The Experts’ Guide to CNC Engraving

/0 Comments/in , , , , , , , , , , , /by

CNC engraving is a process that removes a small amount of material to create detailed images or shapes. Many manufacturers use this method for labeling parts or creating complex designs; however, not everyone is aware of the key techniques necessary for optimal results. When using an engraving tool, it is essential to consider several challenges that could affect both the tool and the operation.

Advantages of CNC Engraving

Compared to other engraving methods, CNC engraving is fast, consistent, and cost-effective. Thanks to their repeatability, CNC machines deliver consistent results when paired with a high-quality engraving tool. We suggest running the tool at a minimum of 6,000 RPM.

If your machine supports it, increasing the RPM can lead to even greater results. Running at lower speeds can negatively impact tool life. Choosing the right engraving tool requires considering production volume and tool engagement time. Key factors such as tip design, angle, and coating play a crucial role in maximizing efficiency and durability.

Proper Engraver Tool Selection

Most machinists understand that a square-corner end mill does not last as long as a corner-radius or ball-end mill due to its fragile cutting edge.

The same principle applies to CNC engraving tools. An engraver that comes to a sharp point is more fragile than one with a tipped-off or radius tip. For long production runs, consider using a tip-off or rounded tip design, as these geometries distribute cutting forces more evenly across the cutting edge, improving tool longevity. A tip-flat design will last longer than a pointed tip but not as long as a radius tip. If high-detail work is required, a pointed tip is preferable because it provides greater precision.

Pointed Tip Engraving Cutters
Tipped Off Engraving Cutters
Tip Radius Engraving Cutters

Environment and Detail Considerations

Similar to tip geometry, the engraving angle plays a critical role in visibility. The environment in which the engraving is used affects how well it can be seen. If the engraving is exposed to harsh conditions with elements like snow, mud, or dirt, debris can accumulate in the grooves, making it difficult to see and clean. A larger angle creates a wider groove, improving visibility and ease of cleaning.

The image below illustrates three different engraving angles offered by Harvey: the leftmost groove is 30° included, the middle groove is 60° included, and the rightmost groove is 120° included. Each of these engravings is only 0.009 inches deep.

Notice that the 120° engraving is more visible at a distance due to increased surface exposure. If a job requires precision and detail, a smaller angle is preferable. While geometry significantly impacts engraving visibility and tool longevity, another key factor in tool performance is the choice of coating.

Choosing a Tool Coating

A coated engraving tool will last longer than an uncoated one because the coating provides a protective barrier between the tool and the workpiece. Additionally, coatings help reduce heat absorption, increase lubricity, and decrease tool wear. Selecting the right coating depends on the material being machined.

For example, our AlTiN and AlTiN-Nano coatings perform best in stainless steel and nickel alloys. For non-ferrous materials such as aluminum or copper, our Amorphous Diamond coating is ideal. As an alternative to our Amorphous Diamond coating, we also offer ZrN or TiB2 coatings.

A common misconception is that diamond-coated tools can be used on ferrous materials. Instead, this leads to rapid heat generation and premature tool failure.

Successfully Running Your Engraver

Selecting the correct engraving tool is just as important as understanding how to operate it properly. Even the highest-quality tool will be wasted if not used correctly. As with any machining operation, you must consider depth of cut, work holding methods, and appropriate speeds and feeds

Cutting Speeds and Feeds for Engraving 

The tip is the most delicate area of the tool which makes running at the correct speed and feed rate crucial. Running at an incorrect speed and feed rate can cause deflection, which will lead to an inaccurate engraving, chipping, breaking, or a poor surface finish.

At Harvey, we recommend a minimum spindle speed of 6,000 RPM. Operating at higher RPMs, when possible, offers even better support for tool tip integrity.

Higher speeds ensure tool stability as it will be less likely to cause vibration and reduces heat buildup during operation. Running too slowly generates excess heat and vibration leading to chipping, breakage, or having a poor surface finish. To help maintain tool tip integrity, it is important to follow the recommended depth of cut and consider the way the engraver enters the material.

Determining Depth of Cut

Many machinists are unaware that taking cuts deeper than 0.009 inches can shorten the lifespan of a Harvey engraving tool. For depth of cut ranging from 0.001 inch to 0.009 inches, you can operate within our stated speed and feed guidelines. If the operation requires a deeper groove, the chip load must be reduced accordingly. For depths between 0.010 inches and 0.015 inches, reduce the chip load by 20%. For depths ranging from 0.016 inches to 0.020 inches, reduce the chip load by 30%. Depth of cut also influences visibility. A deeper cut made with a tool that has a smaller angle can provide similar visibility to a shallower cut made with a tool that has a larger angle.

The image below illustrates different engraving depths using a 30° included angle. From left to right, the depths are 0.009 inches, 0.015 inches, and 0.020 inches. As depth increases, visibility improves. When engaging the tool with the workpiece, it is best to ramp into the material to protect the tool tip.

