2: DFM Guidelines for Specific Manufacturing Processes

Injection Molding

Injection molding is a high-volume process for producing precise plastic parts by injecting molten material into a mold. DFM considerations include:

• Uniform Wall Thickness: Maintain consistent wall thickness (typically 1–3 mm) to ensure even cooling and prevent warping or sink marks. Avoid abrupt transitions; use gradual tapers if thickness changes are necessary.
  • Example: A phone case with uniform 2 mm walls cools evenly, while a design with a 1 mm wall next to a 4 mm rib risks visible defects.
• Draft Angles: Add a taper (1–2° per side) to vertical walls to facilitate part ejection from the mold without damage.
  • Pitfall: A vertical wall with no draft may stick, requiring costly mold modifications.
• Ribs and Bosses: Use ribs (50–60% of wall thickness) for stiffness instead of thick sections. Design bosses (e.g., for screws) with sufficient wall support to avoid sink marks.
• Avoid Sharp Corners: Incorporate fillets (minimum radius 0.5 mm) to reduce stress concentrations and improve mold flow.
• Gate and Parting Line Placement: Position gates (material entry points) in non-visible areas and align parting lines to minimize secondary finishing.
  • Example: A toy car’s gate on the underside avoids visible seams on the body.

Casting

Casting involves pouring molten material (metal or plastic) into a mold to form complex shapes. DFM guidelines vary by type (e.g., sand casting, die casting), but common principles include:

• Draft Angles: Similar to injection molding, include draft (1–3° for sand casting, 0.5–2° for die casting) to ease mold removal.
• Uniform Sections: Avoid large variations in thickness to prevent uneven cooling, shrinkage, or porosity.
  • Example: A cast iron pulley with consistent 10 mm walls cools uniformly, while a design with a 5 mm hub and 20 mm rim risks internal voids.
• Fillets and Radii: Use generous radii (3–5 mm) at corners to improve material flow and reduce stress concentrations.
• Risers and Feeders: Design with adequate material reservoirs to compensate for shrinkage during solidification, consulting with foundry engineers for placement.
• Parting Line Simplicity: Minimize complex parting lines to reduce mold costs and machining needs.
  • Pitfall: A convoluted parting line on a gearbox housing increases tooling complexity and cost.

Sheet Metal Fabrication

Sheet metal fabrication involves cutting, bending, and assembling thin metal sheets. DFM focuses on optimizing bends and features:

• Consistent Bend Radius: Use a uniform bend radius (typically equal to sheet thickness, e.g., 1 mm for 1 mm thick steel) to avoid cracking or distortion.
  • Example: A bracket with a 2 mm radius on 2 mm steel bends cleanly, while a 0.5 mm radius risks tearing.
• Minimum Bend Distance: Place holes or cutouts at least 2–3 times the sheet thickness from bend lines to prevent deformation.
• Flange Length: Ensure flanges are at least 4 times the sheet thickness to maintain structural integrity during bending.
• Relief Notches: Add small notches at bend intersections to prevent tearing when multiple bends meet.
  • Pitfall: A sheet metal box with holes 1 mm from a bend distorts during forming.
• Standard Tooling: Design features compatible with standard punch and die sizes to avoid custom tooling costs.

Welding

Welding joins metal parts using heat and/or pressure, and DFM aims to simplify the process and ensure strong joints:

• Minimize Welds: Reduce the number of welds by combining features into single parts (e.g., via casting or bending) to lower labor and inspection costs.
  • Example: A frame with two bent sheet metal parts replaces a four-piece welded assembly.
• Joint Accessibility: Design weld joints to be easily reached by welding equipment, avoiding tight corners or deep recesses.
• Consistent Material Thickness: Match thicknesses at joints to prevent burn-through or weak bonds; step transitions gradually if needed.
• Weld Type Selection: Specify welds (e.g., fillet, butt) based on load requirements and ease of application. Fillet welds are simpler than full-penetration welds.
  • Pitfall: A thin 1 mm sheet welded to a 5 mm plate risks overheating the thinner section.
• Tolerances: Allow for weld shrinkage (typically 1–2% of length) in the design to avoid post-weld machining.

EDM Machining (Electrical Discharge Machining)

EDM works on the principles of thermal erosion and vaporization. By sparking electricity from the electrode to the machining surface, EDM devices are able to erode and vaporize metal which is then removed from the area using a dielectric fluid.

CNC Machining

CNC machining uses computer-controlled tools to remove material from a solid block. DFM optimizes for tool access and material efficiency:

• Tool Geometry: Design features with radii matching standard end mill sizes (e.g., 3 mm, 6 mm) to avoid custom tools. Minimum internal corner radius should be 1/3 of the feature depth.
  • Example: A pocket with a 4 mm radius matches a common 8 mm end mill, reducing setup time.
• Avoid Deep Features: Limit pocket depths to 3–4 times the tool diameter to maintain rigidity and avoid chatter.
• Tool Access: Ensure all surfaces are reachable without repositioning the workpiece (minimize setups), favoring 3-axis over 5-axis machining when possible.
  • Pitfall: A deep, narrow slot requiring a 5-axis machine increases cost versus a wider, shallower redesign.
• Tolerances: Specify tolerances achievable with standard machining e.g., ±0.1 mm (±0.004”) unless tighter precision is critical, as ±0.01 mm (±0.0004”) tolerances double costs.
• Material Removal: Minimize excess stock removal by starting with near-net-shape blanks (e.g., castings) rather than oversized blocks.