Make sure its the same device reference, I edited my post above to make them both part of device U4
1 Like
Worked like a charm, thanks for the help!
1 Like
Sorry for yet another question but I wanted to know what are the risks of not making a ground plane. Indeed, here’s how the PCB looks for the moment : (I’m new so I reckon many things aren’t optimised so I am opened to any suggestions/modifications)
As you can see, I tried to put as many wires as I could on the front copper (so the red part) to keep the back copper (the blue part) for the ground plane but there is too much of it to do one right ? Or I have to cut it around the blue wires ?
I think I have 3 options :
- I make another layer of copper and pay more and wait more; but everything’s clean
- I don’t make a ground plane at all, and just add wires to the GND pins on my Arduino
- I cut the ground plane around the blue wires I have
That is very application dependant and without knowing many details of the circuit it’s very hard to say what the risk might be. For example, is this a commercial product that will need to go through EMC testing to achieve CE marking ?
Even ignoring EMC for a moment, a GND plane makes it easy for all your return current to get back to GND.
Why not just add one and see how it looks ? then optimise any traces on the same layer that are interrupting it too much. Just make a rectangle using the Filled Zone tool that covers the entire PCB, make sure it’s set for the GND net and hit B to re-fill.
2 Likes
For THT elements more typical (for me) was to have as many as possible signal wires at bottom.
Until you don’t want to pass tests in EMC lab risk is close to 0.
There is some risk because modern ICs like to be fast (have fast slopes) even they don’t have to. It is because to manufacture them as cheep as possible the smallest and smallest technologies are used. The smaller technology the smaller capacitance between wires and faster slopes. Fast slope makes taking very short, high current power pulse. That pulse traveling through GND track generates voltage drop at it and not track R is the most important factor but track L. The effect are differences between GND potential of several ICS what can have the important influence or not depending on ICs functions and so on.
2 Likes
Wanted to write the same but you were faster 
2 Likes
Even a shitty ground plane that’s interrupted by tracks is usually better than none, or at least not worse. And the copper at least improves PCB robustness and lowers resistance to ground.
You might want to make the traces thicker for more robustness and less resistance. There’s a lot of room on your PCB as you’re using relatively large THT components.
2 Likes
larger traces means less resistance ? I thought it worked the other way round
I’m using 0,25mm traces which is already quite large considering I will never exceed 30mA but I’m going to have a look, you’re right I have a bit of space so I could be using it
Larger traces is the same as thicker wire.
Think about fuses, or check out the Kicad calculator on the front page. 
1 Like
Have a play with the Calculator Tools . . .
Example 100mm long track, 1oz copper thickness, 0.25mm wide . . .
now 0.5mm wide . . .
1 Like
Unless he edited it in the mean time, thinner is less resistance.
Wider tracks also mean more capacitance, which most often a bad thing. 0.25mm wide tracks is wide enough for easy manufacturing for most PCB manufacturers, and it is good for up to about 200mA, so it’s plenty for all logic signals. Only for power tracks wider tracks have an advantage because it lowers the resistance and voltage drop. I think a bit of resistance is even good for logic level signals, as it dampens oscillations, but it’s probably negligible on a PCB scale.
Your GND plane is atrocious though. And from the way I understand it (contrary to what Jonathan_Haas wrote) a poorly designed GND plane can be detrimental to the design. Area’s of copper that are only connected on one side can act as antenna’s to both pick up and radiate noise, and you can have standing waves in such area’s.
A proper GND plane is a quite important part of a PCB, especially in these modern times with ever higher speed logic (I’ts the flank steepness, not the signalling frequency that counts). A properly designed GND plane is continuous over the whole PCB (except for designed in exceptions such as real antenna’s and isolation barriers and such) In a proper GND plane there should not be a single interruption that is bigger then about 3 to 5mm. That means modifications such as only using short hops to get under other tracks, making the standard clearance smaller so the GND plane sneaks in between the pads of your THT headers and IC’s, and also avoiding groups of via’s that can create bigger holes.
1 Like
I don’t understand who’s right and who’s wrong now haha
It’s true that with the calculators, thicker traces leads to lower resistance…
I know my GND place is atrocious and that’s why I shared it but I feel like I don’t have the experience to make a better one. It’s the first circuit I make with so many wires everywhere…
The speed logic isn’t going to be very important here as I’m not trying to retrieve any data from the SD card. I am only measuring the resistance between every pin (with a voltage divider) and plotting the voltage-current characteristic of each pin relatively to the ground. It’s only like less than 15 measures per second so no high speed logic or anything (everything works analogically except the command of my MUXs).
So your main recommandation would be to try and make the holes in my GND plane smaller, even if it leads to more of them ?
physics 101, resistance of a wire (near DC): R = ρ (L / A) with A being the cross section. So bigger cross section = less resistance, with cross section being a (linear) function of the width of the wire → wider wire = less resistance.
first thing you could do is adding “bridges” for GND everywhere you have long divided sections. also try to minimize the routing on the bottom layer by using it only for jumping over some conflicting wires, not for long tracks like you have it right now. I assume you don’t want to manufacture the PCB yourself so adding more vias is nothing you should be afraid of.
1 Like
Was just about to add something similar, instead I’ll just add this for further reference: How to Calculate Resistance Using Resistivity | Physics | Study.com
1 Like
I can confirm. It is valid recommendation always.
But in amateur designs may not be taken very seriously.
I used to design my 2 layer PCBs with all bottom being GND with no breaks at all.
Here is an example of such PCB:
Blue is everywhere except one 3 pin THT connector.
All vias are GND.
That is definitely a big resounding YES with dominating GOD voice and double echo’s. Big holes hurt the integrity of your GND plane, and the smaller each hole is the better. The total number of holes hardly matter at all.
To underline the importance of a good GND plane you can watch the video below from Rick Hartley. He made an over two hour long presentation of the importance of the GND plane combined with background explanations and design suggestions. All two hours are worth watching, and this again emphasis the importance of a GND plane.
As long as you are working at a hobby level and with relatively slow microcontrollers (it’s the signal flank steepness, not the switching frequency) then you can still hump a long with impaired grounding, but as you go into more faster digital IC’s, sensitive analog stuff and also have to comply with EMC regulations, then a good GND plane becomes essential to your PCB.
2 Likes
I knew that formula but messed it up in my head between the section S and the length.
Thanks for the other tips!
Thanks for all the tips everybody, I will improve the PCB with your recommendations when I have the time. Then I’ll post the GND place again to see if there are any improvements.
Thanks again:))
1 Like
I’m sure I echo everyone’s thoughts when I say . . . You are Welcome
Try and watch some of the video above, I stole some time at work today and watched 90% of it, it will help you loads with GND and Power planes and good practice in relation to signal tracks.
1 Like