Platform forum

Impedance match

Zsolt Danyi , 02-04-2019, 01:35 AM
Hello Robert,

I am working currently with LVDS signals, and after I watched the advaced layout course I still have some question about impedance control.

Question 1:
I use a standard FR-4, 4 layer pcb with the following stack up:

L1-TOP: Signal
L4-Bottom: Signal

If I route my LVDS diff. pairs on TOP, do I have to calculate the conductor height H, from L2 3V3 power plane or L3 the GND plane?
If I calculate from L1-L2, than I have H=140um which is 2x1080 prepreg
If I calculate from L1-L3, than I have H=1305um which is 2x1080 prepreg + L2 + core.
Do I have to reference always from GND layer?

Question 2:
For my backplane, I have to use also a 4 layer PCB, and the datasheet suggests to use one of the the following stack up:

L2: Signal - LVDS L2:Signal
L3:GND L3:Signal
L4-Bottom:Signal L4-Bottom:GND

Which one is better for proper impedance control?
In this case do I have to use Edge coupled stripline asymetrical diff. pairs? Is is possible with standard 4,6,8 layer stack up to use symetrical stripline, because H1 will always differ from H2, right? I can only imagine with custom stackup.
Asymetrical because If I use L2 on either way, the height will be different.
Does it matter if the planes are GND-GND, or 24V-GND or 24V-24V, or it has to be between GND planes if I use Stripline?

Thank you very much.
robertferanec , 02-04-2019, 03:12 AM
a) a good reference plane can only be directly under / above the tracks
b) GND is usually good reference plane, but not always (e.g. for addr/cmd/ctl signals sometimes power is better). Sometimes power plane can be reference plane (for example if you have many decoupling capacitors which are short circuit for high speed signals). In your case try to route most of the high speed stuff on L4.

2) If you only have short signals, you can go with S / POWER / GND / S (route most of high speed on bottom). But if it is a bigger board, go for more layers.
I am not sure about the other questions - maybe some screenshots would help?

This can also help: https://www.fedevel.com/welldoneblog...of-pcb-layers/
Zsolt Danyi , 02-04-2019, 04:17 AM
Thanks Robert the answers, What I meant, sorry it was a little bit misleading.
I just wanted to ask If I have a standard 4 layer PCB, but it could be 6 or 8 layer doesnt matter, If my LVDS signals are between 2 GND layer, then because of the stack up, I have to use asymetrical stripline. In this exmple:
L2: Signal - LVDS

L1-L2 distance = 140um (prepreg)
L2-L3 distance = 1130um (core)

robertferanec , 02-06-2019, 12:21 PM
You can have two GND around your signal layer and they can be asymmetrical, no problem. Use Saturn PCB toolkit to get approximate impedance - Saturn PCB supports asymmetrical stackup and the software is free: http://www.saturnpcb.com/pcb_toolkit/

PS: However, I would not consider GND on TOP layer as reference plane - unless you really can use a solid GND on the TOP layer - however this is usually not possible.
Use our interactive Discord forum to reply or ask new questions.
Discord invite
Discord forum link (after invitation)

Didn't find what you were looking for?