Para español presiona aquí.
We all know how cheap and easy to get chinese electronic boards are, but have you ever thought about their quality and how dangerous or inconvenient it could be to use them in your home or in a paid project?
In this post I am going to tell you about 3 errors I’ve found in some of these boards. If after reading if you continue using them in paid projects, then it will be at your own risk and you will no longer be able to plead insanity or ignorance when in front of the Grand Jury.
On the other hand, we can learn a lot by analyzing the mistakes of others, and what is more important, we will avoid repeating them in our own designs.
Tabla de contenidos
- Oscillations (false activations)
- Using multiturn trimpots
- Final words
Oscillations (false activations)
Many chinese boards that we usually buy are dedicated to:
- Reading some type of analog signal,
- Comparing the read value against a reference DC voltage and,
- Emitting an output signal, normally binary.
Almost all the boards I have analized use the LM393 comparator. There is nothing wrong with the comparator, it just behaves as any other comparator, but with the way one uses it.
It is well known that at the comparison threshold, when both signals are almost equal, the output tends to oscillate. This effect is multiplied if the analog signal of interest is slow (its slope is almost horizontal). And there are lots of slow signals in nature: temperature, liquid levels, obstacle detection, etc: they do not tend to change quickly.
The following image is of an “obstacle detector” sensor based on the LM393 comparator:
And its output, when an object is entering into its detection range very slowly, looks like this. Watch the noise zoom (the oscillations):
And the slower the object enters into the detection zone, the worse the oscillations will be.
The output of another obstacle detector is even more impressive:
I have to point out that the above circuit is different in that it uses an LM555 to generate a 38KHz carrier signal which is then detected by an IR decoder equivalent to the VS1838B (or TSOP1238) and converted to pulses that can be read by any microcontroller… in theory. But the problem remains the same: you get a bunch of (false) pulses when you expect only one.
Did you expect to read a simple pulse? What will happen when the client who paid you for the project receives 10 or 20 pulses when they really expected one for their count?
What is the problem?
The problem is that comparators work like this and as I pointed out, the oscillatory effect is worse the slower the signal to be compared. For fast signals the problem is not so serious, and in most cases it does not exist.
You might be thinking that this problem can be solved with a filter capacitor or by software. It could work. But I have another more interesting and professional solution for you that I will deal with in depth in another article: hysteresis.
What is the solution?
Hysteresis. Although I will deal with this topic in a separate article, I will tell you in advance that hysteresis is the incorporation of a dead zone within the comparison threshold in which nothing will happen, making the output signal come out clean.
Hysteresis is like a flip-flop (or if you don’t mind, a 1-bit memory):
- If you put a logic 1 at its input, its output will go to, say, 0;
- If you put a logic 0 to its input, its output will go to 1.
- And as long as the input signal is in limbo 1-0 the output signal will not change.
(The flip-flop I just described is not entirely accurate; however, it is the memory effect that is important.)
How much is such space-age technology going to cost me? ? Any! Well yes, two resistors and best of all, you will continue to use the LM393, or LM311, or any other comparator you like. It’s that simple.
As I write the article, review the following image and take a look at the references if you want to look what hysteresis is.
This is the point that worries me the most and it is for this reason that I am asking you to reconsider the use of Chinese boards in your projects.
So far I have encountered three kinds of problems, so I will use three sections to describe each one.
- Relays without slots.
- Relays without the minimum safe clearance.
- Relays with thin tracks.
Relays without slots
Most of the low cost Chinese boards that include relays do not incorporate something that we call slots.
And what are those for? We insert slots to prevent or stop PCB charring, move high voltage signals away from low voltage signals, and also to reduce the likelihood of arcing.
- Electric arcs. When a high voltage (voltages greater than 30VAC) is present between two terminals, it could be the case that an electric arc is generated. A damp environment or dirt on the PCB could contribute to this happening.
- Carbon traces. And after the electric arcs has ocurred, we got the problem of carbon traces that remains on the PCB surface. It also could happen due to the high currents that circulate between its tracks on a regular use.
The slots serve two purposes:
1. They prevent carbonization from spreading by increasing the creepage. Creepage is the physical distance that an electrical current must follow on the printed circuit (no longer in the air, as opposed to electric arcs that happen over the PCB).
2. They separate the high voltage from the low voltage signals.
To avoid, and if necessary stop, carbon traces, what we can do is increase the creepage by inserting slots in the relays high voltage pads. I should point out that a carbon trace on a printed circuit board can drive high voltage signals towards low voltage ones because of the increased conductivity due to the carbon trace.
