Tight tolerance quoting often surprises engineers with hidden costs. After machining thousands of precision parts for medical devices and aerospace components, seven key questions determine accurate pricing.
The seven questions cover feature prioritization, material constraints, surface finish strategy, cost drivers, fixturing requirements, setup limitations, and measurement capabilities. Answering these before requesting quotes prevents 2-4x cost surprises and ensures manufacturers understand your actual precision needs.
Learn which tolerances spike costs, when materials limit precision, and how finishes affect dimensions—backed by CNC data from regulated industries.
Table of Contents
Which Features Can Use Standard Tolerances?
Most CNC parts can use standard ±0.005″ (±0.127 mm) tolerances on 70-80% of features. Apply tight tolerances only to dimensions that control how your part physically connects to, fits into, or aligns with other components in your assembly.
Step-by-Step CAD Review Process:
- Find Your Assembly Interfaces Open your CAD assembly and identify where this part touches other components. These contact points need tight tolerances—everything else can be standard.
- Categorize Every Dimension
- Holes: Through holes for screws = standard. Press-fit holes for pins = tight.
- Walls: Structural walls supporting loads = tight. Cosmetic walls = standard.
- External surfaces: Sliding/mating surfaces = tight. Visible-only surfaces = standard.
- Apply the “Gap Test” If a dimension can vary by ±0.005″ without preventing assembly or causing interference, use standard tolerance. If that variation would cause binding, gaps, or misalignment, specify tight.
Common Over-Specification Mistakes:
- Applying ±0.001″ to all exterior dimensions (only mating edges need it)
- Tight tolerances on clearance holes (they’re clearance for a reason)
- Precision specs on internal ribs and supports (unless load-critical)
Design Takeaway: Spend 10 minutes reviewing your assembly to identify actual contact points and load paths. Apply tight tolerances only to dimensions that control these interfaces—typically 20-30% of your total dimensions.
When Do I Actually Need Tolerances Tighter Than ±0.005"?
Specify tighter than ±0.005″ when standard tolerances cause assembly problems or functional failures. Use ±0.002″ for light press fits, ±0.001″ for bearing seats, and ±0.0005″ for sliding interfaces only. Apply the interference calculation: shaft diameter × 0.001″ to determine actual requirements.
Immediate Tolerance Selection Guide:
Application Type Required Tolerance Cost Multiplier Calculation Method
Light Press Fits ±0.001-0.002″ 2-4x Shaft diameter × 0.001″ interference
Bearing Seats ±0.0005-0.001″ 4-6x Check manufacturer tolerance bands
Sliding Interfaces ±0.001″ 3-4x Test if >0.005″ causes binding
Control Shafts ±0.001″ 3-4x Smooth operation requirement
Clearance Holes ±0.005″ (standard) 1x Fastener fits with 0.010″ clearance
Quick Application Examples:
- 10mm press fit shaft: 10.01-10.02mm shaft, 10.00mm hole
- 25mm bearing seat: Check OEM specs, typically 0.025-0.050mm interference
- Control knob shaft: ±0.001″ prevents binding during rotation
From design consultations, we see engineers specify ±0.001″ on control shaft holes because binding occurs with ±0.005″ variation. However, the mounting bosses for the same assembly work perfectly at standard tolerances—no functional benefit from tightening.
When NOT to Tighten: Static joints, adjustable assemblies with built-in compensation, or any surface where ±0.005″ variation doesn’t prevent assembly or cause performance issues.
Design Takeaway: Calculate your actual interference requirements using the table above. If ±0.005″ variation prevents assembly or causes binding, document the functional requirement and specify tighter. Otherwise, use standard tolerances and invest precision where it provides measurable value.
Does My Material Make Tolerances Harder to Hold?
Material grade directly determines achievable tolerances. Use this selection guide: Aluminum 6061 for ±0.001″, 304 stainless for ±0.002″, Delrin/POM for ±0.005″, and Nylon for ±0.010″. Match your tolerance requirements to material capabilities during design phase.
