Tag Archive for: ADOC

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 toolpath displayed

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 of different sizes with same tool

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 diameter, depths of cut, and slot width chart

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.

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

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.

axial and radial depths of cut in peripheral milling and slotting

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 adoc and rdoc 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 axial 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.

axial and radial depth of cut in high efficiency milling

Corner Engagement: How to Machine Corners

Understanding 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.

Challenges of Corner Engagement

Engaging corners improperly can lead to various issues, affecting both performance and quality. Some common challenges include:

  • Chatter:  – visible imperfections in corner finishes
  • Deflection – detected by unwanted wall taper measurements
  • Strange cutting sound – tool squawking or chirping in the corners
  • Tool breakage/failure or chipping – resulting from excessive stress or improper handling

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.”

90 degree end mill 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 with multiple rdocs at 90 degrees

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.

most effective corner engagement of multiple passes into corner

Corner engagement is a critical aspect of machining that demands attention to detail and strategic planning. By implementing effective techniques and leveraging appropriate tools, manufacturers can overcome challenges associated with corner machining and achieve superior results.

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.” 

How to Avoid Common Part Finish Problems

Part Finish Reference Guide

Finishing cuts are used to complete a part, achieving its final dimensions within tolerance and its required surface finish. Most often an aesthetic demand and frequently a print specification, surface finish can lead to a scrapped part if requirements are not met. Meeting finish requirements in-machine has become a major point of improvement in manufacturing, as avoiding hand-finishing can significantly reduce costs and cycle times.

Common Finishing Problems

  • Burrs
  • Scallop marks
  • Chatter Marks

Factors That Influence Part Finish

  • Specific material and hardness
  • Cutting tool speeds & feeds
  • Tool design and deployment
  • Tool projection and deflection
  • Tool-to-workpiece orientation
  • Rigidity of workholding
  • Coolant and lubricity
  • Final-pass depth of cut

Finishing Problem Solutions

  • Tools with high helix angles and flute counts work best for finishing operations. Softer materials show great results with higher helices, while harder materials can benefit greatly from increased flute counts.
  • Increase your RPM and lower your IPT (Figure 2).
  • Ensure that tool runout is extremely minimal.
  • Use precision tool holders that are in good condition, are undamaged, and run true.
  • Opt for a climb milling machining method.
  • Use tooling with Variable Pitch geometry to help reduce chatter.
  • A proper radial depth of cut (RDOC) should be used. For finishing operations, the RDOC should be between 2 and 5 percent of the tool’s Cutter Diameter.
  • For long reach walls, use reduced neck tooling which help to minimize deflection (Figure 3).
  • Extreme contact finishing (3x cutter diameter), may require a 50% feed rate reduction.

part finish guide

length of cut

Common Surface Finish Nomenclature

Ra = Roughness average
Rq = RMS (Root Mean Square) = Ra x 1.1
Rz = Ra x 3.1

part finish guide

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

Necked 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.

image comparing end mills with and without a reduced neck

The total extension of an end mill, referred to as length below shank (LBS), represents the dimension that characterizes the necked length of the tool in use. This measurement is taken from the beginning of the necked section to the bottom of the cutting end of the tool. The neck relief serves the purpose of creating room for chip removal and preventing the shank from friction in deep-pocket milling scenarios.

Depth of Cut Selection

Axial Depth of Cut (ADOC)

To support the walls during thin wall machining, 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.

Chart of proper 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 steps in thin wall milling

Additional Thin Wall Milling Accuracy Tips:

Climb Milling

Climb milling, gaining popularity among machinists seeking efficiency and extended tool life, minimizes heat generation and friction. Chips are ejected behind the cutter, reducing the likelihood of chip recutting. The chip initiates at its widest point and diminishes, leading to the transfer of generated heat into the chip rather than the tool or workpiece. This results in longer tool lifespan, enabling more parts per tool and lessened costs. Additionally, it contributes to a superior part finish by optimizing chip formation at the cutting edge.

drawing demonstrating the difference between conventional and climb milling with the direction of an end mill

Wall Stabilization

Manual vibration dampening and wall stabilization can be achieved by using thermoplastic compounds, or wax, which can be thermally removed.

HEM Toolpaths

The use of HEM toolpaths can optimize tool performance. It is an advanced machining approach which involves combining a low RDOC (Radial Depth of Cut) with a high ADOC (Axial Depth of Cut), along with elevated feed rates. This combination aims to enhance material removal rates and reduce tool wear.

High Efficiency Milling (HEM) varies from conventional milling, where a higher RDOC and lower ADOC are usually recommended. Conventional milling tends to generate concentrated heat in a specific area of the cutting tool, expediting tool wear. Additionally, while conventional milling requires more axial passes, HEM toolpaths involve more radial passes.

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.

Three Harvey tool extended reach tool holders in 3, 5, and 6 inch lengths

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).

Infographic showing result of tool deflection and excess overhang on a part's finish
Infographic showing progressive step drilling procedures and depths of cut with varied length of tools

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).

Inforgraphic showing Deep Cavity Milling and witness marks from multiple step downs

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.

Confidently Machine Deeper With Harvey Tool’s Extended Reach Tool Holders

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 image showing result of failed chip evacuation when 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.

cnc machining setup covered in chips

Radial Depth of Cut

Radial Depth of Cut denotes the distance that a tool advances into a workpiece, also known as Stepover, Cut Width, or XY.

Feed Per Tooth

Feed per tooth translates directly to your tool feed rate, and is commonly referred to as Inches Per Tooth (IPT) or chip load.

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.

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

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.

comparison of radial chip thinning and feed per tooth

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 adjustment profiles

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.

High efficiency milling guidebook download