Chip Thickness

Tag Archive for: Chip Thickness

How to Optimize Results While Machining With Miniature End Mills

July 1, 2020/0 Comments/in Harvey Tool, How-To's, Machining Techniques, Milling, Milling/by Robert Keever

The machining industry generally considers micromachining and miniature end mills to be any end mill with a diameter under 1/8 of an inch. This is also often the point where tolerances must be held to a tighter window. Because the diameter of a tool is directly related to the strength of a tool, miniature end mills are considerably weaker than their larger counterparts, and therefore, lack of strength must be accounted for when micromachining. If you are using these tools in a repetitive application, then optimization of this process is key.

Size Comparison for Harvey Tool’s #13901 Square Miniature End Mill

Key Cutting Differences Between Conventional and Miniature End Mills

Runout

Runout during an operation has a much greater effect on miniature tools, as even a very small amount can have a large impact on the tool engagement and cutting forces. Runout causes the cutting forces to increase due to the uneven engagement of the flutes, prompting some flutes to wear faster than others in conventional tools, and breakage in miniature tools. Tool vibration also impacts the tool life, as the intermittent impacts can cause the tool to chip or, in the case of miniature tools, break. It is extremely important to check the runout of a setup before starting an operation. The example below demonstrates how much of a difference .001” of runout is between a .500” diameter tool and a .031” diameter tool.

The ratio between the chip thickness and the edge radius (the edge prep) is much smaller for miniature tools. This phenomena is sometimes called “the size effect” and often leads to an error in the prediction of cutting forces. When the chip thickness-to-edge radius ratio is smaller, the cutter will be more or less ploughing the material rather than shearing it. This ploughing effect is essentially due to the negative rake angle created by the edge radius when cutting a chip with a small thickness.

If this thickness is less than a certain value (this value depends of the tool being used), the material will squeeze underneath the tool. Once the tool passes and there is no chip formation, part of the plowed material recovers elastically. This elastic recovery causes there to be higher cutting forces and friction due to the increased contact area between the tool and the workpiece. These two factors ultimately lead to a greater amount of tool wear and surface roughness.

chart of edge radius in relation to chip thickness for micromachining — Figure 1: (A) Miniature tool operation where the edge radius is greater than the chip thickness (B) Conventional operation where the edge radius is small than the chip thickness

Tool Deflection in Conventional vs. Micromachining Applications

Tool deflection has a much greater impact on the formation of chips and accuracy of the operation in micromachining operations, when compared to conventional operations. Cutting forces concentrated on the side of the tool cause it to bend in the direction opposite the feed. The magnitude of this deflection depends upon the rigidity of the tool and its distance extended from the spindle. Small diameter tools are inherently less stiff compared to larger diameter tools because they have much less material holding them in place during the operation. In theory, doubling the length sticking out of the holder will result in 8 times more deflection. Doubling the diameter of an end mill it will result in 16 times less deflection. If a miniature cutting tool breaks on the first pass, it is most likely due to the deflection force overcoming the strength of the carbide. Here are some ways you can minimize tool deflection.

Workpiece Homogeny

Workpiece homogeny becomes a questionable factor with decreasing tool diameter. This means that a material may not have uniform properties at an exceptionally small scale due to a number of factors, such as container surfaces, insoluble impurities, grain boundaries, and dislocations. This assumption is generally saved for tools that have a cutter diameter below .020”, as the cutting system needs to be extremely small in order for the homogeny of the microstructure of the material to be called into question.

Surface Finish

Micromachining may result in an increased amount of burrs and surface roughness when compared to conventional machining. In milling, burring increases as feed increases, and decreases as speed increases. During a machining operation, chips are created by the compression and shearing of the workpiece material along the primary shear zone. This shear zone can be seen in Figure 2 below. As stated before, the chip thickness-to-edge radius ratio is much higher in miniature applications. Therefore, plastic and elastic deformation zones are created during cutting and are located adjacent to the primary shear zone (Figure 2a). Consequently, when the cutting edge is close to the border of the workpiece, the elastic zone also reaches this border (Figure 2b). Plastic deformation spreads into this area as the cutting edge advances, and more plastic deformation forms at the border due to the connecting elastic deformation zones (Figure 2c). A permanent burr begins to form when the plastic deformation zones connect (Figure 2d) and are expanded once a chip cracks along the slip line (Figure 2e). When the chips finally break off from the edge of the workpiece, a burr is left behind (Figure 2f).

burr formation mechanism using a miniature end mill — Figure 2: Burr formation mechanism using a miniature end mill

Tool Path Best Practices for Miniature End Mills

Because of the fragility of miniature tools, the tool path must be programmed in such a way as to avoid a sudden amount of cutting force, as well as permit the distribution of cutting forces along multiple axes. For these reasons, the following practices should be considered when writing a program for a miniature tool path:

Ramping Into a Part

Circular ramping is the best practice for moving down axially into a part, as it evenly distributes cutting forces along the x, y, and z planes. If you have to move into a part radially at a certain depth of cut, consider an arching tool path as this gradually loads cutting forces onto the tool instead of all at once.

Micromachining in Circular Paths

You should not use the same speeds and feed for a circular path as you would for a linear path. This is because of an effect called compounded angular velocity. Each tooth on a cutting tool has its own angular velocity when it is active in the spindle. When a circular tool path is used, another angular velocity component is added to the system and, therefore, the teeth on the outer portion of tool path are traveling at a substantially different speed than expected. The feed of the tool must be adjusted depending on whether it is an internal or external circular operation. To find out how to adjust your feed, check out this article on running in circles.

Slotting with a Miniature End Mill

Do not approach a miniature slot the same way as you would a larger slot. With a miniature slot, you want as many flutes on the tool as possible, as this increases the rigidity of the tool through a larger core. This decreases the possibility of the tool breaking due to deflection. Because there is less room for chips to evacuate with a higher number of flutes, the axial engagement must be decreased. With larger diameter tools you may be stepping down 50% – 100% of the tool diameter. But when using miniature end mills with a higher flute count, only step down between 5% – 15%, depending on the size of the diameter and risk of deflection. The feed rate should be increased to compensate for the decreased axial engagement. The feed can be increased even high when using a ball nose end mill as chip thinning occurs at these light depths of cut and begins to act like a high feed mill.

