I made a 5V power supply board for MP2303, please give me some advice

网络游侠2018

I made a 5V power supply board for MP2303, please give me some advice [Copy link]

 

This is the first time I have made a power board for MP2303. I welcome your comments and suggestions. Thank you The attachments are as follows: MP2303-5v.zip (1.75 MB, downloads: 61)

2018-9-19 15:35 上传

点击文件名下载附件

懒猫爱飞

1) There is no big problem with the schematic diagram. 2) The PCB routing can be optimized to be more beautiful, and the layout of the components can be slightly adjusted, which will not affect the function and make it look more beautiful. 3) Some vias can be drilled on the bottom pad of 2303 to facilitate heat dissipation. 4) The bottom pad of 2303 should be grounded in theory. Please check the manual to confirm. I haven't read the manual. 5) The copper-plated network can be set to ground and can be connected to the same network. 6) More vias can be drilled around 2303 to the ground. 7) The layout of the inductor and 2303 is not reasonable. 8) Well, let's say so much for now. Finally, I will encourage you. Come on! 7) There are no fixing holes on the board. 8) If you use the board yourself, the border can be set to rounded corners so that you won't cut your hands when you pick it up.

懒猫爱飞

9) In addition, the board frame should not have a keepout layer, so the copper sheet is laid outside the board.

懒猫爱飞

10) If you don’t understand the design rules, you can check them online or find a tutorial.

涛涛熊

1. There is something wrong with the principle. The freewheeling diode should be between the inductor and the chip, not between the inductor and the load. Otherwise, when the MOS tube is turned off, the inductor cannot form a discharge circuit with the diode. You can check the official recommended schematic diagram of the MP2303A chip. 2. Pay attention to the direction of the current when laying out the PCB. At the same time, the entire DC-DC loop should be as small as possible. It is best to output the feedback resistor after passing through the filter capacitor, and the feedback loop should be as small as possible. 3. In addition, your PCB feedback access network is incorrect. How come 5V and NET2303A_3 are together? 4. In addition, the load should be considered. If the current is too large, the wiring should be as thick as possible, otherwise the overcurrent will not be enough.

xxxlzjxxx

All I can say is to read the Datasheet more

涛涛熊

Yes, refer to the datasheet directly. This type of chip usually has recommended schematics, components and layout guidelines.

涛涛熊

Yes, refer to the datasheet directly. This type of chip usually has recommended schematics, components and layout guidelines.

Arvinˇ

I'm just curious, what software was used for the first physical schematic?

topwon

I won’t talk about the other things yet, I hope I can catch up and the board hasn’t been powered on yet. Brother, the position of R102 in your schematic is wrong.

topwon

Taotao Xiong posted on 2018-9-19 20:11 1. There is something wrong with the principle. The freewheeling diode should be between the inductor and the chip, not between the inductor and the load. Otherwise, when the MOS tube is turned off, the power...

This chip does not need a freewheeling diode. The two diodes in the figure, one is for input reverse connection protection, and the other is for output LED indicator.

topwon

1. The loop area of pin3-inductor L1-capacitor C106, C107-PIN4 (GND) should be as small as possible, and the routing should be as wide as possible to avoid vias. 2. Input capacitors C101, C102, and C103 should be as close to pin2 and pin4 as possible, and there should be no vias. In fact, the 0.1uF capacitor here should be removed. 3. The access point of the feedback loop R105 should not be at the inductor (this is actually inconsistent with the schematic diagram), but after capacitor filtering (chip-inductor-capacitor-feedback point), and the routing of the feedback loop should avoid high-frequency and high-current loops (mentioned in the first point).

网络游侠2018

Arvinˇ posted on 2018-9-20 09:32 I am just curious, what software was used for the first physical schematic?

There is a power supply design software on the MPS official website

网络游侠2018

Lazy Cat Loves Flying published on 2018-9-19 16:56 1) There is no big problem with the schematic diagram 2) The PCB routing can be optimized to be more beautiful, and the layout of the components can also be slightly adjusted without affecting the function...

Thank you

网络游侠2018

Taotao Xiong published on 2018-9-19 20:11 1. There is something wrong with the principle. The freewheeling diode should be between the inductor and the chip, not between the inductor and the load. Otherwise, during the shutdown of the MOS tube, the current...

Thank you for your advice

zhuyebb

9) In addition, the board frame should not have a keepout layer, so the copper sheet is laid outside the board.

网络游侠2018

topwon posted on 2018-9-26 09:51 1. The loop area of pin3-inductor L1-capacitor C106, C107-PIN4 (GND) should be as small as possible, and the routing should be as wide as possible to avoid vias. 2. Input capacitors C101, C10 ...

Thank you

网络游侠2018

topwon posted on 2018-9-26 09:36 I won’t talk about the others yet. I hope I can catch up. The board has not been powered on yet. Brother, the position of R102 in your schematic is wrong.