Can any one tell me which all signals in VGA connector are 75ohm impedance, and 50 ohm impedance on PCB?
please help me.
Thanks in advance,
The analog RGB signals in the cable are 75 Ohm. So you can run the analog signals to the decoder chip as 75 Ohm traces or you can place a 25/50 ohm resistor divider network right next to the input cable connector and then run the analog traces to decoder chip.
We've do it both ways depending on which reference board you are looking at. I prefer the resistor divider right next to the connector then the entire board can be a standard 50 Ohm impedance board, prefect for normal digital signals. You just have to make sure the signal amplitude is correct at the chip pin.
HS, VS, SOG (Sync on green) and DDC signals (SDA, SCL) are not 75 ohm signals?
So, Can i route them directly to my decoder chip (ADV7842) using 50 ohm traces on PCB?
Yes. Only the analog signals are 75 Ohm. SoG is derived from the green signals so you need watch it. Check out our reference designed like the ADV7842-7511. Advantiv™ EVAL-ADV7842-7511 Video Evaluation Board
Again is depends on which decoder chip you are using to how to handle impedance matching while maintaining the correctly signal amplitude
Thank you Guenter,
I referred EVM PCB file, in which it looks like same trace width used for 50ohm signals is used fro 75 ohm also.
And resistor divider network which acts as 75 ohm termination is also placed very near to connector. But i found below sentence in HUG of ADV7842 page no 481.
"The voltage divider 24 ohm/51 ohm, which acts as a 75 ohm termination (refer to Appendix B), should be placed as close as possible to the ADV7842 chip. Any additional trace length between the termination resistors and the input of the ADV7842 increases the magnitude of reflections, which corrupts the graphics signal. 75 ohm matched impedance traces should be used. Trace impedances other than 75 ohms also increase the chance of reflections."
How this point is taken care in evaluation board?
In the prefect world you would place the resistor network right next to the chip and run 75 Ohm traces from the connector to the resistor network. In the less then slightly prefect world we found that placing the divider next to the connector and running 50 Ohm traces to the chip worked well enough for the formats we were spec'd for. You should be safe from reflections as long as the 50 Ohm trace propagation time is less then 1/4 the pixel rate.
The real reason why I don't like mixing 50 and 75 Ohm traces on a single board because it adds to the layout complexity in regards to trace width and pre-preg thickness. I wrote a first order approximation tool found here
PCB Trace Impedance Calculator
that you can use to see how to create a stack up. Of course you should rely on the layout tool to calculate the final impedances.
The information you provided is very helpful
Retrieving data ...