10

I see that a 2 layer PCB is really cheap to prototype. A 4 layer PCB is almost 4x more expensive . I have a design that uses DDR3 RAM where I need to match trace lengths. However I also need to keep the costs down. I observe that going in for a larger 2 layer PCB is more economical compared to a 4 layer PCB. WOuld by design work if I use the 2 layer PCB instead of 4 , although my trace lengths are much longer?

Why is the 4 layer PCB so much more expensive compared to the 2layer? From 2-4 layer is a large price difference? I would like to know why ? Most commercial designs seem to be using 4 layers when they have RAM. Yet they are able to sell for such cheap prices. I get that making in bulk really helps, but by how much does the PCB cost actually come down b? LEts say in small quantities to make a 4 layer PCB is 4$? How much would it be when I make it in quantities of 100?

Rock Tumbler
  • 103
  • 5
  • 4
    Its not just about length matching for high frequency, but also impedance matching. It is nigh on impossible to get \$100\Omega\$ differential traces of that with a two layer board (because the ground plane is so far away). – Tom Carpenter Oct 04 '15 at 03:25
  • Is that not why we use series termination? – Rock Tumbler Oct 04 '15 at 03:39
  • 8
    For large BGA chips it's pretty much impossible to breakout the pinouts on 2 layers, and sometimes even 4 layers is not recommended. – helloworld922 Oct 04 '15 at 03:44
  • 1
    For some circuits you can do this. A DDR3 interface is definitely not one of them! –  Oct 04 '15 at 11:43
  • 1
    The series termination in there for that reason, yes. But if the rest of the traces isn't matched in impedance, a series termination won't help. There is an entire field of electronic engineering dedicated to this. – Tom Carpenter Oct 04 '15 at 14:35
  • 1
    You should not try DDR3 at all yet, and definitely not on a 2-layer board. If you're wanting to use the type of processor which uses that sort of memory technology, you would be much better integrating someone else's CPU module onto your own board. Something like Gumstix or Beagle-whatever. –  Oct 04 '15 at 19:30
  • 1
    You can easily compare 2 layer and 4 layer PCB prices, by visiting web sites which have a price calculator for both. I often use [PCBcart](http://www.pcbcart.com/) who have quite a detailed calculator which is likely to answer your cost questions, but YMMV and there are dozens of alternatives. – gbulmer Oct 05 '15 at 17:59

4 Answers4

15

Ah the horror of trying to make DDR work in two layers :) The long answer is of course to learn about signal integrity and try to understand exactly what you are doing. I have seen this done before, and even pass EMI but with many caveats. First there was only a single DDR part. Second the controller was carefully designed to route out onto all signals in the first two rows of widely spaced balls such that all signals routed with no vias on the top layer to the DDR part. Then the bottom was used for a GND plane, even though it was 60 mils away. Routes were matched, but kept "extremely" short. Finally the part was run as slow as possible, basically the minimum frequency allowed by the DDR part. Oh and we had a spread spectrum clock for EMI.

I would say as a general rule that this is not a good idea and you should stick to four layers and cut cost elsewhere. If you are going to do it don't even expect to get to near full speed, and if you're trying to route multiple parts like a DIMM or clamshell. I would say it's not even worth trying.

Cost depends on so many factors from where you're doing it to how much, it's a much smaller issue at very high volumes than it is at low proto volumes. The headaches you will face trying to debug a two layer design are almost surely never worth it. The increased time to market you will face trying to get it to work is alone worth the cost of a 4 layer in many cases.

You mention volume of 100 like it is high, but it is not at all once you start moving into the thousands, hundreds of thousands there's a steep drop in price from a few hundred pieces. Same if you move off shore somewhere. Just as an example I can think of my US price on 10K units of a 10 layer board is around $50, but my offshore of the same is $25. Your price will also depend on how efficiently you use the panel ( your pcb house makes boards in standard sheet sizes.) If you only fit two per panel and have a lot of waste your cost will go up just as if you only order 2 and leave room for 20 on the panel. Incidentally that's how places that pool together pcb orders work.

