Just wondering why in alot of pcb design guides they suggest separating the digital and analog circuity (i.e. grounding and supplies) and at the same time have a commmon reference point somewhere in the circuit (i.e. join analog ground to digital ground), I realise that the fast digital switching could induce noise on some sensitive analog components and separation is nesscesary but why then join both grounds at one point? also as a separate but poss related question what is meant by the term grond loops in pcbs and why avoid them?
Bolt the above to the chassis, connector shells, heatsinks, etc as many places as practical.
Large currents flowing in the ground plane/chassis structure can induce small voltage drops in the sheet resistance of the ground plane ("ground loops"), so the plane may not be truly equipotential. Be aware of that and take suitable measures.
On a PCB, ground performs at least 3 functions. It is a power supply distribution path, a reference voltage and a shield.
If an analog function treats it as a precision reference voltage, then currents passing through that ground from supply distribution, cause resistive drops, and changing currents from digital logic loads also produce inductive drops. The split ground, single point connection method is an attempt to keep the distribution drops separate from the reference voltage. I often pick one point on the supply distribution ground plane or grid and assign this point as the analog reference ground, connecting it to each function that needs to agree on what exact zero is, by branching traces from that point. Since these reference lines carry almost no current, they don't need pours. If a very sensitive analog function needs quiet shielding, I isolate that part of the distribution plane (or place an island in a layer above it) and tie that shield back to the reference point with one of those branches. But non reference power nodes still connect to the supply distribution layer, to keep current out of shields and reference lines.
If you keep in mind these 3 separate ground functions, you can usually come up with a layout that satisfies all 3, with few compromises.
Excellent addition to my list. This is especially important if some load uses high current, fast edged pulses. Many a beginner has been nailed by using the ground plane as a return to the driver (past sensitive circuits), forgetting that all that (di/dt) is going to create quite a ripple in the ground pond when it comes splashing through. I always try to return the ground side of such loads with a separate trace (right along side, or on on both sides of the outgoing trace), back to the point where the driver is bypassed, so almost all that noise stays out of my ground plane.
I still prefer the 0805 .1uf X7R type. I have had bad luck with anything in a Y5V or Z5U. My stuff hasn't been so miniaturized that using devices smaller than 0805 makes much difference. And the hand rework and modification on small runs is so much easier.
Where there are conductive connections from PCB to chassis make sure that there isn't a huge potential discrepancy between metals, to prevent this link from deteriorating over time. Nickel plating is one method but at the end of the day much of this is guided by current environmental regulations.
Well.... the two have to have a common potential *somewhere* !
Actually it's not fast edges IME.
If the digital ground current flows in the analog ground there will be a small potential due to the resistance of the pcb trace that will enter the analogue signal.
The current is typically connstantly changing so you get 'noise' or tones.
In audio applications you can 'hear the cpu' or whatever. Check out a cheap mobo with integrated sound for example.
See above. It's better than joining them at the psu btw.
Never seen a ground loop in a pcb as such.
A ground loop normally refers to a situation where 2 grounded pices of equipment are connected and a ground current flows in the interconnect due to the 'wall socket' ground potentials being unequal.
As long as it's not made from some boutique ceramic. Remember when all the high density caps suddenly became unobtanium in the 80's? IIRC this was caused by an accident at the only chemical plant that seemed to make the needed ceramic. Lots of Aspirin was consumed in them days.
I usually go for 0.1uF since even the contract assemblers in remote locations will have oodles of them. I never really found a huge difference in RF performance WRT to the smaller sizes, at least not for bypassing.
Chip makers who make ADCs etc usually specify that the digital ground and analog ground connect only under the chip. This is often impractical to do.
Most things with digital and analog circuits also contain ADCs and DACs. Neither of these work well if there is a difference between their digital and analog grounds.
also as a separate but poss related question what is
These days, it is common to have digital stuff, some analog stuff and some sort of power supply all on one PCB.
The digital area almost always determines the number of layers in the PCB and that number is greater than the analog of power supply sections need. You can take advantage of this.
In the digital section the Ground and Vcc layers work as AC ground planes. They naturally form a capacitor. The bypass capacitors add to the coupling between them. If the analog section is going to be run from the same Vcc, it is a good idea to put some impedance in the way to keep the digital sections currents out of the analog sections supply. If you can prevent the current in the Vcc, you've mostly prevented it in the ground plane.
In the analog section, you should use the extra layers to make things that are AC ground for the analog. If the analog doesn't run on the digital's Vcc, take that layer over as an analog supply.
If the analog section is processing lowish frequencies you want to add an extra ground layer in that area to be the analog ground plane. You need to make sure that no large currents can pass through this added layer. This means that you often have to be careful about where and how many places you hook the thing to the overall ground. Beware that the analog circuits also make currents. It is also common practice to add even more grounded copper on the top and bottom surfaces of the PCB. It doesn't cost anything really to add it so go ahead.
In the power supply section, you again want to add more ground plane. The best I've been able to come up with as a general description of what to do is:
Imagine the power supply as being enclosed in a copper box with one hole in it. In your thinking, all of the lines that come and go from the box should pass in and out of this hole.
Right at the hole, they should have a capacitor to ground. Ideally each line should also have some series impedance in it. The inductors normally used in the supply design can be this impedance.
Now if you take this box and merge it with the top surface of the PCB, the bottom of the box will become one of the added ground planes.
About chassis grounding:
You often will find you have competing requirements. For high frequencies, you want the electronics solidly connected to the chassis. For low frequencies, you may want only one point (near the signal entry BNC for example). For safety, you may want no connection. For ESD you may want some connection. I've used parallel RCs to make this all happen at once. It adds a lot of extra capacitors though.
If this equipment is going to be rack mounted with other equipment, never connect the PCB's plane to the chassis at both the front and the back panel. If you have to, float a box within the chassis do so. Racks almost always have 1 billion amps of current circulating in them. I have measured voltages from front to back over 1.5Vp-p. Debugging a problem that only happens when the screws are tight can take days (trust me).
A good question I'd say. Power supplies have large return currents which are grounded and as the resistance of the grounding wire is low but NOT zero a significant voltage drop occurs over the conductor. A low power circuit like a digital one which connects to the same ground would have a reference voltage above ground potential. The switching noise you mentioned can cause considerable ground voltage variation and even if the grounding wire is short , high frquencies in low parasitic inductances translate into higher voltages. Your question is why use a common point as a ground ? Imagine if each IC was connected to the nearest grounded conductor on the PCB. The ICs ground potential would be adversely affected in the ways mentioned above by the seperate circuitry which is connected to ground . A seperate wiring to one point somewhat solves the problem till audio frquencies of 20kHz.
At higher frequencies though the inductances of the grounding wires create more problems then they solve ... so a distributed ground plane is sometimes used , power and ground buses and so on ...
A lot more can be said but just ask if you need more info.
Yes, but I was giving an example of a typical PCB with many circuits including a digital circuit and a Power supply. The current in any one of those circuits (which may include 1 or many seperate digital circuits) is less then the current flowing through the Power supply cables. To be more clearer ... If you had a digital circuit with 20A flowing through it the current flowing through the Power supply cables is greater so that would make it low power compared to the Power supply. OK I know a better terminology could be used but I hoped I was understandable.
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.