Reaming isn’t just about making holes rounder—it’s about achieving precision that drilling alone can’t deliver. With over 15 years machining parts for aerospace, medical, and audio sectors, proper reaming strategy eliminates assembly headaches while keeping costs reasonable.
Designers should know that reaming delivers ±0.005–0.01 mm tolerance with Ra 0.8–1.6 μm finish, but requires careful pre-hole sizing and geometry planning to justify the added cost. Success depends on understanding material constraints, tool access requirements, and when reaming beats boring or honing.
Learn when reaming justifies the extra step, how to size pre-holes correctly, and cost comparisons with alternatives from real production runs.
Table of Contents
What Tolerances Can Reaming Actually Hold?
Reaming delivers ±0.005–0.01 mm hole tolerance consistently—a 5x improvement over drilling’s typical ±0.025–0.05 mm variation. This precision makes reaming ideal for press-fit bearings, alignment pins, and servo motor mounts where hole diameter directly affects assembly performance and component life.
From our production data across 500+ reamed parts, we achieve the specified tolerance on over 95% of features when material and setup are controlled properly. Standard drilling gives you that consistency roughly half the time due to tool wander and chip evacuation issues. For comparison, boring can hit ±0.002 mm but requires dedicated setups that triple cycle time.
| Application Type | Recommended Tolerance | Why This Works |
|---|---|---|
| Press-fit bearings | ±0.008 mm | Ensures proper interference without binding |
| Alignment pins | ±0.01 mm | Prevents binding, allows smooth assembly |
| Clearance holes | ±0.025 mm | Cost-effective while maintaining function |
| Medical O-ring grooves | ±0.008 mm | Required for reliable sealing performance |
| Audio potentiometer bushings | ±0.012 mm | Balances fit with manufacturing cost |
Going tighter than ±0.005 mm requires specialized reamers and climate-controlled environments, often doubling machining cost. ISO 2768-f tolerance class (±0.01 mm for most hole sizes) aligns well with standard reaming capabilities and keeps inspection straightforward.
Design Takeaway: Use the table above to select appropriate tolerances for your application. Avoid over-tolerancing—most assembly problems come from geometric issues, not diameter variation. If you need better than ±0.005 mm, evaluate whether boring or bushing insertion makes more business sense.
Can Reaming Handle the Depth and Alignment I Need?
Reaming works reliably up to 5x diameter depth (50 mm deep for a 10 mm hole) with proper chip evacuation, and maintains ±0.01 mm straightness over typical depths of 2-3x diameter. Beyond these limits, expect 50-100% higher machining costs and consider whether larger clearance holes with pressed-in bushings might be more cost-effective.
The practical design limit is 3x diameter for blind holes and 5x diameter for through-holes. A 10 mm blind hole should stay under 30 mm deep to avoid chip packing issues that double cycle time. We’ve successfully reamed 12 mm through-holes to 60 mm depth in aluminum, but the setup complexity and tool rigidity requirements make this expensive for low-volume production.
Alignment accuracy depends on your assembly tolerance stack-up. Our ±0.01 mm straightness means a 50 mm deep hole might deviate 0.5 mm from true at the bottom—acceptable for clearance applications but problematic for press-fit assemblies. If your design requires a bearing or pin to align within ±0.2 mm over the full depth, reaming alone won’t achieve this reliably.
Tool access becomes critical in complex geometries. Recessed holes or those near walls require straight-line tool approach with adequate clearance. Parts with angled surfaces or intersecting features may need special fixturing, adding $200-500 to setup costs for small quantities.
Design Takeaway: If your hole depth exceeds 3x diameter, evaluate whether your assembly really needs the precision—often a larger clearance hole with a bushing delivers better performance at lower cost. Reserve deep reaming for applications where surface finish on the hole wall is critical to function.
Will My Material Choice Affect the Reamed Finish?
Material selection dramatically impacts both reamed surface finish and machining cost—aluminum achieves Ra 0.8 μm easily while stainless steel typically runs Ra 1.6-3.2 μm due to work hardening, often requiring 2x longer cycle times. For rotating assemblies requiring smooth operation, stick with aluminum or free-machining steel to avoid performance issues and cost escalation.
