Chip Evacuation - In the Loupe Machinist Blog

Tag Archive for: Chip Evacuation

Shining a Light on Diamond End Mills

May 10, 2018/5 Comments/in CNC Machining, Tool Coatings, Tool Selection/by Robert Keever

Diamond tooling and diamond-coated end mills are a great option when machining highly abrasive materials, as the coating properties help to significantly increase tool life relative to uncoated carbide tools. Diamond tools and diamond-like coated tools are only recommended for non-ferrous applications, including highly abrasive materials ranging from graphite to green ceramics, as they have a tendency to break down in the presence of extreme heat.

Understanding the Properties of Diamond Coatings

To ensure proper diamond tooling selection, it’s critical to understand the unique properties and makeup of the coatings, as there are often several diamond coating variations to choose from. Harvey Tool, for example, stocks Amorphous Diamond, CVD Diamond, and PCD Diamond End Mills for customers looking to achieve significantly greater tool life when working in non-ferrous applications.

Diamond, the hardest known material on earth, obtains its strength from the structure of carbon molecules. Graphite, a relatively brittle material, can have the same chemical formula as diamond, but is a completely different material; while Graphite has a sp² bonded hexagonal structure, diamond has a sp³ bonded cubic structure. The cubic structure is harder than the hexagonal structure as more single bonds can be formed to interweave the carbon into a stronger network of molecules.

Amorphous Diamond Coating

Amorphous Diamond is transferred onto carbide tools through a process called physical vapor deposition (PVD). This process spreads a mono-layer of DLC coating about 0.5 – 2.5 microns thick onto any given tool by evaporating a source material and allowing it to condense onto that tool over the course of a few hours.

Chemical Vapor Deposition (CVD)

Chemical Vapor Deposition (CVD) is a coating process used to grow multiple layers of polycrystalline diamond onto carbide tooling. This procedure takes much longer than the standard PVD coating method. During the coating process, hydrogen molecules are dissociated from the carbon molecules deposited onto the tool, leaving a diamond matrix under the right temperature and pressure conditions. Under the wrong conditions, the tool may be simply coated in graphite. 6% cobalt carbide blanks allow for the best adhesion of diamond and a substrate. CVD diamond coated end mills have a typical thickness of coating that is between 8 and 10 microns thick.

Polycrystalline Diamond (PCD)

Polycrystalline Diamond (PCD) is a synthetic diamond, meaning it is grown in a lab and contains mostly cubic structures. Diamond hardness ranges from about 80 GPa up to about 98 GPa. PCD end mills have the same diamond structure as CVD diamond tools but the binding technique is different. The diamond starts in a powdery form that is sintered onto a carbide plate using cobalt as a solvent metal substrate. This is done at an extreme temperature and pressure as the cobalt infiltrates the powder, causing the grains to grow together. This effectively creates a thick diamond wafer, between 010” and .030” in width, with a carbide base. This carbide base is then brazed onto the head an end mill and sharpened.

How Diamond Coatings Differ

Coating Hardness & Thickness

Polycrystalline tools (CVD or sintered) have a much higher hardness, thickness, and max working temperature than Amorphous Diamond oated tools. As mentioned previously, a PCD tool consists of a diamond wafer brazed to a carbide body while a CVD tool is a carbide end mill with a relatively thick layer of polycrystalline diamond grown into it. This grown layer causes the CVD tools to have a rounded cutting edge compared to PCD and Amorphous Diamond coated tools. PCD tools have the thickest diamond layer that is ground to a sharp edge for maximum performance and tool life. The difference between PCD tools and CVD coated tools lies in the thickness of this coat and the sharpness of the cutting edge. Amorphous Diamond tools maintain a sharper edge than CVD coated tools because of their thin coating.

Flute Styles

Harvey Tool’s line of PCD end mills are all straight fluted, CVD coated tools are all helically fluted, and Amorphous Diamond tools are offered in a variety of options. The contrast between straight fluted and helically fluted can be seen in the images below, PCD (top) and CVD (bottom). Electrical discharge machining, grinding or erosion are used cut the PCD wafer to the specifications. The size of this wafer limits the range of diameters that can be achieved during manufacturing. In most situations a helically fluted tool would be preferred over a straight fluted tool but with true diamond tooling that is not the case. The materials that PCD tools and CVD coated tools are typically used to cut produce a powdery chip that does not require the same evacuation that a metallic or plastic chip necessitates.

PCD Ball End Mill

CVD Ball End Mill

Proper Uses

CVD tools are ideally suited for abrasive material not requiring a sharp cutting edge – typically materials that produce a powdery chip such as composites and graphite. Amorphous Diamond tools have a broad range of non-ferrous applications spanning from carbon fiber to precious metals but ceramics are typically outside their range as they can be too abrasive and wear away the coating. PCD tools overlap their CVD and DLC coated counterparts as they can be used for any non-ferrous abrasive material.

