New and could very well use some feedback ;)

[Anonymous]

Hi all,

I got started using Eagle yesterday designing my very first PCB for a small project I'm playing with.

So far I've added sparkfun libraries, even made a library item for something not in the libraries I had, designed a schema and created a board... Let's call it a productive day 😉

I would really like some feedback on what I've done. Have I done the rights things, or did I make some very standard rookie mistakes?

Is there any way I van add my project here, and if so, which files?

Thank you all!

[jorge_garcia]

Hi daafPKQCW,

I hope you're doing well. You can just upload the .sch and .brd files, it usually works best if you zip up the files. Just reply to this post with files zipped up and other users may then check them out and provide feedback.

Rachael is usually very insightful when discussing PCB design and Cameron is a consumate professional so you'll probably have some very experienced eyes checking out your work.

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

Best Regards,

[Anonymous]

Here we go!

Would love to hear if this makes sense... I've ordered a bunch from Seeed also!

Thanks!

[Anonymous]

1. clean up the schematics, proper hygiene and beauty is vital
2. use lead-in to the pins in layout, keep healthy distance between traces and pins
3. mind your supply layers!!!
4. properly design supply layers
5. decouple your supply layers
6. take care of supply layers layout
7. route control relay (+other power) ground separately, decouple separately
8. route your "grinder" properly, far away from logic traces and shield it with gnd to power gnd
9. always use as thick wires as reasonable and never thinner!
10. keep further away from board edge until you have been in the design for 10 years
11. use 2-layer board to your advantage, at least route power in wide pairs top-bottom to lower inductance, emi, etc.
12. much more of the above
13. use a ddddd... reverse diode on the relays, man!!!
14. did I mention to use a flooded polygon to create power planes already enough?
15. well, use more of that and more, there is never enough ground and supply layers, NEVER

[Anonymous]

[Anonymous]

Additionally, as a noob, keep 6 to 10 milimeter distance between any powerline connections and at LEAST 6 to 10 mm from anything that is powerline mains and the rest of the electronics!

Did I already mention to use capacitors, and losts of them? I did, I mention it again.

[Anonymous]

"or did I make some very standard rookie mistakes?"

...said the rookie soldier, while scraping the ekrazit our of a hand grenade.

Basically, to make a good design, be paranoid, always assume that you will screw up something and that people will die as a result. Houses will burn down. Etc. Imagine the worst to be able to see how it might happen. Even experienced designers do mistakes, and noobs do mistakes at a rate of mistakes_rate^(rookiness_factor)^(ignorance factor+1)

Recently I did a VERY good design, but with a design choice that would be very troublesome, as a result, I have to rework it... 😕

[Anonymous]

Hey ADresden,

Thank you for your comprehensive response! It raises comprehensive questions though.

I think we have established I am Jon Snow. Especially when it comes to electronics. I'm a programmer who happens to start dabbling in this field. When hooking things up to my Arduino on a bread board everything seemed to work. This to sketch a basis where I'm coming from.

---

1. clean up the schematics, proper hygiene and beauty is vital

---

I can fully appreciate this, I like things clean, my code, my house, my schematics... but... uh... what is "unclean" about my current schematics? What is though of as "not proper"

---

2. use lead-in to the pins in layout, keep healthy distance between traces and pins

---

What are lead-in's?

---

3. mind your supply layers!!!
4. properly design supply layers
6. take care of supply layers layout

---

Did I say I'm a complete novice? mind my what?

---

5. decouple your supply layers

---

Uhm... decoupling...? yes.... I would love to do that... what is it?

---

7. route control relay (+other power) ground separately, decouple separately

---

I'm beginning to sound like an imbecil  here... but, what exactly does this mean?

---

8. route your "grinder" properly, far away from logic traces and shield it with gnd to power gnd

---

Hey! I get the first part of this one! but, what is "shielding it with gnd to power gnd"

---

9. always use as thick wires as reasonable and never thinner!

---

This I do get.. I already went 5x thicker than the default setting was... How do I know what is the right thickness? There is no real power running through this board anywhere.. It's all 5V components that draw next to nothing (as far as I can tell). Even the relays do not switch higher voltage, they just simulate a switch in the "grinder" that is in a 5v circuit itself.

---

10. keep further away from board edge until you have been in the design for 10 years

---

Haha.. ok, I guess I like living on the edge sometimes... Why though, and what changes after 10 years?

