STM32F103 min system with USB-TTL converter?

[bjdhjy888]

Hi,

     I recently managed to build my own STM32F103 min. system on a PCB. I was so happy about it. I flashed my LED blinking .hex file onto it, using someone else's USB-TTL module.

     I wanted to learn more, so I designed and improved my STM32F103 system with my own USB-TTL circuit added onboard. But no .hex file could be flashed onto it. (I used FlyMCU for the flashing).

     I then used my multimeter to check the voltages of my AMS1117-3.3 chip and noticed its output voltages were too high at 4.5V.

     I used FT232RL SSOP-28 for the conversion.

     I also reviewed my schematic and PCB layout and did find an error that one of the pins of my AMS1117-3.3 was not linked to GND of my micro USB.

     However, even after I fixed it using a flying lead on my PCB, the problem remained, i.e., I could not communicate with my STM32.

     Could someone on here help me review my schematic? Thank you so much!

[ataradov]

Someone probably can. Why not attach the schematic here?

[bjdhjy888]

Thank you.
Here is my schematic. I apologize if they don't look too professional, as I'm a newbie.
Would someone please help me find out where I did wrong? (The system worked perfectly before I adeed my FT232RL and AMS1117.)

[Psi]

Ok, one thing i will say.
Ya should wire the ft232rl 3.3v output pin to vccio instead of using 5V from USB.
Then TX/RX are 3.3V level and will match the STM32

I can't recall which pins on STM32 are 5V tolerant.
But if the pin you're using for TX is not 5V tolerant it will backfeed 5V onto the STM32 VCC and this will cause major problems

Also please correct all the SCH pin names to match the actual IC pins. I assume you just repurposed some other sch component?

There's lots of stuff in that SCH that i have no idea what it's doing.

[bjdhjy888]

Yes, I am correcting my SCH. Thanks.
I hope my SCH will be easy for people to read once it's corrected. 

[bjdhjy888]

Ok, one thing i will say.
Ya should wire the ft232rl 3.3v output pin to vccio instead of using 5V from USB.
Then TX/RX are 3.3V level and will match the STM32

I can't recall which pins on STM32 are 5V tolerant.
But if the pin you're using for TX is not 5V tolerant it will backfeed 5V onto the STM32 VCC and this will cause major problems

Also please correct all the SCH pin names to match the actual IC pins. I assume you just repurposed some other sch component?

There's lots of stuff in that SCH that i have no idea what it's doing.

So you are saying this  is wrong? (I followed this pic I got from the Internet)

[mvs]

I recently managed to build my own STM32F103 min system on a PCB. I was so happy about it. I uploaded my LED blinking hex file onto it using someone else's USB-TTL converter.
I wanted to learn more, so I designed and building STM32F103 min system with my own USB-TTL converter circuit. But no program could be uploaded onto it. (I used FlyMCU for the uploading).
...
Could someone on here help me review my schematics? Thank you so much!

Getting to a bootloader in manual way might be a bit tricky. Usually RTS and DTR pins of USB-UART bridge are used to manipulate RESET and BOOT0 pins of STM32, allowing FlyMCU to do it for you automatically.

[ataradov]

This is a totally unreadable schematic. I know you want to do things quick, but as you can see, it does not work out this way. Clean up the schematic and the issue may become obvious.

[ajb]

Your schematic and layout both need a LOT of work.  But that's okay, you said you're a beginner, and people here can help you learn.

