Design example for commercial high speed pcb

[yefj]

Hello ,Is there a PCB example which is routing differential signal over many layers.where there could be many differential ports in between then.
Is there such real life example I could try to do EM simulation from it?
Thanks.

 

[berkeman]

Hello ,Is there a PCB example which is routing differential signal over many layers.where there could be many differential ports in between then.

I believe that @Baluncore and I have both said that this is a bad practice, so there are probably very few examples of it. You really need to route fast signal traces in a consistent way on the same layer in order to minimize $Z_0$ discontinuities that will cause ringing, signal integrity issues and EMI problems.

 

[Baluncore]

Hello ,Is there a PCB example which is routing differential signal over many layers.where there could be many differential ports in between then.

What do you mean by "many differential ports in between then"?
Please provide a link to a simple circuit example that you want to route.

 

[yefj]

Hello , The basic Idea looks like the photo shown below.
basickaly its a signal transition that accurs at very high digital signal passing threw from top layer to the buttom layer and we have not one differential pair but 10 such pairs.
Is there a manual or design example I could use to build and simulate such PCB on my own?
Thanks.

 

[Baluncore]

1. Each differential pair must pass through a separate hole in all the other layers.

2. Look up the data on the differential outputs and inputs of the chips being used. Those differential signals will be on adjacent pins. If possible, drop the signals directly from their solder pads to the other side of the PCB.

3. The two vias will start by being circular holes, drilled in the PCB. They will then be plated to become a balanced cylindrical transmission line. Look up the differential impedance equations for such a geometry. You know your required impedance, so knowing the via drill size you can calculate the centre separation for the PCB material Er you are using.

4. Work out the dimensions of the parallel tracks on the surface of the PCB material with Er, that will make a differential transmission line with the required impedance. Find the equation for line impedance, if you can't, don't use that geometry line, because no one else does.

5. Start by simulating one pair of terminated tracks on the PCB surface, then with a two-via transmission line near the middle. The test signal should be a differential step pulse, to a termination resistor at the far end. Look at the TDR signal, and try to get a flat response that shows no differential impedance steps between the vias, surface transmission line, and the termination resistor.

6. Use the simulated TDR to work out how to feather or juggle, the surface connections to the via, that will hide the 90° junctions, as there will be a different lump of capacitance between tracks per inductance of track, at that turn.

I know it is old, and ECL is a fun differential logic, but download a copy for bedtime reading of the "Motorola MECL System Design Handbook". Chapters 2, 3, and 7 are important. Learn to think like a signal.
https://dn721801.ca.archive.org/0/i..._Motorola_MECL_System_Design_Handbook_4ed.pdf

 

[berkeman]

Learn to think like a signal.