What are drilling, reaming, honing and boring?

Compared to machining external cylindrical surfaces, hole machining conditions are significantly worse, making hole machining more difficult. This is because:

1) The size of the tool used for hole machining is limited by the size of the hole being machined, resulting in poor rigidity and a tendency to bend, deform, and vibrate.

2) When drilling with a fixed-size tool, the size of the hole often directly depends on the tool's corresponding dimensions, and tool manufacturing errors and wear directly affect hole machining accuracy.

3) When drilling, the cutting zone is inside the workpiece, resulting in poor chip removal and heat dissipation, making it difficult to control machining accuracy and surface quality.

A. Drilling and Reaming

1. Drilling

Drilling is the first step in drilling a hole in solid material. The diameter of the hole is generally less than 80mm. There are two drilling methods: one with a rotating drill bit and the other with a rotating workpiece. The errors generated by these two drilling methods are different. In the rotating drill method, due to asymmetric cutting edges and insufficient drill rigidity, the drill bit can cause the centerline of the drilled hole to deviate or become crooked, but the hole diameter remains essentially unchanged. In the rotating workpiece method, the opposite is true: the drill bit can cause the hole diameter to change, but the centerline remains straight.

Common drilling tools include twist drills, center drills, and deep-hole drills. The twist drill is the most commonly used, with diameters ranging from 0.1 to 80mm.

Due to structural limitations, drill bits have low bending and torsional stiffness, coupled with poor centering, resulting in low drilling accuracy, generally only reaching IT13 to IT11. Surface roughness is also high, with Ra typically ranging from 50 to 12.5μm. However, drilling offers a high metal removal rate and high cutting efficiency. Drilling is primarily used for holes with low quality requirements, such as bolt holes, threaded holes, and oil holes. Holes requiring higher precision and surface quality should be achieved through subsequent processing, such as reaming, reaming, boring, or grinding.

2. Hole Reaming

Hole reaming is the process of using a reaming drill to further increase the diameter and improve the quality of an already drilled, cast, or forged hole. This process can be used as a pre-processing step before finishing or as a final step for holes with lower requirements. A reaming drill is similar to a twist drill, but has more teeth and lacks a chisel edge.

Compared with drilling, reaming has the following characteristics: (1) reaming drills have more teeth (3 to 8 teeth), good guidance, and more stable cutting; (2) reaming drills have no chisel edge, and the cutting conditions are good; (3) the machining allowance is small, the chip groove can be made shallower, the drill core can be made thicker, and the tool body strength and rigidity are better. The precision of reaming is generally IT11 to IT10, and the surface roughness Ra is 12.5 to 6.3 μm. Reaming is often used to process holes with a diameter less than . When drilling holes with larger diameters (D ≥ 30 mm), a small drill bit (diameter 0.5 to 0.7 times the hole diameter) is often used to pre-drill the hole first, and then a reaming drill of the corresponding size is used to reame the hole. This can improve the processing quality and production efficiency of the hole. In addition to processing cylindrical holes, reaming can also use various special-shaped reaming drills (also known as countersinks) to process various countersunk holes and countersunk end faces. The front end of the countersink drill often has a guide column, which is guided by the machined hole.

B. Reaming

Reaming is a finishing method for holes and is widely used in production. For smaller holes, reaming is a more economical and practical method compared to internal grinding and fine boring.

1. Reamers

Reamers are generally divided into hand reamers and machine reamers. Hand reamers have straight shanks and longer working parts, providing better guiding. Hand reamers are available in both integral and adjustable OD configurations. Machine reamers are available in both shank-mounted and sleeve-mount configurations. Reamers can be used not only for round holes but also for tapered holes using tapered reamers.

2. Reaming Process and Applications

The reaming allowance significantly impacts the quality of the hole. Excessive allowance places a heavy load on the reamer, quickly dulling the cutting edge and making it difficult to achieve a smooth surface and maintain dimensional tolerances. Too little allowance prevents the removal of tool marks left by the previous process, thus failing to improve the hole quality. Generally, the rough reaming allowance is 0.35-0.15mm, and the fine reaming allowance is 0.15-0.05mm.

To avoid built-up edge, reaming is typically performed at a lower cutting speed (v < 8m/min when using a high-speed steel reamer on steel and cast iron). The feed rate is related to the diameter of the hole being machined. The larger the hole diameter, the higher the feed rate. When using a high-speed steel reamer on steel and cast iron, the feed rate is typically 0.3-1mm/r.

