CNC Reaming Guide: Hole Tolerance, Allowance and Surface Finish

CNC reaming is a finishing process for holes that need better diameter control, roundness or surface finish than drilling alone can normally provide. A reamer removes a small, controlled amount of material from an existing hole. It does not create the hole from solid stock, and it cannot automatically correct every error left by the previous operation.

For buyers and designers, this distinction matters. A drawing may call for a precision dowel hole, bearing bore, valve passage or locating feature, but the final result depends on more than the nominal diameter. The drilled or bored hole must leave the correct reaming allowance, the reamer must suit the material and hole type, chips must evacuate in the right direction, and the finished hole must be inspected at the correct depth and temperature.

This guide explains how CNC reaming works, how it differs from drilling and boring, how much stock should be left, why reamed holes become oversize or undersize, how to specify fit and surface requirements and what information a supplier needs for an accurate quotation.

What Is CNC Reaming?

CNC reaming enlarges and finishes a previously machined hole with a multi-edge cutting tool called a reamer. The tool has a short lead or chamfer that performs most of the cutting and a longer section that guides and sizes the hole.

A typical sequence is:

1. Spot or pilot the location when required.

2. Drill the hole below final size.

3. Bore, interpolate or otherwise correct the pre-hole if position or straightness requires it.

4. Ream to the specified diameter.

5. Deburr, clean and inspect the finished feature.

Reaming is normally chosen when the hole needs a repeatable finished size and good surface without the time or complexity of a full boring or honing process. It is widely used for dowel pins, bushings, shafts, bearings, valve components, hydraulic parts, automotive housings and precision assembly features.

What a Reamer Can and Cannot Correct

A reamer primarily follows the existing hole. It can improve diameter, roundness and surface texture when the pre-hole is suitable, but it has limited ability to relocate a hole or straighten a badly wandering axis.

Kennametal explains this practical difference in its boring guide: reaming is fast and effective for finishing, while boring is better able to cut a straight path rather than simply follow drill walk.

Reaming Can Often Improve

• Final diameter consistency.

• Roundness when the pre-hole error is modest.

• Surface finish.

• Repeatability across a production batch.

• Fit between the hole and a pin, shaft or bushing.

• Minor taper or tool marks when sufficient stock remains.

Reaming Cannot Reliably Fix

• A hole located far outside its position tolerance.

• Severe drill wander or curved deep holes.

• Major ovality or lobing.

• A pre-hole that is already too large.

• An interrupted feature that is incompatible with the reamer.

• Poor fixturing or part movement.

• Inadequate tool access.

• A tolerance tighter than the complete machine, tool and inspection system can hold.

If the location is critical, the supplier may drill, then bore or circular-interpolate the hole before reaming. The intermediate operation creates a more accurate axis for the reamer to follow.

CNC Reaming vs Drilling, Boring and Honing

Each process serves a different purpose.

When to Choose Reaming

Reaming is a strong option when:

• The hole already has acceptable position and straightness.

• The required diameter is available as a standard or economical custom reamer.

• Production quantity justifies a dedicated finishing tool.

• The required finish and tolerance are within the process capability.

• The geometry permits stable entry and chip evacuation.

When Boring May Be Better

Boring may be preferred when:

• The pre-hole location needs correction.

• One adjustable tool must produce several nearby diameters.

• The hole is large enough for a boring bar.

• The design requires close coaxiality to another feature.

• The interrupted cut would damage a multi-edge reamer.

• Small diameter adjustments are needed during setup.

When Honing or Grinding May Be Better

Honing or grinding may be needed for unusually fine surface texture, very close geometry, hard material or special functional patterns. A bearing or sealing bore may need more than a dimensionally correct reamed surface.

Reaming Allowance: How Much Material Should Be Left?

Reaming allowance is the difference between the pre-hole diameter and the finished reamed diameter. It is normally expressed on diameter, although tool data may describe radial stock. The distinction must be clear.

For example, if a hole is drilled to 9.80 mm and reamed to 10.00 mm, the total diametral allowance is 0.20 mm and the radial stock is 0.10 mm per side.

There is no universal reaming allowance. The correct value depends on:

• Final hole diameter.