---

11. use 2-layer board to your advantage, at least route power in wide pairs top-bottom to lower inductance, emi, etc.

---

Could you elaborate on this? (that is a less dumb sounding way of asking you to explain).

---

13. use a ddddd... reverse diode on the relays, man!!!

---

What? why?

---

14. did I mention to use a flooded polygon to create power planes already enough?

---

No, you did not... see my response to #11...

---

Additionally, as a noob, keep 6 to 10 milimeter distance between any powerline connections and at LEAST 6 to 10 mm from anything that is powerline mains and the rest of the electronics!

---

When you say powerline, you mean 110v-230v AC? or are you talking about the basic 5v DC lines on the board as well?

---

Did I already mention to use capacitors, and losts of them? I did, I mention it again.

---

 Nope, don't think you did.. But I hear ya'... where, why and what type do you suggest...?

I would very much prevent houses from burning down (there might be a few very ugly exceptions...), since all these components are 5v linked to arduino board... how big would you asses the risk?

Thank you again!

Daaf

[Anonymous]

Read the other posts as well, but basically, once you have read the terms I mentioned above, they burn into your brain and once you see someone else talking about it, displaying it, showing it in an example, reading it in a datasheet, you will know what to look for!

There is too much to be explained, but I gave you what you are looking for first and foremost.

The only thing that is mostly mine: the "lead-in"; imagine if the thickness of the wires you have there suddenly increased, how many shorts would you have? Lead the traces in a manner that you make one 45-degree turn and later another 45-degree turn.

Like in the old film "karate kid", you will wonder "why am I doing this, why do I have to do this?"| You will see at the right time. With the proper routing technique, as you will see dirt and oxides accumulate, you will notice that the isolating distance has been kept the best it could be. You never know what happens.

Anyway, long world of reading is before you, days and months, but the things above are the best starting point.

((The picture of your edited schematics is below, how did you not see it?!))

[jorge_garcia]

Hi @Anonymous,

I hope you're doing well. Thank you for posting your design for scrutiny. You've done a great job for it being your first board, however there are a few small things you can do to make it better. Most of this is inline with @Anonymous 's comments but I'm going to try to simplify it and focus and what you need to do for this board. 

Schematic

1. In the same way that you used GND symbols to define your GND net, you can use a +5V symbol to define the power rail. In this way you can avoid a long net that's hard to follow going to every part just to feed power. You can find this symbol in the supply1 library that comes with EAGLE. This is probably the biggest critique of the design.

2. You should stick to just 90 degree bends in the schematic, it's not a hard-fast rule but it's good practice and it helps when reading the schematic. Check the connections to your Loadcell for an example of what to fix.

3. You are running nets through the inside boundary of the loadcell and the Arduino. Again, not a hard fast rule but you don't want to have nets running through the middle of the symbol because again it affects readibility. In the case of the load cell if you right-click on it and select mirror you will find that it looks much better because the nets won't run through the middle.

4. Make sure to put diodes with the anodes connected to ground and their cathodes connected to the input of the relay coil. These will avoid a large voltage spike when you turn of the relays that can blow your arduino.

5. Decoupling, is the process of the adding capacitance (Usually 0.1uF or so) near the voltage pins of active components to help keep the power supply clean and free of transients. In this case you are using off the shelf parts that already contain decoupling capacitors so not strictly necessary here but it's good to form the habit.

Board

1. You can improve the noise performance of the circuit and it's reliability by using the POLYGON command to create a ground pour (a large plane of copper) on the bottom layer. This allows for the best path for current to return to the source, avoiding impedance changes which can add noise in the form of signal distortion. Additionally the plane can serve as a shield from EMI and other noise sources.

You have done a good job. I fully expect the board to work and I hope you continue on this exciting adventure of PCB design.

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

Best Regards,

[Anonymous]

There is a "polygon" icon in Eagle, learn to use it. you can draw in layer 1 or 16, for example. Wow, it has some options, you will say. Then you will discover that you can rename the polygon to say VCC or GND. Thus, creating one on top, say VCC and on bottom GND, you have created a proper power supply planes with the lowest inductance.

That is the answer to the #14

[Anonymous]

Hi ​Jorge, Hi ADresden,

Thank you both for your continuing help!

I've gone and changed what I understood. I've cleanup my schematic (straight angles, no more crossing through parts, added 5V) and on the board I've added the ground pours (looks more like a pcb the way I expected it this way!).

