Design for Manufacturing (DFM): Making Your Product Producible#
You've defined your requirements. Your design meets every specification. The CAD model is beautiful. Then you send it to manufacturing and hear: "We can't make this," or worse, "We can make it, but it'll cost three times what you budgeted."
This scenario plays out in engineering departments daily. A bracket that should cost $15 ends up at $60 because it requires exotic machining operations. An assembly that should take 10 minutes takes 45 because parts don't align properly. A tolerance stack-up that looked fine on paper creates 30% scrap rate in production.
The difference between designs that work on paper and designs that work in manufacturing is Design for Manufacturing (DFM)—the practice of designing products specifically to optimize them for efficient, cost-effective, and reliable production.
After 17 years developing products across aerospace, automotive, packaging, and heavy equipment, I've seen brilliant designs fail in manufacturing and mediocre concepts succeed because someone understood DFM. This article shares the principles, techniques, and real-world examples that separate producible designs from expensive nightmares.
Let me share a story that captures why DFM matters.
A client came to us with a brake lever assembly for heavy equipment. The original design had been developed by a talented engineer who optimized for strength and aesthetics. The lever arm was a beautiful organic shape machined from billet aluminum, with compound curves that required 5-axis CNC machining. The mounting bracket had tight positional tolerances requiring precision grinding after welding. The fasteners were metric hex-head cap screws in a region where standard socket head cap screws would have worked fine.
First production run cost per assembly: $385. Target cost: $120.
The redesign process took six weeks and involved:
- Changing the lever arm to a bent tube design with end caps (from 5-axis milling to simple tube bending and turning)
- Redesigning the mounting bracket for laser cutting and bending instead of welding and grinding
- Switching to standard fasteners available locally
- Relaxing several unnecessary tolerances
- Consolidating two brackets into a single formed part
Final production cost: $98 per assembly. Annual savings at 500 units/year: $143,500.
The original design met every functional requirement. It was strong, reliable, and worked perfectly. But it was never designed with manufacturing in mind. The $50,000 redesign project (engineering time, new tooling, requalification testing) could have been avoided entirely if DFM principles had been applied from the start.
That's the power—and the importance—of Design for Manufacturing.
Design for Manufacturing is the practice of designing products to optimize the manufacturing process. The goal is to achieve required functionality while minimizing complexity, reducing costs, improving quality, and shortening production time.
A common misconception: DFM means "cheap and dirty" or sacrificing performance for cost. That's backwards.
Good DFM maintains or improves product quality while reducing manufacturing complexity and cost. Often, DFM improvements make products more reliable because simpler designs have fewer failure modes.
Traditional design thinking: "How can I make this work?"
DFM thinking: "How can I make this easy to manufacture?"
This shift happens early in the design process, not as an afterthought. The best time to implement DFM is during conceptual design when you're still choosing approaches, not after detailed CAD models are complete.
Manufacturing cost typically breaks down as:
- Material: 30-50%
- Labor (direct and indirect): 25-40%
- Tooling and setup: 10-20%
- Overhead: 15-25%
DFM improvements can impact all of these. A design change that eliminates one machining operation might save 15 minutes of labor, reduce setup requirements, and eliminate a specialized tool. That 15-minute savings compounds across every unit produced.
Whether you're designing for:
- CNC machining
- Sheet metal fabrication
- Injection molding
- Casting or forging
- Welding and assembly
- Additive manufacturing
- Printed circuit board assembly
Each process has specific DFM guidelines, but the core principles remain consistent: simplicity, standardization, and designing for the process capabilities.
These fundamental principles apply regardless of manufacturing process. Master these, and you'll design more producible products from the start.
Every additional part adds cost through material, handling, assembly time, inventory, and potential failure points.
Guidelines:
- Consolidate parts where possible
- Use multifunctional features (structural parts that also locate or align)
- Consider integral features instead of separate fasteners or brackets
- Evaluate if separate parts truly add value
Example: A three-piece bracket assembly (base plate, mounting ears, fasteners) redesigned as a single formed sheet metal part. Part count: 8 → 1. Assembly time: 12 minutes → 0 minutes.
When not to consolidate: When it increases complexity more than it reduces part count, or when serviceability requires separation.
Exotic manufacturing processes are expensive and limit your supplier base. Standard processes are cheaper, faster, and more widely available.
Guidelines:
- Use common machining operations (drilling, milling, turning)
- Design for standard sheet metal operations (laser cutting, bending, forming)
- Avoid processes that require specialized equipment unless absolutely necessary
- Consider supplier capabilities in your region
Cost impact: A part requiring EDM wire cutting costs 3-5× more than one that can be laser cut or milled.
Custom materials and special fasteners add cost, lead time, and inventory complexity.
Guidelines:
- Select materials readily available from local suppliers
- Use standard stock sizes (plates, tubes, bar stock)
- Specify standard fasteners (hex head, socket head, standard lengths)
- Avoid "almost standard" dimensions that require custom sizes
Example: Specifying 38mm diameter tubing instead of standard 1.5" (38.1mm) requires custom ordering. Lead time: 2 weeks → 12 weeks. Minimum order: 1 length → 100 lengths.
Assembly labor is expensive. Make it fast, foolproof, and forgiving.
Guidelines:
- Self-locating features (chamfers, pilots, pins)
- Symmetrical parts (no "this end up" confusion)
- Minimize fastener types and sizes
- Design for one-way assembly (can't be assembled incorrectly)
- Accessibility for tools (standard wrench/socket clearances)
Cost impact: Reducing assembly time from 45 minutes to 30 minutes saves $8-12 per unit in labor (at $30-45/hour loaded rate).