We recommend a ramp angle of 1° to 3° for ferrous materials such as stainless steel, and 3° to 10° for non-ferrous materials like aluminum or copper. If ramping is not an option, you may plunge the tool into the material. However, the chip load must be reduced by 50% during entry. Once the desired depth is reached, you can return to the recommended running parameters. Another key consideration is ensuring the workpiece is securely held in place.

Workholding Considerations

Runout or vibration during engraving can result in uneven cuts and tool failure. To prevent this, ensure that engraving tools are held in a sturdy toolholder and that the workpiece is secured. A shrink-fit toolholder minimizes runout and provides excellent stability. While ER collets are acceptable, they wear overtime. To verify an ER collet’s suitability, place an indicator on the tool shank and rotate the tool within the collet. The goal is to achieve the least possible runout, ideally no more than 0.0003 inches.

The workpiece should also be properly secured, either in a vise or a fixture. To detect vibrations during operation, listen for irregular noise or feel for vibrations through the CNC machine door. For cooling, coolants are recommended for metallic workpieces, while an air blast is preferable for non-metallic materials such as plastic.

Conclusion

When selecting an engraving tool, it is essential to choose the correct geometry for the operation, as well as the appropriate coating for the material being machined. Regardless of tip geometry, the engraving tool’s tip is its most fragile part. Proper speed, feed rate, and depth of cut are crucial for maximizing tool life.

For metallic workpieces, a cooling method such as coolant is necessary, while non-metallic workpieces require an air blast. Before starting a new engraving operation, double-check tool runout and ensure that the workpiece is securely held in place.

By following these best practices, CNC engraving operations can achieve high precision, longevity, and optimal tool performance.

Are You Ready to Put Your Engraving Knowledge to Use?

Browse Harvey Tool’s full selection of precision engravers, coatings, and geometries designed for optimal performance in a wide range of materials.

The Benefits of Combined Drill & Countersinks

/0 Comments/in , , , , , , , , , , /by

Two of the most frequently recurring operations across a variety of applications are CNC drilling and countersinking. Since these two processes are often interdependent, managing space in the tool crib and time lost on tool changes can become cumbersome when using dedicated tools for each operation. Using combined drill and countersinks eliminates these concerns and has become a go-to tool across machine shops.  

valor holemaking combined drill and countersink tools on a table with a slide caliper and ruler
Variety of Combined Drill & Countersinks

What is a Combination Drill & Countersink Tool?

A Combined Drill & Countersink is a specialized tool designed to perform two critical operations in one step: drilling a hole and creating a countersink. These tools are typically short and rigid, ideal for producing either a shallow conic or a center hole. Their double-ended design minimizes downtime by enabling quick transitions between tasks.

Valor Holemaking’s Combined Drill & Countersink

Key Features of Combined Drill & Countersinks

They feature a smaller drilling pilot and larger diameter countersink. The drill pilot resembles a spot drill, making it useful for predrilling applications. The stub length of the drill mitigates deflection and ensures accurate location of a hole’s center. When preparing a spot hole for a longer drill, it prevents walking or wobbling off-center. 

Common Applications for Combined Drill & Countersinks

Many holemaking applications begin with spotting and end with countersinking, making combination multi-functional tools cost-effective and time efficient. As the tool drills into the material, the larger countersink diameter chamfers the top edges, allowing fasteners to sit flush with the surface.

Where and How to Use a Combined Drill & Countersink

The primary use of a combined drill and countersink is to create center holes in materials that will be turned between two centers. These centers help accurately position a workpiece along its axis between a lathe chuck and tailstock. Live centers are used in applications requiring a high level of concentricity and support. They typically feature a 60° included angle, which is the angle most combined drills and countersinks are manufactured with. For this reason, combined drill and countersinks are often referred to as center drills.

Combined drill and countersinks are also essential in any application where screws need to sit flush in the workpiece. Holes need to be drilled and countersunk across all industries. Flush-mounted fasteners are required in applications such as aircraft panels and structural components, automotive engine components, boat hulls and marine components, electronic device housings, and covers of all types.

Example of countersunk hole

Types of Combination Drill/sinks: 60°, 82°, and 90° Angles

Harvey Tool and Valor Holemaking offer combined drill and countersinks in 60°, 82°, and 90° included angles. While 60° tools are most commonly used for center drilling, 82° and 90° included angles are designed to match the angles of the most popular flat and oval head screws. These tools allow users to create countersunk fastener holes in a single step.

Important Tips for Running Combination Drills

When running a combined drill-and-countersink, it is important to ensure that chiploads (IPR) are based on the drill diameter. Since the drill diameter is always smaller than the chamfer area, it is safer to use parameters designed for the drill portion of the tool rather than calculating an effective cutter diameter for the chamfer.

Valor Holemaking Combined Drill & Countersink in the Spindle
Valor Holemaking Combined Drill & Countersink in the Spindle

Why These Tools Are Essential in Machining

Combined drill & countersinks are cost-effective and efficient tools to have in your arsenal. Whether you’re preparing a workpiece for turning between centers, spot drilling, or creating countersunk holes for fasteners, these reliable tools complete the job quickly and effectively.

