One of the most fun parts of creating a real electronic circuit is (in my opinion) designing the Printed Circuit Board or PCB layout.
This is the point where our abstract circuit schematic made by symbols and lines, becomes a real circuit that can be manufactured, assembled and used.
PCB design requires some extra skills such as visual-spatial intelligence that is not “traditionally” part of the standard Computing/Maths/Electronics archetype which is normally more abstract/analytical-number oriented. These skills are normally found in the lights of architects and mechanical engineers.
This makes PCB design a sort of art/science trade, where engineering/rational decisions are taken to maximize and benefit the functionality of the circuit. However, since there is no “equation” or “formula”, if you give a circuit to 10 different PCB designers, you will get 10 different PCBs.
The objective of this article is to teach the reader different guidelines that will improve the electrical, mechanical and thermal performance of his/her PCB design.
At the end of the article, a review will be done to the PCB of the Solar Mobile Charger and Powerbank so the reader can visualize how to apply the previously mentioned guidelines.
Only interested in applying these guidelines to your design? Download the PCB Design Checklist spreadsheet
Privacy Notice: Your email address will not be shared and you will only receive relevant content. Zero Spam
The PCB is an electromechanical component that needs special considerations when put together with the rest of the product.
Compatibility with the product’s enclosure
Unless you are designing a developing board that needs to show its parts to the external world, your PCB will be fixed to an enclosure. This enclosure will have some spatial and functional constraints that need to be addressed when designing the PCB.
The most obvious and important constraint, the size of the PCB. The PCB engineer needs to work alongside the enclosure designer and agree on a PCB size in terms of length and width.
The PCB cannot be too small, otherwise, components won’t fit, or the board could overheat, while in the other hand, a product might need to be small and portable, therefore it cannot be big and chunky.
Unless the enclosure has some specially designed cavities where the PCB will fit, the PCB will normally be fixed to the enclosure through screws and washers. Either from stand-offs or directly connected to the enclosure.
Hole locations need to be mutually agreed as well. They will normally be spaced out or near heavy parts of the board that could break from excessive mechanical stress (think in big capacitors and transformers). The hole also needs some space around to fit a washer, therefore you will normally not place components near it.
To properly determine connectors locations, you need a good understanding of the system where your device will be placed. For example, in a car, you might want two connectors to be on opposite sides of the board because the wiring of the car has been made that way.
Also, as a general guideline to avoid EMI, connectors are normally placed on the same edge of the board.
Height of components
When designing a PCB, it is very easy to forget about the third dimension of height, as all PCB layout design software work in 2D, looking from the top.
Some components such as electrolytic capacitors and connectors have a considerable height. Ask the enclosure designer for a max height parameter so you are well aware of not reaching this limit while choosing and placing components
From a mechanical point of view, there are a few warning lights when it comes to placing components.
If working with a double-sided board, most components, particularly heavy ones, must be placed on the layer that will be the relative top for most of the product life. This will reduce the mechanical stress on the solder joints of components.
Another important factor is avoiding placing relatively big and heavy components on the edge of the board. The farther you go from the middle of the board, the more and easily it bends.
If you place heavy components on the edge, these will put pressure and bend the board. Also, as the edge is where the board is most bent, it can also break the soldering joints of the component.
As in any other part of the device, the PCB is also a victim of changes in temperature.
Most of the heat dissipated on the PCB will come from the components itself.
However, some heat can also come from not properly sized traces. The heat dissipated on the PCB traces is directly proportional to its resistance, which is a function of its dimension and material. The material and thickness is normally a fixed value (copper and 1oz), therefore we are left to play with the width and length.
As a general rule, for high current nets, traces should be made as wide as possible to decrease its resistance, as a guideline, you can use the following table:
PCB Maximum Temperature
This will vary depending on the PCB used, but in general, the PCB should not have a hot spot of more than 170 degrees Celsius.
To visualize this, you either need a prototype PCB and a thermal camera or a thermal simulation software.
Improving Components dissipation
PCB’s are made mostly of fibreglass and copper. Copper is a thermally conductive material and it can be used as a heatsink for components that need help in dissipating excessive heat.
This can be achieved by pouring copper on the same layer the component is placed or by adding a layer of copper underneath and then connect it with a good amount of vias that act as thermal conductive points.
The main function of a PCB is to electrically connect components so they work as intended. We will explore some techniques and considerations to have in mind in order to make the device reach its best electrical performance.
Ground planes and returning currents
In applications where more than a couple of components are placed on the PCB, a ground plane can drastically improve the electrical performance of the circuit.
The ground plane acts as a low impedance current return path for all components in the circuit and makes the layout easier. It also works as a board-wide heatsink.
Keep traces as short as possible
A short trace will have less impedance (resistance, inductance and capacitance). This is particularly important for high-speed signals.
