The following is just one of several blog posts relevant to High Efficiency Milling and Micromachining. To achieve a full understanding of this popular machining method, view any of the additional HEM posts below!
High Efficiency Milling (HEM) is a technique for roughing that utilizes a lower Radial Depth of Cut (RDOC), and a higher Axial Depth of Cut (ADOC). This delays the rate of tool wear, reducing the chance of failure and prolonging tool life while boosting productivity and Material Removal Rates (MRR). Because this machining method boosts MRR, miniature tooling (<.125”) and micromachining is commonly overlooked for HEM operations. Further, many shops also do not have the high RPM capabilities necessary to see the benefits of HEM for miniature tooling. However, if used properly, miniature tooling can produce the same benefits of HEM that larger diameter tooling can.
Benefits of HEM:
Extended tool life and performance.
Faster cycle times.
Overall cost savings
Preventing Common Challenges in Micromachining
Utilizing miniature tooling for HEM, while beneficial if performed correctly, presents challenges that all machinists must be mindful of. Knowing what to keep an eye out for is a pivotal first step to success.
Tool Fragility & Breakage with Miniature Tooling
Breakage is one of the main challenges associated with utilizing high efficiency micromachining with miniature tools due to the fragility of the tool. Spindle runout and vibration, tool deflection, material inconsistencies, and uneven loading are just some of the problems which can lead to a broken tool. To prevent this, more attention must be paid to the machine setup and material to ensure the tools have the highest chance of success.
As a general rule, HEM should not be considered when using tools with cutting diameters less than .031”. While possible, HEM may still be prohibitively challenging or risky at diameters below .062”, and your application and machine must be considered carefully.
Techniques to Prevent Tool Failure:
Ensure workpiece is secure and supported.
Use the shortest overall length and length of cut as possible.
Managing Excessive Heat & Thermal Shock in Micromachining
Due to the small nature of miniature tooling and the high running speeds they require, heat generation can quickly become an issue. When heat is not controlled, the workpiece and tooling may experience thermal cracking, melting, burning, built up edge, or warping.
To combat high heat, coolant is often used to decrease the surface temperature of the material as well as aid in chip evacuation and lubricity. However, care must be taken to ensure that using coolant doesn’t cool the material too quickly or unevenly. If an improper coolant method is used, thermal shock can occur. Thermal shock happens when a material expands unevenly, creating micro fractures that propagate throughout the material and can crack, warp, or change the physical properties of the material.
Techniques to Prevent Heat & Thermal Shock:
Run your coated tool dry or with compressed air while ensuring sufficient chip evacuation.
If performed properly, miniature tooling micromachining (<.125”) can reap the same benefits of HEM that larger diameter tooling can: reduced tool wear, accelerated part production rates, and greater machining accuracy. However, more care must be taken to monitor the machining process and to prevent tool fragility, excessive heat, and thermal shock.
Check out this example of HEM toolpaths (trochoidal milling) being run with a 3/16″ Harvey Tool End Mill in aluminum.
https://www.harveyperformance.com/wp-content/uploads/2017/08/HEM-Miniature-Tooling-Featured-1.jpg6001599Tim Limahttp://www.harveyperformance.com/wp-content/uploads/2018/08/Logo_HarveyPerformanceCompany-4.pngTim Lima2017-08-21 12:32:542021-11-19 08:28:25Applying HEM to Micromachining
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.
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.
High Efficiency Milling 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.
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.
https://www.harveyperformance.com/wp-content/uploads/2017/08/Featured-Image-Intro-to-HEM-IMG.jpg5251400Harvey Performance Companyhttp://www.harveyperformance.com/wp-content/uploads/2018/08/Logo_HarveyPerformanceCompany-4.pngHarvey Performance Company2017-08-11 15:33:262021-11-19 08:29:26Introduction to High Efficiency Milling
In today’s manufacturing industry, titanium and its alloys have become staples in aerospace, medical, automotive, and firearm applications. This popular metal is resistant to rust and chemicals, is recyclable, and is extremely strong for its weight. However, there are several challenges that must be considered when machining titanium and selecting the appropriate tools and parameters for the job.
