Configuring power planes on a 4-layer PCB

[pavjayt]

I can use some suggestions in laying out power planes on a 4-layer PCB that has both analog & digital signals while the Analog section has a 30Hz, 10-20MHz and 50MHz signals while the Digital section has 30Hz & 16KHz TTL signals. Based upon this article, it looks like its better to have top layer GND plane, LY2-solid GND plane, LY3-VCC, bottom GND plane.

What do you guys suggest?

thanks

 

[4pyros]

For the most part you will want to separate the analog and digital grounds like left and right or top and bottom.

 

[ronsimpson]

PCB design is a art not a science, and every one has their opinion.

If I had to make a board with very low RF radiation I would put ground as top and power as bottom with the traces in the middle. The problem is you can't see the traces and if there is a problem you can't cut traces.

I usually (in a 4 layer board) put power and ground inside and traces top and bottom. With SMT I want to keep the traces with the parts to reduce the number of VIAs.
Normally I have a local ground on the top side. Example: All of one layer is ground but I don't want high current in that layer. I have several squares of ground on the top side with some VIAs connecting to the ground layer. Each ground square contains one IC or a group of ICs that make up a function. All the noise for that function should stay in that square. A power pin has a wide trace to the bypass cap and then of to a power VIA. The bypass cap connects to a small top side ground plane and picks up all the IC's ground pins. This way the high currents stay in this local ground.

In your case I might have a digital ground (top side) and a analog ground (top side) then connect then together through a entire board ground (middle layer).
The top side analog ground might be divided down to a switching power ground and a op-amp ground.

Some CAD systems allow for many grounds to be connected together. Often the CAD software is not that smart so I keep track of the grounds in my head.

 

[pavjayt]

For the most part you will want to separate the analog and digital grounds like left and right or top and bottom.

Thanks for that tip, I always follow this and connect both grounds under the lines which go from digital to analog using a ferrite bead chip.

 

[pavjayt]

PCB design is a art not a science, and every one has their opinion.

If I had to make a board with very low RF radiation I would put ground as top and power as bottom with the traces in the middle. The problem is you can't see the traces and if there is a problem you can't cut traces.

I usually (in a 4 layer board) put power and ground inside and traces top and bottom. With SMT I want to keep the traces with the parts to reduce the number of VIAs.
Normally I have a local ground on the top side. Example: All of one layer is ground but I don't want high current in that layer. I have several squares of ground on the top side with some VIAs connecting to the ground layer. Each ground square contains one IC or a group of ICs that make up a function. All the noise for that function should stay in that square. A power pin has a wide trace to the bypass cap and then of to a power VIA. The bypass cap connects to a small top side ground plane and picks up all the IC's ground pins. This way the high currents stay in this local ground.

In your case I might have a digital ground (top side) and a analog ground (top side) then connect then together through a entire board ground (middle layer).
The top side analog ground might be divided down to a switching power ground and a op-amp ground.

Some CAD systems allow for many grounds to be connected together. Often the CAD software is not that smart so I keep track of the grounds in my head.

Thanks Ron, that's very informative. I will try to wrap it around my head to see how effectively I can apply these in my design.

 

[ronsimpson]

art........ every one has their opinion

It is important that you have a reason why you do what you do.
Old papers on PCB layout are OK, funny old man on the internet are probably OK.....You have to use your head and make choices.
At first you only have what you read to guide you but soon you will be making choices based on what you think.

all wise do it this way.............

NO...do it smart. Only you understand you design.

You will make mistakes. Other people will disagree with you. There are many ways that work. (not just one)
----------------------------------------------------------
Years ago we made a board that needed to be very quite. There was a big fight as to where to connect the PCB to chassis ground. There are a number of bolts that held up the board. I conducted a survey with all the engineers. I wanted to know which ground point was best, and which was worst and why. Then for a week I conducted tests. I tried one point grounding at each standoff (bolt) then I tried two point, three point.....I tried all point grounding.

The results was that every "good point" was good. Each "bad point" was bad. So the thinking of each engineer was right. (different but right)
The real surprise was that all points grounded worked very well. (I was not surprised) With all points connected to the aluminum it forced the aluminum to look like another ground layer.

Results; the grounds should either be smart or strong.

 

[pavjayt]

Finally after finding some time now and then I managed to finish the layout. I am no pro and I was doing this by reading articles online from manufacturers like TI, NI etc. I have attached a picture of the layer descriptions and the layout pdf itself. I can certainly add brd and sch files if needed for better understanding. Let me know if you guys have suggestions/improvements.

thanks

 

[ronsimpson]

I am no pro

wow You have put some time into this.

