PCB with mixed DGND and AGND

[Anonymous]

I am working on a PCB with both DGND and AGND.

I need to copper pour the PCB. I am struggling on how to connect DGND and AGND to make the PCB work.

What I should do, copper pour and name "DGND" on one side, and give name "AGND" on another side? There should be a way to connect them, do I need another layer or some components?

Thanks,

Dawn

[jorge_garcia · Accepted solution]

Hello Dawn,

I hope you're doing well. There's actually a few different ways to handle this. They are all work-arounds, in EAGLE all connections are defined by net name. So by definition, you aren't supposed to connect differently named signals without EAGLE complaining. With that said here are the work arounds.

1. You can use 0-ohm resistors to connect the different grounds. EAGLE sees this as another component so the DRC is happy, from the point of view of the DRC this is the cleanest solution since it won't generate any errors. Along the same vein you can create a jumper library with packages consisting of two SMD pads shorted together. This option is slightly less clean because it can create DRC errors.

2. Polygons with the same rank that overlap short to each other since they have the same priority. This can be used to connect DGND and AGND. This is the easiest way to connect these two signals together since all you have to do is overlap the DGND and AGND polygons a little. The downside is that DRC errors are generated where the polygons overlap.

I tend to favor option 2 and just ignore the associated errors, but you can pick whatever is best for you.

Please let me know if there's anything else I can do for you.

Best Regards,

[Anonymous]

Hi Jorge,

Thank you very much for you detailed instruction and explanation.

I have couples of questions about polygon, copper pour, and DGND & AGND connections.

 1. Regarding Polygon - Copper pour.

I got an impression that people usually define a polygon as GND, which makes PCB nicer. Do I need define polygons as AGND and DGND in my case?

 2. Overlap of AGND and DGND.

If I choose to use copper pour, I will define a polygon on the top as DGND, and another polygon at the bottom as AGND. Since the signals are different, can I use via to connect them? I know there are errors by DRC. From PCB function/fabrication point of view, is it OK?

Thanks

Dawn

[rachaelATWH4 · Accepted solution]

---

@Anonymous wrote:

 1. Regarding Polygon - Copper pour.

I got an impression that people usually define a polygon as GND, which makes PCB nicer. Do I need define polygons as AGND and DGND in my case?

 2. Overlap of AGND and DGND.

If I choose to use copper pour, I will define a polygon on the top as DGND, and another polygon at the bottom as AGND. Since the signals are different, can I use via to connect them? I know there are errors by DRC. From PCB function/fabrication point of view, is it OK? 

---

Hi Dawn,

Jorge has given you two good technical ways forwards for what you are trying to achieve but which you choose depends a lot on your circuit design and how well you've done your placement.

First question, how many layers is your board? Having complete separate layers for AGND and DGND may not be ideal unless you have a lot of layers and can spare two for these signals and it may not actually be necessary.

Can you place the components such that AGND and DGND are separated from each other rather than being mixed up across the board? Are there any components which connect to both AGND and DGND? How about power rails? Do the analog and digital parts of your board have different power supplies?

You see, it may be that with good placement you can use a single layer of the PCB with AGND and DGND sharing that plane. It may also be that depending on the nature of the circuitry that AGND and DGND can just be combined to a single GND so long as good placement of components ensures that return currents for digital circuitry do not flow through analog circuits and vice versa. If you do have to have segregated grounds then you need to pay attention to any signals crossing the boundary between AGND and DGND.

With regards to how to connect the two if you do need to keep two separate planes, either of Jorges methods is fine, pick whichever you are most comfortable with.

To answer your specific question about how to connect them if they were planes on each side of the board, it's not as simple as just putting a via through as the via would have to be named either AGND or DGND and would only connect the the side that matches its name so you'd need to put a jumper resistor or a polygon of the same rank to create a short on the other side.

Best Regards,

Rachael

[Anonymous]

Thank you Rachael,

So, in my case, I don't have to use copper pour (polygon), right?

Thanks,

Dawn

[rachaelATWH4]

You'll need copper pours still, but you need to understand your circuit and ensure your placement segregates the AGND and DGND nets so that you don't need two layers for routing them in. You can then do either a split ground plane or if your analog and digital are nicely segregated and it's appropriate for your circuit then you can combine AGND and DGND into a single plane. Can you tell us more about you circuit? Maybe then we can give you better advice on what might be appropriate.

Best Regards,

Rachael