Every manufacturing process has inherent accuracy, surface finish, and geometric limitations. Designing within these capabilities avoids expensive secondary operations.
Guidelines:
- Understand typical process tolerances (±0.010" for most machining, ±0.030" for laser cut sheet metal)
- Don't specify tighter tolerances than necessary
- Avoid features that require secondary operations unless critical
- Design features that are manufacturable in standard setups
Example: Specifying ±0.002" tolerance on a 4" dimension requires precision grinding or multiple machining operations. ±0.010" can be achieved in one standard machining operation. Cost difference: $25 vs. $8 per part.
Make it difficult to manufacture incorrectly rather than relying on inspection to catch errors.
Guidelines:
- Poka-yoke (error-proofing): Asymmetric features prevent incorrect assembly
- Visual verification: Make critical features visible during assembly
- Minimize quality-critical tight tolerances
- Design for in-process verification rather than final inspection
Example: A connector housing with identical ends was frequently assembled backwards (5% defect rate). Adding a small key feature on one end made incorrect assembly impossible. Defect rate: 5% → 0%.
Exotic features that require specialized equipment drive up costs and limit supplier options.
Guidelines:
- Minimum hole diameters for drilling (typically ≥0.125" diameter for depth >3× diameter)
- Minimum internal radii for sheet metal bending (typically 1× material thickness)
- Maximum tool reach and accessibility
- Standard cutter sizes and geometries
Cost impact: A pocket requiring a 0.100" diameter end mill that's 2" deep requires a custom long-reach tool. Using a 0.125" diameter at 1.5" deep uses standard tooling. Cost: $45 vs. $12 per part.
Real manufacturing has variation. Design to accommodate it rather than fight it.
Guidelines:
- Provide adjustment capability where critical
- Use floating fasteners and slotted holes for alignment
- Design for worst-case tolerance stack-ups
- Build in clearance where fits aren't critical
We'll dive deeper into tolerance analysis in the next section.
Material choice profoundly impacts manufacturing cost, quality, and reliability. The "best" material on paper often isn't the best material for production.
When selecting materials, consider this priority order:
- Meets functional requirements (strength, temperature, corrosion resistance, etc.)
- Standard availability (common alloys, standard stock sizes)
- Process compatibility (can be machined, welded, formed as required)
- Supply chain reliability (multiple suppliers, reasonable lead times)
- Cost (material cost, but also processing cost)
Aluminum 6061-T6:
- Excellent machinability
- Standard availability in all forms (plate, bar, tube, angle, channel)
- Weldable (though strength reduced in heat-affected zone)
- Good strength-to-weight ratio
- Moderate cost
Best for: General purpose structural parts, machined components, welded frames
Steel 1018 (mild steel):
- Easy to machine and weld
- Inexpensive
- Standard availability
- Lower strength than alloy steels
- Requires coating for corrosion protection
Best for: Non-critical structural components, jigs and fixtures, brackets
Steel 4140 (alloy steel):
- Good strength when heat treated
- Excellent machinability in annealed condition
- More expensive than mild steel
- Heat treating adds cost and lead time
Best for: High-stress components, shafts, gears, pins
Stainless steel 304/316:
- Corrosion resistant
- More difficult to machine than carbon steel (requires proper speeds/feeds and sharp tooling)
- Work-hardens during machining
- 2-3× cost of carbon steel
Best for: Food processing, medical, marine, chemical exposure applications
Carbon fiber composites:
- Excellent strength-to-weight ratio
- Expensive material and processing
- Requires specialized manufacturing (layup, curing)
- Difficult to machine
- Limited repairability
Best for: When weight savings justifies cost (aerospace, high-performance automotive)
"Almost standard" dimensions:
Standard: 1" × 4" aluminum flat bar, readily available
Almost standard: 25mm × 100mm aluminum flat bar, requires custom order
The dimensional difference is trivial (1" = 25.4mm), but the cost and lead time difference is significant.
Exotic alloys without justification:
Unless you actually need the specific properties, avoid:
- Titanium (expensive, difficult to machine)
- Inconel and other high-temperature alloys (very expensive, very difficult to machine)
- Exotic aluminum alloys (7075, 2024) when 6061 would suffice
Custom extrusions:
Custom extruded profiles are economical at high volumes (>10,000 pieces) but prohibitively expensive at low volumes. Use standard extrusions or fabricate from flat stock.
Sometimes the "perfect" material creates manufacturing challenges:
Hardness: Harder materials are stronger but harder to machine (increased tool wear, slower speeds, higher cost)
Gumminess: Very soft materials (pure aluminum, copper) gum up cutting tools and create poor surface finish
Brittleness: Brittle materials (cast iron, some plastics) are prone to chipping during machining
Work hardening: Some stainless steels and nickel alloys work-harden during machining, making subsequent operations difficult
Your material choice constrains your process options:
Machining-friendly: Free-machining steels (12L14), brass, aluminum 6061
Welding-friendly: Low-carbon steels, aluminum 6061 (with TIG), stainless 304/316
Forming-friendly: Soft aluminum (3003, 5052), low-carbon steel, copper
Casting-friendly: Gray iron, aluminum A356, bronze
If your design requires both tight machined tolerances and welded construction, this creates a conflict (welding distorts, machining after welding is expensive). Better to either:
- Design for bolted assembly instead of welding, or
- Relax tolerances to accommodate welding distortion, or
- Machine after welding (expensive but sometimes necessary)
Original design: Titanium mounting bracket for aerospace application
- Reason specified: Weight reduction
- Material cost: $180
- Machining cost: $320 (difficult material, carbide tooling)
- Total: $500 per bracket
- Weight: 0.45 kg
Analysis: Stress analysis showed factor of safety = 8.5 (way over-designed)
Redesign: Aluminum 7075-T6 with optimized geometry
- Material cost: $25
- Machining cost: $95
- Total: $120 per bracket
- Weight: 0.52 kg (+0.07 kg or 156 grams)
Result: 76% cost reduction for 15.5% weight increase. At annual volume of 200 brackets, savings = $76,000/year. The 31 kg total weight increase across all units was insignificant in this application.
