection, can be found in the Fast Feed Milling Quick Tool Selector Guide; available in both electronic (ISCAR website) and printed versions. If the question refers to a specific application with known details, an optimal solution can be found in the ITA (Iscar Tool Advisor) online software application.

High Speed Machining (HSM)

What does the term "high speed machining" mean?
Often HSM is emphasized as "a high-efficiency method of modern machining with high spindle and feed speed". High speed machining may refer to:
- High cutting speed machining
- High spindle speed machining
- High feed speed machining
These three speeds are interrelated. Increasing spindle speed automatically results in increasing feed speed as well, and likewise higher cutting speed requires a correspondingly higher spindle speed. As cutting speed varies in direct proportion to the diameter of a rotating tool, for tools of different diameters, different spindle speeds are required to ensure that the cutting speed is identical. A cutting speed is also a function of several factors, where a workpiece material and a cutting tool material are dominant. Depending on the cutting tool material, the recommended cutting speed for the same workpiece material may be quite different. A good example of this is machining nickel-base high temperature alloys by cemented carbide and whisker ceramic tools. At the same time, in machining aluminum, for instance, "normal" cutting speeds are significantly higher than in machining the high-temperature alloys.
The term "high speed machining" usually relates to high speed milling, which is a milling method that is characterized by shallow, light cuts combined with high spindle speed.
Is the cutting speed extremely high in high speed machining?

Not always. Let's examine one example. Assume that we machine a material with the use of a ball nose milling cutter of 4 mm in diameter while the depth of cut is 0.1 mm. The effective diameter in this case will be 1.25 mm. If the cutting speed as 60 m/min is required, the cutter should rotate at 15280 rpm. If the cutting speed will be 100 m/min, the rotational speed of the cutter will increase up to 25465 rpm! High speed machining does not automatically mean that the cutting speed is high.
Is it correct that a machine tool intended for high speed machining must have a high speed main drive?

Yes, but not only. As rotational speeds and feed speeds are interrelated, the machine tool should also feature a high speed feed drive. Furthermore, the machine tool must have appropriate fast control systems, high rigidity and many other design features, to make it suitable for high speed machining.
Can high speed machining be applied to machining hard steel?

Yes. In machining hard steel – which are difficult-to-cut materials – intensive heat generation and vibration take place. This is a source of poor tool life, reduction of accuracy, loss of stability etc. that makes machining operations unpredictable. High speed machining with its shallow cuts produces much lower cutting forces and heat, and therefore can solve these issues.
Why is high speed machining becoming more and more popular in rough machining operations?

Technological advances, especially in producing workpieces that are half-finished products, place special emphasis on high speed machining. Methods such as precise casting, metal injection molding, and 3D printing ensure that the production of workpieces is very close to the final shape of a part. As a result, the need to remove a high volume of materials by means of traditional rough cutting decreases. As high speed machining features low stock removal, it offers a precise method of producing workpieces.
How does trochoidal milling relate to high speed machining?

In trochoidal milling, a fast-rotating tool moves along an arc and “slices” a thin but wide layer of material. This milling method features small widths (or radial depths) of cut and high speed rotation of the tool and may be considered as a high speed machining technique.
Does ISCAR provide information about maximum rotational velocities for milling cutters?

Yes. This information can be found in catalogues, guides, leaflets and other technical documentations. In many cases, the maximum rotational velocity permitted for indexable milling cutters is marked directly on a cutter body.
Should a high-speed machining (HSM) tool and toolholder assembly be balanced?

The answer is yes. Typically, a tool is mounted on a toolholder and the toolholder is fitted into the spindle of a high-speed machine.
In high-speed milling, the dynamic characteristics of a tool cannot be separated from a toolholder and particular focus must be given to the assembly of the tool and toolholder.
What is peel milling?

Generally, peel milling relates to a milling method based on the combination of a large depth of cut with a small radial engagement of a milling cutter. Trochoidal milling can be considered a particular part of the peel milling process, and both peel milling and trochoidal milling are often used alike.

Milling Slots and Grooves

Which tools are used for milling slots?

Generally speaking, milling tools of different types – side milling cutters, endmills, extended flite (long-edge) milling cutters and even face mills – are suitable for milling slots and grooves. However, only the side milling cutters with teeth on face and periphery are designed especially for machining slots and grooves, while the others are intended for various milling operations. ISCAR’s line of slot milling tools comprises the side milling cutters.
What is the difference between “slot” and “groove”?

The words “slot” and “groove” are often synonymous. But if “slot” usually relates to a narrow, comparatively long, mainly longitudinal opening that is usually open-ended (at least from one side); “groove”, as a rule, means a circular (called “undercut”) or helical channel. It is been said that “a slot is an open-ended groove”.
Slot milling tools are often referenced as slotting tools. Is this correct?

The word “slotting”, commonly known as “slot milling”, is widespread in shop talk but the two actions are not identical or interchangeable. Slotting refers specifically to a stage in planning or shaping – a machining process where a single-point cutting tool moves linearly and piston wise, and a workpiece is fixed or moves only linearly concurrent with the tool.
Why are slot milling cutters called side and face milling cutters?

A slot milling cutter has teeth on its face and periphery, and features a cutting face and sides for the simultaneous machining of three surfaces: the bottom and the two sidewalls of a slot.
What are the main types of slot milling cutters?

The slot milling cutters differ in their adaptation (mounting methods). They have either arbor hole or shank-type configurations or, alternatively, interchangeable cutting heads for modularly assembled tools.
What is ISCAR’s program for slot milling cutters?

ISCAR is engaged in developing slot milling cutters in various fields:
- Cutters carrying indexable inserts
- Assembled MULTI-MASTER slot milling tools with replaceable heads
- Assembled T-SLOT milling cutters with replaceable solid carbide cutting heads
Which slot is defined as narrow?

The term “narrow slot” generally defines a deep slot of small width. A more rigorous but empirical rule considers a “narrow slot” to be the slot with a width less than 5 mm and a depth of at least 2.5 times the width.
What type of milling does ISCAR recommend for these types of cutters?

Down milling is normally recommended, where chip thickness is formed from thick to thin.
What is the difference between indexable slotting cutters and slitting cutters?

Originally, slotting cutters were intended for milling slots and grooves while slitting cutters were used for slitting or cutting-off. Each type of cutters featured different accuracy requirements, and slitting cutters were less precise. However, technological progress has significantly leveled out differences between slotting and slitting cutters in indexable milling.
Why are the terms "axial depth of cut" and "radial depth of cut" very common in milling slots and grooves?

In milling, a depth of cut is usually measured along the axis of a cutter, axially, while a width of cut – radially, in the direction perpendicular to the axis. Hence the depth of cut and the width of cut also can refer to as "axial depth of cut" and "radial depth of cut" accordingly.
However, this generally accepted approach may sometimes lead to confusion in the case of disc slot milling cutters. The axial depth of cut here is equal to the width of cutter teeth, and it defines the width of a milled slot. The radial depth of cut in the such a case reflects the slot depth.
Therefore, in machining disc milling cutters, using the terms "axial depth of cut" and "radial depth of cut" helps in preventing possible misunderstandings.
Can an ISCAR SD-SP solid carbide slot milling head be mounted on a MULTI-MASTER shank?

No, interchangeable SD-SP slot milling heads are not suitable for direct mounting on MULTI-MASTER shanks. However, mounting is possible when using an SD CAB one-end T-threaded and one-end splined adapter.

Extended Flute Cutters

Why “extended flute” cutters?

The cutting blade of an extended flute cutter consists of a set of indexable inserts that are placed gradually with a mutual offset of one another. Compared to an ordinary indexable mill whose length of cut is limited by the cutting edge of its insert, the cutting length of the extended flute cutter is significantly larger – it is “extended” due to the set of inserts.
What are the other technical terms for extended flute cutters?

Extended flute cutters are also referred to as long-edge cutters and porcupine cutters (known as “porkies” in shop talk).
What are the main applications for extended flute cutters?

Extended flute cutters are designed for high-performance rough milling: milling deep shoulders (known as “deep shouldering” in shoptalk), deep pockets and cavities (“pocketing”), and wide edges (“edging”).
Can extended flute cutters be applied to semi-finish operations?

Yes. There are solutions that ensure this type of machining. For example, ISCAR HELITANG FIN LNK cutters carrying tangentially clamped peripherally ground inserts were designed especially for semi-finish milling.
Why do many types of indexable inserts for extended flute cutters feature a chip splitting design?
Extended flute cutters work in heavy-load conditions. The following factors considerably improve cutter performance, which is why a chip splitting geometry is often integrated into the extended flute cutters’ design:
- Chip splitting results in a wide chip being divided into small segments, which improves chip evacuation and chip handling.
- The action of chip splitting strengthens vibration dampening of a cutter.
- In many cases, chip splitting reduces cutting forces and power consumption, and leads to less heat generation during milling.
- The small segments have fewer tendencies to be re-cut; this greatly improves rough milling of deep cavities and increases tool life.
What are the design configurations of ISCAR’s extended flute cutters?
The ISCAR standard line of extended flute cutters comprises various designs:
- Shell mills
- Mills with cylindrical shanks (smooth or with flats, known as “Weldon-type”)
- Mills with tapered shanks (7:24, HSK)
- CAMFIX polygonal taper shank and replaceable cutting heads with a FLEXFIT connection
Can ISCAR’s extended flute cutters incorporate internal coolant supply channels?

Most of ISCAR’s extended flute cutters have an internal channel for coolant supply through the body of the cutter.
Does ISCAR recommend extended flute cutters for milling titanium?

Yes. Milling titanium usually involves removing considerable machining stock. It is a process with a significant buy-to-fly ratio and a large amount of metal needs to be removed. Extended flute cutters possess significant performance advantages in this area and their use can dramatically cut cycle time.
Why are some extended flute cutters defined as ‘fully effective’?