Titanium is available in many varieties, including nearly 40 ASTM grades, as well as several additional alloys. Grades 1 through 4 are considered commercially pure titanium with varying requirements on ultimate tensile strength. Grade 5 (Ti6Al4V or Ti 6-4) is the most common combination, alloyed with 6 percent aluminum and 4 percent vanadium. Although titanium and its alloys are often grouped together, there are some key differences between them that must be noted before determining the ideal machining approach.
Helical Solutions’ HVTI End Mill is a great choice for high efficiency toolpaths in Titanium.
Although titanium may have more desirable material properties than your average steel, it also behaves more flexibly, and is often not as rigid as other metals. This requires a secure grip on titanium workpieces, and as rigid a machine setup as is possible. Other considerations include avoiding interrupted cuts, and keeping the tool in motion at all times of contact with the workpiece. Dwelling in a drilled hole or stopping a tool next to a profiled wall will cause the tool to rub – creating excess heat, work-hardening the material, and causing premature tool wear.
Heat is a formidable enemy, and heat generation must be considered when selecting speeds and feeds. While commercially pure grades of titanium are softer and gummier than most of its alloys, the addition of alloying elements typically raises the hardness of titanium. This increases concerns regarding generated heat and tool wear. Maintaining a larger chipload and avoiding unnecessary rubbing aids with tool performance in the harder titanium alloys, and will minimize the amount of work hardening produced. Choosing a lower RPM, paired with a larger chipload, can provide a significant reduction in temperature when compared to higher speed options. Due to its low conduction properties, keeping temperatures to a minimum will put less stress on the tool and reduce wear. Using high-pressure coolant is also an effective method to reduce heat generation when machining titanium.
These camshaft covers were custom made in titanium for Mitsubishi Evos. Photo courtesy of @RebootEng (Instagram)
Galling and Built-Up Edge
The next hurdle to consider is that titanium has a strong tendency to adhere to a cutting tool, creating built up edge. This is a tricky issue which can be reduced by using copious amounts of high pressure coolant aimed directly at the cutting surface. The goal is to remove chips as soon as possible to prevent chip re-cutting, and keep the flutes clean and clear of debris. Galling is a big concern in the commercially pure grades of titanium due to their “gummy” nature. This can be addressed using the strategies mentioned previously, such as continuing feed at all times of workpiece contact, and using plenty of high-pressure coolant.
While the primary concerns when machining titanium and its alloys may shift, the methods for mitigating them remain somewhat constant. The main ideas are to avoid galling, heat generation, work hardening, and workpiece or tool deflection. Use a lot of coolant at high pressure, keep speeds down and feeds up, keep the tool in motion when in contact with the workpiece, and use as rigid of a setup as possible.
In addition, selecting a proper tool coating can help make your job a successful one. With the high heat being generated during titanium machining operations, having a coating that can adequately deal with the temperature is key to maintaining performance through an operation. The proper coating will also help to avoid galling and evacuate chips effectively. Coatings such as Harvey Tool’s Aluminum Titanium Nitride (AlTiN Nano) produce an oxide layer at high temperatures, and will increase lubricity of the tool.
Helical Solutions offers the HVTI-6 line of tooling optimized for High Efficiency Milling (HEM) in Titanium and its alloys. Helical’s HVTI-6 features its Aplus coating which offers added lubricity and high temperature resistance for improved tool life and faster speeds and feeds.
As titanium and its many alloys continue to grow in use across various industries, more machinists will be tasked with cutting this difficult material. However, heat management and appropriate chip evacuation, when paired with the correct coating, will enable a successful run.
https://www.harveyperformance.com/wp-content/uploads/2017/08/Featured-Image-Tackling-Titanium-IMG.jpg5251400Tom Pylehttp://www.harveyperformance.com/wp-content/uploads/2018/08/Logo_HarveyPerformanceCompany-4.pngTom Pyle2017-08-08 16:00:512021-11-19 08:29:47Tackling Titanium: A Guide to Machining Titanium and Its Alloys
Tool entry is pivotal to machining success, as it’s one of the most punishing operations for a cutter. Entering a part in a way that’s not ideal for the tool or operation could lead to a damaged part or exhausted shop resources. Below, we’ll explore the most common part entry methods, as well as tips for how to perform them successfully.
Pre-drilling a hole to full pocket depth (and 5-10% larger than the end mill diameter) is the safest practice of dropping your end mill into a pocket. This method ensures the least amount of end work abuse and premature tool wear.