Before finalizing material choice:
Tolerance stack-ups are where many designs fail in production. Parts that fit perfectly in CAD create assembly nightmares when manufacturing variation is included.
Tolerance: The permissible variation in a dimension
Example: 25.0 ±0.5mm means anywhere from 24.5mm to 25.5mm is acceptable
Tolerance stack-up: How individual part tolerances combine to affect assembly dimensions
Consider a simple assembly: Three plates stacked with fasteners
- Plate A thickness: 10.0 ±0.3mm
- Plate B thickness: 10.0 ±0.3mm
- Plate C thickness: 10.0 ±0.3mm
- Total stack nominal: 30.0mm
Worst-case stack-up:
- Maximum: 10.3 + 10.3 + 10.3 = 30.9mm (+0.9mm variation)
- Minimum: 9.7 + 9.7 + 9.7 = 29.1mm (-0.9mm variation)
If your fastener length is 30.0 ±0.3mm (29.7-30.3mm), you have a problem:
- Minimum fastener (29.7mm) with maximum stack (30.9mm) = doesn't reach
- Maximum fastener (30.3mm) with minimum stack (29.1mm) = protrudes 1.2mm
This is a simplified example, but tolerance stack-ups get complex quickly with multiple parts, multiple dimensions, and different tolerance types.
Worst-case (arithmetic) stack-up:
Sum all maximum tolerances in one direction, all minimum tolerances in the other direction. This assumes all parts are at their extreme limits simultaneously.
Pros: Guarantees 100% assemblies work (if analysis is correct)
Cons: Very conservative, leads to tight tolerances and high costs
Statistical (RSS) stack-up:
Assumes normal distribution of part dimensions and uses root-sum-square calculation. Based on probability that parts will be near nominal, not all at extremes.
Pros: More realistic, allows looser tolerances
Cons: Some percentage of assemblies won't meet spec (typically 0.3% for 3σ limits)
Formula:
Total tolerance = √(T₁² + T₂² + T₃² + ... + Tₙ²)
For our three-plate example using RSS:
Total tolerance = √(0.3² + 0.3² + 0.3²) = √0.27 = ±0.52mm
Much tighter than the ±0.9mm from worst-case analysis.
Use worst-case analysis for:
- Safety-critical assemblies
- Small production runs (can't rely on statistics)
- When failures are very expensive (aerospace, medical)
- Regulatory requirements
Use statistical analysis for:
- High-volume production
- Cost-sensitive designs
- When rework is acceptable for small percentage
- Commercial/industrial products
Step 1: Identify the critical dimension
What dimension determines if the assembly works? Common examples:
- Gap between mating parts
- Total length affecting fit in envelope
- Alignment of bolt holes
- Clearance for moving parts
Step 2: Draw the tolerance chain
Sketch the assembly showing all dimensions that contribute to the critical dimension. This visualizes what adds and what subtracts.
Step 3: List all contributing tolerances
Create a table:
| Part | Dimension | Nominal | Tolerance | Min | Max |
|---|
| Base plate | Thickness | 10.0 | ±0.3 | 9.7 | 10.3 |
| Spacer | Length | 15.0 | ±0.2 | 14.8 | 15.2 |
| Cover | Thickness | 5.0 | ±0.2 | 4.8 | 5.2 |
| Bolt | Length | 32.0 | ±0.3 | 31.7 | 32.3 |
Step 4: Calculate worst-case stack-up
-
Add all maximums: 10.3 + 15.2 + 5.2 = 30.7mm (parts)
-
Maximum bolt: 32.3mm
-
Worst-case gap: 32.3 - 30.7 = 1.6mm (excessive gap, bolt loose)
-
Add all minimums: 9.7 + 14.8 + 4.8 = 29.3mm (parts)
-
Minimum bolt: 31.7mm
-
Worst-case interference: 31.7 - 29.3 = 2.4mm (bolt bottoms out, doesn't clamp)
Step 5: Decide if acceptable
If worst-case stack-up creates problems, you have options:
- Tighten tolerances (expensive)
- Add adjustment capability (shims, slotted holes)
- Use statistical analysis (accept some scrap/rework)
- Redesign to eliminate sensitivity
- Add selective assembly (match parts into groups)
Strategy 1: Minimize the tolerance chain length
Fewer parts in the chain = less accumulated variation
Example: Instead of three plates stacked, use one thicker plate. Tolerance chain: 3 parts → 1 part.
Strategy 2: Design with floating fasteners
Slotted holes or oversized clearance holes accommodate variation in hole positions
Example: Through-holes with ±0.5mm positional tolerance, use clearance holes 2mm oversize. Accommodates ±1mm variation.