• Workpiece material and hardness.

• Reamer material and geometry.

• Pre-hole quality and runout.

• Through-hole or blind-hole condition.

• Required tolerance and surface finish.

• Machine rigidity and spindle condition.

• Coolant delivery.

• Conventional or high-performance reaming strategy.

Always use the tool manufacturer's data for the exact reamer. MAPAL's FixReam technical data, for example, gives material- and diameter-specific stock-removal guidance rather than one allowance for every application.

Too Little Allowance

If the pre-hole is too close to final size, the cutting edges may not engage consistently. The reamer can rub instead of cut, follow high and low spots, create an uneven finish or wear prematurely. A small pre-hole error may remain visible because there is not enough stock to clean up the complete circumference.

Too Much Allowance

Excess stock increases cutting force, torque, heat and chip volume. The reamer may chatter, deflect, chip or produce a tapered and oversized hole. Reaming should not be used as a heavy roughing operation.

Allowance Must Cover Pre-Hole Variation

The nominal drill size is not the only concern. Measure the actual pre-hole diameter, roundness and taper across representative parts. If the pre-hole varies more than the finishing allowance, some holes may cut properly while others rub or overload the reamer.

Reamer Anatomy and Cutting Action

Understanding the tool helps explain common defects.

Lead or Chamfer

The lead enters the pre-hole and performs the cutting. Its angle and length influence force, guidance, chip formation and suitability for blind or through holes.

Flutes

Flutes provide cutting edges and chip space. Straight, right-hand spiral and left-hand spiral designs move chips differently and suit different hole conditions.

Margins and Guide Lands

Margins or guide lands support the tool against the finished bore. They help stabilize size and surface but can rub if the tool, coolant or allowance is wrong.

Back Taper

The reamer body may reduce slightly in diameter behind the cutting area. This prevents unnecessary rubbing and reduces the risk of scoring during withdrawal.

Shank and Holder

The holder connects the tool to the spindle. Runout, contamination, overhang and clamping method directly affect how evenly the cutting edges share the load.

Common Types of Reamers

Solid Carbide Reamers

Solid carbide provides rigidity, wear resistance and high-speed capability. It is common for precision production in stable machines. Carbide is less tolerant of impact and severe misalignment than a more flexible high-speed-steel tool.

High-Speed Steel and Cobalt Reamers

HSS and cobalt tools can be tougher and more forgiving in some low-volume or manual applications. They usually operate at lower cutting speeds than carbide and may be economical for prototypes or larger stocked size ranges.

Chucking Reamers

Chucking reamers are general machine reamers with a straight shank. They are available in many standard metric and inch sizes and in different flute configurations.

Expansion and Adjustable Reamers

An expansion reamer can be adjusted over a limited range to compensate for wear or reach a target size. It is not a universal substitute for a correctly sized tool. Adjustment, measurement and edge condition require control.

Replaceable-Head Reamers

Replaceable-head systems combine a reusable holder with a precision cutting head. They can reduce tool-change and inventory cost in production while supporting through-coolant delivery.

Single-Blade and Guide-Pad Reamers

These tools use one or more cutting edges with guide pads that support the tool in the bore. MAPAL describes how guide-pad reamers absorb cutting forces and support fine bore machining. They are especially relevant to demanding production applications.

PCD Reamers

Polycrystalline diamond tools provide long life and excellent finish in non-ferrous and abrasive materials such as high-silicon aluminum. They are not used for ordinary ferrous machining because of chemical and thermal limitations.

Combination Drill-Reamers

A combination tool creates and finishes the hole in one cycle. It can reduce tool changes and improve productivity when geometry, volume and machine conditions suit the design. MAPAL's Tritan Drill-Reamer is an example of combining drilling and reaming functions.

Combination tools are application-specific. They reduce flexibility and may not correct position as well as separate drilling, boring and reaming operations.

Straight Flutes vs Spiral Flutes

Flute direction influences chip flow.

Straight-Flute Reamers

Straight flutes are common for general reaming. They can be suitable for both through and blind holes depending on the tool geometry and material. They may struggle when long chips have no clear path.