Material Tolerance Capability Chart:
Material Grade Best Achievable Tolerance Characteristics Best Applications
Aluminum 6061 ±0.001″ Excellent machinability, stable Precision housings, brackets
Aluminum 7075 ±0.001″ High strength, good stability Aerospace components
Steel 1018/4140 ±0.001″ Excellent dimensional stability Structural, mechanical parts
Stainless 304/316 ±0.002″ Work hardens, needs proper speeds Corrosion-resistant precision
Brass 360 ±0.001″ Good machinability, stable Fittings, electrical components
Delrin/POM ±0.005″ Best plastic for precision Gears, bushings, insulators
Nylon 6/66 ±0.010″ Thermal expansion issues General mechanical, non-precision
Material Selection Decision Matrix:
Your Requirements Recommended Material Realistic Tolerance
Precision + Corrosion Resistance 316 Stainless ±0.002″
Precision + Light Weight 7075 Aluminum ±0.001″
Precision + Low Cost 6061 Aluminum ±0.001″
Chemical Resistance + Some Precision Delrin/POM ±0.005″
High Strength + Precision 4140 Steel ±0.001″
When Your First Choice Won’t Work: If plastic part needs ±0.001″, switch to aluminum or use metal inserts. If stainless won’t hold ±0.001″, accept ±0.002″ or plan secondary grinding. Design with material strengths rather than fighting limitations.
From our DFM experience, medical device housings requiring both biocompatibility and ±0.001″ sealing surfaces work best in 316 stainless steel machined to ±0.002″, then ground to final tolerance only where sealing occurs.
Design Takeaway: Check material tolerance capability BEFORE finalizing designs. If your specification shows 6063 aluminum with ±0.001″ tolerances, switch to 6061 or accept ±0.002″ realistic capability. Design with material strengths rather than fighting material limitations.
How Do Surface Finishes Affect My Tolerance Strategy?
Surface finish directly enables or limits tolerance capability. For ±0.001″ tolerances, specify Ra 1.6 μm maximum finish. For ±0.002″, Ra 3.2 μm works adequately. Plan post-processing dimensional changes upfront—anodizing adds 0.013-0.025mm, requiring machining undersize to compensate.
Surface Finish Requirements by Tolerance:
Your Tolerance Goal Minimum Required Ra Recommended Ra Why This Matters
±0.001″ 1.6 μm maximum 0.8 – 1.6 μm Tool marks interfere with measurement accuracy
±0.002″ 3.2 μm maximum 1.6 – 3.2 μm Acceptable measurement consistency
±0.003″ 3.2 – 6.3 μm 3.2 μm Standard machined finish sufficient
±0.005″ (standard) 6.3 μm acceptable 3.2 – 6.3 μm As-machined finish works fine
Immediate Decision Framework:
Step 1: Check Your Tolerance vs Current Ra Spec Look at your drawing tolerances, then verify surface finish callouts match the table above. If you specify ±0.001″ tolerance with Ra 6.3 μm finish, you’ll get measurement inconsistencies.
Step 2: Plan for Post-Processing Dimensional Changes
- Anodizing: Machine 0.013-0.025mm undersize, inspect after coating
- Chrome plating: Machine 0.005-0.015mm undersize for critical dimensions
- Powder coating: Machine 0.025-0.075mm undersize depending on thickness
- Bead blasting: Expect 0.002-0.005mm material removal
Step 3: Trade-off Analysis – Improve Finish vs Loosen Tolerance Before specifying expensive finishes, ask: “Can I loosen the tolerance instead?” A bearing seat might work at ±0.002″ with Ra 3.2 μm finish rather than ±0.001″ with expensive grinding to Ra 0.8 μm.
Real Design Decision Examples:
During design reviews, we often see medical device sealing surfaces with ±0.001″ tolerances but Ra 3.2 μm finish specs. This creates leakage because surface roughness allows fluid bypass regardless of dimensional accuracy. The solution: specify Ra 0.8 μm for proper sealing function.
