Design For Manufacturing Considerations DFM & DFMA
See - Engineering Design for Manufacturing (Book) for extended details and concepts.
Successful mechanical design and engineering is environment and process dependent. There are many factors that affect the design. The following are major factors:
1) Product scope, intent and complexity
2) Time to market
4) Product Competitive Environment
5) Organization infrastructure
6) Design, engineering and manufacturing tools
7) Staff experience
General Design Guidelines
Practice the "KIS" principle, (Keep It Simple)
For each assembly component, there is opportunity for a defective component and an assembly challenge. As the number of parts goes up, the total cost of fabricating and assembling the product goes up. Tolerance accumulation becomes more significant and may require additional design and manufacturing to produce an acceptable assembly. Additionally, creating design documents and manufacturing processes are additive, resulting in a more expensive product due to NRE (Non-recurring Engineering) and manufacturing costs. Costs related to purchasing, stocking, and general infrastructure also go down as the number of components is reduced. Inventory levels are reduced with fewer components. As the product structure and required operations are simplified, fewer fabrication and assembly steps are required, manufacturing processes and lead-times are reduced. The designer, engineer's and manufacturing should concurrently review all components within an assembly to determine whether components can be eliminated, combined with another component, or the function can be performed in a simpler way.
Design using "off the shelf" standard or OEM components to simplify design and manufacturing activities, to minimize the amount and diversity of inventories, and to standardize handling and assembly operations. Standard components will result in reduced NRE costs and higher quality. Standard component design charts can be used resulting in efficient design, PM&P activities and manufacturing tool inventories. Manufacturing education is simplified and automation as the result of operation standardization can be designed and implemented.
Design for ease of fabrication and assembly. Select processes compatible with the design intent, materials and production volumes. Select materials compatible with production processes and that minimize processing time while meeting functional requirements. Avoid unnecessary part features because they involve extra processing effort and/or more complex tooling.
Consider the following design guidelines:
- For higher volume parts, consider castings, extrusions or other volume manufacturing processes to reduce machining and inmachine time
- Consult with manufacturing to determine and design for solid mounting or other fixture-locating features on the component.
- Avoid thin walls, thin webs, or similar features that will result in distortions due to manufacturing
- Avoid undercuts that will require special operations & tools
- Design around standard cutters, drill bit sizes or other tools
- Avoid small holes and threaded features as tool breakage and part scrap increases
- Design for full thread depth. Usually 1.5 x major diameter provides adequate holding strength
- Drilled hole depth (to the sharp point of the tool) is recommended to be at least equal to the full thread plus major diameter, but never less than .050"
- Material thickness as measured from the bottom of the drilled hole to next surface should not be less than the major diameter of the thread or diameter of hole, and not less than .050".
- When material thickness allows, thru holes are preferred
Fixture/tooling material selection
When designing steel fixtures or tooling where high accuracy flatness, perpendicularity, parallelism or true position is required, specify the material as low carbon hot rolled. This material is very stable and will retain form much better than CRS (Cold Rolled Steel).
Flatness should be applied with reasonable overall form tolerance as well as on a per unit basis as a means to prevent abrupt surface variation within a relatively small area of the feature. Depending on material thickness and application, a note can be added to design drawing: "FLATNESS MAY BE MEASURED WITH COMPONENT IN RESTRAINED CONDITION". Where applicable, note should include specific retraining requirements
- Always specify largest radius possible. Small diameter tools add significant cost to manufacturing process.
- When design requires metalized plating such as nickel, silver or other, specify a CR "Controlled Radius" as applicable (CNC manufacturing). CAD model or design for non-standard radii. CNC machining will create a "hard corner" in that the machine will race to a radius corner and abruptly change onto the next direction. The CNC change of direction often creates "tool chatter" resulting in rough sharp edges at the radius corner. Non-standard or CR (Controlled Radius) will result in the CNC cutter to slow down and blend a smooth radius at the corner feature. The smooth radius feature will facilitate good metalized plating and avoid flaking common to small sharp edges.
- When depth exceeds 5 X the diameter of the pocket radii, consult manufacturing on alternative fabrication methods. Depths of up to 10 X are possible when machining aluminum but, not all manufacturing facilities have capability
- For deep sharp corner cutouts that require broaching or EDM, specify radii max at all cutout corners i.e. (4X R .008 MAX)
Dimensional Tolerancing Specification and GD&T
Where specific fits and function are required, utilize industry standard dimensioning and tolernacing standard such ASME Y14.5-2009 Geometric Dimensioning and Tolerancing GD&T.
For surface composite curves such as, internal pockets, or other profiles that for CNC manufacturing a continuous cutting path will be established and manufactured. Design for and specify unilateral tolerances (+/- .010). Reason: Often the machine tools used to manufacture the components utilize a feature called "Cutter Compensation". This allows size control variation of the features being machined without having to control the NC program (file) to an exact match with the cutter diameter. For a continuous path, if "X" dimension has +0, -.005 and "Y" dimension has +.005, -0 tolerance specified, the cutter compensation cannot be used to control size, because adding or subtracting from cutter path input automatically invokes an error to the dimension of the other toleranced continuous path surface. Simply, a offset is input into the machine relative to the cutting tool to manufacture for mid tolerance of surface "X" at -.0025 however, this path is not compatible with the "y" surface in that the nominal offset is .0025 out of tolerance.
Design of tolerances should be within manufacturing capabilities.
Concurrently designing for manufacturing will greatly improve product quality and reduce fabrication costs. Consult with manufacturing early in the design process. After completion of preliminary drawings, meet with manufacturing and review design intent, requirements and determine manufacturing process requirements. Manufacturing should review tolerances and determine process capabilities to meet dimensional limits. Manufacturing should identify tolerance challenges that require design and requirements review. In general, design should avoid unnecessarily tight tolerances that are beyond the natural capability of the manufacturing processes. Determine when new production process capabilities are needed early to allow sufficient time to determine optimal process parameters and establish a controlled process. Tolerance stack-ups should be considered on mating parts. Overall assembly tolerances should be calculated, and interface as well as clearance requirements understood. Surface finish requirements can be established based on actual manufacturing processes employed however, surface finish requirements should be understood and design intent accurately defined.
Simplify design and assembly so that the assembly process is unambiguous. Components should be designed so that they can only be assembled in one way; they cannot be reversed. Roll pins, dowel pins or offset mounting holes can be employed.
Design for components orientation and handling to minimize non-value-added manual effort, ambiguity or difficulty in orienting and merging parts. Basic principles to facilitate parts handling and orienting are:
- Parts must be designed to consistently orient themselves. Examples are dowel pins.
- Product design must avoid parts that can become tangled, wedged or disoriented.
- Verify clearance for assembly tooling such as hand tools and fixtures.
- With hidden features that require a particular orientation, provide an external feature, guide surface or design alignment fixturing or tooling to correctly orient the part.
- Design in fasteners large enough that are easy to handle and install
Design for efficient joining and fastening.
Threaded fasteners (screws, bolts, nuts and washers) can be time-consuming to assemble. Consider design alternatives that will reduce fastener count. Use uniform screw sizes here practical.