Strategy 3: Use datum-based dimensioning
Dimension critical features from a common reference face rather than creating chain dimensions
Bad: Hole A to Hole B: 50±0.2mm, Hole B to Hole C: 50±0.2mm
Good: Hole A to Datum: 50±0.2mm, Hole B to Datum: 100±0.2mm, Hole C to Datum: 150±0.2mm
Total variation in C location: ±0.2mm (not ±0.4mm)
Strategy 4: Build in adjustment
For critical alignments, include adjustment capability:
- Shims for spacing (discrete adjustment)
- Slotted mounting holes (continuous adjustment)
- Threaded adjusters (fine adjustment)
- Eccentric bushings (rotational adjustment)
Strategy 5: Self-locating features
Design features that naturally find correct position regardless of variation:
- Tapered pilot diameters
- Conical seats
- V-blocks for cylindrical parts
- Formed flanges that nest
Default machining tolerances (if nothing specified):
- Linear dimensions: ±0.010" (±0.25mm)
- Hole diameters: +0.003/-0.000" (+0.08/-0.00mm)
- Angular: ±1°
These are achievable with standard machining operations without extraordinary care.
When to tighten tolerances:
- Bearing fits (typically ±0.001-0.002" or tighter)
- Precision alignments (optical, measurement equipment)
- High-speed rotating parts (balance requirements)
- Mating threads (class 3 fits)
- Critical functional gaps
When to relax tolerances:
- Clearance holes for fasteners (±0.030" / ±0.75mm is fine)
- Non-critical dimensions (spacing, overall length not affecting function)
- Rough surfaces or visual-only features
- Structural shapes where strength, not precision, matters
Cost impact of tolerances:
- ±0.010" (0.25mm): Standard machining, low cost
- ±0.005" (0.13mm): Careful machining, moderate cost (+20-30%)
- ±0.002" (0.05mm): Precision machining, high cost (+50-100%)
- ±0.001" (0.025mm): Grinding/precision machining, very high cost (+200-400%)
GD&T provides more precise control than ± tolerances for complex features. It's essential for:
- Mating parts with critical fit requirements
- Parts with datums that establish coordinate systems
- Functional tolerancing (controlling what matters for function)
Common GD&T symbols:
- Position (⌖): Controls location of features
- Flatness (⏤): Controls surface flatness
- Perpendicularity (⊥): Controls angle between features
- Parallelism (‖): Controls parallel relationship
- Concentricity (◎): Controls coaxial relationship
When to use GD&T:
- Complex assemblies with multiple mating interfaces
- High-volume production where tight process control is economical
- Safety-critical assemblies
- When communicating with contract manufacturers
When not to bother:
- Simple parts with few critical dimensions
- Low-volume prototype or custom work
- When your machine shop isn't familiar with GD&T (causes confusion, not clarity)
Problem: Conveyor belt runs off-center, requiring constant adjustment
Analysis: Tolerance stack-up in frame width
- Two 50×50mm square tubes: ±0.75mm each
- Gap nominal: 600mm
- Gap tolerance: ±1.5mm total
- Belt width: 610mm ±5mm
Worst case: Frame gap = 603mm, Belt width = 615mm = 12mm interference
Solution: Redesign with adjustability
- Slotted mounting holes on one side frame
- Allows ±10mm adjustment
- Now accommodates full tolerance range
- One-time setup during installation
For complex assemblies, allocate tolerance budget strategically:
- Calculate total allowable variation in critical dimension
- List all contributing dimensions
- Allocate tighter tolerances where easy/cheap to achieve
- Allocate looser tolerances where tight tolerances are expensive
- Verify total stack-up meets budget
Example: Total gap must be 10.0 ±0.5mm
| Part | Nominal | Standard Tolerance | Cost | Budget Allocation | Final Tolerance |
|---|
| Part A | 25.0mm | ±0.25mm | Low | 40% | ±0.20mm |
| Part B | 15.0mm | ±0.25mm | Low | 40% | ±0.20mm |
| Part C | 30.0mm | ±0.50mm | High | 20% | ±0.10mm |
Check: √(0.20² + 0.20² + 0.10²) = √0.09 = ±0.30mm < 0.50mm budget ✓
Tightening Part C would have been expensive; instead, tighten A and B where it's cheaper.
Each manufacturing process has unique DFM considerations. Here are practical guidelines for common processes.
General rules:
- Minimize setups (every re-fixturing adds cost and accumulates error)
- Use standard tooling (standard drill sizes, end mills)
- Avoid deep pockets (depth > 4× width requires custom long tools)
- Provide tool access and clearance
- Avoid sharp internal corners (use radius = tool radius)
Drilling:
- Minimum hole diameter: 0.125" (3mm) for depth >3× diameter
- Use standard drill sizes (fractional, number, letter sizes)
- Specify drill depth, not through-hole, when possible (allows flat-bottom hole, easier)
- Avoid angled or curved surfaces (use pilot flat)
Milling:
- Inside corner radius = cutter radius (minimum 0.031" / 0.8mm)
- Avoid thin walls (< 0.060" / 1.5mm in aluminum, < 0.040" / 1mm in steel)
- Prefer 2.5D features (constant depth) over 3D sculptured surfaces
- Avoid deep narrow slots (slot width < 3× depth)
Turning:
- Minimize tool changes (profile with single tool if possible)
- Avoid interrupted cuts if possible (cost and tool wear)
- Keep length-to-diameter ratio < 10:1 (or design for steady rest)
- Internal features easier than external features of same complexity
Threading:
- Prefer standard thread sizes and pitches
- Avoid deep threaded holes (>2× diameter is difficult)
- Blind threaded holes need clearance beyond thread (1-2 pitches)
- External threads easier/cheaper than internal threads
General rules:
- Design for standard sheet sizes (4'×8', 5'×10' most common)
- Minimize scrap (nest parts efficiently on sheet)
- Use standard material thicknesses (14ga, 16ga, 18ga, etc.)
