Newbie question: Benefit of copper pours?

What benefit is there to adding a ‘copper pour’ to boards?

I’ve noticed a tendency towards adding pours to boards lately. Just wondering.

not a fan of whole board pours on top/bottom. they can be used as a crutch to avoid thinking about return current, potentially leading to design errors. dedicating a plane to ground is better.

just as an example, I had a design I made a year ago, upon revisiting for a minor tweak it I noticed some DRC errors. turns out I failed to properly connect GND to some pins, but my top copper pour made those connections. however, the pour algorithm in kicad had changed a bit and they were no longer connected. if I’d not run DRC I might have produced nonfunctional boards


You should find the answer in articles serie I mentioned some time ago:


I do have planes for ground and 5V on the boards I’m currently working on (except where mains voltage comes into play), so I’ll just put it down to ‘designer’s preference’.

IMHO there are a number of “angles” from which to view the question of copper pours:

  1. The raw pcb stock starts out fully plated. It needs to be etched away to make your pcb, and etching it away does not save money or much of anything.
  2. The copper plating spreads heat; this is usually helpful.
  3. Unless you have no current flow, points along a net (most notably ground) generally are not at exactly the same potential. Partitioning ground can be useful in some circumstances (such as separating noise generating circuits from noise sensitive ones) but a solid ground plane will often provide the best equipotential ground performance and the lowest overall noise.
  4. See Printed circuit boards in

Adding to @BobZ’s list of “angles” into more of a niche design flow. (Granted I may be working with old information, technology may have improved.) Back a couple decades ago when I was laying out flex circuits I was advised by the flex board house to leave as much copper on as I could to aid in dimensional stability of the flex board substrate. (They also advised cross-hatched fills to avoid delamination over large copper pour areas.) The substrate they were using could/would shrink a little during processing if not stabilized by copper, especially for dual layer/sided flex boards. If the shrink forces combined too much especially around a via there may be reliability issues. THT pads weren’t to much of an issue though because the soldering process would bridge any cracks that formed in the hole walls, but vias didn’t get that benefit.

Now, this was back in the '90s, and I haven’t done any flex boards since then so, as I said above, technology may have gotten better since then.


as a dinosaur who makes his own single-sided PCBs I have a lot of copper pours without any electrical meaning:

  1. Copper to stabilize the (single-sided) pads mechanically for connectors and big THTs.
  2. Copper to save chemicals
1 Like

This usually isn’t the case (at least for boards with PTH, I’m not sure about single sided). Usually the bare material has thinner copper that has holes drilled and activated and then has the negative mask of the final copper applied. This is then electroplated to the final thickness. Only after that is the negative mask removed and a mask in the shape of final copper applied. Then the original thinner copper is etched away.

The removed copper also doesn’t go down the drain. It’s extracted from the etchant.

Although I haven’t seen any manufacturer that charges you based on copper area, it would be false to state that it doesn’t save anything in the final process.

Well, yes OK I neglected to mention plating after etching, and I did not know whether copper was salvaged from the solution after etching. But I will bet that the fresh etching solution also costs money; more money for more etching. My point is that for designs working with low voltage (such as under 50V) and unless the pc fabs change the pricing structure, the advantage is almost always with less etching and more copper on the board.

1 Like

Coming back to this to wrap up the topic.

The boards I’d designed with inner ground / VCC layers have been redone as 2 layers.
I ended up incorporating a ground pour on one board as an attempt to put a shield between the analog and digital portions of my project.
I did try making a board with a ‘whole board’ copper pour with the intent of removing a minimum of copper (testing out the idea).

I will reiterate some benefits of pours vs planes.

  1. Dimensional stability for multi-layer boards.
  2. Improved thermal management.
  3. Power and ground planes are generally less flexible than pours, and sometimes that flexibility is needed for design and/or cost reasons. If you need to do things like planar transformers or similar, you will use every layer of the board for a winding, but you will also be trying to get as much copper in the PCB as you possibly can.

I have designed a number of high density power converters and pulsed power circuits, and pours are an absolute necessity for the reasons above, and probably more. As an aside, if pours result in a bad board, then either the user did not specify the design rules properly, skipped the DRC, or the design rule system is buggy or inadequate. Note that I do my professional designs in Altium right now, but once there is a stable KiCad with rule-based DRC, I will try to switch. Altium is not a panacea, and I have been badly bitten by an Altium DRC bug in the past - oh yeah, I forgot they said it was not a bug, but rather an undocumented feature…


Following are the benefits of using copper pours:

  1. Overall thermal dissipation capacity of the circuit increases
  2. Multiple pins can be connected using a single plane. This makes the current to follow its own (shortest possible) path.
  3. Using planes (copper pours) in ground connections allows you to make star connections.
  4. Once the board is ready, we cover the top and bottom layers of the board with the ground to avoid the noise signals. It also acts as protection circuitry.

It is a misconception that the current will flow the shortest path.

The detailed answer is that it will always follow the path of least impedance. If you have any reasonably high frequency signal (example a fast rising digital signal) on your board then it is quite likely that the return current inside your pour will very closely follow the trace for that signal (this minimizes the area and therefore inductance).

This is the reason why an uninterrupted ground plane is of a benefit for this. In such a case you the designer do not need to care (less) where you lay down your signal traces as the return path is automatically there already. If you however have an interruption in your plane then you will need to be aware of that while laying down traces as you should not cross the gab with a signal path that needs the plane for its return path. (otherwise the current can no longer follow the trace closely and you might create a mini slot antenna)


This topic was automatically closed 90 days after the last reply. New replies are no longer allowed.