To make matters worse, many relays, by design, have a high-voltage potential terminal between two low-voltage signals, so that, in the event of a fault, the high voltage could reach the low-voltage circuitry:
With electrical arcs, since they occur in air, the only thing left for us to do is move the relay away from the rest of the circuit, as I will discuss in the next subsection.
What is the solution?
- Insert slots in each high voltage relay pad used in the circuit, and also in all those places where there is a possibility that high voltage signals reach the low voltage circuitry. The width of the groove must be at least 1.0 mm.
- If your PCB is two-sided, place the tracks that go to the relay coil on one side, and place the high-voltage tracks on the other side.
Use both techniques whenever possible.
Is it expensive to add the slots? Nope! In fact, PCB manufacturers do not charge for them since they have long been considered part of the manufacturing package.
I am going to make my board with homemade techniques, how do I do it? Well, here it is more difficult, unless you have a CNC machine, and no, we don’t always have one at hand. However, in this case, introduce a safe separation clearance (distance), as I will discuss it in the next section.
Another nice cleatance and creepage explanation (it will download a PDF document)
Relays without the minimum safe clearance
In the following image you will see that a potential high voltage signal is practically attached to a track that carries 0V, and very close to a 5V one, and is almost attached to the coil terminals.
This image comes from a very famous event counter in the world of electronics. Didn’t it scare you?
When I bought the board and saw this problem I got scared. I immediately envisioned a scenario where a motor would turn on and count turns, then turn off, then turn on again, and so on.
When the motor turns on that implies high currents, much greater than 10A than the relays and their tracks that must conduct it (up to 20 times the nameplate current of the motor). The starting current of a motor is called inrush current. Fortunately, the duration of this initial current is very short, but since it is intense it could cause the aforementioned electric arcs and carbon traces.
What is the solution?
Here we have three solutions, I’ve repeated two from last section, but equally valid:
1. Move the relay as far as possible from the low voltage circuitry (increase the clearance).
2. Insert a slot, as I mentioned in the previous section. Or better yet, insert two slots, although the first one is enough:
1. The slot that separates the high voltage terminal from the coil terminals.
2. A slot that separates the entire body of the relay from the low voltage area
3. If your PCB is two-layers, on one layer place the tracks that go to the relay coil, and on the opposite layer place the high voltage traces.
Clearance is the space or distance between tracks, or between tracks and pads (or vias). So we need to increase the clearance between the high voltage tracks and the low voltage circuitry as much as possible.
This solution could have a small cost, since a larger board will cost us a little more money. But with some imagination and creativity we could implement these solutions while keeping the PCB size small enough.
However, in order to save a few cents, the Chinese sellers have preferred to design dangerous boards. Nonetheless, neither you nor I are like them and we do put security before cost.
In the particular case of the counter with which I begin this section, the solution was as simple as placing the relay horizontally, but those Chinese sellers don’t care about our safety. They are not our friends.
You can no longer say I didn’t warn you.
Relays with thin tracks
Almost all Chinese boards use relays marked for 10A and 127VAC/250VAC, but the width of their tracks does not correspond to that current:
The following relay is a catalog of design errors:
- It has no slots.
- The power tracks are thin and do not allow for a current reinforcement (as I’ll explain later).
- A high voltage terminal pad from the relay is very close to the 0V terminal.
- This same high voltage terminal track starts at the top layer and then goes back to the bottom layer through a pad.
- Near this pad, and another high-voltage pad, a signal passes for the coil.
- A low voltage signal changes layers and goes under the high voltage track, and then changes back.
- The signal terminals have leftover copper (not seen but there they are).
- Even mechanical mounting holes are dangerously close to high voltage.
Back to our topic: there is a formula to determine the width of the track that can handle this current, but intuitively we understand that the thicker the track, the better. Well, the Chinese have other ideas, as if they were going to charge for the extra copper.
And while it doesn’t cost them anything to use thick tracks, they insist on making blundering design mistakes. The following boards (555, standalone, thermostat) have traces too thin to properly handle currents up to 10A.
The meter board has indeed placed thick tracks, but at the cost of being glued to the low voltage circuitry. Where did the Chinese learn to design like this?
In a previous section I talked about carbonization due to excess current: the thinner the track, the higher the probability of carbon traces, and eventually, electric arcs could occur.
What is the solution?
We have 3 solutions that you can carry out even on homemade boards:
- Very thick tracks, 7.19 mm to be exact (for the 10A case), but since that will not always be physically possible, here comes the second part:
- Tracks thinner than 7mm, but with exposed tin, and
- Keep tracks as short and straight as possible.
