14 Tips For PCB Design For Assembly
Designing with PCB assembly in mind is one of the most important and frequently misunderstood elements. This series is dedicated to helping you become a designing pro—someone whose PCB design has been optimized on the first try, ensuring a smooth quickturn PCB production process. Follow these tips when you design for assembly.
What is Design for Assembly (DFA)?
Before going any further, let’s discuss what PCB assembly entails. After a PCB design is submitted and approved—be it flex, high density interconnect (HDI), or otherwise—it is fabricated. Once that is complete, the bare boards will need to be assembled with additional components, including processors and memory.
Simple enough. The problem that often emerges—at least, among those who are not yet PCB Masters—is that the initial PCB design does not fully take assembly into account. Instead, they focus exclusively on the board itself without broader context of how the board will be used within the product or application.
Overlooking PCB assembly can lead to significant complications. A PCB design may seem perfectly acceptable when viewed in isolation, but certain design decisions may make assembly difficult later on. For example, components may be situated too close to one another, which could lead to a non-functioning product, or cause performance issues. We’ll discuss this in-depth later in the article.
Then there’s also the question of component availability. In order for the PCB assembly process to flow smoothly—and, therefore, for the PCB production as a whole to progress effectively—the assembly vendor needs to have the requisite components on hand as soon as the boards arrive. If they aren’t available, the whole process will be delayed, undermining the value of a quickturn approach to PCB production.
Becoming a PCB Assembly Master
Those are just some of the issues that will arise if you aren’t approaching design with PCB assembly in mind. The question is, how do PCB masters avoid making these mistakes? Here are a few key tips.
1. Pay attention to part-to-part spacing.
One of the frequently asked questions posed by designers who are not yet PCB masters is in regard to the component-to-component spacing. Placing a component too close to another component can create various issues which may require redesign and refabrication, which results in a loss of time and money.
PCB masters use several techniques to avoid part-to-part spacing issues during assembly. They design their footprint in such a way that there is always enough gap between component boundaries. This alleviates any potential issues that could arise from components being too close during placement.
Designers must carefully place components so the place-bound component shapes do not overlap each other. In Example One, you can see putting components based on the place-bound shape will automatically keep them 50 mils apart. If the board does not have enough space, PCB Masters can disregard the place-bound shape and move components closer to one another, keeping the minimum spacing rules in mind.
Ensure component rules, requirements, and proximity regulations have been established in your PCB design software. PCB masters have specific component-to-component spacing guidelines for various part types. For example, the minimum spacing between discrete components like caps and resistors should always be at least 10 mils, with 30 mils being the preferred spacing. This simple action will help avoid many of the proximity issues. These issues can otherwise lead to assembly delays or other complications down the line. For additional spacing rules, refer to Table 1.1.
Table 1.1: Spacing Component-to-Component
2. Choose components during the design phase.
PCB Masters choose components early in the design process, realizing that this is the best way to ensure there are no conflicts between the actual design and the components being assembled. If you factor in component sizes from the very beginning, component space and sizes are no longer a concern and the PCB assembly process can proceed without barriers. This also leads to the next tip.
The PCB designer should talk to the circuit designer and engineers to see if the component size can be reduced, creating additional space on the board. After all, a smaller part will mean a smaller footprint on the board.
3. Separate non-lead-free from lead-free components.
Never mix lead-free components with components that are not specified for lead-free assembly. If any component requires lead-free assembly and no substitute for conventional leaded solder is available, then the entire board must be assembled lead-free and all components must be qualified for lead-free assembly.
Sometimes the only package available for a particular device is a lead-free BGA. However, boards that will be used for military projects typically must be assembled with conventional leaded solder, per government requirements. The designer must either obtain a waiver from the customer to allow lead-free assembly; modify the design to use a device that is available in a package for assembly with conventional leaded solder; or have the BGA reballed for leaded solder (an expensive procedure that can damage parts).
3. Evenly place your large components.
Distribute large components across a board as evenly as possible during layout, to achieve the best possible thermal distribution during solder reflow. Make sure the assembly contractor tailors a thermal profile for the reflow oven unique to each assembly job.
