Tag Archive for: Part Finish

Reducing Tool Runout

Tool runout is a given in any machine shop, and can never be 100% avoided. Thus, it is important to establish an acceptable level of runout for any project, and stay within that range to optimize productivity and prolong tool life. Smaller runout levels are always better, but choice of machine and tool holder, stick-out, tool reach, and many other factors all have an influence on the amount of runout in every setup.

Defining Tool Runout

Tool runout is the measurement of how far a cutting tool, holder, or spindle rotates off of its true axis. This can be seen in low quality end mills where the cutting diameter is true to size when measured while stationary, but measures above tolerance while rotating.

The first step to minimizing runout is understanding what individual factors cause runout in every machine setup. Runout is seen in the accuracy of every cutting tool, collet, tool holder, and spindle. Every added connection between a machine and the workpiece it is cutting will introduce a higher level of runout. Each increase can add to the total runout further and further. Steps should be taken with every piece of tooling and equipment to minimize runout for best performance, increased tool life, and quality finished products.

Measuring Runout

Determining the runout of your system is the first step towards finding how to combat it. Runout is measured using an indicator that measures the variation of a tool’s diameter as it rotates. This is done with either a dial/probe indicator or a laser measuring device. While most dial indicators are both portable and easy to use, they are not as accurate as the available laser indicators, and can also make a runout measurement worse by pushing on a tool. This is mostly a concern for miniature and micro-tooling, where lasers should be strictly used due to the tool’s fragile nature.  Most end mill manufacturers recommend using a laser runout indicator in place of a dial indicator wherever possible.

Z-Mike Laser

Z-Mike laser measurement devices are common instruments used to measure levels of tool runout.

Runout should be measured at the point where a tool will be cutting, typically at the end of the tools, or along a portion of the length of cut. A dial indicator may not be plausible in these instances due to the inconsistent shape of a tool’s flutes. Laser measuring devices offer another advantage due to this fact.

High Quality Tools

The amount of runout in each component of a system, as-manufactured, often has a significant impact on the total runout of a given setup. Cutting tools all have a restriction on maximum runout allowed when manufactured, and some can have allowances of .0002” or less. This is often the value that should be strived for in a complete system as well. For miniature tooling down to .001” diameter, this measurement will have to be held to an even smaller value. As the ratio of tool runout to tool diameter becomes larger, threats of tool failure increase. As stated earlier, starting with a tool that has minimal runout is pivotal in keeping the total runout of a system to a minimum. This is runout that cannot be avoided.

Precision Tool Holders

The next step to minimizing runout is ensuring that you are using a high quality, precision tool holder. These often come in the form of shrink-fit, or press-fit tool holders offering accurate and precise tool rotation.  Uniform pressure around the entire circumference of a shank is essential for reducing runout. Set screw based holders should be avoided, as they push the tool off-center with their uneven holding pressure.  Collet-based tool holders also often introduce an extra amount of runout due to their additional components. Each added connection in a tool holding system allows more methods of runout to appear. Shrink-fit and press-fit tool holders are inherently better at minimizing runout due to their fewer components.

end mill in holder above completed part

Included in your tool holding considerations should be machine tool cleanliness. Often, chips can become lodged in the spindle, and cause an obstruction between two high-precision surfaces in the system. Ensuring that your tool holder and spindle are clean and free of chips and debris is paramount when setting up for every job.

Shank Modifications

Apart from equipment itself, many other factors can contribute to an increasing amount of tool runout. These can include how long a tool is, how rigid a machine setup is, and how far a tool is hanging out of its holder.  Shank modifications, along with their methods of tool holding can have a large impact. Often thought of as an older, obsolete technology, Weldon flats are found guilty of adding large amounts of runout in many shops. While many shops still use Weldon flats to ensure a secure grip on their tools, having a set screw pushing a tool to one side can push it off center, yielding very high levels of runout. Haimer Safe Lock™ is another option increasing in popularity that is a much higher performance holding technology. The Safe-Lock™ system is designed with the same tolerances as shrink fit and other high precision tool holders. It is able to minimize runout, while firmly holding a tool in place with no chance of pull-out.

haimer safe lock tool holder for reducing tool runout

The Haimer Safe-Lock™ system is one option to greatly reduce tool runout.