Helical Interpolation is a very common and safe practice of tool entry with ferrous materials. Employing corner radius end mills during this operation will decrease tool wear and lessen corner breakdown. With this method, use a programmed helix diameter of greater than 110-120% of the cutter diameter.
This type of operation can be very successful, but institutes many different torsional forces the cutter must withstand. A strong core is key for this method, as is room for proper chip evacuation. Using tools with a corner radius, which strengthen its cutting portion, will help.
This method of tool entry is similar to ramping in both method and benefit. However, while ramping enters the part from the top, arcing does so from the side. The end mill follows a curved tool path, or arc, when milling, this gradually increasing the load on the tool as it enters the part. Additionally, the load put on the tool decreases as it exits the part, helping to avoid shock loading and tool breakage.
This is a common, yet often problematic method of entering a part. A straight plunge into a part can easily lead to tool breakage. If opting for this machining method, however, certain criteria must be met for best chances of machining success. The tool must be center cutting, as end milling incorporates a flat entry point making chip evacuation extremely difficult. Drill bits are intended for straight plunging, however, and should be used for this type of operation.
Straight Tool Entry
Straight entry into the part takes a toll on the cutter, as does a straight plunge. Until the cutter is fully engaged, the feed rate upon entry is recommended to be reduced by at least 50% during this operation.
Roll-In Tool Entry
Rolling into the cut ensures a cutter to work its way to full engagement and naturally acquire proper chip thickness. The feed rate in this scenario should be reduced by 50%.
https://www.harveyperformance.com/wp-content/uploads/2017/07/Feature-Image-Tool-Entry-IMG.jpg5251400Harvey Performance Companyhttp://www.harveyperformance.com/wp-content/uploads/2018/08/Logo_HarveyPerformanceCompany-4.pngHarvey Performance Company2017-07-17 14:53:062021-11-19 08:30:10Most Common Methods of Tool Entry
Tool wear is the breakdown and gradual failure of a cutting tool due to regular operation. Every tool will experience tool wear at some point in its life. Excessive wear will show inconsistencies and have unwanted effects on your workpiece, so it is important to avoid tool wear in order to achieve optimal end mill performance. Tool wear can also lead to failure, which in turn can lead to serious damage, rework, and scrapped parts.
To prolong tool life, identifying and mitigating the various signs of tool wear is key. Both thermal and mechanical stresses cause tool wear, with heat and abrasion being the major culprits. Learning how to identify the most common types of tool wear and what causes them can help machinists remedy issues quickly and extend tool longevity.
The wear land is a pattern of uniform abrasion on the cutting edge of the tool, caused by mechanical abrasion from the workpiece. This dulls the cutting edge of a tool, and can even alter dimensions such as the tool diameter. At higher speeds, excessive heat becomes more of an issue, causing more damage to the cutting edge, especially when an appropriate tool coating is not used.
If the wear land becomes excessive or causes premature tool failure, reducing the cutting speed and optimizing coolant usage can help. High Efficiency Milling (HEM) toolpaths can help reduce wear by spreading the work done by the tool over its entire length of cut. This prevents localized wear and will prolong tool life by using the entire cutting edge available.
Chipping can be easily identified by a nicked or flaked edge on the cutting tool, or by examining the surface finish of a part. A poor surface finish can often indicate that a tool has experienced some sort of chipping, which can lead to eventual catastrophic tool failure if it is not caught.
Chipping is typically caused by excessive loads and shock-loading during operation, but it can also be caused by thermal cracking, another type of tool wear which is explored in further detail below. To counter chipping, ensure the milling operation is completely free of vibration and chatter. Taking a look at the speeds and feeds can also help. Interrupted cuts and repeated part entry can also have a negative impact on a tool. Reducing feed rates for these situations can mitigate the risk of chipping.
Thermal cracking is often identified by cracks in the tool perpendicular to the cutting edge. Cracks form slowly, but they can lead to both chipping and premature tool failure.
Thermal cracking, as its name suggests, is caused by extreme temperature fluctuations during milling. Adding a proper coating to an end mill is beneficial in providing heat resistance and reduced abrasion on a tool. HEM toolpaths provide excellent protection against thermal cracking, as these toolpaths spread the heat across the cutting edge of the tool, reducing the overall temperature and preventing serious fluctuations in heat.
