 Hello, welcome to RF guidelines for STM32WB session. In the first part, we deal with components, schematic and matching network for design to design RF path for STM32WB. Watching this video, you get basic information about the layout of RF path for STM32WB. Also you get the comprehensive information for PCB technology. In this part, we explain basic differences between commonly used RF lines and show a couple of examples of size and impedance calculations. To start several remarks, FL4 material is commonly used in RF design. It is widely used mostly for its mechanical and electrical insulating values. Also it is the cheap material. On the other hand, it has not too much stability of the dielectric constant and losses over the frequency and over the temperature. For higher frequencies it is better to use more capable materials which are dedicated for microwaves. It reports better losses and better stability over the frequency. They are also more expensive. But for designs where the RF line is short, FL4 is sufficient material especially at lower frequencies as Bluetooth band is. You can often meet with stacked up substrates. It uses multiple layers. These are widely used where the application of several layers is necessary. It helps also with EMI, signal integrity and to separate individual signals from each other. In these cases is need to care about the determination of the right RF reference plane. There exist the rules for distribution of the each layer. Each layer is dedicated for one or more kind of signal. So as an example best solution for four layer board is to put the signal layers as close to supply layers between supply layer and ground layer to use thicker dielectricun. Tight coupling between signal and supply layer decreases crosstalks. For the sixth layer board is the best to put two signal layers between and close to supply layers. The inner layers should be used for fast signals and the outer ones for slow signals. It helps a lot to EMI. Other rules are the same as for four layer board. The top and ground layer are also for RF line. And now we can move to RF lines. Common lines used in PCB layout aren't suitable for transmission and RF power. All transmission lines have resistance, inductance and capacitance. These parameters create the complex impedance of the RF line. Therefore the impedance is frequency dependent. The RF line has to be well defined for transmitting the signal. Each component connected to RF line has the input and output impedance. If the connected impedances are equal to each other, exactly complex conjugated, then we talk about impedance matching. The transmitted power is maximized. In other words, the system is in resonance. And the real parts of the impedances are equal. It is the state we want to reach. The impedance that is almost used in RF system is 50 ohm. There were developed several types of RF lines for PCB. They are suitable for various configurations, each has its own features. We are commonly meet with two basic ones. It is grounded coplanar waveguide. The grounded coplanar waveguide consists of the signal conductor, top ground layer and bottom ground layer. The impedance is determined by width of the conductor, gap between signal conductor and top ground plane, height between the top and bottom ground plane, thickness of the top layer and dielectric constant of the dielectric material. Advantage of this RF line is modification of the impedance with only changing the gap without changing the width. It is really needed in several cases. It also includes wires that should be at most lambda over 10 apart. There exist many various tools on the web. Note that they do not give the exactly same results. It is caused by including further minority influences. The second most used is microstrip line. Microstrip line consists of the signal conductor and bottom ground layer. As you can see, it is much simpler. The line impedance is determined by width of conductor, height between the top conductor and bottom ground plane, thickness of the top conductor layer and dielectric constant of the substrate. Advantage of this line is better compatibility with antenna, mainly for chip antennas. There exist many calculators on the web as similarly as for grounded Coplanar waveguide. Here we have the example of grounded Coplanar waveguide. Let's have four layers stack up. The definition of each layer is given by the table. Although the core and prepreg materials are the same, they have a bit different dielectric constant and dissipation factors. It is due to their various thicknesses, density and placement of fibreglass inside. The task is what is the trick with for one choosing gap and different reference planes. Let's calculate it. For calculation, we can use several available tools. We enter the dielectric constant dissipation factor, sometimes called as lost tangent, requested impedance 50 ohm and frequency 2.45 GHz. We also fill in the gap value for example 0.5 mm, height of the substrate 76 mm and conductor thickness on the top layer. We will get the width, physical length, loss and recalculated impedance. We will make it for both reference planes. So in second case, the change of height is 315 µm. We can see that in both cases, we are able to obtain the same impedance for different widths and heights. Let's summarize these results to the table. Although impedances are almost the same, the widths are different. From perspective of difficulty of manufacturability, the width of the line in the first case is on the limit of class 7. That is more expensive than to second case where class 3 is enough. Even the loss of the RF track is higher against the second case. It is a marginal due to very short line for most applications with STN32WB. The point is that it is