When reaming, appropriate cutting fluid must be used for cooling, lubrication, and cleaning to prevent built-up edge and ensure prompt chip removal. Compared to grinding and boring, reaming offers higher productivity and easier hole accuracy. However, reaming cannot correct for positional errors in the hole axis; hole positional accuracy should be ensured by the preceding process. Reaming is not suitable for step holes or blind holes.

The dimensional accuracy of reamed holes is generally IT9-IT7, with a surface roughness Ra of 3.2-0.8 μm. For medium-sized holes with high precision requirements (such as IT7-level precision holes), the drilling-reaming-reaming process is a typical processing solution commonly used in production.

C. Boring

Boring is a processing method that uses a cutting tool to enlarge a prefabricated hole. Boring can be performed on a boring machine or a lathe.

1. Boring method

There are three different boring processing methods.

(1) The workpiece rotates and the tool feeds. Most boring on a lathe belongs to this boring method. The process characteristics are: the axis of the hole after processing is consistent with the rotation axis of the workpiece, the roundness of the hole mainly depends on the rotation accuracy of the machine tool spindle, and the axial geometric shape error of the hole mainly depends on the position accuracy of the tool feed direction relative to the workpiece rotation axis. This boring method is suitable for processing holes that have coaxiality requirements with the outer cylindrical surface.

(2) The tool rotates and the workpiece feeds. The boring machine spindle drives the boring tool to rotate, and the worktable drives the workpiece to feed.

(3) The tool rotates and feeds. When boring with this boring method, the overhang length of the boring bar varies, and the stress and deformation of the boring bar also vary. The hole diameter near the spindle box is large, and the hole diameter away from the spindle box is small, forming a tapered hole. In addition, as the overhang length of the boring bar increases, the bending deformation of the spindle due to its own weight also increases, and the axis of the processed hole will bend accordingly. This boring method is only suitable for processing shorter holes.

2. Diamond boring

Compared with general boring, diamond boring is characterized by small back cutting amount, small feed rate, and high cutting speed. It can obtain very high processing accuracy (IT7~IT6) and very smooth surface (Ra is 0.4~0.05 μm). Diamond boring was originally performed with diamond boring tools, but carbide, CBN, and synthetic diamond tools are now commonly used. It is primarily used for machining non-ferrous metal workpieces, but can also be used for machining cast iron and steel.

Common cutting parameters for diamond boring are: pre-boring depth of 0.2-0.6mm, final boring depth of 0.1mm; feed rate of 0.01-0.14mm/r; cutting speed of 100-250m/min for cast iron, 150-300m/min for steel, and 300-2000m/min for non-ferrous metals.

To ensure high machining accuracy and surface quality when using diamond boring, the machine tool (diamond boring machine) must possess high geometric accuracy and rigidity. Precision angular contact ball bearings or hydrostatic plain bearings are often used for spindle support, and high-speed rotating parts must be precisely balanced. Furthermore, the feed mechanism must operate very smoothly to ensure smooth, low-speed feed motion of the worktable.

Diamond boring offers excellent machining quality and high production efficiency, making it widely used in large-scale mass production for the final machining of precision holes, such as engine cylinder bores, piston pin holes, and spindle holes in machine tool spindle boxes. However, it is important to note that when using diamond boring for ferrous metals, only boring tools made of carbide and CBN should be used; boring tools made of diamond should not be used. This is because the carbon atoms in diamond have a strong affinity for iron group elements, resulting in a shorter tool life.

3. Boring Tools

Boring tools can be divided into single-edge and double-edge boring tools.

4. Boring Process Characteristics and Applications

Compared to the drilling-reaming-reaming process, boring is not limited by tool size in terms of hole diameter. Boring also offers strong error correction capabilities, allowing correction of deviations in the original hole axis through multiple passes. It also maintains a high degree of positional accuracy between the bored hole and the positioning surface.

Compared to external turning, boring suffers from lower toolholder rigidity, greater deformation, poor heat dissipation, and significant thermal deformation of the workpiece and tool. Consequently, boring's machining quality and production efficiency are inferior to those of external turning.

From the above analysis, it can be seen that boring has a wide range of machining applications, capable of producing holes of various sizes and accuracy levels. For larger holes and hole systems requiring high dimensional and positional accuracy, boring is virtually the only machining method. Boring achieves machining accuracy levels of IT9 to IT7. Boring can be performed on various machine tools, including boring machines, lathes, and milling machines. Its flexibility and maneuverability make it widely used in production. In large-scale mass production, boring dies are often used to improve boring efficiency.

