Functionality is usually the main focus the first time someone designs a circuit board. With time and experience, designers are able to focus on improving their designs to not simply be functional but also to increase performance. A seasoned designer can make the board robust and cheap while still easy to manufacture and assemble. Particularly, those only vaguely aware of the requirements for mass methodologies of soldering, such as reflow or wave soldering, will create boards that can only be hand soldered or will require extensive manual rework. While hand soldering can be more forgiving of poor layout, this is at the expense of increased time and frustration. Every board designed is unique, will have different requirements, and will require different trade-offs on the design, but there are basic guidelines of component placement that will go a long way toward creating a professional board that can be easily moved from the design table to reality.
An overall strategy that will help considerably, no matter the soldering method, is grouping components into functional blocks. There are typically different portions of a circuit on the board, a portion dedicated to power, another portion to communications, another portion to digital logic, and so on. When first approaching the board, it is important to group these together as much as possible. Not only does it help keep things organized and easier to track, but it also decreases the average track length and provides a good place from which to start. Once all of the parts have been placed on the board and grouped together, you can get an idea of about how much space you will need and can make a good approximation of the board size. Of course, the board size can change at any time, but it is helpful to have some loose constraints as it is natural to expand to fill the space provided.
Eliminate Shadowing with Proper Pad Placement
If you anticipate using wave soldering, keep in mind the direction the board will move through the wave. The largest concern with wave soldering is to eliminate shadowing. As the solder flows across a board, shadows are created when a small part of the board behind the component doesn’t receive solder. While this shadow is small for small items such as the leads of through-hole resistors, larger, surface-mounted devices in particular create a significant shadow. To avoid the shadowing effect, you use a combination of staggering pads so that one pad is not directly behind another. Another option is to put enough space between the components so that the solder comes back together in time for the next part. Spacing between components needs to be a minimum of 25 mil but could be up to 100 mil if it is a larger pad.For reflow spacing, a general rule of thumb is that the parts can be approximately one half the distance required for wave soldering. Reflow soldering has a different type of shadowing that may be a concern, and that is the shadow cast by taller components. If the infrared source of the reflow oven is not directly over a part, but at an angle, a taller part can leave the smaller part in a shadow. Most reflow ovens provide convection heating to even out the temperature profile, but there are still warm and cool pockets. Even in conveyors where the entire board is moving, thus changing the angle of the infrared source and the flow of air, the time in the shadow could be sufficient to ensure that the solder paste of the smaller components do not actually reflow. If two tall components are placed next to each other with connections between them, those connections are highly unlikely to receive the energy they need for the solder to flow. PCB assembly shops with vapor reflow capabilities avoid this issue by providing uniform, consistent heat across the entire board.
Consider Component Size
There are certain size restrictions that need to be considered for assembly. If a main consideration for the design is size or if the board deals with high frequency signals, there may be the temptation, or even the requirement, to use passives in the English 0201 or 01005 package sizes. However, not all assembly houses can mount components that small which can result in a premium for those services. If the board is going to be mixed technology and will be wave soldered, the restrictions are even more acute. 0805 and smaller surface-mount devices should not be wave soldered as the surface area underneath the component is not sufficiently large for placing the glue properly.
Beside size restrictions, care must be taken in terms of the thermal mass of adjoining components. If one portion of the board contains many large components while another portion contains only small passives, there will be a thermal mass imbalance across the board. For the solder and joints to reach the necessary temperature to ensure a good bond, the side of the board with a larger thermal mass requires a higher temperature than the side of the board with the smaller thermal mass. However, both sides are subjected to the same conditions. Either the larger components won’t be well soldered or the smaller components will be subjected to damaging levels of heat. By intermixing the two sizes as much as possible while still maintaining the functional blocks and avoiding shadowing, thermal load is spread more evenly across the board.
Align Polarized Components in the Same Direction
To reduce the opportunity for mistakes, it is also a good practice to align all polarized components in the same direction. All polarized capacitors, diodes, or LEDs should have their anode in one direction, cathode in the other. This information can even be silk screened or placed in the copper layer to help the assembler, whether it be you or someone else, know how to place the parts. If a general direction is not provided, then properly labeling every polarized component is important for the same reasons. If the boards will be hand soldered, it will reduce the risk of human error on every board. Even for machine populated boards, if the pick-and-place is programmed incorrectly due to unclear polarization, it will be a very costly mistake.
Traces and Pads
The setup of the traces and pads can significantly affect the ease of assembly and rework required for your board. From skewed to tombstoned components, careful trace and pad design can practically eliminate these problems. For reflow soldering surface mount devices, the key ideas to consider when laying these out are knowing what pads will come to temperature faster than others and knowing what direction the solder will go when reflowed. These factors become more important as the component becomes smaller, and therefore lighter. Very small passives, such as 0805 components and below, are much more susceptible to becoming skewed or tombstoning than their larger counterparts.