4. Avoid mixing technologies.
Whenever possible, avoid mixing technologies. The payoff of a single through-hole, for example, doesn’t outweigh the additional time and money spent. It would be more efficient to either use multiple through-holes or none. If you do use through-hole technologies, placing all through-holes on one side of the board will reduce manufacturing time.
5. Pick the appropriate package size.
Communication between the electrical engineer and PCB designer should begin during the early stages of layout. The designer should review the BOM and carefully examine the parts being used in the design. The designer may recommend larger components if there is space on the board and the current design uses unnecessarily small components. This will help avoid complications during assembly. For example, it is beneficial to use a 0402 size capacitor/resistor rather than a 0201 whenever possible.
A PCB Master would choose a 0805 capacitor over a 1206 cap—if the 0805 can fulfil all the necessary requirements. This will free up significant space on the board.
They are also manufactured by various vendors. Choosing these components will avoid delays during the assembly process. It also gives both the electrical engineer or the designer the option of choosing alternate parts without changing the schematic or layout, a timely solution to components not in stock.
Finally, it is important to choose the appropriate package size while in the PCB design phase. A PCB Master only chooses smaller packages when there is a good reason to; otherwise, lean toward bigger options. In too many cases, electrical engineers choose unnecessarily small component packages. This can create issues in terms of assembly yield, as it is more difficult to touch up and rework smaller components. Depending on the amount of rework needed, it may be more cost-effective to completely rebuild the board the remove and solder on new components.
After you’ve confirmed an ideal package size, you can begin choosing components in the same density category.
6. Look for long lead-time components.
As mentioned above, component availability can potentially cause significant delays. However, PCB Masters avoid this issue by checking the availability of all components before beginning the design. If there are parts which require long lead-times, they can be ordered early and be consigned to the PCB assembly vendor. The assembly vendor can also handle the procurement of the more widely available parts, so every component will be ready and waiting when your boards are ready to be assembled.
7. Keep your BOM up to date while designing.
A BOM is a key aspect of both design and assembly. If there are any issues in your BOM, the assembly house will place the project on-hold until the issues have been resolved with an engineer. One way to make sure your BOM is updated is to review your BOM any time there is a change in your design. When you add new components to your schematic while the layout is in process, make sure you’ve also updated the BOM with the correct part number, description, and component values. During the design process, the engineer might change a component due to long lead-times, size, or availability and forget to update the BOM with the new part number. This can lead to various assembly issues and cause delays.
Format every bill of materials according to the below example to precisely identify all of the components to be assembled on each board. The properly formatted BOM has columns indicating:
- Full manufacturer’s part number
- Manufacturer’s name
- Item number
- Quantity per board
- Reference designators, separated by commas
- A complete part description
It may also include:
- Distributor’s name
- Distributor’s part number
8. Carefully inspect your footprint development.
Component footprints are another major aspect of layout design. A PCB Master will make sure their footprints are created accurately as per the land pattern recommended in the datasheet. It is very important to use the numbering key correctly from the datasheet to identify the correct part and its land pattern. Reading the datasheet incorrectly will result in an incorrect footprint, which could require a complete redesign and re-fabrication of the boards.
The image below shows an example of the numbering key and various types of footprints.
9. Be sure all indicators are present.
The leading show-stopper in assembly is missing pin 1 indicators or component polarity/orientation indicators on the silkscreen. Nearly 75% of the assembly orders my facility receives fail to identify the location of pin 1 for each IC, or they misrepresent or neglect to indicate the polarity of some capacitors, diodes, or LEDs.
The best way to avoid assembly problems: Confer with your manufacturer before design even begins.
Obey the convention for marking the polarity of diodes, including LEDs: Put a K on the silkscreen layer at the cathode end. Alternatively, use the electrical symbol for diodes in the correct orientation to guide assembly. Never indicate diode polarity based on the anode pad. Use a K to designate the cathode or line up the diode symbol in the correct position. Don’t substitute any other marks or your contractor will misinterpret what you intend.