A Closer Look at Helical Solutions’ Tapered End Mills

/0 Comments/in , , , , , , , , /by

Helical Solutions offers a variety of Tapered End Mills designed to enhance performance and efficiency in tapered wall applications. In this blog post, we’ll dive into the geometry of tapered end mills and explore their common applications to understand when they could be utilized to optimize your CNC machining application.

Tapered End Mill Geometry

Tapered End Mills bring many advantages to machining compared to standard end mills, but what is a Tapered End Mill? A standard end mill will have the same cutting diameter throughout the whole length of cut, whereas a taper mills starts at the shank or neck at a larger diameter and tapers down at a specific angle.

The angle of the taper can vary, but Helical Solutions’ tools feature angles ranging from .05° to 5°, which allows for a broad spectrum of cutting operations. A tapered length of cut or tapered neck can also provide increased strength and rigidity, compared to that of a standard end mill. Having a tapered length of cut makes it easier to create flat tapered walls on 3-axis machines and leads to a better finish.

Tapered End Mill

Standard End Mill

Common Taper Mill Applications

Tapered End Mills are used in any machining process that requires an angled surface. These tools are engineered for light profiling and finishing applications in mold and die pockets and other tapered wall applications.

Mold & Die Applications

Mold and die applications are a mass production manufacturing method that consists of shaping different types of metals and other materials. Molds are used to shape metals, allowing them to become solid in the mold, while dies use a mechanical force to cut the material into the desired shape.

A couple examples of mold and die applications are plastic bottles, car body parts, electronic components, cutlery, coins, and metal stamping parts.

Mold Tool & Die Example

Tapered End Mills Profiles

Taper mills are great for profiling with the ball nose version, and for light finishing and creating required draft angles with the square version. Which style is right for you?

Ball Nose Taper Mills

Ball Nose Tapered End Mills are great for profiling because the full radius at the bottom eliminates sharp edges, which leads to a smoother process.

Square Profile Tooling

The square version of the tapered end mill has a higher flute count and helix angle with a sharp cutting edge. This is better for light finishes on the walls of tools.

The draft angle determined in the design process is the amount of mold design can be tapered. A draft angle is a strategic angle or slope designed in the mold. The tapered angle in the tool allows for the draft angle to be formed easier compared to a straight shanked end mill. Having a draft angle in the mold allows for easier removal of the part so it does not get stuck to the mold.

Helical Solutions’ Tapered End Mills

Helical Solutions’ offering of Tapered End Mills feature a tapered profile design, variable pitch geometry for reduced harmonics and increased feed rates, and Aplus coating for increased performance in Cast Iron, Steel, and even Stainless Steel. These tools are offered in a 4 Flute Ball style, and a 5 Flute Square style, so you can select the end profile that best suits your specific toolpath.

Helical’s Tapered End Mills

4 Flute Ball (HTPR-4)

Helical’s 4 Flute Ball Tapered End Mills (HTPR-4) are fully stocked in 6 different angles per side (0.5°, 1°, 1.5°, 2°, 3°, 5°), and in 3 different cutter diameters (1/8”, 3/16”, ¼”). These tools feature a ball nose profile, allowing them to excel in a variety of different applications from 3D contouring and profiling to slotting. A Ball Nose End Mill has a full form radius, allowing machinists to utilize the entire radius when contouring and finishing a 3D surface.

5 Flute Square (HPTR-5)

Helical’s 5 Flute Square Tapered End Mills (HTPR-5) is also is also fully stocked 6 different angles per side (0.5°, 1°, 1.5°, 2°, 3°, 5°), and in 3 different cutter diameters (1/8”, 3/16”, ¼”). These tools feature a square profile for more precise finishing and the 5 flute design creates a larger core, allowing for better tool strength in roughing applications.

Taper Mill Tooling Wrapped-up

By understanding the unique features and advantages of this tooling, machinists can make informed decisions and achieve superior results in their projects. These feature unique geometry that enhances machining capabilities and ensures reliability and accuracy across a range of tapered wall applications.

Mastering Precision: Pilot Drills in CNC Machining

/4 Comments/in , , , , , , , , , , , /by

When it comes to achieving precision in CNC drilling applications, the choice of tools and techniques can make a significant difference in the outcome. One essential element that often doesn’t get the spotlight it deserves is the Pilot Drill. This blog post will explore the importance of pilot drills, their applications, and best practices for integrating them into your CNC machining processes.

What is a Pilot Drill?

A pilot drill is used to create a guide hole in deep drilling applications where precision is required. This guide hole keeps the drill on center, maintaining straightness throughout the cut. By creating a pilot hole, machinists can also improve the quality of the finished product and extend the life of their tools.

