Issue link: https://iconnect007.uberflip.com/i/1391285
JULY 2021 I DESIGN007 MAGAZINE 29 nection points from layer to layer is better. Floating copper will have some resonance frequency to it. You will not know what that is as you design your board. Smaller pieces of copper will resonate at a higher frequency than larger pieces due to the propagation times that bounce at the edges. So generally, we try to tie any larger sections down to other layers with a via and not have long meandering sections just creating mini antennas all over the board. e decision to use ground flooding or not should be made on a case-by-case basis, based on signal frequency and noise margins associ- ated with that. In my experience it usually does not hurt if done properly. Be mindful of the increased risk of shorts in the manufacturing process if the polygon to other copper value is set too low. Just because a manufacturer can do a minimal gap does not mean that minimal gap will give you the best yield. Always be design- ing for the best costs and yields. Eric Bogatin: It is never a good practice to flood copper on unused regions. Use a dot pattern to get more uniform copper plating and to bal- ance the copper, but do not flood copper. It provides no value and will oen create more problems than it could ever, in the best case, potentially solve. Lee Ritchey: ere is no good reason to flood unused space in signal layers with ground. It just makes the Gerber files much larger, and it might actually hurt signal integrity if done incorrectly. Cherie Litson: No, not always. If you only have a few traces on a layer, then flooding that layer with copper and tying it to GND or PWR will balance the fabrication process and decrease your bow and twist. If I have an RF board, I have to be careful where I'm creating capaci- tance between the layers or where I need to have no copper as it will interfere with Blue- tooth signals. DESIGN007 is six-layer stack-up is simply one example. is technique can be used on all PC boards: four-layer boards, or 8, 10, 12, 20, or 40 layers. Chris Young: ere is no one answer that fits all situations when it comes to flooding routing layers with copper (usually GND). ere are a lot of factors that should be considered, and I suggest taking a needs-based approach. Here are some reasons that I have flooded a layer or a region with copper: • To increase the heat capacity of a PCB to improve its heat-sinking capability • To provide copper balance in a PCB where thieving is not allowed • To reduce the difficulty for a PCB fabrica- tor to meet multiple controlled impedance requirements within a single PCB • To strengthen a PCB to make it more resilient to mechanical stress • To shield a signal from unwanted noise or other aggressor signals Heidi Barnes: Flooding all unused areas with copper is kind of a funny way to put it, since the copper is already there, and it comes for free. CAD tools start with a blank PCB and put copper down. A real PCB starts with cop- per and then etches away what is not needed. e RF/microwave world has been doing solid fill with vias for a long time to provide shield- ing and very low impedance ground. One can even add edge plating to take the shielding and low impedance a step further. Maximizing the copper ground fill can also add mechani- cal strength. However, one does need to watch the stackup symmetry to avoid warping, and etch uniformity oen leads to cross-hatched ground fill instead of solid fill. Carl Schattke: is will vary from project to project and intended application. Generally speaking, more ground is better. More con-