- Avoid mixing materials in same assembly (galvanic corrosion, different expansion)
Laser/Plasma/Waterjet cutting:
- Minimum feature size ≈ material thickness
- Minimum hole diameter ≈ 1.5× material thickness
- Avoid tiny tabs and delicate features
- Inside corners have radius (kerf width)
- Design for parts to drop free (no trapped cutouts)
Bending:
- Minimum bend radius = material thickness
- Allow clearance for bending (flange must clear bend)
- Keep holes >4× material thickness from bend line
- Avoid bending over tapped or threaded features
- Consider bend sequence (some bends block access for later bends)
Forming and stamping:
- Design for draw depth limits (< 3× die diameter generally)
- Provide adequate corner radii (3× material thickness minimum)
- Avoid deep narrow ribs or channels
- Consider springback (material returns slightly after forming)
Welding:
- Design for weld access (at least 1" clearance for welding torch)
- Avoid blind welds where quality can't be verified
- Prefer continuous welds over intermittent (faster)
- Design fixtures that maintain alignment during welding
- Allow for welding distortion (±0.030-0.060" / 0.75-1.5mm typical)
- Avoid mixing thin and thick materials (burn-through risk)
General rules:
- Maintain uniform wall thickness (minimize thick-to-thin transitions)
- Provide draft angle (1-3° minimum for part ejection)
- Design for single parting line
- Minimize undercuts (use internal slides/lifters only when necessary)
Wall thickness:
- Typical range: 0.040-0.200" (1-5mm)
- Avoid thick sections (causes sink marks and voids)
- Transition gradually between thicknesses (3:1 ratio max)
Ribs and bosses:
- Rib thickness = 50-70% of wall thickness
- Boss diameter >2× core pin diameter
- Round base of ribs and bosses (reduce stress concentration)
Draft angles:
- Minimum 1° for smooth surfaces
- 2-3° for textured surfaces
- More draft = easier ejection = longer tool life
Undercuts:
- Avoid if possible (add cost and complexity)
- External undercuts: design for hand-loading if low volume
- Internal undercuts: require slides, lifters (expensive)
General rules:
- Provide adequate draft (3-5° for sand casting, 1-3° for die casting)
- Uniform wall thickness where possible
- Fillet all internal corners (reduce stress concentration and improve flow)
- Design parting line location carefully
- Consider machining for critical features
Sand casting:
- Rough surface finish (200-400 μin Ra)
- Generous fillets (R = 0.25-0.50" typical)
- Avoid thin sections (< 0.188" / 5mm in aluminum)
- Expect machining of critical surfaces
Die casting:
- Good surface finish (as-cast often acceptable)
- Thin walls possible (0.040" / 1mm minimum)
- Complex features achievable
- High tooling cost (economical >10,000 pieces)
Investment casting:
- Excellent detail and surface finish
- Complex geometries possible
- Smaller size range (typically < 50 lbs)
- Moderate tooling cost
Design for weld strength:
- Fillet welds stronger in shear than tension
- Size weld to load (bigger is not always better)
- Intermittent welds acceptable for low-stress applications
- Consider fatigue loading (smooth transitions, no stops/starts)
Weld joint design:
- Prefer lap joints over butt joints (easier fit-up)
- Use backing plates for butt welds when practical
- Design for down-hand welding when possible
- Avoid overhead and vertical welding if possible (difficult, lower quality)
Fixture requirements:
- Weld fixtures required for complex assemblies
- Design fixtures early in process
- Include reference surfaces for checking after welding
FDM (Fused Deposition Modeling):
- Layer lines visible (orientation matters for appearance)
- Overhangs >45° require support (removed after printing)
- Hollow parts require drain holes for support removal
- Anisotropic strength (weaker perpendicular to layers)
SLA/SLS (Resin-based):
- Smoother surface finish than FDM
- Better detail resolution
- More expensive material and equipment
- UV-curable resins (consider yellowing over time)
Metal additive (DMLS/SLM):
- Internal features possible (conformal cooling, lightweighting)
- Overhangs require support (difficult to remove from internal features)
- Heat treating often required
- Expensive process (only justified for complex geometry or low volume)
DFM for additive:
- Orient for minimum support requirements
- Design self-supporting features when possible (less than 45° overhang)
- Minimum wall thickness: 0.040" / 1mm for most materials
- Consider post-processing (support removal, surface finishing)
Let me share several real projects where DFM improvements created significant value.