 

[MCU88]

PCB design is a art not a science, and every one has their opinion.

Well, actually every study in academia is an science to begin with. The definition of the word science is "an understanding of an entity"

 

[ronsimpson]

Many PCB designers I know, do not know the circuits. They do what I call "connect the dots". No understanding of an entity.
Many PCB designers I know call it art.

 

[MCU88]

Many PCB designers I know, do not know the circuits. They do what I call "connect the dots". No understanding of an entity.
Many PCB designers I know call it art.

And they are probably highly paid and hard working just doing and knowing what they have to to get the job done. The greater the genius the greater the holes in his socks.

 

[Cicero]

Well, actually every study in academia is an science to begin with. The definition of the word science is "an understanding of an entity"

You must be fun at parties...

 

[MCU88]

You must be fun at parties...

I am a bit too old for parties... I still enjoy a stiff drink and a few tabs of morphine and diazepam from time to time however though. Loud music as well sometimes perks me up at 5am when I need to get stuck into an project.

 

[NorthGuy]

Many PCB designers I know, do not know the circuits. They do what I call "connect the dots". No understanding of an entity.
Many PCB designers I know call it art.

I imagine connecting the dots while meeting all the requirements set by those who design the circuit might be really hard work, and, without a doubt, some sort of art. I bet the circuit designer would be willing to relax some of his requirements, and perhaps slightly bend the rules, if he had to design the board by himself.

 

[MCU88]

I imagine connecting the dots while meeting all the requirements set by those who design the circuit might be really hard work, and, without a doubt, some sort of art. I bet the circuit designer would be willing to relax some of his requirements, and perhaps slightly bend the rules, if he had to design the board by himself.

You need an University degree to get a good job working for someone doing this kind of work. You can of course work for yourself as an unqualified / under-qualified person.

 

[NorthGuy]

You need an University degree to get a good job working for someone doing this kind of work. You can of course work for yourself as an unqualified / under-qualified person.

Yes. University education has devolved dramatically nowadays and is hardly enough for laying PCB traces.

 

[pavjayt]

wow You have put some time into this.

I did, but over the course of three months , any suggestions or tips. I can send you the sch and brd files if it helps.

thanks

 

[pavjayt]

Anyone have any suggestions/tips on improving this circuit layout? that would be very helpful.

thanks

 

[Cicero]

Just from a quick look, I can maybe offer some insight here perhaps:

1. I can't see much decoupling? That is a critical part of digital design, and preferably, any decoupling caps should be located on the same layer as the IC, and routed first to the power pins of the IC, not just to the power planes. Think of the loop sizes for these as well.
2. You've separated the grounds which is fine, I guess, but you need to be VERY careful then. Are both the power and grounds going through ferrite beads, or just the power?
3. You've got separated power polygon pours, but have routed tracks directly across these pours (U7 to U6 for example). You need to think of the return current paths this affects, and the large ground loops you have now created by doing that! Especially the high frequency return current paths which you will now force to route themselves in a huge loop around your pours to get back.

 

[pavjayt]

Just from a quick look, I can maybe offer some insight here perhaps:

1. I can't see much decoupling? That is a critical part of digital design, and preferably, any decoupling caps should be located on the same layer as the IC, and routed first to the power pins of the IC, not just to the power planes. Think of the loop sizes for these as well.
2. You've separated the grounds which is fine, I guess, but you need to be VERY careful then. Are both the power and grounds going through ferrite beads, or just the power?
3. You've got separated power polygon pours, but have routed tracks directly across these pours (U7 to U6 for example). You need to think of the return current paths this affects, and the large ground loops you have now created by doing that! Especially the high frequency return current paths which you will now force to route themselves in a huge loop around your pours to get back.

Thanks for your observations Cicero

I had two decoupling caps on couple of ICs in digital side (ex: U4, U6), but I can add one more on all other ICs in digital section. Glad you mentioned about routing power lines to ICs, I followed this very carefully when routing so that the power goes to caps first and then to IC power pins.

Both power and gnds are going through ferrite beads, but I am still abit unsure about the value of the ferrite beads that I have to use. My digital signal has a max of 16KHz frequency signals while my analog section has at max 20Mhz signals. At present I am using this variant.

This is one thing that I am unsure of, some say if these are signals that are going to a DAC, its fine and some say the otherway araound. In this case, my U7 is a DAC (AD7533KRZ) and U6 is 74VHC4040M. What would be your recommend here?

thanks again.