Posts

An Introduction to Reamers & CNC Reaming

Most machinists are familiar with CNC drilling, but did you know that the common practice for holemaking is to always use a reamer? When done correctly, reaming can be a fast and highly accurate operation that results in precision holes.

Critical Reamer Geometries

reamers

By examining a Harvey Tool Miniature Reamer and its critical dimensions, we can better understand the functionality of this useful tool. In the above image of a straight flute reamer, D1 references the reamer diameter, the specific size intended for your hole; and D2 points to the shank diameter. At Harvey Tool, reamer shanks are oversized to help maintain tool strength, stiffness, and accuracy. Shanks also have an h6 tolerance, which is crucial for high precision tool holders, such as heat shrink collets. Other critical dimensions of a reamer include its overall length (L1), margin length (L2), overall reach (L3), and chamfer length (L4).

Harvey Tool also offers Miniature Reamers – Right Hand Spiral. This tool is designed to leave a superior part finish and help with chip evacuation in blind hole applications.

The Functions of Miniature Reamers

Reamers Provide Precision – As mentioned earlier, reamers are great for machining precision hole diameters. To use a reamer properly, you must first have a pre-drilled hole that’s between 90% and 94% of the final hole diameter. For example, if you need a finished a hole of .220″, your predrilled hole should be somewhere between .1980″ and .2068″. This allows the tool to take enough material off to leave a great finish, but does not overwork it, potentially causing damage. The tolerance for uncoated reamers is +.0000″/-.0002″, while the tolerance for AlTiN coating is +.0002″/-.0000″. These tolerances provide you the peace of mind of knowing that your hole will meet exact specifications.

Achieve a Quality CNC Finish – When a high surface finish is required of a hole, reamers should always be used to reach the desired tolerance. Both the pre-drilled hole and the tool’s margin help to keep the reamer centered while cutting, leading to a better finish.

Minimize Machining Production Runs – For machine shops, consistency is a priority. This is especially true in production runs. The last thing a machinist wants to see is an oversized hole on a part they have already preformed many operations on. Remember, reamers have the benefit of offering consistent hole size, preventing an out of tolerance finish. These consistent holes lead to valuable time savings and reduced scrap costs.

CNC Machining Exotic Alloys: When machining Inconel, titanium, and other high-cost materials, reaming your hole is important to ensure that the desired finish specification is met. With reamers, a machinists can better predict tool life, leading to a better finished product and less scrap ratios. It is important to note that Harvey Tool reamers are offered AlTiN coated and fully stocked in every .0005” increment from .0080” to .0640”.

Workholding Styles & Considerations

Machinists have a number of variables to consider when setting up workholding devices for a machining operation. When it comes to workholding, there are some major differences between holding a loosely toleranced duplicate part with a 10-minute cycle time and holding a tightly toleranced specialized part with a 10-hour cycle time. Determining which method works best for your machining job is essential to maintaining an efficient operation.

Workholding Devices

Ideal workholding devices have easily repeatable setups. For this reason, some machines have standard workholding devices. Vises are generally used with milling machines while chucks or collets are used when running a lathe machine. Sometimes, a part may need a customized workholding setup in order to secure the piece properly during machining. Fixtures and jigs are examples of customized workholding devices.

Fixtures and Jigs

A jig is a work holding device that holds, supports and locates a workpiece and guides the cutting tool into a specific operation (usually through the use of one or more bushings). A fixture is essentially the same type of device, but the main difference is that it does not guide the cutting tool into a specified operation. Fixtures are typically used in milling operations while jigs are generally used in drilling, reaming, tapping and boring. Jigs and fixtures are more precise relative to standard workholding devices, which leads to tighter tolerances. They can also be indexable, allowing them to control the cutting tool movement as well as workpiece movement. Both jigs and fixtures are made up of the same basic components: fixture bodies, locators, supports, and clamps.

The 4 Fixture Bodies

There are 4 basic types of fixture bodies: faceplates, baseplates, angle plates, and tombstones.

Faceplates: Typically used in lathe operations, where components are secured to the faceplate and then mounted onto the spindle.

Baseplates: Common in milling and drilling operations and are mounted to the worktable.

