0
\$\begingroup\$

I was in the middle of soldering a PCB I designed when I realized I forgot to decouple the RFM69HCW module with 0.1uF. Does anyone have any insight to how damaging this is, and if I need to redesign and redo my board? I'd prefer to not have to spend the time and money if I don't have to. The 3.3V is being supplied from the external circuit of a TPS563200 (step-down converter) on a 0.3mm trace, 15mm in length. The board is grounded by a ground plane, though the connection to the plane is rather far away as it passes through 5 smt components before connecting to a grounded TH component. Is this okay for me to move forward or should I redesign my board?

enter image description here enter image description here enter image description here enter image description here

\$\endgroup\$
8
  • 1
    \$\begingroup\$ Damaging, unlikely. As the datasheet says, the supply pins of the module should be connected to ensure correct operation. Is this a one-off hobby project or a professional job project with multi-million production run for customers and consumers? Maybe post schematics and PCB layout to get a better answer. \$\endgroup\$
    – Justme
    Jun 20, 2023 at 6:18
  • \$\begingroup\$ Edited to add my schematic and design. The issue I have is that I know buck converters are super noisy compared to linear regulators, but after all of the external circuitry that you add in accordance to the datasheet, I don't know how noisy they are exactly and if it's that significant. I'd prefer that they didn't have a ton of restarts, like no more than a couple instantaneous spikes per day, partially because it's not a huge major project but it is one I'm giving to someone and won't be seeing again. \$\endgroup\$
    – 1W0n_29
    Jun 20, 2023 at 13:55
  • \$\begingroup\$ Please take a higher resolution screenshot -- the schematic is unreadable. \$\endgroup\$ Jun 20, 2023 at 13:56
  • 1
    \$\begingroup\$ Is it necessary to do a new board? Just solder on 100nF ceramic caps, SMD or with leads, to places where they are missing? The LVC245 has floating inputs so it may cause problems. Also I don't see how the SPI bus can ever work as MOSI and MISO are both converted to same direction, and also the AVR running at 5V does not have to understand 3.3V logic levels. \$\endgroup\$
    – Justme
    Jun 20, 2023 at 14:17
  • 1
    \$\begingroup\$ @1W0n_29 It is bidirectional, but only to one direction at a time, so you can't use it like that. And I checked that specific AVR model (if correct) will see 3.0V as logic high, but some need higher than 3.3V so with another AVR model it may fail unless you level shift it back to 5V. There are also other errors (regulator feedbacks) that make it not work, and would it be simpler to just use 3V3 for the whole thing. \$\endgroup\$
    – Justme
    Jun 21, 2023 at 10:41

2 Answers 2

2
\$\begingroup\$

Try it out to see whether it works or not before doing a redesign. You cannot damage anything just because of a missing decoupling capacitor.

EDIT due to comment: The above sentence assumes, that your power supply is properly designed and stable.

The worst thing that could happen, is that the module could show weird unreproducible behaviour from time to time due to undervoltage resets.

However, I think your design will work either way since the module you're talking about has decoupling caps on board.

Edit after posting schematic and layout:
By reading the comments of your original post, I can see that you will do a redesign anyway due to a badly selected level shifter.

I see a couple of improvements that you can do on your layout:
1.) Grouping: Try to give your layout more structure by grouping together what belongs together. Make physical sections to separate the power supplies, the microcontroller stuff and the RF transciever. You can then route each section individually and your board will probably look tidier. Try to separate the DC-Converers, the Clock and the RF transciever.

2.) Decoupling capacitors and grounding: Connect all your capacitors directly to the ground plane on the bottom layer through a via. Each capacitor (and each ground Pin of each IC) should have it's own ground via. Try to make the bottom layer a ground-only plane and avoid routing of other signals there.enter image description here See this article for the image source and more information.

3.) Power supply: All DC converter IC's have strict layout guidelines that should be followed in order to lower the switching noise on the output. A recommended PCB layout is typically shown in the datasheet. Stick to it. Additionally, I can suggest you to read this article about DC/DC converter noise filtering. It is also important to use the correct parts (Inductor + Capacitor) for output filtering. Also here, the datasheet typically provides formulas for calculating their sizes and sometimes also part numbers. If you are unsure, you can also use freely available (but often vendor specific) simulation tools such as the WEBENCH power designer from TI. The simulator will give you information about the expected output noise and will also suggest the filtering component sizes and part numbers.

\$\endgroup\$
3
  • \$\begingroup\$ I wouldn't say "cannot". I've seen switching regulators blown from the cap being 2cm away. Which, with the poor layout and routing here, might actually be relevant? Hard to say. \$\endgroup\$ Jun 20, 2023 at 13:55
  • 1
    \$\begingroup\$ The design won't anyway work due to othet issues. \$\endgroup\$
    – Justme
    Jun 21, 2023 at 7:30
  • \$\begingroup\$ @TimWilliams Yeah "cannot" is a hard word here :) But I guess in your scenario, the problem is more due to an unstable power supply and not really the presence/absence of a 100nF decoupling capacitor on some IC. Anyway, I added a sidenote in my post. Thank you :) \$\endgroup\$
    – Mau5
    Jun 21, 2023 at 23:58
1
\$\begingroup\$

It seems to be necessary to do a new board anyway if you want to fix any errors.

Otherwise you could just solder on extra bypass caps and hack the board to work.

For example the regulator feedback pins are incorrectly connected, the MCU can't communicate SPI via level shifter, the level shifter has unused pins left disconnected, and the 3V3 data pin is not shifted up to 5V level for the MCU. Usually 5V MCUs cannot work with 3.3V input levels. This is not an exhaustive list and there may still be serious or less serious errors.

\$\endgroup\$

Your Answer

By clicking “Post Your Answer”, you agree to our terms of service and acknowledge you have read our privacy policy.

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