How to determine the number of layers in a PCB

Does anybody know a practical method to find the number of layers in a given PCB ?

zepertino
it depends on the complexity of the design.
basically to full fill the emc and emi requirement the minimum no of layers should be 8. but u can adjust the number of layers as per the priority of the signal integrity required.

the other factor is the BGA depending on the no fo coloum / row the layer stackup increase , this is because of the track escape from the BGA .

regards
binu g

****h*****p://www-ese.fnal.gov/ese-dfe/dfehome.htm&&&&

check this site,,,,

zepertino
I'll try to share with you some of my expirience.
First of all you need to determine the number of power layers, it depends on the voltages you connect to the IC's. For example if you use only 3.3 Volt devices and all of them use digital power (no analog IC's like power convertors or analog opamps), then 1 power layer will be enough. If you have 3.3 Volt and 5 Volt devices, and also 3.3 Volt analog devices you might need 3 power layers, but if you have 1 or 2 5 Volt devices in this case you can connect their power using thick conductors - then you don't need 3 power layers, but only two : one digital 3.3 Volt and one analog 3.3 Volt. This way you decide how much power layers you have.
Now the Ground layers. If you have only digital devices you need only one GND layer.
If you have also analog, you might want to split the Analog GND to a separate GND layer. Now let's say you have 1 digital power 3.3V, 1 analog power 3.3AV , digital ground GND and analog ground AGND. It is already 4 layers.
Now we go to the layout itself.
If you have BGA devices on the board, check how much conductors you can pass between the BGA balls. Some of the you can pass 2 conductors, some of them 1. Usually you can find this information in the device datasheet or application notes. You can also find there how many layers you need for layout of the BGA device.
Any other device has less limitation than BGA and you can manage with 2 layers for it's layout. For our example let's say you habe fBGA device (fine pitch BGA) so you can pass only 1 conductor between the balls/vias of this BGA, and you need 4 layers for it. So now you have 8 layers : 4 Power and Ground and 4 for signals.

Hope it helps.

i have one quetion
that how to arrange the stack
wheter to put all power and ground planes first and than signal or vise versa or
we have to sandwitch the signal layer inbetween ground and power plane.

thanx in advance

zepertino said:

Does anybody know a practical method to find the number of layers in a given PCB ?

Click to expand...

Do you want to knoe how many layers a PCB that you have, has? Or do you want to design your own?

If the answer is yes to the first question, then there are different ways. Some companies (like my old one), put an ID section on the board, with text on each layer, we used to put it in a small, unused corner of the board to identify the number of layers with numbers (1-16). Others, create a small, empty section on the board, and make that section smaller for each layer, but if they don't have such process, you maey need to cut a setction of the PCB and heat it up and try to desolve the glue in between layers, or, scrap them one by one!

Sometimes, if you are lucky, you can identify dfferent layers on the side of the PCB, by looking at the cut-out of the boards.

If the answer to the first question is no, then you got your answer from others here.

BR,
/Farhad

zepertino ,
for 4 layers (2 signals, 2 power anf GND) :

----TOP signals
----L2 GND
----L3 Power
----Bottom signals

for 6 layers (4 signals, 2 power and GND)

----TOP
----L2 GND
----L3 internal signals
----L4 internal signals
----L5 Power
----Bottom signals

for 8 layers (6 signals, 2 power and GND)

----TOP
----L2 internal signals
----L3 GND
----L4 internal signals
----L5 internal signals
----L6 Power
----L7 internal signals
----Bottom signals

If your design is very high speed you need to add more GND layers to isolate routng layers.

Regards,
shurilo

The number of layers in a pcb design depends on the design complexity and also maximum thickness you can have .

Hello,

You are telling about 8-layered PCBs but if you want to make mass production you should reduce cost and PCB is one of the most cost effective part of a device. So you may design a two layered PCB -of course depending on your design complexity. If you have enough space it would be easier with using vias for top-->bottom or vice versa transitions. Then EMC can be maintaned by hardware tricks (like capacitors, ferrites..)