Titanium Machining Cost Savings with Helical Solutions

When the manufacturing team at Geospace Technologies was looking for better tool life and improved performance on a Titanium CNC milling job, they turned to Harvey Performance Company and local Application Engineer Mike Kanigowski to dial in some Helical Solutions End Mills. With Mike’s help, Geospace Technologies, led by Lead Mill Programmer Tranquilino Sosa, achieved massive success and cost-savings, which led them to completely shift their tooling repertoire to Helical’s high-performance end mills in their shop.

Struggling with Tool Life

Prior to switching to Helical, Geospace Technologies was experiencing trouble with tool life on a job that required both roughing and finishing toolpaths on a Titanium (Ti-6AL-4V) part. For their roughing pass, Geospace was using a competitor’s 4 flute, 3/8” diameter end mill with a 30° helix angle and TiALN coating. In traditional roughing toolpaths, this tool was running at 1,750 RPM with a 10 IPM feed rate. The tool would take four step downs, three with an axial depth of cut of .200”, and a final pass at .100” for a total depth of .700”.

When finishing, the team used a 1/2” version of the same competitor tool, running at 900 RPM with an 8 IPM feed rate. This would take two passes, one at .400” deep and the last down to the bottom of the part at .700”.

geospace technologies

With this strategy and tooling, the team was creating high-quality parts at a cycle time of 15 minutes and 22 seconds per part, but were only seeing the roughing tool last for 60 parts on average, and the finishing tool for around 120 parts. This was causing tool costs to be higher than they would like, and costing the team precious time with frequent tool changes.

Sosa had seen some of the success that other shops were having with Titanium milling using Helical Solutions end mills, and so they reached out to Kanigowski to see how Helical could help them lower their cost per part while achieving an even better finish.

Dialing in Tool Selection

When Mike got in touch with the team at Geospace, he knew there were some immediate benefits to changing the toolpaths used in this job. Using their ESPRIT software, the team was able to dial in a new program using high efficiency milling (HEM) toolpaths through ESPRIT’s “Profit Milling” technology.

With HEM toolpaths in place, Geospace was going to need new high performance tools to take full advantage of the programming adjustments. After much testing and evaluating several options from Helical’s extensive line of end mills for Titanium, Geospace settled on two solid tools.

Helical offers many different options for Titanium milling in HEM toolpaths. During testing, the team at Geospace decided on Helical EDP 59424, a 3/8” diameter, 7 flute, corner radius end mill. This tool features variable pitch geometry and offset chipbreakers for optimal chip evacuation, reduced harmonics, and minimized tool pressure, as well as Helical’s Aplus coating for high temperature resistance, decreased wear, and improved tool life.

7 flute chipbreaker
7 Flute Chipbeaker Tools Fresh Off the Grinder

When looking at the finishing toolpath, Geospace decided on Helical EDP 82566, a 3/8”, 6 flute, square end mill from Helical’s well known HEV-6 product line. This tool featured a variable pitch design to help mitigate chatter and leave a superior finish. While Helical also offers several tools for finishing toolpaths in Titanium, during testing this tool provided Geospace with the best finish for their specific part geometry.

HEV-6
Example of a Tool from Helical Solutions HEV-6 Tooling Line

Experiencing the “Helical Difference”

With the new tools in place, Sosa’s team reached out to Helical for help dialing in speeds and feeds. The Helical tech team was able to get them set up on Machining Advisor Pro, an advanced speeds and feeds calculator developed by the experts behind Helical Solutions tooling. With this “miracle worker” application in their arsenal, the team was able to easily dial in their new tools for their specific material grade, depth of cut, and machine setup.  

The team saw immediate positive results and cost-savings on this job. They were able to increase their roughing toolpaths to 4,500 RPM and 157 IPM. The finishing path remained largely the same, but resulted in a much improved final part. In total, cycle time dropped from 15 minutes and 22 seconds per part to 12 minutes and 17 seconds per part, which was great, but the improvement in tool life was where Sosa was most impressed.

titanium end mills

With the new Helical end mill in the shop, Geospace was able to run both tools for 580 parts with very minimal wear on the tool. This was a nearly 1000% improvement in tool life for their roughing passes and a 483% improvement in tool life for the finishing operation. In total, one roughing tool was able to last more than 42 hours in the cut before needing to be replaced.

Eliminating the need for a tool change every 60 parts was also a significant time-saver. Constant tool changes were causing serious machine downtime, which was eliminated with the longer tool life experienced with the Helical end mills. What seems like a minor inconvenience will truly add up to dozens of hours in saved time over the course of a few months for Sosa’s team.

titanium machining tool wear
A Closeup of the 7 Flute Chipbreaker After 42 Hours In The Cut

Geospace was thrilled with the results they saw on this Titanium job, as they had never experienced long tool life in Titanium with any other competitor brand. Sosa and his team are excited to continue using Helical Solutions product across all of their other jobs going forward and to continue working with Kanigowski and the Helical tech team on dialing in tool selection and speeds and feeds on future projects.

