Could be this stack-up correct/appropriate for a 14 layer pcb?

The PCB includes a CPLD at 50 MHz and a Gigabit Ethernet transceiver at 125 MHz. Both mounted in Primary Component Side.

There are 4 different voltage. Layer 7 is a non-splitted main power plane. Layer 8 is a splitted power planes with three differents voltages.

Any suggestion with the prepeg thickness? IMHO, It will be better if the High Speed Signals are closer to the GND power and further between then.

Units are microns

enter image description here

  • \$\begingroup\$ What frequencies are you operating at for your "high speed" signals? What are the units of your thickness measurements? \$\endgroup\$
    – The Photon
    Commented May 3, 2013 at 16:20
  • \$\begingroup\$ @ThePhoton the units are microns, Sorry. The main clock signals are 125 Mhz and 50 Mhz. At this moment I don't know the parameters of the high speed signals. I'm in the beginning of the design. But I think that if there is a 125 MHz clock I have to consider high speed signals in some way. \$\endgroup\$ Commented May 3, 2013 at 16:39
  • 1
    \$\begingroup\$ For sure you're in the frequency range where you should consider signal integrity issues, but exactly how careful you have to be depends a lot on the frequency. Overall your stackup looks good, but I might shring the distance between signal and ground planes and increase the distance between adjacent signal planes, if possible. Also realize that usually every other dielectric layer is a prepreg and the in-between layers are "core" layers. \$\endgroup\$
    – The Photon
    Commented May 3, 2013 at 16:48
  • \$\begingroup\$ Notice that clock frequency is of limited interest here. The interesting parameter is rise/fall time. Typically this is in the range of 200ps for modern digital parts. You can convert this to frequency range by the 350/tr formula... 350ps => 1GHz... 200ps => 1.8GHz (now you know why you need a 2GHz scope bandwidth to see a modern digital signal :-) \$\endgroup\$ Commented May 3, 2013 at 18:59
  • \$\begingroup\$ There is some relation between the frequency and the rise/fall time. Higher frequency lower rise/fall time. As I read It's considered that the rise/fall could be around the 10% of T. (T is the period of the signal. 1/f). \$\endgroup\$ Commented May 3, 2013 at 19:21

1 Answer 1


I am sure there is no such thing as a correct stackup. It's all engineering - which is usually compromises between many things. This is true for a stackup also, where you have to compromise between manufacturability, impedances, sourcing, crosstalk, loss etc.

There is a great deal of knowledge about this, which would be too long for one answer here. I suggest you get a book like the first Lee Ritchey book - this is available as a free download from www.ee-training.dk (plug, true... but a really good book about this subject).

A few things to get you started:

1) You want power and ground plane pairs closely spaced to build low inductance capacitance for your power distribution (PDN - check out pdntool.com)

2) You want narrow traces so you can fit a lot of routing in few layers, so you are probably looking at around 4 mil traces.

3) You want known impedance for all traces - maybe 50R. This can tell you what thickness of the dielectric should be (use a 2D field solver to find this - free example: TNT). Probably also somewhere around 100um/4mil.

4) You want to limit crosstalk to a reasonable level. Use an IBIS simulator to find the required spacing. Now you know roughly how much routing you can fit in each layer. Use that (plus the number of layers required by your escape routing from the big BGA packages you may have) to help you find how many routing layers you need.

5) You have to decide between a signal-plane-signal-plane... or a plane-signal-signal-plane... type stackup. In doing this you will want to look at broadside coupling with an IBIS simulator. Can be a lot more than you expect.

And there is a lot more to "Stackup Design" (Google it - Lee Ritchey has a full day course on this)...

Think about why you want 35um Cu, when skin effect limits you to 20um at 20 MHz? Usually 17um is what you want for most digital high speed boards.

Another idea for a 14L stackup might be something like this:

1: sig 2: gnd 3: pwr 4: sig 5: gnd 6: sig 7: pwr 8: gnd 9: sig 10: gnd 11: sig 12: pwr 13: gnd 14: sig

Use closely spaced pwr/gnd - 100um/4mil dielectric between.

Advantages to a stackup like this:

1) More pwr/gnd pairs gives you better PDN 2) 17um Cu gives you better defined etch for finer widths 3) No X/Y restrictions on routing layers 4) No problem using split pwr planes as references because of the closely coupled pwr/gnd pairs. This point needs further explanation.

Remember: PDN is many cases the most important part of modern digital designs, so you want to get that right. This will help you pass EMI also.

Not sure this answers your question, but at least it should give you some idea on how to tackle this in a professional way.

Disclaimer: Yes I take signal integrity (SI) and power integrity (PI) very seriously because I have seen emphasis on SI/PI reduce number of board spins etc. for many companies over the last 15 years.

  • \$\begingroup\$ In my honest opinion, capacitance between adjacent PCB planes is overrated. The capacitance is not high enough to eliminate discrete caps or otherwise good design practices. It might be an "added bonus", but you can't rely on it to get the job done. \$\endgroup\$
    – user3624
    Commented May 3, 2013 at 16:01
  • \$\begingroup\$ @user21976 You point really interesting points. I would like to know the opinions about this stackup and what are the advantages of other 14-layers stackups. \$\endgroup\$ Commented May 3, 2013 at 16:46
  • \$\begingroup\$ David: Agree that interplane capacitance is normally not enough in itself. It plays an important role however in the higher end of the frequency range. \$\endgroup\$ Commented May 3, 2013 at 18:49
  • \$\begingroup\$ Jesús: Advantages to a stackup like what I suggested: 1) more pwr/gnd pairs gives you better PDN 2) 17um Cu gives you better defined etch for finer widths 3) No X/Y restrictions on routing layers 4) No problem using split pwr planes as references because of the closely coupled pwr/gnd pairs... \$\endgroup\$ Commented May 3, 2013 at 18:51
  • \$\begingroup\$ David: There is another benefit in closely coupled pwr/gnd planes in that you can use split power planes (never split the gnd planes) and still route traces referenced to the pwr plane with no restrictions. \$\endgroup\$ Commented May 3, 2013 at 18:56

Your Answer

By clicking “Post Your Answer”, you agree to our terms of service and acknowledge you have read our privacy policy.

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