Slowing Down Your Feed Around Corners

Corners of a part create an additional amount of cutting forces as more of the tool becomes engaged with the part. For this reason it is beneficial to slow down your feed when machining around corners to gradually introduce the tool to these forces.

Climb Milling vs. Conventional Milling in Micromachining Applications

This is somewhat of a tricky question to answer when it comes to micromachining. Climb milling should be utilized whenever a quality surface finish is called for on the part print. This type of tool path ultimately leads to more predictable/lower cutting forces and therefore higher quality surface finish. In climb milling, the cutter engages the maximum chip thickness at the beginning of the cut, giving it a tendency to push away from the workpiece. This can potentially cause chatter issues if the setup does not have enough rigidity. In conventional milling, as the cutter rotates back into the cut it pulls itself into the material and increases cutting forces. Conventional milling should be utilized for parts with long thin walls as well as delicate operations.

Combined Roughing and Finishing Operations

These operations should be considered when micromachining tall thin walled parts as in some cases there is not sufficient support for the part for a finishing pass.

Helpful Tips for Achieving Successful Micromachining Operations With Miniature End Mills

Try to minimize runout and deflection as much as possible when micromachining with miniature end mills. This can be achieved by using a shrink-fit or press-fit tool holder. Maximize the amount of shank contact with the collet while minimizing the amount of stick-out during an operation. Double check your print and make sure that you have the largest possible end mill because bigger tools mean less deflection.

Choose an appropriate depth of cut so that the chip thickness to edge radius ratio is not too small as this will cause a ploughing effect.
If possible, test the hardness of the workpiece before machining to confirm the mechanical properties of the material advertised by the vender. This gives the operator an idea of the quality of the material.
Use a coated tool if possible when working in ferrous materials due to the excess amount of heat that is generated when machining these types of metals. Tool coatings can increase tool life between 30%-200% and allows for higher speeds, which is key in micro-machining.
Consider using a support material to control the advent of burrs during a micromachining application. The support material is deposited on the workpiece surface to provide auxiliary support force as well as increase the stiffness of the original edge of the workpiece. During the operation, the support material burrs and is plastically deformed rather than the workpiece.
Use flood coolant to lower cutting forces and a greater surface finish.
Scrutinize the tool path that is to be applied as a few adjustments can go a long way in extending the life of a miniature tool.
Double-check tool geometry to make sure it is appropriate for the material you are machining. When available, use variable pitch and variable helix tools as this will reduce harmonics at the exceptionally high RPMs that miniature tools are typically run at.

variable pitch versus non-variable pitch — Figure 3: Variable pitch tool (yellow) vs. a non-variable pitch tool (black)

The Geometries and Purposes of a Slitting Saw

September 10, 2019/7 Comments/in CNC Machining, Harvey Tool, Machining Techniques, Tool Geometry, Tool Information Guides, Tool Selection/by Harvey Performance Company

When a machinist needs to cut material significantly deeper than wide, a Slitting Saw is an ideal choice to get the job done. These are unique due to their 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 tool that has a hole in the middle and teeth on the outer diameter. Used in conjunction with an arbor, this tool 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 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 saws. Jewelers Saws have a high tooth count enabling them to cut tiny, precise features, and Slitting Knives have 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. Non-Ferrous slitting saws have fewer teeth, allowing for aggressively deep depths of cut.

Common Applications:

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.
Undercutting Applications
1. Saws can perform undercutting applications if mounted correctly, which can eliminate the need to remount the workpiece completely.
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, this tool should never be used with construction tools such as a table or circular saw. Brittle saw blades 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.

Machining Precious Metals

July 1, 2019/10 Comments/in How-To's, Machining Techniques, Material Specific/by Robert Keever

Precious metals can be particularly difficult to machine due to their wide range of material properties and high cost if a part has to be scrapped. The following article will introduce these elements and their alloys as well as provide a guide on how to machine them effectively and efficiently.

About the Elements

Sometimes called “noble” metals, precious metals consist of eight elements that lie in the middle of the periodic table (seen below in Figure 1). The eight metals are:

Ruthenium (Ru)
Rhodium (Rh)
Palladium (Pd)
Silver (Ag)
Osmium (Os)
Iridium (Ir)
Platinum (Pt)
Gold (Au)

These elements are some of the rarest materials on earth, and can therefore be enormously expensive. Gold and silver can be found in pure nugget form, making them more easily available. However, the other six elements are typically found mixed in the raw ore of the four metals they sit below on the periodic table: Iron (Fe), Cobalt (Co), Nickel (Ni), and Copper (Cu). These elements are a subset of precious metals and are generally called Platinum Group Metals (PGM). Because they are found together in raw ore, this makes mining and extraction difficult, dramatically increasing their cost. Because of their high price tag, machining these materials right the first time is incredibly important to a shop’s efficiency.

Figure 1: Periodic table with the 8 precious metals boxed in blue. Image source: clearscience.tumblr.com

Basic Properties and Compositions of Precious Metals

Precious metals have notable material properties as they are characteristically soft, ductile, and oxidation resistant. They are called “noble” metals because of their resistance to most types of chemical and environmental attack. Table 1 lists a few telling material properties of precious metals in their elemental form. For comparison purposes, they are side-by-side with 6061 Al and 4140 Steel. Generally, only gold and silver are used in their purest form as the platinum group metals are alloys that consist mainly of platinum (with a smaller composition of Ru, Rh, Pa, Os, Ir). Precious metals are notable for being extremely dense and having a high melting point, which make them suitable for a variety of applications.

Table 1: Cold-worked Material Properties of Precious Metals, 4140 Steel and 6061 Aluminum

Common Machining Applications of Precious Metals

Silver and gold have particularly favorable thermal conductivity and electrical resistivity. These values are listed in Table 2, along with CC1000 (annealed copper) and annealed 6061 aluminum, for comparison purposes. Copper is generally used in electrical wiring because of its relatively low electrical resistivity, even though silver would make a better substitute. The obvious reason this isn’t the general convention is the cost of silver vs. copper. That being said, copper is generally plated with gold at electrical contact areas because it tends to oxide after extended use, which lowers its resistivity. As stated before, gold and the other precious metals are known to be resistant to oxidation. This corrosion resistance is the main reason that they are used in cathodic protection systems of the electronics industry.

