Complex parts require more than a single operation. Features such as contours, chamfers, engraved details, and precision holes often demand multiple tooling strategies working together throughout the machining process.
In the video below, watch a single component progress from a block of Ti-6Al-4V to a finished part through more than 10 machining applications, each supported by specialized Harvey Tool solutions.
Explore the full range of solutions available in the 2026 Harvey Tool Catalog, featuring more than 31,000 miniature and specialty cutting tools designed to support even the most demanding applications.
https://www.harveyperformance.com/wp-content/uploads/2026/02/Feature-Image-Harvey-Tool-2026-Catalog-Video-IMG.jpg5251400Harvey Performance Companyhttp://www.harveyperformance.com/wp-content/uploads/2018/08/Logo_HarveyPerformanceCompany-4.pngHarvey Performance Company2026-02-27 15:07:592026-03-31 09:47:45Machining a Complex Part with Harvey Tool
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.
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?
Harvey Performance Company’s Don Grandt Employs a Novel “Heavy Radial Efficiency Milling” or “HREM” Technique to Boost Tool Life and Minimize Heat Generation in Titanium
For all the characteristics that make Titanium ideal for extreme conditions, such as its high strength, low density, and corrosion resistant properties, it also makes it very difficult to machine. A modern approach to machining, High Efficiency Milling (HEM), helps. It involves using the theory of chip thinning by applying a smaller Radial Depth of Cut (RDOC), and a larger Axial Depth of Cut (ADOC). This method puts the vast majority of an end mill’s cutting edge to work, evenly distributing heat throughout it. An HEM toolpath works by taking more radial passes with a lower RDOC.
But from experience, Harvey Performance Company National Applications Engineer and “Cutting Tool Counselor,” Don Grandt, has found that there’s a better way to machine titanium. Rather than HEM, Don employs a strategy he calls “Heavy Radial Efficiency Milling (HREM)”, something he’s developed over time with a tried and true “Theory, Science, Experience (TSE) Triple Knowledge Approach” to machining.
The Theory:
In switching from a regular toolpath to a standard HEM toolpath, machinists are permitted to increase the surface foot and boost material removal rates because there is less heat generated at the cutting edge due to the lighter radial depth of cut being utilized.
In titanium, specifically, recommended parameters for HEM are often in the ballpark of 400-500 SFM and 121-152 M/Min, with a radial step over of 6% of the cutting diameter. This allows you to increase the speed to achieve higher feed rates.
However, Don has noticed that most of the heat is coming from the SFM or M/Min when machining titanium, and not the RDOC, thus prematurely fatiguing the cutting edge of the tool in HEM toolpaths. He uses the “MRR Triangle” to compensate for this.
In a 2022 episode of In the Loupe TV, a collection of videos Don creates to educate the machining industry on popular machining methods, tips, tricks, and more, he dives into the Material Removal Rate Triangle, explaining that it’s a representation of how IPM, ADOC, and RDOC interact.
“Each one of these things…contributes to your MRR, material removal rate. I know I don’t want to change that, I don’t want to stop it, and I don’t want to slow the customer down. So what do I do?
Three things (IPM, ADOC, and RDOC) are bringing in the heat. Which one’s causing the most heat? That’s what I want to find out. Because guess what? If I find out which one’s causing the most heat, and I can bring that down, then I can bring one of my other things over, adjust it, keep my MRR, and stay productive.”
In this case, Don opts to increase the RDOC while running the tool at lower SFM-M/MIN, the backbone of the “HREM” toolpath. An illustration of this toolpath, compared to a traditional and standard HEM toolpath, is below.
The Science:
While Don’s strategy can be utilized using any End Mill for Titanium, including Harvey Tool’s offering of Variable Pitch End Mills for Titanium Alloys, the below comparison of HEM vs. HREM toolpaths showcases a 6 Flute Helical Solutions End Mill for Titanium.
HEM vs. HREM Parameters Comparison (3.51 Cubes of Material)
HEM Parameters for ½”, 6 Flute Tool in Ti6AL4V
HREM Parameters for ½”, 6 Flute Tool in Ti6AL4v
ADOC
1.0
1.0
RDOC
.030/6% Stepover
.130/27% Stepover
SFM
400
220
RPM
3056
1680
FPT
.0064
.0026
IPM
118
27
Spindle Load
31%
40%
This chart compares an HEM toolpath to an HREM toolpath, using the same Helical Solutions End Mill in Ti6AL4V Titanium.