Some things in no particular order:

* While you have decoupling capacitors, they are way too far away to be doing their jobs.  Decoupling caps need to be mounted as close as possible to the IC supply pins to be effective
* Also there appear to be no decoupling caps dedicated to the FT232.  Read the datasheet for the FT232 and follow all of its guidelines for layout and support components exactly. 
* Use reasonable schematic symbols for components.  You appear to be using battery symbols for headers and for crystals.  This is confusing.
* That can't be the right symbol for the MCU, either.  This is hugely confusing to anyone reading your schematic, including you when you come back to this schematic in a week.  Be nice to future you.
* Use power ports instead of wires for gnd and supply nets.  This will immediately clear up a lot of clutter in the schematic.
* Use schematic symbols with proper names for pins, or at least name the nets attached to those pins.  It's impossible to see if your FT232 is even close to correctly connected without referring to the datasheet. 
* Use a ground plane.  Trying to do an MCU and USB on a two layer board with those skinny traces (and no decoupling caps) is asking for all sorts of trouble.  It can be done, but just get in the habit of making the bottom side a solid ground pour with as few interruptions as possible.
* The routing for your crystal needs to be tightened way up.  Currently the loop area encompasses a quarter of the board.  That means it's an antenna, and will radiate like crazy.

It's possible that your current PCB is still usable, but frankly I wouldn't put good odds on getting the FT232 to work as-is.  I would highly recommend you start by redoing the schematic, and post here (not necessarily this thread, but on these forums) for feedback as needed.  Then start over with a new board design, and again, post here for feedback.  There are lots of threads here of that sort, so it's worth taking a look at them, as well as other resources on layout.  With a better schematic and a better PCB, you will have a much easier time troubleshooting.  As it is, it's virtually impossible to say whether your FT232 isn't working because it got fried when the regulator was mis-wired, or because the layout is simply not up to it.

If you decide to start a new thread, please post a link here so we can follow up and see how it goes.  Good luck!

[bjdhjy888]

I couldn't be happier to read you guys' helpful tips. God bless your hearts. I love this forum!

Now, I am re-constructing my schematic from scratch. I will also re-do my PCB layout all over again, following your instructions. Some explanations below:

1. I manually downloaded my .hex file onto my STM32 to learn more and have full control, though I know it might be indeed trickier than doing it automatically with something else.

2. Yes, I indeed wanted to acomplish my 1st STM32 project quickly. This was good and bad attitude. Now, I want to re-do this project carefully and slowly with a solid fundation.

3. Yes, I knew those capacitors were supposed to be placed in close vacinity to my STM32, but I kinda hesitate to do so, as it might still work and I could solder the 0805 capacitors easier with extra spaces.

4. Do I really need to follow the datasheet of FT232 exactly? The schematic I found from the Internet had no other capacitors. Does that mean that schematic is inaccurate? I better follow FT232's datasheet stringently?

5. I was new to Altium Designer and could not find the proper symbols for my desired components, so I repurposed them. Now, I'm correcting them using the correct ones.

6. By "power ports", do you mean these?


7. For the MCU pins, would this be better?


8. Finally, I did pour copper on both side of the PCB and connected it to GND. The reason you didn't see it was that I deleted it on purpose from my PCB, so you could see the circuits better. In real life, my PCB looks like this:



Again, please forgive me for being inexperiened(6-month old self-taught engineer, with learned YouTube lessons, technical books and hands-on kits) and thank you!

[ataradov]

I don't think the problem is with bypass capacitors or the layout of the board. I'm pretty sure, if there is a problem, it is in the schematic or soldering.

Another problem with capacitors is their actual placement. While it is OK to leave some space for ease of soldering, they must be located on a shortest path from each VDD pin. They won't do anything if they are neatly placed in a row in the corner of the board.

So lets start with a cleaned up schematic. Those are power ports and it looks like a correct symbol. Redraw the schematic using them, and we'll from there.

[bjdhjy888]

Thank you.

I have another question for pouring the copper.

https://www.novatel.com/assets/Documents/Papers/OEM7700-Product-Sheet.pdf



In the above link, you will see a pic of NovAtel's board, on which it features its copper at its four corners and on its two upper and lower sides. Note that there are no green pastes covering these specific areas. The copper basically covers all its rims and via's.

They look cool and I guess their purpose is to eliminate noise or interferences. Correct? No to mention the dots(via's?) on the copper for the same purpose?

My question is, how do you make such feature with Altium Designer? Would I be able to acomplish such work with the software? I did not see such function in the software. Does anyone have any clues?