Cut to the Point

Harvey Tool carries physical vapor deposition diamond-like carbon coated tools, chemical vapor deposition diamond tools and polycrystalline diamond tools. PCD tools are composed of the thickest diamond wafer brazed onto a carbide shank and are ground to a sharp edge. CVD coated tools have the diamond grown into a carbide end mill. Amorphous Diamond coated tools have the DLC coated onto them through the PVD process. For more information on the diamond coating best suited for your operation, contact a Harvey Tool Tech Team Member for immediate help.

Tool Deflection & Its Remedies

May 3, 2018/6 Comments/in CNC Machining, How-To's, Machining 101, Troubleshooting Tips/by Jacob Concepcion

What is Tool Deflection?

Every machinist must be aware of tool deflection, as too much deflection can lead to catastrophic failure in the tool or workpiece. Deflection is the displacement of an object under a load causing curvature and/or fracture.

For Example: When looking at a diving board at rest without the pressure of a person’s weight upon it, the board is straight. But as the diver progresses down further to the end of the board, it bends further. Deflection in tooling can be thought of in a similar way.

Signs of Tool Deflection

Shortened tool life and/or tool breakage
Subpar surface finish
Part dimensional inaccuracies

Tool Deflection Remedies

Minimize Overhang

Overhang refers to the distance a tool is sticking out of the tool holder. Simply, as overhang increases, the tool’s likelihood of deflection increases. The larger distance a tool hangs out of the holder, the less shank there is to grip, and depending on the shank length, this could lead to harmonics in the tool that can cause fracture. Simply put, For optimal working conditions, minimize overhang by chucking the tool as much as possible.

extended reach tool in tool holder with overhang depth called out — Image Source: @NuevaPrecision

Long Flute vs. Long Reach

Another way to minimize deflection is having a full grasp on the differences between a long flute and a long reach tool. The reason for such a difference in rigidity between the two is the core diameter of the tool. The more material, the more rigid the tool; the shorter the length of flute, the more rigid the tool and the longer the tool life. While each tooling option has its benefits and necessary uses, using the right option for an operation is important.

The below charts illustrate the relationship between force on the tip and length of flute showing how much the tool will deflect if only the tip is engaged while cutting. One of the key ways to get the longest life out of your tool is by increasing rigidity by selecting the smallest reach and length of cut on the largest diameter tool.

tool deflection in relation to length of tool

Click Here to Learn More About Proper Tool Holding and Runout

When to Opt for a Long Reach Tool

Reached tools are typically used to remove material where there is a gap that the shank would not fit in, but a noncutting extension of the cutter diameter would. This length of reach behind the cutting edge is also slightly reduced from the cutter diameter to prevent heeling (rubbing of noncutting surface against the part). Reached tools are one of the best tools to add to a tool crib because of their versatility and tool life.

long reach ball end mill — Long Reach Tool: Variable Helix End Mills for Exotic Alloys – Ball – Long Reach, Stub Flute

When to Opt for a Long Flute Tool

Long Flute tools have longer lengths of cut and are typically used for either maintaining a seamless wall on the side of a part, or within a slot for finishing applications. The core diameter is the same size throughout the cutting length, leading to more potential for deflection within a part. This possibly can lead to a tapered edge if too little of the cutting edge is engaged with a high feed rate. When cutting in deep slots, these tools are very effective. When using HEM, they are also very beneficial due to their chip evacuation capabilities that reached tools do not have.

long flute end milling tool — Long Flute Tool: Miniature End Mills – Square Long Flute

Deflection & Tool Core Strength

Diameter is an important factor when calculating deflection. Machinists oftentimes use the cutter diameter in the calculation of long flute tools, when in actuality the core diameter (shown below) is the necessary dimension. This is because the fluted portion of a tool has an absence of material in the flute valleys. For a reached tool, the core diameter would be used in the calculation until its reached portion, at which point it transitions to the neck diameter. When changing these values, it can lower deflection to a point where it is not noticeable for the reached tool but could affect critical dimensions in a long flute tool.

core diameter vs neck diameter infographic

Deflection Summarized

Tool deflection can cause damage to your tool and scrap your part if not properly accounted for prior to beginning a job. Be sure to minimize the distance from the tool holder to the tip of the tool to keep deflection to a minimum. For more information on ways to reduce tool deflection in your machining, view Diving into Depth of Cut.

Attacking Aluminum: a Machining Guide

April 24, 2018/11 Comments/in Aluminum, CNC Machining, Helical Solutions, Material Specific, Milling, Tech Tips/by Harvey Performance Company

Aluminum is one of the most commonly machined materials, as most forms of the material feature excellent machinability, and is thus a commonly used material in manufacturing. Because of this, the competition for aluminum machining can be intense. Understanding the basics behind tool selection, running parameters, and advanced milling techniques for aluminum can help machinists earn a competitive advantage.

Material Properties

Aluminum is a highly formable, workable, lightweight material. Parts made from this material can be found in nearly every industry. Additionally, Aluminum has become a popular choice for prototypes due to its low-cost and flexibility.

Aluminum is available in two basic forms: Cast and Wrought. Wrought Aluminum is typically stronger, more expensive, and contains a lower percentage of outside elements in its alloys. Wrought Aluminum is also more heat-resistant than Cast and has a higher level of machinability.