Audio control shafts specified at ±0.001″ with as-machined finish cause binding during rotation. Tool marks create high spots that interfere with smooth operation. Upgrading to Ra 1.6 μm finish enables proper function.
Design Takeaway: Review every tight tolerance on your drawing and verify the surface finish spec enables that precision. If you need ±0.001″ function, budget for Ra 1.6 μm finish. If that’s too expensive, reconsider whether ±0.002″ tolerance with cheaper finish meets your actual requirements.
Which Tolerances Drive the Highest Cost?
Tolerances tighter than ±0.002″ create exponential cost increases. Conduct a tolerance audit: identify features that don’t affect assembly or function, then relax 70-80% of tight specifications to standard ±0.005″. Focus precision on the 3-5 dimensions that actually control part performance.
Tolerance Cost Audit Process:
Step 1: List All Dimensions Tighter Than ±0.005″ Print your drawing and highlight every dimension with tolerances like ±0.003″, ±0.002″, ±0.001″. These are your cost drivers.
Step 2: Function vs Cost Analysis
Tolerance Cost Impact Justify With This Question
±0.001″ 4-6x cost Does ±0.005″ prevent assembly or cause failure?
±0.002″ 2-3x cost Does ±0.005″ cause interference or poor fit?
±0.003″ 1.5-2x cost Does ±0.005″ affect function or appearance?
Step 3: High-Cost Feature Identification
- Small features (<5mm) with tight tolerances = highest cost multiplier
- Multiple tight tolerances on one part = setup and inspection costs compound
- Geometric tolerances (GD&T) with tight bands = CMM inspection required
Immediate Cost Reduction Strategy:
Category 1: Always Relax These (70% of tight tolerances)
- Wall thickness dimensions (unless structural)
- Clearance hole diameters for fasteners
- External cosmetic surfaces that don’t mate
- Internal features that don’t contact other parts
Category 2: Usually Can Relax (20% of tight tolerances)
- Mounting boss locations with adjustable hardware
- Non-critical radii and chamfers
- Features with built-in adjustment mechanisms
Category 3: Keep Tight (10% of tight tolerances)
- Bearing seats and press-fit interfaces
- Sealing surfaces and O-ring grooves
- Assembly datum surfaces for alignment
Real Project Cost Optimization:
During a recent design consultation, a consumer electronics housing had 12 dimensions at ±0.001″. Our audit identified that only connector cutouts (2 dimensions) actually needed precision for proper fit. Relaxing the remaining 10 dimensions to ±0.005″ reduced the manufacturing quote from $280 to $165 per unit—40% cost reduction with zero functional impact.
Design Takeaway: Spend 15 minutes auditing your drawing using the process above. Challenge every tight tolerance with the question: “What fails if this varies by ±0.005″?” If the answer is “nothing critical,” relax the specification and invest precision budget where it actually controls assembly or performance.
Will My Tolerances Need Special Fixturing or Multiple Setups?
Parts with tight tolerances on multiple faces typically require custom fixturing, increasing costs 50-100%. Single-face machining with ±0.005″ tolerances uses standard workholding. Multiple faces with ±0.001″ tolerances demand specialized fixtures and datum control.
Quick Part Assessment:
Count Your Tight Tolerance Faces: Print your drawing and count how many surfaces have tolerances tighter than ±0.003″. One face = standard fixturing. Two or more faces = custom fixturing likely needed.
Wall Thickness Check: Thin walls under 3mm with tight tolerances require distributed clamping to prevent deflection. Standard vise pressure will open tolerances beyond specification.
Feature Relationship Review: Do tight tolerances control relationships between features on different faces? Cross-hole alignment, perpendicularity between surfaces, or datum references across multiple operations require specialized fixturing.
Design Changes to Avoid Fixturing:
Consolidate Critical Features: During design reviews, we often recommend moving tight tolerance features to the same face. A medical housing originally requiring four setups was redesigned with access holes, enabling single-setup machining and 60% cost reduction.
Add Machining Access: Sometimes adding a small access hole eliminates the need to machine from multiple sides, avoiding fixture costs entirely while maintaining functionality.
