shield signal pattern- clarification required

[abhi002]

Hi

Happy new Year 2007.

I have attached a jpg file of shield signal.

Is this type of shield signal is practical?What is the advantage?

Have anyone used this type of shielding?


Regards
Abhi

 

[Rame]

Hi,

It seems the routing are done in ground plane,it is best way to get rid if any emi problems by routing it in the ground plane.I have seen this kinda of board,when the boards are crucial to EMI issues.

Regards

Ramesh

 

[Rame]

Hey abhi,

in addition to my previous reply find the article from Dr Eric Bogatin which addresses to your need.


Are Guard Traces Worth It?
By Dr. Eric Bogatin



October 2006

The board is finally back from the fab supplier. You power it on for the first time and find that a sensitive LVDS line has 30 mV too much noise coming from an adjacent CMOS-level control line running at 3.3 V. The noise is only 1 percent of the control line voltage, but almost 10 percent of the LVDS signal. What do you do? How do you reduce the coupled noise between the two lines?

In the last design review, you remember that a colleague said that when he had a noise problem, he fixed it using a guard trace, which he swears by now. Should you add a guard trace between the LVDS line and control line?

A guard trace is just another signal line that routes between an aggressor line and a victim line. Its ends are often terminated with 50 ohms, shorted, or left floating. The idea is that this extra line “guards” the victim line and somewhat shields any noise that might try to couple between the aggressor line and the victim line.

In fact, if you add a guard trace and then measure the noise on the victim line the noise is dramatically reduced, by more than a factor of 5. But the reason behind this might surprise you.

In microstrip geometry, there is both near end noise and far end noise between two adjacent, co-parallel lines. About the only thing that affects the near end noise is the trace-to-trace spacing. If the coupled length is longer than 1 inch for a 300 psec rise-time signal, changing the coupled length doesn’t affect the near end noise.

Far end noise is less affected by spacing. However, increasing the rise time (rarely an option) or decreasing the co-parallel length decreases the far end noise. Of course, the best way to reduce and virtually eliminate far end noise is to route the traces in stripline geometry rather than microstrip geometry.

What’s the impact on near and far end noise from using a guard trace?

To fit a guard trace between the two lines, you must increase the spacing to 3x the line width. This allows you to insert the trace between the lines with a space on either side equal to the line width.

You can evaluate this problem by putting in the numbers either by calculation, using a variety of 2D field solvers such as Polar Instruments SI9000, or by measurement of specially fabricated test vehicles.

This example examines measurements on microstrip test lines using an Agilent E5230A VNA to take the measurements and Agilent’s ADS software to convert the frequency domain measurements into the time domain. In the example, an effective 1-V signal with a 100 psec 10-90 percent rise-time signal is launched into the aggressor line. The near end noise and far end noise are measured on the victim line in three situations:

Spacing is equal to the line width
Spacing is increased to 3x the line width
Spacing is increased to 3x the line width and a guard trace is added (the guard trace is terminated with 50 ohms on each end)
From the measurements shown in Figure 1, you can see that the near and far end noise when the traces are close together is serious: near end crosstalk (NEXT) of 2.5 percent and far end crosstalk (FEXT) of 15 percent.

By moving the traces farther apart, to a spacing equal to 3x the line width, the NEXT is reduced to 0.6 percent and the FEXT is reduced to 5.5 percent. This is a reduction of a factor of 5 in the near end noise and a factor of 3 in the far end noise.

By adding the extra guard trace between the two lines and terminating its ends, there is a very slight further reduction in the near and far end noise, but it is hardly noticeable.

Are guard traces effective at reducing noise? For near end noise levels at the 0.5 percent (-45 dB) level, guard traces are irrelevant. Just increasing the spacing to 3x the line width does all the work. Adding the guard trace provides no added value. If you need far end noise to be lower than 5 percent, you can decrease the coupled length, increase the rise time, or route the lines in buried traces.

However, when high isolation is needed, as in mixed signal applications where 100 dB isolation is important, a guard trace between stripline traces with ground vias stitched up and down its length is essential.

In Figure 1, the top graph shows the measured near end crosstalk on a quiet line with a 1-V signal on the aggressor line for the three configurations. The bottom graph shows the measured far end noise on a quiet line with a 1-V, 100 psec rise-time signal on the aggressor line and a 6-inch coupled length. There is virtually no difference in the noise magnitude between increasing the spacing between traces and adding a guard trace.










Question: Should the ends of a guard trace be open, shorted, or terminated with 50 ohms?

Answer: The most effective end termination for a guard trace is with 50 ohms. Though the initial noise in a victim line isn’t affected by the guard trace termination, if the ends are open or shorted any noise induced in the guard trace will reflect from its ends and rattle around on the guard trace line. This noise couples to the victim line and shows up for as long as 10 round-trip times of flights. Alternatively, you can add shorting vias to the guard traces spaced about 1/10th of a wavelength of the highest frequency component of the application’s signal.

Question from Brad of the Syracuse Research Corporation: What is a back-drilled via?

Answer: A back-drilled via is a normal through-hole via in a PCB that connects two signal layers, but the dangling stub hanging down from the last signal layer to the bottom of the board has literally been drilled out. A drill bit with a diameter a few mils larger than the drilled and plated hole drills a "blind" via to within a few mils of the lowest signal layer. This removes the copper stub and prevents a potentially disastrous resonance in the 5 to 10 GHz range. All high-performance backplanes use back-drilled vias.


Hope this article have cleared some of your doubts related to shielding.


Regards

Ramesh

 

[abhi002]

Hi,

It seems the routing are done in ground plane,it is best way to get rid if any emi problems by routing it in the ground plane.I have seen this kinda of board,when the boards are crucial to EMI issues.

Hi Ramesh,

thanks for the article.This is the same that i was expecting.But i doubt about your first reply because somewhere i heard that routing in planes are the higher causes of EMI.

Can you clarify it?

Regards,
abhi

 

[Rame]

Hi,

No,Routing in the ground plane is good for EMI issues.This was told by an SI engineer from Cadence,noida.but then i don't have any document as such to post.

Since iam pcb design engineer,i don't have in depth knowledge related Si Issues.But then,it is always good practise to route the critical signal close to the ground plane,like wise if you route it in the reference ground plane,it will be better then earlier.


You can ask some SI engineers out here,they might clarify your doubt.


Regards

Ramesh

 

[kender]

Since there are a lot of direct responses to your question, I feel like I can propose an alternative without deraining a thread. You can shield your signal, mainatin the inetgrity of your ground plane, save the routing trouble and make the board more testable. Just add a pair of coax connectors (SMA, MCX, MMCX etc) and connects the source and the destination with a coax cable.

 

[mystery]

I do not recommend to route on the gnd plane layer. You should avoid from big slots on the gnd layer, it may couse some other emi problems.

 

[abhi002]

thanks mystery.

as i think if u route in planes it can disturb ur return paths of other signals,the same as you split the plane.

i am just guessing,not sure.

abhi

 

[Rame]

Hi Abhi,

Still your looking for an answer here in the thread!.If your critical signal is routed in ground plane,it splits i do agree with that,consequently if i have gnd reference plane etched exactly to the critical signal above in the split plane(which has critical signal routed),the problem for any emi issues is solved.This will work for 6 layers and above,again here you need to be carefully in selected layerstackup beforehand to critical routing.



Regards

Ramesh

 

[abhi002]

thanks a lot for all the responses.

i think i got the answers to my question.