Thanks.

[ataradov]

The opening is to ensure contact with the metal case or mounting chassis. This is done for EMI reasons, but this design is far too low speed to worry about that.

I don't know specifics for Altium, but generally all you need to do is modify solder mask polygon to whatever shape you want to keep open.

Via stitching in this case looks like it was done manually by simply dropping a lot of vias. But I'm sure Altium has tools to do that automatically, since even KiCad does. This is more useful for your design, but again, not really critical. Just place a few vias here and there along the ground planes and you will be fine.

[Psi]

Ok, one thing i will say.
Ya should wire the ft232rl 3.3v output pin to vccio instead of using 5V from USB.
Then TX/RX are 3.3V level and will match the STM32

I can't recall which pins on STM32 are 5V tolerant.
But if the pin you're using for TX is not 5V tolerant it will backfeed 5V onto the STM32 VCC and this will cause major problems

Also please correct all the SCH pin names to match the actual IC pins. I assume you just repurposed some other sch component?

There's lots of stuff in that SCH that i have no idea what it's doing.

So you are saying this  is wrong? (I followed this pic I got from the Internet)

There's multiple ways to connect power to a FT232RL depend on what your connecting the chip to.

Put simply...
The way you have it the FT232RL core runs at 5V, so all its outputs are 5V.
If you have a 3.3V processor they usually don't like 5V on their inputs, so the FT232RL provides an onboard 3.3v regulator.
To use it you feed the 3.3v output pin into VCCIO. This makes the FT232RL core run at 3.3V and so all the outputs are all 3.3V to match the STM32 inputs.

[Doctorandus_P]

Why do you not simply buy some ST-Link V2's from Ali / Ebay / China?
These cost less than a the FTDI chips and you can not only program the STM32 with it, but you can also use them for debugging.

The hardware of these is also just a STM32 in a nice small aluminum USB stick format. You can pull the aluminimum tube off to look what's inside (and for re-programming etc.).

Unfortunately there are some different variants of these, and not all have the same quality.

Most of these can also be re-flashed with the "black magic probe" firmware to increase their capabilities, but I haven't yet seen a need to dive into this.

[MFraylich]

I use "blue pills" STM32F103CB boards for every task an arduino would be used for and am sure that the F103 chips don't need a USB-TTL converter, as the USB on these boards connect directly to the chip. You might need to configure it in the bootloader (I use STM32duino bootloader and this needs to be flashed to the board, instructions on this below if needed).

STM32F103C bootloader and USB fix for STM32duino

    1. Set B0 (right when USB is top) to 1.
    2. Install Flasher from en.flasher-stm32. Available from https://www.st.com/en/development-tools/flasher-stm32.html
    3. Connect the STM to a UART interface with RX of the UART to pin A9 and TX to pin A10.
    4. Use the flasher to add the DFU bootloader in STM32duino-bootloader.
    5. Remove power and move B0 back to 0.
    6. Install the Maple drivers using the bat files from https://github.com/rogerclarkmelbourne/Arduino_STM32
    7. Add http://dan.drown.org/stm32duino/package_STM32duino_index.json to the board manager in preferences.
    8. In Arduino IDE go to boards manager and install Arduino SAM for the Due board to get the correct g++ files.
    9. Connect the board using its USB connector to the PC.
    10. Select STM32F103C and the 128k Flash option and make sure “STM32duino bootloader” is selected as the upload method. At this point the device doesn’t have a port, don’t worry.
    11. Flash a sketch to the board and it will install the full bootloader, the device will now have a port.
    12. Use the board!

Perhaps this will solve the problem.

[ajb]

I'm glad you had ground pours, that's good! 

4. Do I really need to follow the datasheet of FT232 exactly? The schematic I found from the Internet had no other capacitors. Does that mean that schematic is inaccurate? I better follow FT232's datasheet stringently?

