Posts

How Boring Bar Geometries Impact Cutting Operations

Boring is a turning operation that allows a machinist to make a pre-existing hole bigger through multiple iterations of internal boring. It has a number of advantages over traditional drilling methods:

  • The ability to cost-effectively produce a hole outside standard drill sizes
  • The creation of more precise holes, and therefore tighter tolerances
  • A greater finish quality
  • The opportunity to create multiple dimensions within the bore itself

 

Solid carbide boring bars, such as those offered by Micro 100,  have a few standard dimensions that give the tool basic functionality in removing material from an internal bore. These include:

Minimum Bore Diameter (D1): The minimum diameter of a hole for the cutting end of the tool to completely fit inside without making contact at opposing sides

Maximum Bore Depth (L2): Maximum depth that the tool can reach inside a hole without contact from the shank portion

Shank Diameter (D2): Diameter of the portion of the tool in contact with the tool holder

Overall Length (L1): Total length of the tool

Centerline Offset (F): The distance between a tool’s tip and the shank’s centerline axis

Tool Selection

In order to minimize tool deflection and therefore risk of tool failure, it is important to choose a tool with a max bore depth that is only slightly larger than the length it is intended to cut. It is also beneficial to maximize the boring bar and shank diameter as this will increase the rigidity of the tool. This must be balanced with leaving enough room for chips to evacuate. This balance ultimately comes down to the material being bored. A harder material with a lower feed rate and depths of cut may not need as much space for chips to evacuate, but may require a larger and more rigid tool. Conversely, a softer material with more aggressive running parameters will need more room for chip evacuation, but may not require as rigid of a tool.

Geometries

In addition, they have a number of different geometric features in order to adequately handle the three types of forces acting upon the tool during this machining process. During a standard boring operation, the greatest of these forces is tangential, followed by feed (sometimes called axial), and finally radial. Tangential force acts perpendicular to the rake surface and pushes the tool away from the centerline. Feed force does not cause deflection, but pushes back on the tool and acts parallel to the centerline. Radial force pushes the tool towards the center of the bore.

 

Defining the Geometric Features of Boring Bars:

Nose Radius: the roundness of a tool’s cutting point

Side Clearance (Radial Clearance): The angle measuring the tilt of the nose relative to the axis parallel to the centerline of the tool

End Clearance (Axial Clearance): The angle measuring the tilt of the end face relative to the axis running perpendicular to the centerline of the tool

Side Rake Angle: The angle measuring the sideways tilt of the side face of the tool

Back Rake Angle: The angle measuring the degree to which the back face is tilted in relation to the centerline of the workpiece

Side Relief Angle: The angle measuring how far the bottom face is tilted away from the workpiece

End Relief Angle: The angle measuring the tilt of the end face relative to the line running perpendicular to the center axis of the tool

Effects of Geometric Features on Cutting Operations:

Nose Radius: A large nose radius makes more contact with the workpiece, extending the life of the tool and the cutting edge as well as leaving a better finish. However, too large of a radius will lead to chatter as the tool is more exposed to tangential and radial cutting forces.

Another way this feature affects the cutting action is in determining how much of the cutting edge is struck by tangential force. The magnitude of this effect is largely dependent on the feed and depth of cut. Different combinations of depth of cuts and nose angles will result in either shorter or longer lengths of the cutting edge being exposed to the tangential force. The overall effect being the degree of edge wear. If only a small portion of the cutting edge is exposed to a large force it would be worn down faster than if a longer portion of the edge is succumb to the same force. This phenomenon also occurs with the increase and decrease of the end cutting edge angle.

End Cutting Edge Angle: The main purpose of the end cutting angle is for clearance when cutting in the positive Z direction (moving into the hole). This clearance allows the nose radius to be the main point of contact between the tool and the workpiece. Increasing the end cutting edge angle in the positive direction decreases the strength of the tip, but also decreases feed force. This is another situation where balance of tip strength and cutting force reduction must be found. It is also important to note that the angle may need to be changed depending on the type of boring one is performing.