The design of the cutters known as ‘fully effective’ features the inserts interlinked and overlapping, resulting in a continuous flute. Many other cutters are “half effective”, where the inserts are placed alternately and 2 flutes are necessary to cover the area that the fully effective cutters can cover with only one flute.

Milling Gears and Splines

Does ISCAR provide tools for milling gears and splines?
ISCAR’s current tool program, for milling spur gears with straight teeth and splines, has been developed to include three types of cutter:
- cutters with indexable inserts
- cutters with replaceable cutting heads based on the T-SLOT concept
- cutters with replaceable MULTI-MASTER cutting heads
For which method of generating teeth are ISCAR’s milling tools intended?

Form milling and power skiving.
When talking about generating a tooth profile, what is meant by “form milling”?

Form milling is one of the methods for generating tooth profiles. In form milling, a milling cutter with a working shape like the contour of a tooth space, machines every tooth individually; and a workpiece is indexed through a pitch after generating one space.
Are there other methods of generating tooth profiles, apart from form milling?

The principal methods (in addition to form milling) include gear hobbing, which uses a hob, a cutter with a set of teeth along a helix that mills the workpiece and that rotates together with the workpiece in a similar way to a worm-wheel drive; gear shaping with the use of a gear-shaping cutter, a rotating tool that visually resembles a mill; and by power skiving - a technique that combines gear milling and gear shaping. There are also other methods of generating teeth profiles, such as gear broaching, gear grinding, and gear rolling.
Is milling gear teeth the final operation of a gear-making process?

In general, milling gear teeth is not the final operation in the gear-making process. After this operation, it is necessary to remove burrs and then the sharp edges of the teeth should be rounded or chamfered, for better engagement. Gear rounding, and gear chamfering operations are necessary to avoid quenching gears with sharp edges, which may cause various micro cracks that affect gear life. In addition, milling teeth ensures parameters that feature only gears of relatively low accuracy. As manufacturing precise gears demands tougher characteristics of accuracy and surface finish, other processes such as gear shaving, gear grinding, gear honing, etc., are also applied.
Usually, form gear milling relates mainly to individual and low-batch production. Why do manufacturers of general-purpose cutting tools, including ISCAR, include form gear milling cutters in their program for standard lines?

With batch manufacturing, milling gear teeth is made on specific gear hobbing machines as gear hobbing productivity is substantially higher. However, advanced multifunctional machine tools increasingly widen the range of machining operations that can be performed. Technological processes developed for these machines are oriented to maximize machining operation for one-setup manufacturing, creating a new source for more accurate and productive manufacturing. Milling gears and splines is one of the operations suitable for performing on the new machines.
These new machines require appropriate tooling and manufacturers of general-purpose cutting tools are reconsidering the role of gear-milling cutters in their programs for standard product lines.
What is the module in gearing?

The module (modulus) is one of the main basic parameters of a gear in metric system. It is measured in mm. The module m of a gear with pitch diameter d and number of teeth z is the ratio of the pitch diameter to the number of teeth (d/z).
Does the inch (Imperial) system of gearing also use the module as a basic parameter in gearing?

The inch (Imperial) system operates another basic parameter: the diametral pitch. This is the number of gear teeth per one inch of the pitch diameter. If a gear has N teeth and it features pitch diameter D (in inches), diametral pitch P is calculated as N/D. Sometimes, when specifying gears in inch units, the so-called English module is used. In principle, this module has the same meaning as the module in the metric system, e.g. the ratio of the pitch diameter and the number of teeth; however, the pitch diameter should be taken in inches and not in millimeters like in the metric system.
What is the difference between gear and splines?

Gears in a gear train are intended for transmitting rotational movement between 2 shafts (while the axes of the shafts are not always parallel) and, in most cases, this transmission is combined with changing torque and rotational speed. The gears are used also for transforming rotational movement into linear movement. A splined joint is a demounted connection of two parts to transfer the torque from one to another. The torque is not changed here.
What is the difference between splines and serrations?

Within this context, serrations represent a type of spline. The serrations feature V-shaped space between teeth. They are commonly used in small-size connections.

Grooving

What is the first choice for Heavy Duty Grooving?
- For Groove Only applications, use the DOVEIQGRIP TIGER insert that comes in widths of 10 - 20 mm
- For Groove-Turn applications, use the SUMO-GRIP TAGB insert that comes in widths of 6 - 14 mm
What is the best chip former to machine ductile/gummy materials?

Use the "N" chip former. It is offered in 3 - 8 mm widths for external GIMN inserts and 2 -5 mm widths for internal GEMI/GINI inserts.
What are the recommended grades to use on ISO-M / ISO-P materials?
- The first choice for many applications is IC808
- If you need a harder grade with more wear resistance use IC807
- If you need a tougher grade with more impact resistance (Interrupted cuts) use IC830
What is the best grade to machine ISO-S (high temperature alloys)?
- Use IC806 is to machine high temperature alloys as your first choice.
- For harder ISO-S materials (HRC>35) use IC804
What grooving tool-holders should I use on Swiss-Type machines?

Use our unique Side-Lock GEHSR/GHSR tools, which provide both front and back access that is much easier for Swiss-Type machines (as opposed to the conventional top clamping).
What are the most recommended grades/geometries for grooving/groove-turning cast iron?

Use the TGMA/GIA inserts that feature a K-Land combined with grades IC5010 or IC428
What are the most recommended grades/geometries for grooving/groove-turning aluminum?
- Use the GIPA/GIDA/FSPA inserts that feature a very sharp and positive cutting edge and a polished top rake combined with IC20 carbide grade or ID5 PCD
- For widths of 6 – 8 mm, FSPA round inserts are the best choice due to their superior clamping method
What tools/inserts should I use for internal grooving in small diameter bores?
- Bore diameter 2 – 10 mm: use PICCO inserts on PICCO ACE tools
- Bore diameter 8 – 20 mm: use GIQR inserts on MGCH tools
- Bore diameter 12 – 25 mm: use GEMI/GEPI inserts on GEHIR tools
How can I reduce vibrations?
- Use the minimum possible overhang
- Work with constant RPM
- Reduce the RPM if needed
- Reduce the insert width in order to decrease the cutting force
- For widths of 6 and 8 mm, use WHISPERLINE Anti-Vibration blades
In what cases do you recommend the use of JETCUT tools with internal coolant?

JETCUT tools are recommended for all coolant pressure levels (10 – 340 Bar) and all applications, as they deliver a repetitive and reliable coolant supply directly to the cutting edge at the exact point where it is needed, improving tool life and chip control
Does ISCAR provide the PENTA star-type blank inserts for final shaping?

Yes. ISCAR's grooving line also consists of blank inserts to ensure customization for producing tailor-made profiles.

Parting

What are ISCAR’s priorities for PARTING OFF?
- For general applications up to 38mm part diameter, use DO-GRIP style double-ended inserts
- Above 38mm: Use TANG GRIP style –single ended insert
- Up to 40mm diameter: Use PENTA IQ , a highly economical insert with 5 cutting edges
What is the best grade for machining steel (ISO P)?
- IC808/908
What is the best grade for machining stainless steel (ISO M)?
- C830/5400
What is the best insert geometry / chipformer for machining steel?
- Use "C" geometry, for example DGN 3102C
What is the best insert geometry / chipformer for machining stainless steel?
- Use "J" geometry, for example DGN 3102J
What are the most recommended tools and inserts for machining miniature parts?
- First choice is ISCAR DO-GRIP style (double-ended inserts) which has positive geometry, for example DGN 3102J & DGN 3000P
  * Use tools with Short Head dimensions, for example DGTR 12B-1.4D24SH
- Second choice is to use ISCAR PENTA CUT, an economical insert with 5 cutting edges, for example :
  * PENTA 24N200J020 IC1008 (insert)
  * PCHR 12-24 (tool)
What is the best tool for heavy duty applications?
- Use ISCAR TANG GRIP (single ended) insert – choose width according to part diameter
- For heavy duty applications ISCAR offers 5-12.7mm insert widths
- IC830 is the most suitable grade
- Recommended insert geometry /chipformer is "C" type
How to reduce the bur on the part?
- Use an R or L style of insert - these inserts have a lead angle, so the cutting edge is not straight
- Also use a positive cutting rake, for example: DGR -3102J-6D (6D =6 degrees lead angle)
- It is highly recommended to reduce the feed by 50% at the final cut
How to improve insert lifespan?

Analyze the failure phenomena and choose grade accordingly:
Wear: use a harder grade such as IC808 or 807
Breakages: choose a harder grade such as IC830
Which is the best insert for an interrupted cut?

Use a negative cutting rake, "C" chipformer and IC830 grade
How to improve chip control when long chips appear?
- Select the correct chipformer and cutting parameters in order to obtain good chip formation
- Choose a more aggressive chipformer
- To increase feed, please refer to ISCAR user guide
How to improve part straightness and surface?
- Use neutral insert and a stable tool with the minimum overhang needed
- Adjust the cutting parameters
Can a JETCROWN tool block carry different square adapters?

Yes. A JETCROWN tool block is intended for mounting square adapters of different dimensions. An adapter is clamped on the block by use of a crown which is a specially designed part of the JETCROWN tool assembly that ensures pinpointed high-pressure coolant supply. Important to note that for each insert width a separate crown is required. Refer to ISCAR's catalogues and technical guides for more data.
Why has ISCAR introduced new tool blocks with a reinforced rib on the opposite side of the block in addition to the existing line of tool blocks in the LOGIQ-F-GRIP line?

