DFM: Design for Manufacture
Design for Manufacturability (DFM) means designing parts and various processes to make them easy to manufacture, cost-effective, and efficient. It involves considering potential production difficulties during the design phase to reduce production issues, improve efficiency, and lower costs. Both hardware and software design.
DFM Analysis Stages
| Stage | Collaborative Design | Comprehensive Analysis | Basic Pre-release Analysis | Post-release Review |
| Focus | Practicality, Usability | Efficiency, Cost-effectiveness | Reliability, Implementation of DFM, and DFT (ICT) Principles | Feedback collection, and continuous improvement |
| Key Considerations | Innovation, and user needs | Costs, Supply chain | Standards, and manufacturing compatibility | Use cases, Feedback (Customer surveys) |
Different stages of DFM analysis yield different results. The earlier the DFM stage, the easier it is to resolve problems, leading to minimal losses.
DFM Process Requirements for PCB Design
1. Size Range
The dimensions should not exceed the processing capability of the equipment. The commonly used size range is “Width (200 mm to 250 mm) × Length (250 mm to 350 mm).” For PCBs with a long side of less than 125mm, a short side of less than 100mm, or irregular edges, a panel design is required.
2. Shape
The board should be rectangular. If panelization is not needed, all four corners of the board should be rounded; if panelization is required, then after panelization, all four corners of the board should also be rounded, with the minimum corner radius being r=1mm, and r=2.0mm recommended.
To ensure stability during the transmission process, the design should consider using a panelization method to convert irregularly shaped PCBs into rectangular shapes, especially filling in notches at the corners.
- For SMT boards, notches are allowed, but the size of the notch must be less than one-third of the length of the edge it is on to ensure smooth transmission of the PCB on the conveyor.
- For internal rounded corners, a minimum radius of 0.8 mm is recommended; if necessary, the radius can be reduced to 0.4 mm.
Regarding the design requirements for gold fingers, as shown in the diagram, besides designing the insertion edge with a chamfer as required, both sides of the insertion board should also have a chamfer of (1 to 1.5) × 45° or rounded corners of R1 to R1.5.
3. Transmission Edge
- To reduce the deformation of the PCB during soldering, for PCBs that are not panelized, the long side is generally used as the direction of transmission; for panelized PCBs, the long side should also be used as the transmission direction. For PCBs where the ratio of the short side to the long side exceeds 80%, the short side can be used for transmission.
- Since terminal single boards generally use a panelized design, the process edge is typically used as the transmission edge, and the narrowest part of the process edge should be at least 4.5 mm.
4. MARK Points
| MARK Type | Description | Application |
| 1. Basic MARK | Used to meet basic production and alignment requirements | General Use |
| 2. Enhanced MARK | Used to meet more stringent production and alignment requirements | Precision Equipment |
| 3. Special MARK | Designed for specific needs such as QFP, BGA to meet precision and complex alignment requirements | High Precision Equipment |
Optical Alignment Reference Symbol (also known as MARK Point)
MARK points, also called reference points, provide a common measurable point for all steps in the assembly process, ensuring that each device used in assembly can accurately locate the circuit pattern. Therefore, MARK points are crucial for SMT production.
In PCB design, MARK points serve as position identification points for automatic placement machines. The choice of MARK points directly affects the efficiency of the automatic placement machines. Generally, the selection of MARK points is related to the model of the automatic placement machine.
- MARK Point Shape: The preferred shape for MARK points is a solid circle with a diameter of 1mm (±0.2mm), made of bare copper (which can be protected by a clear anti-oxidation coating), tin-plated, or nickel-plated. It is important to ensure flatness, smooth and even edges, and a color that distinctly contrasts with the surrounding background. To ensure the recognition effectiveness of printing and placement equipment, the area around the MARK points should be free of any other traces, silkscreens, pads, or wait-cuts.
- MARK points should be marked as solid circles; a complete MARK point includes both the marker point (or feature point) and a clear area around it.
- Mark points should be placed as far apart as possible on the diagonals of the circuit board or panel, ideally positioned at the longest diagonal.
- To ensure precision in assembly, SMT equipment requires that every PCB in all products produced by SMT have at least one pair of MARK points that meet design requirements and are recognizable by SMT machinery. Consideration can be given to having individual MARK points on single boards (as shown in the diagram below for both single boards and panelized boards). Panelized MARK points or combined MARK points serve only an auxiliary positioning function.
