Top GND Fill on 4 Layer PCB, Yey or Ney?

[ssashton]

Quick question, I hope!

I'm laying out a switching DC-DC converter on a 4-layer PCB. There is a solid GND plane on the 1st inner layer. Should I also stitch a GND fill on the top layer?

I've read (somewhere) that it is not good practice to connect components directly to a top GND fill if you have an inner plane. So each component has a via directly to the main GND plane and not connected to the top fill. However I'm uncertain if it's a good idea to add GND fill on the top layer around the outside of the converter to 'catch' EMI?

In my image I have highlighted the GND nets. The grey colour is the inner GND plane.

Thank you!

[Siwastaja]

Properly stitched top fill - best
No top fill - OK
Unstitched top with long antennae between tracks etc. - worst

If feeling lazy, better leave unfilled. I usually do fill the top, it doesn't take long to add stitching and selectively remove areas where you can't fit the vias, such as narrow passages (adjusting the pour parameters takes care of most narrow fingers, selectively add a few pour cutouts and job done).

What is shown in the image is good.

[ssashton]

I did the 3rd one on my last prototype. Top fill and only connected to a single GND point 

So now I'm a bit nervous.

[spostma]

Use only one ground plane!
Explanation in attachment...

Years ago, I got an excellent EMC expert advice session at the DARE! CE testing by  senior test engineer there.
They also design multi-GHz test equipment themselves, and really know their part in HF and CE compliant design.
I made notes for myself of this valuable session, and attached it FYI.

I hope this helps you pass the CE testing!

[ssashton]

Thanks for your replies!

I was using large power fills but after reading the notes from Spostma I have changed to using only traces.

Attached is my current design. What do you guys think?

As before, the grey layer you can see under the audio line level parts is the main internal ground plane that is across the entire PCB.

You can see that I did not put any  top or bottom layer ground fill around the line level audio parts, that is mainly because there is not very much space for via stitching. So I thought it's best to not fill that area.

[ssashton]

A 3D View.

[BillyO]

There are times when a copper fill can be used and times where it should not.  Stitching is also to be used with precautions and is good where the integrity of voltage planes is not compromised by doing the stitching.  It gets complicated.

If you have a simple circuit where all teh traces are on one layer and contained in a small area, a voltage referenced copper pour that encompasses that trace area and has multiple points of attachment to one of the voltage planes can help reduce the impedance of the power supply.  Below is an example.  It is a 4 layer board.  Layer 1 (top) is a ground plane, layer 2 is a Vcc plane, layer 3 is another ground plane.  The 4th layer (pictured) is the one with traces.  The copper pour around the traces is connected to the Vcc plane at several (5) low impedance places.  It's only purpose is to reduce power supply impedance and is not there to be a ground plane for the signal traces.  If you wanted, it could be stitched to the Vcc plane if you didn't go overboard to the extent that the ground planes get compromised.  But in this case, it's not really nesseccary.

[dobsonr741]

The green power track to C34 is tiny. It negates the ESR the cap might supposed to provide. An island for that power rail is appropriate, wherever you find the place for it. Just do not interrupt the continuity of the power plane when pacing it.

[ssashton]

I'm not sure which bit you are referring too, would you be able to highlight it?

C34 is not connected to the power traces. Also I don't have a power plane, only those green trace.

[ssashton]

I'm looking at this on my mobile and when I select the red top layer image in my previous post it opens the 3d view instead. Like s file name has been messed up. Does this happen for anybody else? 

[dobsonr741]

C47 is is - sorry mistyped.

[ssashton]

Guys, it seems like there was an error in the forum database. When I enlarge the Top Layer image it opens the 3D view instead.

The top layer was the most importiant 

Here is the images again. Sorry if it made some confusion!

[ssashton]

My current stack-up is:

Top: Signal traces (mostly small signal and some power for the amp IC)
Inner 1: Ground plane
Inner 2: Power traces
Bottom: Signal traces (mostly switching speaker output)

This puts my high current un-filtered switched speaker traces on the bottom layer, separated from the ground plane by the power layer.

What do you think about swapping the order of the 2nd inner and bottom layers so the speaker traces are closer to the GND plane? Do the inner layers have less copper weight?

Top: Signal traces (mostly small signal and some power for the amp IC)
Inner 1: Ground plane
Inner 2: Signal traces (mostly switching speaker output)
Bottom: Power traces

[langwadt]

What do you think about swapping the order of the 2nd inner and bottom layers so the speaker traces are closer to the GND plane? Do the inner layers have less copper weight?

yes usually, they start the same weight, then out layers get plated with the vias