There are cases where the reinforced rib interferes and prevents clamping the ISCAR LOGIQ-F-GRIP block on typical turret positions. Such a problem can be solved by using the blocks which have the rib on the opposite side. In these cases, ISCAR has added blocks with another rib location to the LOGIQ-F-GRIP product line.

Drilling

What is the recommended coolant flow rate?

Depends on diameter. For example, the minimal flow rate for 6 mm SUMOCHAM is 5 liters per minute. For 20 mm, the minimal flow rate require is 18 liters per minute. For more information, please refer to SUMOCHAM user guide in our catalogue, page 491.
What is the recommended coolant pressure?

Depends on diameter and tool length. For example, the minimal pressure for 6 mm SUMOCHAM on 8xD is 12 bar. For 25 mm SUMOCHAM on 12xD, the minimal pressure required is 4.5 bar. For more information, please refer to SUMOCHAM user guide in our catalogue, page 491.
What straightness can be achieved with the SUMOCHAM line?

With a stable set-up, deviation may vary from 0.03 mm to 0.05 mm for each 100 mm of drilling depth. Important: Achieved results may vary due to machine, fixture, adaptation, etc.
What is the correct deep drilling cycle with the pre-hole and the next tool?

In order to avoid mistakes, it is best to prepare the pre-hole with the same geometry that you intend to use for the subsequent deep drilling operation. For a more detailed explanation, please refer to our catalogue, page 492.
Is it possible to make boring operation with SUMOCHAM?

No, the SUMOCHAM family is not designed for boring operations. Failure of the tool and insert may occur.
What is the recommended geometry for titanium?

The first choice is ICG. The second choice is ICP.
Is it possible to regrind SUMOCHAM heads?

Yes, ICP/ICK/ICM/ICN geometries can be reground up to three times. Please see a detailed explanation on pages 502-504 in our catalogue. Note: FCP/HCP/ICG/ICH geometries can be reground only at TEFEN.
What is the maximum permitted run-out for SUMOCHAM?

To achieve best performance and tool life, radial and axial run-out should not exceed 0.02 mm. A detailed user guide can be found in our catalogue, starting on page 490.
Is it possible to use SUMOCHAM for interrupted cut operations?

SUMOCHAM cannot withstand interrupted cut operations. Loss of clamping force of the tool may happen, eventually leading to falling out of the insert.
What solution does ISCAR recommend for hard materials?

For hard materials we recommend our SCD-AH solid carbide drills made from IC903 grade, or a semi-standard option for SUMOCHAM line, the ICH heads.
What type of adapter is recommended?

The recommended adapter is the one that is most suited for the tool's shank. For example, if the shank is round, the most accurate adapter would be of the HYDRO type. Please refer to page 829 in our catalogue.
What should be the maximum exit be for the SUMOCHAM exit hole?

The exit for the materials should not be more than 2-3 mm less than the diameter edge of the insert.
What is your recommended solution for aluminum machining?

Answer: Depends on the application. SUMOCHAM line has ICN inserts, which offer a dedicated solution for rilling non-ferrous materials.
What are the criteria to look for to indicate when SUMOCHAM heads are worn out?

It is best to measure wear on a microscope. Additional indicators for wear are illustrated on page 493 in our catalogue.
Which hole is considered as "short" and which as "deep"?

Commonly used terms “short” and “deep” holes do not have a strict definition. It is widely accepted that drilling a hole of diameter d and (10…12)×d or higher in depth relates to deep drilling, while holes having depth up to 5×d, are short.
In the terminology used by ISCAR, only a drilling depth of 12×d and higher is considered as deep. Consequently, the holes with shallower depths are short.
What is a cutting length series of drills?

The drills vary in their cutting length. In general, tool manufacturers normalize the drills by cutting length series (short, regular, etc.), according to the ratio "cutting length/drill diameter". At ISCAR, drills intended for machining short holes are usually divided into the following length series: short (up to 3×d), long (4×d and 5×d) and extra-long (8×d and 12×d).
Why is a center drill referred to as a "countersink" and even as a "spot drill"?

A center drill is needed for forming a conical hole in workpieces. This hole is used for supporting the workpieces by the centers of machine tools. One of the methods for forming conical holes is countersinking - machining by a specially designed cutter, a countersink. In fact, the center drill performs a combination of two operations simultaneously: drilling and countersinking. Therefore, the center drill is often referenced as a “combined countersink”. Sometimes, a center drill is considered a spot drill; however this specification is not strictly correct. A spot drill only drills but a center drill performs two operations: drilling and countersinking, therefore “spot a hole” and “drill a center hole” are not the same.
In center drilling, does a Multi-Master replaceable solid carbide head offer a real alternative to reversible high-speed steel (HSS) drill bits?

Reversible HSS center drill bits are the most popular tools for center drilling: they are simple, always available for purchase, and feature low prices. The Multi-Master replaceable solid carbide head enables significant increases in cutting speed and feed, resulting in higher productivity and reduced machining costs, especially in cases of machining difficult-to-cut material. In addition, the tool life of the head is much longer. A brief economical calculation will show the preferred alternative for each case.
Is a chip-splitting cutting geometry suitable for drills of a relatively small diameter?

A chip-splitting cutting geometry may be used in drilling tools. There are different drill cutting edge designs with chip splitting grooves, for example the SUMOCHAM ICG heads. Splitting chips into small segments improves chip evacuation and cutting speed. Under the same cutting conditions, a straight-style edge ensures better surface finish. Therefore, chip-splitting geometry is suitable mainly for rough drilling operations.
What are the advantages of the concave, pagoda-shape, cutting edges of SUMOCHAMIQ exchangeable drilling heads?

The shape of the cutting edge substantially enhances the self-centering capability of the drill and enables drilling holes of depths up to 12×d directly into solid material, without pre-drilling a pilot hole. In addition, the HCP geometry facilitates gradual penetration into machined material which reduces the cutting forces, obtaining better hole quality – particularly when the drilling depth is significant.
What are the advantages of chamfering rings for drills?

A chamfering ring is intended for mounting in the body of a standard drill in the desired position according to the drill tip. The ring mounting configures a combined holemaking tool that can perform drilling and chamfering in one operation.
Is it possible to regrind LOGIQ3CHAM 3 flute exchangeable drill heads directly at the customers' premises?

Regrinding new geometries of these 3 flute drill heads is complicated and cannot usually be done locally.
What are the ISCAR products for deep drilling?

ISCAR's line of deep drilling tools comprises gundrills and drills for ejector and single tube (STS) systems.
Can the SUMOCHAM drills be mounted in FLEXFIT threaded adaptors and tool holders?

ISCAR produces modular drills combining SUMOCHAM design with a FLEXFIT threaded connection to enable mounting. A wide range of FLEXFIT threaded adaptors and flatted shanks ensures configuration of the assembled drill with a maximally shortened overhang, so that the modular drills can be used on machines with limited space for tooling (for example on multi-spindle and Swiss-type machines).
Do the terms "step drill" and "subland drill" mean the same?

Not exactly. A step drill is a drill with cutting areas of different diameters to generate a step-diameter hole in one pass. A subland drill is a solid twist step drill, which features different lands for each diameter. However, a step twist drill has the same land along the drill body. Usually, there are two drilling areas in a subland drill. A subland drill is a sub type of step drill.
When should a carbide guide pad in a deep drilling tool be reversed or replaced?

Even though the guide pads do not cut material, they, like carbide cutting inserts or heads, are subject to wear. A damaged or worn out guide pad causes unacceptable roughness and scratching of the machined hole surface.
The pads should be thoroughly examined visually before applying a drill. If a pad is damaged or the pad working corner wears out approximately 70% of the corner width, the pad should be reversed or replaced.
What is a stub drill?

Commonly called a twist drill with a shortened length of flute to make the drill stronger and more rigid.
Stub drills are often referred to as extra-short-length drills.
What is the main application of ISCAR's flat drills and drilling heads?

The main application of these tools is their drilling hole with a nearly flat bottom. For example, counterbores for screw heads, spring seats, seal housings, etc.
The advantage is that no pre-drilling is required when drilling directly into solid materials.
ISCAR's product range of tools for machining composite materials includes solid carbide drills with PCD nibs and wafers.
Can these drills be resharpened?

Yes, they can. Both drill types have a large area for multiple regrinding and can be reground several times.
Which drills are considered as micro drills?

Even though there is no general definition, drills in a diameter of less than 2-3 mm (0.08-.125") are often referred to as micro drills. Sometimes, such drills are also named "small-size drills".
What is a drill mill?

It is a combined rotating tool that comprises two cutting sections: a drill tool and milling peripheral cutter. The drilling tool is intended to drill a hole. By combining the milling cutter, the hole can be enlarged.
Does ISCAR provide flat bottom drills with 3 flutes?

ISCAR LOGIQ-3-CHAM family comprises 3 flute flat bottom drilling heads which can be mounted on any drill type related to this family, to create a flat bottom hole in solid material without pre-drilling.
What is the MODUDRILL?

ISCAR's MODUDRILL is a modular drilling tool system. A typical MODUDRILL tool is an assembly of tools which comprises a steel body and exchangeable drilling heads mounted on the same body. There are two types of the heads: the first with guide pads carrying indexable carbide inserts, and the second with replaceable CHAM-IQ-DRILL solid carbide heads. In addition, the system contains a steel extension that can be mounted on the body to increase the drilling depth.
What is an NC spotting drill?

An NC spotting drill (also referred to as a NC spot drill) is a precise drill that features a small cutting depth, typically around the height of a drill point. NC spotting drills are intended mainly for pre-drilling an accurate location and to ensure precise and fast subsequent drilling operations without guide bushings, especially on CNC machines. Typically, the NC spotting drills have a 90-degrees point angle.
What is peck drilling?