Table 2: Thermal Conductivity and Electrical Resistivity of Ag, Au, Cu, and Al

Platinum and its respective alloys offer the most amount of applications as it can achieve a number of different mechanical properties while still maintaining the benefits of a precious metal (high melting point, ductility, and oxidation resistance). Table 3 lists platinum and a number of other PGMs each with their own mechanical properties. The variance of these properties depends on the alloying element(s) being added to the platinum, the percentage of alloying metal, and whether or not the material has been cold-worked or annealed. Alloying can significantly increase the tensile strength and hardness of a material while decreasing its ductility at the same time. The ratio of this tensile strength/hardness increase to ductility decrease depends on the metal added as well as how much is added, as seen in Table 3. Generally this depends on the particle size of the element added as well as its natural crystalline structure. Ruthenium and Osmium have a specific crystal structure that has a significant hardening effect when added to platinum. Pt-Os alloys in particular are extremely hard and practically unworkable, which doesn’t yield many real-world applications. However, the addition of the other 4 PGMs to platinum allow for a range of mechanical properties with various usages.

Table 3: PGM material properties (Note: the hardness and tensile strength are cold worked values)

Platinum and its alloys are biocompatible, giving them the ability to be placed in the human body for long periods of time without causing adverse reactions or poisoning. Therefore, medical devices including heart muscle screw fixations, stents, and marker bands for angioplasty devices are made from platinum and its alloys. Gold and palladium are also commonly used in dental applications.

Pt-Ir alloys are noticeably harder and stronger than any of the other alloys and make excellent heads for spark plugs in the automobile industry. Rhodium is sometimes added to Pt-Ir alloys to make the material less springy (as they are used as medical spring wire) while also increasing its workability. Pt and Pt-Rh wire pairs are extremely effective at measuring temperatures and are therefore used in thermocouples.

Machining Precious Metals

The two parameters that have the most effect when machining are hardness and percent elongation. Hardness is well-known by machinists and engineers across the manufacturing industry as it indicates a material’s resistance to deformation or cutting. Percent elongation is a measurement used to quantify material ductility. It indicates to a designer the degree to which a structure will deform plastically (permanently) before fracture. For example, a ductile plastic such as ultrahigh molecular weight polyethylene (UHMWPE) has a percent elongation of 350-525%, while a more brittle material such as oil-quenched and tempered cast iron (grade 120-90-02) has a percent elongation of about 2%. Therefore, the greater the percent elongation, the greater the material’s “gumminess.” Gummy materials are prone to built-up edge and have a tendency to produce long stringy chips.

Tools for Precious Metals

Material ductility makes a sharp cutting tool essential for cutting precious metals. Variable Helix for Aluminum Alloy tools can be used for the softer materials such as pure gold, silver, and platinum.

Figure 2: Variable Helix Square End Mill for Aluminum Alloys

Higher hardness materials still require a sharp cutting edge. Therefore, one’s best option is to invest in a PCD Diamond tool. The PCD wafer has the ability to cut extremely hard materials while maintaining a sharp cutting edge for a relatively long period of time, compared to standard HSS and carbide cutting edges.

Figure 3: PCD Diamond Square End Mill

Speeds and Feeds charts:

Figure 4: Speeds and Feeds for precious metals when using a Square Non-ferrous, 3x LOC

Figure 5: Speeds and Feeds for precious metals when using a 2-Flute Square PCD end mill

What to Know About Helical Solution’s Zplus Coating

April 1, 2019/0 Comments/in Aluminum, CNC Machining, Helical Solutions, Machining Techniques, Material Specific, Tool Coatings, Tool Selection/by Harvey Performance Company

Non-ferrous and non-metallic materials are not usually considered difficult to machine, and therefore, machinists often overlook the use of tool coatings. But while these materials may not present the same machining difficulties as hardened steels and other ferrous materials, a coating can still vastly improve performance in non-ferrous applications. For instance, materials such as aluminum and graphite can cause machinists headaches because of the difficulty they often create from abrasion. To alleviate these issues in non-ferrous machining applications, a popular coating choice is Helical Solution’s Zplus coating.

What is Helical Solutions’ Zplus Coating?

Helical’s Zplus is a Zirconium Nitride-based coating, applied by a Physical Vapor Deposition (PVD) process. This method of coating takes place in a vacuum and forms layers only microns thick onto the properly prepared tool. Zirconium Nitride does not chemically react to a variety of non-ferrous metals, increasing the lubricity of the tool and aiding in chip evacuation.

When Should a Machinist Use Helical Solution’s Zplus?

Working with Abrasive Materials

While Zplus was created initially for working in aluminum, its hardness level and maximum working temperature of 1,110°F enables it to work well in abrasive forms of other non-ferrous materials, as well. This coating decreases the coefficient of friction between the tool and the part, allowing it to move easier through more abrasive materials. This abrasion resistance decreases the rate of tool wear, prolonging tool life.

Concerns with Efficient Chip Evacuation

One of the primary functions of this coating is to increase the smoothness of the flutes of the tool, which allows for more efficient chip removal. By decreasing the amount of friction between the tool and the material, chips will not stick to the tool, helping to prevent chip packing. The increased lubricity and smoothness provided by the coating allows for a higher level of performance from the cutting tool. Zplus is also recommended for use in softer, gummy alloys, as the smooth surface encourages maximum lubricity within the material – this decreases the likelihood of those gummier chips sticking to the tool while machining.

Large Production Runs

Uncoated tools can work well in many forms of non-ferrous applications. However, to get a genuinely cost-effective tool for your job, the proper coating is highly recommended. Large production runs are known for putting a lot of wear and tear on tools due to their increased use, and by utilizing an appropriate coating, there can be a significant improvement in the tools working life.

3 flute corner radius end mill for aluminum

When is Zplus Coating Not Beneficial to My Application?

