PCB Ground Question

Thread Starter

mattd860

Joined Jan 9, 2016
58
Hi all - Can you please comment on the grounding technique that I've used in the PCB below? The top layer (red leads) carry all the positive voltage and the bottom layer (green leads/plane) is the ground.

Basically the entire bottom layer is a single ground plane. I've surrounded the 28-dip IC and relays with a ground plane to reduce the affects of interference. All grounds are connected to the ground pin on the B1 connector.

I just want to make sure my grounding method is ok or not. I'm not sure if using a single ground plane to ground everything on the board is ok.

Thanks!

CircuitBoard1.JPG
 
Last edited:

SLK001

Joined Nov 29, 2011
1,548
Your ground plane looks terrible! For instance, the ground for C2, C3, C4, C7 and C8 are HIGH IMPEDANCE grounds and are the LAST things you want ground to be. Also with VR1 and VR2. Also, get rid of your heat reliefs on the rest of your grounds.

The best practice would be to flood both sides with ground plane and stitch them together with thru vias.

What PCB package are you using? It looks really primitive.
 

Thread Starter

mattd860

Joined Jan 9, 2016
58
I used this to create the PCB - http://www.expresspcb.com/expresspcb. I'm not married to the program but I tried a couple and I liked this the because it was easy to create custom components and like to a schematic.

Can you please explain the problem with the high impedance grounds of the capacitors? This circuit works fine on my breadboard but my breadboards isn't using a ground plane.
 

crutschow

Joined Mar 14, 2008
25,121
SLK001 is referring to the leads from the capacitors and other components to grounds.
All components going to ground should directly connected to the ground plane underneath them (such as C1 is).
There's no reason for that cutout in the middle of your groundplane.
 

crutschow

Joined Mar 14, 2008
25,121
...........
Also, get rid of your heat reliefs on the rest of your grounds.
................
If you get rid of those, it makes it difficult to solder since the ground plane pulls away the heat. That's the purpose of the heat reliefs to a ground plane.
 

Thread Starter

mattd860

Joined Jan 9, 2016
58
SLK001 is referring to the leads from the capacitors and other components to grounds.
All components going to ground should directly connected to the ground plane underneath them (such as C1 is).
There's no reason for that cutout in the middle of your groundplane.

Thanks! The components in the 'cutout' such as the capacitors and the voltage regulators are connected to the ground plane via the green leads. It may be hard to see but the leads are connected right to the plane.

I designed it this way because I was worried about bridging the leads on the components when I solder them. Perhaps I was overly cautious about this.
 

SLK001

Joined Nov 29, 2011
1,548
If you get rid of those, it makes it difficult to solder since the ground plane pulls away the heat. That's the purpose of the heat reliefs to a ground plane.
That's true. However, heat flow and electron flow (like to GROUND) are EXACTLY the same. If you impede heat flow, you also impede electron flow - thus causing problems with your circuit.

There are ways to make it easier to solder components to a ground plane (such as preheating with a heat gun). However, there are no easy ways to make it easier for electrons to flow once the copper is laid. This circuit is all thru-hole construction, so there is really no problem in soldering the parts.

If you want a place where ground WILL cause an issue with THIS board, the crystal H1 with its parallel capacitors C7 and C8 will NOT be at the frequency wanted. It may be close, but sometimes "close" isn't good enough. It is up to the designer to determine just how close is good enough.
 

Thread Starter

mattd860

Joined Jan 9, 2016
58
If you want a place where ground WILL cause an issue with THIS board, the crystal H1 with its parallel capacitors C7 and C8 will NOT be at the frequency wanted. It may be close, but sometimes "close" isn't good enough. It is up to the designer to determine just how close is good enough.

SLK - Can you elaborate on the issues with the crystal H1 and capacitors? I am free to move parts around to make them work as designed.

Please take a look at the new design below. I've made an additional ground plane on the top layer to further dissipate heat. It should also be known that I will be installing an aluminum heat sink underneath each of the Voltage Regulators which is why I've left all the free space around them.