In peck drilling also referred to as drilling with peck feed or simply "pecking", a drill is repetitively retracted to evacuate chips to dissipate heat.
Kaj je sveder za tiskana vezja?

Sveder za tiskana vezja je zelo natančen mikro sveder, ki je namenjen za vrtanje kompozitnih laminatov - osnovnega materiala za izdelavo tiskanih vezij. Imenujemo jih tudi tiskane vezne plošče (označujemo jih PCB in PWB).
Kaj je 'potisna sila' pri vrtanju?

Pri vrtanju je potisna sila aksialna sila, ki deluje v smeri podajanja.Ta sila obremeni sveder vzdolž njegove osi. Potisna sila je rezultanta aksialnih sil na konico svedra, glavnih rezalnih robov in manjših rezalnih robov svedra. Približno 50% potisne sile prenaša sama konica svedra.
Kolikšno natančnost izvrtin zagotavljajo ISCAR-jevi SUMOCHAM svedri z izmenljivimi trdokovinskimi konicami?

ISCAR-jevi SUMOCHAM svedri z izmenljivimi trdokovinskimi konicami zagotavljajo natančnost izvrtin v ISO tolerančnih razredih IT10-IT9 pri običajnih pogojih obdelave.

Reaming

When is a reaming operation required?

A reaming operation is needed when the tolerance or/and surface finish requirements are tight and can't be achieved by drilling or boring.
For what tolerance field are the standard reamers suitable?

Standard ISCAR reamers are suitable for IT7 field.
Are the standard reamers suitable for all materials?

Standard reamers are suitable for most materials, but for the ISO N and ISO S material groups, it is preferable to consult the technical department for the most suitable solution.
What is the average tool life for a reamer?

Since there are many different factors that affect its tool life (such as material, coolant, tolerance, runout etc.), it is difficult to estimate tool life and each case should be investigated individually.
Is it possible to ream without any coolant?

No. It is impossible to ream without coolant; the most optimal situation is working with internal coolant but reaming with external coolant is also an option.
What recommended stock material should be left over before reaming?

The recommended stock material depends on the machined material, reamer diameter and the tool used for hole preparation. In general, it can range from 0.15 to 0.4 mm per diameter.
What is the highest spindle runout possible for a reaming operation?

In general, the highest spindle runout possible for reaming is around 0.01mm, but this also depends on the size and tolerance requirement. Above 0.01mm, the customer should use an ADJ system for runout compensation and adjustment.
What is the main advantage an ISCAR's reamer with rolling devices?

This reamer combines a BAYO-T-REAM high-speed reamer with a rolling device in one single tool. This ensures achieving an accurate hole with exceptional, mirror-like, surface finish.
Kaj pomenijo črke "BN" in številka za njimi v oznakah izmenljivih glav za povrtavanje BAYO-T-REAM?

Črke "BN" v oznakah glav za povrtavanje BAYO-T-REAM se nanašajo na "velikost bajoneta". Številka za "BN" označuje specifično velikost priključka za namestitev glave za povrtavanje na držalo, kot je BN5, BN6 itd.

ISO

How to increase productivity for super alloys and Ni-based materials with ISCAR Ceramic Grades?

ISCAR has a wide range of ceramic grades, such as the IW7, for machining super alloys and Ni-based materials.
Our ceramic grades have the ability to work ten times faster in cutting speed - from 150M/min up to 450M/min - which is ten times higher than any conventional carbide inserts. This dramatically increases productivity.
What is ISCAR’s first choice in chip formers for steel machining?

ISCAR introduces three new chipformers for finishing medium and rough turning of steel: F3P, M3P and R3P.
The chipformers, combined with ISCAR’s SUMO TEC grades, deliver higher productivity, longer tool life, improved workpiece quality, and more reliable performance. The new chipformers generate less heat and avoid the problem of chips attaching themselves to cutting tools and components. Chips are broken down into smaller pieces, preventing them from tangling around the workpiece and enabling more efficient removal from conveyor belts.
How to improve chip control with the CBN insert?

CBN inserts are mainly used for machining hard materials with high hardness levels from 55 and up to 62 Rc. Conventional CBN inserts offer a wide range of brazed and flat tips that produce long and curled chips during the turning/machining of hard steel. The result is long chips that scratch the work piece and damage the surface quality. The ISCAR solution is a new CBN insert with ground chip breaker on the cutting edge, providing excellent chip control in medium to finishing applications with high surface quality.
How to reduce vibrations on a boring bar with a high overhang of more than 4xBD?

Throughout the world, machinists have to deal with the presence of problematic vibrations on a daily basis. To help solve these difficulties, ISCAR’s Research and Development division has produced an anti-vibration boring bar which contains the dampening mechanism inside the body. This reduces and even eliminates vibrations when using boring bars with a high overhang. The new anti-vibration line is called WHISPERLINE.
How to increase productivity in gray cast iron machining with ISCAR Ceramic Grades?

Gray cast iron is recognized as the most popular material in the automotive industry. For machining gray cast iron, ISCAR offers a wide range of ceramic grades such as IS6 SiAlON inserts.
The IS6 grade was developed in order to increase productivity in gray cast iron machining. The main advantage of our IS6 SiAlON ceramic grades is the ability to work three to four times faster in cutting speed, from 400M/min and up to 1200M/min, which is three times higher than any conventional carbide inserts. This increases productivity dramatically.
What is ISCAR’s first choice in chip formers for stainless steel?

ISCAR is introducing 3 new chipformers: F3M, M3M and R3M for finishing, medium and rough turning stainless steel which, together with the most advanced SUMOTEC grades, provide higher productivity, tool life and performance reliability.
The F3M chipformer has positive rake angles for smooth cutting, reduced cutting forces and insert wear, leading to dramatically increased tool life.
The M3M chipformer is for medium machining of stainless steel with reinforced cutting edge and positive rake angle to reduce cutting forces and for smooth cutting.
The R3M chipformer for chip breakers is for rough machining of stainless steel with reinforced cutting edge and positive rake angle to reduce cutting forces.
What is the effect of high-pressure coolant?

The main advantage of the JETCUT tools is the ability to supply the coolant directly into the cutting zone to ensure high coolant efficiency in order to improve chip control, reduce heat and extend insert life.
The high pressure coolant effect is mainly achieved in the machining of sticky and gummy materials such as super alloys, stainless steel, titanium etc…
Does ISCAR provide tools for Y-axis turning?

Yes, ISCAR provides these tools.

Ceramic Grades & Inserts

How to increase productivity of Ni-based and other superalloys with ISCAR ceramic grades?

ISCAR has a wide range of ceramic grades, for example IW7, for machining Ni-based and other superalloys. Our ceramic grades have the ability to work 10 times faster in cutting speed, starting from 150M/min and going up to 450M/min which is 10 times higher than any conventional carbide inserts. This increases productivity dramatically.
Which chip formers does ISCAR recommend for steel machining?

ISCAR has introduced three new chip formers for finishing medium and rough turning of steel: F3P, M3P and R3P. Combined with ISCAR’s SUMO TEC grades, the chip formers offer higher productivity, longer tool life, improved workpiece quality and more reliable performance. The new chip formers generate less heat and avoid the problem of chips attaching themselves to cutting tools and components. Chips are broken down into smaller pieces, preventing them from tangling around the workpiece and enabling more efficient removal from conveyor belts.
How to improve chip control with CBN inserts?

CBN inserts are mainly for machining hard materials with high hardness - from 55 and up to 62 Rc materials. Conventional CBN inserts offer a wide range of brazed and flat tips that produce long and curled chips during the turning machining of hard steel, resulting in long chips that scratch the work piece and damaging the surface quality. The ISCAR solution is a new CBN insert with ground chip breaker on the cutting edge, which provides excellent chip control in medium to finishing applications with high surface quality.
How to reduce vibrations on boring bars with a high overhang of more than 4xBD?

Throughout the world, machinists deal daily with problematic vibrations. ISCAR’s Research and Development department has designed and developed the WHISPERLINE range of anti-vibration tools to resolve this issue, including a boring bar with the dampening mechanism inside the body that eliminates and reduces vibrations when using bars with a high overhang.
How to increase productivity of gray cast iron with ISCAR ceramic grades?

The most popular material in the automotive industry is gray cast iron. For machining gray cast iron, ISCAR offers a wide range of ceramic grades including IS6 SIALON inserts. Developed especially to increase productivity in gray cast iron, the IS6 SAILON grade can work 3 or 4 times faster in cutting speed - from 400M/min and up to 1200M/min which is 3 times higher than any conventional carbide inserts. This increases productivity dramatically.
What is ISCAR’s first choice in chip formers for stainless steel?

ISCAR has introduced three new chip formers: F3M, M3M and R3M for finishing, medium and rough turning stainless steel. Combined with the most advanced SUMOTEC grades, the chip formers provide higher productivity, tool life and performance reliability. The F3M Chipformer has positive rake angles for smooth cutting, reduced cutting forces and insert wear, leading to dramatically increased tool life. The M3M Chipformer is designed for medium machining of stainless steel with reinforced cutting edge and Positive rake angle, to reduce cutting forces and ensure smooth cutting. The R3M Chipformer for chip breakers is designed for rough machining of stainless steel with reinforced cutting edge and positive rake angle, to reduce cutting forces.
What is the effect of high-pressure coolant?

JETCUT tools have the ability to supply coolant directly into the cutting zone, ensuring high coolant efficiency, improved chip control, reduced heat and longer insert life. The high pressure coolant effect is applied to the machining of sticky and gummy materials such as super alloys, stainless steel, titanium etc.

Threading

What is the most suitable grade for machining stainless steel?

IC1007
What is the most suitable grade for machining HTA?

IC806
What is the most suitable grade for low speed and unstable machines?

IC228
What is the smallest recommended pass for thread profile?