Finishing Applications

When your parts finish is vital to its final application, a machinist may want to consider going with an uncoated tool. As with any coating, ZrN will leave a very minor rounded edge on the tip of the cutting edge. The best finish often requires an extremely sharp tool, and an uncoated tool will have a sharper cutting edge than its coated version.

Effective Ways to Reduce Heat Generation

October 25, 2018/1 Comment/in High Efficiency Milling, How-To's, Machining Techniques, Quick Tips/by Guy Petrillo

Any cutting tool application will generate heat, but knowing how to counteract it will improve the life of your tool. Heat can be good and doesn’t need to totally be avoided, but controlling heat will help prolong your tool life. Sometimes, an overheating tool or workpiece is easy to spot due to smoke or deformation. Other times, the signs are not as obvious. Taking every precaution possible to redirect heat will prolong your tool’s usable life, avoid scrapped parts, and will result in significant cost savings.

Reduce Heat Generation with HEM Tool Paths

High Efficiency Milling (HEM), is one way a machinist should explore to manage heat generation during machining. HEM is a roughing technique that uses the theory of chip thinning by applying a smaller radial depth of cut (RDOC) and a larger axial depth of cut (ADOC). HEM uses RDOC and ADOC similar to finishing operations but increases speeds and feeds, resulting in greater material removal rates (MRR). This technique is usually used for removing large amounts of material in roughing and pocketing applications. HEM utilizes the full length of cut and more effectively uses the full potential of the tool, optimizing tool life and productivity. You will need to take more radial passes on your workpiece, but using HEM will evenly spread heat across the whole cutting edge of your tool, instead of building heat along one small portion, reducing the possibility of tool failure and breakage.

Chip Thinning Awareness

Chip thinning occurs when tool paths include varying radial depths of cut, and relates to chip thickness and feed per tooth. HEM is based off of the principal of chip thinning. However, if not properly executed, chip thinning can cause a lot of heat generation. When performing HEM, you effectively reduce your stepover and increase your speeds and feeds to run your machine at high rates. But if your machine isn’t capable of running high enough speeds and feeds, or you do not adjust accordingly to your reduced stepover, trouble will occur in the form of rubbing between the material and tool. Rubbing creates friction and mass amounts of heat which can cause your material to deform and your tool to overheat. Chip thinning can be good when used correctly in HEM, but if you fall below the line of reduced stepover without higher speeds and feeds, you will cause rubbing and tool failure. Because of this, it’s always important to be aware of your chips during machining.

Consider Climb Milling

There are two ways to cut materials when milling: conventional milling and climb milling. The difference between the two is the relationship of the rotation of the cutter to the direction of feed. In climb milling, the cutter rotates with the feed, as opposed to conventional milling where the cutter rotates against the feed.

When conventional milling, chips start at theoretical zero and increase in size, causing rubbing and potentially work hardening. For this reason, it’s usually recommended for tools with higher toughness or for breaking through case hardened materials.

In climb milling, the chip starts at maximum width and decreases, causing the heat generated to transfer into the chip instead of the tool or workpiece. When going from max width to theoretical zero, heat will be transferred to the chip and pushed away from the workpiece, reducing the possibility of damage to the workpiece. Climb milling also produces a cleaner shear plane which will cause less tool rubbing, decreasing heat and improving tool life. When climb milling, chips are removed behind the cutter, reducing your chances of re-cutting. climb milling effectively reduces heat generated to the tool and workpiece by transferring heat into the chip, reducing rubbing and by reducing your chances of re-cutting chips.

Utilize Proper Coolant Methods

If used properly, coolant can be an extremely effective way to keep your tool from excessive heat generation. There are many different types of coolant and different ways coolant can be delivered to your tool. Coolant can be compressed air, water-based, straight oil-based, soluble oil-based, synthetic or semi-synthetic. It can be delivered as mist, flood, high pressure or minimum quantity lubricant.

Different applications and tools require different types and delivery of coolant, as using the wrong delivery or type could lead to part or tool damage. For instance, using high pressure coolant with miniature tooling could lead to tool breakage. In materials where chip evacuation is a major pain point such as aluminum, coolant is often used to flush chips away from the workpiece, rather than for heat moderation. When cutting material that produces long, stringy chips without coolant, you run the risk of creating built-up edge from the chips evacuating improperly. Using coolant will allow those chips to slide out of your toolpath easily, avoiding the chance of re-cutting and causing tool failure. In materials like titanium that don’t transfer heat well, proper coolant usage can prevent the material from overheating. With certain materials, however, thermal shock becomes an issue. This is when coolant is delivered to a very hot material and decreases its temperature rapidly, impacting the material’s properties. Coolant can be expensive and wasteful if not necessary for the application, so it’s important to always make sure you know the proper ways to use coolant before starting a job.

Importance of Controlling Heat Generation

Heat can be a tool’s worst nightmare if you do not know how to control it. High efficiency milling will distribute heat throughout the whole tool instead of one small portion, making it less likely for your tool to overheat and fail. By keeping RDOC constant throughout your toolpath, you will decrease the chances of rubbing, a common cause of heat generation. Climb milling is the most effective way to transfer heat into the chip, as it will reduce rubbing and lessen the chance of re-chipping. This will effectively prolong tool life. Coolant is another method for keeping temperatures moderated, but should be used with caution as the type of coolant delivery and certain material properties can impact its effectiveness.

5 Questions to Ask Before Selecting an End Mill

October 16, 2018/0 Comments/in CNC Machining, Getting Started, Machining 101, Machining Techniques, Tool Selection/by Harvey Performance Company

Few steps in the machining process are as important as proper end mill selection. Complicating the process is the fact that each individual tool has its own unique geometries, each pivotal to the eventual outcome of your part. We recommend asking yourself 5 key questions before beginning the tool selection process. In doing so, you can ensure that you are doing your due diligence in selecting the best tool for your application. Taking the extra time to ensure that you’re selecting the optimal tool will reduce cycle time, increase tool life, and produce a higher quality product.

Question 1: What Material Am I Cutting?