Please see below for a head-to-head breakdown of the Helical end mills’ performance in terms of total costs and productivity gained versus that of the competitor. These numbers are measured per 1,000 parts, taking into account tooling costs, tool change time, labor costs, running parameters, and cycle times.


titanium machining cost savings

Chipbreaker Tooling: Not Just for Roughing

When many people think about solid carbide tools with chip breakers, they are usually tooling up for a roughing application. While the chip breaker tool is a great choice for such applications, it can be utilized in a number of other areas too. In this post, we’ll examine many other benefits of the chip breaker style of tooling.

High Efficiency Milling (HEM)

High Efficiency Milling (HEM) uses CAM software to program advanced toolpaths that reduce cutting forces. These tool paths employ smaller end mills with a higher number of flutes (for a stronger core) running at higher speeds and feeds. This strategy includes a light radial depth of cut (RDOC), high axial depth of cut (ADOC), and a controlled angle of engagement.

Helical’s chipbreaking tools include serrated indents along the edge of flute for the entire length of cut. Because HEM utilizes heavy axial depths of cuts, these tools are able to break long chips into smaller ones. In addition to improving chip control and reducing cutting resistance, chipbreaker tools also help in decreasing heat load within the chips. This delays tool wear along the cutting edge and improves cutting performance. 

Check out this testimony from a Helical Solutions customer:

“We were able to get going with the 7 flute tools with the chipbreaker. I have to say the difference was INCREDIBLE! We can now rough the entire part with one tool. Also, the operator doesn’t have to open the door to clear chips hardly at all. We were able to rough and finish a 4.15 dia. bore 2 inches deep through the part without having to clear chips at all. Before we had to clear the chips out at least 15-20 times. Many thanks for your support.”

Slotting

When slotting, a major concern is chip control. A large buildup of chips can cause the recutting of chips, which adds a lot of heat back into the tool. Chip buildup can also cause a heavy amount of chattering. Both of these conditions are detrimental to tool life. A chip breaking tool can help reduce chip build-up when slotting which will extend tool life. Remember when slotting that 4 flute tools should be utilized in steel. For aluminum and other non- ferrous materials, a 3 flute tool is best.

Trochoidal Slotting

Trochoidal slotting is a form of slotting that uses HEM techniques to form a slot. Trochoidal milling implements a series of circular cuts to create a slot wider than the cutting tool’s cutting diameter. Using the logic listed in the earlier paragraphs of this article, a chipbreaker should be used when performing this operation.

Advantages of Trochoidal Slotting:

Decreased cutting forces

Reduced heat

Greater machining accuracy

Improved tool life

Faster cycle times

One tool for multiple slot sizes

Finishing

A little known fact about Helical’s chipbreaker style tool is that the chip breakers are offset flute to flute, which allows for a quality finish on the walls of the part. When utilizing light depths of cuts, high-quality finishes can be achieved.

Hardenability of Steel

Many types of steel have a beneficial response to a method of heat treatment known as quenching. One of the most important criteria in the selection process of a workpiece material is hardenability. Hardenability describes how deep a metal can be hardened upon quenching from high temperature, and can also be referred to as the depth of hardening.

Steel At Microscopic Scale:

The first level of classification of steels at a microscopic level is their crystal structure, the way in which atoms are arranged in space. Body-Centered Cubic (BCC) and Face Centered Cubic (FCC) configurations are examples of metallic crystal structures. Examples of BCC and FCC crystal structures can be seen below in Figure 1. Keep in mind that the images in Figure 1 are meant to display atomic position and that the distance between the atoms is exaggerated.

Figure 1: Example of a BCC crystal structure (left) and FCC crystal structure (right)

The next level of classification is a phase. A phase is a uniform portion of a material that has the same physical and chemical properties. Steel has 3 different phases:

  1. Austenite: Face-Centered cubic iron; also iron and steel alloys that have the FCC crystal structure.
  2. Ferrite: Body-centered cubic iron and steel alloys that have a BCC crystal structure.
  3. Cementite: Iron carbide (Fe3C)

The final level of classification discussed in this article is the microstructure. The three phases seen above can be combined to form different microstructures of steel. Examples of these microstructures and their general mechanical properties are shown below:

  • Martensite: the hardest and strongest microstructure, yet the most brittle
  • Pearlite: Hard, strong, and ductile but not particularly tough
  • Bainite: has desirable strength-ductility combination, harder than pearlite but not as hard as martensite

Hardening at Microscopic Scale:

The hardenability of steel is a function of the carbon content of the material, other alloying elements, and the grain size of the austenite. Austenite is a gamma phase iron and at high temperatures its atomic structure undergoes a transition from a BCC configuration to an FCC configuration.

High hardenability refers to the ability of the alloy to produce a high martensite percentage throughout the body of the material upon quenching. Hardened steels are created by rapidly quenching the material from a high temperature. This involves a rapid transition from a state of 100% austenite to a high percentage of martensite. If the steel is more than 0.15% carbon, the martensite becomes a highly strained body-centered cubic form and is supersaturated with carbon. The carbon effectively shuts down most slip planes within the microstructure, creating a very hard and brittle material. If the quenching rate is not fast enough, carbon will diffuse out of the austenitic phase. The steel then becomes pearlite, bainite, or if kept hot long enough, ferrite. None of the microstructures just stated have the same strength as martensite after tempering and are generally seen as unfavorable for most applications.