Relax Non-Critical Relationships: Question whether features on opposite faces really need ±0.001″ relationship control, or if ±0.005″ maintains function with standard fixturing.
When Fixturing is Unavoidable: Aerospace components with datum reference requirements, thin-wall enclosures, and precision cross-hole alignments typically justify fixture costs for functional necessity.
Design Takeaway: Review your part and identify faces containing tight tolerances. If possible, orient critical dimensions to enable single-face machining. When multiple faces require precision, budget for custom fixturing and consider design modifications that reduce setup complexity.
How Do You Measure Tolerances Under ±0.001"?
Tolerances under ±0.001″ require coordinate measuring machines (CMM) and add 15-25% to part costs. Standard shop calipers cannot reliably verify precision specifications. Ensure your machine shop has proper measurement capability before specifying tight tolerances.
Measurement Requirements by Tolerance:
- ±0.001″: Requires CMM with climate control. Standard micrometers introduce too much measurement variation for reliable verification.
- ±0.0005″: High-precision CMM with temperature compensation and skilled operators. Not available in all machine shops.
- ±0.0002″: Ultra-precision measurement lab with environmental controls. Often requires third-party certification.
Supplier Qualification Questions:
Before specifying tight tolerances, ask your machine shop: “Do you have CMM capability for ±0.001″ verification?” Many shops can machine precision but lack proper measurement equipment for verification.
Check Environmental Controls: CMM measurement requires temperature-controlled environment. Shops without climate control cannot reliably measure tight tolerances.
Inspection Certification: Medical and aerospace applications often require certified measurement reports. Verify your supplier can provide required documentation.
Drawing Specification Guidance:
Add Measurement Notes: For ±0.001″ tolerances, add “CMM inspection required” to your drawing. This ensures suppliers understand measurement expectations upfront.
Critical Feature Identification: Mark which dimensions need full measurement reports versus quick verification. Not every tight tolerance requires comprehensive documentation.
Budget Planning: Tight tolerance measurement typically adds 15-25% to total part cost through inspection time and equipment requirements.
From our supplier qualification experience, many excellent machine shops can hold ±0.001″ tolerances but lack CMM capability for verification. This creates expensive surprises during project execution when measurement requirements become clear.
Design Takeaway: Verify measurement capability during supplier selection, not after parts are quoted. Add measurement requirements to your drawings and budget accordingly. Consider whether your application truly needs certified measurement or if supplier process control suffices.
Conclusion
Tight tolerance specifications directly impact manufacturing cost, setup complexity, and inspection requirements. Reserve precision tolerances for functionally critical features—typically 10-20% of your dimensions—while using standard ±0.005″ elsewhere to control costs without compromising performance.
Contact us to explore manufacturing solutions tailored to your precision machining requirements.
Frequently Asked Questions
Yes, relaxing non-functional tolerances from ±0.001″ to ±0.005″ typically reduces costs 30-50% without affecting performance. Identify which dimensions don’t control assembly relationships and adjust specifications accordingly during design optimization.
Ask specifically about their measurement capability—many shops can machine tight tolerances but lack CMM equipment for verification. Request capability statements and sample inspection reports before committing to precision specifications.
±0.0005″ tolerances cost 6-8x more than standard work and often require secondary operations like grinding. ±0.001″ provides 4x cost increase but achievable with precision CNC machining. Choose based on actual functional requirements, not safety margins.
Focus tight tolerances on datum features and interfaces between parts. Use tolerance analysis to determine which individual part tolerances can be relaxed while maintaining assembly function. Consider design changes that eliminate critical stackups entirely.
No. Use looser tolerances (±0.005″) during prototyping since design changes are likely. Reserve tight tolerances for final production designs where function is proven and changes are minimal, avoiding rework costs on prototype iterations.
Use ISO 2768-m standard tolerances (±0.1-0.3mm depending on size) for general dimensions. This provides adequate function for most applications while keeping costs reasonable. Only specify tighter tolerances where assembly fit or performance requires precision control.
