Solid Pour vs. Hatched or line pour.

[Falcon69]

So, which is better, electrically?

I personally like the 45 degree hatch look that you can do in DipTrace when pouring, but, what are the disadvantages or advantages over a solid pour?

[zapta]

Dave has a large (and very good) PDF about PCB layout somewhere. IIRC he says there that there is not reason this days to do hatched, just solid.

[tautech]

So, which is better, electrically?

I personally like the 45 degree hatch look that you can do in DipTrace when pouring, but, what are the disadvantages or advantages over a solid pour?

Some recent discussion here:
https://www.eevblog.com/forum/eda/pcb-2-layers-design/msg497231/#msg497231

[zapta]

"Polygon can either be “solid” fills of copper, or “hatched” copper tracks in a crisscross fashion. Solid fills are
preferred, hatched fills are basically a thing of the past."

David L. Jones,   PCB Design Tutorial, 2004.

[Falcon69]

Yes, but I personally like the look of hatch fills better.  My question was is there anything electrically advantaged or disadvantaged with using hatched vs. copper?

If there's no disadvantage, then I'll go hatched for my boards.

I was explained in a previous post that having a copper pour without it connected to ground with at least 2 vias so current can flow, could introduce noise into the circuit.  That makes sense to me.

But, with a hatched pour, there's not really any unconnected island, just little 0.2mm or so square holes all over the place.

[Mr.B]

I once designed and built a board that had many components and tracks top side and basically one big solid ground pour on the bottom.
Board size was 150mm x 150mm.
Using the "frypan" reflow method I had trouble with the board warping as it heated up.
A friend suggested that the hatch pour would have reduced the warping.
I am not sure as to how accurate that is, but it makes sense.

[tautech]

Dave has a large (and very good) PDF about PCB layout somewhere. IIRC he says there that there is not reason this days to do hatched, just solid.

It's in his Wiki:
http://www.alternatezone.com/electronics/pcbdesign.htm

[Neilm]

Hatched fills were used in the past as computers could handle the hatch easier than handling a solid area on the screen.

If you are just using it for a copper balance, then I suppose it doesn't really matter but personally, I look at hatch pattens and think "RF antennae". I use solid fills tied to 0V every 10mm or so.

[nctnico]

So, which is better, electrically?

I personally like the 45 degree hatch look that you can do in DipTrace when pouring, but, what are the disadvantages or advantages over a solid pour?

Sometimes hatched is preferred to lower the capacitance (for example on capacitive touch designs). As others suggested board warping and heat capacity could be reasons to use a non-solid pour.

[John_ITIC]

What is the purpose of pouring copper in the first place? The main reason in my designs is that the copper pour forms a low ESR power plane capacitance with the power plane below it. For example, if there is a power plane on the next layer then pour GND. Having proper, and as large as possible, power planes with low physical separation is very important for high-speed electronics with regards to power integrity. Of course, pouring a hatched pattern will not result in nearly as much plane capacitance as a solid pour.

http://speedingedge.com/right-first-time/

[IconicPCB]

Experience has shown that polygons are sometimes troublesome when generating Gerber files.

Drawn fill such as cross hatch for example does not rely on internal and external polygon abstractions in data. This "real" data results in a simpler Gerber structure albeit certainly larger file.
Further down the road "real" data may present fewer problems or reduced number of steps in processing data and checking it for manufacturability.

Personally I prefer "real" data. Additionally the board with hatched pours will end up with lower thermal mass, important when reflowing in some smaller ovens ( again from personal experience). 

[nctnico]

Of course, pouring a hatched pattern will not result in nearly as much plane capacitance as a solid pour.

Actually the fringe fields contribute much more to the capacitance between PCB traces than the copper area.