Why does it cost more? Well it's a lot ore work, involves double the material and requires a bit more precision or skill. A two layer is just a piece of FR4 copper clad on both sides, just drill some holes, mask, etch away and post process. For a four layer board mask and etch the two layer, then laminate two more outer layers on either side mask and etch again being very careful that they line up properly, then drill and post process. That's just an example but the point is the process has more steps, more labor, more material and more cost.

It might be worth mentioning that there are chips for the mobile industry that take things like LPDDR4 mounted directly on top of them for an all in one solution. Still I would want a four layer board for proper power distribution, decoupling, and routing of other signals but it's an interrsting angle to consider.

Some Hardware Guy
  • 15,815
  • 1
  • 31
  • 44
  • 1
    +1 for including the cost part of the question in your answer, which is currently omitted from all of the other answers. – Dan Henderson Oct 04 '15 at 15:45
9

There are number of reasons in which you have multilayer boards, and when it comes to high speed design, DDR3 for instance, there is alot more happening than just the connections from pin to pin.

At high speeds, the physics behind electric, and magnetic feilds become a factor as well as power speed requirements. It's no longer a case of just connecting from point A to point B. The route you take, will have an effect, so at high frequency, you might actually lose space because you cant/shouldnt route signals in this area, or near this group of signals etc.. Power supplies are slow, and cannot keep up with the demand of current in digital circuits. You could have a power supply right next to the pin, and your chip may still not work well, because digital circuits require fast currents, and lots of it. The power supply might have a high current rating, but a power supply does not have a fast response. And thats where decoupling capacitors, bulk capacitors, and the overall power network distribution come into play. All these things are required for high speed, and some of them depend on the layer stack. Not just the number of layers, but what the layers actually are.

Controlling the feilds, and reducing their effects, EMI, sheilding, inter plane capacitance, signal integrity, power integrity and routing complexity, are the reason why you have might have a multilayer board vs a 2 layer board. You could MAYBE get away with a 2 layer board, but you would have to either model the circuit board (parasitics) and depending on what your high frequency content is, have look at and see if all your requirements are being met.

So can you reduce the number of layers ?

Yes you can.

Will it work ?

Yes. No. Maybe. All of the above.

Try searching this site, for some of the terms in bold. It might answer some questions, or create some new ones.

efox29
  • 11,827
  • 9
  • 56
  • 102
5

Henry Ott suggests five EMC-related objectives that a board design should try to achieve. They are:

  1. A signal layer should always be adjacent to a plane.
  2. Signal layers should be close to their adjacent planes.
  3. Power and ground planes should be closely coupled together.
  4. High-speed signals should be routed on buried layers located between planes. In this way the planes can act as shields and contain the radiation from the high-speed traces.
  5. Multiple ground planes are very advantageous, since they will lower the ground (reference plane) impedance of the board and reduce the common-mode radiation.

According to Ott, the smallest number of layers that can satisfy all of these objectives is eight. From top to bottom, the layers are:

  1. Component pads and low-frequency signals
  2. Power
  3. Ground
  4. High-frequency signals
  5. High-frequency signals
  6. Ground
  7. Power
  8. Low-frequency signals and test pads

So if maximum EMI/EMC performance is your goal, making your board larger won't help. You have to have enough layers. Even for moderate signal integrity concerns, a solid ground plane is a nice thing to have.

Adam Haun
  • 21,331
  • 4
  • 50
  • 91
1

The straight out topological answer is "no".

There are things you can do on a two layer board that you simply can't do one a single layer board, no matter how big. Full stop.

GreenAsJade
  • 173
  • 1
  • 1
  • 8
  • like what? cross wires? You can do that with a jumper wire. – ratchet freak Oct 04 '15 at 10:53
  • 1
    Is that cheating? I guess for a pragmatic answer, you're right: in which case, the question seems "obvious". Of course you can do anything with a big enough board and enough dangling wire :) – GreenAsJade Oct 04 '15 at 22:43