Hi all,

I'm designing an amplifier that operates in the tens of MHz range and have been following this guide from TI: http://www.ti.com/lit/an/sloa046/sloa046.pdf

However, right it in the beginning it states "To achieve a good high-speed layout, a two-layer PCB is the minimum requirement". I'm using a single-sided design right now. So my question is: how necessary is a two-layer PCB for my application (amplifier in tens of MHz)? I am using surface mounted components and trying to keep my traces short and far enough apart to prevent capacitive coupling. I'm just worried that I'm screwed from the get-go by using a single-sided design.

Thank you for your time!

 

Getting a high frequency design to work properly requires a low impedance ground which is readily provided by a ground plane. The becomes difficult with a single sided board but it may be possible, depending upon the number of components and the circuit configuration. This involves using a "flooded ground" where basically all the area between and around traces is the ground plane. The trick is to layout the parts and route the traces so that all high frequency signal returns (including decoupling caps) go to a solid contiguous piece of this ground. Connecting different parts of the ground together with a low impedance connection can be difficult.

Why are you using a single-sided board? Are you building yout own?

 

Cool thanks for the swift reply. That is my layout right now, I basically ground the underside of the board. Then I poke holes wherever I want ground to be and solder a small wire through these holes to the underside of the board. So I suppose I am flooding the whole board with ground. However, I'm not routing all my traces to one piece of this ground so this is perhaps where I'm getting my capacitive coupling problems.

I am building my own board. Probably the main reason I'm using single-sided is because I'm not sure how to design a double-sided board and thought I could get away with single-sided if I was clever. I suppose I could try routing all my ground traces so they all return to one piece of ground. If the resulting trace length from this ends up getting too long I may need to do a double-sided design. Does anyone know of any good design guides for double-sided designs? I'm not sure where to begin. Thanks again!

 

If the bottom of the board is a ground plane, then how do you run the traces? You don't have to route the traces to one spot on the plane (which defeats the purpose of the plane). The plane is the ground and you connect all grounds directly to that, keeping the ground traces as short as possible.

The problem with RF grounds is generally not capacitance, but the inductance of the traces.

Here's an app note, that may help (see page 5).

 

Yeah think I may have miscommunicated my PCB set-up previously. I figure I basically have a two-sided board. I'm using a FR4 1 oz copper board. I ground the bottom and then have all my circuit traces on the top. I then just have a pad, a hole, and small wire run through the hole and soldered onto the back wherever I want ground.

Thanks for the note! It's good to know I should keep my trace lengths less than 1/30th of a wavelength. Also what are people's thoughts on having turns in traces? I know 90 degree turns are no good so I've been doing two 45 degree turns.

Also, I was thinking about running ground traces in between some of the signal traces that are particularly close together. In the TI document I linked earlier, it stated that:
"If signal traces run parallel due to shortage of space, a gap of at least three times the signal trace width should be maintained. Better decoupling is provided if a grounding trace is routed between the two signal traces."

So, in some parts of my board the signal traces are pretty close (.3 mm traces spaced .3mm apart) and obviously don't fulfill that requirement. I'm hoping to have ground holes nearby so that they will couple to ground rather than coupling to each other. What do y'all think?

Thanks!

 

................................

Also, I was thinking about running ground traces in between some of the signal traces that are particularly close together. In the TI document I linked earlier, it stated that:
"If signal traces run parallel due to shortage of space, a gap of at least three times the signal trace width should be maintained. Better decoupling is provided if a grounding trace is routed between the two signal traces."

So, in some parts of my board the signal traces are pretty close (.3 mm traces spaced .3mm apart) and obviously don't fulfill that requirement. I'm hoping to have ground holes nearby so that they will couple to ground rather than coupling to each other. What do y'all think?

Ground points nearby will have little effect on coupling between traces. You either need to separate them further or run a ground trace between them to minimize coupling if the traces are carrying sensitive signals.

Incidentally the coupling between traces can be inductive as well as capacitive.

 

Thanks for the reply. Two questions:

1. Aren't I effectively making a ground trace if I have a hole to the grounded underside and then soldering a wire through. I think I would be flooding the copper surrounding the hole with ground, making it as if there was a ground trace.

2. I thought inductive coupling would be more of a factor at lower frequencies? At the higher frequencies, the inductive reactance would be rather high and there would be a higher resistance to a change in current and thus perhaps a greater resistance to the electromagnetic induction required for inductive coupling.

I guess to prove this I would need a relation between a change in current and the mutual inductance between two conductors. I'm not really sure how to calculate mutual inductance for anything but a transformer so I guess I'll start with that. The induced emf is proportional to the change in flux and flux is dependent on the number of magnetic field lines "cut" by the surface enclosed by the secondary conductor (loop in the case of a transformer). Since the density of these magnetic field lines is proportional to current, any resistance to a change in current will result in a resistance to a change in flux. This effectively results in a resistance to electromagnetic induction that is proportional to the inductive reactance which increases with frequency....I think. Not sure if my logic checks out or if I screwed up the E&M somewhere. Anyway I kind of got carried away but it's pretty neat stuff to think about. Thank you for all your help!

 

1. Yes, the the copper on the bottom acts as ground plane so any wire through the board and soldered to the plane acts as a ground trace.

2. Inductive coupling can be a factor at high frequencies when the trace acts as a transmission line. The characteristics of the transmission line are determined by the line inductance and capacitance. Typically the characteristic impedance of a trace over a ground plane is in the neighborhood of a hundred ohms.

 

Sweet thanks. I thought transmission line considerations came into when the length of the line divided by the wavelength it's carrying was greater than 0.01. Seems like for a 50 MHz signal (6m wavelength) I would need a trace length greater than 600mm. Since my board is about 80mm by 60mm I think I'm ok. Thanks for all your help! I've learned a lot through this whole discussion.