ground plane vs ground trace

[HDingmar]

First, in two layer board, I've heard that people said, the ground trace should be made to the power ground point even when the ground copper is poured on these two layer, could anybody tell me why?

Then, if I use four layer(internal layers are power plane and ground plane), is it true that I don't have to make any power or ground trace on the signal layer, and just use via to the perspective internal layer whenever the power or ground is needed. This is very easy to do and require much less skill to route when it compares to the two layer board. And the cost of four layer board is pretty much the same as two layer one.I don't see any reason to use two layer board instead of four one.

Considering the separation of analog circuit and digital circuit. What I do is using a solid ground plane for digital signal, and making ground trace and mini-partitioned ground on the signal layer for the every analog circuit, and connect these analog circuit ground at the power ground point with star topology. can anybody provide my some advice of my strategy?

I'm designing motor driver and controller, which includes microchip(a lot of digital signal), and motor driver (big current and sometimes high frequency because of commutation), is there any book or documentation that you can recommend to me? I'm really appreciated.

 

[E Kafeman]

One single layer, mostly filled with a big area of ground, assumes that there only is one kind of ground-current, and that there is no need to differentiate between analog, digital, power or RF ground. RF currents or digital ground current do often not work well together with high (switched) DC currents in ground plane.
RF ground can be an advantage to place in top layer as decoupling loop area are becomes a bit smaller => smaller radiation antennas an less internal losses.
In that case is it maybe not even desired to have LF small signal ground layer below a RF ground area due to capacitive coupling.
Star-grounding is often the most simple solution. The idea behind this type of ground is that different types of ground-current not should interfere with each other: **broken link removed**

 

[enjunear]

Assuming that your microcontroller isn't running with gigabit ethernet (or some other digital signal with super-fast rise/fall times and ultra-critical timing needs), then your combined digital/motor controller board should be fine. You can run a single power plane and ground plane, but I'd still recommend clustering your power electronics in one area and your digital hardware in another, then putting cuts in your ground planes to make "walls" between the sections. The power/gnd planes can be connected, but I'd break them up with gaps to increase path lengths, which decreases the likelihood of crossing ground return paths for digital and analog signals (think of it like a fire break... a swath of forest that's cut down to the dirt to prevent a fire from jumping across it).

Like Kafeman said, when you start putting RF, high-speed digital and analog together, things get a lot messier. This is especially true in radio system designs. Often they contain a many-watt power conversion stage (often switch-mode, so they create LOTS of noise and switching frequencies), a high-speed digital section for data processing (signal encryption and/or high-speed data, etc), and a many-watt RF power amplification stage to boost the excitier signal up to 10's or 100's of watts of RF power to go to the antenna. In systems like that, a great deal of effort goes into segregating, isolating and decoupling the various signal types from one another. Most of the time they are multiple boards, or, at the very least, opposite sides of boards with HUGE cuts between the circuit sections to prevent unwanted coupling.

 

[HDingmar]

thank you for the material you recommend, it indeed provides me some new idea how to do the grounding. I still have one question regarding the RF signal. The microcontroller do has a 8Mhz external crystal, after PLL and bus frequency is 40Mhz. However, this high freq all stay inside the chip. The I/O signal do not have very high frequency (except USB data line, and some 1k to 10Khz PWM signal ). My question is should I consider this component's circuit as a RF circuit or normal circuit?
Right now I'm thinking of having a split ground plane(internal)

One single layer, mostly filled with a big area of ground, assumes that there only is one kind of ground-current, and that there is no need to differentiate between analog, digital, power or RF ground. RF currents or digital ground current do often not work well together with high (switched) DC currents in ground plane.
RF ground can be an advantage to place in top layer as decoupling loop area are becomes a bit smaller => smaller radiation antennas an less internal losses.
In that case is it maybe not even desired to have LF small signal ground layer below a RF ground area due to capacitive coupling.
Star-grounding is often the most simple solution. The idea behind this type of ground is that different types of ground-current not should interfere with each other: **broken link removed**

 

[tony_lth]

I think it should be normal circuits. 40M is not high freq, you should consider such issues at up to GHz.

 

[enjunear]

thank you for the material you recommend, it indeed provides me some new idea how to do the grounding. I still have one question regarding the RF signal. The microcontroller do has a 8Mhz external crystal, after PLL and bus frequency is 40Mhz. However, this high freq all stay inside the chip. The I/O signal do not have very high frequency (except USB data line, and some 1k to 10Khz PWM signal ). My question is should I consider this component's circuit as a RF circuit or normal circuit?
Right now I'm thinking of having a split ground plane(internal)

You can start to see coupling effects in the few MHz range, but since the 40 MHz signal is internal to the device (and you have sufficient coupling caps on the microcontroller), then you won't have to worry about it getting into your board. Everything else will be pretty tame, so just separate your digital and analog circuits with a split in the ground plane, and a via fence, and you should be just fine.

 

[E Kafeman]

Effective motor driving circuits can cause nasty harmonics and high current spikes. Not always best environment for high impedance digital signals.

 

[FvM]

I my opinion, there are only few cases, where the ground separation suggestions form the EE Times article are really useful. E.g. systems with a single mixed signal IC, not injection too much interferenced into the analog ground. It's particular popular for simplified reference designs and evaluation boards. Most real world systems have either multiple mixed signal ICs or are using iCs like high speed ADCs, that produce considerable more interferences on the analog than on the digital supply. Split ground planes risk to make the analog plane an antenna for higher harmonics of these interferences.

Separate ground traces for special signals, e.g. an analog reference voltage can be still meaningfull. They shouldn't carry large and preferably no high frequency currents.

The original post is raising the question of a separate power ground, which can be reasonable, I think. Of course it must provide sufficient current capabality and can be implemented by copper pours or a separate partial plane. The connection between power ground and common ground plane should be a single star point. Typical candidates for a separate power ground are either on-board switch-mode supplies or power interfaces, like the said motor control circuits.