You can do either way. But the primary reason doing it with symbols is that you can keep the design coherent to the reader.
Drawing everything separately allows you to structure the design in a similar kind of way as you structure text. This makes it easier for others and yourself later to follow the train of thought. Since its structured by functionality, in separate sentences and paragraphs so to speak. The benefit of the lines at all places is it mimics how its being done in reality better.
But the application is actually meant to overcome this. This is why its split into 2 parts doing the design and then layout. So you don’t actually need to concern yourself with the layout in the schematic stage and you can concentrate on making things as readable as possible. Which helps when you move away from simple designs. Not that all connected lines can not be readable, but a lot of lines crossing can be confusing and takes more time to draw well.
I do use the lines strategy sometimes when I need to work with very beginners so that they can breadboard the design easier for testing. Also lines strategy is better if you intend to actually make a IC design, but off course kicad is not designed for this.
One thing I don’t think anyone has mentioned yet . . . are you running KiCad, loading your project and then launching the Schematic Editor and PCB Editor from there ? or are you running them stand alone ? if you run them from outside the project they won’t be linked so you won’t get the benefit of the Netlist.
Last time I was doing it was 2017.
Are you still using KiCad 4.0.7?
Since V5 you have direct connection between schematic and PCB and need not go through netlist.
At PCB you just click “Update PCB from schematic” icon in toolbox.
Double click is faster than selecting anything from Context Menu.
Fridge_Alarm.kicad_sch (67.6 KB)
This is the schematic for a project I’m working on. I didn’t do a breadboard for fhis my first step was the schematic then I created the PCB design and then I started breadboarding. I’m calling it Fridge Alarm. We have a second fridge in the kitchen that has a stubborn door. Many a morning we’ve woken up to find the door had been partially open all night long and most stuff on the top shelf are garbage. The fridge alarm will monitor temperature and light and sound an alarm if either the light is on for too long or the temperature rises too high. Since I did this schematic I’ve learned that I might not need the transistor on the buzzer.
Hope I did this right.
Both GNDs ought to be connected together but they are not. It’s unclear if they are connected internally on the devkit but why take the chance? Thus you only need one GND PWR_FLAG.
You can rotate and mirror the DS18B20 symbol to make the wires from it neater. Similarly you can mirror the ESP32 module so that sensor inputs are on the left, and buzzer output is on the right.
Nice drawing.
Pin 23 needs fixing.
I’d connect pins 2 & 23 with a wire so they are on the same net.
I prefer reading L to R, so, if it was my drawing, I’d place the power in on the Left with the Gnd connection on the bottom and I’d rotate and mirror U2 so pin 2 faced U1 and U2 Gnd was under U2 VDD. That way Gnd was at the bottom of the drawing and V+ is at the top of the drawing.
Note: I write, “I prefer”. You may not agree.
If the Gnds are connected internally, how much current is available through that connection? Will the buzzer kill that U1 internal connection, especially if that buzzer fails sometime in the future?
Same with
Using the transistor with R2 will ensure the current for the buzzer doesn’t kill U1.
Fridge_Alarm.kicad_pcb (85.8 KB)
Here is the finished PCB but looking at the schematic again I believe I may have the barrel jack in wrong. I think it needs to be mirrored.
Thanks for all the suggestions.
Don’t be afraid to increase the width of your tracks. You’ve paid for the copper so you might as well use some. The wider the tracks , the more physically robust they are.
Where will this board live?
Will the sensors need to be remotely located? ie. in the fridge?
Will the sensors need connectors to join to the PCB?
If you need connectors, will they fit into the PCB footprints on the board?
For me much more usable are screen shots as I can see them.
At home I am writing from Win7 PC and KiCad needs Win10+ so I can’t see KiCad files.
At work I have KiCad V8 at Win10 PC, but this ‘working PC’ I have disconnected from net, and connected to net I have second PC, but Win7 (I’m not used to throw away still working electronics). So to see KiCad file I have to move it with pendrive to second PC.
Reed switch + magnet installed at door + time delay circuit can’t be used?
Capital “K” is for Kelvin, 1000x multiplier is lower case k for kilo.
It’s unusual to use the “Ohm” character, or units for resistors. I would not even know how to type that. I’d just enter 10k and 4k7 resistors. This notation is known as RKM_code
jmk put all copper tracks on one layer, now put a GND zone on the other layer.
TO-92 with the close pin spacing is a bit of a nuisance. KiCad has some footprints in which the pins are spread about a bit (either in line or in a triangle). That’s easier to solder.
Vertical resistors are wobbly and prone to bending. Using horizontal resistors is more common, and they look neater.
Learn to use net classes. 0.25mm is fine for digital signal tracks (Especially on the top, where the height of all the other parts protect the PCB from damage. Solder mask is pretty robust also). But for power track it’s better to use wider tracks (assigned by netclass). This also helps with recognizing nets while you route them.
Always add some capacitors to your circuits. 100nF ceramics to IC packages (In this case meh, the ESP32 should already have them), but also add a bulk electrolytic capacitor (something like 10uF) to decouple from the power input cable.
Add mounting holes. It’s normal to add these to the schematic and assign footprints, just like all other parts. KiCad has built in libraries for those.
Add project name, date, (KiCad) Logo. This helps with finding your documentation if you want to change something many years later, and it’s always good to spread “Made with KiCad” logo’s (It’s in KiCad’s default libraries).
Connectors are always troublesome. Even if the plug size of the barrel jack is the same (Often 2.1mm / 5.5mm, but 2.5mm / 5.5mm also exists) the footprints on the PCB are not standardized. There are often differences in pad locations between different brands.
Those big LDR’s are made of Cadmium Sulphide, and not RoHS compliant, and this makes them difficult to source. But there are easy and cheap replacements, for example: BF5A04GA
Also, for a project as simple as this, I would not order a PCB but just solder it together no matrix board. I would draw both the schematic (as documentation) and the PCB layout (to see if it all fits) but just solder some wires after that. Matrix board is not good enough to pass EMC tests, but you don’t have the equipment to test that anyway
Also do you have a power supply with barrel jack output that puts out regulated 5V required by the ESP32 module? Most of the wall warts I’m aware of have USB outputs not barrel jack outputs. Maybe you should design for power from a Micro USB or USB-C connector. I wrote up on those power connectors here: Instead of a barrel connector try... | Ken Yap | Hackaday.io
