Reaming is a sizing and finishing operation performed on a pre-existing hole using a rotating cutting tool called a reamer that is fed into the hole to slightly enlarge and improve its geometric accuracy and surface finish. The goal is to produce holes with extreme precision in size, roundness, straightness and surface finish.

Unlike drilling, which creates the initial hole, reaming removes only a small amount of material (typically 2-5% of the hole diameter) to bring the hole to exact specifications. This process is essential when applications demand tight tolerances, such as dowel pin holes, bearing seats or precision shaft fittings.

The 3 Main Hole Making Operations

Three primary methods for creating precision holes in machining: drilling, boring and reaming. Each serves a distinct purpose in the hole-making process.

Drilling creates the initial hole by removing material with a rotating drill bit. It’s the fastest method but produces relatively rough surfaces with limited accuracy. Drills typically have two or three cutting edges and are designed for material removal rather than precision sizing. However, modern carbide drills produce decent quality holes, which are good enough in most cases. When a hole demands higher quality, boring and reaming come into play.

Boring uses single-point cutters to enlarge existing holes and improve geometric accuracy. This method offers superior control over hole geometry and can correct location errors from previous operations. Boring excels when position accuracy is critical. Boring tools can also be adjusted; thus a single tool can serve a wide range of diameters.

Reaming provides the highest precision for hole diameter, roundness and surface finish by removing minimal material from a drilled hole. However, reamers follow the existing hole path and cannot fix positional errors. They will “copy the mistake” if the pre-drilled hole is misaligned.

Drilling is primarily a hole-making operation, not a sizing operation. Boring offers the best control over geometry and true position, with the ability to correct location errors. Reaming delivers the tightest size and surface finish but cannot correct location errors.

Basic Reamer Structure and Cutting Action

Understanding how a reamer cuts is fundamental to using it effectively. Unlike endmills that cut with multiple edges along their length, reamers primarily rely on small chamfers at the tool’s tip to perform cutting. These chamfered cutting edges do all the work.

The face of a reamer cannot cut, and the outer edges (flutes) are not cutting either. Their critical task is to guide the tool through the hole, using the already reamed section as a drill bushing to aid alignment. As the reamer advances, the chamfered edges remove material while the body follows the path established by the previously cut portion.

This design makes the pre-drilled hole critical. Since reamers follow the existing hole, starting with a quality drill and proper hole size is essential. The 3% rule of thumb recommends leaving 2-5% diameter stock allowance after drilling for the reamer to remove. Too much allowance overworks the cutting chamfers, degrading surface finish. Too little causes the tool to rub instead of cutting cleanly, generating heat and accelerating wear.

Types of Reamers and Their Applications

Reamers fall into two main categories: hand reamers and chucking reamers.

Hand reamers are designed to be held by hand or with a wrench. They feature extended cutting edges along their flutes and often have a square interface on the shank end. These tools are suitable for fabrication work, but will chatter and fail if used in CNC machines.

Chucking reamers are designed to be held precisely in machine tool chucks and fed axially into the workpiece. This article focuses on chucking reamers.

Main Chucking Reamer Types

• Straight-flute reamers are the most common type. They are typically made from carbide and work on both blind and through holes. This is the first choice for most applications.
• Straight-flute reamers are the most common type. They are typically made from carbide and work on both blind and through holes. This is the first choice for most applications. –Left-hand spiral reamers (still right-hand cutting) force chips forward, making them suitable only for through holes. – Right-hand spiral reamers pull chips out, working better for blind holes.
• Carbide-tipped or high speed steel reamers offer cost advantages for larger diameter holes where solid carbide becomes expensive.

Best Practices for Reaming Operations

Cutting fluids are essential. They lubricate cutting edges, cool the tool and workpiece, flush away chips, prevent built-up edge, and reduce friction and wear. Use flood coolant when possible, applying from both sides for through holes. For blind holes, oil-based fluids work best because they remain in the hole better.

Secure workpiece clamping prevents problems. Even minor looseness causes chatter, poor finish or an inaccurate hole size.

Spindle speeds and feed rates require balance. Slower speeds between 100–500 rpm work best for most reaming, depending on material and hole size. This prevents chatter while allowing effective cutting. Feed rates should match spindle speeds based on material hardness, typically ranging from 0.002– 0.012 ipr. Harder materials require slower, more controlled feeds.

Apply smooth, continuous pressure. Excessive pressure breaks the reamer or causes chatter; insufficient pressure leads to poor cutting.

Clear chips periodically in deep holes. Back the tool out regularly to clear chips and apply fresh cutting fluid. Allowing chips to pack into flutes increases friction and can cause tool breakage, especially with straight flutes.

CNC Programming Tips

• For optimal results, use a G85 canned cycle that feeds in and feeds out. This produces better surface finishes. While a G81 cycle (feed in, rapid out) saves cycle time, it often leaves marks inside holes, which compromises surface finish.
• Never run a reamer backwards. Always maintain a clockwise rotation with an M3 command.
• Check reamer runout with an indicator or tool presetter. Runout causes oversized holes and poor finishes. The reamer must be held precisely centered in the chuck.

Summary

Reaming transforms pre-drilled holes into precision features with tight tolerances and superior surface finishes. The key to success lies in understanding that reamers work differently from drills. They follow existing holes and remove minimal material through small chamfered cutting edges.

Start with a quality drill and leave 2-5% stock allowance. Use proper cutting fluids, secure clamping, and appropriate speeds and feeds. Choose straight-flute carbide reamers for general work, and spiral-flute designs for interrupted cuts or specific chip evacuation needs.

When applications demand holes with tolerances down to ±0.0002" and surface finishes of 15–30 μin, reaming is the go-to solution. It’s an indispensable process that takes hole quality well beyond what drilling alone can achieve.