Intro to Trochoidal Milling

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

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


What Is Trochoidal Milling?

Trochoidal milling is a method of machining used to create a slot wider than the cutting tool’s cutting diameter. This is accomplished using a series of circular cuts known as a trochoidal tool path. A form of High Efficiency Milling (HEM), trochoidal milling leverages high speeds while maintaining a low radial depth of cut (RDOC) and a high axial depth of cut (ADOC).

Trochoidal milling is largely based on the theory surrounding chip thinning in machining. Conventional thinking suggests that cutting tools have an optimal chip load that determines the ideal width and size of the chips produced. The concept of combating chip thinning involves machining with a chip load that is larger than “optimal” in order to maintain a constant maximum chip thickness.

In contrast to a completely linear radial tool path in conventional machining, trochoidal milling takes advantage of a spiral tool path with a low RDOC to reduce load and wear on the tool (Figure 1).

trochoidal milling

Advantages of Trochoidal Milling

  • Decreased cutting forces
  • Reduced heat
  • Greater machining accuracy
  • Improved tool life
  • Faster cycle times
  • One tool for multiple slot sizes

Trochoidal milling can be very advantageous in certain applications. The reduced radial engagement of the cutting edge decreases the amount of heat produced in the cut while also decreasing the cutting forces and load on the spindle. The reduced radial forces allow for greater accuracy during production and make it possible to machine finer and more precise features on a part.

In addition, the lower radial depth of cut allows for a higher axial depth of cut, meaning that the entire length of the cutting edge can be utilized. This ensures that heat and cutting forces are distributed across the tool’s cutting edge, rather than concentrated on a single section. The reduced heat and wear, combined with their uniform spread on the cutting edge, resulting in significantly improved tool life over conventional slotting methods.

Given the reduced destructive forces, the cutting tool’s speeds can be increased. Since the entire length of cut is utilized, trochoidal milling can eliminate the need for multiple axial depths of cut. Increased running parameters and a reduced number of passes greatly reduce cycle time.

Since trochoidal milling uses a tool to machine a slot wider than its cutting diameter, the same tool can be used to create slots of varying sizes, rather than just one. This can free up space in your tool carousel and save time on tool change-outs, depending on the requirements of the part (Figure 2).

trochoidal milling paths

Although slotting is a roughing operation, the reduced radial depth of cut and decreased cutting forces from trochoidal milling often result in an improved finish over a conventional slotting toolpath. However, a finishing pass along the walls of the workpiece might be required to remove any cusps left from the spiral motion of the cutting tool.

Click Here to Learn More About The Efficiency-Boosting Power of High Efficiency Milling

Challenges of Trochoidal Milling

The challenges of trochoidal milling are typically found with the machinery and software. The right machine to take advantage of trochoidal milling will not only be capable of high speeds and feeds but will also be capable of a constantly changing feed rate as the tool moves along it’s spiral path. Inability to have a changing feed rate will cause chip thinning which can yield non-ideal results and potentially cause tool breakage. Special software might also be required to program tool paths and feed rates for this process. This is further complicated by factors like the ratio of the cutter diameter to the size of the groove, as well as the radial depth of cut for these different ratios. Most figures suggest the cutter diameter be 50%-70% of the final slot width, while the radial depth of cut should equal 10%-35% of cutter diameter (Table 1), but the safest option is always to consult the tool manufacturer.

trochoidal milling table

Trochoidal Milling and Micromachining

Benefits When Micromachining

Micromachining can also benefit from trochoidal milling. The decreased radial engagement and lower cutting forces produced during a trochoidal tool path put less force on the cutting tools. This is especially important for smaller diameter tools, as they are weaker and less rigid, and the reduced cutting forces decrease the chance of deflection and breakage.

