 Hello, this video will present selected layout guidelines for designs with STM32WL. We will focus on two main topics, component placement and RF layout. In the component placement part, we will discuss placement and routing of inductors and capacitors, the coupling capacitors, HSC crystal and SMPS. In the RF layout part, we will discuss transmission lines, discontinuities, bends, ground planes, bias and shielding and how to minimize unintentional radiation. The last short section will summarize sources where you can find more information, for example application nodes and reference designs. Let's move on to the first chapter about component placement. If placing capacitors or inductors, very short, thick connections are recommended. Wires must be placed as close as possible to the component. Here you can see examples of connections which are better to avoid. If you use thermal reliefs, it might increase parasitic inductance if used in the RF part. To get the best RF parameters, it's better to avoid them and use something like this. Pass around can reduce the parasitic inductance and bring better ground connection. If the part of the component is directly connected to the transmission line, it's good to align the part size with width of the transmission line. This can minimize discontinuities in the signal flow. If you place several inductors close to each other, it's good to minimize their mutual coupling by rotating them 90 degrees. When placing decoupling capacitors, a general rule of thumb is recommended. Capacitors with lower capacitance are placed close to the power supply pin at first. This is due to the fact that lower capacitors have higher resonance frequency and still behave like capacitors at higher frequencies. We can see it in this chart. At a certain high frequency, the 100 nanofarad capacitor behaves like inductor, but the 100 picofarad still behaves like a capacitor. It's also recommended to minimize the ground loop between the power supply pin and the decoupling capacitors. If a multi-layer PCB is used, the grounding layer should be as close as possible to the layer with components. In this slide, you can see the example of power supply pins of the QFN48 package and position of the decoupling capacitors on the reference board. When the crystal is used for the HSC oscillator, then the crystal might be affected by heat produced by the STN32WL. It might cause the tuning of the crystal frequency which has significant effect to the RF parameters. To minimize this effect, a thermal barrier is recommended. It is a gap in the ground plane layer which reduces the thermal flow from the STN32WL. If high frequency stability is needed in the design, then TCXO is recommended instead of crystal. In the SMPS part, the inductor must be placed as close as possible to the SMPS pins. Here we can see the examples with PGA and QFN packages. The ground plane, which is disabled in the pictures, is recommended below this section. Wide traces are also recommended if possible. The next section will focus to RF layout design. Fundamental part of the RF design is a transmission line, but what is it? We can say that it is a structure that guides the RF signal between RF circuits, for example RF switch and filter. One of the most important parameters is characteristic impedance. This impedance depends on geometric and material parameters of the layout and the PCB. Typical impedance in RF engineering is 50 ohms. It means that all components and interconnections among them should have this impedance. If this is fulfilled, there are no losses in the system. If some component has different impedance, then matching network is usually needed, as in this case when the antenna impedance is matched to 50 ohms at the working frequency. As it was mentioned, the characteristic impedance depends on geometrical and material parameters of the PCB. Main geometrical parameters are PCB height, trace width and gap between the trace and the ground. Scale parameters are characterized mainly by dielectric constant epsilon r of the PCB material. One of the widely used types of transmission lines is coplaying a wave guide with a ground plane. Commonly used abbreviations are CPWG, GCPW, etc. It consists of the main or active trace, two ground planes around and the ground plane below. In cross-section it looks like this. The top and bottom ground planes are connected by wires. Important mechanical parameters which determine impedance of the line are width of the trace, gap between the trace and the ground plane, thickness of the conductor and height of the substrate between the main trace and the ground plane. Here we can see some examples about how the characteristic impedance of a coplaying a wave guide depends on geometric parameters. If the width of the main trace is narrower, then the characteristic impedance is higher and vice versa. In the next figure we can see that the narrower gap between the trace and the ground plane sets a lower characteristic impedance and vice versa. The type of RF transmission line which is typically used in designs with STM32WL is differential transmission line. It consists of two parallel traces and the ground plane below. Typical impedance of this transmission line is 100 ohms. Here we can see it in the cross-section. Parameters that affect the characteristic impedance are width of the traces, gap between the traces, thickness of conductor and height of the substrate. The electric constant of the substrate has also impact. From the previous slides we know that the characteristic impedance depends on geometric and material parameters of the PCB. But how to get the right characteristic impedance based on these parameters? There are several options. We can use RF line calculators which implement relatively simple formulas. There are many such calculators available on the internet. The usage is quick and easy. For most cases it should be okay and it can give a result which is close to the real one. If the transmission line is more complicated, for example there are discontinuities or complicated layout around, then the results are not so precise. In this case, electromagnetic field simulator can give more precise results. Generally, it's based on some numerical method of solving Maxwell's equations. A disadvantage of this approach is that the simulation workflow is relatively slow and specialized software tools are needed. The next options how to apply the characteristic impedance correctly is to reuse the stackup and layout from reference boards. The disadvantage is limited use, especially when modifications are needed. Solid uninterrupted ground plane below transmission lines is very important. It is the error where the return current flows. If the return current flows directly to the transmission line, then the current loop is minimized. Here we can see examples of our evaluation boards. The solid ground plane is recommended under the whole RF section. Conditions on different layers must be stitched together by wires. Discontinuities occur when connecting parts with different characteristic impedance. This impedance mismatch causes a reflection of the transmitted RF power. Here we can see the example where two transmission lines with different widths are connected. The difference between widths is quite big and it causes the big discontinuity. A way to mitigate this problem is to use several smaller step discontinuities. The best way is to use a smooth transmission between the transmission lines. Another typical place where impedance discontinuities occur is at the junctions of transmission lines and pads. In this case it is recommended to have size of the pad aligned with width of the transmission line. Here we can see the typical example with an RF switch. Perpendicular bands of transmission lines are not recommended in RF. As you can see from the equivalent circuit, it adds another parasitic components which may affect the transferred signal. In this case a band of this shape is recommended. As partially mentioned earlier, big ground planes on different layers should be stitched together by wires. Typical distance among the wires can be calculated by the following formula where lambda or wavelength is calculated like this. For example, if we assume working frequency 900 MHz, 10th harmonic as the highest frequency and the effective permittivity of 3, then the recommended distance is between 1 and 2 mm. To minimize the unintentional radiation, more attention should be paid to the RF output part where the signal intensity is high and the spectral content of the signal is rich. Equivalent circuit of the power amplifier output stage is shown here. To minimize the unintentional radiation, it's recommended to flat the ground plane and stitch it with another ground layers by wires. If there are another sensitive technologies implemented around, the metal shield box can also help. In this slide we can see typical schematic and recommended layout with discrete components in the matching network. We can see all recommended rules. More information on this topic can be found in the application node 5407. Reference designs can be also used as a source of information. Thank you for watching. Bye!