Fracture is the complete loss of tool usage due to sudden breakage, often as a result of improper speeds and feeds, an incorrect coating, or an inappropriate depth of cut. Tool holder issues or loose work holding can also cause a fracture, as can inconsistencies in workpiece material properties.
Adjusting the speeds, feeds, and depth of cut and checking the setup for rigidity will help to reduce fracturing. Optimizing coolant usage can also be helpful to avoid hot spots in materials which can dull a cutting edge and cause a fracture. HEM toolpaths prevent fracture by offering a more consistent load on a tool. Shock loading is reduced, causing less stress on a tool, which lessens the likelihood of breakage and increases tool life.
It is important to monitor tools and keep them in good, working condition to avoid downtime and save money. Wear is caused by both thermal and mechanical forces, which can be mitigated by running with appropriate running parameters and HEM toolpaths to spread wear over the entire length of cut. While every tool will eventually experience some sort of tool wear, the effects can be delayed by paying close attention to speeds and feeds and depth of cut. Preemptive action should be taken to correct issues before they cause complete tool failure.
https://www.harveyperformance.com/wp-content/uploads/2017/07/Feature-Image-Tool-Wear-IMG.jpg5251400Harvey Performance Companyhttp://www.harveyperformance.com/wp-content/uploads/2018/08/Logo_HarveyPerformanceCompany-4.pngHarvey Performance Company2017-07-11 16:30:432022-10-17 10:06:57How to Avoid 4 Major Types of Tool Wear
During the milling process, and especially during corner engagement, tools undergo significant variations in cutting forces. One common and difficult situation is when a cutting tool experiences an “inside corner” condition. This is where the tool’s engagement angle significantly increases, potentially resulting in poor performance.
Machining this difficult area with the wrong approach may result in:
Deflection – detected by unwanted “measured” wall taper
Strange cutting sound – tool squawking or chirping in the corners
Tool breakage/failure or chipping
Least Effective Approach (Figure 1)
Generating an inside part radius that matches the radius of the tool at a 90° direction range is not a desirable approach to machining a corner. In this approach, the tool experiences extra material to cut (dark gray), an increased engagement angle, and a direction change. As a result, issues including chatter, tool deflection/ breakage, and poor surface finish may occur.
Feed rate may need to be lessened depending on the “tool radius-to-part radius ratio.”
More Effective Approach (Figure 2)
Generating an inside part radius that matches the radius of the tool with a sweeping direction change is a more desirable approach for corner engagement. The smaller radial depths of cut (RDOC) in this example help to manage the angle of engagement, but at the final pass, the tool will still experience a very high engagement angle. Common results of this approach will be chatter, tool deflection/breakage and poor surface finish.
Feed rate may need to be reduced by 30-50% depending on the “tool radius-to-part radius ratio.”
Most Effective Approach For Corner Engagement (Figure 3)
Generating an inside part radius with a smaller tool and a sweeping action creates a much more desirable machining approach. The manageable RDOC and smaller tool diameter allow for management of the tool engagement angle, higher feed rates and better surface finishes. As the cutter reaches full radial depth, its engagement angle will increase, but the feed reduction should be much less than in the previous approaches.
Feed rate may need to be heightened depending on the “tool-to-part ratio.” Utilize tools that are smaller than the corner you are machining.
https://www.harveyperformance.com/wp-content/uploads/2017/05/Featured-Image-Corner-Engagement-IMG.jpg5251400Harvey Performance Companyhttp://www.harveyperformance.com/wp-content/uploads/2018/08/Logo_HarveyPerformanceCompany-4.pngHarvey Performance Company2017-05-15 07:00:142021-11-19 08:18:58Corner Engagement: How to Machine Corners
Poor tool life and premature tool failure are concerns in every machining application. Something as simple as tool path selection – and how a tool first enters a part – can make all the difference. Tool entry has a great deal of influence on its overall success, as it’s one of the most punishing operations for a cutter. Ramping into a part, via a circular or linear toolpath, is one of the most popular and oftentimes the most successful methods (Figure 1). Below, learn what ramping is, its benefits, and in which situations it can be used.