Challenges When Micromachining

While trochoidal milling with miniature tooling is theoretically beneficial, there are additional challenges associated with smaller tools. Miniature cutting tools are much more susceptible to breakage due to spindle runout and vibration, material inconsistencies, uneven loading, and many other variables that arise during machining. Depending on your application, it may be worth using the tool with the greatest diameter for the extra strength. Although there are potential benefits at the miniature level, more attention must be paid to the machine setup and material to ensure the tools have the highest chance of success.

Just like HEM, as a general rule, trochoidal milling should not be considered when using tools with cutting diameters less than .031”. While possible, trochoidal milling may still be prohibitively challenging or risky at diameters below .062”, and your application and machine must be considered carefully.

Conclusion

Trochoidal milling is a High Efficiency Milling technique (high speed, high ADOC, low RDOC) characterized by a circular, or trochoidal, tool path. This milling style is proven to offer significant machining process benefits, such as increasing tool life, reducing machining times, and fewer tools required for a job. However, it is critical to have a machine and software capable of high speeds and feeds and constantly changing feed rates to avoid critical tool failure. While miniature tools can still benefit from trochoidal milling, the risk of tool breakage must be considered carefully, especially at cutter diameters below .062”. Although trochoidal milling can increase your machining efficiency in many applications, it is always a good idea to consult your tool manufacturer beforehand.

A great example of trochoidal milling in action can be seen in this video, where a 1/2″ Helical Solutions end mill with variable helix, variable pitch was used to machine a block of 316 stainless steel.

Diving Into Depth of Cut: Peripheral, Slotting, & HEM Approaches

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 How to Avoid 4 Major Types of Tool Wear I Intro to Trochoidal Milling


Every machining operation entails a radial and axial depth of cut strategy. Radial depth of cut (RDOC), the distance a tool is stepping over into a workpiece; and Axial depth of cut (ADOC), the distance a tool engages a workpiece along its centerline, are the backbones of machining. Machining to appropriate depths – whether slotting or peripheral milling (profiling, roughing, and finishing), is vital to your machining success (Figure 1).

Below, you will be introduced to the traditional methods for both peripheral milling and slotting. Additionally, High Efficiency Milling (HEM) strategies – and appropriate cutting depths for this method – will be explained.

HEM Webinar Ad

Quick Definitions:

Radial Depth of Cut (RDOC): The distance a tool is stepping over into a workpiece. Also referred to as Stepover, Cut Width, or XY.

Axial Depth of Cut (ADOC): The distance a tool engages a workpiece along its centerline. Also referred to as Stepdown, or Cut Depth.

Peripheral Milling: An application in which only a percentage of the tool’s cutter diameter is engaging a part.

Slotting: An application in which the tool’s entire cutter diameter is engaging a part.

High Efficiency Milling (HEM): A newer machining strategy in which a light RDOC and heavy ADOC is paired with increased feed rates to achieve higher material removal rates and decreased tool wear.

depth of cut

Peripheral Milling Styles and Appropriate RDOC

The amount a tool engages a workpiece radially during peripheral milling is dependent upon the operation being performed (Figure 2). In finishing applications, smaller amounts of material are removed from a wall, equating to about 3-5% of the cutter diameter per radial pass. In heavy roughing applications, 30-50% of the tool’s cutter diameter is engaged with the part. Although heavy roughing involves a higher RDOC than finishing, the ADOC is most often smaller than for finishing due to load on the tool.

peripheral milling with roughing

Slotting Styles and Appropriate ADOC Engagement

The amount a tool engages a part axially during a slotting operation must be appropriate for the tool being used (Figure 3). Using an inappropriate approach could lead to tool deflection and damage, and poor part quality.

End mills come in various length of cut options, as well as numerous reached options. Choosing the tool that allows the completion of a project with the least deflection, and highest productivity, is critical. As the ADOC needed to slot can be lower, a stub length of cut is often the strongest and most appropriate tool choice. As slot depths increase, longer lengths of cut become necessary, but reached tooling should be used where allowable.

slotting depth of cut

Depth of Cut Strategy for High Efficiency Milling (HEM)

Pairing a light RDOC and heavy ADOC with high performance toolpaths is a machining strategy known as High Efficiency Milling or HEM. With this machining style, feed rates can be increased and cuts are kept uniform to evenly distribute stresses across the cutting portion of the tool, prolonging tool life.