Runout will never be completely eliminated from a machining system. However, steps can (and should) be taken to keep it to a minimum using every method possible. Keeping a tool running true will extend tool life, increase performance, and ultimately save your shop time and money. Runout is a common concern in the metalworking industry, but it is often overlooked when it could be main issue causing part rejections and unacceptable results. Every piece of a machine tool plays a part in the resultant runout, and none should be overlooked.

Most Common Methods of Tool Entry

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-Drilled Hole

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. It also facilitates smoother chip evacuation, reducing the risk of chip buildup and potential tool breakage. Machinists often use this technique when working with materials prone to chip welding or built-up edge formation, ensuring consistent machining performance.

tool entry predrill


Helical Interpolation

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. Moreover, helical interpolation offers advantages in achieving precise surface finishes, making it a preferred choice for applications requiring high precision and surface quality, such as aerospace and medical device manufacturing.

helical interpolation


Ramping-In

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. Additionally, ramping-in allows for efficient material removal with reduced axial forces, minimizing workpiece distortion and enhancing dimensional accuracy. Machinists often employ this technique in contouring and pocketing operations, where maintaining part integrity is crucial.

ramping

Suggested Starting Ramp Angles:

Hard/Ferrous Materials: 1°-3°

Soft/Non-Ferrous Materials: 3°-10°

For more information on this popular tool entry method, see Ramping to Success.


Arcing

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. Machinists often utilize this technique in mold making, die sinking, and 3D contouring operations, enhancing productivity and surface finish quality.

arching with end mill


Straight Plunge

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.

tool entry


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. Machinists often resort to straight tool entry in simple machining operations with limited tool access or where other entry methods are impractical. However, it’s crucial to monitor tool wear and chip evacuation carefully to prevent chip buildup and potential tool breakage. Adjusting cutting parameters based on material properties and part geometry can further enhance machining efficiency and tool life.

tool entry


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%. Roll-in tool entry is particularly advantageous in slotting and profiling operations, where maintaining consistent chip thickness is critical for surface finish quality and dimensional accuracy. Machinists often utilize this technique in high-speed machining applications, maximizing material removal rates while minimizing tool wear and heat generation.

tool entry

Mastering various tool entry techniques is essential for machining success. By understanding and implementing these methods effectively, machinists can optimize performance while prolonging the lifespan of their tools. Continual evaluation of cutting conditions and adaptation of entry strategies based on material properties and part geometry are key to achieving superior machining results.

How to Avoid 4 Major Types of Tool Wear

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

Introduction to High Efficiency Milling I High Speed Machining vs. HEM I How to Combat Chip Thinning I Diving into Depth of Cut I Intro to Trochoidal Milling


What Is Tool Wear?

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.

two close up images comparing an end mill with no tool wear and another with excessive tool wear
An example of a tool with no wear
end mill with excessive tool wear on cutting edge
An example of a tool with excessive wear

Download the Free, 50+ Page High Efficiency Milling Guidebook Today

To prolong tool life, identifying and mitigating the various signs of cutting 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.

Types of Tool Wear And Their Solutions

Abrasive Wear

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.

Utilizing Proper Tool Coatings

Using a tool coating with a high microhardness rating is crucial to avoiding abrasive wear. Microhardness ratings help determine a cutting tool’s level of wear resistance. For example, bare tungsten carbide has a Vickers Hardness (HV) ranging from 760 HV to 1740 HV while coatings such as TiN have an HV of 2213 or more. Despite facing maximum forces during cutting operations, the addition of coating on a tool significantly improves its ease of material removal due to higher hardness. When hardness in a coating is elevated wear is mitigated due to the stack up.

end mill with abrasive wear on cutting edge

Coolant Usage

If the wear land becomes excessive or causes premature tool failure, reducing the cutting speed and optimizing coolant usage can help. Coolant is directed towards the cutting action of a tool during CNC operations. It prevents tool failure by countering high temperatures. Generally machinists opt for either Flood or High Pressure coolant methods. Flooding allows for low pressure chip flushing by providing lubricity. High Pressure coolant provides almost instant cooling of a part and works to evacuate chips at a faster rate. Both methods improve part finish and minimize chip recutting, which can damage a cutting tool.