6061-T6 aluminum consistently produces Ra 0.8-1.2 μm with standard tooling, making it ideal when bearing performance or cosmetic appearance matters. 304 stainless achieves Ra 1.6-2.4 μm but requires flood coolant and slower feeds, typically adding 50-75% to machining time. For static assemblies like mounting brackets, this surface difference rarely affects function.
Brass and bronze machine exceptionally well for reaming, often achieving Ra 0.6-1.0 μm with minimal tool wear, making them excellent choices for precision bushings or bearing surfaces in low-corrosion environments. Carbon steel grades like 1018 and 4140 provide good compromise between machinability and strength.
Avoid work-hardening materials like 316 stainless and PEEK for reamed holes unless absolutely required—these materials can cause tool chatter and dimensional drift that compromises hole quality. Glass-filled nylon machines predictably but produces Ra 3.2-6.3 μm due to fiber pullout, making it unsuitable for precision bearing applications.
Critical design consideration for plastics: thermal expansion during cutting causes Delrin parts to measure 0.01-0.02 mm oversize immediately after machining. Plan for 2-4 hour stabilization time before final inspection or critical assembly operations.
Design Takeaway: Choose aluminum when surface finish affects performance or appearance. Use stainless steel only when corrosion resistance justifies the cost penalty. For plastic parts requiring tight fits, plan for thermal effects in your assembly process or specify post-machining dimensional verification before critical operations.
Does My Part's Geometry Allow Tool Access for Reaming?
Reaming requires straight-line tool approach with at least 2x hole diameter clearance around the entry point—a 10 mm reamed hole needs 20 mm clearance radius for standard tooling. Simple geometry check: if you can’t draw a straight line from your spindle to the hole center without hitting ribs, bosses, or walls, expect $300-800 in custom tooling costs or design changes.
The critical constraint is tool length versus rigidity. Standard reamers work best with length-to-diameter ratios under 4:1 to prevent deflection and chatter. Common problem areas include holes in L-bracket corners, behind mounting ribs, or in deep pockets where standard tools can’t reach. For these situations, we need specialized extended-reach tools that cost 3-5x more and run 50-100% slower to maintain stability.
Intersecting holes create tool entry problems. Reamers need flat, perpendicular surfaces to start cleanly—angled or curved entry points cause the tool to wander and create oversized holes. If your hole must start on an angled surface, plan for a spot-facing operation to create a flat entry area, adding another setup to your process.
Wall proximity matters significantly. Holes closer than 1.5x diameter from edges risk breakthrough during cutting, especially in materials like aluminum where chips can grab and pull. We’ve successfully reamed holes 8 mm from thick aluminum plate edges, but thin-walled housings often crack or deform under cutting forces.
Design Takeaway: Before finalizing your design, verify tool access by sketching clearance circles around each reamed hole in your CAD model. If standard tooling can’t reach, consider moving the hole, adding access relief, or switching to drilling with post-process honing for better economics.
What Design Rules Should I Follow for Reamed Holes?
Follow these key design rules: maintain minimum 1.5x diameter wall thickness around holes, keep holes at least 2x diameter from edges, and avoid placing reamed holes on angled surfaces steeper than 15° from perpendicular. Breaking these rules typically results in oval holes, wall breakthrough, or poor surface finish that requires expensive rework or part replacement.
Wall thickness directly affects hole quality. Less than 1.5x diameter thickness causes walls to deflect under cutting forces, creating oval holes that won’t accept press-fit bearings properly. We recommend 3x diameter thickness for optimal roundness, but 1.5x works for most applications. Parts thinner than 1x diameter often warp during reaming—the cutting forces literally bend the part, requiring costly straightening operations afterward.
Edge distance prevents catastrophic breakthrough. Holes closer than 2x diameter from edges can break through during cutting, especially in soft materials where chips tend to grab. This typically ruins the part entirely since welding repair affects heat treatment and dimensional stability. Quick CAD check: sketch a circle 2x your hole diameter around each feature—if it overlaps an edge, move the hole or add material.
Surface preparation affects success rates significantly. Reamed holes starting on angled surfaces cause tools to walk, creating oversized features that fail inspection. If angled entry is unavoidable, add a spot-face operation to create a flat starting surface, or consider whether a larger clearance hole with bushings might be more economical.