Notice that in this independent study, the ADOC remains consistent, the IPM decreases, but the RDOC is substantially increased.
The change in parameters, utilizing the MRR Triangle as a model, generates consistent results in both time and MRR output, so what’s the benefit of making the change? Tool life. And again, it boils down to heat generation.
Toolpath Results
Traditional HEM Strategy
“HREM” Strategy
HEM Parameters for ½”, 6 Flute Tool in Ti6AL4V
HREM Parameters for ½”, 6 Flute Tool in Ti6AL4v
Max Tangential Force
228
397
Peak Tool Temperature
1,218° F / 660° C
857° F / 458° C
Cubes of Material Removed
3.51 Cubes of Ti6AL4V
3.51 Cubes of Ti6AL4V
Here, we can identify that, though more max tangential force is applied to the tool in the HREM method, significantly less heat is generated.
While any cutting tool will generate heat, controlling it is pivotal to prolonging the life of your tool.
The Experience:
From the example above, where the same Helical Solutions End Mill for Titanium was utilized, you can see that by simply increasing the RDOC and slowing down the feed, while accommodating the chip with more flutes, the MRR remains consistent but the cutting edge of the tool faired much better.
Toolpath Results
HEM Example
HREM Example
Before Utilizing an HREM Strategy
While HREM can be beneficial in extending the life of your cutting tool when machining titanium, there are several things that machinists must be mindful of before beginning. Notably, an HREM strategy will add more tangential force to your setup, meaning that fixturing, horsepower, and bending force must be properly accounted for.
In addition, the longer the tool’s length of cut, the less radial there is to be had. This means that if a tool’s length of cut is 2x the diameter, the maximum RDOC will be 27%. With 2.5x length of cut, the maximum radial will only be 20%. As the length of cut increases, the radial decreases, meaning that machinists must make adjustments accordingly to reduce the SFM and, in turn, reduce heat generation and built-up edge (BUE).
Harvey Performance Company Brand Tooling Best Suited for HREM
Leading cutting tool brands Helical Solutions and Harvey Tool offer several cutting tool options specifically designed for the machining of Titanium Alloys. Helical’s offering is extensive, with options ranging from roughers to 5, 6, 7, and multi-flute finishers. Included in this range of fully stocked product is the popular HVTI-6 line, which is optimized specifically for advanced machining toolpaths, such as HEM and HREM, in Titanium.
Harvey Tool’s Material Specific End Mill offering includes options for Titanium Alloys, as well. Featuring variable pitch geometry, options include both square and corner radius profiles. A new Variable Pitch End Mills for Titanium Alloys – Ball offering is set to be released in August 2025.
In Conclusion
By rethinking conventional titanium machining strategies, Don’s “Heavy Radial Efficiency Milling” (HREM) approach challenges the standard High Efficiency Milling (HEM) model with proven results. Through his “Theory, Science, Experience” methodology, Don demonstrates that increasing radial engagement while reducing surface speed can significantly lower tool temperatures and extend tool life, all without sacrificing productivity. Backed by data and real-world trials, HREM offers a compelling alternative for shops looking to optimize titanium machining performance in the most demanding applications.
Mold, Tool, and Die manufacturing demands a high level of precision. Whether you’re machining hardened tool steels, creating detailed mold cavities, or producing dies with complex geometries, the tooling used plays a critical role in ensuring consistent, repeatable results. To explore the full selection of tools relevant to this industry, including application-specific geometries and coatings, visit Harvey Tool’s Mold, Tool & Die Featured Solutions page.
Harvey Tool offers a comprehensive range of tools specifically engineered to meet the unique challenges of the Mold, Tool & Die industry. From tools designed to reach deep cavities to those that maintain surface finish in demanding materials, this offering is built to support precision and reliability throughout the machining process.
Tools included in this lineup are:
CVD Diamond End Mills– This Harvey Tool lineup of Diamond Tooling for Non-Ferrous Materials features true crystalline CVD diamond on a solid carbide substrate, making it ideal for machining graphite, composites, green carbide, and green ceramics.
End Mills for Hardened Steels– Engineered for hardened steels from 46Rc to 68Rc, this tool includes the latest generation AlTiN Nano coating for enhanced hardness and thermal resistance.
End Mills for Aluminum Alloys– We know a part is only as successful as its finish. That’s why our aluminum finishing solutions are crafted for mirror-like surface quality.