Left-Hand Spiral, Right-Hand Cut

This configuration tends to push chips forward, making it useful for through holes where chips can exit ahead of the tool. It also helps resist the tendency to pull the reamer into the work.

Right-Hand Spiral, Right-Hand Cut

This configuration tends to draw chips back toward the entry and may be selected for blind holes. It can also provide a smoother cutting action in some materials and interrupted conditions.

These are general tendencies, not a substitute for the toolmaker's application guidance. Hole orientation, coolant, material and lead geometry also affect chip direction.

Through-Hole Reaming

A through hole provides an exit for the lead and chips. It is usually easier to ream than a blind hole, but the design still needs clearance.

Important considerations include:

• The reamer lead must pass completely through the full-diameter requirement.

• The fixture must leave exit clearance.

• Chips must not pack against a backing plate.

• Breakthrough burrs require control.

• The cutting edges must not strike a fixture or adjacent part.

The usable full-diameter length begins behind the lead. A drawing that requires precision size to the final edge should be reviewed for tool overtravel and burr control.

Blind-Hole Reaming

Blind holes are more difficult because chips cannot simply exit ahead of the tool. The bottom also limits how far the cutting lead can travel.

The drawing should distinguish:

• Total hole depth.

• Full-diameter reamed depth.

• Drill-point or relief depth.

• Required bottom form.

• Clearance for the reamer lead and chips.

A standard reamer cannot produce its full diameter all the way to a perfectly flat blind bottom. The lead requires axial space. If the assembly needs full-size engagement close to the bottom, the design may require extra depth, a bottoming reamer, boring or another finishing process.

Coolant and chip evacuation are especially important. A geometry that pushes chips forward can pack them at the bottom, so the reamer style must match the blind-hole condition.

Entry Chamfers, Exit Edges and Interrupted Holes

Entry Chamfer

A small, concentric entry chamfer can help the reamer engage smoothly and protect the finished edge. A large or off-center chamfer may reduce guidance.

The chamfer should be created in the same setup as the hole when concentricity matters. A cosmetic hand chamfer added later can become uneven around a close-tolerance bore.

Angled Entry

An angled or curved entry loads one side of the reamer first. This can cause deflection, chatter or edge damage. Add a spotface or prepared pilot surface when the design permits.

Cross Holes and Keyways

Cross holes, grooves and keyways interrupt the cut. The cutting edges repeatedly enter and leave material, which can chip the tool and create a poor finish. A spiral-flute reamer, tougher cutting material, reduced interruption or a different finishing method may be needed.

Identify every interruption on the drawing and 3D model. Do not assume the supplier will discover a hidden cross passage from the main view.

Cutting Speed, Feed and Coolant

Reaming performance depends on a balanced combination of speed and feed.

Cutting Speed

Reaming speed is selected for the workpiece, tool material, coating, diameter and coolant. Running too fast can create heat, wear and built-up edge. Running too slowly can also produce built-up edge or rubbing in adhesive materials.

Feed

Each cutting edge needs enough feed to cut rather than rub. An extremely low feed is not automatically safer. It may worsen finish and tool life. Too much feed increases force, lobing and taper.

Coolant

Coolant lubricates the margins, controls heat and moves chips. Through-tool delivery is valuable for deeper, blind or high-performance applications. Clean, correctly mixed coolant protects small passages and cutting edges.

Consistent Motion

Avoid dwelling at the bottom unless the toolmaker specifically calls for it. Dwelling can rub the bore and create marks. The reamer should normally feed smoothly through the cut and withdraw under a controlled method.

The exact values should come from the reamer supplier and be validated on the actual material and setup. Generic internet speeds and feeds do not account for all application variables.

Reamer Runout and Toolholding

Runout makes one flute remove more material than the others. The result can be oversize diameter, lobing, chatter, poor finish and premature wear.

Control measures include:

• Clean the spindle, holder and tool shank.

• Use a precision collet, hydraulic chuck or shrink-fit holder as appropriate.

• Measure runout near the cutting end, not only at the holder.

• Minimize unnecessary tool overhang.

• Inspect damaged collets and spindle tapers.