Bigger than honing size
Why doesn’t the chip breaker function?

Apparently the depth of cut is too small, so the chip breaker is inefficient
How we can improve chip control?
Improve chip control by selecting the correct infeed type:
- Radial infeed
- Flank infeed
- Alternating flank infeed
How we can shorten process time?

Use with multi tooth threading inserts (2M, 3M)
Using two or three teeth combinations allow fewer passes and shorter cutting times. These are available for the most common profiles and pitches and are a good choice for economic threading in mass production.
What is the difference between partial to full profile insert?
Partial profile:
- Performs different thread standards and is suitable for a wide range of pitches that have a common angle (60º or 55º)
- Inserts with a small root-corner radius suitable for the smallest pitch of the range
- Additional operations to complete the outer/internal diameter is necessary
- Not recommended for mass production
- Eliminates the need for different inserts
Full profile:
- Performs complete thread profile
- Root corner radius is only
- Suitable for the relevant pitch
- Recommended for mass production
- Suitable for one profile only
How to select the correct anvil?

Anvils for positive inclination angle are applicable when turning RH thread with RH holders or LH thread with LH tool holders.
Anvils for negative inclination are used when turning RH thread with LH holder or LH thread with RH tool holder.
Use AE Anvils for EX-RH and IN-LH Tool holders.
Use Al Anvils for IN-RH and EX-LH Tool holders.
Which screw threads are considered as miniature and which as micro?

Principally, both the definitions of "miniature" and "micro" are not universally standardized, and different industries have their own specific size ranges for miniature and micro screw threads.
In general, miniature screw threads typically refer to threads with diameters ranging from around 0.3 mm (.012") up to about 2 mm (.08"). These threads are commonly used in applications such as electronics, small appliances, and precision instruments.
On the other hand, micro screw threads are usually even smaller, with diameters typically 0.3 mm (.012") and below. These extremely small threads are commonly found in microelectronics, medical devices, optical equipment, and other specialized industries where precision and miniaturization are crucial.

Tool Material Grades

What is a tool material?

In cutting tools, a tool material is the material from which the active (cutting) part of a tool is produced. This is the material that directly cuts the workpiece during machining.
How does ISCAR designate its tool materials?

ISCAR’s system of designating tool material grades uses letters and numbers. The letters indicate the material group:
IB – cubic boron nitride (CBN)
IC – cemented carbide and cermet
ID – polycrystalline diamond (PCD)
IS – ceramics
DT – cemented carbide with dual (CVD+PVD) coating
What is a carbide grade?

A combination of cemented carbide, coating and post-coating treatment produces a carbide grade. Only one of these components - the cemented carbide - is the necessary element of the grade. The others are optional. Cemented carbide is a composite material comprising hard carbide particles that are cemented by binding metal (mainly cobalt).
Most cemented carbides used for producing cutting tools integrate wear-resistant coating and are known as “coated cemented carbides”. There are also various treatment processes that are applied to already coated cemented carbide (for example, the rake surface of an indexable insert). “Cemented carbide” can refer both to the substrate of a coated grade and to an uncoated grade.
How does ISCAR classify carbide grades?

The international standard ISO 513 classifies hard cutting material based on their reasonable applicability with respect to the materials. ISCAR adopted this standard and uses the same approach in tool development. Cemented carbides are very hard materials and therefore they can cut most engineering materials, which are softer. Some carbide grades demonstrate better performance than others in cutting tools applied to machining a specific class of materials.
The groups of application of carbide grades in accordance with ISO 513 include letters and numbers after the letter. What do they mean?

The letters in the group of application define a class of engineering materials, to which a tool that is produced from a specific grade, can be applied successfully. The classification numbers show hardness-toughness ratio of the grade in an arbitrary scale. Higher numbers indicate an increase in grade toughness, while lower numbers indicate an increase in grade hardness.
What is SUMO TEC technology?

SUMO TEC is a specific post-coating treatment process developed by ISCAR. The treatment has the effect of making coated surfaces even and uniform, minimizing inner stresses and droplets in coating. In CVD coatings, due to the difference in thermal expansion coefficients between the substrate and the coating layers, internal tensile stresses are produced. Also, PVD coatings feature surface droplets. These factors negatively affect a coating and therefore shorten insert tool life.
Applying SUMOTEC post-coating technologies considerably reduces and even removes these unwanted defects and results in increasing tool life and greater productivity.
Why are PVD nano layered coatings considered so efficient and progressive?

PVD coatings were introduced during the late 1980’s. With the use of advanced nanotechnology, PVD coatings performed a gigantic step in overcoming complex problems that were impeding progress in the field.
Developments in science and technology brought a new class of wear-resistant nano layered coatings. These coatings are a combination of layers having a thickness of up to 50 nm (nanometers) and demonstrate significant increases in the strength of the coating compared to conventional methods.
The designation of ISCAR’s carbide grades usually starts from letters “IC”. Why is grade DT7150 (DO-TEC) designated differently?

Coating technology features two principal directions - Chemical Vapor Deposition (CVD) and Physical Vapor Deposition (PVD). Technology development allows both methods – CVD and PVD – to be combined for insert coatings, as a means of controlling coating properties.
ISCAR’s carbide grade DT7150 features a tough substrate and a dual MT CVD (Medium Temperature CVD) and TiAlN PVD coating. The grade was originally developed to improve the productive machining of special-purpose hard cast iron.
Why are several of ISCAR’s carbide grades referred to by customers as “sun tan” grades?

Some PVD coated (like IC840 or IC882) and CVD coated (IC5820, for example) carbide grades, originally developed for machining ISO S and ISO M materials, feature a bronze chocolate color. The “sunbathed” appearance of the inserts produced from these grades resulted in the shop talk definition “sun tan” grade.
What are the fundamental differences between these commonly used definitions: "ultra-fine", "submicron" and "fine" carbide grades?

Each of these definitions relate to the size of the carbide grains in a carbide grade substrate. Sizes may slightly differ for various standards and norms of carbide product manufacturers, but usually they refer to the following:
1 - 1.4 μm (40 - 55 μin) grain size         fine grade
0.7 - 0.9 μm (27.5 - 35 μin) grain size   submicron grade
0.2 - 0.6 μm (8 - 24 μin) grain size        ultra-fine grade

In addition, depending on the grain size, there are medium, coarse, extra coarse and even nano carbide grades. The last, for example, features extremely small grain sizes: less than 0.2 μm or 8 μin.
Which terms are correct: "cemented carbide", "tungsten carbide", "wolfram carbide" or "hard metal"?

All four terms refer to cemented tungsten carbide. "Tungsten" is another name for the chemical element Wolfram. (Incidentally, the word origin is Swedish, meaning "heavy stone").
In the field of cutting tool manufacturing, the terms "cemented carbide", "tungsten carbide" and the abbreviation "HM" (hard metal) are usually used.
What are the main properties of ceramics as a cutting tool material?

When compared with cemented carbides, ceramics possess considerably higher hot hardness and chemical inertness. This means that ceramics ensure much greater cutting speeds and eliminate diffusion wear. Ceramics have lower crack resistance – this feature emphasizes the importance of cutting-edge preparation as a factor of successful machining.
What are the main types of ceramics?
There are two main types of ceramics:
- Based on aluminum oxide or alumina (Al₂O₃)
- Based on silicon nitride (Si₃N₄)
Aluminum oxide based ceramics include pure ("oxide" or "white"), mixed ("black"), and reinforced ceramics.
Silicon nitride based ceramics can be divided into several types, according to content, mechanical properties and production technology. SiAlON ("sialon") ceramics generally fall into this category.
As cutting materials, ceramics lie between cemented carbides and super hard materials such as polycrystalline diamond (PCD) and cubic boron nitride (CBN), according to their toughness-hardness characteristics.
What are the advantages of whisker-reinforced ceramics?

Whisker-reinforced or "whisker" ceramics are aluminum oxide based ceramics that are reinforced by uniformly dispersed silicon carbide whiskers. Whisker ceramics have higher hardness and strength than unreinforced alumina based ceramics, which improves cutting performance.
What is sialon?

Sialon or, more accurately, SiAlON, is a type of ceramic comprising silicon (Si), aluminum (Al), oxygen (O) and nitrogen (N). SiAlON may be considered as a type of silicon nitride based ceramic but features less toughness and higher oxidation resistance. It is simpler to produce SiAlON than to produce other silicon nitride based ceramics.
What is cermet?

The word "cermet" is made from "ceramic" and "metal". It designates an artificial composite material usually manufactured by powder metallurgy technology. Cermet is a type of cemented carbide where hard particles are represented by titanium-based compounds instead of the tungsten carbides that characterize the cemented carbides commonly used in cutting tools. When compared with tungsten carbides, cermet has higher resistance to abrasive and oxidation wear but its toughness is considerably smaller. In addition, cermet is very sensitive to thermal load.
What is the difference between CBN and PCBN?

Both CBN and PCBN relate to Boron Nitride (BN) - a polymorph material formed by two chemical elements. Boron Nitride exists in different crystal structures. One is cubic and the BN in this structure is Cubic Boron Nitride (CBN).
As a cutting tool material, CBN is used as a polycrystalline compound, where CBN particles and an added binder are sintered together. The material produced is "Polycrystalline CBN" or simply "PCBN". The percentage of CBN can vary in different PCBN grades. In the context of cutting tools, the commonly used abbreviations "CBN" and "PCBN" may be considered as synonyms.
Can the cutting ceramics, CBN and PCD be applied to machining titanium?

Cutting ceramics and cubic boron nitride (CBN) are not suitable for machining titanium, although polycrystalline diamond (PCD) has proved itself in finish machining titanium in several cases.
Does ISO 513 standard relate to cemented carbides only?