Cast Aluminum has less tensile strength but with a higher flexibility. It costs less, and has higher percentages of outside elements (silicon, magnesium, etc.) in its alloys, making it more abrasive than Wrought.

Shop Helical Solutions’ End Mills for Aluminum & Non-ferrous Materials

Tool Geometry

There are a few coating options available for Aluminum tooling, including the popular gold-colored ZrN (Zirconium Nitride) and the lesser known but highly effective TiB₂ (Titanium Diboride). Uncoated tooling can also provide solid machining performance. However, the real key to high performance machining in Aluminum is knowing the proper flute count and helix angle required for your operation.

Flute Count

End mills for aluminum are often available in either 2 flute or 3 flute styles. With higher flute counts, it would become difficult to evacuate chips effectively at the high speeds at which you can run in aluminum. This is because aluminum alloys leave a large chip, and chip valleys become smaller with each additional flute on an end mill.

Traditionally, 2 flute end mills have been the preferred choice for Aluminum. However, 3 flute end mills have proven to be more successful in many finishing operations, and with the right parameters they can also work successfully as roughers. While much of the debate between 2 and 3 flute end mills for Aluminum boils down to personal preference, the operation, rigidity, and desired material removal rates can also have an effect on tool selection.

Helix Angles

The helix angle of a tool is measured by the angle formed between the centerline of the tool and a straight line tangent along the cutting edge. Cutting tools for aluminum typically feature higher helix angles than standard end mills. Specialized helix angles for Aluminum are typically either 35°, 40°, or 45°. Variable helix tools are also available and make a great choice for reducing chatter and harmonics while also increasing material removal rates.

35, 40, and 45 degree helix choices for Aluminum Machining end mills

A helix angle of 35° or 40° is a good choice for traditional roughing and slotting applications. A 45° helix angle is the preferred choice for finishing, but also for High Efficiency Milling toolpaths as the high helix angle wraps around the tool faster and makes for a more aggressive cut.

Tooling Options

When machining aluminum, standard 2 or 3 flute tools will often get the job done. However, for certain applications and machine setups there are some more tooling options to consider for even better performance.

helical solutions end mills for aluminum and non-ferrous materials ad

Chipbreaker Tooling

One of the most important things to consider when machining aluminum (and many other materials) is effective chip evacuation. Standard 2-3 flute end mills running at recommended speeds and feeds and proper chip loads can evacuate chips fairly well. However, 3 flute chipbreaker tooling can run at increased speed and feed rates for even better performance. The unique offset chip breaker geometry creates smaller chips for optimal evacuation while still leaving a semi-finished surface.

These tools are excellent for more advanced toolpaths like High Efficiency Milling, which is another important tool for a successful aluminum machining experience.

High Balance End Mills

High balance end mills are designed to significantly increase performance in highly balanced machining centers capable of elevated RPMs and feed rates. These tools are precision balanced specifically for high velocity machining in aluminum (up to 33,000 RPM).

Zoomed in image of helical solutions High Balance coolant through Tool for Aluminum

Helical Solutions offers high balance tooling in standard 2 flute styles, as well as coolant-through 3 flute styles for reduced heat, enhanced chip evacuation, and increased material removal rates. These tools, like the chipbreakers, are also an excellent choice for High Efficiency Milling toolpaths.

Running Parameters

Setting the right parameters for aluminum applications is vital to optimizing productivity and achieving better machining results. Since aluminum is an easier material to machine, pushing your machine to its limits and getting the most out of your tool is vital to stay ahead of the competition and keep winning business.

While there are many factors that go into the parameters for every job, there are some general guidelines to follow when machining aluminum. For cast aluminum alloys (i.e. 308, 356, 380), a surface footage of 500-1000 SFM is recommended, with RPMs varying based on cutter diameter. The basic calculation to find a starting point for RPMs would be (3.82 x SFM) / Diameter.

In wrought aluminum alloys (i.e. 2024, 6061, 7075), a surface footage of 800-1500 SFM is recommended, with the same calculation being used to find a starting point for RPMs.

High Efficiency Milling

High Efficiency Milling, commonly known as HEM, is a strategy that is rapidly gaining popularity in the manufacturing industry. Many CAM programs are now including HEM toolpaths, and while virtually any machine can perform HEM, the CNC controller must feature a fast processor to keep up with the additional lines of code. A great example of High Efficiency Milling toolpaths in Aluminum can be seen below.

At its core, HEM is a roughing technique that utilizes a low Radial Depth of Cut (RDOC) and a high Axial Depth of Cut (ADOC) to take full advantage of the cutting edge of the tool. To learn more about how High Efficiency Milling can increase your efficiency, extend your tool life to keep costs down, and get greater performance for aluminum (and other materials), click here to download the HEM Guidebook.

In Summary

Aluminum is a versatile material with a high level of machinability, but it should not be overlooked. Understanding the best ways to tackle it is important for achieving the desired results. Optimizing your tool crib, machine setups, and toolpaths for aluminum is essential to stay ahead of the competition and make your shop more efficient.