The successful heat treatment of a steel depends on three factors:

  1. The size and shape of the specimen
  2. The composition of the steel
  3. The method of quenching

1. The size and shape of the specimen

During the quenching process, heat must be transferred to the surface of the specimen before it can be dissipated into the quenching medium. Consequently, the rate at which the interior of the specimen cools is dependent on its surface area to volume ratio. The larger the ratio, the more rapid the specimen will cool and therefore the deeper the hardening effect. For example, a 3-inch cylindrical bar with a 1-inch diameter will have a higher hardenability than a 3-inch bar with a 1.5-inch diameter. Because of this effect, parts with more corners and edges are more amendable to hardening by quenching than regular and rounded shapes. Figure 2 is a sample time-temperature transformation (TTT) diagram of the cooling curves of an oil-quenched 95 mm bar. The surface will transform into 100% martensite while the core will contain some bainite and thus have a lower hardness.

Figure 2: Sample time temperature transformation (TTT) diagram also known as an isothermal transformation diagram

2.  The composition of the steel

It’s important to remember that different alloys of steel contain different elemental compositions. The ratio of these elements relative to the amount of iron within the steel yield a wide variety of mechanical properties. Increasing the carbon content makes steel harder and stronger but less ductile. The predominant alloying element of stainless steels in chromium, which gives the metal its strong resistance to corrosion. Since humans have been tinkering with the composition of steel for over a millennium, the number of combinations is endless.

Because there are so many combinations that yield so many different mechanical properties, standardized tests are used to help categorize different types of steel. A common test for hardenability is the Jominy Test, shown in Figure 3 below. During this test a standard block of material is heated until it is 100% austenite. The block is then quickly moved to an apparatus where it is water quenched. The surface, or the area in contact with the water, is immediately cooled and the rate of cooling drops as a function of distance from the surface. A flat is then ground onto the block along the length of the sample. The hardness at various points is measured along this flat. This data is then plotted in a hardenability chart with hardness as the y-axis and distance as the x-axis.

Figure 3: Diagram of a Jominy end quench specimen mounted during quenching (left) and post hardness testing (right)

Hardenability curves are constructed from the results of Jominy Tests. Examples of a few steel alloy curves are shown in Figure 4. With a diminishing cooling rate (steeper drop in hardness over a short distance), more time is allowed for carbon diffusion and the formation of a greater proportion of softer pearlite. This means less martensite and a lower hardenability. A material that retains higher hardness values over relatively long distances is considered highly hardenable. Also, the greater the difference in hardness between the two ends, the lower the hardenability. It is typical of hardenability curves that as the distance from the quenched end increases, the cooling rate decreases. 1040 steel initially has the same hardness as both 4140 and 4340 but cools extremely quickly over the length of the sample. 4140 and 4340 steel cool at a more gradual rate and therefore have a higher hardenability. 4340 has a less extreme rate of coolness relative to 4140 and thus has the highest hardenability of the trio.

Figure 4: Hardenability charts for 4140, 1040 and 4340 steels

Hardenability curves are dependent on carbon content. A greater percentage of carbon present in steel will increase its hardness. It should be noted that all three alloys in Figure 4 contain the same amount of carbon (0.40% C).  Carbon is not the only alloying element that can have an effect on hardenability. The disparity in hardenability behavior between these three steels can be explained in terms of their alloying elements. Table 1 below shows a comparison of the alloying content in each of the steels. 1040 is a plain carbon steel and therefore has the lowest hardenability as there are no other elements besides iron to block the carbon atoms from escaping the matrix. The nickel added to 4340 allows for a slightly greater amount of martensite to form compared to 4140, giving it the highest hardenability of these three alloys. Most metallic alloying elements slow down the formation of pearlite, ferrite and bainite, therefore they increase a steel’s hardenability.

Table 1: Shows the alloying contents of 4340, 4140, and 1040 steel

Type of Steel: Nickel (wt %): Molybdenum (wt %): Chromium (wt %):
4340 1.85% 0.25% 0.80%
4140 0.00% 0.20% 1.00%
1040 0.00% 0.00% 0.00%

There can be a variation in hardenability within one material group. During the industrial production of steel, there are always slight unavoidable variations in the elemental composition and average grain size from one batch to another. Most of the time a material’s hardenability is represented by maximum and minimum curves set as limits.

Hardenability also increases with increasing austenitic grain size. A grain is an individual crystal in a polycrystalline metal. Think of a stained glass window (like the one seen below), the colored glass would be the grains while the soldering material holding it altogether would be the grain boundaries. Austenite, ferrite, and cementite are all different types of grains that make up the different microstructures of steel. It is at the grain boundaries that the pearlite and bainite will form. This is detrimental to the hardening process as martensite is the desired microstructure, the other types get in the way of its growth. Martensite forms from the rapid cooling of austenite grains and its transformation process is still not well understood. With increasing grain size, there are more austenite grains and fewer grain boundaries. Therefore, there are fewer opportunities for microstructures like pearlite and bainite to form and more opportunities for martensite to form.

Figure 5: The colorful glass pieces represent grains of austenite which transforms into the desirable martensite upon quenching. The black portions in between the color portions represent grain boundaries. Sites where pearlite or bainite will form upon quenching.

