In addition to the impedance of the RF signal line, the laminated structure of the RF PCB single board also needs to consider issues such as heat dissipation, current, devices, EMC, structure and skin effect. Usually we are in the layering and stacking of multilayer printed boards. Follow some basic principles:
A) Each layer of the RF PCB is covered with a large area without a power plane. The upper and lower adjacent layers of the RF wiring layer should be ground planes.
Even if it is a digital-analog mixed board, the digital part can have a power plane, but the RF area still has to meet the requirement of large-area paving on each floor.
B) For the RF double panel, the top layer is the signal layer, and the bottom layer is the ground plane.
Four-layer RF single board, the top layer is the signal layer, the second and fourth layers are ground planes, and the third layer is for power and control lines. In special cases, some RF signal lines can be used on the third layer. More layers of RF boards, and so on.
C) For the RF backplane, the upper and lower surface layers are both ground. In order to reduce the impedance discontinuity caused by vias and connectors, the second, third, fourth, and fifth layers use digital signals.
The other stripline layers on the bottom surface are all bottom signal layers. Similarly, the two adjacent layers of the RF signal layer should be ground, and each layer should be covered with a large area.
D) For high-power, high-current RF boards, the RF main link should be placed on the top layer and connected with a wider microstrip line.
This is conducive to heat dissipation and energy loss, reducing wire corrosion errors.
E) The power plane of the digital part should be close to the ground plane and arranged below the ground plane.
In this way, the capacitance between the two metal plates can be used as a smoothing capacitor for the power supply, and at the same time, the ground plane can also shield the radiation current distributed on the power plane.
The specific stacking method and plane division requirements can refer to the “20050818 Printed Circuit Board Design Specification-EMC Requirements” promulgated by the EDA Design Department, and the online standards shall prevail.
2
RF board wiring requirements
2.1 Corner
If the RF signal traces go at right angles, the effective line width at the corners will increase, and the impedance will become discontinuous and cause reflections. Therefore, it is necessary to deal with the corners, mainly in two methods: corner cutting and rounding.
(1) The cut corner is suitable for relatively small bends, and the applicable frequency of the cut corner can reach 10GHz
(2) The radius of the arc angle should be large enough. Generally speaking, ensure: R>3W.
2.2 Microstrip wiring
The top layer of the PCB carries the RF signal, and the plane layer under the RF signal must be a complete ground plane to form a microstrip line structure. To ensure the structural integrity of the microstrip line, there are the following requirements:
(1) The edges on both sides of the microstrip line must be at least 3W wide from the edge of the ground plane below. And in the 3W range, there must be no non-grounded vias.
(2) The distance between the microstrip line and the shielding wall should be kept above 2W. (Note: W is the line width).
(3) Uncoupled microstrip lines in the same layer should be treated with ground copper skin and ground vias should be added to the ground copper skin. The hole spacing is less than λ/20, and they are evenly arranged.
The edge of the ground copper foil should be smooth, flat, and no sharp burrs. It is recommended that the edge of the ground-clad copper is greater than or equal to the width of 1.5W or 3H from the edge of the microstrip line, and H represents the thickness of the microstrip substrate medium.
(4) It is forbidden for RF signal wiring to cross the ground plane gap of the second layer.
2.3 Stripline wiring
Radio frequency signals sometimes pass through the middle layer of the PCB. The most common one is from the third layer. The second and fourth layers must be a complete ground plane, that is, an eccentric stripline structure. The structural integrity of the strip line shall be guaranteed. The requirements shall be:
(1) The edges on both sides of the strip line are at least 3W wide from the upper and lower ground plane edges, and within 3W, there must be no non-grounded vias.
(2) It is forbidden for the RF stripline to cross the gap between the upper and lower ground planes.
(3) The strip lines in the same layer should be treated with ground copper skin and ground vias should be added to the ground copper skin. The hole spacing is less than λ/20, and they are evenly arranged. The edge of the ground copper foil should be smooth, flat and no sharp burrs.
It is recommended that the edge of the ground-clad copper skin is greater than or equal to the width of 1.5W or the width of 3H from the edge of the strip line. H represents the total thickness of the upper and lower dielectric layers of the strip line.
(4) If the strip line is to transmit high-power signals, in order to avoid the 50 ohm line width being too thin, usually the copper skins of the upper and lower reference planes of the strip line area should be hollowed out, and the width of the hollowing out is the strip line More than 5 times the total dielectric thickness, if the line width still does not meet the requirements, then the upper and lower adjacent second layer reference planes are hollowed out.