The answer is no. This ISO 513 standard specifies application and specification of hard cutting materials such as cemented carbides, ceramics, diamond, and boron nitride.
What is the main application of diamond-like carbon (DLC) coated tools?

DLC-coated tools are intended mostly for machining aluminum and non-ferrous materials (ISO N group of application).
Which cutting materials are referred to as ultra-hard?

Usually, diamond and cubic boron nitride (CBN) are the two hardest cutting materials considered as ultra-hard.
What is the difference between TiAlN and AlTiN coatings?

The main difference between titanium aluminum nitride (TiAlN) or aluminum titanium nitride (AlTiN) coatings is the content of aluminum which is not above 50% with reference to TiAlN, and more than 50% in AlTiN. The dominating metallic element is written first in the coating formula.
What is a superlattice?

In cutting tool coatings, this is another term for multi-layer nano coating.
What is the main function of coatings in cutting tools?

The main function of cutting tool coatings is to improve the wear strength of a tool, specifically to increase resistance to abrasion, adhesive wear, and to provide thermal protection for prolonged tool life.
What is the advantage of natural diamond as a tool material when compared to synthetic polycrystalline diamond (PCD)?

The monocrystalline structure of natural diamond provides a perfect cutting-edge contour without any junction points. This feature provides a substantial advantage to ensure ultra-high, really "mirror" surface finish required in some applications such as machining crucial parts of optical equipment. In contrast, a PCD cutting edge is formed by various crystals. This produces appropriate junctions on the edge, consequently every junction produces its own trace on a machined surface.
Which PCBN grade is considered to possess high CBN content and which has low?

This subject is not defined, yet depending on CBN percentage the PCBN grades are divided according to:
- high-CBN-content grades (85% and more),
- low-CBN-content grades (about 55%).
What is MT CVD?

In cutting tools, MT CVD is a method for coating products made of cutting materials, specifically replaceable inserts from cemented carbides, based on chemical vapor deposition (CVD). Additional letters "MT" are "medium" (sometimes also referred to as "moderate") "temperature" as MT CVD utilizes temperatures around 800°C (1470°F). This is significantly lower when compared to 900-1000°C (1650-1830°F) that feature typical CVD coating process.
What is HSS-PM?

HSS-PM is the abbreviation that relates to high-speed steel (HSS), produced by use of powder metallurgy (PM) technology.
What is the purpose of adding various substances to pure tungsten carbide in carbide grades?

In tungsten carbide grades, cobalt is commonly used as the binder, while other substances are added to enhance the performance capabilities of the grade. For instance, the addition of tantalum carbide (TaC) improves thermal deformation resistance, while the addition of titanium carbide (TiC) helps reduce crater formation.

Engineering Materials

When giving recommendations about cutting data, how does ISCAR classify engineering materials?

ISCAR material groups are organized in accordance with international standard ISO 513 Classification and application of hard cutting materials for metal removal with defined cutting edges — Designation of the main groups and groups of application and technical guides VDI 3323 Anwendungseignung von Harten Schneidstoffen (English: Information on applicability of hard cutting materials for machining by chip removal). VDI (Verein Deutscher Ingenieure) is the Association of German Engineers.
The ISO 513 standard specifies cutting tools intended for machining stainless steel as the tools that apply to Group M. Is this correct?

In ISO 513, Group M (yellow identification color) relates to the tools for machining stainless steel of austenitic and austenitic/ferritic (duplex) structure. Ferritic and martensitic stainless steel belong to Group P (blue color) and starting cutting data should be set accordingly.
Is machining titanium like machining austenitic stainless steel?

Commercially pure titanium and, with some applications, α- or α-β- titanium alloys may be machined like austenitic stainless steel but not treated β- and near-β- alloys.
What is “titanium beta”?

“Titanium beta” is an expression that occurs in aerospace industry lingo/shop talk. It can refer to two different materials - a β-annealed α-β- titanium alloy or, rarely, a β-alloy. Therefore the expression should be exactly specified before using it, or even avoided to prevent possible misunderstanding.
Why is the machinability of materials from ISO M and S groups considered together?

These materials are difficult-to-cut materials and have common features that affect machinability: low thermal conductivity and high specific cutting force.
Does cast iron relate to ISO Group K?

The majority of cast iron grades (grey, nodular, malleable) relate to Group K.
When machining hardened or chilled cast iron, appropriate cutting tools (and corresponding cutting data) should be chosen as recommended for Group H.
Austempered ductile iron (ADI) in its soft condition is connected with Group P.
Austempered ductile iron (ADI) in its hardened condition is connected to Group H.
Which steel is pre-hardened and which is hard?
Steel producers supply steels in different delivery conditions: annealed, pre-hardened, hardened. The loosely defined term "pre-hardened steel" relates to steel that is hardened and tempered to a hardness that is not too high - generally this is less than HRC 45. The terms "pre-hardened" and "hard steel" are allied to cutting tool development and the ability of the tools to cut material. Commonly, the steels can be divided into the following conditional groups depending on their hardness:
- Soft (annealed to hardness up to HB 250)
- Pre-hardened to two ranges:
  - HRC 30-37
  - HRC 38-44
- Hardened to three ranges:
  - HRC 45-49
  - HRC 50-55
  - HRC 56-63 and more
As for "hard steel", usually it refers to steel hardened to HRC 60 and more.
What is Ebonite and how to machine this material?

Ebonite is a hard vulcanized rubber containing a high percentage of sulfur. For the purpose of identifying a suitable tool and appropriate cutting data, Ebonite is characterized by ISCAR material group 30 (ISO N application class). To machine Ebonite effectively, we advise following ISCAR’s recommendations for this group.
Are hard metal and heavy metal the same?

No.
In metalworking, "hard metal" is a commonly used name for cemented carbide, which is a sintered hard material based on wolfram (tungsten) carbide. Cemented carbide is often referred as simply tungsten carbide. It is the main cutting tool material used today.
Heavy metals are metals with high atomic weight or density. In the metalworking industry, the term “heavy metal” usually refers to heavy metal alloys, which are sintered composite materials containing 90% or more tungsten.
What is the difference between duplex and super duplex stainless steels?

Duplex stainless steel has a two-phase metallurgical structure: austenitic-ferritic, approximately in equal shares.
Super duplex stainless steel is a type of duplex stainless steel that contains an increased percentage of chromium and molybdenum for better corrosion resistance.
From a machinability point of view, these steels are hard-to-cut.
Is machining common in manufacturing plastic products? What is the machinability of plastics?

It is really hard to imagine life today without plastics - organic materials based on synthetic or natural high-molecular compounds (polymers). Plastic products surround us everywhere. Step by step, plastics have replaced traditional materials in many industrial fields, and today plastic is considered one of the most important structural materials. Manufacturing plastic parts is connected mostly with chemical processes; however, for some cases machining is also required. From the point of view of technology, there are three major classes of plastics: thermoplastics, thermosets, and elastomers. According to their use, plastics may be divided into commodity plastics and engineering plastics. Machining is more common for producing parts from engineering plastics, which are represented primarily by thermoplastics. Plastics have very good machinability. In comparison with metals, cutting plastics is performed usually with much higher speeds and feeds, while the applied cutting tools feature significantly less wear. However, selecting appropriate cutting tools is essential to obtain the accuracy required and excellent surface finish.
What is Vitallium and how to machine this material?

Vitallium is a cobalt (Co)-chrome (Cr) alloy that contents approximately 60% of Co, 30% of Cr, 8% of molybdenum and some other elements. Vitallium was developed in the 1930's, and is now used mainly in joint replacement surgery and dental medicine. The alloy is hard-to-machine. Cutting data should be set according to recommendations, related to ISCAR material groups 34 and 35.
What is the difference between stainless steel and corrosion resistant steel?
These definitions are generally used synonymously, along with definitions such as rust-resistant steel, inox steel, and non-corrosive steel.
In fact, stainless steel may actually be divided into the following types according to their main functional features:
- Corrosion-resistant steel, resistant to corrosion under normal conditions
- Oxidation- or rust-resistant steel, resistant to corrosion under high temperatures in aggressive environments
- Heat-resistant or high-temperature steel that does not change its strength under high temperature stress
Therefore, corrosion-resistant steel can be considered as a type of stainless steel.
What are the main difficulties in machining workpieces from high temperature superalloys with honeycomb structures?

The main difficulty in machining these workpieces is low workpiece stiffness, caused by the workpiece's thin-wall structure. Due to the honeycomb structure, a workpiece often cannot be clamped properly, which results in a further reduction in the entire technological system's rigidity.
What is Nitinol and what is its machineability?

Nitinol, also referred to as Nickel Titanium or Ni-Ti, is an intermetallic alloy of Nickel and Titanium. Machining of Nitinol causes intensive abrasion and oxidation wear on the cutting tool. In addition, cutting speed substantially affects tool life - if the speed is too slow or too high, tool life drops dramatically. In general, tools intended for the ISO S application group are used for machining Nitinol.
Which stainless steel is considered as super austenitic?

Super austenitic stainless steel is austenitic stainless steel, which features high content of Molybdenum (more than 6%) and increased percentage of Chromium and Nickel. The combination of materials results in high resistance to pitting corrosion. Usually austenitic stainless steel with pitting resistance and an equivalent number (PREN) of more than 40 is super austenitic. Generally, super austenitic stainless steel has less machinability characteristics when compared to austenitic stainless steel.
What is "pitting resistance equivalent number"?

The "Pitting resistance equivalent number" (PREN) is a conditional value that characterizes theoretical resistance of stainless steel to pitting corrosion based on the stainless-steel content. There are several ways to calculate PREN by use of equations.
What is "mild steel"?

"Mild steel" is another name for low carbon steel.
What are the main difficulties in machining Hadfield steel?

