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.
You are correct I am in the land of crazy date conventions. I often use 20211126 style because I like to sort things but I am in a minority.
Does anyone know the part number for this kind of enclosure?
A drawing showing the mounting holes might help for designing a PCB.
Cosmin,
Can you recommend enclosures use in the pool industry?
While I have no professional experience I know there are enclosures rated for exposure to the environment and I have read the phrase “wash down” which I think implies spraying with a water hose and perhaps even a pressure washer. IP66 NEMA might be it.
There are also compression fittings to go around cables. Again I do not know the industry to know how to find them.
Please advise so we can help you better.
The enclosure must be IP65 min., but can also be an DIN rail enclosure no matter the IP grade, wich can be mouted in an IP65 bigger box with din rail. At the beggining I didn’t know how big/small the PCB will be so I had to wait and see before I can choose an enclosure.
I will choose the enclosure and I will post drawings and dimmension.
Thank you, guys!
1 Like
From my point off view, anyone who has a better idea the the original, can make modifications as long they will lead to a better PCB. You don"t have the stick to the oroginal “design” if you find a better position for a component or a better component as a replacement.
For ex.: I can’t find any THT 80k resisistor so I plan on adding another resistor in serial, like 33k+47k
I haven’t thought so far, I think it’s because of my lack of professional knowledge in electronics … but if you can, and want to, you can make additions or changes to the PCB. This module is intended to monitor and report PH, ORP, PRESSURE and FLOW to a smart home central control unit. The module and the central unit communicate wirelessly through 868 mhz. The central unit also controls wirelessly some actuators that start and stop the pumps. So no mains connected to the board itself.
Maybe these infos help.
Where from this value comes? Are you sure you can’t use standard 82k value?
Why THT. When SMD began to be available for us we started to use them (about 1990). There is no problem to hand solder 0603.
I understand by the relay outputs. I’m used to have wide tracks connected to relay contacts. I double them - the same track at top and bottom (appropriate schematic to avoid crossing these tracks).
Seeing only PCBs I assume you have at the beginning the isolated DC/DC converter. Such converters frequently generate so high common noise that they need to be shorted (input to output) by appropriate capacitor to be in accordance with EMC rules. What datasheet says about it?
Many years ago we were asked if we can improve the device that its manufacturer had continuous problems with them. He had about 50 of them installed and got lot of calls to service them - disconnecting/connecting 12V supply wires helped. Their diagnose was: devices overheat and freeze. When I sow the PCB having 0 protection elements and with 1-wire touch-button socket connected directly to microprocessor pin I told them: The sequence is opposite - microcontroller gets latch-up (because of ESD from touch-button) and then consumes as much current as possible so regulator get hot and its thermal protection limits the current. So the regulator structure is kept at about 120°C and no wonder the housing of the device gets warm.
Your PCB is at that stage now - 0 protection elements. For each wire connected to device you should consider what kind of interference you can expect at it (ESD, Burst, Surge) and how to protect your circuits against them. It depends what is there connected, if that has separate supply and how long is the connection. Right software (ignoring for example short state changes made by ESD) is also a part of protection.
Remember that it happens that lightning strikes somewhere near the building with your devices.
Some time ago I posted here links to (in my opinion) very good papers about that:
See also few posts later in that thread other links I posted.
From what I understood from the guy who designed the whole thing, any other value except 80k will alter the readings of the pressure sensor…
Regarding what you said about protecting the circuits, I don’t have the knowledge to make those improvents… you are asking me to run before I learn to walk.
Any modifications or suggestions are more the welcome.
Regards,
Cosmin