about LVDS bus separation

[wilbert_hj]

I am designing a high speed board.LVDS bus are used in this design.

The LVDS bus signal speed is above 500MHz,so the SI problem is very important.
but my PCB have no enough room for LVDS bus trace group routing. I have to pour some GND copper plane between LVDS pairs in each LVDS signal group to control crosstalk effect.

The LVDS routes in 0.1mm width/0.15mm between differential lines. Can anyone can tell me what is the minimum value of the GND copper seperation distance?

I simply placed one GND signal line in 0.3mm in width as the seperation between differential lines(the LVDS bus signal plane is stacked between GND/PWR planes.)

Will there be any problems in my design? eager for some advice!

Thanks!

 

[wilbert_hj]

I need help!can someone give me some advice?!

 

[Uky]

You will have to maintain a solid ground plane underneath all LVDS differential pairs. The differential impedance must be controlled.

There is no way to tell whether you will have any problems without knowing all parameters of your PCB such as dielectric constant, layer thickness, trace width, trace separation etc.

Search the data sheets for your transceivers for suitable impedance levels.

There are a number of free software tools that can be downloaded.

Not all of them can calculate differential impedance though.

Or you can contact National Semiconductor and try to get a handy paper slide rule calculator called "Transmission Line Rapidesigner". p/n 633200-001

 

[wilbert_hj]

my board is impedance controled,and the impeddance is 100Ohm as diffiferntial lines.

maybe you have not understand my question.my question can be described as below:
1.) Is it necesary for me to palce some GND copper between LVDS bus lines(8 LVDS pairs as a data bus)?
2.)If it is necessary, what is the minimum value of the copper width? Now,i placed only a GND line between LVDS pairs,the line width is 0.15mm.is it enough for signal crosstalk separation?

Help me!

 

[JAY-R]

HELLO!!!

I already experienced to route LVDS signal many times already and based on my own experience regarding inputting GND guard on each pair there is a certain thickness of the GND and certain clearance between the signal and GND.

Normally client gave this specs:

Signal width:
Clearance Between Signal Pair:
Minimun GND Width:
Clearance between Signal and GND:

This specs are given based on the simulation result on there lab.


Assuming you are independent designer, and based on my experince on LVDS you can take 0.2mm(0.3mm is better if you have enough space) clearance between GND and signal and please keep 0.3mm minimum for GND width(thicker the better) for each pair. Make sure to input GND via on end side of the GND to avoid antenna and to make solid GND and much better if you can input lots of GND via but make sure to maintain the 0.2mm to LVDS signal.

Also same as other advice please make a solid GND plane underneath the LVDS signal.


I hope you understand my explanation and my grammar.

JAY-R---->>>Philippines