Angle plates: Two plates perpendicular to each other but some are adjustable or customized to change the angle of the workpiece.

Tombstones: Large vertically oriented rectangular fixtures that orients a workpiece perpendicular to the worktable. Tombstones also have two sides to accommodate multiple parts.

workholding

Locators

Locators are characterized by four criteria: assembled, integral, fixed, and adjustable. Assembled locators, can be attached and removed from the fixture, which is contrary to integral locators that are built into the fixture. Fixed locators allow for no moving components, while adjustable locators permit movement through the use of threads and/or springs, and can adjust to a workpiece’s size. These can be combined to provide the appropriate rigidity-assembly convenience ratio. For example, a V-locator fixture is the combination of assembled and fixed locators. It can be secured to a fixture but has no moving components.

workholding

Supports

Supports do exactly what their name suggests, they support the workpiece during the machining process to avoid workpiece deformation. These components can double as locators and also come fixed, adjustable and integral, or assembled. Generally, supports are placed under the workpiece during manufacturing but this also depends on the geometry of the workpiece, the machine being operated and where the cutting tool will make contact. Supports can come in different shapes and sizes. For example, rest buttons are smaller support components used in series either from underneath the workpiece or from the sides. Concurrently, parallel supports are placed on either side of the part to provide general support.

workholding

Clamps

Clamps are devices used for strengthening or holding things together, and come in different shapes, sizes and strengths. Vises and chucks have movable jaws and are considered standard clamps. One atypical example is the toggle clamp, which has a pivot pin that acts as a fulcrum for a lever system. One of the more convenient types is a power clamping system. There are two type of power clamping methods: hydraulic and pneumatic.

workholding

Example of a standard fixture setup.

Hydraulic Systems

Hydraulic Systems create a gripping force by attaining power from compressing a liquid. This type of power clamp is generally used with larger workpieces as it usually takes up less space relative to pneumatic clamps.

Pneumatic clamps

Pneumatic clamps attain their gripping force from the power created by a compressed gas (usually air). These systems are generally bulkier and are used for smaller workpieces that require less room on the worktable. Power clamping offers a few advantages over conventional clamping. First, these systems can be activated and deactivated quickly to save on changeover time. Second, they place uniform pressure on the part, which help prevent errors and deformation. A significant disadvantage they pose is the cost of a system but this can be quickly offset by production time saved.

Key Guidelines to Follow

Lastly, there are a few guidelines to follow when choosing the appropriate fixture or jig setup.

Ensure Proper Tolerancing

The tolerances of the workholding device being used should be 20%-50% tighter than those of the workpiece.

Utilize Acceptable Locating & Supporting Pieces

Locating and supporting pieces should be made of a hardened material to prevent wear and allow for several uses without the workpieces they support falling out of tolerance. Supports and locators should also be standardized so that they can be easily replaced.

Place Clamps in Correct Locations

Clamps should be placed above the locations of supports to allow the force of the clamp to pass into the support without deforming the workpiece. Clamps, locators and supports should also be placed to distribute cutting forces as evenly as possible throughout the part. The setup should allow for easy clamping and not require much change over time

Maximize Machining Flexibility

The design of the fixture or jigs should maximize the amount of operations that can be performed in one orientation. During the machining operation, the setup should be rigid and stable.

Bottom Line

Workholding can be accomplished in a number of different ways and accomplish the same task of successfully gripping a part during a machining operation with the end result being in tolerance. The quality of this workholding may differ greatly as some setups will be more efficient than others. For example, there is no reason to create an elaborate jig for creating a small slot down the center of a rectangular brick of aluminum; a vise grip would work just fine. Maximizing the efficiency and effectiveness of an operators’ workholding setup will boost productivity by saving on changeover, time as well as cost of scrapped, out of tolerance parts.

