This post was last edited by Jacktang on 2018-3-11 17:33 1 Silkscreen design in RF PCB design 1.1 Device package silkscreen 1.1.1 The device package silkscreen line must not cross the device pads and other welding areas, and the spacing between pads must be greater than 20mil. 1.1.2 For devices with directional regulations, the silkscreen mark must indicate its direction. 1.1.3 For integrated device packages, the pin number and counting direction must be indicated. 1.2 Project code silkscreen 1.2.1 The size of the project code silkscreen characters shall be set according to the actual situation, with clear identification as the principle. 1.2.2 The position of the character silkscreen must be close to the attributed element, but cannot overlap with the package silkscreen and pads. 1.2.3 The directionality of the character silkscreen must comply with national standards. 1.3 Instructions and comments The size of the silk screen for instructions and comments shall be in accordance with Article 4.2.1, and the placement shall not cover the silk screen, pads, or project codes of other elements. 1.4 Silk screen line parameter design 1.4.1 All silk screen logos must be set on the silk screen layer. 1.4.2 The silk screen line width setting must be greater than 8mil. 2 Pad and via design in RF PCB design 2.1 SMT pad and via spacing setting In RF PCB design, the spacing between SMT pads and vias shall not be less than 10mil, and the spacing between SMT pad grounding vias and pads shall not be greater than 10mil. 2.2 SMT pads and vias. SMT pads shall not overlap or cover each other, and vias shall not overlap or cover each other. 2.3 Design requirements for RF board grounding vias 2.3.1 The design of RF board grounding vias shall follow the basic rule of not dividing the power and ground planes. 2.3.2 In the design of RF board, the number of via types should be minimized, and the number of via types in the whole board should not exceed 6. 3 RF PCB copper coating rules 3.1 Free flooding 3.1.1 The first rule of large-area copper coating is to ensure the closed requirements of the design plane. 3.1.2 Free flooding copper coating should ensure the smoothness of the closed line and avoid the generation of sharp corners and burrs. 3.1.3 When free flooding on the microstrip board, attention should be paid to the balance requirements of the microstrip line signal and the isolation interval setting of sensitive signals. 3.1.4 In the design of other functions, when free flooding, attention should be paid to the principles of international safety regulations to meet the requirements of withstand voltage test and electrostatic requirements. The test conditions are determined according to the characteristics of the system. 3.2 Directional filling 3.2.1 Directional filling should also follow the requirements of 6.1.1 to 6.1.4. 3.2.2 For RF boards, it is not allowed to design the filling area as a grid and window form to achieve full plane filling. 3.2.3 Directional filling should be connected with a certain network to avoid short circuits and other design errors in the design. 3.2.4 Pay attention to the setting of solder mask and the design of size for the filling area under the oscillator and other special devices. 3.3 Island processing 3.3.1 In RF PCB design, islands should be processed and configured accordingly, and they can be ignored in other designs. 3.3.2 In special cases, islands can be added to the printed circuit board to meet the requirements of electromagnetic compatibility design. 4 Solder mask design and processing 4.1 Solder mask layer setting 4.1.1 Since RF boards sometimes do not have solder mask, it is necessary to design corresponding parameters in the file, and different layers correspond to different solder mask layers. 4.1.2 For microstrip boards, special requirements for solder mask layers should be designed. 4.2 Solder mask window design Solder mask windows should be completely consistent with the corresponding window requirements. For solder mask windows for shielding grounding, good grounding should be ensured. 4.3 Microstrip board solder mask design requirements4.3.1 For printed boards with mass production and processing requirements, the needs of single board processing technology requirements must be considered and RF boards with solder mask must be designed. 4.3.2 When microstrip boards are processed in batches, the bottom layer must be designed without solder mask. 4.3.3 If the process requirements can reach a certain level, the peelable solder mask process can be used for processing. 5 RF PCB design slotting and hollowing design5.1 Layer distribution parameter setting5.1.1 The slotting and hollowing design must be designed in the drilling layer to ensure the correctness of the processing. 5.1.2 The slotting and hollowing line width parameter design shall not be greater than 10mil. 5.1.3 For slotting and hollowing design, the precise processing dimensions and accuracy requirements must be marked in the design. 5.2 Slotting parameter setting5.2.1 The slotting shall not split the power and ground planes. 5.2.2 The slotting shall consider the requirements of the whole board assembly process and the strength requirements of the printed board. 5.2.3 Electrical slots must meet the requirements of international safety standards. 