Knowing the material you are working with and its properties will help narrow down your end mill selection considerably. Each material has a distinct set of mechanical properties that give it unique characteristics when machining. For instance, plastic materials require a different machining strategy – and different tooling geometries – than steels do. Choosing a tool with geometries tailored towards those unique characteristics will help to improve tool performance and longevity.

Harvey Tool stocks a wide variety of High Performance Miniature End Mills. Its offering includes tooling optimized for hardened steels, exotic alloys, medium alloy steels, free machining steels, aluminum alloys, highly abrasive materials, plastics, and composites. If the tool you’re selecting will only be used in a single material type, opting for a material specific end mill is likely your best bet. These material specific tools provide tailored geometries and coatings best suited to your specific material’s characteristics. But if you’re aiming for machining flexibility across a wide array of materials, Harvey Tool’s miniature end mill section is a great place to start.

Shop Harvey Tool’s Massive Offering of Fully Stocked Miniature End Mills

Helical Solutions also provides a diverse product offering tailored to specific materials, including Aluminum Alloys & Non-Ferrous Materials; and Steels, High-Temp Alloys, & Titanium. Each section includes a wide variety of flute counts – from 2 flute end mills to Multi-Flute Finishers, and with many different profiles, coating options, and geometries.

Question 2: Which Operations Will I Be Performing?

An application can require one or many operations. Common machining operations include:

Traditional Roughing
Slotting
Finishing
Contouring
Plunging
High Efficiency Milling

By understanding the operations(s) needed for a job, a machinist will have a better understanding of the tooling that will be needed. For instance, if the job includes traditional roughing and slotting, selecting a Helical Solutions Chipbreaker Rougher to hog out a greater deal of material would be a better choice than a Finisher with many flutes.

Question 3: How Many Flutes Do I Need?

One of the most significant considerations during end mill selection is determining proper flute count. Both the material and application play an important role in this decision.

Material:

When working in Non-Ferrous Materials, the most common options are the 2 or 3-flute tools. Traditionally, the 2-flute option has been the desired choice because it allows for excellent chip clearance. However, the 3-flute option has proven success in finishing and High Efficiency Milling applications, because the higher flute count will have more contact points with the material.

Ferrous Materials can be machined using anywhere from 3 to 14-flutes, depending on the operation being performed.

Application:

Traditional Roughing: When roughing, a large amount of material must pass through the tool’s flute valleys en route to being evacuated. Because of this, a low number of flutes – and larger flute valleys – are recommend. Tools with 3, 4, or 5 flutes are commonly used for traditional roughing.

Slotting: A 4-flute option is the best choice, as the lower flute count results in larger flute valleys and more efficient chip evacuation.

Finishing: When finishing in a ferrous material, a high flute count is recommended for best results. Finishing End Mills include anywhere from 5-to-14 flutes. The proper tool depends on how much material remains to be removed from a part.

High Efficiency Milling: HEM is a style of roughing that can be very effective and result in significant time savings for machine shops. When machining an HEM toolpath, opt for 5 to 7-flutes.

Question 4: What Specific Tool Dimensions are Needed?

After specifying the material you are working in, the operation(s) that are going to be performed, and the number of flutes required, the next step is making sure that your end mill selection has the correct dimensions for the job. Examples of key considerations include cutter diameter, length of cut, reach, and profile.

Cutter Diameter

The cutter diameter is the dimension that will define the width of a slot, formed by the cutting edges of the tool as it rotates. Selecting a cutter diameter that is the wrong size – either too large or small – can lead to the job not being completed successfully or a final part not being to specifications. For example, smaller cutter diameters offer more clearance within tight pockets, while larger tools provide increased rigidity in high volume jobs.

Length of Cut & Reach

The length of cut needed for any end mill should be dictated by the longest contact length during an operation. This should be only as long as needed, and no longer. Selecting the shortest tool possible will result in minimized overhang, a more rigid setup, and reduced chatter. As a rule of thumb, if an application calls for cutting at a depth greater than 5x the tool diameter, it may be optimal to explore necked reach options as a substitute to a long length of cut.

Tool Profile

The most common profile styles for end mills are square, corner radius, and ball. The square profile on an end mill has flutes with sharp corners that are squared off at 90°. A corner radius profile replaces the fragile sharp corner with a radius, adding strength and helping to prevent chipping while prolonging tool life. Finally, a ball profile features flutes with no flat bottom, and is rounded off at the end creating a “ball nose” at the tip of the tool. This is the strongest end mill style. A fully rounded cutting edge has no corner, removing the mostly likely failure point from the tool, contrary to a sharp edge on a square profile end mill. An end mill profile is often chosen by part requirements, such as square corners within a pocket, requiring a square end mill. When possible, opt for a tool with the largest corner radius allowable by your part requirements. We recommend a corner radii whenever your application allows for it. If square corners are absolutely required, consider roughing with a corner radius tool and finishing with the square profile tool.

Question 5: Should I Use a Coated Tool?

When used in the correct application, a coated tool will help to boost performance by providing the following benefits:

More Aggressive Running Parameters
Prolonged Tool life
Improved Chip Evacuation

Harvey Tool and Helical Solutions offer many different coatings, each with their own set of benefits. Coatings for ferrous materials, such as AlTiN Nano or TPlus, typically have a high max working temperature, making them suitable for materials with a low thermal conductivity. Coatings for non-ferrous applications, such as TiB2 or ZPlus, have a low coefficient of friction, allowing for easier machining operations. Other coatings, such as Amorphous Diamond or CVD Diamond Coatings, are best used in abrasive materials because of their high hardness rating.

Ready to Decide on an End Mill

There are many factors that should be considered while looking for the optimal tooling for the job, but asking the aforementioned five key question during the process will help you to make the right decision. As always, The Harvey Performance Company Technical Service Department is always available to provide recommendations and walk you through the tool selection process, if need be.

Harvey Tool Technical Support: 800-645-5609

Helical Solutions Technical Support: 866-543-5422

Get to Know Machining Advisor Pro

September 13, 2018/2 Comments/in CNC Machining, CNC Programming, Machining 101, Machining Advisor Pro Help, Quick Tips/by David Pichette

Machining Advisor Pro (MAP) is a tool to quickly, seamlessly, and accurately deliver recommended running parameters to machinists using Helical Solutions end mills. This download-free and mobile-friendly application takes into account a user’s machine, tool path, set-up, and material to offer tailored, specific speeds and feed parameters to the tools they are using.