- When assembling boards, the relative positions of MARK points on each board must be the same. Do not move the position of the MARK point on any board for any reason, which will cause the position of the MARK point on each board to be mismatched. The assembly methods are:
① For Yin-Yang (or positive-negative) boards, the diagonal MARK positions must be identical.
② For mirror-image boards, each MARK position must be identical. R1=R2.
- On a PCB, all MARK points are only effective if they appear in pairs on the same diagonal. Therefore, MARK points must always appear in pairs to be usable.
5. Dimensions:
- The minimum diameter for MARK point markers is 1.0 mm, with the maximum diameter being 3.0 mm. The size variation of MARK point markers on the same printed circuit board should not exceed 25 microns.
- It is particularly emphasized that the size of all MARK points on a PCB with the same board number must be consistent, including PCBs produced by different manufacturers with the same board number.
- It is recommended that RD-layout standardize the diameter of MARK point markers in all drawings to 1.0 mm.
6. Edge Distance:
- The distance from the edge of the MARK point to the edge of the printed circuit board must be at least 5.0 mm (the minimum spacing requirement for machine clamping of PCBs), and it must be located within the PCB, not on the edge.
- The minimum clearance around the MARK point must also be met. To clarify, the distance from the edge of the MARK point to the board edge must be at least 3.0 mm, not from the center of the MARK point.
7. Clearance Requirements
Around the MARK point marker, there must be an area free of any other circuit features or markings. The clearance area radius r should be at least 2R, where R is the radius of the MARK point. When r reaches 3R, machine recognition is more effective. The contrast in color between the MARK point and its surroundings should be enhanced. No characters (such as copper plating or silkscreen) are allowed within radius r.
- Materials: MARK point markers can be made of bare copper, bare copper protected with a clear anti-oxidation coating, nickel-plated, tin-plated, or with a solder coating. If a solder mask is used, it should not cover the MARK point or its surrounding clear area.
- Flatness: The surface flatness of the MARK point markers should be within 15 microns [0.0006 inches].
- Contrast: a) The best performance is achieved when there is a high contrast between the MARK point markers and the substrate material of the printed circuit board. b) The background within all MARK points must be consistent.
8. Positioning Holes
- Each PCB should have at least two positioning holes designed at its corners.
- Panelized positioning holes should number four, distributed at each corner, with a standard hole diameter of 2.00 ± 0.08 mm. The center of the positioning holes should be 5 mm from the nearest board edge.
- The minimum distance from any component or pad next to a positioning hole to the edge of the hole should be at least 1.5 mm.
9. Hole Metallization
- Positioning holes and non-ground mounting holes should generally be designed as non-metalized holes. If issues arise in the SMT process, steel mesh design optimization (PasteMask optimization) is necessary. This involves creating two masks (SOLDER MASK and PASTE MASK) when generating Gerber files.
- The SOLDER MASK is used for the solder-resist material application, while the PASTE MASK is used to make the stencil for the solder paste application.
10. SMT Stencil Design Principles
The thickness of the SMT stencil should meet the requirements of the finest pitch QFP and BGA components, considering the smallest CHIP components. The general principles and special opening design principles for SMT solder paste stencils are outlined, ensuring high opening precision and smooth hole walls for effective solder paste release.
DFM Case Studies
Case 1: Gold Finger Solder Contamination
A product had components placed too close to the gold fingers, causing solder contamination after placement. The solution involved modifying the PCB design to adjust the distance between pads and gold fingers, applying high-temperature adhesive tape before reflow soldering, and inspecting the boards under a microscope after repair.
Case 2: Pad Green Oil Issue
High thermal dissipation requirements led to large holes in thermal pads, with poor plugging capabilities causing green oil on pads and component leads opening. The interim solution was to cancel the plugging method, modify the stencil design, and inspect the soldering and solder ball conditions after reflow soldering.
Case 3: MARK Point Issues
MARK points had diameter and shape inconsistencies, making them unrecognizable by SMT machines. The solution involved ensuring proper MARK point design, positioning, and maintaining uniform size across all boards, including those from different manufacturers.
Case 4: BGA Problems
Issues with BGA pads included inconsistent sizes, lack of solder mask, improper connection to traces, excessive surface line width, and unprocessed vias. Solutions included redesigning the pads, applying proper solder masks, ensuring central via placement, and managing via-in-pad designs to prevent soldering defects.
By continually optimizing production processes, forming issue-tracking forms, and providing comprehensive training, production efficiency, and quality can be significantly improved.