Traditional Strategy

  • Heavy RDOC
  • Light ADOC
  • Conservative Feed Rate

Newer Strategy – High Efficiency Milling (HEM)

  • Light RDOC
  • Heavy ADOC
  • Increased Feed Rate

Click Here to Access Our Free Educational Webinar on High Efficiency Milling

HEM involves using 7-30% of the tool diameter radially and up to twice the cutter diameter axially, paired with increased feed rates (Figure 4).  Accounting for chip thinning, this combination of running parameters can result in noticeably higher metal removal rates (MRR). Modern CAM software often offers a complete high performance solution with built-in features for HEM toolpaths.  These principals can also be applied to trochoidal toolpaths for slotting applications.

depth of cut

Corner Engagement: How to Machine Corners

Corner Engagement

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:

  • Chatter – visible in “poor” corner finish
  • 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.”

corner engagement

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.”

corner engagement effective approach

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.

corner engagement

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.

ramping

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).

Ramping

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 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.

conventional milling


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*

conventional milling

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

climb milling


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).

Circular Interpolation: Machining Circular Tool Paths

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.

Cutting Circular Tool Paths

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:

Internal Adjusted Feed = (Major Diameter-Cutter Diameter) / (Major Diameter) × Linear Feed

Circular Tool Paths

External Circular Tool Paths

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.

External Adjusted Feed = (Major Diameter+Cutter Diameter) / (Major Diameter) × Linear Feed

Optimize Your Performance

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.

Your Guide to Thin Wall Milling

Milling part features with thin wall characteristics, while also maintaining dimensional accuracy and straightness, can be difficult at best. Although multiple factors contribute, some key components are discussed below and can help to increase your thin wall milling accuracy.

Use Proper Tooling

Long length tooling with a long length of cut can spell trouble in thin wall milling situations due to deflection, chatter and breakage. It is essential to keep your tool as strong as possible while maintaining the ability to reach to the desired depth. Necked-down tooling provides added tool strength while also helping you to reach greater than 3x Diameter depths.

Axial Depth of Cut (ADOC)

To support the walls during thin wall milling, keep a wide-cross section behind it. We recommend utilizing a “stepped down” approach, which divides the total wall height to manageable depths while working each side of the wall. The Axial Depth of Cut (ADOC) dimension will vary depending on the material (and its hardness) being cut.

ADOC in thin wall milling

Radial Depth of Cut (RDOC)

A progressive Radial Depth Of Cut (RDOC) strategy is also important as the thin wall height is increasing. Reducing tool pressure while support stock is disappearing is equally important to keep the thin wall stable.

  • Detail A represents a 5-step progressive radial approach. The number of passes will depend upon your particular application, material hardness and final wall dimensions.
  • This approach helps to keep the pressure off the wall as you make your way towards it. Additionally, it is recommended to alternate sides when using this RDOC strategy.
  • The final RDOC passes should be very light to keep wall vibration to a minimum while maximizing your part finish.

RDOC in thin wall milling

Additional Thin Wall Milling Accuracy Tips:

  • Climb milling will help to keep tool pressure to a minimum.
  • Manual vibration dampening and wall stabilization can be achieved by using thermoplastic compounds, or wax, which can be thermally removed.
  • The use of ultra-high performance tool paths can optimize tool performance.

How to Tackle Deep Cavity Milling the Right Way

Deep cavity milling is a common yet demanding milling operation. In this style, the tool has a large amount of overhang – or how far a cutting tool is sticking out from its tool holder. The most common challenges of deep cavity milling include tool deflection, chip evacuation, and tool reach.

Avoid Tool Deflection

Excess overhang is the leading cause of tool deflection, due to a lack of rigidity. Besides immediate tool breakage and potential part scrapping, excessive overhang can compromise dimensional accuracy and prevent a desirable finish.

