Stripline impedace ..?

Question

i have a doubt in stripline impedance calculation.

general strip line calculations are taking strip line as having 2 planes on top and bottom . in our case stackup is such that, on bottom side plane and top side another signal layer. whether same strip line formulas will hold (I am using Saturn PCB toolkit).

my question is,in my present stack up one of the internal sig layer is 4.5mil from immediate GND layer and 5 mil from immediate signal layer.

now if increase the distance between signal layers and decrease the distance between signal to GND layer, how trace width will change for same impedance ?

I am adding part of Stack up Here S02 Layer has above GND layer @ 4.5mils and below S03 @ 5 mils

Answer 1

I can't fully understand your question without a picture but I know of a useful stripline calculator here: -

If it isn't one of the configurations in the column down the left side then maybe you can approximate it to one?

Answer 2

Let's say your stripline is on layer 3, and layer 4 is a ground plane.

Case 1: Layer 2 has a copper fill above the line

If layer 2 has an unbroken copper region above the stripline with a low impedance connection to power and/or ground, then it doesn't matter if that layer is a "signal layer" or a "plane layer". There is a ground return path on that layer, and your stripline will behave like a stripline with a reference on that layer.

Case 2: Layer 2 does not have copper fill above the line

If layer 2 does not have an unbroken copper region, (whether it's a "signal layer" or a "plane layer" that happens to have a void in that area) then there is no current return path there, and that layer is not providing the return plane for the stripline.

If layer 1 has an unbroken copper region, then you can calculate the stripline characteristics using the total height from layer 3 to layer 1 for the uppper ground-plane distance.

If neither layer 1 nor layer 2 has an unbroken ground plane above your track, then you don't have a stripline; instead you have a buried microstrip, and you should use a buried microstrip calculator to determine the correct geometry instead of a stripline calculator.

In either of these cases, if layer 2 has tracks running nearby and parallel to your line, there is the possibility of coupling signal from the "stripline" to the other track, which will cause loss on the "stripline" and crosstalk on the other line. Try to route nearby tracks on layer 2 perpendicular to the high speed track on layer 3.