How to Begin With Machining Advisor Pro

This section will provide a detailed breakdown of Machining Advisor Pro, moving along step-by-step throughout the entire process of determining your tailored running parameters.

Register Quickly on Desktop or Mobile

To begin with Machining Advisor Pro, start by accessing its web page on the Harvey Performance Company website, or use the mobile version by downloading the application from the App Store or Google Play.

Whether you are using Machining Advisor Pro from the web or your mobile device, machinists must first create an account. The registration process will only need to be done once before you will be able to log into Machining Advisor Pro on both the mobile and web applications immediately.

Simply Activate Your Account

The final step in the registration process is to activate your account. To do this, simply click the activation link in the email that was sent to the email address used when registering. If you do not see the email in your inbox, we recommend checking your spam folders or company email filters. From here, you’re able to begin using MAP.

Using Machining Advisor Pro

A user’s experience will be different depending on whether they’re using the web or mobile application. For instance, after logging in, users on the web application will view a single page that contains the Tool, Material, Operation, Machine, Parameter, and Recommendation sections.

On the mobile application, however, the “Input Specs” section is immediately visible. This is a summary of the Tool, Material, Operation, and Machine sections that allow a user to review and access any section. Return to this screen at any point by clicking on the gear icon in the bottom left of the screen.

Identify Your Helical Tool

To get started generating your running parameters, specify the Helical Solutions tool that you are using. This can be done by entering the tool number into the “Tool #” input field (highlighted in red below). As you type the tool number, MAP will filter through Helical’s 4,800-plus tools to begin identifying the specific tool you are looking for.

Once the tool is selected, the “Tool Details” section will populate the information that is specific to the chosen tool. This information will include the type of tool chosen, its unit of measure, profile, and other key dimensional attributes.

Select the Material You’re Working In

Once your tool information is imported, the material you’re working in will need to be specified. To access this screen on the mobile application, either swipe your screen to the left or click on the “Material” tab seen at the bottom of the screen. You will move from screen to screen across each step in the mobile application by using the same method.

In this section, there are more than 300 specific material grades and conditions available to users. The first dropdown menu will allow you to specify the material you are working in. Then, you can choose the subgroup of that material that is most applicable to your application. In some cases, you will also need to choose a material condition. For example, you can select from “T4” or “T6” condition for 6061 Aluminum.

Machining Advisor Pro provides optimized feeds and speeds that are specific to your application, so it is important that the condition of your material is selected.

Pick an Operation

The next section of MAP allows the user to define their specific operation. In this section, you will define the tool path strategy that will be used in this application. This can be done by either selecting the tool path from the dropdown menu or clicking on “Tool Path Info” for a visual breakdown and more information on each available toolpath.

Tailor Parameters to Your Machine’s Capabilities

The final section on mobile, and the fourth web section, is the machine section. This is where a user can define the attributes of the machine that you are using. This will include the Max RPM, Max IPM, Spindle, Holder, and work holding security. Running Parameters will adjust based on your responses.

Access Machining Advisor Pro Parameters

Once the Tool, Material, Operation, and Machine sections are populated there will be enough information to generate the initial parameters, speed, and feed. To access these on the mobile app, either swipe left when on the machine tab or tap on the “Output” tab on the bottom menu.

Please note that these are only initial values. Machining Advisor Pro gives you the ability to alter the stick out, axial depth of cut, and radial depth of cut to match the specific application. These changes can either be made by entering the exact numeric value, the % of cutter diameter, or by altering the slider bars. You are now able to lock RDOC or ADOC while adjusting the other depth of cut, allowing for more customization when developing parameters.

The parameters section also offers a visual representation of the portion of the tool that will be engaged with the materials as well as the Tool Engagement Angle.

MAP’s Recommendations

At this point, you can now review the recommended feeds and speeds that Machining Advisor Pro suggests based on the information you have input. These optimized running parameters can then be further refined by altering the speed and feed percentages.

Machining Advisor Pro recommendations can be saved by clicking on the PDF button that is found in the recommendation section on both the web and mobile platforms. This will automatically generate a PDF of the recommendations, allowing you to print, email, or share with others.

Machining Advisor Pro Summarized

The final section, exclusive to the mobile application, is the “Summary” section. To access this section, first tap on the checkmark icon in the bottom menu. This will open a section that is similar to the “Input Specs” section, which will give you a summary of the total parameter outputs. If anything needs to change, you can easily jump to each output item by tapping on the section you need to adjust.

This is also where you would go to reset the application to clear all of the inputs and start a new setup. On the web version, this button is found in the upper right-hand corner and looks like a “refresh” icon on a web browser.

Contact Us

For the mobile application, we have implemented an in-app messaging service. This was done to give the user a tool to easily communicate any question they have about the application from within the app. It allows the user to not only send messages, but to also include screenshots of what they are seeing! This can be accessed by clicking on the “Contact Us” option in the same hamburger menu that the Logout and Help & Tips are found.

Click this link to sign up today!

Slaying Stainless Steel: Machining Guide

June 19, 2018/17 Comments/in CNC Machining, Helical Solutions, Material Specific, Tech Tips, Trending Now/by Harvey Performance Company

Stainless steel can be as common as Aluminum in many shops, especially when manufacturing parts for the aerospace and automotive industries. It is a fairly versatile material with many different alloys and grades which can accommodate a wide variety of applications. However, milling steel can also be immensely difficult. Stainless steels are notorious end mill assassins, so dialing in your speeds and feeds and selecting the proper tool is essential for machining success.

Material Properties

Stainless steels are high-alloy steels with superior corrosion resistance to carbon and low-alloy steels. This is largely due to their high chromium content, with most grades of stainless steel alloys containing at least 10% of the element.

Stainless steel can be broken out into one of five categories: Austenitic, Ferritic, Martensitic, Precipitation Hardened (PH), and Duplex. In each category, there is one basic, general purpose alloy. From there, small changes in composition are made to the base in order to create specific properties for various applications.