• Confirm that the pre-hole is aligned with the spindle path.

• Use a floating holder only when the process and machine require it.

A floating reamer holder can compensate for small alignment error in some applications, but it cannot fix a loose fixture, bent tool or badly located pre-hole. Modern rigid CNC setups often use accurate fixed holders when machine alignment is controlled.

Why Reamed Holes Become Oversize

An oversized hole may result from:

• Excessive tool runout.

• A reamer ground or adjusted too large.

• Built-up edge changing the effective diameter.

• Chatter or vibration.

• Too much reaming allowance.

• Excessive cutting speed or unsuitable feed.

• Misalignment between tool and pre-hole.

• Trapped or recut chips.

• Thermal expansion during cutting or inspection.

• Worn guide pads or damaged cutting edges.

Do not assume that replacing the reamer with a smaller nominal tool will solve the root cause. Measure runout, inspect the cutting edges and compare results by depth and part sequence.

Why Reamed Holes Become Undersize

An undersized result can be caused by:

• Tool wear.

• Material springback or elastic recovery.

• Thermal contraction after measurement.

• Insufficient allowance causing rubbing rather than full cleanup.

• Built-up material or chip adhesion reducing effective cutting.

• An incorrect or poorly adjusted reamer.

• Burrs, contamination or measurement error.

• Coating or treatment applied after machining.

Plastics, thin walls and some ductile materials may relax after the tool exits. Measure at an agreed temperature and time when material behavior is significant.

Common Reaming Defects and Troubleshooting

Tapered Hole

Possible causes include misalignment, tool wear, excessive overhang, chip packing, uneven allowance or part deflection. Measure at the entrance, middle and bottom to identify the direction and magnitude of taper.

Bell-Mouth at the Entry

The entry becomes larger than the rest of the hole. Runout, unstable engagement, a poor chamfer or misalignment can contribute. The reamer may deflect until more guide length enters the bore.

Lobing or Poor Roundness

Uneven flute loading, vibration, a poor pre-hole, runout or unsuitable flute spacing can create a multi-lobed profile. A two-point bore gauge can miss some lobing patterns, so the inspection method matters.

Chatter Marks

Chatter leaves periodic marks and may enlarge the hole. Improve rigidity, reduce overhang, check allowance and runout, and review speed, feed and flute geometry.

Scored Surface

Chips trapped between the reamer and wall can score the bore. Built-up edge, damaged margins, poor coolant or reversing through chips can also leave scratches.

Poor Finish with Correct Diameter

A hole can pass a plug gauge and still fail the functional finish. Check edge condition, coolant, allowance, pre-hole texture, feed and chip evacuation. Specify a roughness value only when it is functionally necessary.

Short Tool Life

Common causes include excessive runout, too much stock, incorrect speed, hard scale, interrupted cuts, poor coolant and unsuitable cutting material. Track tool life by parts or cutting length rather than waiting for random failure.

Material-Specific Reaming Considerations

Aluminum

Aluminum can adhere to cutting edges and margins. Sharp, polished geometries and suitable lubrication help prevent built-up edge. High-silicon aluminum is abrasive and may justify PCD or another wear-resistant cutting material.

Carbon and Alloy Steel

Steel machinability changes with alloy and hardness. Coating, carbide grade and lead geometry should suit the condition. Scale and inconsistent heat treatment can shorten tool life.

Stainless Steel

Austenitic stainless steel can work-harden and form built-up edge. The reamer must cut positively with suitable feed and continuous lubrication. Repeated rubbing or dwelling can damage the surface and tool.

Titanium

Titanium concentrates heat at the edge and can spring back against the margins. Tool geometry, coating, coolant and allowance require careful validation. MAPAL publishes dedicated titanium reaming and fine-boring guidance for application-specific tooling.

Cast Iron

Cast iron produces short, abrasive chips. Dry or minimum-lubrication strategies may be used with appropriate tooling, but fine particles require safe extraction and machine protection.

Brass and Bronze

Free-cutting copper alloys can ream efficiently, while some bronzes are abrasive or prone to grabbing. Lead angle and rake should match the alloy.

