So recently when i was routing a PCB , I came across the option to either 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.

So what benefits does a hatched ground plane have over solid ground plane and vice versa.

  • 2
    A hatched plane must weigh a tiny bit less... could that ever matter? – joeforker Oct 12 '10 at 20:05
  • 2
    We've gone plaid! – joeforker Oct 12 '10 at 20:05
  • 2
    I cannot image a situation where the weight of the board would matter to that precision where a different change did not make it better. – Kortuk Oct 13 '10 at 1:37
  • 1
    I know large solid ground planes have a completely different heat up rate compared to non-ground plane. This effect reflow soldering. I could see hatching having an effect in this, but I would imagine it would be small. – Kellenjb Oct 13 '10 at 3:02

11 Answers 11

up vote 22 down vote accepted

As others said its 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 your stuck in some really weird situation. Modern PCB construction and assembly techniques no longer require it.

  • Crosshatched should be used specifically for increasing impedance of the traces. With a small crosshatch(ie. no traces go over a gap together) there will not be many crosstalk problems but give you the impedance you need. – Kortuk Oct 12 '10 at 20:50
  • I already gave you a +1, but please edit to note that the crosshatching should only be used in an impedance situations. It is still acceptable for high speed signals, you just need to make sure traces are sufficiently separated to stop crosstalk. – Kortuk Oct 12 '10 at 20:58
  • i don't completely agree, but i edited to replace my general language with more specific issues as frequency increases – Mark Oct 12 '10 at 22:42
  • the hatched ground plane does not have to decrease in size with frequency, it must decrease in size with relation to trace spacing to remove crosstalk. – Kortuk Oct 13 '10 at 1:34
  • 1
    In general, I agree. Never use hatched ground planes. This will be true for 99% of people. If you need one and realize it, you probably do not care our opinion, as you know your stuff. – Kortuk Oct 13 '10 at 1:34

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:

  • This is not correct vikram. This is a confusion between hatched ground planes and thermal relief. Mark is correct here. – Kortuk Oct 12 '10 at 22:05
  • After doing much internet surfing for trying to figure this out I am still unsure. Pretty much everything I see online points to this being a fabrication issue. However, I was shown a book that talks about it being an impedance issue. Currently I am leaning toward trusting the book. If the book is correct, my answer is not the correct answer. – Kellenjb Oct 12 '10 at 23:22
  • 3
  • That is what I referenced. – Kortuk Oct 13 '10 at 14:09
  • @Kortuk: I would guess cross-hatched ground planes probably came about when automated tools didn't do thermal reliefs. – supercat May 14 '11 at 15:11

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.

  • Don't modern commercial board makers start with a very tiny amount of copper on the board, only to build up the rest with electroplating, so the amount of copper used up in the process is proportional to what you've laid out? – joeforker Dec 2 '11 at 19:25
  • 1
    @joeforker: Would you call half the copper "a very tiny amount"? my understanding is that modern commercial board makers usually start with boards covered in 17 um ("half-ounce") copper foil, and dissolve the copper in areas where it is not wanted. On the outer layers and inside drilled holes, they then (usually) build up another 17 um ("half-ounce) of copper with some combination of "electroless copper" and electroplating. – davidcary Nov 26 '12 at 5:27
  • I would call 1um a tiny amount, they get this from the electroless plating. Haven't watched the entire movie: – joeforker Nov 28 '12 at 22:07

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.

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.

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.

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, mentioning this.

Hatched plane reduce the magnetic field going vertically into the board.

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.

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.

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.

Your Answer


By clicking "Post Your Answer", you acknowledge that you have read our updated terms of service, privacy policy and cookie policy, and that your continued use of the website is subject to these policies.

Not the answer you're looking for? Browse other questions tagged or ask your own question.