Side Rake Angle: The nose angle is one geometric dimension that determines how much of the cutting edge is hit by tangential force but the side rake angle determines how much that force is redistributed into radial force. A positive rake angle means a lower tangential cutting force as allows for a greater amount of shearing action. However, this angle cannot be too great as it compromises cutting edge integrity by leaving less material for the nose angle and side relief angle.

Back Rake Angle: Sometimes called the top rake angle, the back rake angle for solid carbide boring bars is ground to help control the flow of chips cut on the end portion of the tool. This feature cannot have too sharp of a positive angle as it decreases the tools strength.

Side and End Relief Angles: Like the end cutting edge angle, the main purpose of the side and end relief angles are to provide clearance so that the tools non-cutting portion doesn’t rub against the workpiece. If the angles are too small then there is a risk of abrasion between the tool and the workpiece. This friction leads to increased tool wear, vibration and poor surface finish. The angle measurements will generally be between 0° and 20°.

Boring Bar Geometries Summarized

Boring bars have a few overall dimensions that allow for the boring of a hole without running the tool holder into the workpiece, or breaking the tool instantly upon contact. Solid carbide boring bars have a variety of angles that are combined differently to distribute the 3 types of cutting forces in order to take full advantage of the tool. Maximizing tool performance requires the combination of choosing the right tool along with the appropriate feed rate, depth of cut and RPM. These factors are dependent on the size of the hole, amount of material that needs to be removed, and mechanical properties of the workpiece.

 

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]

The Advances of Multiaxis Machining

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.

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.

A Growing Industry

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.

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

 

Ramping to Success

Poor tool life and premature tool failure are concerns in every machining application. Something as simple as tool path selection – and how a tool first enters a part – can make all the difference. Tool entry has a great deal of influence on its overall success, as it’s one of the most punishing operations for a cutter. Ramping into a part, via a circular or linear toolpath, is one of the most popular and oftentimes the most successful methods (Figure 1). Below, learn what ramping is, its benefits, and in which situations it can be used.

ramping

What is Ramping?

Ramping refers to simultaneous radial and axial motion of a cutting tool, making an angular tool path. Oftentimes, this method is used to approach a part when there is a need to create closed forms such as pockets, cavities, engravings, and holes. In doing so, the need to plunge with an end mill or drill to create a starting point is eliminated. Ramping is particularly important in micromachining where even the slightest imbalance in cutting forces can cause tool failure.

There are two types of ramping toolpaths: Linear and Circular (Figure 2 ).

ramping

Linear Ramping involves moving a cutting tool along two axes (the z-axis and one of the x, y axes). This method has significant more radial engagement with complementary increased cutting forces distributed across only two axes.

Circular Ramping (Helical Interpolation) has a spiral motion of the cutting tool that engages all three axes (x, y, and z axes). This method typically has less radial engagement on the cutting tool, with the cutting forces distributed across the three different axes. This is the recommended method, as it ensures the longest tool life.

Suggested Starting Ramp Angles:

Soft/Non-Ferrous Materials: 3° – 10°

Hard/Ferrous Materials 1° – 3°

Benefits of Ramping

When a tool enters the part via a Ramping method, it gradually increases in depth, preventing any shock loading on end mills. This reduces costs resulting from unnecessary tool breakage. Ramping produces smaller chips when compared to plunging, which makes chip evacuation faster and easier. As a result, cycle time can be decreased by running the end mill at faster parameters. Ramping also creates an extra space in the tool changer that would otherwise be occupied by a drill purposed with machining a starter hole.

Arcing

Similar to ramping in both method and benefit, arcing is another technique of approaching a workpiece (See Figure 3).

While ramping enters the part from the top, arcing enters from the side. The end mill follows a curved tool path (or arc) when milling, thus gradually increasing the load on the tool as the tool enters the part, as well as gradually decreasing the load as the tool exits the part. In this way, shock loading and possible tool breakage are avoided.

For more information on ramping, arcing, and other tool entry methods, please see Helical Solutions’ “Types of Tool Entry.”