First: Preliminary Preparation. This includes preparing the component libraries and schematic. "A workman must first sharpen his tools if he is to do his work well." To produce a good board, in addition to a well‑designed schematic, the layout must also be well executed. Before starting PCB design, you should first prepare the schematic (SCH) component library and the PCB footprint library. You can use the libraries that come with Protel, but it is often difficult to find the right footprints. It is best to create your own libraries based on the standard dimensions of the selected components. As a rule, create the PCB footprint library first, then the SCH component library. The PCB footprint library has higher requirements, as it directly affects board assembly. The SCH component library has relatively looser requirements – you just need to define the pin properties correctly and ensure the mapping to the PCB footprints. PS: pay attention to hidden pins in the standard libraries. After that comes schematic design, and once that is completed, you are ready to start PCB design.
Second: PCB Mechanical Structure Design. In this step, based on the determined board dimensions and mechanical mounting requirements, draw the PCB outline in the PCB design environment, and place the required connectors, buttons/switches, mounting holes, tooling holes, etc., according to the mounting specifications. Fully consider and define the routing and non‑routing areas (for example, the keep‑out area around mounting holes).
Third: PCB Component Placement. Placement is essentially putting the components on the board. If all the preparatory work mentioned above has been done well, you can generate a netlist from the schematic (Design –> Create Netlist), and then import the netlist into the PCB layout (Design –> Load Nets). You will see all the components pile up on the board, with ratlines showing the connections between pins. Then you can start placing components. General placement follows these principles:
①. Partition the board reasonably according to electrical performance – generally into: digital circuit area (both susceptible to interference and generating interference), analogue circuit area (susceptible to interference), and power‑driver area (interference source).
②. Circuits that perform the same function should be placed as close together as possible, and components should be adjusted to achieve the simplest connections. At the same time, adjust the relative positions of functional blocks to minimise inter‑block connections.
③. For heavy components, consider the mounting position and mounting strength. Heat‑generating components should be placed away from temperature‑sensitive components; thermal convection measures should be considered if necessary.
④. I/O driver devices should be placed as close as possible to the edge of the board and to the connectors.
⑤. Clock generators (such as crystals or oscillators) should be placed as close as possible to the devices that use the clock.
⑥. A decoupling capacitor (preferably a monolithic ceramic capacitor with good high‑frequency performance) should be placed between the power input pin and ground of each IC. When board space is tight, a tantalum capacitor may be placed around several ICs.
⑦. A freewheeling diode (1N4148 is sufficient) should be added across relay coils.
⑧. Placement should be balanced, with appropriate density distribution – not top‑heavy or lopsided.
—— Special attention must be paid to the actual physical dimensions (area and height) of the components and their relative positions, to ensure electrical performance as well as manufacturability and ease of assembly. At the same time, while adhering to the above principles, the component placement should be adjusted to be neat and aesthetically pleasing – for example, similar components should be aligned in the same direction, rather than being scattered randomly.
This step affects the overall appearance of the board and the difficulty of subsequent routing, so it requires considerable effort. During placement, for uncertain areas, you can perform preliminary routing to help with the evaluation.
Fourth: Routing. Routing is the most important process in the entire PCB design. It directly determines the performance of the PCB. In PCB design, routing can be divided into three levels of accomplishment: first is "routing completion" – this is the most basic requirement. If the routes are not fully connected and ratlines remain everywhere, the board is unqualified and can be considered as not even entry‑level. Second is meeting electrical performance – this is the standard for a qualified board. After routing is complete, carefully adjust the routing to achieve optimal electrical performance. Third is aesthetics. Even if the routing is fully connected and electrical performance is good, if the board looks messy – with chaotic, colourful traces – it will still be perceived as poor work, making testing and maintenance difficult. Routing should be neat and orderly, not haphazard. All this must be achieved while ensuring electrical performance and meeting other specific requirements – otherwise, it is putting the cart before the horse.
Routing is mainly performed according to the following principles:
①. Generally, power and ground traces should be routed first to ensure the board's electrical performance. Within the allowable range, make the power and ground traces as wide as possible. Ideally, the ground trace should be wider than the power trace, with the priority: ground > power > signal. Typical signal trace widths are 0.2‑0.3 mm, with the minimum down to 0.05‑0.07 mm; power traces are generally 1.2‑2.5 mm. For digital PCBs, a wide ground conductor can form a loop, creating a ground grid (but this should not be used for analogue ground).
②. Route critical traces (such as high‑frequency lines) in advance. Input and output traces should avoid adjacent parallel runs to prevent reflection interference. If necessary, add ground traces for isolation; traces on adjacent layers should be routed perpendicular to each other, as parallel runs can cause parasitic coupling.
