Use of Ground Plane in a PCB/Layout

Hi, this is def. a newbie-kind of question, but I just breadboarded a little 5V regulated PSU for a project I'm doing. I am already making a PCB for the project and had some room left on the PCB, so I thought I would just design the 5V regulator into half the PCB.

My question is the proper use of ground plane. I have two similar-ish layouts here, and the in the post to follow.

Is there a problem using the ground plane as I'm doing, in the this post? Or is how I did it in the second post better?

Thanks,

Mike

And the version not using the ground plane as a gigantic ground...

Thoughts?

Thx.

Can you post a schematic? It's rather boring to reverse-engineer the circuit from a PCB (even if that simple)...

Thanks,
Samuel

Of Course. I have changed some cap values and added an additional flyback diode, but this is essentially it.

Thanks.

Mike

As it now stands..

Well, I meant the exact schematic. Anyway, what I'd consider:

* You're using three different high-frequency decoupling capacitor values (10 nF, 100 nF, 330 nF). This makes assembly more complicated than necessary, and is rather unlikely to provide any benefit. I'd just go with each a 100 nF at the input and output.
* The 2200 uF and 470 uF at the input are in parallel; the 470 uF provides no significant benefit, and you could skip that. If you think 2200 uF is not enough, increase this value (or use two equal values).
* The placement of the components seems slightly arbitrary. The high-frequency decoupling caps should be close to the regulator, with a short connection to minimize series inductance. The bulk output capacitor (33 uF) is not particularly critical, but probably makes most sense close to the output connector.
* I'd connect all components to a ground plane through thermal reliefs except the rectifier. This carries large peak currents which should not enter the ground plane. Use a dedicated trace to the smoothing capacitor (2200 uF) instead.
* It is unusual practice to place the parts values on the silk screen layer. I'd use designators (http://groupdiy.com/index.php?topic=60045.0).

Samuel

Wow! I'm humbled and grateful for your kind and thorough comments Samuel!

I'm driving this with a 120V AC - 10V stepdown transformer.

The reason for the odd layout is I was trying to make it as small as possible for a project I'm doing. I guess omitting some caps would help!

I thought that "more is better" when it comes to smoothing caps - my calculations showed around 600-700uF would be fine for this, but I wanted the regulator to have a smooth ride so I thought to beef up the caps prior to it. I'm new to using regulators so I guess I'm a little shocked they work so well with just a smoothing cap and a 0.1uF prior to input and 0.1 prior to output?

Regarding the labels, yes, great post! Makes so much sense.

I'll rethink some of this based on your thoughtful and kind input.

Thanks much!

Mike

OK it's late and I'm tired, but here's a first pass using your suggestions Samuel.

Any other thoughts?

Thanks!

Best,

Mike

* As mentioned before, C4 should be closer to VR1 than C3. Also I'd use the same fooprint for C2 and C4.
* Route the BR1-C1 connection on the top layer, so you don't have to break the ground plane. Same applies for the D1-VR1 traces.
* Connect VR1 directly to the ground plane, not through the top layer (now it's actually floating).

Samuel

Great points!

Actually VR1 is connected to a via that goes to the ground plane. But if it's better for it to just have a thermal pad that's fine.

Thx it's 3:26am and I can't sleep but I'll make suggested changes and post again tomorrow.

Thanks again resident genius Samuel!

All right...another revision.

Should the tiny caps be ceramic or does it matter? Right now I've got polyester film.

The regulator and smoothing caps have thermal pads for connection to ground plane, but I also added a trace to a via because the thermal pads weren't connecting on all sides due to proximity to other pads. Is that OK?

Any other thoughts Samuel?

Many, many thanks.

Mike

Phrazemaster said:

Actually VR1 is connected to a via that goes to the ground plane.

Click to expand...

Yes, but that bit of the ground plane was floating.

The latest revision looks good; the extra plane connects for VR1 and C1 are unnecessary, but don't hurt either. Standard practice to give more room between pads is to make them oval.

Both Polyester film and ceramic will work as decoupling capacitors here.

Samuel

Samuel, thanks for taking me to school. It was an unexpected gift and I know my work will be that much better because of you.

Thanks!!!

Hi again, still a nooby question, but do I need to connect the ground plane of this board to the chassis ground of my PSU? I have another commercial 5V PSU, a little board complete with transformer, and it does not connect to the PSU earth ground at all. It's a "floating ground" I suppose one might say.

Is this safe to do, or is it best practice to run a line from this board to earth ground? I'm thinking it's not necessary, but I wanted to make sure. The attached pic shows this board with an additional 0V GND connector, but again maybe this isn't necessary. You wouldn't run a ground line if you had a 5V battery in the case, so why would you here?

Thoughts?

Thanks,

Mike

This is a question that needs to be answered at the system level. Standard safety practice for "Class I" equipment (https://en.wikipedia.org/wiki/Appliance_classes) is to connect the secondary winding of the transformer (or more generally speaking, "circuit ground") and the chassis to safety ground, and use an appropriate mains fuse ahead of the mains transformer. This gives basic protection from insulation faults in the transformer (and other situations where dangerous voltages may become touchable).

Samuel

Thank-you Samuel. The article was interesting as well.

The secondary winding of this transformer is 20VAC, with a 10V center tap. I know you didn't mean to connect this to ground!

If I were to connect the ground plane of this board to the safety/earth star point in the power supply, wouldn't that drain off all the lovely +5VDC I just got through creating? Electrons find the path of least resistance, so if faced with a choice between a pure earth/ground connection or to run the voltmeter in my PSU, which would have more resistance, they would just short to ground, right? Leaving no power...

I am using the left and center tap of this transformer for this board. The outer taps are being used to power a main board that is in fact connected to the earth ground.

I'm sure this is very basic. Thanks for your additional thoughts.

Best,

Mike

OK I thought about this more deeply and looked harder at it. I see that adding a connection to the chassis/earth ground will not be a problem, as the +5VDC has no immediate return path as I misstated above (I think). Therefore there is no problem with adding a ground connection directly to the PCB ground plane.

Is my thinking correct?

Thanks,

Mike

Phrazemaster said:

Is my thinking correct?

Click to expand...

As far as I understand your concerns, yes. The +5 V is relative to the local "GND" net of the power supply, and connecting this to an external "GND" (safety ground) simply refers the +5 V to this without shorting the supply.

Samuel

Samuel! This makes so much sense!

Thanks!