The Importance of Pilot Drills in CNC Machining

1. Enhanced Accuracy

The primary advantage of using a pilot drill is the enhanced accuracy it provides. When working with harder materials or complex geometries, a small pilot hole helps maintain the alignment of the longer drill, reducing the risk of misalignment and defects.

2. Extended Tool Life

Using a pilot drill can significantly extend the life of your deep-hole drilling tools. By first creating a pilot hole, the chasing drill experiences less stress, reducing wear and tear, and the chance of breakage, ultimately leading to cost savings from longer tool life.

3. Improved Chip Removal

Pilot drilling can enhance chip removal, particularly in deep-hole drilling scenarios. The smaller pilot hole allows for better coolant flow, which is crucial for effective chip evacuation and maintaining optimal cutting temperatures.

Applications of Pilot Drills

Pilot drills are versatile and can be used in various applications, including:

  1. Deep-hole Drilling: Pilot holes create a guide when drilling deep holes for improved centering and straightness.
  2. Tapping Operations: A pilot hole can facilitate easier and more accurate tapping.
  3. Reaming: When preparing for reaming operations, a pilot drill can ensure the hole is properly aligned and sized.
  4. Screw and Bolt Holes: Pilot holes are essential for ensuring screws and bolts are inserted correctly and securely.

Best Practices for Using Pilot Drills

1. Application      

Piloting is recommended for tighter tolerance holes when drilling at depths of 8xD or greater. Valor Holemaking provides a custom tolerance of +0.0002/+0.0005 (+0.005mm/+0.013mm) to create the perfect oversized guide hole for their traditional drill lines capable of drilling 8xD or greater. Valor Holemaking’s Pilot Drills also include a +2/+1 deg angle tolerance to ensure a larger angle than the chasing drill. Piloting depth is recommended as 3xD for all applications drilling 8xD or greater.

2. Choose the Right Size and Point Angle

Selecting the appropriate size for your pilot drill is crucial. As a rule of thumb, the diameter of the pilot hole should be slightly larger than the diameter of the final hole. This allows for optimal support for the chasing drill while preventing excessive material removal. The pilot drill’s point angle should be equal to or larger than the succeeding drill. This allows the tip of the succeeding drill to engage the material before the flank does (see figure below).

3. Optimize Feed Rates

When using a pilot drill, ensure that the feed rates are optimized for both the pilot and the larger drill. Adjusting the feed rate can improve performance and reduce the risk of tool breakage. Valor Holemaking’s downloadable speeds and feeds tables and Machining Adviser Pro are excellent resources, and you can always consult Valor Holemaking’s Tech Team for further assistance!

4. Use Proper Coolants

Effective cooling and lubrication are vital in metal machining. Ensure that your pilot drill is adequately cooled with flood coolant or adjust speeds and feeds to maintain tool integrity and enhance cutting performance.

5. Maintain Tool Condition

Regularly check the condition of your pilot drills. Worn or damaged pilot drills can lead to inaccuracies and affect the performance of subsequent operations.

6. Integrate with CNC Programming

Incorporate pilot drilling into your CNC programs to ensure that it’s executed at the right stage of your machining process. Program one revolution or brief dwell at the bottom of the pilot hole to ensure a clean surface. This will help streamline operations and improve overall efficiency.

 

Conclusion

Pilot drills may seem like a small detail in the larger scope of CNC machining, but their impact on precision, tool life, and overall efficiency is significant. By understanding their importance and implementing best practices, machinists can enhance their processes and achieve superior results. Whether you’re a seasoned CNC operator or just starting out, incorporating pilot drills into your workflow is a smart move that can lead to greater accuracy and success in metal machining.


Mastering CNC Drilling: Geometries and Key Factors

/0 Comments/in , , , , , , , , , /by

Selecting the proper drill for a specific application is essential to ensuring a successful cnc drilling job. Achieving a perfectly machined hole can often be challenging. There are many machining woes that can occur when drilling into a material. These can greatly affect hole quality, and regardless of the material being machined, there is often zero margin for error to ensure all components meet specifications.

To ensure you are selecting and using the correct drill, you need not only a deep understanding of drill geometries, but also the factors that influence the performance of the drill and quality of the hole. In this comprehensive guide, we’ll dive into drill geometries, while also exploring the performance factors that determine CNC drilling results. Furthermore, we’ll connect these to the strategic decisions that drive the tool selection process, so you can gain a competitive edge at the spindle.

Performance Factors Influencing CNC Drilling Success

Part Material

Different materials require different drill geometries and cutting speeds to maintain hole quality and prevent excessive wear. With different types of materials, whether it be a softer non-ferrous material like aluminum or a harder ferrous material like stainless steels, you’ll face different challenges as you manufacture your part. To ensure that you’re getting the best performance and tool life possible features and geometries must be considered.

metal blocks that have many holes from cnc drilling operations

CNC Drill Geometries

It is important to understand the different geometries of a drill to understand how they affect an application. For an in depth dive into drill geometries, read 10 CNC Drill Geometries Every Machinist Must Know. This breaks down the unique aspects of geometries and how they affect the cnc drilling process.