Ramping refers to simultaneous radial and axial motion of a cutting tool, making an angular tool path. Oftentimes, this method is used to approach a part when there is a need to create closed forms such as pockets, cavities, engravings, and holes. In doing so, the need to plunge with an end mill or drill to create a starting point is eliminated. Ramping is particularly important in micromachining where even the slightest imbalance in cutting forces can cause tool failure.
There are two types of ramping toolpaths: Linear and Circular (Figure 2 ).
Linear Ramping involves moving a cutting tool along two axes (the z-axis and one of the x, y axes). This method has significant more radial engagement with complementary increased cutting forces distributed across only two axes.
Circular Ramping (Helical Interpolation) has a spiral motion of the cutting tool that engages all three axes (x, y, and z axes). This method typically has less radial engagement on the cutting tool, with the cutting forces distributed across the three different axes. This is the recommended method, as it ensures the longest tool life.
Suggested Starting Ramp Angles:
Soft/Non-Ferrous Materials: 3° – 10°
Hard/Ferrous Materials 1° – 3°
Benefits of Ramping
When a tool enters the part via a Ramping method, it gradually increases in depth, preventing any shock loading on end mills. This reduces costs resulting from unnecessary tool breakage. Ramping produces smaller chips when compared to plunging, which makes chip evacuation faster and easier. As a result, cycle time can be decreased by running the end mill at faster parameters. Ramping also creates an extra space in the tool changer that would otherwise be occupied by a drill purposed with machining a starter hole.
Similar to ramping in both method and benefit, arcing is another technique of approaching a workpiece (See Figure 3).
While ramping enters the part from the top, arcing enters from the side. The end mill follows a curved tool path (or arc) when milling, thus gradually increasing the load on the tool as the tool enters the part, as well as gradually decreasing the load as the tool exits the part. In this way, shock loading and possible tool breakage are avoided.
For more information on ramping, arcing, and other tool entry methods, please see Helical Solutions’ “Types of Tool Entry.”
https://www.harveyperformance.com/wp-content/uploads/2017/05/Featured-Image-Ramping-to-Success-IMG.jpg5251400Harvey Performance Companyhttp://www.harveyperformance.com/wp-content/uploads/2018/08/Logo_HarveyPerformanceCompany-4.pngHarvey Performance Company2017-05-10 09:00:392022-04-20 16:52:12Ramping to Success
There are two distinct ways to cut materials when milling: Conventional Milling (Up) and Climb Milling (Down). The difference between these two techniques is the relationship of the rotation of the cutter to the direction of feed. In Conventional Milling, the cutter rotates against the direction of the feed. During Climb Milling, the cutter rotates with the feed.
Conventional Milling is the traditional approach when cutting because the backlash, or the play between the lead screw and the nut in the machine table, is eliminated (Figure 1). Recently, however, Climb Milling has been recognized as the preferred way to approach a workpiece since most machines today compensate for backlash or have a backlash eliminator.
Key Conventional and Climb Milling Properties:
Conventional Milling (Figure 2)
Chip width starts from zero and increases which causes more heat to diffuse into the workpiece and produces work hardening
Tool rubs more at the beginning of the cut causing faster tool wear and decreases tool life
Chips are carried upward by the tooth and fall in front of cutter creating a marred finish and re-cutting of chips
Upwards forces created in horizontal milling* tend to lift the workpiece, more intricate and expansive work holdings are needed to lessen the lift created*
Climb Milling (Figure 3)
Chip width starts from maximum and decreases so heat generated will more likely transfer to the chip
Creates cleaner shear plane which causes the tool to rub less and increases tool life
Chips are removed behind the cutter which reduces the chance of recutting
Downwards forces in horizontal milling is created that helps hold the workpiece down, less complex work holdings are need when coupled with these forces
Horizontal milling is when the center line of the tool is parallel to the work piece
When to Choose Conventional or Climb Milling
Climb Milling is generally the best way to machine parts today since it reduces the load from the cutting edge, leaves a better surface finish, and improves tool life. During Conventional Milling, the cutter tends to dig into the workpiece and may cause the part to be cut out of tolerance.
However, though Climb Milling is the preferred way to machine parts, there are times when Conventional Milling is the necessary milling style. One such example is if your machine does not counteract backlash. In this case, Conventional Milling should be implemented. In addition, this style should also be utilized on casting, forgings or when the part is case hardened (since the cut begins under the surface of the material).