Tool deflection causes wall taper to occur (Figure 1), resulting in unintended dimensions and, most likely, an unusable part. By using the largest possible diameter, necked tooling, and progressively stepping down with lighter Axial Depths Of Cut (ADOC), wall taper is greatly reduced (Figure 2).

tool deflection

progressive step drilling

Achieve Optimal Finish

Although increasing your step-downs and decreasing your ADOC are ideal for roughing in deep cavities, this process oftentimes leaves witness marks at each step down. In order to achieve a quality finish, Long Reach, Long Flute Finishing End Mills (coupled with a light Radial Depth of Cut) are required (Figure 3).

Deep Cavity Milling

Mill to the Required Depth

Avoiding tool deflection and achieving an acceptable finish are challenges that need to be acknowledged, but what if you can’t even reach your required depth? Inability to reach the required depth can be a result of the wrong tool holder or simply a problem of not having access to long enough tooling.

Fortunately, your tool holder’s effective reach can be easily increased with Harvey Tool’s Extended Reach Tool Holder, which allows you to reach up to 6 inches deeper.

Evacuate Chips Effectively

Many machining operations are challenged by chip evacuation, but none more so than Deep Cavity Milling. With a deep cavity, chips face more obstruction, making it more difficult to evacuate them. This frequently results in greater tool wear from chip cutting and halted production from clogged flute valleys.

High pressure coolant, especially through the spindle, aids in the chip evacuation process. However, air coolant is a better option if heat and lubricity are not concerns, since coolant-chip mixtures can form a “slurry” at the bottom of deep cavities (Figure 4). When machining hardened alloys, where smaller, powder-like chips are created, slurry’s are a commonality
that must be avoided.

Deep Cavity Milling

How to Combat Chip Thinning

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 Diving into Depth of Cut I How to Avoid 4 Major Types of Tool Wear I Intro to Trochoidal Milling


Defining Chip Thinning

Chip Thinning is a phenomenon that occurs with varying Radial Depths Of Cut (RDOC), and relates to chip thickness and feed per tooth. While these two values are often mistaken as the same, they are separate variables that have a direct impact on each other. Feed per tooth translates directly to your tool feed rate, and is commonly referred to as Inches Per Tooth (IPT) or chip load.

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

Chip Thickness

Chip thickness is often overlooked. It refers to the actual thickness of each chip cut by a tool, measured at its largest cross-section. Users should be careful not to confuse chip thickness and feed per tooth, as these are each directly related to the ideal cutting conditions.

How Chip Thinning Occurs

When using a 50% step over (left side of Figure 1), the chip thickness and feed per tooth are equal to each other. Each tooth will engage the workpiece at a right angle, allowing for the most effective cutting action, and avoiding rubbing as much as possible. Once the RDOC falls below 50% of the cutter diameter (right side of Figure 1), the maximum chip thickness decreases, in turn changing the ideal cutting conditions of the application. This can lead to poor part finish, inefficient cycle times, and premature tool wear. Properly adjusting the running parameters can greatly help reduce these issues.

radial chip thinning

The aim is to achieve a constant chip thickness by adjusting the feed rate when cutting at different RDOC. This can be done with the following equation using the Tool Diameter (D), RDOC, Chip Thickness (CT), and Feed Rate (IPT). For chip thickness, use the recommended value of IPT at 50% step over. Finding an adjusted feed rate is as simple as plugging in the desired values and solving for IPT. This keeps the chip thickness constant at different depths of cut. The adjustment is illustrated in Figure 2.

Inches Per Tooth (Chip Thinning Adjustment)

IPT chip thinning formula
radial chip thinning

Lasting Benefits

In summary, the purpose of these chip thinning adjustments is to get the most out of your tool. Keeping the chip thickness constant ensures that a tool is doing as much work as it can within any given cut. Other benefits include: reduced rubbing, increased material removal rates, and improved tool life.