Drill Geometries and Drill Walking

CNC drill walking occurs when a drill lacks sufficient engagement with the material. This causes it to deviate from its intended tool path, leading to inaccuracies in hole placement and dimensions. This occurs due to various factors, often including improper drill geometry choice. Understanding how different drill geometries influence drill walking is crucial to ensure you’re achieving precision and consistency in every hole.

Point Angles

The point angle dictates cutting forces and chip evacuation. Choosing the right angle, such as 118° or 135°, based on material hardness, ensures efficient drilling and prevents walking. The shallower the point angle, the better the distribution of cutting forces on the material. Higher angles walk less, as the point grabs into the material easier. Machinists must weight these options when choosing the proper drill.

Web Thickness

Web thickness is the distance between cutting edges or flutes at the face of the drill. This is where stability is generated in a tool. Webs that are too thin can increase the likelihood of breakages, while webs that are too thick will generate unnecessary cutting forces. Finding the proper blend of stability and cutting force is a common struggle for machinists.

CNC Drill Length Considerations

Flute and overall length impact stability and chip evacuation. Matching these lengths to drilling depth prevents deflection and enhances hole quality.

While it may be easiest to purchase a long drill that will work in a variety of scenarios, it is not the best choice to ensure precision. Machinists should best match their required depth to the effective depth of a drill. This ensures that the tool will be as rigid as possible, generating the straightest holes.

As tool length increases, rigidity decreases. Therefore, a properly matched drill will be as rigid as the situation allows. This affords the machinist with the best possible outcome for their unique drilling application.

Coolant-Through Drilling

Proper cooling and lubrication extends tool life and ensures excellent hole quality. If your machine is equipped with the option to run through spindle coolant tooling, it can be extremely beneficial to your application. Unlike an end mill, where chips often have the ability to evacuate outward from the tool, the chips in a drilling operating are held captive inside the feature as it’s being drilled. Here, chips are only able to evacuate through the drill fluting

Through spindle coolant not only cools and lubricates a drill at the point of material removal, but also forcibly evacuates the chips. This can increase your tool’s life while reducing or removing the need for peck cycles all together. This means faster cycle times and higher production rates for your product.

On the other hand, coolant can be fed externally, and sprayed onto the tooling. This will aid in cooling and lubricity. The downside is it is less efficient than utilizing a coolant-through drill. In deep hole drilling applications, external coolant is often ineffective for chip evacuation efforts, and is not the ideal choice for the best results.

Speeds & Feeds

Optimizing speeds & feeds is essential for efficient and accurate drilling. There is not a “one size fits all approach” for speeds & feeds, as all tools and materials require a slightly different approach.

Finding the right balance for each material prevents tool wear and ensures effective chip evacuation. Valor Holemaking offers comprehensive starting parameters in the form of Speeds & Feeds Charts and each tool is also supported by Machining Advisor Pro. This tool allows machinist to custom generate speeds & feeds based off the exact tool path, material, and machine setup.

Rigidity and Stability

A sturdy machining setup reduces vibrations during drilling, improving hole quality. The same can be said about the drill within. A rigid tool is a stable tool, especially as the depth requirements increase. Stability is especially important for drilling heavy-duty materials. This can be impacted by several factors, most importantly the quality of the tool and its design, as well as its chip management capabilities. High precision and high-performance solid carbide drills are designed for the utmost rigidity to ensure repeatability time after time and part after part.

Software and Programming

CNC programming software simplifies creating and editing drilling programs. Compatibility with common CAD/CAM software streamlines integration. Much like machine quality, proper programming is an important step in ensuring precision in CNC drilling applications. CAD/CAM integration ensures the correct dimensions are input to the software to best ensure the tool correctly fits the required parameters.

Exploring CNC Drilling Geometries & Key Factors: Wrapped Up

There are many different drill geometries and factors that can directly impact a drill’s performance and hole quality. Understanding these features can greatly assist in your tool selection process, allowing you to improve productivity and hole quality, so you can gain a competitive edge at the spindle. Drilling is often the most precise aspect of machining, so mastering geometries is critical to success.

Corner Comparison: Corner Chamfer vs. Corner Radius

/0 Comments/in , , , , , /by

Using Finite Element Analysis (FEA) simulations by Third Wave Systems’ AdvantEdge CAE product, we tested different end mill corner geometries to compare their effects on both the tool and the workpiece. We studied and compared four 4 flute tools with either a 0.010” or 0.030” radius or chamfer. All tools were tested in 304 stainless steel at 1865 RPM, 244 SFM, and 0.0045 IPT for one revolution.

Both Corner Radius and Corner Chamfer tools offer advantages over Square End Mills by improving tool strength and reducing wear, though their benefits vary. One drawback of corner radius end mills is chip thinning along the radius, which can generate excess heat due to changes in chip thickness. This can lead to premature tool wear, poor surface finish, and potential work hardening. On the other hand, Corner Chamfers have the disadvantage of sharp corners where the chamfer meets the outer diameter (OD) and the end of the tool, causing local stress concentrations.

