Electrical Engineering Stack Exchange is a question and answer site for electronics and electrical engineering professionals, students, and enthusiasts. Join them; it only takes a minute:

Sign up
Here's how it works:
  1. Anybody can ask a question
  2. Anybody can answer
  3. The best answers are voted up and rise to the top

On many boards I've seen, there are little copper dots used for the purpose of "Copper Thieving". They're small round copper dots connected to nothing and arranged in an array. Supposedly they're for balancing the copper on the boards to improve manufacturability, but no explanation I've heard has convinced me that they're needed or useful. What are they for and do they actually work?

Below is an example with squares.

 Example with Squares

share|improve this question
Do you have a picture example? – helloworld922 Oct 16 '13 at 19:57
@helloworld922: Added – Gustavo Litovsky Oct 16 '13 at 20:03
This is a real-world example. – mng Oct 16 '13 at 23:51
I usually talk to the vendor making the PCB(s) and ask them to do a DFM (design for manufacture) review. The vendor best knows their capabilities and process limits and should be able to advise if features like this are necessary. Then it's up to you as a designer to add them - which keeps you in control of the design. Some PCB manufacturing companies will publish a design rules guide which may have this information in anyway. – AndyK Jun 15 '15 at 10:32
up vote 22 down vote accepted

Copper dots (or grid/solid fill) are used mainly to balance the thermal properties of the board, to minimize twist and warp as the board goes through the thermal cycling associated with reflow and improving yield.

A secondary purpose for them is to reduce the amount of copper that needs to be etched away from the board, balancing the etching rates across the board and helping to make the etching solution last longer.

If the PCB designer did not explicitly "pour" copper fill into the open areas of the board's outer layers, the fabrication house will often add the small disconnected dots, because these will have the least effect on the electrical properties of the board.

share|improve this answer
I would hope the fab wouldn't just fill empty space with a pattern without at least asking; what if it's empty for isolation purposes, or RF, etc? What fabs do this so I can stay away? – Nick T Oct 16 '13 at 20:19
@NickT, Fabs that are geared to high(ish) volumes seem to always want to do this. They will ask first. Rather than wait for the Engineering Query, it's good to add a fab note indicating whether you will accept thieving or not. – The Photon Oct 16 '13 at 20:30
Unfortunately this answer is incorrect - but a very common misunderstanding. – Rolf Ostergaard May 17 '14 at 8:05

In general, it is better for the manufacturer when less copper have to be dissolved during the etching process and there is no big continuous areas that need to be etched. It is because of 2 reasons:

  1. Etching more copper means that the etching solutions have to be recycled more frequently - it is an energy and money. An ideal case is if the customer wants a PCB entirely covered with copper. :)

  2. The big solid areas of copper are etched slower than the areas where fine copper pattern is located. That is because the pattern has bigger surface and we know that the chemical reactions speed is bigger if the reaction surface is bigger. This way, after the tracks are already fully etched, the big empty areas are still not, so the PCB have to stay some more time in the solution. This causes some under-etching of the tracks which is not good for the PCB quality because it makes the tracks thinner than intended.

share|improve this answer

Unfortunately the other 3 answers to the question are incorrect, but helps keeping a common misunderstanding alive :-)

Thieving is added to the outer layers in order to help a more balanced chemical process for the plating.

Also notice that there is no need to "balance copper" (or stackups for that matter) in modern PCB fabrication to avoid "warped boards".

I wrote about this on my blog recently. You can find other references on the net.

share|improve this answer
Thanks all for upvoting this answer. If this site works, it should slowly make its way to the top of the list. – Rolf Ostergaard Aug 3 '15 at 18:28

The reaction rate of any etching process is limited by local current densities, access of the reactants into the reaction area and clearance of the reaction products away from the reaction area. Since board etching is essentially a planar or two dimensional process this places further limits on etching performance with reactant delivery and reaction products actively interfering with each other for access to the surface.

While always present in processes, where the problem arises is in the differential etch rates across the board. This can cause thin traces to be etched at a different rate than wider traces. For example, etching a relief from around a fine trace within a background of a ground plane is very different in loading than etching a thin trace with no background ground plane.

This can be corrected for by ensuring that in the design the pattern density remains fairly constant per unit area across the board. Thieving is one way to do this. Some manufacturers will actually place sacrificial elements within the tanks and along side the board to ensure proper yield of different line thicknesses.

Mixing and agitation of the tanks during etch will also help mitigate the differential etch issues.

share|improve this answer

Your Answer


By posting your answer, you agree to the privacy policy and terms of service.

Not the answer you're looking for? Browse other questions tagged or ask your own question.