3. The method of quenching

As previously stated, the type of quench affects the cooling rate. Using oil, water, aqueous polymer quenchants, or air will yield a different hardness through the interior of the workpiece. This also shifts the hardenability curves. Water produces the most severe quench followed by oil and then air. Aqueous polymer quenchants provide quenching rates between those of water and oil and can be tailored to specific applications by changing the polymer concentration and temperature. The degree of agitation also affects the rate of heat removal. The faster the quenching medium moves across the specimen, the greater the quenching effectiveness. Oil quenches are generally used when a water quench may be too severe for a type of steel as it may crack or warp upon treatment.

Figure 6: Metalworker quenching casts in an oil bath

Machining Hardened Steels:

The type of cutter that should be chosen for processing tools chosen for machining a workpiece after hardening depends on a few different variables. Not counting the geometric requirements specific to the application, two of the most important variables are the material hardness and its hardenability. Some relatively high-stress applications require a minimum of 80% martensite to be produced throughout the interior of the workpiece. Usually, moderately stressed parts only require about 50% martensite throughout the workpiece. When machining a quenched metal with very low hardenability a standard coated solid carbide tool may work without a problem. This is because the hardest portion of the workpiece is limited to its surface. When machining a steel with a high hardenability it is recommended that you use a cutter with specialized geometry that is for that specific application. High hardenability will result in a workpiece that is hard throughout its entire volume. Harvey Tool has a number of different cutters for hardened steel throughout the catalog, including drills, end mills, keyseat cutters, and engravers.

Summary:

Hardenability is a measure of the depth to which a ferrous alloy may be hardened by the formation of martensite throughout its entire volume, surface to core. It is an important material property you must consider when choosing a steel as well as cutting tools for a particular application. The hardening of any steel depends on the size and shape of the part, the molecular composition of the steel, and the type of quenching method used.

Grappling with Graphite: A Machining Guide

Despite being a softer material, graphite is actually one of the most difficult materials to machine. There are many considerations machinists need to make in terms of tooling, coolant use, and personal safety when it comes to machining graphite parts. This “In The Loupe” post will examine graphite’s material properties, the key machining techniques to consider, and tips for properly selecting cutting tools to achieve success in this tricky material.

What is Graphite?

While graphite is an allotrope of carbon, the two terms are not simply interchangeable. Carbon is an element that can form into several different allotropes including graphite, diamond, and fullerite. Graphite happens to be the most stable form of carbon, and is the most common, as carbon naturally occurs as graphite under standard conditions.

Graphite is most recognized for its superior conductivity and resistance to high heat and corrosion. This makes it a common material in high heat, high-pressure situations in the aerospace, electrode, nuclear, energy, and military industries.

graphite cnc material

Even though graphite can handle intense high-pressure situations with ease, it is actually a very soft, abrasive, and brittle material. This can cause serious challenges when machining, as graphite can eat up cutting tools, and severely minimize a tool’s usable life. However, with the proper tooling and techniques, there are ways to optimize graphite machining to be more cost-effective than the competition.

Graphite Machining Techniques

Since graphite is such a soft and brittle material, special consideration needs to be made when machining to avoid chipping it. To get a good cut, it is recommended that you take light chip loads and use lower feed rates in graphite. If you were to take a heavy cut at a fast feed rate, you would start chipping the graphite and could cause it to fracture completely. To give a comparison point, chip loads for graphite are similar to those for Aluminum materials, but with less than half the feed rate.

To give you an idea of speeds and feeds for graphite, here is an example using a 1/4″ Harvey Tool CVD Diamond Coated, 4 flute Square End Mill. If that tool was running at a standard RPM of 12,000 at 780 SFM, the recommended chip load would be .00292 for a feed rate of 140 IPM.

graphite electrode machining

In terms of machine setup, the one major tip to remember is to always avoid using coolant. Graphite is a fairly porous material, and so it can absorb coolant and act as a “coolant sponge,” which will cause problems with finished parts. Inside the machine and on the tooling, the coolant can actually react with the graphite dust and create an abrasive slurry, which will cause problems while machining. A vacuum system is recommended for clearing material while machining graphite. Otherwise, coated tools should be able to run dry.

Another thing to note when machining graphite is that because graphite does not produce chips, but rather a cloud of very abrasive dust, it can be harmful to operators and machines without proper care. Operators should be wearing a protective mask to avoid inhaling the graphite dust. Proper ventilation and maintaining air quality in the shop is also key for the protection of machinists when working in graphite.

Since the graphite dust is also extremely conductive, it can easily damage non-protective circuits inside your CNC machine, which can cause major electrical issues. While coolant is not recommended, a vacuum system can help to remove the dust, keeping it from accumulating too much inside the machine and preventing serious problems.

Cutting Tools for Graphite Machining

As previously mentioned, graphite is a notorious cutting tool-killer due to its extremely abrasive nature. Even the highest quality carbide end mills, if left uncoated, will wear quickly on most graphite jobs. This extreme wear may force a tool change during an operation, which could lead to an imperfection in the part when trying to restart the operation where the worn tool left off.

graphite cutting tools

When selecting a cutting tool for graphite machining, the coating and cutting edge is the most important consideration. Flute count, helix angles, and other key features of the tool geometry ultimately come second to the coating when purchasing tooling for graphite.