Avoid Tombstoning By Ensuring Consistent Thermal Loads
Tombstoning is a result of one side of a two-terminal device reflowing faster than the other. As the solder reflows and moves up to cover the terminal, it exerts force, pulling down and toward the pad. If that same force is not being exerted on the other side, as it has not reflowed yet, then the component will be pulled out of the solder paste on the other side and stand straight up, dipped in the reflowed solder. This vertical rectangle is reminiscent of a tombstone, which is why it is called tombstoning. To reduce the chance of this happening, both sides of the device need to have similar thermal loads. This not only includes the size of the pads, but also the traces leading up to them. Even under the solder mask, a large trace requires more energy to be heated than a smaller trace. The easiest solution is to reduce the size of the entire trace. However, if that’s not ideal or possible, then simply necking down the trace for the last 10 mil of the run works as well. If it is a high-current trace and necking is not possible, then providing multiple smaller traces to the pad is preferable to one large trace. Vias absorb a considerable amount of energy as well, so if there is a via directly next to a small passive component, then the via should either be moved farther away or the load should be balanced on the other side of the passive. Particularly in high-frequency designs, the closer the via is to the device, the better.
Control Solder Flow with Traces
For very low-cost boards without a solder mask, the direction a trace leaves the pad is very important. The solder mask typically stops the solder from flowing anywhere except on the pad, however, without that protection, the solder can and will flow as far down a trace as possible. This flow down the trace is generally not a problem in terms of solder deficiency, however, the way it pulls components may skew them off the pad. If the forces on the component are not controlled, it can twist one end of the component so much that the other end comes off the other pad. This can also be controlled with careful design. In essence, the traces leading to the pad need to work in tandem. The simplest method is to have the traces leave the pad directly outward or inward. If this isn’t possible, then have the traces leave the pad in similar directions, which may pull the component in a certain direction, but should be straight and less likely to pull one end off a pad.
Create Thieving Pads to Reduce Bridging
For wave soldering surface-mount components, these two issues are not a concern as the components are glued to the board. The bigger concern for wave soldering besides shadowing is reducing bridging on high pin-count devices. This is done by creating thieving pads for your devices. As a long row of leads have the solder wave flow over them, the leads pull the wave from one lead to the next, depositing the correct amount of solder on each lead. However, at the end of the leads, the solder wave does not have any further leads to pull the wave along. The solder then creates a ball on the last lead, frequently creating a solder bridge between the last two leads. This is fixed by creating a larger pad on the trailing edge of the device. This larger pad has the surface area needed to wick the excess solder off the lead, pulling it away from other leads.
The Board Itself
To ease assembly, the board itself needs to be taken into consideration. While boards can be made in practically any shape imaginable, odd shapes make automation very difficult.
Boards Should Have At Least Two Parallel Edges
To make sure that your boards can be gripped properly, you will need to provide at least two parallel edges. If the board needs to be circular, or some other odd shape, then the printed circuit board manufacturer can leave the boards connected to their larger panel while providing either V-grooves or rat bites so that the boards can be separated after assembly is complete. Do not forget to include overhanging parts, such as connectors, when deciding where the boards will be gripped. If there is an overhanging USB port or audio connector, it will interfere with the grip, and special grips will be required, adding another potentially expensive step to the assembly process.
Include Tooling Holes in Design
Tooling holes can be used throughout the manufacturing and assembly process. By providing tooling holes, boards can be stacked on top of each other, to reduce the amount of drills a machine must make. During assembly, these tooling holes can be used as either mounting holes while in the pick and place for both placing components and applying solder paste. Tooling holes can even be used as fiducials. Well-designed tooling holes can multitask to the point of assisting in electrical testing and in the mounting of a product’s enclosure. These tooling holes can be placed in the supporting portions of a panel or in each board individually. Tooling holes are standardized in size and it would be beneficial to speak to your board assembly house as well as the engineers designing the enclosure to ensure compatibility with all stages of the assembly. Due to variances in the plating process, tooling holes are never plated. Minor variations in the size of the tooling holes could cause a myriad of issues, so in the read-me file you send your circuit board manufacturer, it is best to give explicit instructions to not plate certain holes.
The difference between an adequately designed board and a well designed board can be subtle yet substantial. While there is no strict method that will yield perfect results every time, knowing the tools at your disposal as well as the benefits and drawbacks of different methodologies will allow you to make well-informed decisions that will boost your yield, increase repeatability, decrease costs, and create an efficient design. With time, the tips and tricks introduced here will become a natural part of the process, and you will find particular methods suited to your design style, methods that will result in higher quality circuit boards.