Drill / End Mills: Drill Style vs. Mill Style

Drill / End Mills are one of the most versatile tools in a machinist’s arsenal. These tools can perform a number of different operations, freeing space on your carousel and improving cycle times by limiting the need for tool changes. These operations include:

  1. Drilling
  2. V-Grooving
  3. Milling
  4. Spot Drilling
  5. Chamfering

The ability of the Drill / End Mill to cut along the angled tip as well as the outer diameter gives it the range of operations seen above and makes it an excellent multi-functional tool.

drill mill operations

Drill Style vs. Mill Style

The main difference between Drill / End Mill styles is the point geometry.  They are defined by how the flutes are designed on the end of the tool, using geometry typically seen on either an end mill or a drill.  While mill style tools follow the features of an end mill or chamfer mill, the drill style geometry uses an S-gash at the tip.  This lends strength to the tip of the tool, while giving it the ability to efficiently and accurately penetrate material axially.  While both styles are capable of OD milling, mill style tools will be better for chamfering operations, while drill style will excel in drilling.  The additional option of the Harvey Tool spiral tipped Drill / End Mill is an unprecedented design in the industry.  This tool combines end geometry taken from our helical flute chamfer cutters with a variable helix on the OD for enhanced performance. Versatility without sacrificing finish and optimal performance is the result.

drill mills

Left to Right: 2 Flute Drill Style End, 2 Flute Mill Style End, 4 Flute Mill Style End

Drill Mills: Tool Offering

Harvey Tool currently offers Drill / End Mills in a variety of styles that can perform in different combinations of machining applications:

Mill Style – 2 Flute

This tool is designed for chamfering, milling, drilling non-ferrous materials, and light duty spotting. Drilling and spotting operations are recommended only for tools with an included angle greater than 60°. This is a general rule for all drill mills with a 60° point. Harvey Tool stocks five different angles of 2 flute mill-style Drill / End Mills, which include 60°, 82°, 90°, 100° and 120°. They are offered with an AlTiN coating on all sizes as well as a TiB2 coating for cutting aluminum with a 60° and 90° angle.

drill mill

Mill Style – 4 Flute

4 flute mill-style Drill / End Mills have two flutes that come to center and two flutes that are cut back. This Drill / End Mill is designed for the same operations as the 2 flute style, but has a larger core in addition the higher flute count. The larger core gives the tool more strength and allows it to machine a harder range of materials. The additional flutes create more points of contact when machining, leading to better surface finish. AlTiN coating is offered on all 5 available angles (60°, 82°, 90°, 100°, and 120°) of this tool for great performance in a wide array of ferrous materials.

drill mill

Drill Style – 2 Flute

This tool is specifically designed for the combination of milling, drilling, spotting and light duty chamfering applications in ferrous and non-ferrous materials. This line is offered with a 90°, 120°, and 140° included angle as well as AlTiN coating.

drill mills drill style

Helical Tip – 4 Flute

The Helically Tipped Drill / End Mill offers superior performance in chamfering, milling and light duty spotting operations. The spiral tip design allows for exceptional chip evacuation and surface finish. This combined with an OD variable helix design to reduce chatter and harmonics makes this a valuable tool in any machine shop. It is offered in 60°, 90°, and 120° included angles and comes standard with the latest generation AlTiN Nano coating that offers superior hardness and heat resistance.

 

Selecting the Right Harvey Tool Miniature Drill

Among Harvey Tool’s expansive holemaking solutions product offering are several different types of miniature tooling 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.

spotting drill

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.

spotting drill correct angle

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 drill

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 drill coolant through

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.

flat bottom drill

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.

drill for aluminum

 

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.

drill for hardened steel

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.

drill for prehardened steel

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. miniature reamer

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.

flat bottom counterbores

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

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

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. Pecking 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

miniature drill pecking cycles

High Performance Drills – Flat Bottom

pecking cycles

High Performance Drills – Aluminum & Aluminum Alloys

aluminum pecking cycles

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

High Performance Drills – Hardened Steels

hardened steels pecking cycles
High Performance Drills – Prehardened Steels

prehardened steels pecking cycles

Key Pecking Cycle Takeaways

From the above tables, it’s easy to identify how recommended pecking 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]

Multi-Functional Tools Every Shop Should Have

If there is one thing that all machinists and shop managers can agree on, it’s that time is money. Tool and material costs, employee wages, and keeping the lights on all add up, but most would agree that saving time is one of the best ways to make a shop more efficient.