For graphite machining, a CVD (Chemical Vapor Deposition) diamond coating is recommended whenever possible to maximize tool life and tool performance. These coatings are grown directly into the carbide end mill, improving the hardness and leaving the tool with a coating layer that is 5 times thicker than a PVD Diamond Coating. While not the sharpest edge, the CVD diamond coating provides much longer tool life than other diamond coatings due to the thicker diamond layer.

Even though initial tooling costs may be higher with CVD coated tools versus uncoated tools, since CVD coated tools see considerably longer tool life than uncoated tools, this makes the cost per part shrink significantly. In difficult, abrasive materials like graphite, the uncoated carbide tool will last a short time before the abrasiveness of the graphite completely wears down the cutting edge. Having a CVD coated tool will give you a leg up over the competition, keep your machine running with less downtime for tool changes, and ultimately deliver substantial cost savings.

end mills for graphite
CVD Diamond Coated End Mill from Harvey Tool

Overall, graphite can be a difficult material to machine, but with the right cutting tools and proper speeds and feeds you will be making quality parts in no time. Harvey Tool offers a wide selection of CVD coated end mills in various diameters, reaches, and lengths of cut to ensure you have what you need for any job that comes your way.

High Efficiency Milling for Titanium Made Easy With Helical’s New HVTI Cutter

Titanium is a notoriously difficult material to machine, especially in aggressive toolpaths, such as those associated with High Efficiency Milling (HEM). Helical Solutions’ new line of tooling, the HVTI-6 series of end mills, is optimized specifically for this purpose, and proven to provide 20% more tool life than a competitor’s similar tool.

At face level, these new Helical end mills feature corner radius geometry, 6 flutes, and are Aplus coated for optimal tool life and increased cutting performance. But there is much more to these end mills than the typical geometry of standard 6 flute tools. The HVTI-6 was designed with a combination of a unique rake, core, and edge design that give it a leg up over standard 6 flute tools for Titanium while cutting HEM toolpaths. Click here to watch the HVTI-6 in action!

End Mills for Titanium

The design of the HVTI-6 was the result of significant testing by the Harvey Performance Company Innovation and New Product Development teams. These teams spent many months testing tools, doing in-depth analysis on materials and tool geometry, and pushing these tools through dozens of hours in the cut at testing sites across the country.

The new HVTI-6 cutter experienced higher metal removal rates (MRR) and 20% longer tool life while performing HEM in Titanium when compared to a standard 6 flute tool offered by a Helical Solutions competitor. This type of tool life improvement will produce huge cost savings on tooling, as well as shortened cycle times and lower cost per part.

Helical HVTI Titanium

The Harvey Performance Innovation team targeted Titanium grade Ti6Al4V for their testing, which accounts for the vast majority of the Titanium being machined in North America. The test part was designed and programmed to allow for a more defined agility test of the tool, taking the tool into key geometry cutting exercises like tight corners, long straight line cuts, and rapid movement.

Many hours were spent with Lyndex-Nikken, manufacturers of high-quality rotary tables, tool holders, and machining accessories, at their Chicago headquarters. By working with the team at Lyndex-Nikken, the Harvey Performance Company team was able to test under optimal conditions with top-of-the-line tool holders, work holding, and machining centers. Lyndex was also available to provide their expert support on tool holding techniques and were an integral part of the testing process for these tools. Video of the impressive test cuts taken at the Lyndex facility can be seen below.

WATCH THE HVTI IN ACTION

In these tests, the HVTI was able to run HEM toolpaths at 400 SFM and 120 IPM in Ti6Al4V, which served as the baseline for most of the testing.

While the standard 6 flute tools offered by Helical will still perform to high standards in Titanium and other hard materials (steels, exotic metals, cast iron), the HVTI-6 is a specialized, material-specific tool designed specifically for HEM toolpaths in Titanium. Advanced speeds and feeds for these new tools are already available in Machining Advisor Pro, and the complete offering is now available in the Helical CAM tool libraries for easy programming.

To learn more about the HVTI 6 Flute End Mills for Titanium, please visit the Helical Solutions website. To learn more about HEM techniques, download the HEM Guidebook for a complete guide on this advanced toolpath.

Selecting the Right Chamfer Cutter Tip Geometry

A chamfer cutter, or a chamfer mill, can be found at any machine shop, assembly floor, or hobbyist’s garage. These cutters are simple tools that are used for chamfering or beveling any part in a wide variety of materials. There are many reasons to chamfer a part, ranging from fluid flow and safety, to part aesthetics.

Due to the diversity of needs, tooling manufacturers offer many different angles and sizes of chamfer cutters, and as well as different types of chamfer cutter tip geometries. Harvey Tool, for instance, offers 21 different angles per side, ranging from 15° to 80°, flute counts of 2 to 6, and shank diameters starting at 1/8” up to 1 inch.

After finding a tool with the exact angle they’re looking for, a customer may have to choose a certain chamfer cutter tip that would best suit their operation. Common types of chamfer cutter tips include pointed, flat end, and end cutting. The following three types of chamfer cutter tip styles, offered by Harvey Tool, each serve a unique purpose.