Original design:
- Complex 3D milled bracket from billet aluminum
- Required 5-axis CNC machining
- 8 separate setups for all features
- Machining time: 3.5 hours
- Material cost: $45
- Machining cost: $210
- Total: $255 per bracket
DFM analysis identified:
- Organic curves were aesthetic, not functional
- Multiple pocket depths added complexity
- Some features could be simplified or eliminated
Redesigned with DFM:
- Simplified to 2.5D geometry (constant depths)
- Machined in 3-axis CNC (standard mill)
- 3 setups (reduced from 8)
- Machining time: 1.2 hours
- Material cost: $38 (smaller starting stock)
- Machining cost: $72
- Total: $110 per bracket
Results:
- 57% cost reduction ($145 savings per part)
- Annual savings at 500 units: $72,500
- Lead time reduced from 3 weeks to 5 days
- Qualification testing confirmed equal performance
Original design:
- 5-piece welded bracket assembly
- Laser-cut pieces, complex welding fixture required
- Assembly time: 35 minutes
- Welding caused distortion, required straightening
- Total cost: $88 per assembly
DFM analysis:
- All features could be achieved through bending
- Consolidation possible into single part
Redesign:
- Single laser-cut flat pattern
- 4 bends on press brake
- No welding required
- Assembly time: 0 minutes (it's one part)
- Total cost: $28 per assembly
Results:
- 68% cost reduction
- Eliminated welding distortion issues
- Simplified inventory (1 part instead of 5)
- Improved repeatability (no weld variation)
Original design:
- Machined mounting plate with multiple tapped holes
- All dimensions specified ±0.005" (±0.13mm)
- Surface finish specified 32 μin Ra (polished)
Cost impact:
- Tight tolerances required precision machining
- Surface finish required additional operations
- Cost: $145 per plate
DFM analysis:
- Most dimensions non-critical (only hole pattern mattered)
- Surface finish was aesthetic only
- Actual functional requirement: hole pattern ±0.010" (±0.25mm)
Redesign:
- Relaxed non-critical dimensions to ±0.020" (±0.5mm)
- Hole pattern held at ±0.010" (±0.25mm) via GD&T
- Surface finish relaxed to 125 μin Ra (standard machined)
- Cost: $52 per plate
Results:
- 64% cost reduction
- Maintained all functional requirements
- Easier quality inspection (standard measuring tools)
- Shorter lead times (less machine time)
Original design:
- Assembly used 7 different fastener types
- Metric and imperial mixed
- Socket head, button head, and hex head cap screws
- Various lengths: 12mm, 16mm, 20mm, 25mm, 1", 1.25"
- Total fastener cost: $6.40 per assembly
DFM analysis:
- No functional reason for variety
- Inventory complexity, assembly confusion
- Opportunity to standardize
Redesign:
- Consolidated to 2 fastener types (M6×20mm and M8×25mm)
- All socket head cap screws (unified drive type)
- Bulk pricing on high-volume fasteners
- Fastener cost: $1.85 per assembly
Results:
- 71% fastener cost reduction
- Reduced inventory SKUs (7 → 2)
- Faster assembly (no fastener confusion)
- Fewer assembly errors
Original design:
- Stainless steel 316 plate for equipment base
- Specified for corrosion resistance
- Material cost: $240
- Machining cost: $180 (stainless is tough on tooling)
- Total: $420 per base
DFM analysis:
- Application was indoor, climate-controlled
- Corrosion resistance was overkill
- Occasional washdown with mild detergent
Redesign:
- Changed to carbon steel with powder coat finish
- Material cost: $45
- Machining cost: $85 (easier to machine)
- Powder coating: $35
- Total: $165 per base
Results:
- 61% cost reduction
- Faster machining (carbon steel cuts easier)
- Equal corrosion protection for this application
- Aesthetic improvement (powder coat vs. bare stainless)
Original design:
- Pocket required 0.325" diameter end mill
- Pocket depth: 0.850"
- Custom tool required (standard sizes are 0.250", 0.375")
- Cost: $68 per part
DFM analysis:
- Pocket width was arbitrary (no functional requirement)
- Could be redesigned to use standard tooling
Redesign:
- Changed pocket width to 0.375" (standard 3/8" end mill)
- Adjusted depth to 0.750" (easier standard tool length)
- Cost: $24 per part
Results:
- 65% cost reduction
- Eliminated custom tooling cost
- Faster machining (standard tool more aggressive cutting)
- Improved availability (any shop has 3/8" end mills)
Notice the common themes:
- Simplification: Remove complexity that doesn't add value
- Standardization: Use standard materials, processes, hardware
- Consolidation: Fewer parts = lower cost and better reliability
- Tolerance relaxation: Only specify tight tolerances where critical
- Process selection: Choose processes suited to the design
These aren't one-time redesigns. Applying DFM principles from the start avoids these issues entirely.
DFM should be embedded throughout design, not a late-stage gate. Here's how to implement it effectively.
Timing: During concept development, before detailed CAD
Participants: Design engineer, manufacturing engineer, procurement
Duration: 1-2 hours
Focus questions:
- What manufacturing processes will be required?
- Are there process alternatives to consider?
- What are the high-cost drivers?
- Can we consolidate parts or assemblies?
- Are we using standard materials and hardware?
- What are the critical tolerances and how will we achieve them?
Outcome: Process selection decisions, part count targets, material selection
Value: Changes at concept phase cost hours of engineering time. Changes after detailed design cost weeks.
Timing: After detailed CAD but before ordering tooling or materials
Participants: Design engineer, manufacturing engineer, quality engineer, shop floor expertise
Duration: 2-4 hours for complex assemblies
Review process:
-
Part-by-part review:
- Can this be manufactured as designed?
- What's the most expensive operation?
- Can any features be eliminated or simplified?
- Are tolerances appropriate?
-
Assembly review:
- Are parts easy to locate and align?
- Is assembly sequence logical?
- Are there error-proofing features?
- Can assembly be done with standard tools?
-
Tolerance stack-up review:
- Verify critical dimensions
- Check worst-case scenarios
- Identify if adjustment provisions needed
-
Manufacturability scoring:
Rate each design aspect (1-5 scale):
- Part count (fewer = better)
- Material standardization
- Process complexity
- Tolerance appropriateness
- Assembly ease
- Tooling requirements
Outcome: Action items list with cost/benefit for each potential change
Value: Catches expensive features before any money is spent on production
After production starts, capture lessons learned:
- What went smoothly?
