Ground Plane

[lap2034]

Hello,

What is the main purpose of having a ground plane in a Pcb design and what is the difference between a solid and a grid ground Plane?

I have a microcontroller and I am thinking of passing a ground plane underneath it, such that it would be protected against EmC and stray magnetic field.I am saying wright?

Thanks in Anticipation

 

[buzzp]

Im not familiar with grid grounds but I am with normal ground planes in designs using microcontrollers. How many layers is the PCB? On more than two layers it is common to have a power plane in addition to a ground plane. If you have only two layers then I almost always use the bottom layer for the ground plane. The larger the better. You want to avoid islanding any section of the ground plane. Equally important is good layout practices including component placement (bypass caps at Vcc pins/master clear right next to controller, avoid running any noisy signals next to your Vcc supply or master clear pins(relay coils), etc).
The ground plane provides a low impedance area to dissipate any higher frequency garbage that may be present. Otherwise, any noise will find itself in every area of your circuit and in addition, ground traces will have different impedances causing 'ground loops', although on a smaller scale. Its definately something you want to implement. It may work ok without it in the lab but when it gets out side of the protected area, all kinds of strange things can and will happen.

 

[Comcokid]

The use of a grid ground plane, or hatched ground plane is mainly for processing or production issues.

Before solder-mask-over-bare-copper board processes, it was common to tin-plate or tin-reflow the copper under the solder mask. When a board went through wave solder, solder would be pulled under and lump under the mask. When the board cooled, the different expansion rates of FR4 and solder would result in the board warping. Laying down a grid greatly reduced this warping issue.

In modern boards, the copper may be plated-up to the design copper thickness. Hatching the ground reduces the amount of plating solution needed to do this. Additionally, some high volume board houses may factor costs of copper recover out of etching solutions. In some reflow situations, the copper expansion may again result in possible warping issues if the board is thin or the ground plane size is large.

 

[SteveSmith]

Always build your multilayer boards with an even (2,4,6,8...) number of layers. Otherwise your board will most likely warp. Also, with the power and ground planes next to each other you get additonal interplane capacitance that act as a filter cap.

Regards,

Steve Smith, C.I.D.
Product Engineer
Staco Energy Products Co.

http://www.stacoenergy.com

 

[cbarn24050]

Hi, most micrcontrollers do not need a ground plane. EMI problems mostly come from poor power supply layout and filtering.

 

[buzzp]

The design may not need a plane in most cases but is definately worth implementing to avoid any future headaches and will provide a more stable design. This is true especially if its going into an industrial environment. It will not cost you a thing if your only using two layers.

I wonder how many mfg's have problems with equipment that they don't know about? Usually the result of bad layout, etc is resetting of the micro or getting an interrupt when one should not occur. Generally, the device resets and starts over so several people would attribute this to a "power glitch" and never notify the mfg. If this is for something critical I would use a ground plane and more important is to follow board layout guidelines.

 

[cbarn24050]

HI buzz, it will cost you whatever your doing. A plane takes up an entire layer, on a 2 layer board that means you could have got away with 1 layer without it. A ground plane will not turn a bad layout into a good 1.

 

[buzzp]

It is not necessary to use a whole layer strictly for a ground plane. Successful designs have used less than a whole layer. The idea is to make it as large as you can based on the traces you need to run. Any plane is better than simple traces running back to the ground coming into the enclosure.
No a ground plane will not fix a bad layout but it may help. If you have to add another layer for just a ground plane then you have to look at costs vs benefits (of course). The point is, the ground on the PCB should occupy as much space as possible to keep the impedance low. Whether this is a whole layer or 1/4 of one layer it is still better than none. The only increased cost comes if you have to add a layer to get a decent ground plane. Now if your doing some high frequency design for comms or something then maybe a whole layer might be wise but for a microcontroller its generally not necessary.

 

[Orgasmo]

A ground plane provides a low impedance path for return current directly under the trace that sources the current. The loop formed by these paths comprises an antenna that can lead to EM emission and immunity problems if it is not kept small. The smallest loop has the return path directly under the source path. An incomplete or split ground plane can lead to a large loop area and a highly efficient antenna exactly where you don't want one.

 

[Rakestraw]

I have been very successful using “island” ground planes on mixed signal (Analog & Digital) boards. I have been able to minimize digital noise showing up in the analog circuits with this technique. When I make these islands I am VERY conscious of the “loop” issues that Orgasmo has mentioned. I have also been successful in reducing emissions by using the “island” layout technique. When it comes to ground planes many parameters should be examined and bigger is not always better.