Hello, I’m working on a 4-layer PCB with the top and bottom layers designated for signals and the inner two layers for ground and power. I’m adding ground pours on both the top and bottom layers to streamline the routing, but I’m concerned about potential issues, especially impedance, as my project involves USB C 2.0.
//Quote// Adding ground pours on both the top and bottom to streamline routing…
How exactly does adding ground copper streamline routing? Adding ground copper can improve the copper balance for warp, etching, and plating. It can also be useful in improving signal integrity and EMI. But it can also affect signals / EMI good or bad depending on how it is applied.
If you are concerned that the surface ground pours will inadvertently change specific impedances, I recommend that you configure a rule or keepout to maintain a larger minimum distance from those nets. Online impedance calculators can help you determine at what point that adjacent polys can start having an effect…and then stay a lttle farther away.
Are the USB signals going to be routed on both side of the board? Ideally it is preferable to use the same signal return reference for both sides of the board versus GND and PWR as your stckup suggests. To get around that, you can make the PWR layer a split PWR layer and add GND under the USB signals so the USB return reference is the same for both sides. Also be sure to add stitching vias to tie the various GND polygons together - especially at both ends of the USB signal paths. What you do not want are ground poly areas (or slivers) that are only connected on one end of a pour (which can become an unintentional antenna).
1 Like
Adding ground pours on both the top and bottom must be done with care. The biggest problem I’ve seen with this is the tendency to use a ground pour to make ground connections to several components and then use a single via to connect the fill to a plane layer. Is this what you mean by streamlining routing? Components need to connect to plane layers by the shortest route possible to decrease the connection inductance. Using an area fill to make this connection can make this route very long and increase this inductance. If you are going to add ground pours, first connect all components to the plane layer with a via at each ground pad and then add the pour.