High Efficiency Milling

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. The image referenced below compares traditional (standard) milling and the newer HEM method. HEM evenly disperses heat across the cutting edge by employing a lower radial depth of cut (RDOC) and a higher axial depth of cut (ADOC). This reduces the likelihood of tool failure and lengthens the tool wear process.

infographic with two end mills comparing the difference between standard milling and high efficiency milling at the workpiece

Chipping

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. \When a chipped tool engages with a workpiece the cutting edges are not even leading to high and low spots within the surface finish.

end mill with chipping tool wear

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.

Reduce Chatter

To counter chipping, ensure the milling operation is completely free of vibration and chatter. Chatter occurs because cutting tools experience high forces during CNC machining operations. While machinists cannot entirely avoid chatter, minimizing it prevents vibration marks and excess wear from appearing along the surface of a tool or part. 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

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.

end mill thermal cracking

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

HEM toolpaths provide excellent protection against thermal cracking. As previously mentioned, these toolpaths spread the heat across the cutting edge of the tool, reducing the overall temperature and preventing serious fluctuations in heat.


Harvey HEM guidebook ad

Fracture

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.

Optimal Tool Holding

Tool holder issues or loose work holding can also cause a fracture, as can inconsistencies in workpiece material properties. Establishing a secure connection between the tool and machine reduces the risk of tool runout and scrapped parts. Machinists generally experience improved performance in hydraulic and shrink fit tool holders compared to more mechanical tightening methods.

broken end mill in two pieces from excessive tool wear
Photo courtesy of @cubanana___ on Instagram

Appropriate Depth of Cut

Adjusting the speeds, feeds, and depth of cut and checking the setup for rigidity will help to reduce fracturing. The tool’s axial engagement with a part must be appropriate in order to prevent tool deflection, especially during slotting operations. As pictured below, with increasing slot lengths comes the necessity for longer lengths of cut. Above all, you should choose a tool that offers the highest productivity and least amount of deflection.

drawing of three end mills and their axial depth of cut during cnc slotting operations

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.  

Ball Nose Milling Strategy Guide

Ball Nose Milling Without a Tilt Angle

Ball nose end mills are ideal for machining 3-dimensional contour shapes typically found in the mold and die industry, the manufacturing of turbine blades, and fulfilling general part radius requirements. To properly employ a ball nose end mill (with no tilt angle) and gain the optimal tool life and part finish, follow the 2-step process below (see Figure 1).

infographic of ball nose milling parameters without tilt angle

Shop Harvey Tool’s Vast Selection of Ball Profile End Mills – Click Here to Get Started

Step One: Calculate Your Effective Cutting Diameter

A ball nose end mill’s Effective Cutting Diameter (Deff) differs from its actual cutting diameter when utilizing an Axial Depth of Cut (ADOC) that is less than the full radius of the ball. Calculating the effective cutting diameter can be done using the chart below that represents some common tool diameters and ADOC combinations or by using the traditional calculation (see Figure 2).

ball nose effective cutting diameter chart
ball nose cutting diameter calculation

Step Two: Calculate Your Compensated Speed

Given the new effective cutting diameter a “Compensated Speed” will need to be calculated. If you are using less than the cutter diameter, then its likely your RPM’s will need to be adjusted upward (see Figure 3).

ball nose compensated speed calculation

KEY
ADOC = Axial Depth of Cut
D = Cutting Diameter
Deff = Effective Cutting Diameter
R = Tool Radius (Dia./2)
RDOC = Radial Depth of Cut
SFM = Surface Feet per Minute
Sc = Compensated Speed


Ball Nose Milling With a Tilt Angle

If possible, it is highly recommended to use ball nose end mills on an incline (ß) to avoid a “0” SFM condition at the center of the tool, thus increasing tool life and part finish (Figure 4). For ball nose optimization (and in addition to tilting the tool), it is highly recommended to feed the tool in the direction of the incline and utilize a climb milling technique.

ball nose milling infographic of adoc with tilt angle

To properly employ a ball nose end mill with a tool angle and gain the most optimal tool life and part finish, follow the 2-step process below.

