Differential pair stackup

[JMFernandez]

Hi everybody.

I have a question about differential pair impedance and the stackup. If I want to have a differential impedance value (say 100 ohms or whatever you want) and the layer where I want to have this impedance is an internal layer, this layer must be between two planes? Look at the images below:

If the signal tracks are on the top and bottom, it seems ok if only a plane is under o above of the signal tracks, but if the signal layer is an internal layer, it seems necessary to have two planes: one above and one below. Is this necessary? Why?

Thank you in advance!!

[JMFernandez]

[mairomaster]

That is not necessary, you need just one ground plane next to the differential pair layer. However, if the signals are particularly high speed or sensitive, it would be better to have two planes. That will probably give you better signal integrity and noise immunity. If you can't have two planes surrounding the differential pair layer, be careful not to run noisy signals in parallel to the differential pair on the next signal layer.

[robertferanec]

As mairomaster explained, it does't need to have two planes. However, if you have a look at your stackup, you probably will have more planes in it (grounds, power planes). These planes will be above and below your signal layer. In some cases, these planes will be reference planes (for example if the plane is GND) and it will influence impedance of the tracks on the signal layer and you should include it in the calculation.

Again, as mentioned by mairomaster, you may want to have two planes around your signal layers as it can improve signal quality.

[JMFernandez]

Thank you. And where we should set the limit? I mean, we only should take into account for the calculation the planes that are in the inmediately above or below layer? We should ignore the rest of the planes?. For example if we have a layer where we want to achieve certain value of differential impedance. The layer inmediately below is a GND plane and the inmediately above is a signal layer, but above this layer we have a GND plane. We should ignore this plane?

---------------------- GND
---------------------- SIGNAL
---------------------- DIFF
---------------------- GND

[mairomaster]

If your signal layer is used just for signal tracks, without GND pours etc., I would include the two GND planes in the calculations and purely for the calculations, I would imagine that the signal layer does not exist. Just take the combined thickness of the two dielectrics between the DIFF layer and the upper GND layer (if the two dielectrics are of the same material with the same dielectric constant). That is done because you still have some coupling to the upper GND layer as well, since the SIGNAL layer is normally not very dense and doesn't provide much shielding.

However, it is always best if you use impedance values provided by the manufacturer for the final stack-up. They have special software which takes into account all sorts of stuff and produces accurate values, close to what you will actually get.

[robertferanec]

The reference planes don't have to be the layer immediately above / below the signal layer (e.g. in your picture you will use both GND layers for impedance calculations of "SIGNAL" layer and also for impedance calculation of "DIFF" layer). If in the same stackup you have more GND layers, only use the closest from top and closest from bottom. Notice, further the plane is, less influence it will have on the signal layer. See also mairomaster explanation.

[JMFernandez]

Thank you Robert and mairomaster. Now it is clear.