Do not break the ground plane
Ground planes should be kept without traces and interruptions as much as possible. When braking a ground plane, the return current path of the signal that is on the opposite layer changes, which can cause EMI problems particularly with high-speed signals.
Bypass capacitors are used to keep a stable supply voltage without ripples or dips on digital or high-speed signals ICs. These are normally 1nF-100nF low ESR ceramic capacitors.
To make bypassing effective, the capacitor must be placed as close as possible to the IC pin and the power supply trace should arrive first to the capacitor pad and then routed to the IC.
Traces Width, Length and Angle
As mentioned above, traces should be as wide as they can (especially for high current signals) and have a short length (especially for high-speed signals).
Regarding angles, 90 degrees traces should be avoided as they can cause reflection issues on high-speed signals and some PCB manufacturing machines are not able to properly copy this pattern.
Vias are used to trace a signal through different layers of the PCB.
If you have a high current signal that switches from one plane to the other through a via, it is good practice to use many vias instead of just one in order to reduce the track’s impedance.
Signals that are exactly the same but with inverted polarity with respect to each other are called differential signals. This is a technique used to reduce the noise and distortion that could be radiated into them through a communication path.
A common protocol that uses differential signals to transfer data is USB with signals D+ and D-.
To maximize the benefits of a differential pair, these signals must be routed together with traces of the same length and same distance from any solid plane. This is done so both conductive paths have the same impedance.
Does your circuit have different supplies or signals that need to be electrically isolated from each other? such as a battery from the AC mains?
If this is the case, then you need to have a minimum distance between tracks and components from one side to the other.
This minimum distance is a function of the voltage difference between one side and the other and the pollution degree.
Pollution degree refers to factors of how humid, wet or dusty is the space between a conductive part from one side to the other.
The following table put together by PTR can be used to determine the minimum distance between the conductive surfaces:
Design for Manufacture Considerations
The PCB we are designing needs to be manufactured by machines that have their own limitations and requirements.
These are parameters that need to be configured in the Design Rule Check of your PCB layout design software. This way you will make sure that you will not violate any of them, avoiding a waste of time and money in the future.
In Upverter, you have a whole configuration page dedicated to DRC:
This is defined as the minimum distance between two tracks or pads. Smart Prototyping has a minimum value of 0.15mm (6mil)
Holes and Vias size
Holes and vias also have a minimum diameter specification. For Smart Prototyping this is 0.2mm.
Also, if you are creating custom size holes with solderable pads, is that the pad’s diameters should be at least 1.8 times bigger than the hole diameter.
Fiducial marks are visual markers on the PCB that serve as reference points for the PCB manufacturing machines. These are not always necessary, for example, for the Solar Mobile Charger and Powerbank, Smart Prototyping did not ask for these.
When ordering PCBs, ask the PCB manufacturer if fiducial marks are required.
The silkscreen is the layer where you have your RefDes (C1, R7, etc), labels, logos and anything else you fancy drawing. This ink only gets printed on zones where there is no tin pad present.
When reviewing your design, make sure there are no silkscreen elements over a tin pad.
Check your Gerber
When submitting PCB design files to the manufacturer, it is normally done by sending them files in Gerber format.
When you output these files from your PCB software, it is a good idea to visualize them and compare them with your actual design. Sometimes the translation is not exactly the same as in your screen, however, most of the time the differences are insignificant.
You can check your Gerber by uploading the files on the Online Gerber Viewer from EasyEDA.
Design for Reparability and Testability Considerations
As mentioned in the article What is a Sustainable Electronic Product? in order to achieve a more sustainable product, we need to have repairability in mind when designing. Also, the PCB requires some infrastructure in order to facilitate the task of testing it.
Test points are simply a tin pad coming out of a net so you can probe it and visualize its value. They can also be used to check the value of components at an End Of Line manufacturing process.
However, some discretion should be made as test points can easily act as antennas, both radiating and/or making them susceptible to noise. This is particularly true for high-speed signals such as SPI.
For prototyping, it is useful to have test points in the most relevant nets, these include high-speed communication signals as well.
For manufacturing big volumes or producing the sample for EMC testing, test points are required in every net and between components such as resistors and capacitors. In this case, test points should not be placed in high-speed nets to avoid EMI issues.
The silkscreen layer is not only for the RefDes of the components. I like to add the following annotations on my PCB layouts:
- Electrical Hazard Warnings: if your device is connected to the AC mains or an HV battery, you must place electrical hazard symbols and warnings. You can seriously injure someone and even get fined if you omit this step. Safety first!
- Project info: Title of project, version and date. This will help you identify PCBs in case you have different revisions.
- Copyright notice: if your project is not open source, better be safe than sorry.
- Components likely to fail: this can make the device easier to repair for the technician.