5.2.4 The slot length of the RF board PCB design shall not be equal to 5.3 Hollowing parameter settings and wiring spacing 5.3.1 The spacing between the hollowing frame and the signal line and copper cladding must not be less than 20mil. 5.3.2 The spacing between the hollowing frame and the pads, vias, and components must not be less than 40mil. 6 RF PCB board thickness setting 6.1 Microstrip board thickness setting 6.1.1 In the design of RF boards, the thickness requirement for the microstrip board with a double-sided board structure shall not exceed 1.0mm. 6.1.2 For microstrip boards with a multi-layer structure, the thickness of the ground plane layer and the microstrip line wiring layer shall not exceed 0.5mm. 6.1.3 For RF boards with full-plane grounding on one side, a board thickness of 0.4mm is recommended. 6.2 Control board thickness setting For the thickness of the control board, please refer to the company standard 7 RF PCB layer stacking 7.1 RF microstrip board stacking 7.1.1 The double-sided microstrip board stacking structure uses the TOP layer for signal routing, and the BOTTOM layer uses a full-plane ground. 7.1.2 The four-layer microstrip board stacking structure should be as follows: microstrip line signal layer, ground plane layer, power layer, and ground plane layer. 7.2 RF multi-layer board stacking Except for the bottom layer of the microstrip board, which needs to be fully grounded, other RF boards can use general layer stacking technology. 8 RF PCB layout design 8.1 Basic layout of RF board 8.1.1 The digital part and the analog part should be separated. 8.1.2 The high voltage working area and the low working voltage area should be arranged separately. 8.1.3 The high-frequency and low-frequency circuits should be isolated. 8.1.4 The DC and AC areas should be clearly divided. 8.2 Special layout of RF board 8.2.1 For RF PCB layout, the RF input part and output part should be isolated and distributed, and straight and U-shaped structures can be used. 8.2.2 High-power RF transmitting circuit should be far away from low-power RF receiving circuit. 8.2.3 Ensure that there is at least one ground copper in the high-power area, and do not place vias. 8.2.4 The isolation of sensitive signals and other signals should be distributed according to certain circuit function principles. 8.2.5 High-speed digital signals and RF signals as well as sensitive signals should be isolated and distributed. 8.2.6 TTL circuits and microstrip circuits should be kept at a certain distance. 8.2.7 TTL circuits and ground planes and power planes should be kept at a certain distance. 8.2.8 The influence of long-distance transmission of key signals on signal delay should determine the distribution and location of high-speed devices. 8.2.9 Reasonable distribution of thermal effects and balanced weight stress on the entire board. 8.2.10 Fully consider the testability and debuggability of signals on the entire board. 9 RF PCB design and wiring process 9.1 Microstrip line wiring 9.1.1 Strictly limit the number of vias on the signal line and reduce the number of signal line transformation levels. 9.1.2 Strictly control the number, angle and width of the corners of the signal line. 9.1.3 The microstrip line should be as short as possible. 9.1.4 The microstrip line and other signal lines should maintain a balanced spacing setting. 9.1.5 The microstrip line should pay attention to the crosstalk and coupling to other signal lines. 9.1.6 The microstrip line wiring layer should maintain the stability of the transmission medium to avoid the reduction of transmission efficiency. 9.1.7 It is recommended to route the microstrip line on the TOP layer. 9.1.8 When routing the microstrip line, the closedness of the free loop and the area division of the ground plane should be maintained. 9.1.9 When using coupled microstrip lines, the crosstalk and radiation interference of the coupler to other signals should be considered. 9.2 Stripline Routing 9.2.1 In the RF board PCB design, the stripline is generally distributed in the inner layer. It is necessary to combine the transmission line theory and pay attention to the transmission conditions and impedance matching of the stripline. 9.2.2 Stripline routing must meet the requirements of data transmission rate. 9.2.3 When routing striplines, it is not allowed to cross adjacent layers twice. 9.2.4 When routing striplines, it is necessary to pay attention not to split its high-frequency loop and free crossing area. 9.2.5 In the direction of adjacent striplines, the stripline balance principle must be followed. 9.2.6 The terminal load on the stripline must be matched. 9.2.7 The terminal load driven by the stripline is preferably a single load. 9.2.8 If the stripline is to drive more than two loads, the load spacing must be balanced. 9.2.9 In the coupled stripline structure, the isolation interval with other sensitive signals must be maintained to ensure the EMI of the entire board. 9.3 Control lines, ground lines, power lines and other wiring 9.3.1 The routing should be as short as possible, and sharp inner corners should be avoided at corners. 9.3.2 The wiring used for the power supply and ground pins of components and the wiring of capacitors should be appropriately widened and as short as possible. 9.3.3 The minimum spacing between wires should meet the requirements of crosstalk suppression. 