Three Types of Harvey Tool Chamfer Cutters

Type I: Pointed

This style of chamfer cutter is the only Harvey Tool option that comes to a sharp point. The pointed tip allows the cutter to perform in smaller grooves, slots, and holes, relative to the other two types. This style also allows for easier programming and touch-offs, since the point can be easily located. It’s due to its tip that this version of the cutter has the longest length of cut (with the tool coming to a finished point), compared to the flat end of the other types of chamfer cutters. With only a 2 flute option, this is the most straightforward version of a chamfer cutter offered by Harvey Tool.

Type II: Flat End, Non-End Cutting

Type II chamfer cutters are very similar to the type I style, but feature an end that’s ground down to a flat, non-cutting tip. This flat “tip” removes the pointed part of the chamfer, which is the weakest part of the tool. Due to this change in tool geometry, this tool is given an additional measurement for how much longer the tool would be if it came to a point. This measurement is known as “distance to theoretical sharp corner,” which helps with the programming of the tool. The advantage of the flat end of the cutter now allows for multiple flutes to exist on the tapered profile of the chamfer cutter. With more flutes, this chamfer has improved tool life and finish. The flat, non-end cutting tip flat does limit its use in narrow slots, but another advantage is a lower profile angle with better angular velocity at the tip.

Type III: Flat End, End Cutting

Type III chamfer cutters are an improved and more advanced version of the type II style. The type III boasts a flat end tip with 2 flutes meeting at the center, creating a center cutting-capable version of the type II cutter. The center cutting geometry of this cutter makes it possible to cut with its flat tip. This cutting allows the chamfer cutter to lightly cut into the top of a part to the bottom of it, rather than leave material behind when cutting a chamfer. There are many situations where blending of a tapered wall and floor is needed, and this is where these chamfer cutters shine. The tip diameter is also held to a tight tolerance, which significantly helps with programing it.

In conclusion, there could be many suitable cutters for a single job, and there are many questions you must ask prior to picking your ideal tool. Choosing the right angle comes down to making sure that the angle on the chamfer cutter matches the angle on the part. One needs to be cautious of how the angles are called out, as well. Is the angle an “included angle” or “angle per side?” Is the angle called off of the vertical or horizontal? Next, the larger the shank diameter, the stronger the chamfer and the longer the length of cut, but now, interference with walls or fixtures need to be considered. Flute count comes down to material and finish. Softer materials tend to want less flutes for better chip evacuation, while more flutes will help with finish. After addressing each of these considerations, the correct style of chamfer for your job should be abundantly clear.

The Geometries and Purposes of a Slitting Saw

When a machinist needs to cut material significantly deeper than wide, a Slitting Saw is an ideal choice to get the job done. A Slitting Saw is unique due to its composition and rigidity, which allows it to hold up in a variety of both straightforward and tricky to machine materials.

What is a Slitting Saw?

A Slitting Saw is a flat (with or without a dish), circular-shaped saw that has a hole in the middle and teeth on the outer diameter. Used in conjunction with an arbor, a Slitting Saw is intended for machining purposes that require a large amount of material to be removed within a small diameter, such as slotting or cutoff applications.

Other names for Slitting Saws include (but are not limited to) Slitting Cutters, Slotting Cutters, Jewelers Saws, and Slitting Knives. Both Jewelers Saws and Slitting Knives are particular types of Slitting Saws. Jewelers Saws have a high tooth count enabling them to cut tiny, precise features, and Slitting Knives are Slitting Saws with no teeth at all. On Jewelers Saws, the tooth counts are generally much higher than other types of saws in order to make the cuts as accurate as possible.

Key Terminology

Why Use a Slitting Saw?

These saws are designed for cutting into both ferrous and non-ferrous materials, and by utilizing their unique shape and geometries, they can cut thin slot type features on parts more efficiently than any other machining tool.

Common Applications:

  1. Separating Two Pieces of Material
    1. If an application calls for cutting a piece of material, such as a rod, in half, then a slitting saw will work well to cut the pieces apart while increasing efficiency.
  2. Undercutting Applications
    1. Saws can perform undercutting applications if mounted correctly, which can eliminate the need to remount the workpiece completely.
  3. Slotting into Material
    1. Capable of creating thin slots with a significant depth of cut, Slitting Saws can be just the right tool for the job!

When Not to Use a Slitting Saw

While it may look similar to a stainless steel circular saw blade from a hardware store, a Slitting Saw should never be used with construction tools such as a table or circular saw.  Brittle saw blades such as slitting saws will shatter when used on manual machines, and can cause injury when not used on the proper set up.

In Conclusion

Slitting Saws can be beneficial to a wide variety of machining processes, and it is vital to understand their geometries and purpose before attempting to utilize them in the shop. They are a great tool to have in the shop and can assist with getting jobs done as quickly and efficiently as possible.

Chipbreakers vs. Knuckle Rougher End Mills

Knuckle Roughers and Chipbreakers are common profiles found on roughing end mills that, while fairly similar in appearance, actually serve different functions. Chipbreakers refer to the notches along the cutting edge of a tool that work to break up chips to prevent common evacuation mishaps. Knuckle Roughers refer to the serrated cutting edge of a tool, which works to enhance cutting action for an overall smoother operation.