- Connectors and circuit blocks names: this way anybody can quickly refer to the HW Block Diagram and understand what is what.
- Logos: they give the design some style and branding. Nice finishing touch!
Like a piece of code or a schematic, the PCB layout needs to be reviewed by another engineer. This is a great way to get feedback and discover errors.
Does your PCB look gorgeous and inspiring? One way to achieve this is by having repeated blocks look the same and avoid components placed on weird angles instead of vertical or horizontal.
Anyway, I guess we all have our own concept of beauty. Just remember, functionality always comes first than aesthetics.
Solar Mobile Charger and Powerbank PCB Design Review
Compatibility with the product enclosure
As there are no fixed requirements here, except that it needs to be a portable device, it was taken as a reference the dimensions of the small solar panels.
Therefore it was decided that the PCB had to be smaller than 112*91mm.
The PCB has a size of 65*70mm
There are no heavy components so holes can be distributed uniformly. Two holes were placed and they are not nearby any component. Maybe an extra hole next to the USB-B INPUT would be beneficial.
Judgement: OK but could be improved
Connectors were placed according to the HW Block Diagram. The USB connectors face the external world, while the battery, internal solar and display will be inside the enclosure.
Because the board is small, the EMI guideline of putting all connectors on the same edge can be softly ignored. Still, all power connectors are on the same side.
Height of Components
Tallest components omitting the pushbutton are the JST connectors and there is no hard requirement on their height.
All components were placed on the top layer, however, as there are no heavy components and the position of the board will be changing all the time with real use (think of the product thrown in a bag or pocket, it could be in any position), it doesn’t matter too much from a mechanical stress point of view.
Also, there are no components present on the edges of the board
There will be up to 2A’s of current flowing through the power tracks, must of these tracks are quite chunky, however, the one connecting the battery with the 5V SMPS has a long thin track:
The track measured 0.775mm which is slightly higher than the recommended 0.762mm (30mil) from the table above.
Judgement: OK but needs improvement
PCB Max Temperature
I cannot measure this parameter, however, there is only two hot-spots expected. The battery charger and the SMPS. Both of these components are using the PCB as a heatsink.
The components being both switch mode power supplies should not generate much heat. However, this must be validated by testing with the prototype
Both of the previously mentioned components with expected heat dissipation, have vias connecting them to the ground plane.
This way the heat will be transferred from the casing to the bottom copper layer through the vias.
A double layer PCB was designed with the bottom layer designated as a ground plane
The high-speed signals present in the circuit are: the I2C to communicate with the display and the programmer interface.
Both traces are short.
Do not break the ground plane
The ground plane was broken but only in low current/ low-speed digital signals such as DO_5V_EN. High speed or high current signals have a good return path.
All IC’s have their bypass capacitors as close as possible and with the supply pin arriving first to the capacitor and then to the IC.
Trace width, length and angle
No 90 degrees traces present.
A modification to the trace connecting the battery with the 5V SMPS can be made to reduce its length. All of the components could be rotated 90 degrees clockwise:
Judgement: OK but needs improvement
No power signals changing layer apart from GND from top to bottom. These vias could be larger in order to reduce the track impedance which will benefit this high current circuit.
An example of this improvement is the GND connected to the USB-B INPUT connector:
Judgement: OK but needs improvement
No differential signals present.
No isolation requirements present.
Design for Manufacture
Track clearance, hole size and trace width were all larger or equal than the minimum specified by Smart Prototyping.
No fiducial marks were required by Smart Prototyping.
Some silkscreen was printed over pads:
This error only stopped the continuity of the line, the functionality is unaffected.
Judgement: OK but needs improvement
The Gerber was uploaded to the EasyEDA application:
What I immediately noticed was the holes for THT components seemed solid. I passed my inquiry to the Smart Prototyping representative to check for manufacturing issues and they replied with an OK for manufacturing.
Design for Reparability and Testability
A few test point were placed in important signals such as battery voltage, input and output voltage and regulator voltage output.
Test points for the I2C signal could have been useful, however, I can use the vias.
The PCB was printed with the project info, logo, circuit blocks and connectors names. No electrical hazards present and no weak spots present (I believe, although the charger and boost converter could break from overcurrent?).
Judgement: OK but needs testing
The PCB was sent to an ex-colleague for review.
It is clear that this is a piece of art right 🙂?
In this article, we have covered different aspects of PCB design including: mechanical, thermal, electrical and design for manufacture.
Guidelines have been presented and a review of an electronic product was done using the discussed guidelines.
If you would like to download a PCB Design Checklist that you can use for the development of your electronic product, head over to the Resources section.
Have I missed any important guideline? Please share it in the comments section below!
PCB Design Tutorial Revision A – David L. Jones
PCB Layout – Learn EMC