9.3.4 The number of vias on the same signal line should be reduced as much as possible. It is recommended that the number of vias should not exceed 3. 9.3.5 The longest connection of the signal line between two signal sources is less than 2000mil. 9.3.6 The number of line widths of the printed lines on the same PCB should be reduced as much as possible to achieve the overall balance requirements. 9.3.7 For signal routing with strict terminal impedance requirements, reasonable routing should be performed. 9.3.8 Sensitive signals should be kept away from high-frequency areas and clock signal lines. 9.3.9 The clock signal line should be designed to have a delay according to the characteristics of the components. 9.3.10 Differential signal lines should be designed to be tightly coupled according to their characteristics. 9.3.11 For different power supply circuits, it should be noted that signal wiring should not pass through other power supply areas. 10 RF PCB power distribution process 10.1 Single power supply distribution design 10.1.1 Distributed power supply design 10.1.1.1 For different functional circuits, single power supply adopts different methods, radial wiring and recursive wiring. 10.1.1.2 In RF PCB circuit design, single power supply must use noise suppression circuits for EMI control. 10.1.1.3 For the power supply of RF high-power amplifier circuits, common mode and differential mode noise suppression should be used. 10.1.2 Power plane design 10.1.2.1 When using power plane design for RF boards, it is important to isolate circuits of different frequency bands. 10.1.2.2 The power plane is usually used in the RF board and is applied in the multi-layer board design. 10.1.2.3 When using the power plane design, high-frequency loops and power noise should be avoided. 10.1.3 Power noise design 10.1.3.1 Reasonable selection of bypass capacitors is an effective way to eliminate power noise. 10.1.3.2 Reasonable layout of the power distribution structure can effectively reduce noise coupling. 10.1.3.3 According to the actual situation, reasonable configuration and routing of the filter capacitor can reduce the spread of power noise. 10.1.3.4 The power network should be kept at a certain distance from the microstrip line, strip line and high-frequency clock signal line. 10.1.3.5 Reasonable distribution of the power distribution structure on the connector interface can reduce the power loop area and connection impedance. 10.1.4 Rules for the use of power and ground plane design 10.1.4.1 Pay special attention to the coordination with the ground plane in the design of the RF board power supply, and try to use a close coordination. 10.1.4.2 The power input source and the grounding junction should be as close as possible to the wiring. 10.2 Multi-power distribution design 10.2.1 Multi-power distribution technology 10.2.1.1 Different power supplies occupy different printed circuit board areas. 10.2.1.2 Each power supply should have its own independent loop and ensure that the loop area is minimized. 10.2.1.3 In the multi-power design, there should be obvious isolation intervals and boundaries between different power supplies. 10.2.1.4 When distributing multiple power supplies, considering the actual situation of the circuit, different power supplies occupy different layers, but the closest matching relationship with the corresponding ground plane loop should be maintained. 10.2.1.5 In the multi-power distribution design, it is necessary to avoid signal lines in different power areas crossing other power loops and distribution areas. 10.2.1.6 In the design of using connectors to access and output multiple power supplies, it is necessary to ensure the distribution between different power loops and not to couple noise of different frequency bands into other power loops. 10.2.1.7 In the multi-power design, the safe distance between different power supplies must be ensured to meet the requirements of safety regulations. 10.2.2 High-current power design 10.2.2.1 The high-current design on the RF board must take into account the capacity limitation, and the power line of the power amplifier circuit must ensure sufficient width requirements. 10.2.2.2 The high-current wiring must consider the thermal effect of the entire board and the thermal influence of the material. 10.2.2.3 For the large-current loops that implement large-plane design, the safety margin of the power node must be ensured. 10.2.2.4 The high-current line must maintain a certain spacing area with other power loops. 10.2.3 Principles of multi-power and ground plane design 10.2.3.1 The multi-power design of the RF board must ensure the balanced layout of the corresponding power supply and its ground plane. 10.2.3.2 Different power planes must be tightly coupled with their ground loops to keep the loop area as small as possible. 10.2.3.3 For the connector current sink node of the multi-power design, the sink loop area should be minimized. 10.3 Design principles for power planes 10.3.1 The distribution principle of the power plane should ensure good coupling with the ground plane and maintain the balanced characteristics of the power supply. 10.3.2 In RF circuits, for microstrip boards, multiple power planes are generally not set separately, and the power supply is designed in the circuit functional area as much as possible. 