Force Analysis

The graphs above demonstrate the force exerted on the tool during cutting and how the corner size impacts the required force. As each flute engages, the forces peak in each direction. The 0.010” Chamfer generates the greatest force, while the 0.030” Chamfer requires the least. The forces with the radiused tools are very similar and fall between those of the two chamfered tools.

Temperature Analysis

The peak tool temperature graph shows the impact of chip thinning on corner radius tools and the overall corner size. The 0.030” Radius generated the most heat, while the 0.030” Chamfer generated the least. The temperature differences between the 0.010” Chamfer and 0.010” Radius was minimal, with the 0.010” Radius generated slightly less heat.

Chip and Workpiece Temperature

Understanding the temperature of the chip and workpiece is crucial for assessing tool performance. The contours above illustrate that the most heat is generated along the 0.030” Radius, followed by the 0.010” Radius. Corner Chamfer tools performed better, maintaining a lower overall temperature due to the absence of chip thinning.

Stress Analysis

The minimum principal stress on the backside of the flute indicates areas prone to tool failure. While there were slight differences between the chamfers and radii, the most notable finding was the reduction in stress with increased corner break size.

Similarly, the Mises stress analysis shows where stress is concentrated within the tool, potentially leading to failure. Again, the most significant observation was the reduction in stress with larger corner breaks.

Corner Chamfer vs. Corner Radius: Wrapped Up

Considering all factors, the 0.030” Corner Chamfer proved to be the best overall tool for 304 stainless steel. This is partly due to 304’s tendency to work harden, making excess heat generation particularly detrimental. When working with heat-sensitive materials, Corner Chamfer tools are preferable, especially during roughing, as they generate less heat due to the absence of chip thinning. Although there are minor stress concentrations at the sharp corners of Corner Chamfer tools, these are outweighed by the benefits of reduced heat generation. Larger radii exacerbate chip thinning’s impact on heat generation. While both tool styles offer advantages over square end mills, Corner Chamfer tools are more beneficial in high-heat applications where work hardening and tool wear are concerns.

Harvey Tool offers a range of Corner Chamfer Tools, with sizes ranging from 0.047” to 0.500” and various chamfer sizes to suit different applications.

Traditional vs Free Cutting Honeycomb Core Tools

/0 Comments/in , , , , , , /by

Precision cutting plays a pivotal role in the manufacturing of honeycomb core. CoreHog, a leading provider of composite cutting solutions, offers two distinct styles of Honeycomb Core Finishing Tools: Traditional Finishing Core Tools and Free Cutting Tools. In this post, we explore the advantages and limitations of both Traditional Finishing Core Tools and Free Cutting Core Tools, helping you determine the right choice for your unique manufacturing needs.

CoreHog’s Large Core Finishing Tool

Advantages of Traditional Honeycomb Finishing Tools:

CoreHog’s Finishing Core Tools are designed to handle substantial cutting tasks, efficiently. With three size ranges available, they excel at removing high volumes of material and boast excellent tool life, making them ideal for production applications.

assembly infographic of corehog's honeycomb core finishing tools

Assembly Configuration of CoreHog’s Large & Free Cutting Finishing Core Tools


However, these tools may pose limitations in specific applications. Traditional tools exert tool pressure, but depending on the tool geometry and part profile, the pressure may be too much for the part. This becomes more pronounced when cutting knife edge features such as chamfers and bevels, where the pressure exerted by the tool can cause the part to arch, dislodging it from the table, and ultimately causing it to deviate from specifications.

Introducing Free Cutting Core Finishing Tools:­­

To address the limitations of traditional honeycomb core finishing tools when cutting knife edge features, CoreHog offers Free Cutting Finishing Core Tools. The innovative design reduces tool pressure seen in both the Coreslicer and CoreHogger. The Free Cutting Coreslicer features a more acute and sharper angle, reducing the upward pressure exerted on the part during cutting.

 Differentiation of angle between the Large Coreslicer and the Free Cutting Coreslicer

Further, these tools feature a CoreHogger with a reduced diameter, allowing for greater offset between the CoreHogger and Coreslicer. This allows the Coreslicer to be more forward and free cutting, engaging with the material prior to the CoreHogger and reducing the resulting pressure typically exhibited by the CoreHogger.  

large and free cutting honeycomb core finishing tools

Reduced diameter design of Free Cutting CoreHogger decreases tool pressure on the part.

When to Use Free Cutting Tools:

CoreHog’s Free Cutting Core Finishing Tools are particularly well-suited for applications involving chamfering, beveling, and cutting angled profiles in honeycomb core materials. By reducing pressure and preventing lifting on the part, these tools ensure precise cuts without compromising part quality.

