Safety distance requirementsIncludes electrical clearance (spatial distance), creepage distance (surface distance) and insulation penetration distance.1. Electrical clearance: The shortest distance measured along the air between two adjacent conductors or between a conductor and the adjacent motor housing surface.2. Creepage distance: The shortest distance between two adjacent conductors or between a conductor and the adjacent motor housing surface measured along the insulating surface.1. Creepage distance and electrical clearance distance requirements:1. Creepage distance: When the input voltage is 50V-250V, the L-N before the fuse is ≥2.5mm; when the input voltage is 250V-500V, the L-N before the fuse is ≥5.0mm; electrical clearance: When the input voltage is 50V-250V, the L-N before the fuse is ≥1.7mm; when the input voltage is 250V-500V, the L-N before the fuse is ≥3.0mm; there is no requirement after the fuse, but try to keep a certain distance to avoid short circuit damage to the power supply;2. The primary side AC to DC part ≥ 2.0mm;3. The primary side DC ground to ground ≥4.0mm, such as the primary side ground to the earth;4. The primary side to the secondary side is ≥6.4mm, and the pitch of the components such as optocouplers and Y capacitors is ≤6.4mm, so slots should be cut;5. The insulation between the two poles of the transformer shall be ≥6.4mm and ≥8mm.
In Figure 2, when laying out the PCB, the driving resistor R3 should be close to Q1 (MOS tube), and the current sampling resistors R4 and C2 should be close to the 4th pin of IC1. As shown in Figure 1, R should be as close to the operational amplifier as possible to shorten the high impedance line. Because the input impedance of the operational amplifier is very high, it is easily interfered. The output impedance is low and not easily interfered. A long line is equivalent to a receiving antenna, which is easy to introduce external interference.
When layout in A of Figure 3, R1 and R2 should be placed close to transistor Q1. Because the input impedance of Q1 is very high, the base line is too long and is easily interfered, R1 and R2 cannot be far away from Q1.When layout in B of Figure 3, C2 should be close to D2, because the input impedance of Q2 transistor is very high. If the line from Q2 to D2 is too long, it is easy to be interfered. C2 should be moved near D2.2. Small signal traces should be kept as far away from large current traces as possible and should not be parallel to each other, D>=2.0mm.
3. Small signal line processing: The circuit board wiring should be concentrated as much as possible to reduce the board area and improve the anti-interference ability.4. When routing a current loop, minimize the enclosed area as much as possible.
Such as: current sampling signal line and signal line from optocoupler5. Optocoupler devices are prone to interference and should be kept away from strong electric and magnetic field devices, such as high current traces, transformers, high potential pulsating devices, etc.6. When supplying power to multiple ICs, pay attention to Vcc and ground wires.
Multiple grounding points in series cause mutual interference7. Noise requirements1. Try to reduce the area surrounded by the high-frequency pulse current as follows (Figure 1, Figure 2)
2. The filter capacitor should be as close to the switch tube or rectifier diode as possible, as shown in Figure 2 above. C1 should be as close to Q1 as possible, C3 should be close to D1, and so on.3. The area where the pulse current flows is far away from the input and output terminals, so that the noise source is separated from the input and output ports.
Figure 3: The MOS tube and transformer are too close to the input. The electromagnetic radiation energy directly acts on the input end. Therefore, the EMI test fails.Figure 4: The MOS tube and transformer are far away from the input, and the distance between the electric and magnetic radiation energy and the input end is increased, and they cannot directly act on the input end, so EMI conduction can pass through.4. The control circuit and the power circuit are separated and single-point grounding is adopted, as shown in Figure 5.
The components around the control IC are grounded to the ground pin of the IC; then the ground pin is led out to the ground wire of the large capacitor. The third pin of the optocoupler is connected to the first pin of the IC, and the fourth pin is connected to the second pin of the IC. See Figure 6.5. If necessary, the output filter inductor can be placed on the ground loop.6. Use multiple low-ESR capacitors in parallel for filtering.7. Use copper foil for low-inductance and low-resistance wiring. There should not be too long parallel lines between adjacent lines. Try to avoid parallel and vertical lines. Do not change the line width suddenly. Do not make sudden corners (ie: ≤ right angle). (Parallel lines in the same current loop can enhance anti-interference ability)8. Anti-interference requirements:1. Shorten the connection between high-frequency components as much as possible, try to reduce their distributed parameters and mutual electromagnetic interference, components that are susceptible to interference should not be too close to components with strong interference, and input and output components should be kept as far away as possible.2. There may be a high potential difference between some components or wires, so the distance between them should be increased to avoid discharge causing accidental short circuits.