Hadfield steel has a high content of Manganese: 12% in average, and therefore often referred to as "manganese steel". It has austenitic structure which ensures high abrasive wear resistance combined with excellent impact toughness and high ductility. When machined, this steel hardens and adversely impacts machinability. Due to the high ductility of austenite and its tendency to work hardening, Hadfield steel is a very difficult-to-cut material.
What should be taken into account when machining Beryllium and its alloys?

In machining Beryllium (Be) and its alloys, the fine Beryllium dust generated while cutting the material can be dangerous to health. It is essential to use machine tools equipped with appropriate chip collecting units.
Due to Beryllium’s high brittleness, the machined surface may be damaged during machining by microcracks and microflow. To avoid surface damage, the machining process should be under control - rigid workpiece clamping and eliminating vibrations are extremely important.
Beryllium bronze, which is also known as beryllium copper or BeCu, has good machinability. When machining this alloy, users should follow ISCAR's recommendations regarding the cutting data that relates to copper alloys.
What is Zamak and how to machine it?

Zamak, also referred to as ZAMAK, ZAMAC, or Zamac, is a group of zinc-based alloys. The principal alloying elements are aluminum, magnesium and copper. These alloys feature good machinability and their cutting usually does not cause difficulties. ISCAR's tools for the ISO N group of applications are recommended for machining Zamak.
Which cast iron is named "vermicular" and what is its machinability?

Vermicular cast iron is another name for compacted graphite iron (CGI). The structure of this iron features vermicular (worm-shaped) graphite particles.
According to its machinability properties, vermicular cast iron or CGI, falls between grey and nodular cast iron.
What is "bainitic ductile cast iron"?

"Bainitic ductile cast iron" (BDCI) is another name for austempered ductile iron (ADI) that is also referred as "ausferritic spheroidal graphite cast iron".
What is the machinability of maraging steel?

Usually maraging steel is machined in annealed conditions without any specific problems. When steel is aged (heat treated), its machining becomes more difficult. A general rule for selecting cutting tools and finding initial cutting data is to use the same recommendations as in the case of high alloy steel of the same hardness.
What is "Nichrome" and how is it machined?

"Nichrome" is the name of a whole group of Nickel-Chromium alloys. It is also referred to as Chrome-Nickel, NiCr, Ni-Cr, etc. The well-recognized Nichrome 80 (Nichrome 80/20) comprises 80% Nickel and 20% Chromium. Other Nichrome grades may contain additional elements such as Iron.
In machining Nichrome, the initial cutting data can be chosen as it’s recommended for Nickel-based superalloys.
Which materials are considered exotic?

In addition to mainstream engineering materials such as iron-based alloys (steel, stainless steel, cast iron) and common nonferrous metal alloys (aluminum alloys, brass, bronze), there are exotic types of material that were developed to answer specific demands. These exotic materials feature a dedicated application; they are rare and not commonly used and are generally more expensive to fabricate.
An accurate agreed definition of exotic material does not exist. Many experts refer to them as metals, like Beryllium, Zirconium, etc. and their alloys, ceramics, composites, and superalloys. When considering the use of structural materials, superalloys and composites should be distinguished first. Machining exotic materials can be difficult.
What is Stellite, and how to machine it?

Stellite is a range of hard cobalt-chromium alloys that are used for wear resistance and tool materials.
Stellite has poor machinability, approximately ten times less when compared with free-cutting steel. Therefore, machining Stellite by cemented carbide tools features very low cutting speeds, yet the speed can be significantly increased by applying cutting tools from whisker reinforced ceramic.
How to mill Nylon 6?

Nylon 6, also referred to as cast nylon or polyamide, is a polymer, thermoplastic resin. Typically, parts from cast nylon are produced by molding (casting), but in some cases, there is a need to machine this type of material. As a general rule, there are no problems in milling cast nylon, although at times difficulties may arise such as overheating, chip evacuation, and deformation of a part after machining due to the elasticity of cast nylon.
In milling, a typical initial cutting speed is estimated at 400-470 m/min. (1300-1550 sfm) for milling cutters with indexable inserts, and 450-530 m/min. (1480-1750 sfm) for solid carbide endmills and endmills with exchangeable carbide heads. Next, according to the results, the cutting speed can be increased up to 900-1000 m/min (2950-3300 sfm). The greater values may cause overheating, and therefore, are not recommended. Pinpointed air coolant, especially through a cutter body is highly recommended, if not to say necessary.
How to machine naval high-tensile steels?

Naval steels include various high-tensile, high-yield, alloy steels that are used mostly in marine applications, particularly for hulls of vessels and submarines. Typical representatives of these steels are 100 HLES, HY-80, HY-100, and others.
The general approach to machining high-strength steels is based on recommendations regarding alloy steels with similar strength and hardness characteristics.
What is PPSU and how is it machined?

PPSU is an acronym of polyphenylsulfone - a type of high temperature thermoplastic. Therefore, when machining PPSU, follow ISCAR's recommendations related to cutting thermoplastics.
When specifying materials to be machined, ISO standards use the letter “P” for steel, “M” for stainless steel, and “K” for cast iron. These letters are not directly associated with the material. However, when designating non-ferrous metals, superalloys, and hard materials, the ISO standard uses the letters” N”, “S” and “H”, which are appropriate acronyms. Can you explain a reason?

ISO adopted the material classification principles that were developed in Germany, and therefore, the origin of the identification letters is in German. For example, the letter “P” relates to the German word «Plastisch» (plastic), "K" to «Kurzspanend» (produced short chips), and "H" to "Hart" (hard), just to name a few.
Why does ISCAR continue to use outdated designations such as GGG for nodular cast iron when specifying engineering materials in different guides and ITA software?

The answer is very simple, outdated designations are still common in the industry and used by the manufacturer. Designations that begin with "GG" for gray cast iron, "GGG" for nodular cast iron (according to the old DIN standards), or "En" for steel (according to the old BS standards), have been replaced by other designations in their appropriate standards. However, despite the newer and formal changes, various outdated material designations are the everyday language of the professional world. Therefore, modern designations have been simultaneously preserved with a few outdated designations, which remain popular among manufacturing professionals.
As a side note, a similar situation may be observed with commercial names. Some materials are well known by their trademark and not by their standard designation.
What is considered high-temperature aluminum?

Generally, high-temperature aluminum is an aluminum alloy with more than 12% silicon content. This aluminum alloy is hypereutectic (also referred as to "hypereutectic aluminum"), while low thermal expansion and low specific gravity makes the alloy a typical material for hypereutectic pistons. From a machinability point of view, the high-temperature aluminum features considerable abrasiveness.
What is "pure iron" and how can it be machined?

Pure iron is the general name of low-carbon non-alloy steel that features an extremely high content of iron (Fe) with an overall trace of other chemical elements of up to 0.1%.
Pure iron is referred to commercially as ARMCO (American Rolling Mill Corporation). Shop talk language refers pure iron as "Armco-Iron". Also, pure iron is referred to as "soft magnetic iron".
To machine pure iron, it is recommended to follow ISCAR’s Group 1 (P1) - Material Group Classification guide when selecting the suitable cutting tool and determining the initial cutting data.
How to distinguish cold-rolled and hot-rolled steels by their designation?

Terms "hot rolled" or "cold rolled" relate to steel fabrication methods, and do not specify the composition or the mechanical properties of a steel, which are generally the main parameters for steel designation systems. However, in some cases technical documentation may use these terms or their abbreviations such as HR or CR for highlighting the method of fabrication.
High temperature superalloys comprise several types of materials. How can the machinability of these materials vary depending on the material type?

High temperature superalloys (HTSA) are divided into the three following groups depending on the prevailing element: iron (Fe)-, nickel (Ni)- and cobalt (Co)-based superalloys. Generally, machinability drops in the same order: from Fe- to Co-based HTSA. In addition, material fabrication method (casting, forging, sintering etc.) have impact on machinability within the group, too.
From the machinability point of view, are iron-based high temperature superalloys comparable with difficult-to-cut austenitic stainless steels?

Yes, correct.
What is "CPM steel"?

Acronym "CPM" means Crucible Particle Metallurgy – a powder metallurgy method of steelmaking which was developed by Crucible Industries.
How to machine Alumina Ceramics?

Alumina Ceramic is a general name for a whole group of aluminum-oxide-based ceramic materials that differ in the aluminum oxide (alumina) percentage and their substantial, properties. Due to the high hardness and low thermal conductivity, more common methods to machine Alumina Ceramics are abrasive machining, electro-discharge machining, laser-assistant cutting and others. As for "traditional" cutting, applying carbide tools usually requires the tools to be diamond coated. At the same time, some Alumina Ceramics grades of relatively low hardness (around 85 Shore D) may be machined by commonly coated carbide tools.
What is "cupronickel" and its machinability?

Cupronickel, which is also referred to as "copper nickel", "nickel copper" and "cupro-nickel", is a cooper alloy with Nickel as a main alloying element. Machinability of cupronickel is low when compared to common copper alloys.
What is "ultra-high carbon steel"?

In some steel classification systems high carbon steel that is extremely rich in carbon (usually exceeding 1% but it depends on the system) is named as "ultra-high carbon". The definitions such as "UHC steel" or "very high carbon steel" and abbreviation "UHCS" are common for designating such steels. Ultra-high carbon steel has increased strength yet brittle.
Which group of stainless steels precipitation hardened (PH) stainless steel belongs to: martensitic or austenitic?

Precipitation hardened stainless steel can be both martensitic and austenitic however, the most common of these steel types is martensitic. There is also semi-austenitic precipitation hardened stainless steel, which is austenitic when annealed, and martensitic when hardened.
Are austempered ductile iron (ADI) and austenitic nodular cast iron the same material?