While they are specialty tools, dovetail style cutters have a broad range of applications. Dovetails are typically used to cut O-ring grooves in fluid and pressure devices, industrial slides and detailed undercutting work. Dovetail cutters have a trapezoidal shape—like the shape of a dove’s tail. General purpose dovetails are used to undercut or deburr features in a workpiece. O-ring dovetail cutters are held to specific standards to cut a groove that is wider at the bottom than the top. This trapezoidal groove shape is designed to hold the O-ring and keep it from being displaced.
The dovetail cutter’s design makes it fragile, finicky, and highly susceptible to failure. In calculating job specifications, machinists frequently treat dovetail cutters as larger than they really are because of their design, leading to unnecessary tool breakage. They mistake the tool’s larger end diameter as the critical dimension when in fact the smaller neck diameter is more important in making machining calculations.
As the tools are downsized for micro-applications, their unique shape requires special considerations. When machinists understand the true size of the tool, however, they can minimize breakage and optimize cycle time.
Miniature Matters – Micro Dovetailing
As the trend towards miniaturization continues, more dovetailing applications arise along with the need for applying the proper technique when dovetailing microscale parts and features. However, there are several common misunderstandings about the proper use of dovetails, which can lead to increased tool breakage and less-than-optimal cycle times.
There are seven common mistakes made when dovetailing and several strategies for avoiding them:
1. Not Taking Advantage of Drop Holes
Many O-ring applications allow for a drop hole to insert the cutter into the groove. Take advantage of a drop hole if the part design allows it, as it will permit usage of the largest, most rigid tool possible, minimizing the chance of breakage (Figure 1).
2. Misunderstanding a Dovetail’s True Neck Diameter.
The dovetail’s profile includes a small neck diameter behind a larger end-cutting diameter. In addition, the flute runs through the neck, further reducing the tool’s core diameter. (In the example shown in Figure 2, this factor produces a core diameter of just 0.014″.) The net result is that an otherwise larger tool becomes more of a microtool. The torque generated by the larger diameter is, in effect, multiplied as it moves to the narrower neck diameter. You must remember that excess stress may be placed on the tool, leading to breakage. Furthermore, as the included angle of a dovetail increases, the neck diameter and core diameter are further reduced. O-ring dovetail cutters have an included angle of 48°. Another common included angle for general purpose dovetails is 90°. Figure 3 illustrates how two 0.100″-dia. dovetail tools have different neck diameters of 0.070″ vs. 0.034″ and different included angles of 48° vs. 90°.
3. Calculating Speeds and Feeds from the Wrong Diameter.
Machinists frequently use the wrong tool diameter to calculate feed rates for dovetail cutters, increasing breakage. In micromachining applications where the margin for error is significantly reduced, calculating the feed on the wrong diameter can cause instantaneous tool failure. Due to the angular slope of a dovetail cutter’s profile, the tool has a variable diameter. While the larger end diameter is used for speed calculations, the smaller neck diameter should be used for feed calculations. This yields a smaller chip load per tooth. For example, a 0.083″-dia. tool cutting aluminum might have a chip load of approximately 0.00065 IPT, while a 0.024″-dia. mill cutting the same material might have a 0.0002-ipt chip load. This means the smaller tool has a chip load three times smaller than the larger tool, which requires a significantly different feed calculation.
4. Errors in Considering Depth of Cut.
In micromachining applications, machinists must choose a depth of cut (DOC) that does not exceed the limits of the fragile tool. Typically, a square end mill roughs a slot and the dovetail cutter then removes the remaining triangular-shaped portion. As the dovetail is stepped over with each subsequent radial cut, the cutter’s engagement increases with each pass. A standard end mill allows for multiple passes by varying the axial DOC. However, a dovetail cutter has a fixed axial DOC, which allows changes to be made only to the radial DOC. Therefore, the size of each successive step-over must decrease to maintain a more consistent tool load and avoid tool breakage (Figure 4).
5. Failing to Climb Mill.
Although conventional milling has the benefit of gradually loading the tool, in low-chip load applications (as dictated by a dovetail cutter’s small neck diameter) the tool has a tendency to rub or push the workpiece as it enters the cut, creating chatter, deflection and premature cutting edge failure. The dovetail has a long cutting surface and tooth pressure becomes increasingly critical with each pass. Due to the low chip loads encountered in micromachining, this approach is even more critical to avoid rubbing. Although climb milling loads the tool faster than conventional milling, it allows the tool to cut more freely, providing less deflection, finer finish and longer cutting-edge life. As a result, climb milling is recommended when dovetailing.
