Non-Negotiable Design Elements

• Internal corner radii: All internal corners MUST have a radius (minimum 1.5mm or 1/16")
• Tool access: Every feature must be accessible by standard tooling
• Hole depth limitations: Maximum hole depth cannot exceed 10x diameter
• Draft angles: Deep pockets (>4x width) require minimum 3° draft angles
• Minimum machinable feature: 0.8mm (0.032") for metals, 1.5mm (0.060") for plastics
• Maximum depth-to-width ratio: 4:1 for blind pockets, slots, and channels
• Thread depth limitation: No threads deeper than 3x diameter for blind holes
• Fixturing allowance: Parts must have adequate surfaces for workholding

Physical Manufacturing Constraints

• Maximum part dimensions: Based on machine envelope (typically 1000mm x 500mm x 250mm)
• Minimum corner radius equals tool radius: Interior corners cannot be sharper than the tool used
• Surface accessibility: All surfaces must be accessible from at least one approach direction
• No sharp internal edges: All internal edges must have fillets
• Hole bottom form: Blind holes will have conical bottoms from drill point (118° typical)
• Machine tolerance limitations: Standard tolerance of ±0.125mm (±0.005"), tighter tolerances may require secondary processes

Essential Design for High-Performance Applications

• Thin wall vibration: Walls thinner than 1mm will vibrate during machining, compromising accuracy
• Chip evacuation paths: Design must allow for chip evacuation during deep pocket machining
• Datum structure: Include primary, secondary, and tertiary datum surfaces for precision alignment
• Tool deflection compensation: Deep features require tapered walls (0.5-1°) to account for tool deflection
• Balanced material removal: Design symmetrical features to prevent uneven stress distribution
• Constant tool engagement: Avoid designs requiring sudden changes in tool engagement
• Residual stress management: Consider machining sequence to balance internal stresses

Material Selection

• Consider machinability: Materials like aluminum 6061-T6, brass, and some plastics (ABS, Delrin) are easier to machine than stainless steel or titanium
• Material properties: Select materials based on required strength, weight, temperature resistance, and chemical compatibility
• Cost efficiency: Standard materials are more cost-effective than exotic alloys

Wall Thickness

• Minimum thickness for metals: 0.8mm (0.032") minimum, 1.5mm (0.060") recommended
• Minimum thickness for plastics: 1.5mm (0.060") minimum, 2.5mm (0.100") recommended
• Uniform thickness: Maintain consistent wall thickness when possible
• Avoid thin walls: Thin walls flex during machining, causing dimensional inaccuracies

Corner Radii

• Interior corners: Always include radii (minimum 1.5mm or 1/16")
• Avoid sharp internal corners: Square internal corners require additional operations
• Exterior corners: Can be sharp but consider adding small radii (0.5mm) to prevent burrs

Hole Design

• Minimum diameter: Should be at least 1/3 of material thickness
• Recommended minimum: 1.5mm (0.060") for metals, 2.5mm (0.100") for plastics
• Maximum depth: Limit hole depth to 4x diameter for precision
• Standard sizing: Use standard drill sizes when possible
• Hole spacing: Keep at least 1x material thickness between holes

Tolerances

• Standard tolerances: ±0.125mm (±0.005") for CNC milling
• Tighter tolerances: Increase cost significantly, specify only where necessary
• Surface finish: Ra 3.2μm (125μin) is standard, finer finishes increase cost

Pockets and Cavities

• Minimum corner radius: Equal to the smallest end mill radius (typically 1.5mm or 1/16")
• Maximum depth: Limit to 4x width for rectangular pockets
• Floor radius: Design with a floor radius when possible for better tool life
• Avoid narrow, deep pockets: Hard to machine and may require specialized tooling

Threads

• External vs. internal: External threads are easier to machine than internal
• Standard threads: Use standard thread specifications (ISO, UNC, UNF)
• Minimum size for internal threads: M3 or #4-40 minimum
• Minimum size for external threads: M2 or #2-56 minimum
• Thread depth: 1.5x diameter maximum for blind holes

Slots and Grooves

• Minimum width: Equal to the smallest end mill diameter (typically 1.5mm or 1/16")
• Maximum depth: 3x slot width for stability
• T-slots and dovetails: Require special tooling, increase costs

Text and Markings

• Raised text: Easier than engraved text
• Minimum text height: 1.5mm (0.060") for legibility
• Font style: Sans-serif fonts with consistent line thickness work best
• Line width: Minimum 0.5mm (0.020") for engraved lines

Deep Features

• Deep pockets, holes, or cavities exceeding 4x tool diameter increase machining time and risk of tool breakage
• Design parts to be machined from both sides when possible

Inaccessible Features

• Ensure all features can be reached by standard tooling
• Consider tool length-to-diameter ratio limitations
• Design for standard 3-axis or 3+2 axis machining when possible

Insufficient Draft Angles

• Include 3-5° draft angles for deep pockets
• Helps with tool access and part removal

Unnecessary Precision

• Specify tight tolerances only where functionally required
• Overly precise dimensions increase cost without adding value

Thin Sections

• Avoid thin webs or sections that might vibrate or deform during machining
• Minimum web thickness should be at least 1/3 of its height

Simplify Geometry

• Minimize the number of setups required
• Design for standard tooling and processes
• Combine features when possible

Standard Features

• Use standard hole sizes, threads, and slot dimensions
• Avoid custom or non-standard dimensions

Optimize for Standard Stock

• Design parts to fit within standard material stock sizes
• Consider nested part layouts for efficient material usage

Surface Finishing

• Specify critical surfaces only
• Use as-machined finish where acceptable

Preferred File Formats

• STEP, STP, IGES, X_T (Parasolid)
• Include both native CAD and neutral formats when possible

Model Requirements

• Submit fully defined 3D models
• Ensure all features are properly modeled
• Include thread callouts in annotations

Drawing Requirements

• Include dimensions and tolerances
• Specify critical dimensions
• Note any special requirements or finishes

Aluminum

• Excellent machinability
• Good strength-to-weight ratio
• Standard tolerances easily achieved
• Thin walls down to 0.8mm possible

Steel

• Requires slower cutting speeds
• Heat treatment considerations
• Minimum 1mm wall thickness recommended
• Greater tool wear than aluminum

Plastics

• Thermal expansion considerations
• Heat sensitivity during machining
• Typically require thicker walls than metals
• May flex during machining

Aerospace Applications

Defense Industry Requirements

Robotics Industry Specifics

5-Axis Machining Opportunities

• Complex geometries: Design for single-setup machining where possible
• Undercut features: Utilize 5-axis capabilities for features unreachable with 3-axis
• Tool orientation optimization: Design to avoid extreme tool angles