Issue link: https://iconnect007.uberflip.com/i/1457913
48 DESIGN007 MAGAZINE I MARCH 2022 margin in the final design. Remember also that these simulations are modeled with lossless copper and substrate material. Any real FR-4 PCB will start to have significant losses by 3 GHz, and these losses always help by lowering the peak currents and undesired coupling at very high frequencies. Application As we have seen, every copper structure on the PCB must be less than a half a wavelength, and preferably less than a quarter wavelength, for the highest frequency at which the struc- tures will be excited 6 . Here is how I apply the "less than a quarter wavelength" rule of thumb when I start laying out a PCB. I calculate what a quarter wave- length is for the highest frequency signal on my PCB, and I make a note of that. If I strategically place my vias at a distance less than this around my high-frequency copper pours I will be fine, and there will be some places where I can't maintain this spacing because of other routing requirements, and that's okay. In those places, you can skip one of the vias or place them as best you can at slightly larger distances and the PCB will still work. You can see this in Figure 11 where some vias appear missing because I had to dodge other traces on other layers; your design will still work. You probably can't tell your PCB soware tool that there is a constraint of a via every "X inches," but at the end of the design, you can set the visible grid to whatever you calcu- lated as the appropriate spacing and make sure that the grid is displayed and very bright. is will give you visual cues as to how you did placing the vias and where you may need to squeeze in more. A final note on stitching via hole sizes: If you look at some of the pic- tures of evaluation boards on the inter- net 2 , you will see that a lot of the time very large holes are used for the stitch- ing vias. is is because, in an X/Y view from the plane of the PCB traces, a large hole has a large copper width in the X and Y directions of the PCB. is large hole effectively makes a wall-like structure, instead of the "stake" that a smaller hole would produce, and it makes the stitching more effective at higher frequencies with a smaller number of drill holes needed. While using a large hole has advantages on a simple evaluation board, these large holes also block the routing channels needed for more complex PCBs. I usually use my design's minimum hole size for my stitching vias to keep my routing options open, and it works just fine. Figure 11: Having a ground pour on the outer signal layers helps when probing high-frequency signals; it is quite easy to place the scope probe ground spring into a nearby stitching via to make the ground contact. Even "slapping on" resistors and capacitors to fix design issues is easier when you have copper pours on the outer layers, and honestly: Who hasn't had to add a part to fix a prototype now and again?