Step One: Calculate Your Effective Cutting Diameter

The chart below that represents some common effective cutting diameters and ADOCs at a 15º tilt angle. Otherwise, the traditional calculation below may be used (see Figure 5).

ball nose effective cutting diameter chart
ball nose cutting diameter calculation

Step Two: Calculate Your Compensated Speed

Given the new effective cutting diameter a compensated speed will need to be calculated. If you are using less than the cutter diameter, then its likely your RPM’s will need to be adjusted upward (see Figure 6).

ball nose compensated speed calculation

KEY
Deff = Effective Cutting Diameter
SFM = Mfg Recommended Surface Feet per Minute
Sc = Compensated Speed

6 Uses of Double Angle Shank Cutters

Ramping to Success

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.

illustrated end mill ramping into part

Check Out Our Micromachining Webinar to Get More Life Out of Your Miniature Cutting Tools

What is Ramping?

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 ).

circular and linear ramping

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.

Arcing

Similar to ramping in both method and benefit, arcing is another technique of approaching a workpiece (See Figure 3).

illustration of end mill arcing tool entry

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.” 

Climb Milling vs. Conventional Milling

There are two distinct ways to cut materials when CNC 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 as seen in Figure 1 below. 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.

infographic showcasing conventional milling with backlash elimination


Key Conventional and Climb Milling Properties:

Conventional Milling (Figure 2)

As previously stated, traditionally conventional milling has been the common choice for most machinists. This is where the cutting edge of the tool is actually rotating away from the direction of the feed. An example of this is seen in Figure 2 below. Until recently, this has been the common choice due to backlash however, the rise of climb milling has caused machinists or machines to adapt and compensate for this issue.

That is not to say there aren’t benefits to climb milling. For example, this strategy offers a machinist more control and less vibration than its climb milling counterpart. Similarly, for materials that traditionally chatter or tear, conventional milling would be the proper strategy to choose. On the other hand, here are some reasons why it might be most beneficial to adopt a climb milling strategy:

  • 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*

infographic of conventional milling and its feed and rotation paths

Climb Milling (Figure 3)

As machinists are always trying to find ways to increase efficiency and tool life, climb milling has gotten a lot of recent traction in the space. Less heat is generated within the tool, and friction is more easily mitigated. These two alone lead to longer tool life, allowing for more parts completed per tool, lowering a shops bottom line. Also, climb milling can lead to a better surface finish due to how the chips are formed at the cutting edge.

With more modern machines now compensating for backlash or utilize backlash eliminators, it has become a much easier strategy to adopt within shops. While we went over some reasons why climb milling is not an effective strategy above, here are some reasons why a machinist may want to explore climb milling:

  • 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 chip 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

infographic of climb milling and its rotation and feed comparisons


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 often the current 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. Without accounting for backlash, breakage can occur due to the forces within the machine during tool engagement.

In addition, conventional milling should also be utilized on casting, forgings or when the part is case hardened. This is due to the cut beginning under the surface of the material, where it will gradually build a chip. Climb milling into these materials will see maximum chip thickness on engagement, which could lead to premature failure of the cutting edge due to the forces generated.

Dodging Dovetail Headaches: 7 Common Dovetail Mistakes

Cutting With Dovetails

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.

Check our Harvey Tool’s Comprehensive Selection of Dovetail Cutters that Ship to You Today.

Avoiding Tool Failure

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).

infographic examining drop hole allowance parameters with dovetails
Figure 1. These pictured tools are designed to mill a groove for a Parker Hannifin O-ring groove No. AS568A-102 (left). These O-rings have cross sections of 0.103″. There is a large variation in the tools’ neck diameters. The tool at right, with a neck diameter of 0.024″, is for applications without a drop hole, while the other tool, with a neck diameter of 0.088″, is for drop-hole applications. The drop-hole allowance allows application of the more rigid tool.

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°.

nondrop-hole dovetail cutters
Figure 2. The dovetail tool pictured is the nondrop-hole example from Figure 1. The cross section illustrates the relationship between the end diameter of the tool (0.083″) and the significantly smaller core diameter (0.014″). Understanding this relationship and the effect of torque on a small core diameter is critical to developing appropriate dovetailing operating parameters.
dovetail cutters with different neck diameters
Figure 3: These dovetail tools have the same end diameter but different neck diameters (0.070″ vs. 0.034″) and different included angles (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).

microdovetailing with dovetail cutter
Figure 4: In microdovetailing operations, increased contact requires diminishing stepover to maintain constant tool load.

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.