Copper Balancing

[Nikos A.]

Dear all,

I have completed the designing of a 4-layer RF PCB and the manufacturer ask if it possible to balance the copper at the inner and outer layers.
The stack up is RF SIGNALS(red)-GND(yellow)-VCC(orange)-SIGNALS(blue)

This is my first PCB and I don't how to manipulate with copper balancing. Furthermore, I am not sure whether or not this extra copper is going to affect/degrade the performance of my RF PCB. Also, the extra copper shall be grounded or not?

Please find attached some screen shots (in single layer mode) of the layers.

Also, as you can notice I didn't apply vcc plane. Should I apply?

Thanks in advance

[Rerouter]

A 4 layer board is made as 2 glued together 2 layer pcbs. For those 2 pcbs if the amount of copper is drastically different. The board that is drastically unbalanced will end up curved. E.g. ground plane on one side. Sparse traces on the other. Had it happen on a few of my projects early days.

If your signals are ground referenced. Then treat them as coplanar waveguildes and run ground plane to balance out the boards a little.

Aim for atleast 50% copper fill on a board that has a full plane on the other side.

[Yansi]

4layer board is not made out of two glued together 2layer PCBs! A common miss-conception.

It is made out of an internal 2layer substrate, and two outer prepregs - which for RF PCBs may be of different (lower loss) dielectric.


OP: Fill the 3rd layer also with GND.

[Ian.M]

... or make it a well filled power plane.

[vealmike]

To balance the board, fill layer3 with copper.

Rf?
Fill layer 3 with your power plane, not ground. Would I be right to guess that layer 3 is power routing anyway?

General comments:
Are you doing via in pad? Be aware that this can make soldering your components tricky. Ideally you should make sure the via is plated over, otherwise it wicks solder away from the joint. Even with this, soldering is harder as the via sucks heat from the joint.

If you have a high speed signal, place a ceramic decoupler close to any place the signal jumps from layer 1 to 4. A signal propagating on layer 1 will induce a equal and opposite current in the plane on layer 2.
What people new to high speed struggle with is that the current in the plane follows the path of the signal. The current in the plane will flow directly beneath the signal, not take the shortest path, or spread out over the whole plane.
When your signal jumps layers and references a new plane , you need to stich the reference planes to provide a path for the return current.

In your case, with a signal in layer 1, the return current is on the plane in layer 2. When signal jumps to layer 4, then the return current flows in the plane on layer 3.
So you need to stitch the planes together.
If the planes are the same (e.g. both GND) then just stitch with a via. If they are different (e.g. GND layer 2, VCC layer 3) stitch with a decoupling cap.
The stitching structure needs to be close to the signal via to minimise the loop area (inductance) between signal current and return current paths.
Also ensure that there is plenty of decoupling between power and ground at any IC or connector.

In general it looks like you need a lot more decoupling.

HTH

[T3sl4co1l]

4layer board is not made out of two glued together 2layer PCBs! A common miss-conception.

It is made out of an internal 2layer substrate, and two outer prepregs - which for RF PCBs may be of different (lower loss) dielectric.


OP: Fill the 3rd layer also with GND.

It is both, however you want to order it.

Standard proto is done this way however, and you will most likely pay full-custom price for the pair-stack build.


Yeah, you say 3rd layer is "VCC", but there's only four nets routed on it?  If you don't need to pour VCC, why not add a few more vias and route everything 2-layer?  Fine, that's probably awful for RF.  Then pour VCC on the 3rd layer, like the name suggests.  It's only better that way (or, it should be anyway)!

Tim

[dmills]

Yea it is the L2/L3 imbalance they are complaining about, flood L3 with a VCC polygon, it will fix this and lower your supply impedance at the same time.

I am guessing some sort of Doherty amplifier?

Regards, Dan.

[Nikos A.]

vealmike thank you for your reply and your comments.

Yes layer 3 is power routing. Why you suggest to fill with power plane instead of ground?

In general  I avoid doing vias on pads. The only vias I placed are under SMA connector pads.

I do not have any RF signal goes from layer 1 to layer 4. All the RF signals are in layer 1. At Layer 4 are the control signals which are driven to layer 1 through vias.

[vealmike]

vealmike thank you for your reply and your comments.

Yes layer 3 is power routing. Why you suggest to fill with power plane instead of ground?

In general  I avoid doing vias on pads. The only vias I placed are under SMA connector pads.

I do not have any RF signal goes from layer 1 to layer 4. All the RF signals are in layer 1. At Layer 4 are the control signals which are driven to layer 1 through vias.

You're welcome.
You will generally get better signal quality if you route both power and ground as planes. Putting power on that plane gives you a solid plane. If you fill with ground, the plane will have cuts and islands to allow for your power routing. From an ac perspective power and ground are the same thing, provided you have plenty of decoupling. So why would you fill with ground, and have to stitch the islands together with inductive vias when you could fill with power and get a solid plane?

Return currents flow in the nearest plane and  (where they can) track the signal current. Think of the return current as lazy. If it flows in a loop, the loop becomes an aerial, which radiates power. So to avoid doing that, the return current follows the path of the signal current as closely as possible.
As all your high speed is on 1 then all the high speed return currents will be on 2. As 2 is a solid plane it will shield 3 & 4 from the signal / return currents, so you could argue that it doesn't matter what you do with 3 in this case. But as has been previously said, creating a solid power plane lowers your supply impedance. This is because you get a free capacitor with layers 2&3 acting as big low impedance plates.



Via in pad - fine. you can do it, it just gets more expensive to ensure good design for manufacture, or for a hobby board makes soldering harder. 

Rf signals jumping layers - great, if they're all on 1 you don't have to worry about this either.

[Nikos A.]

Thank you vealmike, that was a great explanation!!