Figure 1: The heat sink blocks the wind, which is not conducive to heat dissipation; Figure 2: Good ventilation is conducive to heat dissipation2. Keep a distance between capacitors, ICs, etc. and thermal components (heat sink, rectifier bridge, freewheeling inductor, power resistor) to avoid being affected by heat.3. Current loop: In order to facilitate threading, the lead holes should not be too far or too close.4. The input/output and AC/socket must ensure that the two wires are of the same length, leaving a certain amount of space margin. Pay attention to the position of the plug wire buckle, the convenience of plugging and unplugging, the neat output wire holes, and the good welding wires.5. Components cannot touch each other, and the screw positions of MOS tubes and rectifier tubes and pressure strips cannot touch other components, so as to simplify the assembly process as much as possible. Capacitors and resistors cannot touch pressure strips or screws. When laying out the board, you can consider the position of screws and pressure strips first. As shown in Figure 3 below:
6. Except for temperature switches, thermistors, etc., key components that are sensitive to temperature (such as ICs) should be kept away from heating elements. Devices that generate more heat should be kept at a certain distance from devices such as capacitors that affect the life of the entire machine.7. For the layout of adjustable components such as potentiometers, adjustable inductors, variable capacitors, micro switches, etc., the structural requirements of the entire machine should be considered. If they are adjusted inside the machine, they should be placed in a place on the PCB board that is convenient for adjustment. If they are adjusted outside the machine, their position should be consistent with the position of the adjustment knob on the chassis panel.8. Space should be reserved for the positioning hole bracket of the printed PCB board.9. Components located at the edge of the circuit board should generally be no less than 2mm away from the edge of the circuit board.10. Keep the output line, lamp line, and fan line in a row as much as possible, and keep the polarity consistent with the panel.11. General layout: Do not connect high voltage to the small board, and place high voltage components on the large board. If there are special circumstances, safety regulations must be considered. As shown in Figure 4, place R1 and R2 on the large board and introduce a low voltage line.12. The primary heat sink should be kept at a distance of more than 5mm from the outer casing (except for the wrapped wheat sheet).13. Pay attention to the height of the reverse side components when laying out the board. As shown in Figure 5:
14. Pay attention to safety regulations for primary and secondary Y capacitors and transformer cores.2. Layout requirements of unit circuits1. Arrange the positions of various functional circuit units according to the circuit flow, make the layout convenient for signal flow, and keep the signal in the same direction as much as possible.2. Take the core components of each functional circuit as the center and layout around it. The components should be arranged evenly, neatly and compactly on the PCB, and the connecting leads between the components should be minimized and shortened as much as possible.3. When working at high frequencies, the distribution parameters of components must be considered. In general, the components of the circuit should be arranged in parallel as much as possible. This is not only beautiful, but also easy to assemble and solder, and easy to mass produce.3. Wiring principles1. The wires used for input and output should be kept away from parallel adjacent wires as much as possible. It is best to add a ground wire between the wires to avoid feedback coupling.2. The width of the trace is mainly determined by the adhesion strength between the conductor and the insulating substrate and the current value flowing through them. When the copper foil is 50μm thick and 1mm wide, the temperature rise will not exceed 3℃ when a current of 1A flows through it. Based on this, it can be inferred that a 2-ounce (70μm) thick copper foil with a width of 1mm can flow a current of 1.5A and the temperature rise will not exceed 3℃ (Note: natural cooling).3. The electrical clearance width between the input control circuit part and the output current and control part (i.e. the distance between the small current wiring and the output wiring) is: 0.75mm--1.0mm (Min 0.3mm). The reason is that if the copper foil and the pad are too close, it is easy to cause a short circuit and also easy to cause adverse reactions of electrical interference.4. The bends of the ROUTE line are generally arc-shaped, while right angles and acute angles will affect the electrical performance in high-frequency circuits.5. According to the size of the line current, the width of the power line should be as thick as possible to reduce the loop impedance. At the same time, the direction of the power line and the ground line should be consistent with the direction of data transmission to reduce the surrounding area, which will help enhance the anti-noise ability.A: Most heat sinks also use single-point grounding to improve noise suppression capabilities as shown below:
After change: Single-point grounding has no magnetic field loop, and EMI test is OK.7. Filter capacitor routingA: Noise and ripple are completely filtered out by the filter capacitor.
B: When the ripple current is too large, multiple capacitors are connected in parallel, and the ripple current passes through the first capacitor. When the ripple current is too large, multiple capacitors are connected in parallel, and the ripple current passes through the first capacitor. The heat generated is also greater than that of the second and third capacitors, and it is easy to be damaged. When routing, try to evenly distribute the ripple current to each capacitor. The routing is as shown in Figures A and B below. If space permits, the routing method in Figure B can also be used.
8. The pin of the high-voltage and high-frequency electrolytic capacitor has a rivet, as shown in the figure below. It should be kept away from the top layer of copper foil and comply with safety regulations.
During mass production, the magnetic core of the current sampling line collided with the copper foil of the line, causing a malfunction.10. Do not run high-voltage lines under metal film resistors, and try to run low-voltage lines in the middle of the resistor. If the resistor is broken, it is easy to short-circuit with the copper wire below.11. Add tin:A: Add tin to the narrower copper foil of the power line;B: RC absorption circuit, not only does it require tinning due to the large current, but it is also conducive to heat dissipation;C: Add tin under the thermal component to dissipate heat. Do not press the pad when adding tin.12. Signal lines cannot pass through transformers, heat sinks, or MOS pins.13. If the output is superimposed, the capacitor before the differential mode inductor is connected to the front end ground, and the capacitor after the differential mode inductor is connected to the output ground.