­­Traditional vs. Free Cutting Core Finishing Tool: Summarized

In conclusion, choosing the right cutting tool is crucial for achieving precise results in composite manufacturing. While traditional finishing core tools excel in handling substantial tasks, they may pose challenges when cutting angled profiles in honeycomb core materials. CoreHog’s Free Cutting Core Finishing Tools offer a solution by minimizing pressure on the part, making them ideal for chamfering, beveling, and most other angled profiles. However, in finicky applications where the knife edge part is extremely shallow, a Valve Stem Cutter may still be necessary to achieve your desired cut. By understanding your specific cutting requirements, you can select the most suitable tool for your application, ensuring optimal results in your honeycomb manufacturing processes.

8 Unique Facts About Thread Forming Taps

/32 Comments/in , , , , , , , , /by

Unlike most CNC cutting tools, Thread Forming Taps, otherwise known as Form Taps, Forming Taps, or Roll Taps, work by molding the workpiece rather than cutting it. Because of this, Form Taps do not contain any flutes, as there is no cutting action taking place, nor are there any chips to evacuate. Below are 8 unique facts of Thread Forming Taps (and some may surprise you).

1. Chips Aren’t Formed

When using a Form Tap, chips are not formed, nor is any part material evacuated (Yes, you read that right). With thread forming, the tool is void of any flutes, as chip evacuation is not a concern. Form Taps quite literally mold the workpiece, rather than cut it, to produce threads. Material is displaced within a hole to make way for the threads being formed.

Increase Your Tapping Efficiency 20x With Titan USA’s Thread Form Taps

2. Cutting Oils Allow for Reduced Friction & Heat Generation

Did you know that Thread Forming Taps require good lubrication? But why is that the case if chips are not being evacuated, and how does lubrication enter the part with such a limited area between the tool and the perimeter of the hole being threaded? Despite the fact that chips aren’t being formed or evacuated, cutting oils aid the Form Tap as it interacts with the part material, and reduces friction and heat generation. Lube vent grooves are narrow channels engineered into the side of Forming Taps that are designed to provide just enough room for lubricant to make its way into – and out of – a part.

titan usa thread forming tool

Not all materials are well suited for Thread Forming Taps. In fact, attempting to use a tap in the wrong material can result in significant part and tool damage. The best materials for this unique type of operation include aluminum, brass, copper, 300 stainless steel, and leaded steel. In other words, any material that leaves a stringy chip is a good candidate for cold forming threads. Materials that leave a powdery chip, such as cast iron, are likely too brittle, resulting in ineffective, porous threads.

4. Threads Produced Are Stronger Than Conventional Tapping Threads

Thread forming produces much stronger threads than conventional tapping methods, due to the displacements of the grain of the metal in the workpiece. Further, cutting taps produce chips, which may interfere with the tapping process.

5. Chip Evacuation is Never a Concern With Thread Forming

In conventional tapping applications, as with most machining applications, chip evacuation is a concern. This is especially true in blind holes, or holes with a bottom, as chips created at the very bottom of the hole oftentimes have a long distance to travel before being efficiently evacuated. With form taps, however, chip removal is never a concern.

6. Form Taps Offer Extended Tool Life

Thread Forming Taps are incredibly efficient, as their tool life is substantial (Up to 20x longer than cutting taps), as they have no cutting edges to dull. Further, Thread Forms can be run at faster speeds (Up to 2x faster than Cutting Taps).

Pro Tip: To prolong tool life even further, opt for a coated tool. Titan USA Form Taps, for example, are fully stocked in both uncoated and TiN coated styles.

titan usa thread forming tool on stack of red product packaging containers

7. A Simple Formula Will Help You Find the Right Drill Size

When selecting a Tap, you must be familiar with the following formula, which will help a machinist determine the proper drill size needed for creating the starter hole, before a Thread Forming Tap is used to finish the application:

Drill Size = Major Diameter – [(0.0068 x desired % of thread) / Threads Per Inch]
Drill Size (mm) = Major Diameter – [(0.0068 x desired % of thread x pitch (mm)]

two titan usa thread form taps

8. Thread Forming Taps Need a Larger Hole Size

  1. Thread Form Taps require a larger pre-tap hole size than a cutting tap. This is because these tools impact the sides of the hole consistently during the thread forming process. If the pre-tap hole size is too small, the tool would have to work too hard to perform its job, resulting in excessive tool wear, torque, and possible breakage.

As an example, a ¼-20 cut tap requires a #7 drill size for the starter hole, whereas a ¼-20 roll tap requires a #1 drill size for 65% thread.

Chipbreaker Tooling: Not Just for Roughing

/2 Comments/in , , , , , /by

When many people think about solid carbide tools with chip breakers, they are usually tooling up for a roughing application. While the chipbreaker tool is a great choice for such applications, it can be utilized in a number of other areas too. In this post, we’ll examine many other benefits of the chip breaker style of tooling.

High Efficiency Milling (HEM)

High Efficiency Milling (HEM) uses CAM software to program advanced toolpaths that reduce cutting forces. These tool paths employ smaller end mills with a higher number of flutes (for a stronger core) running at higher speeds and feeds. This strategy includes a light radial depth of cut (RDOC), high axial depth of cut (ADOC), and a controlled angle of engagement.