Engineering Plastics

Plastics may heat, smear, expand or recover after cutting. Sharp tools and controlled temperature are important. Moisture-conditioned dimensions and post-machining relaxation should be considered for nylon and similar materials.

Specifying a Reamed Hole on a Drawing

A useful drawing describes function and acceptance, not the supplier's entire machining program.

Include:

• Nominal diameter and size tolerance.

• Fit class when a recognized fit system applies.

• Hole depth or full-diameter engagement depth.

• Through or blind condition.

• Position relative to defined datums.

• Perpendicularity, cylindricity or straightness only when required.

• Surface roughness if functionally necessary.

• Entry chamfer and exit edge requirement.

• Internal burr requirements at cross holes.

• Final coating or treatment and whether size applies before or after it.

• Inspection and reporting requirements.

Avoid notes such as “ream as required” without a finished size and acceptance criterion. Also avoid applying the tightest tolerance to every hole when only one feature locates the assembly.

H7 and Other Hole Tolerance Classes

An H7 callout belongs to the ISO system of limits and fits. The letter identifies the tolerance-zone position and the number identifies the tolerance grade. The numerical tolerance is not the same for every nominal diameter.

Do not treat H7 as a machining process. A supplier may produce an H7 hole by reaming, boring, honing, grinding or another method depending on size, material, quantity and geometry.

If a hole mates with a shaft, specify or communicate the intended fit and operating condition. A clearance fit for easy assembly is different from a transition or interference fit for permanent location. Our CNC machining article library includes related guides on tolerances, dowel holes and bearing fits.

Position Tolerance vs Hole Size

Size and position control different things.

• Size tolerance limits the hole diameter.

• Position tolerance limits where the hole axis may lie relative to datums.

• Perpendicularity may control axis orientation.

• Cylindricity controls the full cylindrical surface form.

• Straightness may control the axis or surface element, depending on the callout.

A perfectly sized reamed hole can still be in the wrong place. If assembly location matters, define datums and position tolerance rather than relying on coordinate dimensions with ambiguous plus/minus limits.

How Reamed Holes Are Inspected

Go/No-Go Plug Gauges

Limit plug gauges provide fast acceptance for production. The GO side checks the maximum material condition of the hole, while the NO-GO side checks the opposite limit according to the gauge design and applicable standard.

A plug gauge gives a functional size decision but does not report the actual diameter, taper or roundness.

Pin Gauges

Gauge pins can estimate size and check accessibility. Cleanliness, burrs, temperature and operator technique affect the result. Do not force a pin into a precision bore.

Bore Gauges and Internal Micrometers

These instruments can measure diameter at multiple depths and directions. They require correct setting, alignment and operator technique.

Air Gauging

Air gauges are useful for fast, sensitive comparison of bore size and can detect variation with minimal contact. Tooling and masters must be calibrated for the application.

Coordinate Measuring Machines

A CMM can evaluate size, position and orientation when the probe can reach the feature and the measurement strategy is appropriate. A few measured points may not fully reveal lobing or local damage.

Roundness and Form Measurement

Dedicated roundness or cylindricity equipment may be needed for demanding geometric requirements. The measuring system should resolve the specified tolerance and sample enough sections along the bore.

Surface Roughness Measurement

A stylus or optical instrument may measure bore finish when access allows. State the roughness parameter, cutoff and evaluation standard where the result is critical.

Temperature and Cleanliness

Precision hole measurement should occur at a controlled or documented temperature. Chips, oil film, burrs and gauge contamination can change the result. Clean both the hole and instrument without damaging the surface.

Reaming Thin Walls and Flexible Parts

Reaming force can expand a thin wall during cutting. After the tool exits or the fixture releases, the hole may shrink, become oval or move relative to other features.

Possible process strategies include:

• Support the wall close to the hole.

• Leave temporary material for rigidity.

• Rough machine symmetrically.

• Reduce clamping distortion.

• Use a sharp, low-force reamer.

• Finish after major stress-releasing operations.

• Measure the part in the same free or restrained condition defined by the drawing.

Designers should increase local thickness, add a boss or move the hole away from a free edge when function permits.

Reaming After Heat Treatment or Coating

Process sequence changes the final size.