A: Try to reduce the area enclosed by the high-frequency pulse current. The area enclosed by the five loops marked in the figure above should be as small as possible.B: Keep the power line and ground line as close as possible to reduce the area they surround, thereby reducing the electromagnetic interference caused by the cutting of the external magnetic field loop and reducing the external electromagnetic radiation of the loop.C: The large capacitor should be as close to the MOS tube as possible, and the output RC absorption loop should be as close to the rectifier tube as possible.D: The wiring of power lines and ground lines should be as thick and short as possible to reduce loop resistance. The corners should be smooth and the line width should not change suddenly as shown in the following figure:
15. The first layer of wire cannot be placed under the magnetic ring of the I-shaped inductor, power resistor, heat sink, and manganese copper wire vertical transformer core.16. The distance between the slot and the copper foil for routing should be more than 10MIL, and pay attention to the safety regulations of the upper and lower metal parts.
17. The driving transformer, inductor, and current loop must be consistent at all ends.18. Double-sided boards generally have more vias at high current routing locations, and the vias should be tinned to increase current-carrying capacity.19. In a single-sided board, the jumper should not touch other components. If the jumper is connected to a high-voltage component, it should maintain a certain safety distance from the low-voltage component. At the same time, it should maintain a distance of more than 1mm from the heat sink.IV. Case AnalysisThe size of switching power supplies is getting smaller and smaller, its operating frequency is getting higher and higher, and the density of internal devices is getting higher and higher, which puts more and more stringent requirements on the anti-interference of PCB wiring. For the wiring of some cases, the problems found and their solutions are as follows:1. Overall layoutCase 1 is a six-layer board. The first layout is to place the control part on the component side and the power part on the solder side. During debugging, it was found that the interference was very large. The reason was that the PWM IC and the optocoupler were placed in an unreasonable position, such as:
As shown in the figure above, the PWM IC and the optocoupler are placed under the MOS tube, and there is only a 2.0mm PCB layer between them. The MOS tube directly interferes with the PWM IC, which was later improved as follows:
Move the PWM IC and optocoupler away from each other, and make sure there are no devices with pulsating components flowing above them.2. Routing issuesThe power routing should be as short as possible to reduce the area surrounded by the loop and avoid interference. Small signal lines have a small area, such as the current loop:
The larger the area covered by A and B lines, the more interference it receives. Because it is a feedback coupler, the feedback line should be short and no pulsating signal can cross or run parallel to it.
The current sampling line and drive line of the PWM IC chip, as well as the synchronous signal line, should be kept as far away as possible when routing, and should not be routed in parallel, otherwise they will interfere with each other. The current waveform is:
During layout, the direction of the DIP packaged IC must be placed perpendicular to the direction of the soldering furnace, not parallel, as shown in the figure below; if there are difficulties in layout, the IC can be placed horizontally (the placement direction of the SOP packaged IC is opposite to that of the DIP).
The wiring direction is horizontal or vertical. From vertical to horizontal, it is necessary to go 45 degrees. If the width of the copper foil entering the round pad is smaller than the diameter of the round pad, a teardrop is required. The wiring should be as short as possible, especially the clock line, low-level signal line and all high-frequency loop wiring should be shorter.The ground wires and power supply systems of analog circuits and digital circuits should be completely separated. If there is a large area of ground wires and power line areas on the printed circuit board (area exceeding 500 square millimeters), a window should be opened locally. As shown in the following figure:
The distance between the center of the pins of horizontally inserted components (resistors, diodes, etc.) must be 300mil, 400mil and 500mil. (If not necessary, 240mil can also be used, but it is used with IN4148 diodes or 1/16W resistors. 1/4W resistors start from 10.0mm) The distance between the center of the jumper pins must be 200mil, 300mil, 500mil, 600mil, 700mil, 800mil, 900mil, 1000mil. The diameter of the heat dissipation hole on the PCB board cannot be greater than 140mil.If there are holes larger than Φ12 or square holes larger than 12MM on the PCB, a hole cover must be made to prevent the solder from flowing out, as shown below (the hole is 1.0MM)
In order to improve the accuracy of mounting the SMD components on the PCB, the PCB must be provided with calibration marks (MARKS), and each board must have at least two marks, which are set on a set of diagonal corners of the PCB, as shown below:
The center hole of the component pad should be slightly larger than the lead diameter of the device. If the pad is too large, it is easy to form a cold solder joint. The outer diameter D of the pad is generally not less than (d+1.2) mm, where d is the lead hole diameter. For high-density digital circuits, the minimum pad diameter can be (d+1.0) mm. The pad with a hole diameter greater than 2.5 mm should be appropriately enlarged. The components should be placed neatly and in the same direction as much as possible.For the SMD components on the PCB, the long axis line should be arranged perpendicular to the long axis line of the PCB board as much as possible to prevent them from breaking.
提升卡
变色卡
千斤顶
京公网安备 11010802033920号