- (Some also place tracks the same width as the power tracks on the opposite layer, and parallel to them, but without exposing the tin.)
The exposed tin will allow you to reinforce the track either with solder or, in extreme cases, with wire and solder from the relay pad to the connection pad.
These solutions come at no cost, but the Chinese just don’t care about you.
Mezcla de señales de alta tensión con baja
I’m always in shock every time I analyze Chinese boards. I purchased a very famous thermostat and was preparing to make the electrical connections when I noticed something incredibly dangerous: a potential high voltage connection is immediately at the 12VDC supply.
What is the problem?
That you may want to connect the 12VDC power cable, but somewhere you forgot to disconnect the high voltage, and inadvertently:
- You put your screwdriver on the high voltage terminal, or
- You touch with your finger the bottom of the board on the high voltage terminal. Here you could argue many things defending the Chinese, who neither know you nor care about you, but deep down nobody with a bit of common sense would place high and low voltage side by side, that’s wrong, that’s not how we design our electronics.
And if that wasn’t bad enough, and contrary to what you might argue, it also doesn’t have high-voltage signs that will eventually alert you to danger.
What is the solution?
A solution in a new design is what common sense dictates: place the high voltage connector(s) as far away as possible, in a place that is far from the user. Perhaps place them in diametrically opposite places from low voltage and in a place that is difficult to access.
And of course we are going to require visual aids in the PCB screen printing to tell us to be careful.
On the other hand, in already manufactured designs like the one I mentioned, what you can do is to connect the neutral of the load onto the board, and the live of the high voltage leave it separately.
Using multiturn trimpots
This situation is not nearly as dangerous as the problems in the previous section, however it is functionally terrible.
Take this next LM555 based timer as an example, which can delay between 0.1 and 11 seconds. How do you go about simply setting it to delay for 5 seconds? And to delay for 8 seconds? and to delay for 2 seconds? You are going to have to give the trimpot a lot of turns, and with trial and error, eventually arrive at the desired delay time. I don’t like this procedure, do you?
Does your client, is going to guess every time he wants to change the corresponding parameter?
This same situation will hapen with obstacle detection or temperature detection boards: how many turns do I need to detect objects at 8 cm… and at 4 cm… and at 12 cm? How many turns do I need to detect 50 degrees centigrades, 35 centigrades degrees, 60 centigrades degrees?
What is the solution?
Here we have two solutions:
- Use single turn potentiometers, and there are many types of these. Those that are small in size include a mark, while larger ones can be fitted with knobs. Whichever you choose will allow you to put some kind of mark over the PCB’s silkscreen layer, or on the case, indicating the position of the case for certain values.
- If you insist on using multiturn trimpots, or your application requires fine calibration, then you should place a test point on your PCB so that every time you need to calibrate you can connect with ease a multimeter or oscilloscope. (In fact, there would be two test points: one for the signal to be calibrated and one for easy access to the 0V of the circuit). Keep in mind, though, that you’re going to need some kind of table that tells you that X volts correspond to Y centimeters/seconds/degrees centigrades for the kind of applications you’re dealing with.
Chinese boards should be considered as toys, or proof of concept elements, or simply as objects of entertainment.
I am not saying that one should not buy them, I personally do it for the aforementioned purposes. But I am concerned for all those hobbyists who pretend to be engineers and incorporate such boards into sensitive circuits or paid projects.
We must never abuse the ignorance of our clients (in the field of Electronics); they are trusting us and we should never make final designs based on these boards and the horrible connections between them, that makes them even more dangerous.
Make your proof of concept, show it to your client, and when you have their approval, then make the printed circuit(s) integrating all the electronic components of the design using the best practices; maybe you can even include some of the ones I’ve discussed in this article.
Take a look the following sequence of images where I show you the evolution from an idea I had to a final product. Before the first prototype I used modules, an Arduino UNO clone and spaghetti wiring:
I want to mention an important point before closing: we should stop accepting the chinese garbage as something “normal”. We don’t have the obligation of correcting their mistakes; instead we have to push ourselves to create our own designs.
I hope you find this article useful and from now on you will consider the pros and cons of using Chinese boards. And don’t forget that you can also learn from bad designs.
- After reading this article you will never look at chinese boards the same, or how to learn from the mistakes of others: Design mistakes - septiembre 13, 2022
- Después de leer este artículo no volverás a ver igual a las tarjetas chinas, o de cómo aprender de los errores de otros: Errores de diseño - septiembre 6, 2022
- What’s inside the 555 on-delay (chinese) timer? (Schematic included) - agosto 11, 2022