End Mills for Medium Alloy Steels– Engineered for versatility, these CNC-ground, AlTiN-coated tools excel in machining stainless, tool, and medium alloy steels.
Miniature Tapered End Mills– Tackling deep part features? Harvey Tool’s tapered Miniature End Mills offer unique geometries that take the challenge out of tough-to-reach cuts.
Diamond tooling is essential to many moldmaking processes, particularly during electrode production and when machining non-metallic materials. Harvey Tool’s offering includes a wide selection of Diamond End Mills designed for use in abrasive and non-ferrous materials such as graphite, green carbide, green ceramics, and composites—materials commonly encountered in mold and die work.
These tools feature a CVD (Chemical Vapor Deposition) coating to promote longer tool life and uphold tight tolerances over extended machining cycles.
Highlighted tooling includes:
Finishers – Ball Profile (CVD Diamond) With available radii as small as 0.005″, these tools are ideal for finishing high-detail electrodes and intricate features.
Finishers – Corner Radius (CVD Diamond) Designed for applications requiring edge strength and tight tolerances, available with corner radii from 0.005″ to 0.0625″.
Diamond End Mills are frequently used in electrode machining for EDM (Electrical Discharge Machining), where precision in non-metallic workpieces directly influences final mold quality.
All tools in the Mold, Tool & Die offering are fully stocked and available to ship same day, helping to reduce lead times and keep your production on schedule.
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.
https://www.harveyperformance.com/wp-content/uploads/2025/01/DSC_0434.jpg5251400Thomas Donahuehttp://www.harveyperformance.com/wp-content/uploads/2018/08/Logo_HarveyPerformanceCompany-4.pngThomas Donahue2025-01-29 15:55:382025-01-30 09:14:54A Closer Look at Helical Solutions’ Tapered End Mills
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.
Carbon fiber is a woven cloth made of crystalline filaments of carbon cured with a polymer, which can be layered and shaped around a mold. It is an ideal material due to its impressive strength-to-weight ratio , meaning it’s very strong, but not heavy. Carbon fiber is five times lighter than steel with an equal elastic modulus, making it a better choice for many applications. Further, it is corrosion-resistant, non-flammable, and non-toxic, properties that make it an ideal material to use in aerospace, medical, construction, and military industries.
Machining Carbon Fiber
Machining Carbon Fiber can be challenging. The layered structure of the carbon fiber material can lead to delamination, uncut fibers, fiber tear-out, uneven tool wear, and poor surface finishes. Luckily, many cutting tool companies, like CoreHog, specially design tooling with different geometries that can help eliminate these manufacturing problems:
Straight Flute End Mills: Apply all the cutting forces radially, which helps prevent delamination.
Compression Cutters: Create opposite cutting forces, stabilizing material removal and preventing delamination, fiber pullout, and burrs along the surface.
Chipbreaker Cutters: Shear the fibers and shorten the chips, preventing fiber buildup around the cutter.
Diamond Cut End Mills: Utilize both left-hand and right-hand flutes to break up and shear through the fibers, ideal for roughing and profiling carbon fiber.
In the aerospace industry, carbon fiber is used in plane structures to replace alloys, creating lighter planes and thus, reducing fuel consumption. Recreational sports also utilize carbon fiber to decrease weight. It is often seen as a leading material in skis, bikes, and tennis rackets, as the lighter weight can help improve performance. In professional sports leagues like Formula 1 and NASCAR, carbon fiber has grown in prevalence in recent years. Another advantageous quality of carbon fiber is its suitability in X-ray machines, allowing imaging to pass through without interruption, making it useful in many medical devices and implants.
Recycling Carbon Fiber
Why is Recycling Carbon Fiber Difficult?
Carbon fiber sheets require a significant amount of energy to produce. These large sheets are then cut down to the part size needed, and the excess material is often discarded, increasing waste production. This material is not biodegradable and is typically sent to a landfill where it will remain permanently. Further complicating recycling, carbon fiber is built to hold its shape and strength and cannot be melted down and reshaped like many plastics. When recycled, its properties are heavily degraded, rendering it useless for applications that experience heavy forces or loads.
How is Carbon Fiber Recycled?
Solvolysis
Solvolysis uses a chemical solvent to break down the polymer encasing the carbon fiber cloth. The waste carbon fiber is shredded into smaller pieces, increasing the surface area. The solvent, chosen based on the polymers used in the carbon fiber, breaks down the polymer chains, separating the carbon fiber from the polymer. Techniques like centrifugation are used to separate the substances. The carbon fiber can be further purified to restore its properties and then combined with virgin fibers to create new fabric or used by itself. This process enables the recovery of carbon fiber without sacrificing material properties.