Selecting the Right Harvey Tool Miniature Drill

April 19, 2018/0 Comments/in Drilling, Drilling & Holemaking, Harvey Tool, Holemaking, Tool Geometry, Tool Information Guides, Tool Selection/by Harvey Performance Company

Among Harvey Tool’s expansive holemaking solutions product offering are several different types of miniature drill options and their complements. Options range from Miniature Spotting Drills to Miniature High Performance Drills – Deep Hole – Coolant Through. But which tools are appropriate for the hole you aim to leave in your part? Which tool might your current carousel be missing, leaving efficiency and performance behind? Understanding how to properly fill your tool repertoire for your desired holemaking result is the first step toward achieving success.

Pre-Drilling Considerations

Miniature Spotting Drills

Depending on the depth of your desired machined hole and its tolerance mandates, as well as the surface of the machine you will be drilling, opting first for a Miniature Spotting Drill might be beneficial. This tool pinpoints the exact location of a hole to prevent common deep-hole drilling mishaps such as walking, or straying from a desired path. It can also help to promote accuracy in instances where there is an uneven part surface for first contact. Some machinists even use Spotting Drills to leave a chamfer on the top of a pre-drilled hole. For extremely irregular surfaces, however, such as the side of a cylinder or an inclined plane, a Flat Bottom Drill or Flat Bottom Counterbore may be needed to lessen these irregularities prior to the drilling process.

Tech Tip: When spotting a hole, the spot angle should be equal to or wider than the angle of your chosen miniature drill. Simply, the miniature drill tip should contact the part before its flute face does.

Selecting the Right Miniature Drill

Harvey Tool stocks several different types of miniature drills, but which option is right for you, and how does each drill differ in geometry?

Miniature Drills

Harvey Tool Miniature Drills are popular for machinists seeking flexibility and versatility with their holemaking operation. Because this line of tooling is offered uncoated in sizes as small as .002” in diameter, machinists no longer need to compromise on precision to reach very micro sizes. Also, this line of tooling is designed for use in several different materials where specificity is not required.

Miniature High Performance Drills – Deep Hole – Coolant Through

For situations in which chip evacuation may be difficult due to the drill depth, Harvey Tool’s Deep Hole – Coolant Through Miniature Drills might be your best option. The coolant delivery from the drill tip will help to flush chips from within a hole, and prevent heeling on the hole’s sides, even at depths up to 20 multiples of the drill diameter.

Miniature High Performance Drills – Flat Bottom

Choose Miniature High Performance Flat Bottom Drills when drilling on inclined and rounded surfaces, or when aiming to leave a flat bottom on your hole. Also, when drilling intersecting holes, half holes, shoulders, or thin plates, its flat bottom tool geometry helps to promote accuracy and a clean finish.

Miniature High Performance Drills – Aluminum Alloys

The line of High Performance Drills for Aluminum Alloys feature TiB2 coating, which has an extremely low affinity to Aluminum and thus will fend off built-up edge. Its special 3 flute design allows for maximum chip flow, hole accuracy, finish, and elevated speeds and feeds parameters in this easy-to-machine material.

Miniature High Performance Drills – Hardened Steels

Miniature High Performance Drills – Hardened Steels features a specialized flute shape for improved chip evacuation and maximum rigidity. Additionally, each drill is coated in AlTiN Nano coating for hardness, and heat resistance in materials 48 Rc to 68 Rc.

Miniature High Performance Drills – Prehardened Steels

As temperatures rise during machining, the AlTiN coating featured on Harvey Tool’s Miniature High Performance Drills – Prehardened Steels creates an aluminum oxide layer which helps to reduce thermal conductivity of the tool and helps to promote heat transfer to the chip, as well as improve lubricity and heat resistance in ferrous materials.

Post-Drilling Considerations

Miniature Reamers

For many operations, drilling the actual hole is only the beginning of the job. Some parts may require an ultra-tight tolerance, for which a Miniature Reamer (tolerances of +.0000″/-.0002″ for uncoated and +.0002″/-.0000″ for AlTiN Coated) can be used to bring a hole to size.

Tech Tip: In order to maintain appropriate stock removal amounts based on the reamer size, a hole should be pre-drilled at a diameter that is 90-94 percent of the finished reamed hole diameter.

Flat Bottom Counterbores

Other operations may require a hole with a flat bottom to allow for a superior connection with another part. Flat Bottom Counterbores leave a flat profile and straighten misaligned holes. For more information on why to use a Flat Bottom Counterbore, read 10 Reasons to Use Flat Bottom Tools.

Key Next Steps

Now that you’re familiar with miniature drills and complementary holemaking tooling, you must now learn key ways to go about the job. Understanding the importance of pecking cycles, and using the correct approach, is vital for both the life of your tool and the end result on your part. Read this post’s complement “Choosing the Right Pecking Cycle Approach,” for more information on the approach that’s best for your application.

