50
\$\begingroup\$

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?

\$\endgroup\$
5
  • 2
    \$\begingroup\$ A hatched plane must weigh a tiny bit less... could that ever matter? \$\endgroup\$
    – joeforker
    Oct 12, 2010 at 20:05
  • 4
    \$\begingroup\$ We've gone plaid! \$\endgroup\$
    – joeforker
    Oct 12, 2010 at 20:05
  • 2
    \$\begingroup\$ 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. \$\endgroup\$
    – Kortuk
    Oct 13, 2010 at 1:37
  • 2
    \$\begingroup\$ 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. \$\endgroup\$
    – Kellenjb
    Oct 13, 2010 at 3:02
  • \$\begingroup\$ How about the hatched style has increased surface are between copper and air that makes better heat dissipation? \$\endgroup\$ May 22, 2020 at 18:29

14 Answers 14

34
\$\begingroup\$

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.

\$\endgroup\$
5
  • 1
    \$\begingroup\$ 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. \$\endgroup\$
    – Kortuk
    Oct 12, 2010 at 20:50
  • 1
    \$\begingroup\$ 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. \$\endgroup\$
    – Kortuk
    Oct 12, 2010 at 20:58
  • \$\begingroup\$ i don't completely agree, but i edited to replace my general language with more specific issues as frequency increases \$\endgroup\$
    – Mark
    Oct 12, 2010 at 22:42
  • \$\begingroup\$ 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. \$\endgroup\$
    – Kortuk
    Oct 13, 2010 at 1:34
  • 1
    \$\begingroup\$ 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. \$\endgroup\$
    – Kortuk
    Oct 13, 2010 at 1:34
10
\$\begingroup\$

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.

\$\endgroup\$
1
  • \$\begingroup\$ I came here to post this. Do not underestimate the stiffness of a solid copper plane on a flex PCB. \$\endgroup\$
    – DPF
    May 22, 2020 at 21:17
7
\$\begingroup\$

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

\$\endgroup\$
6
  • \$\begingroup\$ This is not correct vikram. This is a confusion between hatched ground planes and thermal relief. Mark is correct here. \$\endgroup\$
    – Kortuk
    Oct 12, 2010 at 22:05
  • \$\begingroup\$ 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. \$\endgroup\$
    – Kellenjb
    Oct 12, 2010 at 23:22
  • 3
    \$\begingroup\$ amazon.com/High-Speed-Digital-Design-Handbook/dp/0133957241 covers it \$\endgroup\$
    – Mark
    Oct 13, 2010 at 3:18
  • \$\begingroup\$ That is what I referenced. \$\endgroup\$
    – Kortuk
    Oct 13, 2010 at 14:09
  • \$\begingroup\$ @Kortuk: I would guess cross-hatched ground planes probably came about when automated tools didn't do thermal reliefs. \$\endgroup\$
    – supercat
    May 14, 2011 at 15:11
7
\$\begingroup\$

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.

\$\endgroup\$
6
\$\begingroup\$

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.

\$\endgroup\$
5
\$\begingroup\$

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.

\$\endgroup\$
3
  • \$\begingroup\$ 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? \$\endgroup\$
    – joeforker
    Dec 2, 2011 at 19:25
  • 3
    \$\begingroup\$ @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. \$\endgroup\$
    – davidcary
    Nov 26, 2012 at 5:27
  • \$\begingroup\$ I would call 1um a tiny amount, they get this from the electroless plating. Haven't watched the entire movie: eurocircuits.com/index.php/making-a-pcb-eductional-movies \$\endgroup\$
    – joeforker
    Nov 28, 2012 at 22:07
4
\$\begingroup\$

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.

\$\endgroup\$
3
\$\begingroup\$

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.

\$\endgroup\$
1
  • \$\begingroup\$ Bubbled copper planes were usually due to mask over solder-plated copper vs. the now-common mask over copper with ENIG or HASL only on exposed copper surfaces. The solder under the mask allowed more solder to wick under the mask. \$\endgroup\$
    – SteveRay
    Dec 19, 2018 at 19:24
1
\$\begingroup\$

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.

\$\endgroup\$
0
\$\begingroup\$

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

\$\endgroup\$
0
\$\begingroup\$

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.

\$\endgroup\$
0
\$\begingroup\$

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.

\$\endgroup\$
0
\$\begingroup\$

Another reason to use cross-hatching in a plane, according to IPC, to acquire a proper adhered solder mask into melting metal surface.

\$\endgroup\$
3
  • \$\begingroup\$ That is interesting, can you give a link or a more precise definition where the IPC is stating that? \$\endgroup\$
    – jusaca
    Jun 13, 2020 at 14:07
  • \$\begingroup\$ I read it on a IPC-CID guide. It's not an specific IPC standard, just a recommendation. \$\endgroup\$
    – csedano
    Jul 19, 2020 at 11:07
  • \$\begingroup\$ I'd be interested in that reasoning too... A vertical magnetic field would require that the current makes a loop in the horizontal plane. I won't say that this is false but I'd be really interested in the reasonings why this should happen more with solid copper vs X-Hatch. \$\endgroup\$
    – kruemi
    Jan 29, 2021 at 12:57
0
\$\begingroup\$

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

\$\endgroup\$
1
  • \$\begingroup\$ Your answer could be improved if you included a synopsis of the article you cite. This would allow the reader to decide if they needed to read the whole thing.. For example "Ground planes are hatched because.... This is an obsolete technique for rigid boards. but useful in flexible ones. For further information see ..." \$\endgroup\$ Dec 27, 2021 at 22:24

Your Answer

By clicking “Post Your Answer”, you agree to our terms of service, privacy policy and cookie policy

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