1. Home
  2. Electronics Design
  3. Some beginner board layout questions

Some beginner board layout questions

Hi,

I've just upgraded Eagle to the non-profit license, so I can now (in theory :-) do 4-layer boards.

  1. If I have a ground layer and I have one part as an analogue ground plane and another as a digital ground plane (two adjacent rectangles) how and where should they be connected?

  1. Given that I have a ground plane, should I still do copper pouring in the signal layers (and connect them to ground)?

  2. This probably isn't relevant for my first project (guitar-computer interface: differential signal, 192 kHz, 24 bit ADC with pre-amp and USB/FW), but which is the cleaner solution for, say, a single signal crossing: 2 vias with a trace on the bottom signal layer, or a zero ohm SMD with the other signal passing under it?

  1. One of the circuits I am copying/modifying has a 1uF / 63V electrolytic decoupling capacitor (directly in the signal path) before any amplification. Wouldn't a plastic (polyethyleneterephthalate) one be better, from a noise point of view?

  2. Is it OK/possible/desirable to place a via on an SMD pad (e.g. for resistors & capacitors to ground)?

  1. I suppose it's better not to route signals underneath opamps (from a noise point of view)? What if the path then has to become a fair bit longer? Is there a rule of thumb here?

Thanks for any answers!

colin

Reply to
Colin Howarth
Loading thread data ...

The usual advice is to connect under the point where the signal goes from analog to digital - the A/D converter, or the D/A converter that provides the interface.

The thought that you should keep in mind is that every digital signal track running over ground plane injects current into the ground plane (via the track to ground capacitance) whenever the singal changes, and you don't want this current to circulate througn the analog ground plane (where it can produce voltage drops which can inject curent into the analog signal traces.

It's less urgently necessary, but it can still rovide extra screening.

Routing the signal so that there is always ground plane and /or power plane between it and the second signal has to be better. At higher frequencies, the vias introduce discontinuities in the "transmission line" formed by the track running over ground plane, but this isn't usually important at digital audio rates.

Perhaps. The film capacitor will have less leakage current, but it will be bigger than the electrolytic, and consequently a better antenna for electromagentic interference.

It's not popular. The via can wick the solder away from the pad, and prevent the component from forming a good solder bond at the pad.

Not that I know of. A signal running over a buried ground plane isn't all that effective as a radiator or an antenna, so routing stuff under op-amps is less of a worry on a four layer board.

-- Bill Sloman, Nijmegen

Reply to
Bill Sloman

It' almost always better to have obe solid ground plane layer. Splitting or slicing grounds generally causes trouble. Just manage the analog part of your circuit carefully. It does halp to keep large circulating currents away from low-level analog stuff. Really low-level signals should be differential.

Not worth it.

A via in a pad can slurp off solder. Most people use a very short trace between a pad and a via, just long enough to get some solder mask on.

Depends on the signal. If it's unrelated to the opamp signal, like another auidi thing or a digital thing, keep it away. If it's part of the same signal, it's OK.

John

Reply to
John Larkin

Well, you paid for something that you don't own. Cadsoft can lock you out of your work product.

formatting link

You'd better religiously keep a backup of your work product's **full history**.

In the old days, you could swap EAGLE library files with others. Do that today and you could easily be screwed.

Proprietary software has gotten to a high rate of suckage.

Reply to
JeffM

Hmmmm. That's so odd. They don't come across as an evil company. More the opposite in fact with their pricing structure, OSX and Linux support, free "support" and encouragement of hobbyists.

I don't envisage much sharing of libraries myself, other than up and downloading libs to/from their website, which I suppose should be OK.

That said, thanks for the warning. The story you linked does sound monstrously unfair.

--colin

Reply to
Colin Howarth

They aren't, it's IMHO a great company. In about 5 years I never ran into any file corruption problems. Just make sure never to use schematic parts and such from people that loaded a hacked Eagle onto their PCs.

Best of all: No dongles that break off on a bumpy airplane ride and they let you legally install a 2nd copy for the road on you laptop. Now which other CAD company can rival that?

As for the ground split I (strongly) second John's opinion: Don't do that.

Caps in series: In the high fidelity audio world ceramics are usually not the ticket when in the signal path, and neither are electrolytics. A good film cap is best. At least use a smaller film cap in parallel if you have to use an electrolytic.

[...] 
--
Regards, Joerg

http://www.analogconsultants.com/

"gmail" domain blocked because of excessive spam.
Use another domain or send PM.
Reply to
Joerg

One nice thing about PADS (at least the version we run) is that anything - schematics, pcbs, parts, decals, libraries - can be exported and imported in human-readable ASCII, vaguely like an LT Spice file. Rarely a design will do something weird, and an ascii-out/ascii-in cycle cleans it up nicely. You can also do cool things with the ascii files, like run a perl script to create an FPGA pin list.

We stopped upgrading PADS at v5, since it was perfect and Mentor started changing things.

John

Reply to
John Larkin

ElectronDepot website is not affiliated with any of the manufacturers or service providers discussed here. All logos and trade names are the property of their respective owners.