- What was more difficult/expensive than expected?
- What design changes would have helped?
- What should we do differently next time?
Document these in a design guidelines database. Build institutional knowledge that prevents repeating mistakes.
Download this checklist to use in your reviews:
General Design:
Tolerances:
Assembly:
Machining:
Sheet Metal:
Castings/Moldings:
Materials:
Cost Drivers:
Even experienced engineers fall into these traps. Awareness is the first step to avoiding them.
The problem: Specifying ±0.005" on dimensions that could be ±0.020" without affecting function
Why it happens:
- CAD default tolerances
- "Better safe than sorry" mentality
- Copying tolerances from similar parts without thinking
How to avoid it:
- Ask: "What happens if this dimension is off by ±0.020?"
- If answer is "nothing bad," relax the tolerance
- Only specify tight tolerances on critical functional features
- Use tolerance analysis to determine what's actually needed
Cost impact: A dimension that requires ±0.005" instead of ±0.020" might double machining time
The problem: Designing a feature that's difficult or impossible to manufacture with available processes
Examples:
- Sharp internal corners (can't be milled)
- Blind threaded holes too deep (tap will break)
- Undercuts in molded parts (require slides)
- Welds in inaccessible locations
How to avoid it:
- Learn basic manufacturing process capabilities
- Consult with manufacturing engineers early
- Visit the shop floor and watch parts being made
- Ask "how would I make this?" before finalizing design
The problem: Mixing metric and imperial dimensions, fasteners, and tolerances
Why it's bad:
- Assembly confusion and errors
- Inventory complexity (metric and imperial tools, fasteners)
- Potential for cross-threading or wrong hardware
- Quality inspection complexity
How to avoid it:
- Choose one system (metric or imperial) and stick with it
- If inherited mixed design, standardize during redesign
- Clearly mark any exceptions and why they exist
The problem: Designing parts that can't be assembled in practice
Examples:
- Fasteners that can't be accessed with tools
- Parts that must be assembled in impossible order
- Welds that block access for later welds
- No clearance for hands/tools during assembly
How to avoid it:
- Physically mock up assembly sequence with cardboard or foam
- Walk through assembly step-by-step
- Leave clearance for tools (minimum 1" for wrenches, 2" for power tools)
- Design for one-way assembly when possible
The problem: Adding complexity for aesthetics without considering cost
Examples:
- Compound curves requiring 5-axis machining
- Intricate patterns that serve no functional purpose
- Polished finishes on hidden surfaces
- Chamfers and fillets on every edge
How to avoid it:
- Distinguish between visible and hidden surfaces
- Ask if aesthetic features add value proportional to cost
- Consider alternatives (powder coat can cover rough surfaces)
- Reserve expensive features for customer-facing surfaces only
The problem: Designing around a component available from only one supplier
Why it's risky:
- Supply chain vulnerability
- No price competition
- Long lead times if supplier has issues
- Difficult to scale production
How to avoid it:
- Prefer standard components with multiple suppliers
- If custom component required, specify performance, not specific part
- Qualify second source during development
- Design with interchange ability in mind
The problem: Missing or unclear manufacturing information on drawings
Examples:
- Critical dimensions not called out
- No welding symbols or specifications
- Surface finish not specified
- Heat treat or coating requirements not documented
How to avoid it:
- Use complete drawing standards (ASME Y14.5)
- Include all manufacturing notes
- Reference applicable specifications
- Review drawings from manufacturer's perspective
The problem: Not knowing if design changes save or cost money
Why it happens:
- No early manufacturing quotes
- No cost modeling during design
- "Design now, cost later" mentality
How to avoid it:
- Get rough quotes on concept alternatives before detailed design
- Build cost models (estimate machining time, material cost, assembly time)
- Track cost impact of design decisions
- Budget-driven design (design to cost target)
DFM is important, but it's not the only consideration. Sometimes you need to compromise DFM for other priorities.
If your product absolutely requires a feature that's difficult to manufacture, and no alternatives meet performance requirements, you manufacture the difficult feature.
Examples:
- Aerospace parts where weight savings justify complex machining
- High-performance equipment where strength requires exotic materials
- Precision instruments where tolerances can't be relaxed
Guidelines:
- Exhaust all alternatives before accepting difficult manufacturing
- Cost-justify the performance requirement (is it truly necessary?)
- Contain complexity to specific components (keep rest of design simple)
- Document why the complexity is required (prevents future "why did we do this?" questions)
Regulatory compliance sometimes forces design choices that violate DFM principles.
Examples:
- FDA requirements for material traceability and documentation
- UL/CSA requirements for specific clearances and materials
- Pressure vessel codes requiring specific weld procedures
- Aerospace requirements for specific processes and materials
Guidelines:
- Understand requirements thoroughly (don't over-interpret)
- Apply DFM within regulatory constraints
- Look for approved alternatives that are more manufacturable
- Work with regulatory experts to find compliant solutions
Protecting intellectual property sometimes requires design choices that add manufacturing complexity.
Example: Using specific geometric features that define patent claims, even if harder to manufacture
Guidelines:
- Balance IP protection value against manufacturing cost
- Consider trade secret protection vs. patents (sometimes hiding is better than publishing)
- Focus patentable features on truly innovative aspects
- Keep non-critical features simple and manufacturable
At very low volumes (prototypes, custom one-offs), manual processes might be more economical than DFM-optimized designs.