Questions:

- For now I've added a ground pour on the top and bottom layer, both GND, connected with VIA's in several places (came across that as good practice in a tutorial). Is it better to do GND ground pours on both sides or to do a GND and 5V or is there no real best way here and does it depend on your design?

- I'm going to completely redesign the board (made the very basic mistake of not checking the available space where it needs to go...). I'd like to add the diodes to my design but do not completely understand how to place them or what type to get.

When I google the most common type of setup seems to be like in this picture:

Is that the correct way to go? and if so, which diodes should I choose?

- The decoupling using capacitors sounds like a step that should be part of every design, right? where in my design should I put them?

Added my updated version!

[Anonymous]

Whoops.. I see I forgot to name my VIA's GND. 😉

[jorge_garcia]

Hi @Anonymous,

I hope you're doing well. I'm happy you figured out that you need to name the vias to connect to ground. It's OK to have GNDs on both sides it offers additional shielding and noise immunity. It is also OK to have a 5V plane and GND plane. I usually try to have a 5V and a GND plane since that makes routing your power more convenient.

The relay circuit you found is the textbook circuit, so that is the one you should use. Depending on how much current it takes for the relay to latch you may have to beef up the diode. For most applications that 1N4007 or the 1N4148 can do the job.

P.S The folder you zipped up doesn't include your schematic. It includes a different project's schematic.

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

Best Regards,

[Anonymous]

diodes conduct current only in one direction, guess what a wrong connection does.
there is a reason for calling it "antiparalell diode"

the correct diode type is "some"

pours: depends. using vcc+gnd, you create a capacitor able to supply current at ultra high frequencies. which is the purpose of the blocking capacitor (see, I'm using the terms loosely, like a pro 😛 )

So, you place the capacitors usually near power entry and exit. Near the pins, that is. This is done for EMI and functionality (ever had a PC reset of freeze itself, which was solved after you replaced the PSU for a new one? Dry capacitors. I think this explanation shall help)

[Anonymous]

Thank you both for your help again! I'm learning a lot 😉

I did I massive redesign (or so it felt at least). I have limited space in the housing so had to get creative. I had to put some components on both sides, but I guess there is no reason why I couldn't do that, right?

    

(ecad.io makes these great 3d images!) the red block is a part unknown to their system, actually a ready made pcb by sparkfun, the blue blocks are the relays

I think I managed to do a reasonable job. I've added the diodes, as close to the relays as possible. Is my placement correct?

Just some more in those capacitors...

---

@Anonymous wrote:

So, you place the capacitors usually near power entry and exit. Near the pins, that is.

---

- We speak in plural here capacitors, do I need more than one in my case?
- placement near the power entry and exit, just place them parallel, connected to the power supply pins? is there a small drawing somewhere of what the correct placement would be (schematically)?

I hope I got the files right in the zip file this time...

[Anonymous]

sorry, not much time for your file (none), just notes:
I prefer the diodes lying down, not standing, you won't be able to solder those anyway 😄
, also, the diodes can be small, even small signal schottky diodes.

well, the diode is just "any"

The capacitors. Have a look at your mainboard or other piece of well made equipment for inspiration. IBM original equipment for megalomanic interpretation.

I have no doubt it would work without those capacitors, but learn it in this "demo" beforeyou start using parts which would simply not work without it.

And... start disassembling things around. EVERYTHING. One by one.

[Anonymous]

That reminds me: you could just have used one of those "glassy" diodes, and solder it directly over the relay pins. (after soldering in the relay)

That teaches you another thing: leaving enough space around certain pins, so you can do manual soldering for development and not do any short to the ground or other poured plane.

[jorge_garcia]

Hi @Anonymous,

You did a great job! It's OK to place parts on both sides of the board and this is done quite often. As far as the coupling capacitors go for this design you can get away with one at each active component, however for high-speed or high-power designs @Anonymous is correct you might need multiple capacitors in parallel.

The placement of the diodes looks pretty good, but I'm sure you would rather lay them flat.

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

Best Regards,

[Anonymous]

Hey there!

I completely agree, the diodes should be lying down... just couldn't find a 3d option for that in ecad 😉 in the actual solderd version they will be flush against the pcb!

---

@jorge.garcia wrote:

As far as the coupling capacitors go for this design you can get away with one at each active component

---

What are considered 'active parts'? and, if I would feel I would want to add them to this pcb exactly where and how would you advise placing it / them?

sorry, I am a real noob when it comes to these things...