To orient tantalum capacitors, tag the positive side with a plus symbol on the silkscreen. Remember, tantalum capacitors can ignite if mounted with swapped polarity. Short of reverse- engineering a schematic there’s no way for a contractor to figure out part polarity unless it’s clearly displayed. Silkscreens must not interfere with pads, and symbols should not be printed beneath the body of any component.
10. Via-in-pads must be filled
Unless they reside in thermal pads, via-in-pads must be filled. The pad matrix on which a BGA will be installed may include through vias and blind vias, but all of them must be filled and planarized, or solder joints will be compromised. Incorporate vias in the thermal pads under QFNs to help solder flow through to conductive planes. The vias ensure a secure solder joint for the thermal pad and prevent solder from floating the package during assembly, which could hamper forming good solder joints at the QFN contacts. An assembly shop can compensate for a lack of through vias in a thermal pad by adding windowpane-shaped opening in the solderpaste stencil above the pad, to relieve solder pooling and outgassing during assembly, but the fix is less effective than if vias were present.
11. One pad for one connection
Every connection to every component must have its own independent pad. Each pad must be commensurate in size with its mates. If two components share a pad—let’s say, a resistor and a capacitor—neither can be properly aligned during assembly. And if one pad is substantially larger than its mate for a component, component tombstoning can result from an imbalance of solder deposition.
If a pour or plane will be a point of contact, there must be a mask-defined pad of appropriate size. If a device involves non-solder mask defined pads for connections as well as solder mask—defined pads a BGA matrix on a loose pitch in which some adjacent outer balls are common to a ground pour, for example—stipulate in a design note that the board fabricator shall not edit the solder mask apertures for those solder mask-defined pads.
12. Ease CAM setup.
Needless to say, it’s far better to catch issues that might impede assembly before the boards are fabricated. If the board will be fabricated and assembled by the same facility (thereby coordinating operations), verify whether to provide the design data in ODB++ format to speed identifying potential manufacturing issues and ease CAM setup. Outputting a design in ODB++ captures the data for fabrication, assembly, and test in a unified structure that supports automated analysis and avoids time-consuming data conversion at the CAM stage. Practically all major EDA platforms can output design data in the ODB++ format.
13. Address your component delivery.
Technically, the 10th tip does not address design, but component delivery to the contractor. If assembly will be performed on a consignment basis—some or all of the components will be supplied by the assembly customer, instead of being procured by the assembler—the parts must be provided in a carefully organized kit matching the BOM. All SMT components must be supplied in reels, or on continuous tapes at least 6” in length, or in tubes or trays.
Extra components are required for every part number listed on the BOM, to cover attrition during assembly. For example, an assembly shop may require a minimum of 100, or 20% more 0201 1k ohm resistors than called for on the BOM. The parts for each line item on the BOM must be sent in a clearly marked bag separate from the other parts. All ICs must be shipped in their original, unopened protective packages that include desiccant, or else they must be baked for eight hours or so to remove moisture before assembly, which could set back assembly for a day.
In other words, eight strips of eight pieces of a 1005-size 12-pF capacitor do not fulfil a BOM requirement for 64 pieces of that part. The strips are too short for loading the pick-and-place feeders, and under the best circumstances not all the parts will wind up on boards. Check and double-check your components before shipping using our kitting guidelines.
Let me conclude by recommending the best way to avoid assembly problems: Confer with your manufacturer before design even begins.
14. Check these additional PCB assembly tips.
Additional assembly details to keep in mind during the design stage include heat and wash. Make sure you know what the maximum heat levels of your components are, whether they can be washed, and the type of assembly it requires. If it will be hand-soldered, the board design must include the space for a soldering tool.
Make sure your capacitors all face the same direction. This saves the pick and place machine time during component placement.
Pay attention to components that emit heat. The space around these components must be carefully reviewed. Make sure heat does not negatively affect any components or traces around the component.
To continue on the path toward becoming a PCB master, keep an eye open for the next piece in the series.
For more information on design rules, check with our DESIGN SERVICE team.
DOWNLOAD OUR DFM HANDBOOK:bom, capacitor, component, Footprint, pcb assembly, pcb design