PCB Layout - Ground Shielding of High Speed Internal Traces 1

[jmeyer84]

I have a 10-layer PCB design with a controlled impedance of 50 Ohm +/- 10% for all four internal signal planes. On one of the signal planes, I have a signal that carries a 25 MHz clock signal for an LCD. This signal appears to contain several other frequencies and is far from the intended square wave I was hoping for. The trace itself is routed away from other high frequency signals and switching circuits and any other signals that are routed by it are perpendicular. Other associated LCD data signals look good.

I'm wrestling with the idea of running a ground shield trace on both sides of this signal to help protect it from any unwanted EMI. I've seen this done on external layers, but never on an internal layer. I have concerns with it also interfering with the controlled impedance.

Is shielding this signal an appropriate move? Will it interfere with the controlled impedance? Is this typically avoided on internal signal layers?

 

[MikeHalloran]

First, eliminate possible sources of reflections.


Mike Halloran
Pembroke Pines, FL, USA

 

[Comcokid]

25 Mhz is not very fast these days. As MikeHalloran indicated - check for reflections on your controlled impedance trace. Make sure it is sourced and terminated properly. Make sure you're following proper signal layout procedures anywhere you change layers with the signal. Make sure as your stripline travels from source to destination there are no slots or gaps in the ground/shield layers above or below the trace. You indicate it is the clock for an LCD - does that mean it travels through a flex circuit to a flip-chip die on the LCD that is the driver, and is that flex circuit also impedance controlled?

 

[jmeyer84]

Mike and Comcokid, thank you for your input.

I have made the effort to eliminate potential noise sources from the circuit by disabling and bypassing the few power supplies I have available. I have also disabled other potential sources including memories and communication buses. All has had little to no effect on the signal. All other LCD RGB data signals that are routed in the same area with the same length look very clean. Regarding the ~3" flex cable for the LCD, I do not know if it has a controlled impedance. I can tell you that the signal looks the same regardless of whether the cable is connected or not.

So far, I've been able to clean up the signal through a simple RC filter. It looks better, but it's ultimately not the clean signal I'm after. At the moment, I'm modifying the design to include a couple new circuits, including a spread spectrum clock IC and a high-speed comparator just to try out. The LCD works fine as it is, but I'm concerned with any reliability or stability issues this signal may cause under unknown or noisy conditions.

 

[Noway2]

A couple of thoughts on your clock signal. One, it isn't so much the clock frequency that determines whether or not a design is 'high speed' or not, but the edge transition rate. I assume that this is a digital pulse signal, what are the minimum rise and fall times? Two, how did you terminate the clock lines? You mention using an RC filter and putting an RC on the end of the line is a valid method of terminating a run. It is called AC termination and typically the R and C need to be picked and then tuned to the design. Three, is this clock source driving multiple devices? If so, did you create stubs off of the clock line or did you router it as a pass through on the pads? Too many stubs can cause issues. Four, does your controlled clock line transition to a difference reference plane (adjacent power / ground layer) when you switch layers? Alternating reference planes will disturb the impedance see this pdf. Five, are your vias designed sufficiently to not alter the impedance? Six, it sounds like you've taken geometry into consideration, but do you have sufficient height over separation for any long runs of parallel conductors?

When you say, "far from the intended square wave", what does this signal look like? Stair stepping and ringing, as well as runt or inverted pulses are strong indications of a reflections problem.

Also, is your driver capable of delivering into a 50 ohm load? In my experience, 50 ohms is pretty stiff. What are the dimensions of the trace (width, height to reference)? How much variation is there and do you do things like make 90 degree turns?

 

[Comcokid]

One other question - How are you going about probing the signal to see it on a scope? Hopefully not with a probe using a long ground lead. In other words - make sure your method of looking at the signal is not creating the problem you see or making you chase the wrong problem.

 

[DRWeig]

Maybe give us a picture of you oscilloscope trace?

Best to you,

Goober Dave

Haven't see the forum policies? Do so now: Forum Policies

 

[Noway2]

Excellent point from Comcokid: be sure that you are seeing problems, not artifacts of your probing. Here is a link to an article that talks about how to make a "shop probe" using a piece of 50 ohm coax, a 1K resistor, and a BNC connector. It is slightly off on the voltage but will give you a much more accurate depiction of the edges. Keep the ground wire as short as possible and don't use a snap hat and those flying leads.

 

[Noway2]

Forgot the link:

http://www.sigcon.com/Pubs/straight/probes.htm

 

[DanEE]

Good point about suspecting method of probing..

With (suspect) difficult scope probing situations, I've found using a dual trace scope, using two scope inputs with "Add & Invert" options set between the two scope channels (to create a fully isolated, differential scope input), one probe tip on your ground (or signal) reference point, and the other probe tip on the signal of interest..

Scope probe ground leads are NOT connected.

This eliminates any ground loop and common mode noise between the scope and the circuit of interest, subject to the longitudinal balance specs of the scope which should be very high...