For reference, here are the properties of each of these groupings, as well as a few examples of the popular grades and their common uses.

Category	Properties	Popular Grades	Common Uses
Austenitic	Non-magnetic, outstanding corrosion and heat resistance.	304, 316	Food processing equipment, gutters, bolts, nuts, and other fasteners.
Ferritic	Magnetic, lower corrosion and heat resistance than Austenitic.	430, 446	Automotive parts and kitchen appliances.
Martensitic	Magnetic, moderate corrosion resistance – not for severe corrosion.	416, 420, 440	Knives, firearms, surgical instruments, and hand tools.
Precipitation Hardened (PH)	Strongest grade, heat treatable, severe corrosion resistance.	17-4 PH, 15-5 PH	Aerospace components.
Duplex	Stronger mixture of both Austenitic and Ferritic.	244, 2304, 2507	Water treatment plants, pressure vessels.

Tool Selection

Choosing the correct tooling for your application is crucial when machining stainless steel. Roughing, finishing, slotting, and high efficiency milling toolpaths can all be optimized for stainless steel by choosing the correct style of end mill.

Traditional Roughing

For traditional roughing, a 4 or 5 flute end mill is recommended. 5 flute end mills will allow for higher feed rates than their 4 flute counterparts, but either style would work well for roughing applications. Below is an excellent example of traditional roughing in 17-4 Stainless Steel.

Slotting

For slotting in stainless steel, chip evacuation is going to be key. For this reason, 4 flute tools are the best choice because the lower flute count allows for more efficient chip evacuation. Tools with chipbreaker geometry also make for effective slotting in stainless steel, as the smaller chips are easier to evacuate from the cut.

Finishing

When finishing stainless steel parts, a high flute count and/or high helix is required for the best results. Finishing end mills for stainless steel will have a helix angle over 40 degrees, and a flute count of 5 or more. For more aggressive finishing toolpaths, flute count can range from 7 flutes to as high as 14. Below is a great example of a finishing run in 17-4 Stainless Steel.

High Efficiency Milling

High Efficiency Milling can be a very effective machining technique in stainless steels if the correct tools are selected. Chipbreaker roughers would make an excellent choice, in either 5 or 7 flute styles, while standard 5-7 flute, variable pitch end mills can also perform well in HEM toolpaths.

HEV-5

Helical Solutions offers the HEV-5 end mill, which is an extremely versatile tool for a variety of applications. The HEV-5 excels in finishing and HEM toolpaths, and also performs well above average in slotting and traditional roughing. Available in square, corner radius, and long reach styles, this well-rounded tool is an excellent choice to kickstart your tool crib and optimize it for stainless steel machining.

Running Parameters

While tool selection is a critical step to more effective machining, dialing in the proper running parameters is equally important. There are many factors that go into determining the running parameters for stainless steel machining, but there are some general guidelines to follow as a starting point.

Generally speaking, when machining stainless steels a SFM of between 100-350 is recommended, with a chip load ranging between .0005” for a 1/8” end mill up to .006” for a 1” end mill. A full breakdown of these general guidelines is available here.

Machining Advisor Pro

Machining Advisor Pro is a cutting edge resource designed to precisely calculate running parameters for high performance Helical Solutions end mills in materials like stainless steel, aluminum, and much more. Simply input your tool, your exact material grade, and machine setup and Machining Advisor Pro will generate fully customizable running parameters. This free resource allows you to push your tools harder, faster, and smarter to truly dominate the competition.

Dial In Your Stainless Steel Machining Application With Helical Solutions’ Machining Advisor Pro

In Conclusion

Stainless steel machining doesn’t have to be hard. By identifying the proper material grade for each part, selecting the perfect cutting tool, and optimizing running parameters, headaches from milling steel can become a thing of the past.

Tips for Machining Gummy Materials

May 15, 2018/11 Comments/in CNC Machining, Helical Solutions, Tech Tips/by Harvey Performance Company

Machinists face many problems and challenges when manufacturing gummy materials. These types of materials include low carbon steels, stainless steels, nickel alloys, titanium, copper, and metals with high chromium content. Gummy materials have a tendency to produce long, stringy chips, and are prone to creating built-up edge. These common problems can impact surface finish, tool life, and part tolerances.

Continuous Chip With a Built-Up Edge

Continuous chips are long, ribbon-like chips that are formed when the tool cuts through a material, separating chips along the shear plane created by the tool’s cutting edge. These chips slide up the tool face at a constant flow to create a long and stringy chip. The high temperatures, pressures, and friction produced when cutting are all factors that lead to the sticky chips that adhere to the cutting edge. When this built up edge becomes large enough, it can break off leaving behind some excess material on the workpiece, or gouge the workpiece leaving a poor surface finish.

Coolant

Using large amounts of coolant can help with temperature control and chip evacuation while machining gummy materials. Temperature is a big driving force behind built-up edge. The higher the temperature gets, the easier and faster a built-up edge can form. Coolant will keep local temperatures lower and can prevent the material from work hardening and galling. Long, stringy chips have the potential to “nest” around the tool and cause tool failure. Coolant will help break these chips into smaller pieces and move them away from the cutting action by flash cooling them, resulting in fracturing of the chip into smaller pieces. Coolant should be applied directly to the contact area of the tool and workpiece to have the maximum effect.

Tool Engagement

Running Parameters

The tool should be constantly fed into the workpiece. Allowing the tool to dwell can cause work hardening and increase the chance of galling and built up edge. A combination of higher feed rates and lower speeds should also be used to keep material removal rates at a reasonable level. An increase in feed rates will raise the temperature less than an increase in speed. This relates to chip thinning and the ability of a tool to cut the material rather than rub against it.

Climb Milling

Climb milling is the preferred method as it directs more heat into the chip than the tool. Using climb milling, the largest chip cross section is created first, allowing the tool to cut through the material much easier. The heat generated from friction when the tool penetrates the workpiece is transferred to the chip rather than the tool because the thickest part of the chip is able to hold more heat than the thinnest.

