how to check ground plane connectivity

[vixo]

I ordered some boards designed in Altium, but when I got them back some of the grounds aren't connected. I usually do a ground fill on the top and bottom layer to connect all the grounds, I do a DRC check which I rely on to show any nets that aren''t connected.

Does anyone have any idea why this might not show that some of the grounds aren't connected together? if i can't rely on this, is there another way of checking? This seems like such a fundamental flaw I cant quite believe its happened

[vixo]

I just found that it's actually a board error, thankfully. The problem seems to be that the ground connection was relying on one very small via or through hole plate which wasn't quite OK. is there a way within altium to evaluate the connection between two places?

[Bud]

As a sanity check i turn all layers off and check if any rat nest connections still exist. But even with a single via, no matter how small,  connecting two ground pours there would be no rat nest wires, so the designer have to be diligent.

[T3sl4co1l]

The problem, is you've already failed -- a ground pour so tenuous that you have to ask this question, is just begging to have EMI related issues.

The fix?  Stuff it full of vias, tying top and bottom ground together frequently.  Particularly around ground pins, trace crossings, peninsulas, islands...  Doesn't have to be utterly blanketed; they can be every few cm or so in low density areas: along traces, in empty areas, around the board edge, etc.  A few in parallel should be used in critical areas, like around switching converters and RF circuits.

Certainly, such precautions are not needed on every board; if you're only doing DC and low frequency signals, it's probably not going to matter.  But it's good practice to do so anyway, so that when you do have a board with high speed signals (including digital logic, microcontrollers and whatnot), you'll be prepared.

But even then, just for DC, you may find a circuitous ground-return path drops an obnoxious amount of voltage, or blows out at high currents.  Or you may discover instability in active circuits, because whether or not you're intending to use an op-amp at "just DC", the fact remains it's an active component with bandwidth into the MHz!

Unfortunately there isn't a tool to automate optimal placement of stitching vias.  In Altium, there is a tool to generate vias on a general grid, and around critical nets.  (Possibly you can just flag all nets with it?  I'm not sure if it removes overlapping vias properly in that case.  Something to try.)

Tim

[PlainName]

I tend to run proper tracks around the ground and power pins, before plane filling, to catch exactly this kind of problem. Additionally, sometimes a polygon fill can look OK but the route the power has to take is quite convoluted, and having to place an actual track will show that up pretty quickly

[thm_w]

I tend to run proper tracks around the ground and power pins, before plane filling, to catch exactly this kind of problem. Additionally, sometimes a polygon fill can look OK but the route the power has to take is quite convoluted, and having to place an actual track will show that up pretty quickly

Sure but this is a waste of time when you have a design rule check that will look for you.

High power paths are different story and those should be manually inspected as you say.

[julianhigginson]

Well, you could buy the PDN analyser plugin.... set it up right, and it might possibly find that single via current path issue for you.

But as already mentioned... for a problem like this, what you're looking at it a failure in the design process.  Altium just checks connectivity exists or doesn't. As a PCB designer you place parts and route various paths and create planes so that the product has good power and signal integrity.. if it's even possible that a single via break can cut your ground net in half, then unfortunately the problem isn't with the software. And as hinted by Tim already, chances are you're going to have other knock on issues from this design that haven't tripped you up yet.

It would be comforting to feel that if you can apply enough rules to check a PCB layout that *anybody* can do a good PCB design (and maybe Altium pushes this idea a bit with their marketing communications?) The reality of the situation is that simple rules will help a lot for tiny details, but at more fundamental levels this is not the case, so that's false comfort.  Think of a word processor program for instance... it has spell check and grammar check built in, but that can't stop someone from typing up an argument with fundamental logical flaws, will it? All it can do is make sure a logically flawed mess is properly spelled, and grammatically correct.

And I don't say this to belittle you or bring you down... everybody who does anything worthwhile starts with zero experience at some point, and they get the experience to do good work by doing stuff they're not experienced enough to do yet (ideally with good help and support, and room to make mistakes that they can then learn from and improve!) until they get it right.

So, in terms of design process fixes, a senior engineer running a board review before sending out a design is probably what you need here more than anything else.

If you're talking about an open source (or open-able) personal project design, then there's people on here (including me) that would be happy to look at your design with you and discuss how it could be better before the next rev goes out. you could go in the "projects designs and technical stuff" forum here and start that right now.

Otherwise, if it's a commercially sensitive project, maybe you have senior engineers in your business that need to get more involved in board checking before designs go out, OR if you don't have any, you can hire senior engineers on a short contract just to jump into your project and look at it for you to make suggestions as to how it can be improved, without opening up the design to the whole world... And there's also people on here (including me) who can do that.

[asmi]

There is much more simple solution - just use 4 layer boards. With dedicated power and ground planes, all you need to do is drop a via to connect anything to Vcc/GND. And with prices for 4 layers as they are nowadays, it's not that expensive either (especially if you factor in time spent by engineers debugging boards to figure out why PDN doesn't work quite like what they expected it to).