10.3.3 For multi-layer high-speed circuit boards in RF systems, it is generally required that the power plane be designed with equal spacing from all signal layers to maintain signal integrity requirements.3 In the design of multiple power supplies, there should be clear isolation intervals and boundaries between different power supplies. 10.2.1.4 When distributing multiple power supplies, the actual situation of the circuit should be taken into consideration. Different power supplies occupy different layers, but they should maintain the closest coordination with the corresponding ground plane loop. 10.2.1.5 In the design of multiple power supply distribution, it is necessary to avoid signal lines of different power supply areas crossing other power supply loops and distribution areas. 10.2.1.6 In the design of using connectors to access and output multiple power supplies, the distribution between different power supply loops should be guaranteed, and noise of different frequency bands should not be coupled into other power supply loops. 10.2.1.7 In the design of multiple power supplies, the safe distance between different power supplies should be guaranteed to meet the requirements of safety regulations. 10.2.2 High current power supply design 10.2.2.1 The high current design on the RF board must consider the capacity limitation, and the power supply line of the power amplifier circuit must ensure sufficient width requirements. 10.2.2.2 High current wiring must consider the thermal effect of the entire board and the thermal influence of the material. 10.2.2.3 For large current loops that implement large plane design, the safety margin of the power supply node must be guaranteed. 10.2.2.4 The large current line must maintain a certain spacing area with other power supply loops. 10.2.3 Design principles for multiple power supplies and ground planes 10.2.3.1 The multi-power design of the RF board must ensure the balanced layout of the corresponding power supply and its ground plane. 10.2.3.2 Different power planes must be tightly coupled with their ground loops to keep the loop area as small as possible. 10.2.3.3 For the connector current sink of the multi-power design, the sink loop area should be minimized. 10.3 Design principles for power planes 10.3.1 The distribution principle of the power plane must ensure good coupling with the ground plane and maintain the balanced characteristics of the power supply. 10.3.2 In the RF circuit, for microstrip boards, multiple power planes are generally not set separately, and the power supply is designed in the circuit functional area as much as possible. 10.3.3 Multi-layer high-speed circuit boards in RF systems generally require that the power plane be designed with equal spacing from all signal layers to maintain signal integrity requirements.3 In the design of multiple power supplies, there should be clear isolation intervals and boundaries between different power supplies. 10.2.1.4 When distributing multiple power supplies, the actual situation of the circuit should be taken into consideration. Different power supplies occupy different layers, but they should maintain the closest coordination with the corresponding ground plane loop. 10.2.1.5 In the design of multiple power supply distribution, it is necessary to avoid signal lines of different power supply areas crossing other power supply loops and distribution areas. 10.2.1.6 In the design of using connectors to access and output multiple power supplies, the distribution between different power supply loops should be guaranteed, and noise of different frequency bands should not be coupled into other power supply loops. 10.2.1.7 In the design of multiple power supplies, the safe distance between different power supplies should be guaranteed to meet the requirements of safety regulations. 10.2.2 High current power supply design 10.2.2.1 The high current design on the RF board must consider the capacity limitation, and the power supply line of the power amplifier circuit must ensure sufficient width requirements. 10.2.2.2 High current wiring must consider the thermal effect of the entire board and the thermal influence of the material. 10.2.2.3 For large current loops that implement large plane design, the safety margin of the power supply node must be guaranteed. 10.2.2.4 The large current line must maintain a certain spacing area with other power supply loops. 10.2.3 Design principles for multiple power supplies and ground planes 10.2.3.1 The multi-power design of the RF board must ensure the balanced layout of the corresponding power supply and its ground plane. 10.2.3.2 Different power planes must be tightly coupled with their ground loops to keep the loop area as small as possible. 10.2.3.3 For the connector current sink of the multi-power design, the sink loop area should be minimized. 10.3 Design principles for power planes 10.3.1 The distribution principle of the power plane must ensure good coupling with the ground plane and maintain the balanced characteristics of the power supply. 10.3.2 In the RF circuit, for microstrip boards, multiple power planes are generally not set separately, and the power supply is designed in the circuit functional area as much as possible. 10.3.3 Multi-layer high-speed circuit boards in RF systems generally require that the power plane be designed with equal spacing from all signal layers to maintain signal integrity requirements.
提升卡
变色卡
千斤顶
京公网安备 11010802033920号
