PCB Design Process

fighting

PCB Design Process [Copy link]

PCB Design Process

The general PCB design process is as follows: preliminary preparation -> PCB structure design -> PCB layout -> wiring -> wiring optimization and silk screen -> network and DRC inspection and structure inspection -> plate making.

First: preliminary preparation. This includes preparing component libraries and schematics. "If you want to do your work well, you must first sharpen your tools." To make a good board, in addition to designing the principle, you must also draw it well. Before designing the PCB, you must first prepare the component library of the schematic SCH and the component library of the PCB. The component library can use the library provided by peotel, but it is generally difficult to find a suitable one. It is best to make your own component library based on the standard size information of the selected device. In principle, make the component library of the PCB first, and then the component library of the SCH. The component library of the PCB has higher requirements, which directly affects the installation of the board; the component library of the SCH is relatively loose, as long as you pay attention to defining the pin attributes and the corresponding relationship with the PCB components. PS: Pay attention to the hidden pins in the standard library. After that, it is the design of the schematic, and after it is done, you are ready to start the PCB design.

Second: PCB structure design. In this step, the PCB surface is drawn in the PCB design environment according to the determined circuit board size and various mechanical positioning, and the required connectors, buttons/switches, screw holes, assembly holes, etc. are placed according to the positioning requirements. The wiring area and non-wiring area are fully considered and determined (such as how much area around the screw hole belongs to the non-wiring area).

Third: PCB layout. To put it simply, layout means placing components on the board. At this point, if the preparations mentioned above are done, you can generate a network table on the schematic (Design->Create Netlist), and then import the network table on the PCB diagram (Design->Load Nets). You will see all the components stacked up, and there are flying wires between the pins to indicate the connection. Then you can lay out the components. The general layout is carried out according to the following principles:

①. Reasonable division according to electrical performance, generally divided into: digital circuit area (i.e. afraid of interference, but also produces interference), analog circuit area (afraid of interference), power drive area (interference source);

②. Circuits that perform the same function should be placed as close as possible, and the components should be adjusted to ensure the simplest wiring. At the same time, the relative positions of the functional blocks should be adjusted to ensure the simplest wiring between the functional blocks.

③. For components with large mass, the installation position and installation strength should be considered; heating components should be placed separately from temperature sensitive components, and thermal convection measures should be considered if necessary;

④. Place the I/O driver as close to the edge of the printed circuit board and the lead-out connector as possible;

⑤. The clock generator (such as crystal oscillator or clock oscillator) should be as close as possible to the device that uses the clock;

⑥. A decoupling capacitor (usually a monolithic capacitor with good high-frequency performance) needs to be added between the power input pin and the ground of each integrated circuit. When the circuit board space is dense, a tantalum capacitor can also be added around several integrated circuits.

⑦. Add a discharge diode (1N4148 is sufficient) to the relay coil.

⑧. The layout should be balanced, orderly and not top-heavy or one-sided.

——Special attention should be paid to the actual size of the components (the area and height they occupy) and the relative positions of the components when placing them, so as to ensure the electrical performance of the circuit board and the feasibility and convenience of production and installation. At the same time, the placement of the components should be appropriately modified to make them neat and beautiful, while ensuring that the above principles can be reflected. For example, the same components should be placed neatly and in the same direction, and should not be placed in a "scattered" manner.

This step is related to the overall image of the board and the difficulty of the next wiring, so you need to spend a lot of effort to consider it. When laying out, you can do preliminary wiring for places that you are not sure about and give them full consideration.

Fourth: Wiring. Wiring is the most important process in the entire PCB design. This will directly affect the performance of the PCB board. In the design process of PCB, wiring is generally divided into three levels: First, wiring is through, which is the most basic requirement for PCB design. If the lines are not through, and there are flying wires everywhere, it will be an unqualified board, which can be said to be not yet started. The second is the satisfaction of electrical performance. This is the standard for measuring whether a printed circuit board is qualified. This is after the wiring is through, carefully adjust the wiring so that it can achieve the best electrical performance. Then there is beauty. If your wiring is through, there is nothing that affects the performance of the electrical appliances, but it looks messy at first glance, plus colorful and colorful, then no matter how good your electrical performance is, it is still a piece of garbage in the eyes of others. This brings great inconvenience to testing and maintenance. The wiring should be neat and uniform, and it cannot be criss-crossed and disorderly. These must be achieved while ensuring the performance of the electrical appliances and meeting other individual requirements, otherwise it will be a waste of time. When wiring, it is mainly carried out according to the following principles:

①. In general, the power and ground wires should be routed first to ensure the electrical performance of the circuit board. As far as conditions allow, try to widen the width of the power and ground wires. It is best that the ground wire is wider than the power wire. Their relationship is: ground wire > power wire > signal wire. Usually the signal wire width is: 0.2~0.3mm, the thinnest width can reach 0.05~0.07mm, and the power wire is generally 1.2~2.5mm. For the PCB of digital circuits, a wide ground wire can be used to form a loop, that is, to form a ground network (the ground of analog circuits cannot be used in this way)

②. Pre-wire the wires with strict requirements (such as high-frequency wires). Avoid adjacent parallel wires between the input and output terminals to avoid reflection interference. If necessary, add ground wire isolation. The wiring of two adjacent layers should be perpendicular to each other. Parallel wiring is prone to parasitic coupling.

