Take the 2-minute tour ×
Electrical Engineering Stack Exchange is a question and answer site for electronics and electrical engineering professionals, students, and enthusiasts. It's 100% free, no registration required.

Looking at many online PCB fabs, when spec'ing out a board and uploading your gerbers, often you select how many Layers your board should have. Invariably, the options are always multiples of two.

Why is that expected? While if you have three layers, throwing a ground plane in isn't a big deal, but what is the reasoning behind always sticking to even numbers?

share|improve this question
3  
Boards are made from fiberglass (for example) like FR4 with copper platted on both sides - boards are made by chemically removing the copper you don't need. A two sided board is typically 0.16 inches thick. More than two and you use thinner sheets. Guess what? Each one has two sides! A simple insulating layer with no copper is used between sheets. So, 2, 4, 6, 8, 10, 16, etc. Most I have used is 10. –  C. Towne Springer May 1 at 3:04
    
For full explanation see YouTube "Copper Clappers". –  C. Towne Springer May 1 at 3:04
1  
Odd... I never knew 'one' was an even number... XD –  haneefmubarak May 1 at 9:16
2  
@haneefmubarak - You can only get a single sided board if you make it from the peeled off outer skin of a Klein bottle. Otherwise, you can have copper on one side and no-copper on the other but you still get 2 sides. –  Russell McMahon May 1 at 11:17
    
@RussellMcMahon that would be awesome!!! But anyways, you know what I meant :) –  haneefmubarak May 1 at 22:18

4 Answers 4

It's possible to make multilayer boards with odd numbers of layers, but they are non-standard, there is no cost savings and there is another issue- the asymmetrical stack-up will tend to lead to excessive warp and twist, particularly after soldering.

The stack-ups are made from cores with copper on each side, separated by pre-preg insulator, so they naturally come on pairs. It's better to add another routing layer or ground plane than to use odd layers.

Edit: As Brian and others have pointed out, single-layer boards are an exception. Presumably because the foil layer is on the outside of a relatively thick laminate core they do not seem to show so much tendency to warp (though I've had problems with large paper-based phenolic boards after wave soldering). Single layer boards are used in huge quantity for such things as power supplies (where the component density is low and dominated by the large components and clearances required) and disposable consumer goods (where punched boards are de rigueur to meet the price point).

share|improve this answer
3  
they are non-standard ... unless the odd number is 1. Which is probably still the majority of PCBs out there... –  Brian Drummond May 1 at 8:01
    
Interest only: Single later PCBs tend to not be FR4 laminate but instead use things like condensed Yak's Butter. YB is fine enough for getting production cost down but may not be quite so good for whole of life cost. FR4 is very hard on punch tools and punching is cheap compared to routing so punching is favoured for low cost which leads to using YB. A possible problem is cracking of the PCB material. In one case I have experienced the crack broke a track and affected products were DOA due to a saving of a few cents max. –  Russell McMahon May 2 at 2:45
    
@RussellMcMahon Of course a few cents might be a significant part of the BOM of a cheap consumer product. Most of the cracking problems are just bad design like mounting heavy or user-attached parts to the board. Things like PC supplies do okay. BTW I have not tried yak butter (so far) but yak stew is delicious. –  Spehro Pefhany May 2 at 3:36
    
@SpehroPefhany You may not have tried YB - but if not it's likely because you had someone on site carrying out QC during processing and/or before shipment. Failing that you'd fail Russell's 1st law of doing business in C---- -'You have to be there." - and the first you know about the YB is at incoming QC (if then). The problems I saw were due to misalignment of the punching jig in some manner so they applied stresses across a narrowish land between a large hold and PCB edge. This suggests that the punching MAY have been done in 2 or more stages - maybe holes and then outlines or ...? ... –  Russell McMahon May 3 at 6:15
    
... whatever it was, somebody else was interposed between me and the process so it failed the "You have to be there" requirement as they also were not there. || NB: In my "rule" "you" can be anyone proficient who is wholly your person and with no prospect of being swayed or paid by the manufacturer. I know an excellent company in China who does inspections in many areas at excellent prices and is well spoken of by others who have used them, as well as having my recommendation. I'm happy to refer them offlist. The 'leader' is Indonesian and most workers are Chinese. ... –  Russell McMahon May 3 at 6:19

Many boards have only one layer, so a odd number. These are usually very high volume boards where every last penny of production cost matters. These boards are usually made from a phenolic and are punched using a custom die, instead of drilled and routed. The board behind the dashboard of my last car was like this, for example.

share|improve this answer

This is likely because multi-layer boards are made by gluing a stack of regular boards together. The individual boards have copper on both sides, and go through the same etching process regardless of where the copper is. To use a conventional single-clad board to get one less layer would require stocking single-sided material. So it's probably not worth the expense or effort.

share|improve this answer

One could conceive using an insulator on the bottom layer and this is possible but there is little advantage as plated thru holes would be impossible. 3 layer boards are rare but also possible using a 2xboard, one prepreg and one copper layer all laminated

The another exception is a single sided board.

So it is not true that all boards are even sided, single-sided is the best for all consumer goods if possible., not to sacrifice performance or EMC. TVs often use single sided boards with shielded modules. Isn't that odd?

In fact there is very little no cost advantage to even or odd. Least copper is cheapest. In volume it is weight of copper that counts or total copper surface area x layers x oz.

There are many process options in multilayer boards that has little to do with number of layers and more to do with features. So the question has a false assumption. In fact any number of layers is possible and fewer is cheaper. For the best resolution in holes, thruhole feature etching can be <0.05mm whereas clad etching is worse due to flow of acid on the surface only. Then final stackup is controlled by gap in each layer and finished thickness by using various prepreg lamination options. Old school fabricators used only double sided boards. Hence even layers. modern fab houses just etch copper only and add lam to make up the stack and then do plating of holes. BLind or buried vias add cost significantly with multiple press and plating operations. So answer is true., it no longer matters if even or odd

... there are extra costs for excessive holes, excessive drill sizes, excessive milling, blind or buried vias and controlled impedance and extra for polyamide and premium for Rogers Teflon substrates.

I am reminded by my old friend Amit @Sierra that when dealing with 2 or 3 mm tracks and holes, to think of Even layers for sequential processing of laminates to improve yields so a N layer board with interleaved pwr/gnd planes and outside signal planes should be grouped in even numbers if there are many blind interconnects between internal layers. This improves DFM greatly. E.g. enter image description here

share|improve this answer
1  
This doesn't answer the question. –  whatsisname May 1 at 15:09
    
@whatsisname YES it does answer the question - very clearly in the first 2 paragraphs. He says the even layers are NOT invariably required but that odd layers have no great advantage and some disadvantages. Yes? –  Russell McMahon May 2 at 7:15
    
This answer IS useful. The -2 downvotes appear plain silly without an explanation. –  Russell McMahon May 3 at 13:22

Your Answer

 
discard

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.