Question for two-sided PCBs: Ground "areas"

I have question regardings two-sided PCBs:

Is it ok to have ground "areas" on both sides?

The one on the bottom layer is very ragged due to the many
conductor paths.

Or will this result in ground loops or something?

Sorry for asking this dumb question.

There is no problem with this, and it is quite common. Just make sure you tie both grounds together with LOTS of bare wires soldered to each side. Just drill holes where the grounds overlap, and run a wire through and solder. Lots of times a board used for RF will have both sides grounded by means of copper foil crimped over the edges of the board and soldered to the ground plane.

Adding groundplanes for circuits with Hi-Z nodes _could_ influence bandwidth to some more or less noticable degree if the line to plane spacings etc are small. But it won't happen right away.

Still, I prefer no groundplanes, using proper shielded boxes 'instead', but that's not based on hard facts. And if the 'nuisance' is already inside the box then just using a shielded box is not enough of course, more has to be done.

W.r.t. groundloops, you can have a 10-layer PCB and still no groundloops.


Interesting question, and I'm especially curious to the info from those who can base their ideas on hard facts.

Depending on the HF bandwidth of the signals your pcb will be handling the trace geometry will have more or less significance. In general impedance of grounds and power distribution traces are always important so making those traces robust is always useful.

What currents flow where can be significant for high current paths in the power supply, like the circuit formed by charging diodes and reservoir capacitors. In most cases it's easier to control ground integrity by keeping undesired noise (like cap charging currents) isolated and out of other clean ground paths, than to try to brute force it with fat traces. Better yet, use fat traces "and" carefully parse what currents go where.

Using a large ground plane does not mean that the voltage will be 0.0V at all points along that ground plane so be thoughtful about what currents are flowing where. A ground plane above and metal chassis below, promises some degree of shielding but sensitive, high impedance traces should still be keprt short and as direct as possible.

I find it useful when doing layouts to think of traces as small resistors, to better visualize how contamination by undesirable mingling of signals can effect signal purity.

JR

Ok, I think I need more knowledge regardings circuit design and so on.

This is concretely for my re-design of the Gyraf Calrec EQ:
http://www.groupdiy.com/index.php?topic=234793#234793

... and I have no idea which currents there go where.

Yeah, but no one else would have done the re-design and everyone starts at zero and so I thought I'll try it and most paths where somewhat copied from the Gyraf layout.
I think I'll jump into the cold water and try the groundplane only on the top layer and order a prototype PCB.

[quote author="sonicwarrior"]... and I have no idea which currents there go where. [/quote]
I didn't check that link, but if you approached it by using the groundplane whenever you needed a ground, then no groundplane at all and a careful starground would do better and keep better track of what runs where.

[quote author="clintrubber"]a careful starground would do better and keep better track of what runs where.[/quote]

Well, the problem is: I don't how do carefully do a starground and I then still wouldn't know where the currents go. I have marked every ground connection in the silkscreen layer with "GND", so I know where the connections to ground are.
That's why I think I need more knowledge regarding circuit design, circuits in general, etc. .

But as this would take months and maybe I'll never get it, because my free time is limited, I thought about simply groundplaning and stuffing a prototype to see what happens.
Before the groundplaning approach I had "upper" and "lower" paths for ground for each PCB. The groundplaning then simply widened these paths.

In many companies the circuit boards are not laid out by circuit designers but more packaging experts. The circuit designers will sometimes trick the schematic with multiple named grounds that are later combined to preserve a star ground (single path).

My only advice is to be very careful around power supply caps as they can have significant ground currents. Also power supply decopling caps spread around the PCB can dump ripple currents into local grounds if power supply not clean.

To be safe you could treat PS ground as separate from signal grounds and just join them once near the regulator grounds.

Relax and just do it.. if you make a mistake you will learn from it, and that's why god made xacto knives.