Design Takeaway: Verify these rules in CAD before releasing drawings. Adding 2-3 mm of material around critical holes costs nothing in design but can save hundreds in manufacturing rework. When rules conflict with your design intent, consider alternative hole-making methods or part geometry changes early in development.
What Pre-Hole Size Should I Specify for Reaming?
For most reaming operations, specify pre-holes 0.1-0.2 mm smaller than final diameter—a 10.000 mm finished hole should start with a 9.8-9.9 mm drilled hole. On drawings, call out the final reamed dimension with your required tolerance and add a note like “ream after drilling 9.9 mm pilot hole” to communicate the sequence clearly to your machinist.
The stock allowance varies by material and application criticality. Aluminum works well with 0.15 mm stock removal, while harder materials like stainless steel prefer 0.1 mm to avoid tool overload. Larger holes (over 20 mm diameter) can handle up to 0.25 mm stock removal, but precision holes under 6 mm should stay closer to 0.1 mm to prevent tool breakage.
Common specification mistakes cost money unnecessarily. Over-tolerancing pre-holes (like ±0.02 mm) adds drilling cost since reaming corrects diameter anyway—specify ±0.1 mm on pilots instead. Conversely, too much stock removal (over 0.3 mm) causes poor surface finish and may require slower feeds that increase cycle time by 30-50%.
For parts requiring heat treatment, your drawing should specify the machining sequence: “drill 9.8 mm before heat treatment, ream to 10.0 ±0.01 mm after.” This prevents confusion and ensures dimensional accuracy on critical features.
Quick decision rule: if your hole tolerance is ±0.02 mm or tighter, specify pre-hole sizing and sequence on drawings. For looser tolerances (±0.05 mm), let your machinist choose the optimal approach to save communication overhead.
Design Takeaway: Specify final dimensions with tight tolerances, pre-holes with loose tolerances. Add sequencing notes for critical features and heat-treated parts. When hole tolerance exceeds ±0.05 mm, standard drilling alone often works fine—avoid over-specifying operations that don’t add functional value.
Will Heat Treatment Change Hole Size After Reaming?
Heat treatment typically changes hole diameter by 0.01-0.05 mm depending on material and treatment type—for clearance holes with ±0.1 mm tolerance, this is usually acceptable, but press-fits requiring ±0.02 mm need post-treatment machining. Use this decision framework to avoid unnecessary operations while preventing assembly problems.
Different materials behave predictably during heat treatment. Aluminum stress relief causes minimal growth (0.005-0.015 mm), making it manageable for most applications without extra operations. Steel hardening shrinks holes by 0.02-0.04 mm—acceptable for clearance applications but problematic for tight fits where interference becomes excessive.
Smart decision criteria: evaluate your tolerance requirements against expected size changes. Clearance holes with ±0.1 mm tolerance rarely need post-treatment machining. Bearing seats, press-fits, and threaded holes requiring ±0.02 mm control should be called out for finish reaming after heat treatment. This approach avoids over-machining while ensuring critical fits work properly.
Cost consideration: post-heat treatment reaming typically adds 25-40% to hole machining cost due to setup and tool requirements. For non-critical features, consider whether designing with larger clearances eliminates this operation entirely. Sometimes a bushing or larger hole with an O-ring costs less than precision post-treatment machining.
On drawings, specify which holes need post-treatment finishing: “ream to final size after heat treatment” for critical features, and group related holes for single-setup efficiency when positional accuracy matters for assembly.
Design Takeaway: Compare your hole tolerance requirements to expected heat treatment changes—if tolerance is 2x larger than expected change, standard sequencing works fine. For tighter requirements, specify post-treatment finishing or consider design alternatives like bushings that avoid the extra operation and cost.
How Much Does Reaming Add to My Part Cost?
Reaming typically adds $8-15 per hole to standard drilling costs ($2-5 per hole)—a 10 mm reamed hole in aluminum costs about $12 total vs. $3 for drilling alone, while stainless steel can reach $18+ due to slower speeds and tool wear. The 3-4x cost premium pays for itself when tight fits prevent assembly problems that cost $150+ in rework and delays.
Cost breakdown varies by production volume. Single prototypes see the highest per-hole cost ($15-25 total) due to setup overhead. At 25-100 piece quantities, costs drop to $10-15 per hole as setup amortizes. High-volume production (500+ pieces) reaches $6-10 per hole, making reaming economical when assembly tolerances justify the precision.
