I recently drew a PCB for stm32. Please point out any deficiencies.

DB_DOG

I recently drew a PCB for stm32. Please point out any deficiencies. [Copy link]

 

I recently finished drawing a PCB with stm32 as the main control. The whole circuit is an electronic scale that can be connected to the Internet. Because it is the first time to draw a 32-bit board, the arrangement of some components and even the selection of peripheral devices are not in place. If there are any inappropriate places, please point them out directly, thank you very much! ! file:///H:\QQ\1486897171\Image\C2C\W46)46OEM____F`WQK@$9]E.png

DB_DOG

Sorry, I missed something to add, U1 is stm32f103c8t6, Y1 is 8M crystal, U2 is ams1117, U3 is esp8266, U5 is HX711, U6 is an OLED display.

wudayongnb

Do not place vias on pads, and it is best not to run other signal lines under the crystal oscillator. The crystal oscillator should be as close to the microcontroller as possible, and the crystal oscillator trace should not make any turns. The shorter the better. The pads for the USB port on the far right are all outside the edge of the board. The program download interface does not leave a reset signal; the reset button does not work, and directly short-circuits the power supply and ground; is the OLED an I2C interface? If so, there is no pull-up resistor. Several other buttons are not connected to the ground.

dong2213dong

DB_DOG posted on 2017-12-30 09:45 Sorry, I forgot to add that U1 is stm32f103c8t6 Y1 is 8M crystal U2 is ams1117 U3 is esp8266 U5 is HX711 U6 ...

I don't know if this is the first time you draw a board, but I feel that there are a lot of problems with this board. I will briefly talk about a few of them for your reference. 1. The placement of the main control chip STM32, why is it rotated 45°? I feel that if placed normally, many lines can be laid more smoothly. 2. The ground wires are all connected through a via, and the ground wire is so thin, including the power supply VCC. 3. The board wiring space is very sufficient, and some lines change from thick to thin, which is not necessary. 4. The vias are punched on the pads, and your board does not need to do this at all. 5. It is better to pay attention to the placement of some capacitor components, even though it may just be a test board. The above points are not comprehensive. As I said, they are only for your reference

DB_DOG

[quote]wudayongnb posted on 2017-12-30 10:00 Don't put vias on pads. It's best not to run other signal lines under the crystal oscillator. The crystal oscillator should be as close to the microcontroller as possible. The crystal oscillator line should not be bent as much as possible. The closer it is to the microcontroller, the closer it is to the microcontroller. Thank you for your advice. I was drawing a USB interface and wanted to try to see if two fixed pads could fix the USB: Does the power short-circuit to ground refer to the short circuit caused by only a capacitor between vcc and gud without a resistor? OLED is I2C: I want to connect the 3 buttons to the board externally.

DB_DOG

wudayongnb posted on 2017-12-30 10:00 Do not place vias on the pads. It is best not to run other signal lines under the crystal oscillator. The crystal oscillator should be as close to the microcontroller as possible. The crystal oscillator routing should not bend as much as possible. The more...

The grounding of all buttons should finally be led to the GND pad hole.

DB_DOG

dong2213dong posted on 2017-12-30 10:11 I don't know if this is the first time the OP has drawn a board, but I personally feel that there are a lot of things wrong with this board. Let me briefly mention a few for your reference. 1 Main control chip...

Thank you for your patient review and careful comments. This is the fourth board I have drawn. 1: Before drawing, I have already placed the 32 at many angles. In the end, I referred to the smallest system board I had and placed it at a 45-degree angle. 2: Should the upper and lower ground wires be connected through more holes? The power and ground wires are indeed drawn thin. What is the standard for selecting the line width? 3: There is enough space around the board, but the pins of 32 seem to be a bit dense, so the wires from the chip have changed from thin to thick. 4: I saw that the board drawn by my classmates also had vias on the pads, so I tried it, but I didn’t think it would cause any side effects 5: I didn’t pay attention to the placement of the capacitors before, and I don’t know what impact it will have. I would like to hear more about it. I am ignorant and short-sighted, so I hope you can forgive me! !

1399866558

Repaint it.

wudianjun2001

Happy holidays to the host, I wish all your wishes come true and everything goes well in the new year!

wudayongnb

DB_DOG posted on 2017-12-30 11:49 Thank you for your advice. I was drawing a USB interface and wanted to try whether two fixed pads could fix the USB: Does the power short-circuit to ground mean that only VCC and GUD are connected...

Look at your schematic diagram. After the reset button is pressed, is the power and ground short-circuited? The program download interface does not print the reset signal. I2C interfaces must have pull-up resistors.

wudayongnb

DB_DOG posted on 2017-12-30 12:05 Thank you for your patience and careful comments. This is the fourth board I have drawn. 1: Before drawing, I have already placed 32 at many angles, and finally...

The width of the power line is generally 1 ounce of copper thickness, and 1 millimeter carries 1A of current. The via is placed on the pad. If the via is relatively large, it is easy to cause cold soldering. The decoupling capacitor of the microcontroller is generally as close to the pin of the microcontroller as possible.

DB_DOG

wudayongnb posted on 2017-12-30 14:17 The width of the power line is generally 1 ounce of copper, and 1 millimeter carries 1A of current. The via is placed on the pad. If the via is relatively large, it is easy to cause virtual...

OK, thank you for the detailed explanation

DB_DOG

wudayongnb posted on 2017-12-30 14:07 Look at your schematic diagram. After the reset button is pressed, is the power supply and ground short-circuited? The program download interface does not print out the reset signal. The I2C interface is...

OK, I see. It seems that my problem is still quite serious. Thanks for pointing it out.

DB_DOG

1399866558 posted on 2017-12-30 13:48 Repaint it.

I still want to save it

shower.xu

1. The space is relatively large, and there are still more beautiful ways to arrange it. You can arrange the position first and then plan the line. This component can be placed on one side only. 2. Check each network one by one to see if there is any electrical error. You can choose on the left side of the PCB interface. 3. For routing and rules, you can refer to the documents of the board factory. For example, the Jiali Chuang website clearly states the minimum line width and pads. But you can definitely use it this way. 4. Print out 1:1 (assembly drawing) before sending the board and compare the component package and pin position to prevent scaling and reverse drawing.

DB_DOG

shower.xu posted on 2017-12-30 23:11 1. The space is relatively large, and there are still more beautiful ways to arrange it. You can arrange the position first and then plan the line. This component can be placed on only one side. 2. A...

The benefits are not shallow, thank you for your advice.

曹伟1993

I don't know why, even though I chose a square pad, I still routed the wires this way. Don't route the signal wires under the crystal oscillator. The four positioning holes can be grounded to make the board better grounded. There are many other places, so I won't mention them one by one.

DB_DOG

Cao Wei 1993 posted on 2018-1-4 12:25 I don't know why, even though I chose the square pad, I still routed the wires this way. Don't route the signal wires under the crystal oscillator. The four positioning holes can be grounded, which can make the board...

Do you mean that the square pads should not be routed out from the corners? I didn't notice this before, and I'd like to hear more about it!

Kitty0515

I don't understand why the square pad can't be wired out from the corners. Adding teardrops shouldn't have much impact. Waiting for your advice.

LONG_EM

Would it be better to have two layers of boards for the floor?