Heat Treatment

Heat treatment can distort the hole or change hardness. A part may be rough machined, heat treated and then finish reamed, bored, honed or ground. The final tool must be suitable for the hardness and remaining allowance.

Anodizing

Anodizing builds oxide on aluminum surfaces and can reduce the finished hole diameter if the bore is not masked. Specify whether the hole should be anodized and whether the tolerance applies before or after treatment.

Plating and Conversion Coatings

Plating thickness can alter fit. Masking, post-plate sizing or an adjusted pre-finish dimension may be required. The quotation should state who controls the complete process stack.

Passivation

Passivation normally does not add a meaningful coating thickness like plating, but cleaning and handling must still protect the finished bore.

Design Guidelines for Reamed Holes

Use Standard Finished Diameters

Standard reamer sizes are easier to source and replace. A custom diameter may be justified for production but can increase prototype cost and lead time.

Provide Adequate Tool Access

Check the reamer and holder envelope. A nearby wall can prevent a rigid short holder from reaching the hole, forcing excessive overhang.

Give Through Holes Exit Clearance

Allow the lead to pass beyond the precision length without hitting the fixture or another feature. Keep a backing plate away from the chip exit.

Add Bottom Clearance to Blind Holes

Provide space for the lead and chips beyond the required full-diameter depth. If that is impossible, discuss a bottoming tool or alternative process.

Avoid Severe Interruptions

Move cross holes, slots or keyways away from the precision reamed length where possible. If interruption is essential, identify it clearly.

Keep the Entry Stable

Use a flat, perpendicular entry and a concentric chamfer. Avoid beginning the cut on a curved or angled face.

Specify Only Functional Tolerances

A very tight size, position, form and finish on the same hole can require several operations and specialized inspection. Separate what the assembly truly needs from preferences.

Consider Replaceable Bushings

For a wear surface or serviceable location, a standard bushing in a practical housing bore may be more economical than an extremely demanding integral bore.

What Drives CNC Reaming Cost?

Important cost factors include:

• Standard versus custom reamer diameter.

• Material and hardness.

• Number of holes per part.

• Hole depth and access.

• Blind, through or interrupted geometry.

• Pre-hole preparation and boring requirements.

• Tolerance, position and form controls.

• Surface-finish requirement.

• Tool-life risk and replacement frequency.

• Coating or heat-treatment sequence.

• Gauge, CMM and reporting requirements.

• Prototype or production quantity.

For a few prototypes, circular interpolation or boring may avoid the cost of a custom reamer. For hundreds or thousands of repeated holes, a dedicated reamer or combination tool may reduce cycle time and cost per part.

What to Include in a CNC Reaming RFQ

Provide:

• 3D CAD model and controlled 2D drawing.

• Material grade, condition and hardness.

• Finished diameter and tolerance or fit class.

• Hole depth and required full-diameter depth.

• Blind or through condition.

• Entry, exit, cross holes and interruptions.

• Datum and position requirements.

• Form and surface-finish requirements.

• Mating pin, shaft, bearing or bushing information.

• Heat treatment, anodizing, plating or other finishing.

• Whether the finished tolerance applies before or after coating.

• Inspection method and documentation.

• Prototype quantity and future production volume.

Use the complete CNC machining RFQ checklist for revision control, quality documents, packaging and delivery information.

Copy-and-Paste RFQ Template

Please quote the attached CNC-machined part with precision reamed holes. Material: [grade, condition and hardness]. Finished hole: [diameter, tolerance or fit]. Quantity of holes per part: [number]. Full-diameter depth: [value]. Hole type: [through or blind]. Entry and interruptions: [flat, angled, cross hole, keyway or none]. Critical requirements: [position, perpendicularity, roundness, cylindricity and surface finish]. Mating component: [pin, shaft, bearing or bushing]. Final treatment: [none, heat treatment, anodizing, plating or other]. The size requirement applies [before or after treatment]. Quantity: [prototype and production quantities]. Please identify the proposed pre-hole process, reaming allowance, inspection method and any DFM changes that could improve reliability or reduce cost.

