As a full turnkey EMS provider, OCM provides complete system or sub-system assembly – otherwise known as box-build service. This DFM Tip is based on our experience providing box-build services across a wide range of low-volume products. It provides best practices – and reasons for them – related to design considerations that are specific to metal and mechanical sub-assemblies.
General Best Practices
Engineers and designers can follow these general guidelines to reduce the risk of unforeseen manufacturing expenses.
- For higher-volume parts, consider castings, extrusions or other volume manufacturing processes to reduce machining and in–machine time
- Consult with manufacturing/your EMS provider to determine and design for solid mounting or other fixture-locating features on the component
- Design around standard cutters, drill bit sizes or other tools
- Thin walls, thin webs, or similar features – these result in distortions during manufacturing
- Undercuts– these will require special operations & tools
- Small holes and threaded features – these increase the likelihood of tool breakage and part scrap
Design for Handling
These design principles will facilitate parts handling and orientation:
- Design parts to consistently orient themselves (e.g. dowel pins)
- Avoid parts that can become tangled, wedged or disoriented
- Verify clearance for assembly tooling such as hand tools and fixtures
- For hidden features that require a particular orientation, provide an external feature, guide surface – or, design alignment or tooling to correctly orient the part
- Design in fasteners that are large enough to easily handle and install
- Design for efficient joining and fastening
- Avoid use of threaded fasteners (screws, bolts, nuts, washers) where possible, as these can be time consuming to assemble
- Use uniform screw sizes where practical
Threaded Hole Design
For sub-system designs that must include threaded holes for assembly, the following design considerations should be made:
- Design for full thread depth
- Typically, 1.5 times the major diameter will provide adequate holding strength
- The drilled hole depth (to the sharp point of the tool) should be at least equal to the full thread depth plus ½ 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.
Selecting Fixture/Tooling Materials
When designing steel fixtures or tooling where high accuracy in 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. This prevents abrupt surface variation within a relatively small area of the feature. Depending on material thickness and application, a note can be added to the design drawing: “FLATNESS MAYBE MEASURED WITH COMPONENT IN RESTRAINED CONDITION.” Where applicable, the note should include specific restraining requirements.
For interior radii, always specify the largest radius possible, because small-diameter tools add significant cost to the manufacturing process.
When a design requires metalized plating such as nickel, silver or other, specify a Controlled Radius (CR) or non-standard machining applicable for computer-numerical control (CNC) manufacturing.
CNC machining will create a “hard corner”, where the machine will race to a radius corner and abruptly change onto the next direction. The CNC change of direction often creates “tool chatter” which results in rough, sharp edges at the radius corner, and which commonly creates flaking.
Non-standard or CR slows down the cutter to blend a smooth radius at the corner feature. The smooth radius feature will facilitate good metalized plating and avoid flaking.
For deep, sharp corner cutouts that require broaching or electrical discharge machining (EDM), specify the radii maximum at all cutout corners (i.e.: 4X R .008 MAX).
When the depth of the cut exceeds five times the diameter of the pocket radii, consult with manufacturing on alternative fabrication methods. Depths of up to 10 times are possible when machining aluminum, but not all manufacturing facilities have that capability.
When designing tolerances, concurrently designing for manufacturing (DFM) will greatly improve product quality and reduce fabrication costs. In general, designs should avoid unnecessarily tight tolerances that are beyond the natural capability of the manufacturing processes.
It is always beneficial to consult with manufacturing early in the design process regarding tolerances. These items should be reviewed with manufacturing once preliminary sketches are available:
- Design intent
- Tolerances and tolerance challenges
- Tolerance stack-ups on mating parts
- Calculation of overall assembly tolerances
- Interface and clearance requirements
- Surface finish requirements
- Manufacturing process requirements
Designs and assembly should be simplified so that the assembly process is unambiguous. For example, components should be designed so that they can be assembled in only one way. Roll pins, dowel pins or offset mounting holes can be employed.
Likewise, designs for component orientation and handling should minimize non-value-added manual effort, ambiguity or difficulty in orienting and merging parts.
When designing surface composite curves that will require a continuous cutting path in CNC manufacturing – for example, internal pockets – design for and specify unilateral tolerances (+/- .010).
This approach ensures that a feature of many machine tools called “cutter compensation” can be taken advantage of. Cutter compensation allows size control variation of the features being machined without having to control the numerical control program (file) to an exact match with the cutter diameter.
Example scenario: Take a continuous path with these specified tolerances: +0, -.005 for the “X” dimension and +.005, -0 for the “Y” dimension. The cutter compensation cannot be used to control size in this case, because adding or subtracting from the cutter path input would automatically invoke an error to the dimension of the other toleranced continuous path surface. An offset is programmed into the machine for the cutting tool to manufacture for mid-tolerance of surface “X” at -.0025. However, this path is not compatible with the “Y” surface because the nominal offset is .0025 out of tolerance.
In addition to these best practices, OCM has created an online library of “Design For Manufacturing (DFM) Tips”. They are brief and clearly written to help anyone of any technical skill understand critical issues and best practices to ensure that product designs can be manufactured cost-effectively, efficiently, and with high quality.
At OCM Manufacturing, we can work with designers and engineers to ensure that their sub-system assembly plans and prototypes are manufacturable and therefore marketable. Contact one of our Program Managers for details about how we can help.
This article was originally published in Engineers Edge magazine.