about LVDS bus crosstalk suppression

[wilbert_hj]

black magic of lvds

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!

 

[jzo777n]

Hi

Guard traces are usually not so effective for high speed signals.
Best is to separate the pairs or decrease the height above the ground plane

From "High-Speed Digital Design, A Handbook of Black Magic" page 201

"As a rule of thumb, the coupling between microstrips is halved by inserting a third line, grounded at both ends, between them. Their coupling is halved yet again if the third line connects through vias to the local ground plane at frequent intervals."


Between two lines:

Crosstalk < 1/(1+(D/H)*(D/H))

D = distance between the lines
H = Height above the ground plane


You can find more information of this at:

**broken link removed**
**broken link removed**

or in the book mention above by Howard Johnson

 

[goodboy_pl]

please note that another important issue for cross talk is the lenght of the parallel lines; for long TLines, matching is important so u can not use any width too.

one exact methos to calculate such a high speed circuits is EM simulation to find amount of coupling between two adjaccent lines.
advanced simulators like ADS have model of coupled lines in schematic also, easing the simulation.


BEST!