Questions to Ask a CNC Supplier

1. Will the pre-hole be drilled only, or bored before reaming?

2. How will hole position be controlled separately from diameter?

3. What allowance will be left for the selected reamer?

4. Does the tool suit a blind, through or interrupted hole?

5. How will runout be measured and controlled?

6. How will chips and coolant move through the hole?

7. Which gauge or instrument will verify size, taper and roundness?

8. Does the fit apply before or after coating?

9. How will tool wear be detected during the batch?

10. Would boring, honing or a standard diameter be more economical?

Frequently Asked Questions

What is the purpose of CNC reaming?

CNC reaming finishes an existing hole to improve diameter control, roundness, surface finish and production repeatability. It removes a small allowance and is not intended to create the hole from solid stock.

Does a reamer make a hole perfectly straight?

Not necessarily. A reamer tends to follow the existing hole. If straightness or location needs correction, boring or circular interpolation may be required before reaming.

How much material should a reamer remove?

The correct allowance depends on diameter, material, tool, pre-hole quality and application. Use the exact reamer manufacturer's data. Too little stock causes rubbing and incomplete cleanup; too much increases force, heat and chatter.

Should reaming be done before or after heat treatment?

It depends on final hardness, expected distortion and tool capability. Precision parts are often rough machined before heat treatment and finish machined afterward, but the supplier should plan the complete sequence.

Can a blind hole be reamed?

Yes, with a suitable reamer and enough bottom clearance for the lead and chips. The full-diameter depth cannot extend to a perfectly flat bottom without a specialized tool or additional process.

Can reaming fix an off-location drilled hole?

Only to a limited extent. Reamers follow the pre-hole. Boring or milling should normally correct location before reaming when position is critical.

Why is a reamed hole oversized?

Common causes include runout, chatter, excessive allowance, misalignment, built-up edge, damaged cutting edges, trapped chips and thermal effects.

Why is a reamed hole undersized?

Tool wear, material springback, insufficient cleanup, thermal contraction, buildup on the tool or measurement error can produce an undersized result.

Can a reamer improve surface finish?

Yes, if the pre-hole, allowance, tool condition, feed, coolant and chip evacuation are suitable. Reaming cannot always remove deep drilling marks when too little stock remains.

What is the difference between reaming and boring?

Reaming uses a multi-edge sizing tool and is efficient for repeated precision holes. Boring uses a cutting tool that can better correct hole location and straightness and can be adjusted more flexibly.

What does an H7 reamed hole mean?

H7 is an ISO hole tolerance class, not a reaming instruction. Its numerical tolerance depends on nominal diameter. The supplier may use reaming or another finishing process to meet it.

Should a reamer be reversed out of a hole?

Follow the toolmaker's instructions. Reversing cutting direction while the tool remains in the bore can damage edges or score the surface in many applications. Controlled withdrawal is part of the validated cycle.

How is a reamed hole measured?

Methods include plug gauges, pin gauges, bore gauges, air gauges, CMM probes and roundness equipment. The method should match whether the requirement is functional size, actual diameter, taper, position or form.

Can reaming hold position tolerance?

Reaming can preserve a well-prepared hole's location, but it does not replace a process that establishes the axis. The pre-hole, setup and datum strategy determine position capability.

Is a custom reamer always necessary for a nonstandard hole?

No. Boring, circular interpolation, honing or an adjusted reamer may be alternatives. The best choice depends on tolerance, quantity, material and cost.

Final Takeaway

CNC reaming is an efficient precision-hole finishing process when the pre-hole, allowance, tool geometry, holder, coolant and inspection plan work together. It can deliver repeatable size and a good bore surface, but it cannot rescue an oversized hole or reliably relocate a badly wandering drilled axis.

Designers can improve manufacturability by choosing standard diameters, providing stable entries and exit clearance, allowing bottom space in blind holes, identifying cross-hole interruptions and specifying size, position, form and finish as separate functional requirements.

For precision holes in prototypes or production parts, send your model, drawing, material, fit, quantity and final-treatment requirements through the AluPrototype request-a-quote page. Our engineering team can review the pre-hole method, reaming strategy, inspection and DFM options before machining begins.