necessary to take care about preservation of the PCB class or choose suitable stick up even for other impedances used on the board. It is also advisable to use track widths such as pet sizes of inserted components. Then the RF path is almost without discontinuities. This is in terms of line width but this feature can be used advantageously. Now we will show how to handle with this feature. It is possible to define the same impedance for various dimensions of width and gap as the follow chart shows. You are able to keep the same gap between trace and ground or to preserve the same width of trace in case of changing the impedance as it is for example by APD. In microstrip structure is possible only one width value. In this example it is equal to 0.63 mm. Sometimes it is an advantage to define the sizes of RF track in grounded Coplanar wave guide for the same width as for microstrip system. Track without discontinuity when switching to the microstrip leading to the antenna. Now you are able to calculate right RF line dimensions. Let's see further layout requirements. Now we focus on layout. Design of the correct layout is one of the critical point in design process. We will list several issues in which designers make mistakes. SMPS layout for external components. Sometimes it is a critical point. The SMPS is widely used and in case of bad implementation several spurious can appear in output spectrum. Another recommendation to place all component close to the appropriate pins of the chip. To keep traces as short as possible. To use sufficient track width and enough number of ground wires close to the ground pads. For better noise performance is recommended to add 10 nanohenry inductor as mentioned in previous session. To keep other components farther from SMPS components to limit interferences caused by coupling. The IPD doesn't need matching network at its input. There is necessary to preserve the length of the trace to 1.5 mm and the impedance that is close to 60 ohm. Depicted dimensions are valid only for mentioned stack up. Dialectric material, thickness and dielectric constant. For your application you need to recalculate them. Just use the GCPW calculator for getting right size of the track for different dielectric material, height of stack up substrates. The ground wires should be close to ground pads. In the first session we deal with matching network. There are several rules for placement. In case of low pass or bent pass filter you should use the matching network between the chip and the filter. Choose P or T structure. In most cases only two positions will be used at final. Use small packages for passive components. They have less parasitics and they are more suitable for higher frequencies and track size. Put them together as close as possible. The inserted track is part of the matching structure and thus contributes to the mismatch. Often his influence is forgotten. You should use the ground wires close to the ground pads. Do remember that even wire has its inductance. The matching network should be close to the output of the chip. Keep the RF traces short due to losses and due to radiation. Unsuitable length and mismatch can cause the track becomes a radiator. Similarly we can consider about matching network between the filter and the antenna. Here are some recommendations. Between the filter and the antenna should be the matching network. Again there are a couple of possibilities. It is P or T structure. In most cases it will reduce into two components one parallel and one serial one. Use small component packages. As we mentioned previously it has less parasitics and it is more suitable for track dimensions. You should use more steady components to keep their features. Put them together as close as possible to have real matching structure. These components should have a common ground. Use ground wires close to the ground pads. Always the RF currents should have short return path. The matching network should be close to the antenna port. Realize that the track connected to the antenna can behave as a radiator or untune the resonance frequency. If possible keep the RF traces short as well defined in one RF trace system. Define sufficient ground plane size and solid one. Often the reference board for the antennas are much bigger than finally implemented on the customer board. The size of the board and so the ground plane size influences resonance frequency, return loss and efficiency. In very small PCBs it can impact even the antenna structure as it needs to be mirrored in the ground due to its functionality. We briefly mentioned the ground plane and wires. Proper placement of wires on the ground is important for our design. It is often forgotten. The ground plane should be well defined over the PCB. All ground layers regarding RF have to be connected together. When we talk about ground on the top side of PCB very important is to be along the RF trace in certain dimensions from signal conductor in case of grounded coplanar wave guide and in non-effective proximity in case of microstrip line. Along the grounded coplanar wave guide track should be also wires in enough amount. They are placed close to the edge of the ground plane. Regarding wires near the antenna they have to be on the edge of the ground plane that defines antenna ground and couple of them in the ground surface of PCB. They provide the connection to the bottom ground plane or inner plane if defined as reference ground. And last but not least the ground plane has to be well connected to the ground pin of the chip. In close proximity of the ground pin should be placed the ground wire. Hope this helps you to design your own board with STN32WB and you will reach the best RF performance. In case of any questions ST is here for you.