Pyrolysis
Pyrolytic utilizes heat to break down the polymer encasing the carbon fiber cloth. The waste carbon fiber is shredded into smaller pieces and then heated in a controlled environment with limited or no oxygen. At high temperatures, the polymer undergoes thermal decomposition, producing gases, vapors, and char. The gases and vapors can be used as an energy source or further processed, while the char, which is carbon fiber and any original additives, is purified to ensure mechanical properties are maintained. The resulting carbon fiber can be used alone or combined with virgin fibers. Pyrolysis is effective for high-quality fiber recovery and energy recovery from gas byproducts.
Carbon Fiber Considerations
As we innovate with new technology, it is important to consider its impact on our planet. Carbon fiber is an amazing material that can improve many aspects across industries; however, the waste generated is not going anywhere but a landfill. Many companies are investing in producing high-quality recycled carbon fiber. With a shift in focus to designing closed-loop systems for composite materials, the future looks bright.
https://www.harveyperformance.com/wp-content/uploads/2024/07/Feature-Image-Recyling-Carbon-Fiber-IMG.jpg5251400Sarah Wassonhttp://www.harveyperformance.com/wp-content/uploads/2018/08/Logo_HarveyPerformanceCompany-4.pngSarah Wasson2024-07-08 12:00:402024-07-12 12:46:58Recycling Carbon Fiber: Importance & Process
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.
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.
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.
Carbon Fiber Reinforced Polymers (CFRP) is a collection of carbon fibers that, when bound together via resin, creates a material with a wide range of application possibilities. It’s strong, durable, and resistant to corrosion, making it an advantageous material for use in several advanced industries, including the aerospace and automotive industries. Despite its unique abilities, however, machining CFRP is not without its set of challenges, all of which machinists must be cognizant of to achieve desired results. Once CFRP is properly understood and the right cutting tool is selected for the job, the next step is to properly set running parameters for your application.
Running Parameters
Comparison of Metal Machining vs Composite Machining
When machining CFRP, the suggested running parameters are to have a high RPM with low feed rates. Feed rates will need to be adjusted to account for heat minimization, while RPMs may need to be dialed back to prevent excessive fraying, tearing, or splitting of fibers when cutting.
In metal machining, the tool cuts away at material, forming chips. This is possible due to the formation of the metal having natural fracture and stress lines that can be wedged by the cutting tool to create a chip. Unlike metals, machining carbon fiber does not peel away material but rather fracture and break the fibers and resin.
Milling vs Drilling Carbon Fiber
Composite holemaking or drilling is found to be more challenging than milling carbon fiber. It generates more dust due to the drilling speed. Using specific tooling for composites will be crucial in effective drilling. When machining holes, the carbon fiber will relax, creating undersized holes which requires extensive adjustments that are best automated for efficiency.
For help mitigating the challenges of composite holemaking, read Overcoming Composite Holemaking Challenges and browse CoreHog’s offering of drills, specially engineered to mitigate all-too-common holemaking headaches. To achieve better finish and avoid delamination, it is recommended to utilize conventional milling over climb milling within composites contrary to what is recommended in metal machining.
Within the aerospace industry, drilling is the most common application in machining. Like milling, performing operations such as pecking may be preferred even with increased cycle time if it reduces any chances of error that result in scrapping of the part.
Running Parallel to Grain of Fibers
While every part is different, there is a method for reducing fraying, chipping, or delamination by cutting parallel to the fiber direction when possible. This can be like cutting along the grain of wood instead of cutting perpendicular or at an angle to the grain.
Coolant Applications
The use of coolant when machining CFRP can either benefit or negatively affect the part depending on the application. The preferred coolant of choice for machining carbon fiber is typically using water or a water-soluble coolant. This is due to composites having a porous surface that could allow contaminates to enter the part itself. By using water, it prevents any issues after machining where adhesives or paint may need to be applied to the part that otherwise would not have adhered properly with contaminates present.
High Scrapping Costs
Many composite parts are unique in shape and size with custom molded designs that create a large initial cost prior to the machining stage. After the part is molded near to its shape, machining is often used to finish the part or drill holes where needed to finalize the part.