Determining the appropriate style of tool is a very important first step to a successful roughing application.

Understanding the Two Styles

Chipbreaker End Mills

To aid chip evacuation, Chipbreaker End Mills feature a notched profile along the cutting edge that break down long chips into smaller, more manageable pieces. These tools are often utilized in aluminum jobs, as long, stringy chips are common with that material.

Each notch is offset flute-to-flute to enhance the surface finish on the part. This works by ensuring that as each flute rotates and impacts a part, following flutes work to clean up any marks or extra material that was left behind by the first pass. This leaves a semi-finished surface on your part.

In addition to improving chip control and reducing cutting resistance, these tools also help in decreasing heat load within the chips. This delays tool wear along the cutting edge and improves cutting performance. Not only are these tools great for hogging out a great deal of material, but they can be utilized in a wide array of jobs – from aluminum to steels. Further, a machinist can take full advantage of the unique benefits this tool possesses by utilizing High Efficiency Milling toolpaths, meant to promote efficiency and boost tool life.

Knuckle Roughers

Knuckle Rougher End Mills have a serrated cutting edge that generates significantly smaller chips than a standard end mill cutting edge. This allows for smoother machining and a more efficient metal removal process, similar to Chipbreaker End Mills. However, the serrations chop the chips down to much finer sizes, which allows more chips into the flutes during the evacuation process without any packing occurring.

Designed for steels, Knuckle Rougher End Mills are built to withstand harder materials and feature a large core. Because of this, these tools are great for roughing out a lot of material. However, due to the profile on the cutting edge, tracks along the wall can sometimes be left on a part. If finish is a concern, be sure to come in with a finishing tool after the roughing operation. Knuckle Roughers have proven the ability to run at higher chip loads, compared to similar end mills, which makes this a highly desired style for roughing. Further, this style of rougher causes a lot of heat and friction within the chips, so it’s important to run flood coolant when running this tool.

Key Differences Between Knuckle Roughers & Chipbreakers

While the two geometries offer similar benefits, it’s important to understand the distinct differences between them. Chipbreakers feature offset notches, which help to leave an acceptable finish on the walls of a part. Simply, the material left on an initial flute pass is removed by subsequent passes. A Knuckle Rougher does not feature this offset geometry, which can leave track marks on your part. Where part finish is of upmost importance, utilize a Knuckle Rougher to first hog out a great deal of steel, and work a final pass with a Finishing End Mill.

A unique benefit of Knuckle Roughers is the grind they possess – a cylindrical grind, compared to a relieved grind of a Chipbreaker End Mill. Because of this, Knuckle Roughers are easier to resharpen. Therefore, instead of buying a new tool, resharpening this profile is often a cheaper alternative.

Drill / End Mills: Drill Style vs. Mill Style

Drill / End Mills are one of the most versatile tools in a machinist’s arsenal. These tools can perform a number of different operations, freeing space on your carousel and improving cycle times by limiting the need for tool changes. These operations include:

  1. Drilling
  2. V-Grooving
  3. Milling
  4. Spot Drilling
  5. Chamfering

The ability of the Drill / End Mill to cut along the angled tip as well as the outer diameter gives it the range of operations seen above and makes it an excellent multi-functional tool.

drill mill operations

Drill Style vs. Mill Style

The main difference between Drill / End Mill styles is the point geometry.  They are defined by how the flutes are designed on the end of the tool, using geometry typically seen on either an end mill or a drill.  While mill style tools follow the features of an end mill or chamfer mill, the drill style geometry uses an S-gash at the tip.  This lends strength to the tip of the tool, while giving it the ability to efficiently and accurately penetrate material axially.  While both styles are capable of OD milling, mill style tools will be better for chamfering operations, while drill style will excel in drilling.  The additional option of the Harvey Tool spiral tipped Drill / End Mill is an unprecedented design in the industry.  This tool combines end geometry taken from our helical flute chamfer cutters with a variable helix on the OD for enhanced performance. Versatility without sacrificing finish and optimal performance is the result.

drill mills

Left to Right: 2 Flute Drill Style End, 2 Flute Mill Style End, 4 Flute Mill Style End

Drill Mills: Tool Offering

Harvey Tool currently offers Drill / End Mills in a variety of styles that can perform in different combinations of machining applications:

Mill Style – 2 Flute

This tool is designed for chamfering, milling, drilling non-ferrous materials, and light duty spotting. Drilling and spotting operations are recommended only for tools with an included angle greater than 60°. This is a general rule for all drill mills with a 60° point. Harvey Tool stocks five different angles of 2 flute mill-style Drill / End Mills, which include 60°, 82°, 90°, 100° and 120°. They are offered with an AlTiN coating on all sizes as well as a TiB2 coating for cutting aluminum with a 60° and 90° angle.

drill mill

Mill Style – 4 Flute

4 flute mill-style Drill / End Mills have two flutes that come to center and two flutes that are cut back. This Drill / End Mill is designed for the same operations as the 2 flute style, but has a larger core in addition the higher flute count. The larger core gives the tool more strength and allows it to machine a harder range of materials. The additional flutes create more points of contact when machining, leading to better surface finish. AlTiN coating is offered on all 5 available angles (60°, 82°, 90°, 100°, and 120°) of this tool for great performance in a wide array of ferrous materials.

