0
\$\begingroup\$

I designed a schematic with quite a lot of connections (88 comparators into 14 MUXes) I created ground planes on the top and bottom layers to assist with the many ground connections. I just got the PCBs from pcbway.com and I tested the ground and power connections using continuity mode on my multimeter. What I found is that the ground pins and vias with point to point connections visible on the top layer are all connected, but the ones that should have connected to the ground planes on the bottom or top layers are not connected to any other ground pin on the board. So my question is, did I do something wrong when I built the PCB design in eagle? What can I do differently to have some assurance that the board will print correctly next time? I have included links to download the schematic and the board files below.

Schematic - Eagle

Schematic - PDF

Board - Eagle

Board - PDF

\$\endgroup\$
7
  • 4
    \$\begingroup\$ Please also post your schematic and layout in an image format for those of us that don't have eagle. Did you double check the net connectivity in software, and did you follow the minimum clearance and trace width requirements of the manufacturer? I don't know about eagle but in most software you can check these things automatically. You can't see between the outer layers unfortunately, but under a microscope do you see any manufacturing issues on the top or bottom? \$\endgroup\$ – Drew Jul 7 '20 at 2:25
  • \$\begingroup\$ I added the PDF versions, but on closer inspection I did realize that I didn't follow the min width restrictions of the manufacturer. I suspect that is where I went wrong. \$\endgroup\$ – richbai90 Jul 7 '20 at 3:22
  • 3
    \$\begingroup\$ Your ground pours are all chopped up by traces -- you must have ignored a bunch of DRC errors. \$\endgroup\$ – Dave Tweed Jul 7 '20 at 4:52
  • 1
    \$\begingroup\$ I don't use Eagle but I can see a lot of rubber band lines (unrouted traces) in the PDF. As Dave says, this should have generated a plethora of DRC errors. Nothing to do with the trace widths (though you should obey those rules). \$\endgroup\$ – Spehro Pefhany Jul 7 '20 at 5:14
  • 2
    \$\begingroup\$ An autorouter is not for laying out a simple board, it's for automating small parts of a very complex board to make it tractable. Do some small completely manual layouts first, to understand what the tool does. Check every DRC violation the tool throws at you. Some will be real problems on the board, some will be places where you've mis-specified what you wanted to the tool, but you need to understand which is which. \$\endgroup\$ – Neil_UK Jul 7 '20 at 7:14
4
\$\begingroup\$

Your board layout shows multiple unrouted nets (the yellow lines). You need to route them, otherwise your board is not a representation of your schematic.

Eagle has a feature to tell you whether you have unconnected traces. Use that! (DRC)

Generally, this system is a bit strange: you're designing a PCB, which is logical, because you want to place and connect components. Then, instead of using the components you can buy, you opt to use these Sparkfun modules that are meant for people with breadboard/veroboard instead of their own PCB design. You can save a lot of space (and money) by not doing that! Simply use the single component that's on a Sparkfun SPARKFUN-AD-MUX-16X1: that's a CD74HC4067, and it costs cents a piece, and can essentially bought at any credible electronics parts distributor (Mouser, Farnell/element14, Arrow, digikey,rs components).

Also, you've got a metric hellton of LM311 comparators. Which is fine - but there's also chips where there's multiple comparators in a single package, and that makes your job soldering things much, much easier. Also, you've forgotten to add decoupling caps to the comparators. That's a bit of a bad idea. Also, it's not very clear what purpose these comparators serve, but I trust you know what you're doing there.

What completely doesn't work is your method to generate 5V. You need a regulator. A voltage divider cannot work.

I think you need to go back to your schematic design phase and re-evaluate your component choices. Then, you need to come up with a proper way of power your board.

(also, your trace layout is pretty bad - not blaming you, if this is an autorouter result. Also, wouldn't even blame you if it wasn't: The first revision of any board I layout, I basically rip up all connections after I'm done connecting everything, and do it again, but smarter based on the things I've figured out while routing things. For example, if you're looking at your schematic, it would probably make much sense to put your comparators close to where the signals that feed into them come from, instead of all in one heap, or close to where the signals coming out of them go to.)

\$\endgroup\$
2
  • \$\begingroup\$ Thank you for the advice and feedback. As I’m sure is apparent, I’m very new to this. I’m a 3rd year Computer engineering student who just finished their first linear circuits course. I’m doing this as a hobby/learning project so the advice is welcome. \$\endgroup\$ – richbai90 Jul 8 '20 at 3:29
  • 1
    \$\begingroup\$ @richbai90 you're more than welcome! \$\endgroup\$ – Marcus Müller Jul 8 '20 at 6:53

Your Answer

By clicking “Post Your Answer”, you agree to our terms of service, privacy policy and cookie policy

Not the answer you're looking for? Browse other questions tagged or ask your own question.