Importance of Considering Machining Challenges to Avoid Scrapping
Having a set process that is consistent and reliable is important in helping to prevent scrapping. Eliminating human error with machines that can monitor the entire process while automating tool changes when tools are worn, avoids issues before they can happen. A key factor is ensuring the setup is correct, having the right tooling, tool path, and coolant option to perform the operation effectively and accurately. With some parts serving critical functions and with a high cost, there is no exception for poor finish or incorrect cuts emphasizing the importance of having a procedure that gets the job done the right way.
Composite Cutting Tool Life Management
Wear Rate & its Effects
Due to carbon fiber’s abrasion on the cutting tools, a rapid decrease in cutting quality will occur as soon as the tool begins to dull. Fibers will be grabbed instead of fractured, causing fraying and damage to the part. Therefore, tool life should be vigilantly monitored to replace the tool before reaching the point of dullness.
Developing a Process for Success
Unlike metal machining where tools may be utilized until they show signs of wear, this method would be unideal for CFRP as the highly expensive part could be ruined or damaged causing scrapping costs and time. It is good practice to take preventative measures by taking note of typical wear of your tools and using that information to set tool changes before it dulls. Noting tool changes and having high interval checks on cutting and dimension quality will aid in avoiding poor finish or scrapping. Some machines are equipped with tool life management systems which will greatly reduce the chances of having to scrap a part because of tool dullness.
Safety Practices When Machining CFRP
Being that chips are not formed when machining CFRP, and instead, the material is fractured, it creates dust that can spread throughout the air and other surfaces. Not only does this cause hazardous conditions for anyone nearby who may inhale the dust, but the dust is also conductive, which can ruin electronics. To avoid these issues, two different extraction methods can be used depending on the needs of the application.
Wet vs Dry Extraction
The two options for dust extraction are using coolant (wet) or vacuuming (dry). Choosing between the two is dependent on the application, but mostly dictated by the size of the application. Smaller scale machining can be contained through vacuuming, but larger applications would require coolant as vacuuming a large area may be challenging. If a lot of heat will be generated, then it is necessary to have a water-soluble coolant. This would also benefit the use of diamond tooling as they will wear faster at lower temperatures in comparison to carbide tooling. Another would be the dust collection would remain contained with the liquid preventing any airborne exposure.
Disposal Considerations
One benefit of vacuuming over coolant is the disposal process. After machining, the coolant/dust mix would require post-treatment to remove excess water before being transferred to a landfill. This would incur additional costs to the process which may cause some to lean towards vacuuming if heat is not an issue.
Conclusion
With CFRP’s wide range of uses and desirable mechanical properties for its applications, comes the effect of its challenges in machining and high cost of scrapping. Refining this process will be essential for the growing demand of carbon fiber machining in the near future. For more information on CFRP, specifically related to material properties and tool selection, read In the Loupe’s complementary post “Carbon Fiber Reinforced Polymers (CFRP): Material Properties & Tool Selection”.
Machinists oftentimes confuse wood for being an “easy to machine material” during CNC Woodworking because of how much softer the material is than metal. In some sense this is true, as you can program wood cutting parameters in CNC Woodworking with much higher feed rates compared to that of most metals. On the other hand, however, wood has many unique properties that need to be accounted for in order to optimize the cutting process for maximum efficiency.
There are 3 main categories of wood for woodworking: hardwood, softwood and engineered wood.
Hardwood
The textbook definition of a hardwood tree is an angiosperm, more commonly referred to as a broadleaf tree. A few examples would be oak, birch, and maple trees. These types of trees are often used for making high quality furniture, decks, flooring, and construction components.
Softwood
A softwood is a coniferous tree, sometimes known as a gymnosperm. These are typically less dense than hardwoods and are therefore associated with being easier to machine. Do not let the name fool you: some soft woods are harder than some hardwoods. Harvey Tool’s Speeds and Feeds Charts for its offering of Material Specific End Mills for Wood are categorized by Janka hardness for this exact reason. Janka hardness is a modified hardness scale with a test specifically designed for classifying types of wood.
Softwood is used to make furniture, but can also be used for doors, window panes, and paper products. A couple of examples are pine and cedar trees. Table 1 lists 20 common woods with their Janka hardness.