③. The oscillator case should be grounded, and clock traces should be as short as possible and not be routed all over the board. The area under the clock oscillator circuit and special high‑speed logic circuits should have a large ground area, with no other signal traces passing through, to keep the surrounding electric field near zero.
④. Use 45° trace bends wherever possible – avoid 90° bends to reduce high‑frequency radiation (for high‑requirement traces, double‑arc bends may also be used).
⑤. Signal traces should not form loops; if unavoidable, keep the loop area as small as possible. Minimise the number of vias on signal traces.
⑥. Critical traces should be as short and wide as possible, and protected by guard traces on both sides.
⑦. When transmitting sensitive signals or noise‑band signals through flat cables, use a "ground‑signal‑ground" arrangement.
⑧. Test points should be预留 for critical signals to facilitate production and maintenance testing.
⑨. After schematic routing is complete, optimise the routing. After preliminary netlist verification and DRC checks pass, fill the un‑routed areas with ground copper. Use large copper areas as ground planes – connect all unused areas on the board to ground. Alternatively, use a multi‑layer board with dedicated layers for power and ground.
PCB Routing Process Requirements
①. Traces
Generally, signal trace width is 0.3 mm (12 mil), power trace width is 0.77 mm (30 mil) or 1.27 mm (50 mil). The clearance between traces and between trace and pad should be ≥ 0.33 mm (13 mil). In practice, increase the clearance where possible.
When routing density is high, it is possible (though not recommended) to route two traces between IC pins, with trace width of 0.254 mm (10 mil) and spacing ≥ 0.254 mm (10 mil). In special cases where component pins are dense and narrow, trace width and spacing may be reduced accordingly.
②. Pads
The basic requirement for pads and vias is: pad diameter should be at least 0.6 mm larger than the hole diameter. For example, for standard through‑hole resistors, capacitors, and ICs, use pad/hole sizes of 1.6 mm/0.8 mm (63 mil/32 mil). For sockets, pins, and diodes such as 1N4007, use 1.8 mm/1.0 mm (71 mil/39 mil). In practice, the dimensions should be based on the actual component sizes; increase pad sizes where possible.
The designed mounting hole diameter on the PCB should be approximately 0.2‑0.4 mm larger than the actual pin diameter.
③. Vias
Typical via size: 1.27 mm/0.7 mm (50 mil/28 mil).
When routing density is high, via sizes may be reduced slightly, but not too much – consider 1.0 mm/0.6 mm (40 mil/24 mil).
④. Clearance Requirements between Pads, Traces, and Vias
Pad and Via: ≥ 0.3 mm (12 mil)
Pad and Pad: ≥ 0.3 mm (12 mil)
Pad and Trace: ≥ 0.3 mm (12 mil)
Trace and Trace: ≥ 0.3 mm (12 mil)
When density is higher:
Pad and Via: ≥ 0.254 mm (10 mil)
Pad and Pad: ≥ 0.254 mm (10 mil)
Pad and Trace: ≥ 0.254 mm (10 mil)
Trace and Trace: ≥ 0.254 mm (10 mil)
Fifth: Routing Optimisation and Silkscreen. "There is no best, only better!" No matter how carefully you design, after finishing, you will always find areas that could be improved. A general design experience is: optimisation time should be twice the initial routing time. When you feel there is nothing left to modify, you can pour copper (Place –> Polygon Plane). Typically, pour ground copper (pay attention to separating analogue and digital grounds); for multi‑layer boards, you may also need to pour power planes. For silkscreen, ensure it is not covered by components or removed by vias and pads. Also, when designing, view from the component side – text on the bottom layer should be mirrored to avoid confusion.
Sixth: Netlist and DRC Verification and Mechanical Structure Check. First, after confirming that the schematic design is correct, perform a netlist comparison (NETCHECK) between the generated PCB netlist and the schematic netlist to verify the physical connectivity. Based on the output results, correct the design promptly to ensure correct routing connectivity.
After the netlist check passes, run a DRC check on the PCB design, and make corrections based on the results to ensure electrical performance. Finally, further verify and confirm the mechanical mounting structure of the PCB.
Seventh: Board Fabrication. Before this step, it is advisable to have a review process.
PCB design is a task that tests the designer's thoughtfulness and experience – the more meticulous the designer, the better the board. Therefore, design with extreme care, fully considering all factors (for example, ease of maintenance and testing is often overlooked by many), and strive for excellence – then you will surely produce a good board.
About Maxipcb