Tool changes mid-job quickly add up when it comes to cycle times (not to mention tool costs), so using a tool capable of multiple operations whenever possible is an excellent first step. The following multi-functional tools are designed to save time and money at the spindle.

Drill/End Mills

drill mills

One look at Drill/End Mills or “Drill Mills” and it’s obvious that these tools are capable of more than a standard end mill. Two of the intended operations are right in the name (drilling and milling). Besides the obvious, though, drill mills are intended for grooving, spotting, and chamfering, bringing the total to five separate operations.

drill mill operations

Considering the amount of tools normally required to perform all of these common operations, keeping a few drill mills in your tool crib ensures you’re always ready to tackle them, not to mention the potential extra spots in your tool magazine.

Undercutting End Mills

undercutting end mills

Undercutting End Mills, also known as lollipop cutters or spherical ball end mills are surprisingly “well-rounded” tools. Besides milling an undercut feature on a part, which is typically very difficult with a standard end mill, these tools are capable of a few other operations.

undercutting end mill operations

Using an undercutting end mill to deburr in your machine is an excellent way to save time and effort. Some slotting and contouring operations, especially when 5-axis milling, are made far easier with an undercutting end mill, and in some situations, clearance challenges make them necessary.

Double Angle Shank Cutters

double angle shank cutters

Often referred to the “Swiss Army Knife of Machining” due to their versatility, Double Angle Shank Cutters are 6-in1 tools worth keeping on hand in any machine shop. Since these tools cut on all sides of their head, they are useful in a variety of situations.

multi-functional tools

With the ability to thread mill and countersink, Double Angle Shank cutters are perfect for holemaking operations. On top of that, their clearance advantage over standard end mills makes them extremely well suited to a variety of finishing operations in difficult to reach places.

Flat Bottom Tools

flat bottom tools

Flat Bottom Drills and Flat Bottom Counterbores are better suited to holemaking, but they are capable of a large variety of operations. They belong in a category together since their flat bottom geometry is what sets them apart from other tools in the same category. Flat bottom geometry keeps the tool from walking on irregular or angle surfaces and help to correct, straighten, or flatten features created by non-flat bottom tools.

Flat bottom drills are designed for the following operations:

multi-functional tools

While similar in some aspects, flat bottom counterbores are particularly well-suited for these uses:

flat bottom tools

Adjustable Chamfer Cutters

adjustable chamfer cutters

As discussed in a previous post, chamfer mills are capable of more than just chamfering – they are also well-suited for beveling, deburring, spotting, and countersinking. However, these adjustable chamfer cutters aren’t limited to a single angle per side – with a quick adjustment to the carbide insert you can mill any angle from 10° to 80°.

chamfer cutter inserts

When you account for the replaceable insert and the range of angles, this tool has a very high potential for time and tool cost savings.

Tools that are capable of a variety of operations are useful to just about any machine shop. Keeping your tool crib stocked with some or all of these multi-functional tools greatly increases your shop’s flexibility and decreases the chances of being unprepared for a job.

What You Need to Know About Coolant for CNC Machining

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 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.

Types of Coolant Delivery

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 and Coolant Through 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

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.

Most Common Methods of Tool Entry

Tool entry is pivotal to machining success, as it’s one of the most punishing operations for a cutter. Entering a part in a way that’s not ideal for the tool or operation could lead to a damaged part or exhausted shop resources. Below, we’ll explore the most common part entry methods, as well as tips for how to perform them successfully.


Pre-Drilled Hole

Pre-drilling a hole to full pocket depth (and 5-10% larger than the end mill diameter) is the safest practice of dropping your end mill into a pocket. This method ensures the least amount of end work abuse and premature tool wear.

tool entry predrill

 


Helical Interpolation

Helical Interpolation is a very common and safe practice of tool entry with ferrous materials. Employing corner radius end mills during this operation will decrease tool wear and lessen corner breakdown. With this method, use a programmed helix diameter of greater than 110-120% of the cutter diameter.

helical interpolation

 


Ramping-In

This type of operation can be very successful, but institutes many different torsional forces the cutter must withstand. A strong core is key for this method, as is room for proper chip evacuation. Using tools with a corner radius, which strengthen its cutting portion, will help.

ramping

Suggested Starting Ramp Angles:

Hard/Ferrous Materials: 1°-3°

Soft/Non-Ferrous Materials: 3°-10°

For more information on this popular tool entry method, see Ramping to Success.