Common Name:
Janka Imperial Hardness:
Balsa
90
Buckeye, Yellow
350
Willow, Black
360
Pine, Sugar
380
Cottonwood, Eastern
430
Chesnut, American
540
Pine, Red
560
Douglas-Fir, Interior North
600
Birch, Gray
760
Ash, Black
850
Cedar, Eastern Red
900
Cherry, American Black
950
Walnut, Black
1010
Beech, American
1300
Oak, White
1360
Maple, Sugar
1450
Apple
1730
Cherry, Brazilian
2350
Olive
2700
Rosewood, Indian
3170
Table 1: Janka Hardness of Common Woods
Engineered Woods
Engineered wood, or composite wood, is any type of wood fiber, particle, or strand material held together with an adhesive or binding agent. Although some of these materials are easier to machine than solid woods, the adhesive holding the material together can be extremely abrasive. This can cause premature tool wear and create difficulties when cnc woodworking. It’s important to note that some types of engineered woods are more difficult to machine than others, specifically those with a higher amount of binding material. These types should be programmed with less aggressive speeds and feeds. For example, medium density fiberboard (MDF) if more difficult to machine than plywood, but much easier to machine than phenolic.
Figure 1: Example of Medium Density Fiberboard
Properties of Wood
Grain Size
Technically speaking, wood can be considered a natural composite material as it consists of strong and flexible cellulose fibers held together by a stiffer glue-like matrix composed of lignin and hemicellulose. If you think in terms of construction, the cellulose fibers would be the steel rebar, and the concrete would be the lignin and hemicellulose. Wood with large cellulose fibers are considered to be coarse-grained (oak and ash). Woods that have smaller and fewer fibers are considered fine-grained (pine and maple). Softwoods tend to be fine-grained and are therefore stereotyped as being easier to machine since they do not have as many strong fibers to shear. It’s important to note that not all hardwood trees are coarse grained and not all softwood trees are fine-grained.
Figure 2: Simplified diagram of fibers that constitute natural wood. The cellulose fibers run vertically in this depiction.
Moisture Content (MC)
Moisture content (MC) is one of the most important variables to consider when machining wood. An extremely common problem with building anything with wood is its tendency to warp. Moisture variability in the air inevitably affects the moisture content within the wood. Any change in moisture content (whether an increase or a decrease) will disturb the shape of the workpiece. This is why one must take into account what type of moisture a product will be exposed to in its final resting place.
Equilibrium Moisture Content (EMC)
Equilibrium moisture content (EMC) occurs when wood has reached a balance point in its moisture content. Interior EMC values across the United States average at about 8%, with exterior values averaging around 12%. These values vary around the country due to the differences in temperature and humidity. For example, the southeastern United States have an average interior EMC of 11% while the southwest averages about 6% (excluding the coastal region). It’s important to consider what region and application the final product is going to encounter so that the wood with the correct moisture content can be selected before machining. Most species of flat-grain wood will change size 1% for every 4% change in MC. The direction of warping depends on the grain orientation.
Figure 4: Average regional indoor EMC
Generally, power requirements for an operation rise with increasing moisture content, mainly because of the surge in density. Density of wood increases with rising MC. The additional power may be necessary to push a heavier chip out of the cutting zone during CNC Woodworking. It’s worth noting that, like synthetic polymers, wood is a viscoelastic material that absorbs energy as it becomes wetter. The proportional limit of its mechanical properties intensifies as MC increases.
When machining some types of wood, cutting region temperature will surge with increasing MC, but in other species it will decline. Be safe and avoid rapid tool wear by decreasing SFM when machining a wood with a moisture content above 10%. Harvey Tool Speeds and Feeds Charts suggest a decrease of 30 per MC percentage point. As always, though, it depends on the type of wood being machined and the type of operation being performed.
Temperature change is not the only reason higher moisture content is associated with rapid tool wear. Moisture within wood isn’t just associated with water, but also with resins, sugars, oils, starches, alkaloids, and tannin present within the water. These substances react particularly well with high speed steel, and to a lesser degree with carbide.
Knots and Their Effect on CNC Woodworking
A knot is a portion of a branch or limb that has become incorporated in the trunk of a tree. The influence of knots on the mechanical properties of wood is due to the interruption of continuity and change in direction of wood fibers associated with it. These properties are lower in this portion of the wood because the fibers around the knot are distorted and lead to stress concentrations. “Checking” (cracking due to shrinking) often occurs around knots during drying. Hardness and strength perpendicular to the grain are exceptions to generally lower mechanical properties. Because of these last two exceptions, woodworking machining parameters should be reduced when encountering a knotted portion of the workpiece to avoid shock loading.