Choosing the Right Pecking Cycle Approach

April 19, 2018/1 Comment/in CNC Machining, Holemaking, How-To's, Machining 101/by Harvey Performance Company

Utilizing a proper pecking cycle strategy when drilling is important to both the life of your tool and its performance in your part. Recommended cycles vary depending on the drill being used, the material you’re machining, and your desired final product.

Start to Boost Your Accuracy with Harvey Tool’s Drilling Guidebook.

What are Pecking Cycles?

Rather than drill to full drill depth in one single plunge, pecking cycles involve several passes – a little at a time. Peck drilling aids the chip evacuation process, helps support tool accuracy while minimizing walking, prevents chip packing and breakage, and results in a better all around final part.

Recommended Pecking Cycles / Steps

Miniature Drills

High Performance Drills – Flat Bottom

High Performance Drills – Aluminum & Aluminum Alloys

Note: For hole depths 12x or greater, a pilot hole of up to 1.5X Diameter is recommended.

High Performance Drills – Hardened Steels

High Performance Drills – Prehardened Steels

Key Pecking Cycle Takeaways

From the above tables, it’s easy to identify how recommended peck drilling cycles change based on the properties of the material being machined. Unsurprisingly, the harder the material is, the shorter the recommended pecking depths are. As always, miniature drills with a diameter of less than .010″ are extremely fragile and require special precautions to avoid immediate failure. For help with your specific job, contact the Harvey Tool Technical Team at 800-645-5609 or [email protected]

Contouring Considerations

April 2, 2018/0 Comments/in CNC Machining, CNC Programming, Machining Techniques, Tech Tips, Tools In Action/by Jacob Concepcion

What is Contouring?

Contouring a part means creating a fine finish on an irregular or uneven surface. Dissimilar to finishing a flat or even part, cnc contouring involves the finishing of a rounded, curved, or otherwise uniquely shaped part.

CNC Contouring & 5-Axis Machining

5-axis machines are particularly suitable for contouring applications. Because contouring involves the finishing of an intricate or unique part, the multiple axes of movement in play with 5-axis Machining allow for the tool to access tough-to-reach areas, as well as follow intricate tool paths.

Recent Advances

Advanced CAM software can now write the G-Code (the step-by-step program needed to create a finished part) for a machinists application, which has drastically simplified contouring applications. Simply, rather than spend several hours writing the code for an application, the software now handles this step. Despite these advances, most young machinists are still required to write their own G-Codes early on in their careers to gain valuable familiarity with the machines and their abilities. CAM software, for many, is a luxury earned with time.

Benefits of Advanced CAM Software

Increased Time Savings
Because contouring requires very specific tooling movements and rapidly changing cutting parameters, ridding machinists of the burden of writing their own complex code can save valuable prep time and reduce machining downtime.

Reduced Cycle Times
Generated G-Codes can cut several minutes off of a cycle time by removing redundancies within the application. Rather than contouring an area of the part that does not require it, or has been machined already, the CAM Software locates the very specific areas that require machining time and attention to maximize efficiency.

Improved Consistency
CAM Programs that are packaged with CAD Software such as SolidWorks are typically the best in terms of consistency and ability to handle complex designs. While the CAD Software helps a machinist generate the part, the CAM Program tells a machine how to make it.

Proper Tips

Utilize Proper Cut Depths

Prior to running a contouring operation, an initial roughing cut is taken to remove material in steps on the Z-axis so to leave a limited amount of material for the final contouring pass. In this step, it’s pivotal to leave the right amount of material for contouring — too much material for the contouring pass can result in poor surface finish or a damaged part or tool, while too little material can lead to prolonged cycle time, decreased productivity and a sub par end result.

The contouring application should remove from .010″ to 25% of the tool’s cutter diameter. During contouring, it’s possible for the feeds to decrease while speeds increases, leading to a much smoother finish. It is also important to keep in mind that throughout the finishing cut, the amount of engagement between the tool’s cutting edge and the part will vary regularly – even within a single pass.

Use Best Suited Tooling

Ideal tool selection for contouring operations begins by choosing the proper profile of the tool. A large radius or ball profile is very often used for this operation because it does not leave as much evidence of a tool path. Rather, they effectively smooth the material along the face of the part. Undercutting End Mills, also known as lollipop cutters, have spherical ball profiles that make them excellent choices for contouring applications. Harvey Tool’s 300° Reduced Shank Undercutting End Mill, for example, features a high flute count to benefit part finish for light cut depths, while maintaining the ability to reach tough areas of the front or back side of a part.

Fact-Check G-Code

While advanced CAM Software will create the G-Code for an application, saving a machinist valuable time and money, accuracy of this code is still vitally important to the overall outcome of the final product. Machinists must look for issues such as wrong tool call out, rapids that come too close to the material, or even offsets that need correcting. Failure to look G-Code over prior to beginning machining can result in catastrophic machine failure and hundreds of thousands of dollars worth of damage.

Inserting an M01 – or a notation to the machine in the G-Code to stop and await machinist approval before moving on to the next step – can help a machinist to ensure that everything is approved with a next phase of an operation, or if any redundancy is set to occur, prior to continuation.