Examples:
- Prototype tolerances can be hand-fitted rather than designed for automatic assembly
- Custom one-off fixtures can be welded table setup rather than dedicated fixture
- Small quantity parts can be waterjet cut rather than stamped (no tooling cost)
Guidelines:
- Be explicit about volume assumptions ("this design is optimized for < 10 units")
- Plan transition to DFM-optimized design if volume increases
- Don't sacrifice function for DFM at prototype stage
- Do capture lessons learned for volume production redesign
When considering whether to compromise DFM, ask:
- What's the cost impact of the non-DFM approach?
- What's the benefit (performance, compliance, etc.)?
- What's the production volume?
- What's the product lifetime?
Calculate total program cost:
Total cost = NRE (design, tooling) + (unit cost × volume)
Example:
Option A (DFM-optimized): $20,000 NRE + ($50/unit × 1,000 units) = $70,000 total
Option B (complex design): $15,000 NRE + ($95/unit × 1,000 units) = $110,000 total
Decision: Option A worth the extra $5,000 in NRE for $40,000 total savings
But if volume is 100 units:
Option A: $20,000 + ($50 × 100) = $25,000 total
Option B: $15,000 + ($95 × 100) = $24,500 total
Decision: Option B is better at low volume
Use these resources to implement DFM in your projects.
Before starting detailed design:
During CAD modeling:
Before releasing for manufacturing:
Early-stage cost models:
Create simple spreadsheet models:
- Material cost: volume × material density × $/kg
- Machining time: surface area × feed rate = time
- Assembly time: fastener count × time/fastener
- Setup costs: number of operations × $/setup
These rough estimates guide design decisions.
Supplier quotes:
- Get quotes on concept alternatives before detailed design
- Use quick-turn prototype quotes to validate cost models
- Build relationships with suppliers who provide design feedback
DFM software:
Commercial tools analyze CAD models for manufacturability:
- aPriori: Comprehensive cost modeling and DFM analysis
- DFMPro: SolidWorks add-in for manufacturing checks
- Protolabs/Xometry: Online quoting with DFM feedback
These are valuable for high-volume production but may be overkill for small runs.
Keep these resources handy:
Standard tolerances by process:
| Process | Typical Tolerance |
|---|
| Machining | ±0.010" (±0.25mm) |
| Sheet metal | ±0.030" (±0.75mm) |
| Casting | ±0.030" (±0.75mm) |
| Molding | ±0.005" (±0.13mm) |
| Welding | ±0.060" (±1.5mm) |
Standard hardware databases:
- McMaster-Carr catalog (de facto industry standard)
- Grainger industrial supply
- Fastenal engineering tools
Material property databases:
- MatWeb (www.matweb.com (opens in new tab))
- ASM Handbook
- Supplier data sheets
Manufacturing process guides:
- Machinery's Handbook (comprehensive manufacturing reference)
- GD&T standards (ASME Y14.5)
- Welding standards (AWS)
- Sheet metal handbooks (Fabricator's and Welder's Handbook)
You've applied DFM principles to your design. Now what?
Even with excellent DFM, you'll learn from building prototypes:
-
First prototype: Proof of concept, test basic function
- Expect to find assembly issues, interference, tolerance problems
- Document everything that was difficult or didn't work
-
Refined prototype: Incorporate DFM lessons learned
- Fix the issues from first prototype
- Verify improved manufacturability
- Test with production-intent processes where possible
-
Pre-production prototype: Final validation
- Build with production tooling and processes
- Verify assembly procedures and documentation
- Train production staff
With DFM-optimized design and proven prototypes:
- Supplier selection: Choose manufacturers with process capability for your design
- Work instructions: Document assembly sequence and critical checkpoints
- Quality plans: Define inspection points and acceptance criteria
- Continuous improvement: Capture production feedback, iterate design
This article covered making your design producible. The next article tackles how to actually build your first prototypes: "Prototype Strategies: When to 3D Print vs. Machine."
We'll cover:
- Comparison of rapid prototyping technologies
- Cost-benefit analysis by project stage
- Material property considerations
- Hybrid approaches for complex prototypes
If you're facing manufacturing challenges with your design, we can help:
- DFM reviews: We'll review your design and identify opportunities for cost reduction
- Tolerance analysis: Verify your designs will assemble reliably
- Process selection: Recommend optimal manufacturing processes for your application
- Supplier identification: Connect you with qualified manufacturers
Our experience across aerospace, automotive, packaging, and heavy equipment means we've seen most manufacturing challenges and know how to address them.
Contact us to discuss your project and how we can help you develop producible designs that meet your requirements while minimizing cost.
Design for Manufacturing isn't about compromising your vision—it's about achieving your vision in a way that's practical, economical, and scalable.
The best product designs are invisible. They work beautifully, they're reliable, and no one thinks about how difficult (or easy) they were to manufacture. That invisibility comes from applying DFM principles from the start.
Every tolerance you specify, every material you select, every part you add creates consequences downstream. DFM is about making those decisions consciously, understanding the trade-offs, and designing products that work both on paper and in production.
The examples in this article show savings of 50-70% are common when DFM principles are applied. But the benefits go beyond cost: faster production, higher quality, fewer suppliers, simpler inventory, easier maintenance. These compound over the product's lifetime.
Start applying DFM on your next project. Your manufacturing team will thank you. Your budget will thank you. And your customers will benefit from a better product at a better price.
Ready to optimize your designs for manufacturing? Let's discuss your project and identify opportunities to improve producibility while maintaining performance.