No, these are different types of cast iron.
What is K-Alloy?

K-Alloy is a durable die-casting aluminum alloy that features high resistance to corrosion. K-Alloy also is referred as to A304.
What is free-cutting steel?

Free-cutting (or free-machining) steel is a collective name for carbon steels that feature the increased content of Sulphur when compared to common carbon steels with similar Carbon percentage. This attribute provides better machinability and chip control.
What is Tungsten-Copper and how to machine it?

Tungsten-Copper, which is also referred to as Copper-Tungsten, CuW, and WCu, is a composite material, a pseudo alloy, that contains Copper and Tungsten (Wolfram). Depending on the grade, the content of Copper (Cu) in this material typically varies between 10-50%. When compared to pure Tungsten, machining Copper-Tungsten is easier, and the higher the copper content, the better the machinability. Often the machinability of Copper-Tungsten alloys is like grey cast iron. However, effective machining of CuW grades with high copper percentage requires a more positive cutting geometry.
What is the difference between carbon steel and non-alloy steel?

The definitions "carbon steel", "non-alloy steel", and "unalloyed steel" relate to the classification of steel based on its chemical content. Generally, these definitions are considered synonymous. Steel is an alloy of iron and carbon that can also contain various alloying elements to enhance its properties. Steel is produced by smelting iron ore. During the smelting process, alloying elements can be added to steel, resulting in different grades of alloyed steel depending on the percentage of the added element. In the case of carbon (non-alloy, unalloyed) steel, no alloying element is added during smelting, making it a simple alloy of iron and carbon only. However, since iron ore is not completely pure, small quantities or traces of various elements are present in this alloy. National and international standards define the maximum allowable percentage of these elements to classify a steel grade as carbon steel.
What is the difference between brass and bronze?

Both brass and bronze are copper alloys, but brass is a group of copper-zinc alloys, while bronze is a group of copper-tin alloys.
What is electrical steel?

Electrical steel, also known as silicon steel, transformer steel, or e-steel, is an iron-silicon alloy, distinct from ordinary steel that is an iron-carbon alloy. The silicon content in common cold-rolled electrical steel typically does not exceed 3.2%, while in hot-rolled electrical steel, it can be higher, generally capped at 4.5%. Electric steel is commonly manufactured in the form of thin sheets, coils, and plates, and is often machined in stacks. It is worth noting that this steel is frequently delivered with an isolation layer.
What is the difference between "high temperature superalloys (HTSA)" and "heat resistant superalloys (HRSA)"?

Both definitions - "high temperature superalloys" and "heat resistant superalloys" - relate to alloys specifically intended for use in high temperature environments. Essentially, these terms describe alloys that possess high-temperature properties and can withstand elevated temperatures without significant degradation. Therefore, these terms are often used interchangeably in various contexts, but strictly speaking, there are some differences between the two.
"High temperature superalloys" (HTSA) generally refer to alloys designed to maintain their strength and mechanical properties at extremely high temperatures, typically above 1000°C (1832°F). These alloys are used in applications such as gas turbines, jet engines, and rocket propulsion systems.
On the other hand, "heat resistant superalloys" (HRSA) usually relate to alloys that exhibit good resistance to deformation and retain their mechanical properties at elevated temperatures ranging from 650°C (1202°F) to 1000°C (1832°F). These alloys are typically used in applications like heat exchangers, furnaces, and automotive components.

Tool Holding

What is a tool holder?

A tool holder is a device (a tool arrangement) for mounting a cutting tool in a machine tool. One of the tool holder ends carries the cutting tool while the other ends is clamped into the machine tool. Therefore the tool holder acts as an interface between the machine tool and the cutting tool.
Are the terms “tool holding” and “tooling” synonymous?

“Tool holding” is also referred to as “toolholding” and usually relates to tool holding systems that comprise various tool holders, such as arbors, chucks or adaptors, and their accessories (extensions, reducers, rings, sleeves, etc).
“Tooling” is a much broader definition. “Tooling” can refer to cutting tools together with tool- and work holding arrangements that are intended for a machine tool. “Tooling” relates sometimes to tool management and in certain circumstances it refers to tool holding systems.
Does ISCAR supply work holding devices?

No, ISCAR does not supply work holding devices. ISCAR’s products are cutting tools, tool holding, and tool management systems.
Does ISCAR provide tool holders with polygonal taper shank?

Yes. These tool holders are represented by ISCAR’s CAMFIX family.
What are the advantages of thermal (heat) shrink holders?
The advantages of tool holding, based on clamping tools with cylindrical shanks with the use of heat shrink fitting, are as follows:
- High accuracy
- High rigidity
- Excellent repeatability
- Reaches deep cavities due to slim holder design
- Balanced design and assembly’s symmetrical shape eliminate the production of centrifugal forces at high rotational speeds
Are ISCAR’s thermal shrink holders suitable for tools with steel shanks?

Yes. ISCAR’s SRKIN thermal shrink holders are intended for clamping tools with shanks made from cemented carbide, high speed steel (HSS) and steel. The SRKIN product line is fitted DIN69882-8, which is the shrink holder market standard.
ISCAR also produces SRK slim design shrink holders. SRK holders can be used for steel shanks but we recommend using them for carbide shanks.
Does ISCAR produce heating units for mounting cutting tools in thermal shrink holders?

Yes, ISCAR produces the induction heating unit for thermal shrink tool holding. In addition to this unit, ISCAR provides its simplified, “starter” version, which was designed to help the end-user purchase the shrink holding technology in a low cost device.
What are the main design features of X-STREAM SHRINKIN products? In which field would applying these products be the most effective?

X-STREAM SHRINKIN is a family of thermal shrink chucks with coolant jet channels along the shank bore. The family utilizes a patented design for holding tools with shanks, made from cemented carbide, steel or high-speed steel (HSS). The new chucks combine the advantages of high-precision heat shrink clamping with coolant flow, directed to cutting edges. X-STREAM SHRINKIN has already shown excellent performance in milling aerospace parts, particularly titanium blades and blisks (bladed discs), and especially in high speed milling. In machining deep cavities, the efficient cooling provided by the new chucks substantially improves chip evacuation and diminishes chip re-cutting.
What are the SPINJET products and where they are used?

ISCAR’s SPINJET is a family of coolant-driven compact high speed spindles for small diameter tools. It is a type of “booster” for upgrading existing machines to high speed performers. Depending on pressure and coolant flow rate, the spindles maintain a rotational speed of up to 55000 rpm. The versatile SPINJET products have been successfully integrated in tooling solutions for milling, drilling, thread milling, engraving, chamfering, deburring, and even fine radial grinding. The SPINJET spindles are recommended for tools up to 7 mm (.275 in) in diameter, however the optimal diameter range is 0.5-4 mm (.020-.157 in).
Does ISCAR deliver tool holders with identification chips?

ISCAR’s tool holders with HSK shanks incorporate holes for radio-frequency identification chips (RFID). ISCAR’s CAMFIX tool holders with polygonal taper shank of nominal size C4 (32 as specified by ISO 26623-1) and more are produced with this hole.
ISCAR can provide RFID chip mounting for all types of tool holder by special request.
Note: It is essential to adjust the tool holder after mounting an RFID chip.
Does ISCAR supply boring heads with digital displays?

Yes. ISCAR’s ITSBORE family contains adjustable boring heads with digital displays. These heads feature high adjusting accuracy and a simple adjusting process. A clear digital display with a mm/inch value display selection helps to prevent human errors.
What is the difference between mandrel and arbor?

There is no fundamental difference - both terms refer to a bar, usually rotating, that is used for mounting a machined workpiece or a cutting tool.
Does ISCAR supply tool holding devices for tapping?
Yes. Tool holding products for tapping include quick-change ER-type collets, holders with straight shanks and with 7:24 taper shanks, for example:
- GTI toolholders and straight shanks with floating compression/tension mechanism
- GTIN compact product line for tappng based on ER collets
- TCS/TCC quick-change system (part of the ITSBORE modular system)
What is "engineered balance"?

Engineered balance is a general name for design methods to make the mass distribution of a rotary body theoretically symmetrical with the body axis. Using these methods, engineers tried to ensure required balance parameters in the design stage, before production. 3D modelling in a CAD system environment significantly expands the engineered balance possibilities. As the engineered balance relates to virtual objects, it cannot replace a "physical" balancing of real parts. However, an engineered balance design substantially diminishes the mass unbalance of a future product and makes "physical" balancing much easier.
Engineered balance principles are a necessary feature for a skillful design of rotary tool holders.
Products with an engineered balance design are sometimes referred to as "balanced by design".

Shop Talk
Professional
slang

Metal cutting, like other fields of industrial activity, has its own professional jargon that is often used in shop talk. We decided to devote a separate section to more common jargon, even though they may appear already in the other FAQ sections.

Bi-hex – beseda se nanaša na orodje, ključ (nasadni ključ) 12 kotni.

Vskočnik - posebej zasnovan vzmetni vskočnik (obroč), ki za montažo potrebuje plitek utor.

Mik – mikrometer

Dvo-rezni rezkar – vrsta kotnega rezkarja, ki reže tudi v sredini in se lahko uporblja kot sveder. Dvo-rezni rezkarji so poznani tudi kot svedri za utore.

Counterboring and Countersinking

What is a zero flute countersink?

A zero flute countersink is a countersink with a cross through hole that extends through the side of the countersink cone. The intersection of the cone and the hole provides the cutting edge of the countersink. Also referred to as a "cross-hole countersink".
Are the cutting speeds for countersinking and drilling equal?

In countersinking, the cutting speeds are significantly lower when compared to drilling. There is one rule of thumb that is common for machine shop practice: the cutting speed for countersinking is around a third of the cutting speed, recommended for drilling the same material.