Recently while routing a PCB, I came across the option to fill/pour my ground plane with either solid or hatched copper. I've also noticed that the old Arduino Duemilanove also had a hatched ground plane.
What benefits does a hatched ground plane have over solid ground plane and vice versa?
As others said, it's mostly because it was easier to manufacture than solid layers for various reasons.
They also can be used in certain situations where you need controlled impedance on a very thin board. The traces width needed to get 'normal' impedances on such a thin board would be ridiculously narrow but the cross hatching changes the impedance characteristics on adjacent layers to allow wider traces for a given impedance.
If for some reason you need to do this, you can only route controlled impedance traces at 45 deg to the hatch pattern. This approach greatly increases mutual inductance between signals and consequently, cross-talk. Also note that this only works when the size of the hatch is much less than the length of the signal's rise time, this normally correlates to the frequency of the digital signals in question. As such, as frequency increases you reach a point where the hatch pattern would have to be so tightly spaced that you lose any benefit vs a solid plane.
In summary: Never use a cross hatched ground plane, unless you're stuck in some really weird situation. Modern PCB construction and assembly techniques no longer require it.
Another reason to use hatched planes is for a flexible PCB. There are a number of benifits of a hatched plane vs a solid plane. A solid plane has the potential for cracking along a bend line, this is far less likely with a hatched plane. More importantly for a flexible PCB a hatched plane allows for more flexibility in the bends.
One more reason why hatched planes should be preferred for flexible PCBs is the drying process needed with the flexible material (Polyimide) prior to soldering. With a hatched plane, the moisture can exit the flexible carrier material, whereas it is trapped under solid planes.
I believe hatched ground planes are easier to solder on to due to their thermal properties. The counter to this is to use a solid plane but put solder reliefs around each pin/pad that you need to solder to on the ground plane.
Other then that I am not sure of other reasons, maybe others have an idea.
For me, I always use solid planes. It is easier to etch since there isn't a bunch of little things you have to etch off.
EDIT: I did some Google searching and found this page: http://www.diyaudio.com/forums/parts/89354-ground-planes-solid-vs-hatched.html
One common usage of hatched copper pour comes up when designing capacitive touch-sensing user-interface (buttons, sliders, etc.)
As touch introduced change in capacitance is around a pF (+- an order of magnitude, depending on actual implementation), you would like to minimize the baseline capacitance. The solid ground plane around the trace (connecting the button-pad and the controller measuring it) adds more parasitic capacitance than a hatched one. Application note from Texas on Capacitive touch sense (archived), mentioning this.
Cross-hatching avoids problems with large copper areas when using the toner transfer technique, or if a laser printer is used to generate photo-etch artwork. Now I use an inkjet printer to produce transparencies I don't usually bother with it. I use thermal reliefs if I need to make soldering easier on copper areas.
It's not so good from an environmental point of view, perhaps, as more copper has to be removed. OTOH, the copper can be reclaimed by commercial board makers, and doesn't end up in landfill, when the equipment containing the board is disposed of.
Mesh ground planes are use when making flexible PCBs. Using sold grounds makes the FPCB very stiff and causes mechanical breaking of traces on other layers. The Mesh ground plane is a higher inductance plane.
My understanding was that solid panes could cause bubbling during through-hole wave-solder processes due to outgassing from the laminate, but the slower heat/cool times of SMD reflow probably make this less of an issue -I have certainly seen some (very) old boards with bubbled copper planes.
Another issue can be the so called copper balance. https://www.multi-circuit-boards.eu/en/pcb-design-aid/copper-balance.html. If the copper balance between the two sides of a PCB is very different, the board is more likely to bend or twist due to different thermal properties of the two sides.
Mostly however it is used for flexible PCBs as that keeps the PCB more flexible and reduces the chance for breaks in the copper layer.
I suppose that modern production materials have much less of an issue with inbalanced copper.
hatch planes are good for a couple of applications. return path in flex circuits. I use them in areas to reduce thermal transfer. if you have something hot next to a thing you want to keep cool, hatched planes for gnd retruns into the cool areas can help a lot.
Another reason to use cross-hatching in a plane, according to IPC, to acquire a proper adhered solder mask into melting metal surface.
Other manufacturing issues are created by the crosshatch fill. It causes tiny bits of laminar to break away and possible deposit across traces causing shorts and breaks. It also makes the data very large. Large enough to cause issues in CAM, photoplotting and AOI.
There is an interesting article from Altium from 2020, about hatched grounplanes for what they are used today: Rigid flex PCBs and flex PCBs.
The reason for cross hatched copper planes in rigid PCB where adhesion problems.
This article will describe the history of cross-hatch planes, how they are made, the reason they were initially used in rigid PCBs, and their ongoing role and benefit today in flex and rigid-flex boards: https://resources.altium.com/p/history-and-use-cross-hatched-planes
Hatched plane reduce the magnetic field going vertically into the board.