JR

[quote author="clintrubber"]Adding groundplanes for circuits with Hi-Z nodes _could_ influence bandwidth to some more or less noticable degree if the line to plane spacings etc are small. But it won't happen right away.
[/quote]

One other finesse on considerations for trace/ground sandwiches and proximities: the dielectric quality of PCB material can vary a lot. This is not just anecdotal audiophoolery: years ago Tektronix IIRC ran into significant signal distortions when they attempted to use trace/plane capacitances as an integral part of their vertical amplifiers, and found that the distortions arose from the peculiar dielectric properties of some batches of glass-epoxy material. They dubbed the phenomenon "hook" because of the appearance of the distorted step responses.

One would say that things have gotten better and more consistent, but they could just as well take a nosedive at any moment with the migration of just about everything to the Far East, or even just the deterioration of QA in any damn place.

So---for high-Z nodes be wary not only of the magnitude of the stray capacitance but also its quality, and try to minimize the potential effects.

Are there any recommendable books regarding PCB design for analog circuits (which cover and explain the mentioned issues)?

[quote author="sonicwarrior"]Are there any recommendable books regarding PCB design for analog circuits (which cover and explain the mentioned issues)?[/quote]

I am told Henry Ott did a very good talk at a recent AES convention about such things, but I don't have any of the material. Maybe someone in here does.

[quote author="bcarso"][quote author="clintrubber"]Adding groundplanes for circuits with Hi-Z nodes _could_ influence bandwidth to some more or less noticable degree if the line to plane spacings etc are small. But it won't happen right away.
[/quote]


So---for high-Z nodes be wary not only of the magnitude of the stray capacitance but also its quality, and try to minimize the potential effects.[/quote]

If the nodes are that sensitive, the best thing to do is "guard" that pin by surrounding it with the ground trace. Most data sheets will provide application info that shows ho to do this.
One of the more important things that Tek learned, besides the inter-electrode capacitance and dielectric absorbtion problems with some board material, is that distortion in circuits was greatly affected by the symetry of the layout. This is very important in pattern layout of balanced inputs, and a lot of routing programs do not have design rules to make sure the layout keeps things balanced. Most of these programs make the design "pretty". That is why experienced designers usually have to finese the design when the layout program is done.
Board quality can vary, but if you are using stock from someone like Rogers, they are pretty consistent. There is some good pdb layout info on the internet, and also in the usenet group Alt.Binaries.ebooks.technical.

I think I found a good beginners tutorial for PCB designing:
http://alternatezone.com/electronics/files/PCBDesignTutorialRevA.pdf

Another tutorial has many formulas which I don't really understand:
http://ece-www.colorado.edu/~ecen5797/course_material/layout.pdf
(I think this is more a "backing" of a lecture)

I found a book at Amazon:

The Art of Analog Layout
Roy Alan Hastings
# ISBN-10: 013129329X
# ISBN-13: 978-0131293298
http://vig.prenhall.com/catalog/academic/product/0,1144,0131464108,00.html

But it's very expensive (> 70 Euro for paperback) and I'm not shure if "layout" means really "PCB design". :?

"The Circuit Designer's Companion" from Tim Williams seems to be more aimed to digital PCB designs. :sad:

[quote author="sonicwarrior"]I found a book at Amazon:

The Art of Analog Layout
Roy Alan Hastings
# ISBN-10: 013129329X
# ISBN-13: 978-0131293298
http://vig.prenhall.com/catalog/academic/product/0,1144,0131464108,00.html

But it's very expensive (> 70 Euro for paperback) and I'm not shure if "layout" means really "PCB design". :? [/quote]

We have it here, it's a good book but for integrated circuits,
so you better skip this one :!:

Regards,

Peter

[quote author="clintrubber"]
We have it here, it's a good book but for integrated circuits,
so you better skip this one :!: [/quote]

Ok, thanks for the info. :thumb:

[quote author="clintrubber"]
We have it here, it's a good book but for integrated circuits,
so you better skip this one :!:

Regards,

Peter[/quote]

Now that would be some ambitious DIY.

"Honey, did you remember to turn on the silane like I told you??"

Another online resource which might be interesting: layout.pdf

I did some extensive research for a book on PCB design some time ago but much to my surprise there seems not to be much out there. There are several books covering IC design and EMC issues--not sure if they are of much help.

Samuel

here's another related paper:

http://focus.ti.com/lit/an/slyt166/slyt166.pdf