6. Improper Chip Flushing.
Because dovetail cuts are typically made in a semi-enclosed profile, it is critical to flush chips from the cavity. In micro-dovetailing applications, chip packing and recutting due to poorly evacuated chips from a semi-enclosed profile will dull the cutter and lead to premature tool failure. In addition to cooling and lubricating, a high-pressure coolant effectively evacuates chips. However, excessive coolant pressure placed directly on the tool can cause tool vibration and deflection and even break a microtool before it touches the workpiece. Take care to provide adequate pressure to remove chips without putting undue pressure on the tool itself. Specific coolant pressure settings will depend upon the size of the groove, the tool size and the workpiece material. Also, a coolant nozzle on either side of the cutter cleans out the groove ahead of and behind the cutter. An air blast or vacuum hose could also effectively remove chips.
7. Giving the Job Away.
As discussed in item number 3, lower chip loads result in significantly lower material-removal rates, which ultimately increase cycle time. In the previous example, the chip load was three times smaller, which would increase cycle time by the same amount. Cycle time must be factored into your quote to ensure a profitable margin on the job. In addition to the important micro-dovetailing considerations discussed here, don’t forget to apply the basics critical to all tools. These include keeping runout low, using tools with application-specific coatings and ensuring setups are rigid. All of these considerations become more important in micro-applications because as tools get smaller, they become increasingly fragile, decreasing the margin of error. Understanding a dovetail cutter’s profile and calculating job specifications accordingly is critical to a successful operation. Doing so will help you reach your ultimate goal: bidding the job properly and optimizing cycle time without unnecessary breakage.
This article was written by Peter P. Jenkins of Harvey Tool Company, and it originally appeared in MicroManufacturing Magazine.
When machining, proper speeds and feeds are very important to avoid breakage and maximize performance. Traditional end milling formulas use Surface Footage (SFM) and Chip Load (IPT) to calculate Speed (RPM) and Feed (IPM) rates. These formulas dictate the correct machining parameters for use in a linear path in which the end mill’s centerline is travelling in a straight line. Since not all parts are made of flat surfaces, end mills will invariably need to move in a non-linear path. In the case of machining circular tool paths, the path of the end mill’s centerline is circular. Not surprisingly, this is referred to as Circular Interpolation.
All rotating end mills have their own angular velocity at the outside diameter. But when the tool path is circular, there is an additional component that is introduced, resulting in a compound angular velocity. Basically, this means the velocity of the outside diameter is travelling at a substantially different velocity than originally expected. The cause of the compound angular velocity is seen in the disparity between the tool path lengths.
Internal Circular Tool Paths
Figure A shows the cross section of a cutting tool on a linear path, with the teeth having angular velocity due to tool rotation, and the center of the tool having a linear feed. Note that the tool path length will always be equal to the length of the machined edge. Figure B shows the same cutting tool on an internal circular path, as done when machining a hole. In this case, the angular velocity of the teeth is changed as a result of an additional component from the circular path of the tool’s center. The diameter of the tool path is smaller than that of the major diameter being cut. Or, in other words, the tool path length is shorter than the machined edge length, increasing the angular velocity of the teeth. To prevent overfeeding and the possibility of tool breakage, the increased angular velocity of the teeth must be made the same as in the linear case in Figure A. The formula below can be used to properly lower the feed rate for internal machining:
Figure C shows the same cutting tool on an external circular path, as done when machining a post. In this case, the diameter of the tool path is larger than the major diameter being cut. This means that the tool path length is longer than the machined edge length, resulting in a decreased angular velocity. To prevent premature dulling and poor tool life due to over-speeding, use the formula below to properly raise the feed rate for external machining. In this way, the decreased angular velocity of the teeth is made the same as in the linear case in Figure A.
By adjusting the feed in the manner provided, internal applications can avoid tool breakage and costly down time. Further, external applications can enjoy optimized performance and shorter cycle times. It should also be noted that this approach can be applied to parts with radiused corners, elliptical features and when helical interpolation is required.