③. The oscillator housing should be grounded, and the clock line should be as short as possible and should not be led everywhere. The ground area under the clock oscillator circuit and the special high-speed logic circuit should be increased, and other signal lines should not be run, so that the surrounding electric field approaches zero;

④. Use 45° folded line wiring as much as possible, and do not use 90° folded line to reduce the radiation of high-frequency signals; (For high-quality lines, double arc lines should be used)

⑤. No signal line should form a loop. If it is unavoidable, the loop should be as small as possible; the number of vias of the signal line should be as small as possible;

⑥ Make the key lines as short and thick as possible, and add protective ground on both sides.

⑦. When transmitting sensitive signals and noise field band signals through flat cables, they should be led out in the form of "ground wire-signal-ground wire".

⑧. Test points should be reserved for key signals to facilitate production and maintenance testing.

⑨. After the schematic wiring is completed, the wiring should be optimized; at the same time, after the preliminary network check and DRC check are correct, the unwired area is filled with ground wires, and a large area of copper layer is used as the ground wire. On the printed circuit board, all unused areas are connected to the ground as ground wires. Or make a multi-layer board, with the power supply and ground wire occupying one layer each.

——PCB wiring process requirements

①. Line

Generally, the signal line width is 0.3mm (12mil), the power line width is 0.77mm (30mil) or 1.27mm (50mil); the distance between lines and between lines and pads is greater than or equal to 0.33mm (13mil). In actual applications, the distance should be increased when conditions permit.

When the wiring density is high, you can consider (but not recommend) using two lines between IC pins, with a line width of 0.254mm (10mil) and a line spacing of no less than 0.254mm (10mil). In special cases, when the device pins are dense and the width is narrow, the line width and line spacing can be appropriately reduced.

②. Pad (PAD)

The basic requirements for pads (PADs) and transition holes (VIAs) are: the pad diameter should be larger than the hole diameter by 0.6mm; for example, general pin-type resistors, capacitors and integrated circuits use pad/hole sizes of 1.6mm/0.8mm (63mil/32mil), and sockets, pins and diodes 1N4007 use 1.8mm/1.0mm (71mil/39mil). In practical applications, the size should be determined according to the actual size of the components. If conditions permit, the pad size can be appropriately increased;

The component mounting hole diameter designed on the PCB board should be about 0.2 to 0.4 mm larger than the actual size of the component pin.

③. Via

Generally 1.27mm/0.7mm (50mil/28mil);

When the wiring density is high, the via size can be appropriately reduced, but it should not be too small. You can consider using 1.0mm/0.6mm (40mil/24mil).

④． Spacing requirements for pads, wires, and vias

PAD and VIA: ≥ 0.3mm (12mil)

PAD and PAD: ≥ 0.3mm (12mil)

PAD and TRACK: ≥ 0.3mm (12mil)

TRACK and TRACK: ≥ 0.3mm (12mil)

At higher density:

PAD and VIA: ≥ 0.254mm (10mil)

PAD and PAD: ≥ 0.254mm (10mil)

PAD and TRACK: ≥ 0.254mm (10mil)

TRACK and TRACK: ≥ 0.254mm (10mil)

Fifth: Optimize wiring and silk screen. "There is no best, only better"! No matter how hard you think about designing, after you finish drawing, you will still feel that many places can be modified. The general design experience is: the time for optimizing wiring is twice the time for initial wiring. After you feel that there is nothing to modify, you can lay copper (Place->polygon Plane). Copper is generally laid for ground wires (note the separation of analog ground and digital ground), and it may also be necessary to lay power for multi-layer boards. When it comes to silk screen, be careful not to be blocked by the device or removed by vias and pads. At the same time, when designing, look directly at the component side, and the bottom layer of words should be mirrored to avoid confusing the layers.

Sixth: Network and DRC inspection and structural inspection. First, on the premise of ensuring that the circuit schematic design is correct, the generated PCB network file and the schematic network file are subjected to a network check (NETCHECK) of the physical connection relationship, and the design is corrected in time according to the output file results to ensure the correctness of the wiring connection relationship;

After the network check is passed correctly, the PCB design is checked for DRC, and the design is modified in time according to the output file results to ensure the electrical performance of the PCB wiring. Finally, the mechanical installation structure of the PCB needs to be further checked and confirmed.

Seventh: plate making. Before this, it is best to have an audit process.

PCB design is a job that requires careful thinking. The more careful and experienced you are, the better the board you will design. Therefore, you must be extremely careful when designing, and take all factors into full consideration (for example, many people do not consider the convenience of maintenance and inspection). If you keep improving, you will definitely be able to design a good board.

jaylu

Speaking of experience

rain

Yeah, it looks good too.

mdreamj

Good, it should be the essence

xjnqwjx

Thank you Moderator!!![Y]

sxy841012

Leave your name when you pass by, and leave your name when you pass by. Shi Xiaoyan came here for a visit~ ありがとうございます. a ri ga to go za i ma su .Thank you, Banzhu~