D. Honing Holes

1. Honing Principles and Honing Heads

Honing is a method of finishing holes using a honing head with a grinding wheel (oilstone). During honing, the workpiece is stationary while the honing head is rotated and driven by the machine tool spindle in a reciprocating linear motion. During honing, the grinding wheel applies pressure to the workpiece surface, removing a very thin layer of material from the surface. The cutting path forms a cross-shaped pattern. To ensure that the paths of the abrasive grains in the grinding wheel are not repeated, the rotational speed of the honing head and the number of reciprocating strokes per minute of the honing head must be prime numbers.

The intersection angle of the honing paths is related to the reciprocating speed and peripheral speed of the honing head. The size of this angle affects the honing process quality and efficiency. It is generally set at 0° for rough honing and 0° for fine honing. To facilitate the removal of broken abrasive particles and chips, reduce cutting temperatures, and improve machining quality, sufficient cutting fluid should be used during honing.

To ensure uniform machining of the hole wall, the abrasive strip must extend beyond the hole by a certain amount at both ends. To ensure uniform honing allowance and minimize the impact of spindle rotation errors on machining accuracy, a floating connection is typically used between the honing head and the machine spindle.

Radial adjustment of the honing head strips can be manual, pneumatic, or hydraulic.

2. Honing Process Characteristics and Applications

1) Honing can achieve high dimensional and shape accuracy, with machining accuracy reaching IT7-IT6 levels. Hole roundness and cylindricity errors can be controlled within a range of . However, honing does not improve the positional accuracy of the machined hole.

2) Honing can achieve high surface quality, with a surface roughness Ra of 0.2-0.25μm and a minimal depth of 2.5-25μm for the surface metal's deterioration defect layer.

3) Although the circumferential speed of the honing head is not as high as that of grinding (vc = 16-60m/min), honing still offers high productivity due to the large contact area between the abrasive strip and the workpiece and the relatively high reciprocating speed (va = 8-20m/min).

Honing is widely used in mass production to produce precision holes in engine cylinder bores and various hydraulic systems. Hole diameters generally range from 0.5 to 1.5μm and can produce deep holes with aspect ratios greater than 10. However, honing is not suitable for machining holes in non-ferrous metal workpieces with high plasticity, nor can it process holes with keyways or splines.

E. Hole Broaching

1. Broaching and Broaching Tools

Hole broaching is a highly productive finishing method performed on a broaching machine using a specially designed broach. Broaching machines are classified as either horizontal or vertical, with horizontal broaching tools being the most common.

During broaching, the broach only performs low-speed linear motion (main motion). The number of broach teeth operating simultaneously should generally be no less than three; otherwise, the broach will operate unsteadily and ring-shaped ripples may form on the workpiece surface. To avoid excessive broaching forces that could break the broach, the number of teeth operating simultaneously should generally not exceed six to eight.

There are three different methods of hole broaching, described below:

1) Layered Broaching: This method is characterized by the broach removing the workpiece stock layer by layer. To facilitate chip breaking, the teeth are ground with interlaced chip-breaking grooves. Broaches designed for layered broaching are called conventional broaches.

2) Segmented Broaching: This broaching method is characterized by the removal of each layer of metal from the machined surface using a set of teeth (usually consisting of 2-3 teeth per set) of essentially identical dimensions but staggered. Each tooth removes only a portion of a layer of metal. A broach designed for segmented broaching is called a wheel-cut broach.

3) Combined Broaching: This method combines the advantages of both layered and segmented broaching, with segmented broaching used for roughing and layered broaching for finishing. This shortens broaching length, improves productivity, and achieves superior surface quality. A broach designed for combined broaching is called a combined broach.

2. Hole Broaching Process Characteristics and Applications

1) A broach is a multi-edged tool that can sequentially complete roughing, finishing, and finishing of a hole in a single broaching stroke, resulting in high production efficiency.

2) Hole broaching accuracy depends primarily on the accuracy of the broaching tool. Under normal conditions, broaching accuracy can reach IT9-IT7, with surface roughness Ra of 6.3-1.6 μm.

3) During hole broaching, the workpiece is positioned relative to the hole being machined (the broaching tool guide acts as the workpiece positioning element). This makes it difficult to ensure the relative positional accuracy of the hole and other surfaces. For machining rotating parts with coaxiality requirements for internal and external circular surfaces, the hole is often broached first, and then other surfaces are machined using the hole as a positioning reference.

4) Broaches can not only machine round holes, but also form holes and spline holes.

5) Broaches are fixed-size tools with complex shapes and high cost, making them unsuitable for machining large holes.

Broaching is commonly used in mass production to machine through holes on small and medium-sized parts with diameters ranging from 10 to 80 mm and depths no more than five times the hole diameter.