Arcing

This method of tool entry is similar to ramping in both method and benefit. However, while ramping enters the part from the top, arcing does so from the side. The end mill follows a curved tool path, or arc, when milling, this gradually increasing the load on the tool as it enters the part. Additionally, the load put on the tool decreases as it exits the part, helping to avoid shock loading and tool breakage.


Straight Plunge

This is a common, yet often problematic method of entering a part. A straight plunge into a part can easily lead to tool breakage. If opting for this machining method, however, certain criteria must be met for best chances of machining success. The tool must be center cutting, as end milling incorporates a flat entry point making chip evacuation extremely difficult. Drill bits are intended for straight plunging, however, and should be used for this type of operation.

tool entry

 


Straight Tool Entry

Straight entry into the part takes a toll on the cutter, as does a straight plunge. Until the cutter is fully engaged, the feed rate upon entry is recommended to be reduced by at least 50% during this operation.

tool entry

 


Roll-In Tool Entry

Rolling into the cut ensures a cutter to work its way to full engagement and naturally acquire proper chip thickness. The feed rate in this scenario should be reduced by 50%.

tool entry

 

Overcoming Composite Holemaking Challenges

Harvey Tool’s Miniature High Performance Composite Drills are specifically designed with point geometry optimized for the unique properties of composite materials. Our Double Angle style is engineered to overcome common problems in layered composites and our Brad Point style is built to avoid the issues frequently experienced in fibrous composites.

Circular Interpolation: Machining Circular Tool Paths

When machining, proper speeds and feeds are very important to avoid breakage and maximize performance. Traditional end milling formulas use Surface Footage (SFM) and Chip Load (IPT) to calculate Speed (RPM) and Feed (IPM) rates. These formulas dictate the correct machining parameters for use in a linear path in which the end mill’s centerline is travelling in a straight line. Since not all parts are made of flat surfaces, end mills will invariably need to move in a non-linear path. In the case of machining circular tool paths, the path of the end mill’s centerline is circular. Not surprisingly, this is referred to as Circular Interpolation.

Cutting Circular Tool Paths

All rotating end mills have their own angular velocity at the outside diameter. But when the tool path is circular, there is an additional component that is introduced, resulting in a compound angular velocity. Basically, this means the velocity of the outside diameter is travelling at a substantially different velocity than originally expected. The cause of the compound angular velocity is seen in the disparity between the tool path lengths.

Internal Circular Tool Paths

Figure A shows the cross section of a cutting tool on a linear path, with the teeth having angular velocity due to tool rotation, and the center of the tool having a linear feed. Note that the tool path length will always be equal to the length of the machined edge. Figure B shows the same cutting tool on an internal circular path, as done when machining a hole. In this case, the angular velocity of the teeth is changed as a result of an additional component from the circular path of the tool’s center. The diameter of the tool path is smaller than that of the major diameter being cut. Or, in other words, the tool path length is shorter than the machined edge length, increasing the angular velocity of the teeth. To prevent overfeeding and the possibility of tool breakage, the increased angular velocity of the teeth must be made the same as in the linear case in Figure A. The formula below can be used to properly lower the feed rate for internal machining:

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

 

External Circular Tool Paths

Figure C shows the same cutting tool on an external circular path, as done when machining a post. In this case, the diameter of the tool path is larger than the major diameter being cut. This means that the tool path length is longer than the machined edge length, resulting in a decreased angular velocity. To prevent premature dulling and poor tool life due to over-speeding, use the formula below to properly raise the feed rate for external machining. In this way, the decreased angular velocity of the teeth is made the same as in the linear case in Figure A.

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

Optimize Your Performance

By adjusting the feed in the manner provided, internal applications can avoid tool breakage and costly down time. Further, external applications can enjoy optimized performance and shorter cycle times. It should also be noted that this approach can be applied to parts with radiused corners, elliptical features and when helical interpolation is required.