Contouring Summarized

CNC contouring is most often used in 5-axis machines as a finishing operation for uniquely shaped or intricate parts. After an initial roughing pass, the contouring operation – done most often with Undercutting End Mills or Ball End Mills, removes anywhere from .010″ to 25% of the cutter diameter in material from the part to ensure proper part specifications are met and a fine finish is achieved. During contouring, cut only at recommended depths, ensure that G-Code is correct, and use tooling best suited for this operation.

5 Ways Your Shop is Inefficient

March 5, 2018/2 Comments/in Getting Started, Machining 101, Machining Techniques, Troubleshooting Tips/by Harvey Performance Company

5 Ways Your Shop is Inefficient

In today’s ultracompetitive industry, every machine shop seeks even the slightest edge to gain an advantage on their competition and boost their bottom line. However, what many machinists don’t know is that improving their shop’s efficiency might be easier than they thought. The following five ways your shop is inefficient will provide a clear starting point of where to look for machinists desperate to earn a competitive edge.

Premature Tool Decay / Tool Failure

If you’re finding that your tools are failing or breaking at an unacceptable rate, don’t mistake it for commonplace. It doesn’t have to be. Prolonging the life of your tooling starts with finding not just the right tool, but the best one; as well as running it in a way to get its optimal performance. Many machinists mistake premature tool failure with running parameters that were too aggressive. In fact, not pushing the tool to its full potential can actually cause it to decay at an accelerated rate in certain situations.

Tool failure can occur in many different ways: Abrasive Wear, Chipping, Thermal Cracking or Tool Fracture, just to name a few. Understanding each type and its causes can help you to quickly boost your shop’s efficiency by minimizing downtime and saving on replacement tool costs.

close up view of excessive tool wear on a cutting edge

An example of a tool with excessive wear

For more information on tool wear, view Avoiding 4 Major Types of Tool Wear.

Subpar Part Finish

Your shop spends money to employ machinists, run machines, and buy cutting tools. Get your money’s worth, lead the industry, and ensure that you’re providing your customers with the highest quality product. Not only will this help to keep your buyer-seller relationship strong, but it will allow you the flexibility to increase your prices in the future, and will attract prospective customers.

Many factors influence part finish, including the material and its hardness, the speeds and feeds you’re running your tool at, tool deflection, and the tool-to-workpiece orientation.

For more information on ways to improve your part finish, view our Part Finish Reference Guide.

Inefficient Coolant Usage

One often forgotten expense of a machine shop is coolant – and it can be pricey. A 55-gallon drum of coolant can run more than $1,500. What’s worse is that coolant is often applied in excess of what’s required for the job. In fact, some machines even feature a Minimum Quantity Lubricant (MQL) functionality, which applies coolant as an extremely fine mist or aerosol, providing just enough coolant to perform a given operation effectively. While drowning a workpiece in coolant, known as a “Flood Coolant,” is sometimes needed, it is oftentimes utilized on jobs that would suffice with much less.

For more information about coolants and which method of application might be best for your job, view What You Need to Know About Coolant for CNC Machining.

Not Taking Advantage of Tool Versatility

Did you know that several CNC cutting tools can perform multiple operations? For example, a Chamfer Mill can chamfer, bevel, deburr, and countersink. Some Chamfer Mills can even be used as a Spotting Drill. Of course, the complexity of the job will dictate your ability to reap the benefits of a tool’s versatility. For instance, a Spotting Drill is obviously the best option for spotting a hole. If performing a simple operation, though, don’t go out of your way to buy additional tooling when what’s already in your carousel can handle it.

To learn more about versatile tools that can perform multiple applications, check out Multi-Functional Tools Every Shop Should Have.

High Machine Downtime Makes Your Shop Inefficient

What use is a machine that’s not running beside making your shop inefficient? Minimizing machine downtime is a key way to ensure that your shop is reaching its efficiency pinnacle. This can be accomplished a variety of ways, including keeping like-parts together. This allows for a simple swap-in, swap-out of material to be machined by the same cutting tool. This saves valuable time swapping out tooling, and lets your machine to do its job for more time per workday. Production planning is a key factor to running an efficient machine shop.

The Advances of Multiaxis Machining

February 19, 2018/3 Comments/in CNC Machining, CNC Machining Videos, CNC Programming, Machining 101, Machining Techniques, Tools In Action/by Jacob Concepcion

CNC Machine Growth

As the manufacturing industry has developed, so too have the capabilities of machining centers. CNC Machines are constantly being improved and optimized to better handle the requirements of new applications. Perhaps the most important way these machines have improved over time is in the multiple axes of direction they can move, as well as orientation. For instance, a traditional 3-axis machine allows for movement and cutting in three directions, while a 2.5-axis machine can move in three directions but only cut in two. The possible number of axes for a multiaxis machine varies from 4 to 9, depending on the situation. This is assuming that no additional sub-systems are installed to the setup that would provide additional movement. The configuration of a multiaxis machine is dependent on the customer’s operation and the machine manufacturer.

