# Contradicting ideas about differential signal route, confining fields vs Increasing impedance

By initial sense I think we must:

1. keep pair intra-distance as close as possible for field cancellation.
2. Fill surround of pair with GND plane and have via near to it to confine the fields, prevent incoming interference and making it.

The source have 200 ohm differential impedance and the load is 1k differential. I've decided to terminate the line with end termination. Now I must raise the trace impedance to 200/100 ohm to terminate it by 200/100 ohm by:

1. Increase intra-space as more as I can.
2. Remove surrounding GND plane.
3. Reduce trace width.

And these are contradicting each other can you explain why?

My working frequency is 12.2GHZ. (With respect to @ThePhoton)

2 helpful link: Differential impedance and Differential Trace Design Rules - Truth vs Fiction .

• If I remember from your previous question, you're working above 10 GHz. You should probably mention that in your post. – The Photon Jan 7 at 16:16
• The two most important parameters in determining impedance (single-ended or differential) are trace width and thickness of dielectric between trace and nearest plane or planes. You will have to make sure that your PCB stackup will work with your target trace impedance of 200 Ohms. Separation between traces in the differential pair will not have a large effect. You can keep the traces close for cancellation. I have never done a 12 GHz PCB design. I wonder if you need to use RF materials such as Rogers? – mkeith Jan 8 at 9:12
• @mkeith I have seen many clock termination recommendation and none of them recommended to match the line with low impedance of source ~10 ohm with line 50-100 ohm. 1.I can't understand why you are insisting on it. although in my application is not clock and is feed of VCO for PLL. 2.Why you wonder for Rogers? I've opted FR4 because I'm making it in small scale and i believe controlling impedance is not really issue. 3.How simply I can match with 250 ohm can you tell me it's theory? – mohammadsdtmnd Jan 8 at 11:28
• Examples where source, trace, and load impedance are equal: video, ethernet, LVDS, virtually all RF applications including bluetooth, wifi, various cellular and mobile applications. Whether this is required for you depends critically on how long your transmission line is compared to wavelength. Having mismatched impedances at 12 GHz sounds like a pretty bad idea. But a 1 kOhm transmission line may be physically impossible or impractical. – mkeith Jan 8 at 15:47
• 1kohm load in parallel with 250 Ohm resistor = 200 Ohms. You simply place an SMT resistor as close as possible to the load. Whether this will work at 12 GHz I don't know. Most resistors may have significant parasitic effects at 12 GHz. It will also result in most of the signal power going to resistor instead of load. – mkeith Jan 8 at 15:49

keep pair intra-distance as close as possible for field cancellation.

No! You need to adhere to a defined distance to get a defined wave impedance. What you describe is a coupled microstrip line.

Fill surround of pair with GND plane and have via near to it to confine the fields, prevent incoming interference and making it.

... in a defined distance to get a defined impedance.

In fact, you don't need a surrounding GND plane on the same layer – practically all field will be between the two differential conductors; what would be good would be a plane below!

The source have 200 ohm differential impedance and the load is 1k differential.

So, that's a high-impedance load and not really a low-impedance source. I'd recommend having two matching networks: one at the source to match the source to the transmission line impedance, and one at the sink.

You could then use an arbitrary transmission line impedance, e.g. the microwave-typical 50 Ω or the 75 Ω. In theory, 200 Ω should work (and would save you the source matching), too, but it might be hard to build using your PCB materials – it depends, can't tell without knowing with what you're working.

And these are contradicting each other can you explain why?

They are not contradicting. A perfect transmission line does not radiate, so your "as close as possible" simply isn't right – yes, close, but not "as close as possible".

Use a specific calculator to calculate the right dimensions for a coupled microstrip line on a PCB substrate of your PCB's thickness, with your PCB's $$\\varepsilon\$$, and on the frequency you work on.

• Nicely explained but I have seen: 'TI: "Route DP/DM traces close together for noise rejection on differential signals".' what's your idea? here: electronics.stackexchange.com/questions/145580/… and also you can see it here: ultracad.com/mentor/differential%20design%20rules.pdf – mohammadsdtmnd Jan 7 at 11:14
• That's for special cases, where your impedance requirements make the traces and distances largert than the simplified models (e.g. no field anywhere but between and below conductors) tolerate. If you use "typical" impedances on "typical" boards, that's no concern for you, and you simply do impedance matching. Think about it: if a line is impedance matched and the material is lossless, then as much energy as enters the line leaves it. So, there's no possibility for energy to leak and couple into something else (unless you didn't properly match). – Marcus Müller Jan 7 at 11:20
• Do you mean this is for typical purpose but your purpose is not typical? – mohammadsdtmnd Jan 7 at 12:57
• I think we cannot match everything, we can only match odd mode with one resistor between the lines equal to differential impedance of the line?! note the odd imp will increase by getting them away. – mohammadsdtmnd Jan 7 at 13:39
• If you say we need 50 ohm impedance you mean Zodd to be 50 ohm and Zeven is uot needed in differential transmission line? – mohammadsdtmnd Jan 7 at 14:06