Thanks, I will, this was a quick setup to show my question.
Good catch! That wire is not attached to the +ve side of the capacitor. Check out ERC checks to help you catch unconnected pins! (From the Inspect->Electrical Rules Checker menu item).
Almost good, and that is why I added often in my previous post. 
If you look at the ratsnest lines, you see that both terminals of C1 are part of the netlist.
In this particular case the attachment point of the pin is actually in the junction dot. If the pin was not connected you would see a round circle at the attachment point of the pin.
Another small tip:
PCB Editor / Preferences / Preferences / PCB Editor / Editing Options / Ratsnest [x] Show ratsnest with curved lines makes the ratsnest clearer on a crowded PCB. Increasing it’s line thickness is sometimes also beneficial.
Thankyou for the tip, I stumbled across the curved lines today. The ERC check did not catch the unconnected capacitor though!
Ah, it’s because (related to Paul’s comment) the unconnected element is a wire segment. We should probably catch unconnected wire stubs in ERC.
New ERC check added; will be in v9 (or nightlies if you’re brave):
The rest seems to have been solved, but I question your power connections (bottom left in your schematic).
First, attaching a power symbol to a connector in that way is… exotic.
Second, is -12 V really the same as GND? You need to make up your mind (it could be correct, but is unusual).
If you zoom in, those power symbols are indeed not connected. (This isn’t a bug).
Don’t do that.
Schematics are supposed to be clear and self-explanatory. Doing something “clever” is rarely a good idea.
I’m also not so sure whether an arduino nano would survive 12V (or even 24V if you use the +/-12V on the connector).
Maybe it’s one of those newbie misconceptions, if the positive terminal is +12V, well then the negative terminal must be -12V, yeah?
12V is within range of the Nano’s power supply input. 24V is “right out!” as Monty Python puts it.
Without a doubt a newbie misconception. I have more coding skills than electronics and schematics.
Is this correct ?
One tip for clear readable schematics: voltages drop from top to bottom, so your +12V symbols should point up and be above the ground symbols. Second: signal flow is from left to right. So inputs are pointing to the left and outputs to the right. These are no fixed rules and not the best choice in every case, but you see it very often and it helps to grab the essenced of a design in a moment.
Besides that, if you use the diode as reverse current protection you should put a fuse or a resistor between the input and the diode, otherwise it is possible that the diode breaks as open and you still have the reverse voltage across you circuit and (probably) everything else still goes up in flames.
Rotate you power input so that the pins are facing left and +12V pointing up and GND down and everybody will instantly know what’s happening
1 Like
Also I’d rotate C1 and D1 so that they’re vertical next to each other (with the GND connections pointing down of course). Makes it clearer that they’re for smoothing and clamping the voltage.
I would draw the power section like this:
- It keeps to the convention of signals (power) flowing from left to right.
- It follows the convention of voltages going from top to bottom.
- It keeps the symbols non rotated.
- It puts the power conditioning right at the input connector, so you see quickly how it works.
- I put the power flags right on top of the power symbols. I am not sure yet if I keep doing that, but it sure does save some space.
- Note: I put the +12V power symbol on the other side of the fuse.
- Now you can use the +12V power symbol to directly connect to your arduino (and on other locations). In your circuit, Z1 and Z2 also connect to +12V, but they are not protected against reverse voltage by the fuse / diode combination. Mistake or intentional?
- Because all power conditioning stuff is now a small block, it’s easy to move to a convenient place later when your schematic gets more crowded.
Nice, thank you so much for time and help. My plan was to add capacitors to each of the stepper motor drivers (Z1 & Z2) too. Don’t know if it’s needed though. Other boards use it like so.
By drawing the power section like you did, will using the +12V symbol (and net) anywhere on the schematic now give me the benefit of the fuse, diode and capacitor, am I right ?
My plan is though to step down 12V to 7.2V and 5V for use my PCB. The 5V will be powering the nano and 7.2 will power a camera.
Yes. You can also additionally use net labels (hotkey L) to mark special nets. For example the wire between your input connector and the fuse could be labled “+12V_INPUT” or something like this. If you open the schematics setup dialog (right beside the “save” symbol") you can also assign netclasses, like “power”, “high speed”, “LED” or whatever you like. If you assign colors to those net classes you also have an instant impression what type of nets are where on your schematics. Can help greatly with bigger designs, you at you own discretion. Might be looking something like this:
Edit: For the caps on the stepper drivers: follow the instructions in the data sheet or the/a reference design until you are definitely sure you know, what you are doing.
The Nano already has a linear regulator from Vin to its 5V rail so you could power it from 12V, or the 7.2V rail if you prefer to transfer the dissipation to the 12V – 7.2V regulator.