Issue link: https://iconnect007.uberflip.com/i/884055
October 2017 • The PCB Magazine 15 PLANNING A PCB: SIGNAL INTEGRITY AND CONTROLLED IMPEDANCE CONSIDERATIONS ing plane. The result is an unbalanced current flow, delays in signal propagation delays, and increased series inductance. Cuts in the plane (Figure 5) show a discon- tinuity in the signal return current path. The return path has to go all around the gap in the plane. This will raise the characteristic imped- ance at the gap, and the opening can end up as an antenna. The sample shows a split plane where other signals are routed in the plane opening. Let's Talk about Crosstalk Another issue for both EMI and signal integrity is crosstalk. Crosstalk is a coupling to adjacent signals, GND or PWR connection, that is unintended. Crosstalk is normally seen as a major problem with cables, but it can also occur at the PCB level. Increased space between critical lines is normally the solution. And in some cases, the space can be used for less critical lines. Increased spacing is in gener- al very beneficial when coupling falls off with the square of the insulation distance. Increas- ing distance due to crosstalk, can also be an issue in the z-axis of the PCB. When a new PCB design is to begin, design- ers should start communication with manu- facturers at a very early stage. Start with the name/number of the PCB, then the following communication can be linked where it belongs. Do not communicate other PCBs in the same email/ticket. Unfortunately, this happens often and causes unnecessary misunderstandings and extra work. When you as a designer need a stack-up to start routing, there is some information that you need to pass on to the engineers at the PCB manufacturer, so they have a base to start on. What you will get back is a stack-up with values on your impedance traces that you can use in your CAD software. The strengths of PCB manufacturers have traditionally been: • PCB material knowledge • Lamination • Drilling • Plating • Etching • Surface treatment • Mechanical finishing The times have changed and electrical en- gineering is now part of what you get from the manufacturer. Electrical requirements such as impedance, plane capacitance, crosstalk and electrical testing is knowledge that you find in the engineering departments of the PCB manu- facturers who can handle advanced PCBs. This, in combination with your own knowledge and skills is the best combination for a successful stack-up, and well working PCB. The knowledge on how different laminates, types of glass styles, and resin content percentage work in the production process, are examples on knowledge PCB manufacturers know the best. Stack-up with Impedance Requirements Figure 6 shows a sample stack-up that re- flects the drill and via span—information a manufacturer must get before setting up a fi- nal stack-up. This information tells the manu- facturer that the following layers will be cop- per plated in addition to the etching. And that some layers also may need to be plated 2−3 times if there is a combination of mechani- cal and laser-drilled holes. It also informs that eventual holes shall be copper capped as well. Figure 6 also tells the total numbers of layers and where signal and plane layers are located. In addition, the follow information is needed: • Final thickness of the PCB • What impedances that are present on the various signal layers (single end and differential pairs) and their reference layers • Preferred minimum track width. This is valid information for manufacturers, to give the right values back for track widths, due to HDI and or fine-pitch components used in your PCB • If there are minimum distances between layers, due to crosstalk or other electrical reasons • If you have preferred materials, it can be dedicated materials or materials locked to a IPC 4101/(undergroup), you should mention it • Total size of the PCB