Initial Workpiece Engagement

Sudden, large changes in force, like when a tool initially engages a workpiece, have a negative impact on tool life. Using an arc-in tool path to initially engage the material allows for increased stability with a gradual increase in cutting forces and heat. A gradual tool entry such as this is always the preferred method over an abrupt straight entry.

Tool Selection

A tool with a sharp and robust cutting edge should be selected to machine gummy materials. Helical has tooling specifically designed for Titanium and Stainless Steel to make your tool selection process easy.

Additionally, choosing a tool with the correct coating for the material you are machining will help to protect the cutting edge and result in a far lower chance of built up edge or galling than an uncoated tool. A tool with a higher flute count can spread tool wear out over multiple cutting edges, extending tool life. Tool wear is not always linear in gummy materials; as soon as a little bit of wear appears, tool failure will happen relatively quickly. Changing the tool at the first sign of wear may be necessary to ensure that parts are not scrapped.

Gummy Materials Summarized

Every material machines somewhat differently, but understanding what is happening when the tool cuts the workpiece and how this affects tool life and finish will go a long way to successfully completing any job. Built-up edge and excess heat can be minimized by selecting the correct tool and coating for the material, and following the tips and techniques mentioned above. Finally, be sure to check your machine’s runout and ensure maximum rigidity prior to beginning your machining operation.

Selecting the Right Harvey Tool Miniature Drill

April 19, 2018/0 Comments/in Drilling, Drilling & Holemaking, Harvey Tool, Holemaking, Tool Geometry, Tool Information Guides, Tool Selection/by Harvey Performance Company

Among Harvey Tool’s expansive holemaking solutions product offering are several different types of miniature drill options and their complements. Options range from Miniature Spotting Drills to Miniature High Performance Drills – Deep Hole – Coolant Through. But which tools are appropriate for the hole you aim to leave in your part? Which tool might your current carousel be missing, leaving efficiency and performance behind? Understanding how to properly fill your tool repertoire for your desired holemaking result is the first step toward achieving success.

Pre-Drilling Considerations

Miniature Spotting Drills

Depending on the depth of your desired machined hole and its tolerance mandates, as well as the surface of the machine you will be drilling, opting first for a Miniature Spotting Drill might be beneficial. This tool pinpoints the exact location of a hole to prevent common deep-hole drilling mishaps such as walking, or straying from a desired path. It can also help to promote accuracy in instances where there is an uneven part surface for first contact. Some machinists even use Spotting Drills to leave a chamfer on the top of a pre-drilled hole. For extremely irregular surfaces, however, such as the side of a cylinder or an inclined plane, a Flat Bottom Drill or Flat Bottom Counterbore may be needed to lessen these irregularities prior to the drilling process.

Tech Tip: When spotting a hole, the spot angle should be equal to or wider than the angle of your chosen miniature drill. Simply, the miniature drill tip should contact the part before its flute face does.

Selecting the Right Miniature Drill

Harvey Tool stocks several different types of miniature drills, but which option is right for you, and how does each drill differ in geometry?

Miniature Drills

Harvey Tool Miniature Drills are popular for machinists seeking flexibility and versatility with their holemaking operation. Because this line of tooling is offered uncoated in sizes as small as .002” in diameter, machinists no longer need to compromise on precision to reach very micro sizes. Also, this line of tooling is designed for use in several different materials where specificity is not required.

Miniature High Performance Drills – Deep Hole – Coolant Through

For situations in which chip evacuation may be difficult due to the drill depth, Harvey Tool’s Deep Hole – Coolant Through Miniature Drills might be your best option. The coolant delivery from the drill tip will help to flush chips from within a hole, and prevent heeling on the hole’s sides, even at depths up to 20 multiples of the drill diameter.

Miniature High Performance Drills – Flat Bottom

Choose Miniature High Performance Flat Bottom Drills when drilling on inclined and rounded surfaces, or when aiming to leave a flat bottom on your hole. Also, when drilling intersecting holes, half holes, shoulders, or thin plates, its flat bottom tool geometry helps to promote accuracy and a clean finish.

Miniature High Performance Drills – Aluminum Alloys

The line of High Performance Drills for Aluminum Alloys feature TiB2 coating, which has an extremely low affinity to Aluminum and thus will fend off built-up edge. Its special 3 flute design allows for maximum chip flow, hole accuracy, finish, and elevated speeds and feeds parameters in this easy-to-machine material.

Miniature High Performance Drills – Hardened Steels

Miniature High Performance Drills – Hardened Steels features a specialized flute shape for improved chip evacuation and maximum rigidity. Additionally, each drill is coated in AlTiN Nano coating for hardness, and heat resistance in materials 48 Rc to 68 Rc.

Miniature High Performance Drills – Prehardened Steels

As temperatures rise during machining, the AlTiN coating featured on Harvey Tool’s Miniature High Performance Drills – Prehardened Steels creates an aluminum oxide layer which helps to reduce thermal conductivity of the tool and helps to promote heat transfer to the chip, as well as improve lubricity and heat resistance in ferrous materials.

Post-Drilling Considerations

Miniature Reamers

For many operations, drilling the actual hole is only the beginning of the job. Some parts may require an ultra-tight tolerance, for which a Miniature Reamer (tolerances of +.0000″/-.0002″ for uncoated and +.0002″/-.0000″ for AlTiN Coated) can be used to bring a hole to size.

Tech Tip: In order to maintain appropriate stock removal amounts based on the reamer size, a hole should be pre-drilled at a diameter that is 90-94 percent of the finished reamed hole diameter.

Flat Bottom Counterbores

Other operations may require a hole with a flat bottom to allow for a superior connection with another part. Flat Bottom Counterbores leave a flat profile and straighten misaligned holes. For more information on why to use a Flat Bottom Counterbore, read 10 Reasons to Use Flat Bottom Tools.

Key Next Steps

Now that you’re familiar with miniature drills and complementary holemaking tooling, you must now learn key ways to go about the job. Understanding the importance of pecking cycles, and using the correct approach, is vital for both the life of your tool and the end result on your part. Read this post’s complement “Choosing the Right Pecking Cycle Approach,” for more information on the approach that’s best for your application.