drill mill

Drill Style – 2 Flute

This tool is specifically designed for the combination of milling, drilling, spotting and light duty chamfering applications in ferrous and non-ferrous materials. This line is offered with a 90°, 120°, and 140° included angle as well as AlTiN coating.

drill mills drill style

Helical Tip – 4 Flute

The Helically Tipped Drill / End Mill offers superior performance in chamfering, milling and light duty spotting operations. The spiral tip design allows for exceptional chip evacuation and surface finish. This combined with an OD variable helix design to reduce chatter and harmonics makes this a valuable tool in any machine shop. It is offered in 60°, 90°, and 120° included angles and comes standard with the latest generation AlTiN Nano coating that offers superior hardness and heat resistance.

 

Introduction to High Efficiency Milling

The following is just one of several blog posts relevant to High Efficiency Milling. To achieve a full understanding of this popular machining method, view any of the additional HEM posts below!

High Speed Machining vs. HEM I How to Combat Chip Thinning I Diving into Depth of Cut I How to Avoid 4 Major Types of Tool Wear I Intro to Trochoidal Milling


High Efficiency Milling (HEM) is a strategy that is rapidly gaining popularity in the metalworking industry. Most CAM packages now offer modules to generate HEM toolpaths, each with their own proprietary name. In these packages, HEM can also be known as Dynamic Milling or High Efficiency Machining, among others. HEM can result in profound shop efficiency, extended tool life, greater performance, and cost savings. High performance end mills designed to achieve higher speeds and feeds will help machinists to reap the full benefits of this popular machining method.

High Efficiency Milling Defined

HEM is a milling technique for roughing that utilizes a lower Radial Depth of Cut (RDOC) and a higher Axial Depth of Cut (ADOC). This spreads wear evenly across the cutting edge, dissipates heat, and reduces the chance of tool failure.

This strategy differs from traditional or conventional milling, which typically calls for a higher RDOC and lower ADOC. Traditional milling causes heat concentrations in one small portion of the cutting tool, expediting the tool wear process. Further, while Traditional Milling call for more axial passes, HEM toolpaths use more passes radially.

For more information on optimizing Depth of Cut in relation to HEM, see Diving into Depth of Cut: Peripheral, Slotting & HEM Approaches.

High Efficiency Milling

Built-In CAM Applications

Machining technology has been advancing with the development of faster, more powerful machines. In order to keep up, many CAM applications have developed built-in features for HEM toolpaths, including Trochoidal Milling, a method of machining used to create a slot wider than the cutting tool’s cutting diameter.

HEM is largely based on the theory surrounding Radial Chip Thinning, or the phenomenon that occurs with varying RDOC, and relates to the chip thickness and feed per tooth. HEM adjusts parameters to maintain a constant load on the tool through the entire roughing operation, resulting in more aggressive material removal rates (MRR). In this way, HEM differs from other high performance toolpaths, which involve different methods for achieving significant MRR.

Virtually any CNC machine can perform HEM – the key is a fast CNC controller. When converting from a regular program to HEM, about 20 lines of HEM code will be written for every line of regular code. A fast processor is needed to look ahead for the code, and keep up with the operation. In addition, advanced CAM software that intelligently manages tool load by adjusting the IPT and RDOC is also needed.

HEM Case Studies

The following example shows the result a machinist had when using a Helical Solutions HEV-5 tool to perform an HEM operation in 17-4PH stainless steel. While performing HEM, this ½” diameter, 5-flute end mill engaged the part just 12% radially, but 100% axially. This machinist was able to reduce tool wear and was able to complete 40 parts with a single tool, versus only 15 with a traditional roughing toolpath.

The effect of HEM on a roughing application can also be seen in the case study below. While machining 6061 aluminum with Helical’s H45AL-C-3, a 1/2″, 3-flute rougher, this machinist was able to finish a part in 3 minutes, versus 11 minutes with a traditional roughing toolpath. One tool was able to make 900 parts with HEM, a boost of more than 150% over the traditional method.

Importance of Tooling to HEM

Generally speaking, HEM is a matter of running the tool – not the tool itself. Virtually every tool can perform HEM, but using tooling built to withstand the rigors of HEM will result in greater success. While you can run a marathon in any type of shoes, you’d likely get the best results and performance from running shoes.

HEM is often regarded as a machining method for larger diameter tooling because of the aggressive MRR of the operation and the fragility of tooling under 1/8” in size. However, miniature tooling can be used to achieve HEM, too.

Using miniature tooling for HEM can create additional challenges that must be understood prior to beginning your operation.

Best Tools for HEM:

  • High flute count for increased MRR.
  • Large core diameter for added strength.
  • Tool coating optimized for the workpiece material for increased lubricity.
  • Variable Pitch/Variable Helix design for reduced harmonics.

Key Takeaways

HEM is a machining operation which continues to grow in popularity in shops worldwide. A milling technique for roughing that utilizes a lower RDOC and higher ADOC than traditional milling, HEM distributes wear evenly across the cutting edge of a tool, reducing heat concentrations and slowing the rate of tool wear. This is especially true in tooling best suited to promote the benefits of HEM.