CircuitBoard3.JPG
 

SLK001

Joined Nov 29, 2011
1,548
SLK - Can you elaborate on the issues with the crystal H1 and capacitors? I am free to move parts around to make them work as designed.
Your original layout had approximately 8 nH of inductance in series with the capacitors. This newer layer is better, but still has higher inductance than it should. Make the thickness of the traces to the xtal as wide as the pin on the IC, which will further lower the inductance of those lines. I would also rotate C7 and C8 so that they are parallel to each other - there is enough space on your board. I am assuming that the IC is some type of processor, so a slightly off crystal frequency isn't that big of a deal. In the past, I have had crystal oscillators in the 100MHz region that needed to be exact down to the hertz. In that range, everything in the layout was important and needed the correct attention.

You should also turn miters on and limit your traces to 45° increments. It will make your board look more professional.

Do you have to manually add the ground pour?
 

tindel

Joined Sep 16, 2012
716
Usually you don't want to have a ground plane under a crystal and the leads coming from it. The ground plane below the crystal and its traces adds capacitance to the line which could potentially stop the crystal from oscillating.
 

crutschow

Joined Mar 14, 2008
25,121
That's true. However, heat flow and electron flow (like to GROUND) are EXACTLY the same. If you impede heat flow, you also impede electron flow - thus causing problems with your circuit.
True.
The question is: how much of a problem?
I can't imagine many circumstances where the length of the 3 or 4 short traces in a typical heat relief contribute enough resistance or inductance to affect circuit operation, unless you get into the GHz region.
 

crutschow

Joined Mar 14, 2008
25,121
Ok. I'll work on the 45 degree angles. In the mean time. How does this look?

View attachment 100790
For minimum inductance, the ceramic caps C2, C3 and C5, which handle the high frequencies, should all be mounted directly connected to the main trace, not with a short stub going to the trace.
You might also want to do the same with C7 and C8, turning them 90° and mounting them between A1 and H1.
 

Thread Starter

mattd860

Joined Jan 9, 2016
58
Alright it was a bit of a squeeze but I got it all to fit. The circuit works fine on my breadboard with really long leads. I didn't trim the leads on the caps so they are just sticking high above the breadboard holes. But if getting rid of the stubs makes this better and/or more reliable long term then I'm all for it. How does the grounding plane look?

CB5.JPG
 

SLK001

Joined Nov 29, 2011
1,548
True.
The question is: how much of a problem?
I can't imagine many circumstances where the length of the 3 or 4 short traces in a typical heat relief contribute enough resistance or inductance to affect circuit operation, unless you get into the GHz region.
Actually, at VHF frequencies this can become an issue. It's like a death from a thousand cuts - a gradual degradation of circuit performance that make troubleshooting almost impossible.

I'm not saying that at the OPs frequency the thermals will affect the circuit performance that much. I don't use thermals - ever. I have seen research that shows the solder errors from non-thermal relieved boards are no higher than those with the reliefs (tombstoning, etc.). Better soldering profiles mostly fixed that problem.

Soldering thru-hole components without thermals is no more difficult than with thermals - it was done for years before thermal reliefs were devised.

@mattd860 Why do you have two voltage regulators in series?
 

Thread Starter

mattd860

Joined Jan 9, 2016
58
@mattd860 Why do you have two voltage regulators in series?
First voltage regulator reduces 14vdc down to 9vdc and the second voltage regulator reduces 9vdc down to 5vdc. When I only had the 5v regulator it was getting too warm even with the heat sink. Now both regulators stay luke-warm at best.

Might switch to a dc-dc switching regulator in the future but for now I just want to work with this one unless there is a major compelling reason not to.
 

crutschow

Joined Mar 14, 2008
25,121
Alright it was a bit of a squeeze but I got it all to fit. The circuit works fine on my breadboard with really long leads. I didn't trim the leads on the caps so they are just sticking high above the breadboard holes. But if getting rid of the stubs makes this better and/or more reliable long term then I'm all for it. How does the grounding plane look?

View attachment 100795
Looks better to me.
Perhaps it doesn't make a difference in your circuit, but it's just good practice in general, to keep traces as short as possible (thus minimizing lead inductance) for the capacitors that are filtering the high frequencies.
 
Top