Helical’s chipbreaking tools include serrated indents along the edge of flute for the entire length of cut. Because HEM utilizes heavy axial depths of cuts, these tools are able to break long chips into smaller ones. In addition to improving chip control and reducing cutting resistance, chipbreaker tools also help in decreasing heat load within the chips. This delays tool wear along the cutting edge and improves cutting performance. 

chipbreaker in spindle

Check out this testimony from a Helical Solutions customer:

“We were able to get going with the 7 flute tools with the chipbreaker. I have to say the difference was INCREDIBLE! We can now rough the entire part with one tool. Also, the operator doesn’t have to open the door to clear chips hardly at all. We were able to rough and finish a 4.15 dia. bore 2 inches deep through the part without having to clear chips at all. Before we had to clear the chips out at least 15-20 times. Many thanks for your support.”

Explore Helical Solutions’ Chipbreaker Roughers Today

Slotting

When slotting, a major concern is chip control. A large buildup of chips can cause the recutting of chips, which adds a lot of heat back into the tool. Chip buildup can also cause a heavy amount of chattering. Both of these conditions are detrimental to tool life. A chip breaking tool can help reduce chip build-up when slotting which will extend tool life. Remember when slotting that 4 flute tools should be utilized in steel. For aluminum and other non- ferrous materials, a 3 flute tool is best.

3 flute chipbreaker
Helical Solutions 3-Flute Chipbreakers

Trochoidal Slotting

Trochoidal slotting is a form of slotting that uses HEM techniques to form a slot. Trochoidal milling implements a series of circular cuts to create a slot wider than the cutting tool’s cutting diameter. Using the logic listed in the earlier paragraphs of this article, a chipbreaker should be used when performing this operation.

Advantages of Trochoidal Slotting:

Decreased cutting forces

Reduced heat

Greater machining accuracy

Improved tool life

Faster cycle times

One tool for multiple slot sizes

chipbreaker rougher ad

Finishing

A little known fact about Helical’s chipbreaker style tool is that the chip breakers are offset flute to flute, which allows for a quality finish on the walls of the part. When utilizing light depths of cuts, high-quality finishes can be achieved.

5 Things to Know About Helical’s High Feed End Mills

/4 Comments/in , , , , /by

Helical Solutions‘ High Feed End Mills provide many opportunities for machinists, and feature a special end profile to increase machining efficiencies. A High Feed End Mill is a High Efficiency Milling (HEM) style tool with specialized end geometry that utilizes chip thinning, allowing for drastically increased feed rates in certain applications. While standard end mills have square, corner radius, or ball profiles, this Helical tool has a specialized, very specific design that takes advantage of chip thinning, resulting in a tool that can be pushed harder than a traditional end mill.

helical solutions high feed end mills ad with both solid round and coolant through options

Below are 5 things that all machinists should know about this exciting Helical Solutions product offering.

1. They excel in applications with light axial depths of cut

A High Feed End Mill is designed to take a large radial depth of cut (65% to 100% of the cutter diameter) with a small axial depth of cut (2.5% to 5% diameter) depending on the application. This makes them perfect for face milling, roughing, slotting, deep pocketing, and 3D milling. Where HEM toolpaths involve light radial depths of cut and heavy axial depths of cut, these utilize high radial depths of cut and smaller axial depths of cut.

2. This tool reduces radial cutting forces

The end profile of this tool is designed to direct cutting forces upward along the axis of the tool and into the spindle. This reduces radial cutting forces which cause deflection, allowing for longer reach tools while reducing chatter and other issues that may otherwise lead to tool failure. The reduction of radial cutting forces makes this tool excellent for use in machines with lower horsepower, and in thin wall machining applications.

3. High Feed End Mills are rigid tools

The design and short length of cut of these end mills work in tandem with the end geometry to produce a tool with a strong core, further limiting deflection and allowing for tools with greater reach lengths.

Push Harder in HEM With Helical Solutions’ High Feed End Mills

4. They can reduce cycle times

In high RDOC, low ADOC applications, these tools can be pushed significantly faster than traditional end mills, saving time and money over the life of the tool.

5. High Feed End Mills are well suited for hard materials

The rigidity and strength of High Feed End Mills make them excellent in challenging to machine materials. Helical’s High Feed End Mills come coated with Tplus coating, which offers high hardness and extended tool life in high temp alloys and ferrous materials up to 45Rc.

In summary, these tools with specialized end geometry that utilizes chip thinning and light axial depths of cut to allow for significantly increased feed rates in face milling, slotting, roughing, deep pocket milling, and 3D milling applications. The end profile of a High Feed End Mill applies cutting forces back up into the spindle, reducing radial forces that lead to deflection in long reach applications. Combining this end geometry with a stubby length of cut results in a tool that is incredibly rigid and well suited for harder, difficult to machine materials.