Thanks for the advice. I wanted to do filled GND and POW but I don’t know how to do it. 
For me, this is the first time when I “design” a PCB… so, one step after another. For sure this will be v.1 and when I get more experience there will be some improved versions.
P.S.: The “weird looking stuff” are the only possible routes for those circuits. Maybe beacause I did’t find the perfect order for them and some off them had to go around other to make the connection.
First, select the “Add Filled Zones” tool on the right side of the window:
Then click where you want one of the corners of the zone to be. After you click, it will open this dialog:
Select the layer you want the zone on (which defaults to the current layer), and then choose the net (such as GND, for example). You can probably leave all the other settings at the default. Then click “OK”.
After you click “OK”, it will let you draw the outline of the zone. I would recommend drawing the zone a comfortable distance outside the board outline. (Only the area inside the zone AND inside the board outline will be filled.)
When you run DRC, I would recommend checking the “Refill all zones before performing DRC” checkbox, to make sure the zones are up-to-date.
If you want to refill the zones manually, without running DRC, just make sure the “Add Filled Zones” tool is selected, and then right-click anywhere on the PCB view. Choose the “Zones” sub-menu, and then “Fill All”.
1 Like
As of 20211126 there is a PCB file there.
I cloned the repository.
I am running 5.1.10 and when open the project I find that I can open the schematic.
However when I try to open the pcb I get an error message to th effect that my version of KiCAD is older than the version with with the pcb was made.
IIRC there is some kind of daily build version but I have stayed with the current stable. I will check for more recent stable. IIRC there is also a Version 6 in the works. Perhaps it is out…
FYI,
I have updated my KiCad to 5.5.12 but still, cannot open the pcb file.
Anyone else with perhaps the 5.11 or what ever the nightly is called open it and perhaps share a screen shot?
Look at your PCB carefully - you should find many things that could be done better.
For example:
It will be better to connect R4 and R5 GND pins directly at green layer after moving the green wire going between them to the left of R4 GND pin.
The key is to place elements the way to simplify connections that are to be done.
I have 5.1.12 and I’m getting the same error as @ForrestErickson. Are you sure you’re opening the PCB from the GitHub repository?
The screenshot you posted looks like the one that @Cosmin and I have been working on in this thread.
Didn’t see that, but I will take your advice. Thanks.
It’s the same. Someone added it to repo.
"Create a simple two layer PCB for this schematic …
Update the schematic with a few minor changes revised some footprints added one more bypass capacitor C6 added mounting holes Create simple two layer PCB ground pour on bottom layer
denniscote committed 5 days ago"
HI,
I modified the schematic and made a simple two layer PCB mostly as an exercise to test out KiCad v6.0rc1. The board is 3 inches by 5 inches with a ground pour on the bottom side.
I made a pull request to contribute back to the project, but I didn’t follow up here since I thought anyone using the project would see the new files on GitHub.
You will need KiCad V6.0 or a current nightly version to open the file.
2 Likes
I must have already cloned the repo before your commit got merged.
Hello! Where can I find v6.0?
https://downloads.kicad.org/kicad/macos/explore/nightlies
This is the link for the macOS nightly releases. Currently v6.0rc1. It can be found at the bottom the download page at
The same goes for the windows version at https://www.kicad.org/download/windows/
And other versions too I presume.
HTH
Regarding: [quote=“Dennisch, post:45, topic:32106”]
You will need KiCad V6.0
[/quote]
I visited the KiCad web site bout could not find a V6.0. Perhaps it is hidden.
V5.1.12 is featured as the latest stable.
This looks like a usable PCB. It is much better than the PCB posted earlier.
I even see you put in some bridges to stitch gaps in the GND plane but the GND plane can easily be improved further by putting more copper tracks on the front side.
I always find TO92 a bit troublesome for hand soldering because the leads are so close to each other. There is also a footprint for TO92 with the pads in a triangle and this has more room between the pads so shorts are easier to prevent (and to see).
I think C4 and C6 are the decoupling caps for the IC in the middle. You have used quite big footprints. These should be ceramic (not foil) caps, and the ceramic caps usually have a pitch of either 2.54mm or 5.08mm. I would also put these capacitors closer to the pins of the IC.
In the center of the PCB you have a bit of a crowded area. This can be reduced by putting U2 (A connector with Refdes U?) on the left side of U1 (sort of where J12 is now)
If U2 is a radio module, then there should not be a GND plane nearby. (Oops, it has a separate antenna so it’s probably all right).
U4 looks like a voltage regulator. Put a copper zone around the big pad on the left that acts as a heatsink.
Add labels to the connectors to indicate what they are.
I also prefer to use the “oval” variants for THT IC’s. These have bigger pads which are easier to solder.
I also reduce the clearance of the GND plane so the GND plane sneaks in between the pads of the IC’s. This also works better with the Oval pad, as the default round pads do not leave much room between the pins.
I used version 6.0rc1, the first release candidate for the new version of KiCad. It hasn’t been released yet, but it is quite stable and usable, but subject to change as the developers prepare to release version 6.0.
What OS are you looking for?
For macOS and Windows there is a link at the bottom of each download webpage for the current nightly development build. Click on that link and download the latest installer for your OS and CPU.
Hi Paul,
I tried to minimize the changes to the schematic and the components that had already been selected. The placement of U2 was based on the location in the photo of the prototype built on perf-board. The regulator U4 is supplying low current so it is not dissipating very much power, so there is no need for a large heatsink pad which would just make hand soldering the part harder. If I was making changes to the design I would have replaced this part with a simple adjustable through-hole regulator to match the other components. The labels on the schematic are mostly in German, which I don’t understand, so I wasn’t sure if they were useful or not. They could definitely be added.
Again, this was mostly done to try out the latest RC version of KiCad. I thought I would share it rather than just throw it away when I was done. Anyone can take it as a starting point for further improvement.
I hope you are in the US, as I see that the version mismatch message used a US date, viz. 10/14/21. I hope the developers used the locale specific date output routine, and that it will appear as say 14/10/21 in other countries. Better still if it could output in ISO 8601 format, i.e. 2021-10-14.
This is a significantly improved PCB design because there is a very well defined ground.
A well defined ground prevents various signals from mixing as the current from each signal flow back through ground which if thin is quite resistive.
The Mounting Holes M1, - M4 look to be floating, ie not connected to ground.
So I want to ask the question to get people thinking.
Should and how is this ground connected to the enclosure?
If the enclosure has been defined somewhere above I have missed it. The photographs from the GIGHUB repository showed a plastic, non conductive, enclosure. What are the consiquences of this design decision?
The application for this device is a controller for pool equipment (I have not yet figured out what exactly) and there are remote (long cable) sensors. Such applications will experience electrical surges related to lightning and AC Mains power.
Are these circuits resistant to such surges?
What happens if lightning strikes the power or the ground at J1 with, hypothetically 1 Million volts (or 100 Volts)?
Same question for all the other connectors. Like for example J8 Pin 1 the connection to PB2. How much current flows if there is a surge of 100V? Or 10V? Same for J8 pin 2.
What limits the current in the above cases?
I want to share a rule of thumb I learned while designing consumer electronics. NEVER connect a semiconductor in a product to the “outside world” with only a copper trace. You MUST insert as much impedance (resistance and perhaps reactance) in series as is compatible with normal operation of the circuit and signal.
I hope this helps readers consider how to make designs more robust, more Electro-Magneticaly Compatible.