Multiaxis Machining

With this continuous innovation has come the popularity of multiaxis machines – or CNC machines that can perform more than three axes of movement (greater than just the three linear axes X, Y, and Z). Additional axes usually include three rotary axes, as well as movement abilities of the table holding the part or spindle in place. Machines today can move up to 9 axes of direction.

https://www.instagram.com/p/BdssKBsg0Sa/

Multiaxis machines provide several major improvements over CNC machines that only support 3 axes of movement. These benefits include:

Increasing part accuracy/consistency by decreasing the number of manual adjustments that need to be made.
Reducing the amount of human labor needed as there are fewer manual operations to perform.
Improving surface finish as the tool can be moved tangentially across the part surface.
Allowing for highly complex parts to be made in a single setup, saving time and cost.

9-Axis Machine Centers

The basic 9-axis naming convention consists of three sets of three axes.

Set One

The first set is the X, Y, and Z linear axes, where the Z axis is in line with the machine’s spindle, and the X and Y axes are parallel to the surface of the table. This is based on a vertical machining center. For a horizontal machining center, the Z axis would be aligned with the spindle.

Set Two

The second set of axes is the A, B, and C rotary axes, which rotate around the X, Y, and Z axes, respectively. These axes allow for the spindle to be oriented at different angles and in different positions, which enables tools to create more features, thereby decreasing the number of tool changes and maximizing efficiency.

Set Three

The third set of axes is the U, V, and W axes, which are secondary linear axes that are parallel to the X, Y, and Z axes, respectively. While these axes are parallel to the X, Y, and Z axes, they are managed by separate commands. The U axis is common in a lathe machine. This axis allows the cutting tool to move perpendicular to the machine’s spindle, enabling the machined diameter to be adjusted during the machining process.

The Growing Industry of Multiaxis Machining

In summary, as the manufacturing industry has grown, so too have the abilities of CNC Machines. Today, tooling can move across nine different axes, allowing for the machining of more intricate, precise, and delicate parts. Additionally, this development has worked to improve shop efficiency by minimizing manual labor and creating a more perfect final product.

What You Need to Know About Coolant for CNC Machining

December 5, 2017/9 Comments/in CNC Machining, Quick Tips, Tech Tips, Titan USA, Troubleshooting Tips/by Harvey Performance Company

Coolant in purpose is widely understood – it’s used to temper high temperatures common during machining, and aid in chip evacuation. However, there are several types and styles, each with its own benefits and drawbacks. Knowing which cnc coolant – or if any – is appropriate for your job can help to boost your shop’s profitability, capability, and overall machining performance.

Coolant or Lubricant Purpose

Coolant and lubricant are terms used interchangeably, though not all coolants are lubricants. Compressed air, for example, has no lubricating purpose but works only as a cooling option. Direct coolants – those which make physical contact with a part – can be compressed air, water, oil, synthetics, or semi-synthetics. When directed to the cutting action of a tool, these can help to fend off high temperatures that could lead to melting, warping, discoloration, or tool failure. Additionally, coolant can help evacuate chips from a part, preventing chip recutting and aiding in part finish.

Coolant can be expensive, however, and wasteful if not necessary. Understanding the amount of coolant needed for your job can help your shop’s efficiency.

Click Here to Shop Harvey Tool’s Fully Stocked Offering of Deep Hole Coolant Through Drills

Types of Coolant Delivery

CNC coolant is delivered in several different forms – both in properties and pressure. The most common forms include air, mist, flood coolant, high pressure, and Minimum Quantity Lubricant (MQL). Choosing the wrong pressure can lead to part or tool damage, whereas choosing the wrong amount can lead to exhausted shop resources.

Air: Cools and clears chips, but has no lubricity purpose. Air coolant does not cool as efficiently as water or oil-based coolants. For more sensitive materials, air coolant is often preferred over types that come in direct contact with the part. This is true with many plastics, where thermal shock – or rapid expansion and contraction of a part – can occur if direct coolant is applied.

Mist: This type of low pressure coolant is sufficient for instances where chip evacuation and heat are not major concerns. Because the pressure applied is not great in a mist, the part and tool do not undergo additional stresses.

Flood: This low pressure method creates lubricity and flushes chips from a part to avoid chip recutting, a common and tool damaging occurrence.

High Pressure: Similar to flood coolant, but delivered in greater than 1,000 psi. This is a great option for chip removal and evacuation, as it blasts the chips away from the part. While this method will effectively cool a part immediately, the pressure can be high enough to break miniature diameter tooling. This method is used often in deep pocket or drilling operations, and can be delivered via coolant through tooling, or coolant grooves built into the tool itself. Harvey Tool offers Coolant Through Drills, while Titan USA proudly offers Coolant-Fed ThreadMills

Minimum Quantity Lubricant (MQL): Every machine shop focuses on how to gain a competitive advantage – to spend less, make more, and boost shop efficiency. That’s why many shops are opting for MQL, along with its obvious environmental benefits. Using only the necessary amount of coolant will dramatically reduce costs and wasted material. This type of lubricant is applied as an aerosol, or an extremely fine mist, to provide just enough coolant to perform a given operation effectively.

