Ground fill on PCB: Is extra copper truly free and what are the design trade-offs?

Hi all,
I just read a great article by Aubrey Kagan on EETimes about panelising (https://www.eetimes.com/author.asp?doc_id=1319827) and it got me thinking. I know some of you can help me out on this one. I've been designing PCB's for a few years now (Eagle CAD, Altium, and DesignSpark). I understand most of the rules of thumb and good design practices when it comes to designing PCB's for a wide range of applications (mostly digital). I've worked with creepage and clearances on high voltage systems. I've designed co-planar waveguides and a variety of small embedded devices. For the most part, it's not high-frequency stuff.My big question is about ground fill on the top and bottom layers of the PCB. I tend to go with the "copper is free" idea and only remove the copper that I want to separate traces, vias, holes and everything else. With a ground fill on the top and bottom layers, I generally stitch them together with vias. On a two-layer board, I feel this is alright. When I move to a four-layer board, I already have a ground layer on the 2nd layer, but is it bad to still keep the ground copper on the top and bottom layers?I understand for high-frequency stuff, this can change the characteristic impedance. For higher impedance designs, does this extra fill make a difference? And is copper still free?-Mike

Mike
Thanks for the compliment- I feel I am obligated to respond! However I am not sure I have sufficient knowledge for a definitive answer.We don't often do 4 layer boards but when we do, our PCB designer(s) maximises "earth" traces on the outer layers as well. Notwithstanding the "copper is free" argument, there are several possible reasons: 1. We often have 2 or 3 different "earths" for analog and digital circuits  that are only commoned at one point as well as galvanically isolated circuits, but still benefit from larger traces for current dissipation. 2. Heat radiation is better from an outer surface and so it is especially useful when the copper is used as a heatsink. Like yours, our designs are all low frequency so HF implications don't play a role in our decisions. I do hope others chime in with better answers.---On a slightly different topic and nothing to do with what you really asked about- I have trouble persuading my guys to do it consistently, but I would really love thermals everywhere. I have just had a repeat issue on trying to unsuccessfully clear a through-hole connected to an earth plane.

Thanks for the reply Aubrey. I have a few more of your articles on my reading list to get through; I'm really enjoying your writing style. Two great points there  in the affirmative, which I agree with.I've seen a few 4 layer designs where there is no ground fill on the top or bottom, only signals. With plenty of room for ground fill, it seems like a waste in copper, which can only hinder the manufacturer.I am very interested to see what other people think.---On your off topic note, I learned the hard way what thermal reliefs were all about on my very first PCB, which was for an AC sinewave dimmer with 2oz copper (top and bottom layers) and no thermal reliefs. I had copper planes more than an inch squared. I manually tried to solder components to the attached pads and I couldn't do it as much as I tried. I had to use a heatgun to heat up the surrounding copper to get anything to attach. It was a mess. I completely agree with wanting thermals everywhere, it makes life so much easier.

Mike,There is a technique that is used on multilayer boards where you have to ADD copper to areas that would otherwise be bare in order to prevent the boards from warping while being soldered. It also is used on inner trace layers to improve the integrity of the lamination.
If the copper is connected to ground, so much the better.Copper is free but you have to pay for the vias to stitch it together...

Great question! As in many aspects of engineering, the answer is "it depends". First of all, cost - you have already paid for the board material, so removing less of it (more copper on outer layers) doesn't cost any more.  Warpage:  not to worry about for 0.062 and above.  I have designed many boards with almost no copper pours (fill) on outer layers and had no issues at the board house with warpage.  032 boards have had issues I have heard.  4-layer boards: It depends on what you are worried about.  If the answer is shielding, and you are aware of the added capacitance added to your signal then it makes sense to add it on outer layers.  For high frequency precision analog - be careful as you are adding capacitance with may limit bandwidth, or worse, add paracitic capacitance that provides positive feedback to your circuit (then oscillation results).

Mark,You make a good point about paying attention to the effect of the copper on precision analog.The concern about warpage and lamination integrity is something I've only seen on boards with a high layer count (6 or more layers) where the layers are closer together.

Elizabeth, you have me wondering how "thin" is a problem.  I have designed 14-layer 062 boards with no difficulties or concern for warpage, and the dielectric is somewhere around 4mils.  I'll check with some process engineers of if any read this post let us know!

Some great comments here. Thanks for all the responses.
I have only seen warpage problems with higher layer count boards, where there's a lot of copper heating and cooling at different rates. For the lamination, I have heard this is the reason for the 'matrix stitching' method to improve thermal airflow on large copper fills during reflow. This is used to ensure the copper fill doesn't retain the heat when it shouldn't be. I would imagine this stitching method becomes more useful for higher layer count boards.
One of the issues I've had on smaller 2 layer boards is trying to add ground fills with limited space and ending up with a disjointed ground connection that is connected through multiple vias. 

Hi Mike,I'm in the manufacturing business, so I'm better able to comment on the "is copper still free" question than on the finer details of high frequency design.Most PCB houses don't charge for vias anymore, so stitching layers with vias is likely to be free. Check with your specific board house to see if they have limits though.I've never run across a board house that charges based on the amount of etching. Heavier copper will cost more, but that's across the board, not based on how much is etched.Copper isn't free at the board house, but customers aren't charged based on the amount etched off or left on. Non conductive areas are etched away, but copper is also added by electroplating to plate the vias and thicken the traces. Other metals are also electroplated on as needed. Nickle, silver, tin, and/or gold are all electroplated on. Sometimes tin or nickle are added during the process and then etched away later in the process.