ROI justification becomes clear when you consider failure costs. A $12 reamed hole prevents press-fit bearings from spinning loose, eliminates pin misalignment, and avoids field service calls. Compare this to rework costs: drilling out failed press-fits and installing oversized bushings typically costs $150-300 per part plus schedule delays.
Material choice dramatically impacts economics. Aluminum and brass ream efficiently with predictable costs. Stainless steel requires specialized tooling that can double cycle time, making it economical only when corrosion resistance is essential.
Design Takeaway: Budget $10-15 per reamed hole vs. $3-5 for drilling, but consider the 5-10x cost of assembly failures. Justify reaming when fit tolerances affect function—for clearance holes where ±0.05 mm works fine, save the money and use standard drilling.
How Do I Specify Reamed Holes on Technical Drawings?
Specify reamed holes with final diameter, appropriate tolerance (±0.005-0.01 mm based on function), and prominent “REAMED HOLE” callouts to ensure suppliers account for the extra operation in quotes and scheduling. Under-specification leads to standard drilled holes that fail assembly, while over-specification can double quoted costs unnecessarily.
Start with tolerance selection based on actual assembly needs. Use ±0.005 mm for press-fit bearings where interference is critical, ±0.01 mm for alignment pins requiring smooth operation, and ±0.02 mm for close-clearance applications. Each step tighter typically adds 25-40% to machining cost, so specify based on function, not arbitrary precision.
Surface finish callouts should reflect performance requirements. Specify Ra 1.6 μm for bearing surfaces where smoothness affects operation, Ra 0.8 μm for medical applications requiring cleanability, or leave unspecified for non-critical holes. Adding surface finish requirements increases costs by 30-50% due to slower cutting and inspection needs.
Critical communication: mark reamed holes prominently with notes like “REAM TO FINAL SIZE AFTER HEAT TREATMENT” to prevent manufacturing shortcuts. If suppliers don’t recognize reaming requirements during quoting, you’ll face change orders and delays when they discover the extra operations needed.
Design Takeaway: Call out “REAMED HOLE” prominently to ensure accurate quotes and prevent manufacturing surprises. Specify tolerances based on actual fit requirements—each step tighter adds significant cost. Clear specification prevents assembly failures while avoiding over-specification that inflates costs unnecessarily.
Conclusion
Reaming delivers ±0.005-0.01 mm precision when standard drilling isn’t sufficient, but costs 3-4x more per hole. Reserve reaming for press-fits, bearing seats, and alignment features where tolerance affects function—avoid over-specifying for clearance applications. Contact us to explore manufacturing solutions tailored to your precision hole requirements.
Frequently Asked Questions
If your design requires press-fit bearings (H7/h6 fits), alignment pins with <0.1 mm play, or threaded inserts that must seat flush, specify reaming. For snap-fits, clearance bolts, and loose assemblies where ±0.1 mm doesn’t affect function, standard drilling saves 70% of hole machining cost.
Plan for 2-5% rejection rate on tight-tolerance reamed holes. Design recovery options: oversized holes can often accept bushings, while undersized holes may be salvaged with careful honing. Build 10% extra material cost into budgets for critical parts with multiple reamed features.
Vary by function to optimize cost. Use ±0.005 mm only for press-fits and critical alignments, ±0.01 mm for precision clearances, and ±0.02 mm for general applications. This approach can reduce total machining cost by 30-40% compared to uniformly tight tolerancing.
Quick formula: if (reaming premium per hole × quantity) < (cost of one assembly failure × expected failure rate), reaming pays off. Example: 100 parts × $10 reaming premium = $1,000 vs. potential $2,000 rework cost from press-fit failures.
Frame it as insurance against assembly failures: “Spending $10 extra per hole prevents $200 rework costs and schedule delays when bearings don’t fit properly.” Emphasize that reaming eliminates downstream problems rather than just improving precision.
Request capability studies showing their achieved tolerances on similar materials and hole sizes. Ask for CMM inspection reports from recent jobs. If they can’t provide data or seem uncertain about ±0.01 mm capabilities, consider alternative suppliers or relaxed tolerances.