To see all of these coolant styles in action, check out the video below from our partners at CimQuest.

In Conclusion

CNC coolant is all-too-often overlooked as a major component of a machining operation. The type of coolant or lubricant, and the pressure at which it’s applied, is vital to both machining success and optimum shop efficiency. Coolant can be applied as compressed air, mist, in a flooding property, or as high pressure. Certain machines also are MQL able, meaning they can effectively restrict the amount of coolant being applied to the very amount necessary to avoid being wasteful.

3 Steps to Shutting up Tool Chatter

November 8, 2017/25 Comments/in CNC Machining, How-To's, Quick Tips, Troubleshooting Tips/by Harvey Performance Company

What is Chatter in Machining?

Cutting tools undergo a great deal of force during the machining process, which cause vibrations – also known as chatter or harmonics. Avoiding these vibrations entirely is not possible, though minimizing them is pivotal for machining success. Vibrations become damaging when proper machining steps are not followed. This leads to strong, part-ruining chatter. In these situations, parts have what is known as “chatter marks,” or clear vibration marks along the surface of a part. Tools can experience an increased rate of wear due to excess vibration.

zoomed in image of excessive tool wear from cnc machining — An example of a tool with excessive wear.

Shut Up Tool Chatter With Harvey Tool’s Material Specific Tooling

How to Reduce Chatter in Machining

Select the Right Tool for Your Job

It seems elementary, but selecting the best tool for your application can be confusing. With so many different geometric styles for tooling – overall length, length of cut, reach, number of flutes – it can sometimes be difficult to narrow down one specific tool for your job. Oftentimes, machinists opt for general purpose tooling that can perform a variety of operations, overlooking the option that’s optimized for one material and job.

Use Material Specific Tooling

Opting for Material Specific Tooling is helpful, as each material has different needs. For example, steels are machined differently than aluminum materials. Everything from the chip size, to chip evacuation, is different. Variable Helix or Variable Pitch designs help to minimize chatter by reducing harmonics, which are caused by the cutting edge having repeated contact with the workpiece. In order to reduce harmonics, the time intervals between flute contact with the workpiece are varied.

helical reduced neck tool in cnc machine next to part

Consider Tool Length

Overall length is another important factor to consider when deciding on a tool for your job. The more overhang, or length the tool hangs from the spindle, the less secure the spindle-to-tool connection is, and the more vibration. Ensuring that your tool is only as long as needed for your operation is important to minimizing chatter and harmonics. If machining deep within a part, opt for reached tooling or an extended reach tool holder to help solidify the connection.

Ensure a Secure Connection

Tool Holder & Shank Relationship

When it comes to secure tool holding approaches, both the tool shank and the collet are important. A loose tool, unsurprisingly, has more ability to move, or vibrate, during machining. With this in mind, Helical offers Shank Configurations to help the connection including the ToughGRIP Shank, which replaces a smooth, mirror-like surface with a rougher, coarser one for increased friction. Helical is also a licensee of the HAIMER Safe-Lock™, added grooves on the shank of a tool that work opposite of the spindle rotation, securely fastening the tool in place.

image of three end mills secured in their respective tool holders

Choosing Collet Types

Machinists must also know the different types of collets available to them to identify if a better solution might be necessary. For example, Hydraulic Tool Holders or Shrink Fit Tool Holders promote a stronger connection than a Mechanical Spindle Tightening method.

For more information, see Key Tool Holding Considerations

harvey tool material specific tooling ad with 4 end mills pictured side-by-side

Selecting a Chatter Minimizing Strategy

How a tool is run can mean the difference between stellar job results and a ruined part. This includes both the parameters a tool is run at, as well as the direction by which it rotates – either a Conventional Milling or a Climb Milling technique. The key distinction between these two methods lies in the relationship between the cutter’s rotation and the direction of the feed.

Conventional Milling

In conventional milling, the chip width starts from zero and increases gradually, causing the process of heat generation onto the workpiece rather than the chips. Heat generation causes deformities and tool failure such as work hardening, creating more headaches for a machinist. For this reason, conventional milling is generally only recommended for tools with high toughness or for breaking into case hardened materials.

Climb Milling

Most modern machine shops will use a climb milling technique, or when the chip width starts at its maximum and decreases during the cut. Climb Milling will offer a more consistent cut than traditional methods, and puts less stress on the tool. Think of it like weight lifting – doing the heavy lifting will be easiest at the beginning of your workout. Similarly, a cut in which the thickest chip is removed first helps the tool maintain its strength. Because the chip cutting process is more swift, vibrations are minimized.

For more information, see Climb Milling Vs. Conventional Milling

In Conclusion

Vibrations are unavoidable during the machining process, but minimizing them can mean the difference between successful machining and scrapped parts. Following three simple rules can help to keep your chatter and harmonics under control, including: Selecting the right tool, ensuring a secure machine-tool connection, and using it in a climb milling strategy. Both Harvey Tool and Helical Solutions have tools that can help, including shank modifications and Variable Helix or Variable Pitch end mills.