Definitely favor the datasheet over random examples found on the internet!  The datasheet will tend to be fairly conservative, so while it may cost a little bit more in terms of components and board space, it generally gives you a much better chance of having the part work as expected.  Datasheets are NOT infallible, but on the whole, they're FAR more reliable than random schematics on the internet.  As you gain experience you'll be better able to tell what's really required to get a part to work reliably, which won't always be what the datasheet says, but it will usually be pretty close.

Regarding the picture of that Novatel PCB, the way to do that in Altium is generally to place the copper pour using a polygon, place vias as you like, and then place an object on the solder mask layer to create an opening to expose the copper.  (The mask layers are negative layers, in that any object placed on the layer creates an opening in the mask.)  Altium does have a tool for automatically placing stitching vias, but it's kind of clunky.  For small areas it's just as easy to place the vias manually, perhaps with the aid of the grid or by copying and pasting blocks of them.

[bjdhjy888]

Why do you not simply buy some ST-Link V2's from Ali / Ebay / China?
These cost less than a the FTDI chips and you can not only program the STM32 with it, but you can also use them for debugging.

The hardware of these is also just a STM32 in a nice small aluminum USB stick format. You can pull the aluminimum tube off to look what's inside (and for re-programming etc.).

Unfortunately there are some different variants of these, and not all have the same quality.

Most of these can also be re-flashed with the "black magic probe" firmware to increase their capabilities, but I haven't yet seen a need to dive into this.

Thank you for your suggestion.

The reason that I wanted to add my own USB-TTL circuit onto my STM min. system was I think the best way to master electronics is to DIY modules(systems) from scratch. (I did buy them before, including the USB-TTL converter)

I was playing with Arduino and interested in Raspberry Pi, but I realized that despite they are cool platforms with an easy to use IDE and language, I will never fully understand the fundamentals(electronic parts and the C programming language). It's a like good C# programmer may never know what a transistor on an IC is.

I believe that buidling an electronic module from scratch with schematics and then get them manufactured at a PCB factory for further soldering and debugging is the best way to understand them with hands-on experience, though it takes quite a lot of efforts. Just my 2 cents though.

[coromonadalix]

I use "blue pills" STM32F103CB boards for every task an arduino would be used for and am sure that the F103 chips don't need a USB-TTL converter, as the USB on these boards connect directly to the chip. You might need to configure it in the bootloader (I use STM32duino bootloader and this needs to be flashed to the board, instructions on this below if needed).

STM32F103C bootloader and USB fix for STM32duino

    1. Set B0 (right when USB is top) to 1.
    2. Install Flasher from en.flasher-stm32. Available from https://www.st.com/en/development-tools/flasher-stm32.html
    3. Connect the STM to a UART interface with RX of the UART to pin A9 and TX to pin A10.
    4. Use the flasher to add the DFU bootloader in STM32duino-bootloader.
    5. Remove power and move B0 back to 0.
    6. Install the Maple drivers using the bat files from https://github.com/rogerclarkmelbourne/Arduino_STM32
    7. Add http://dan.drown.org/stm32duino/package_STM32duino_index.json to the board manager in preferences.
    8. In Arduino IDE go to boards manager and install Arduino SAM for the Due board to get the correct g++ files.
    9. Connect the board using its USB connector to the PC.
    10. Select STM32F103C and the 128k Flash option and make sure “STM32duino bootloader” is selected as the upload method. At this point the device doesn’t have a port, don’t worry.
    11. Flash a sketch to the board and it will install the full bootloader, the device will now have a port.
    12. Use the board!

Perhaps this will solve the problem.

Be sure r10 is around 1.5 k ohms, there was some connection problems on some computers

Check known issues section :  https://wiki.stm32duino.com/index.php?title=Blue_Pill#Software_installation

[bjdhjy888]

I re-drew my schematic from scratch, correcting all my previous mistakes.
Would you please help me review my latest schematic? Thank you so much!
The STM32 min. systems is supposed to blink an LED, with the function of USB-TTL.

[thm_w]

I re-drew my schematic from scratch, correcting all my previous mistakes.
Would you please help me review my latest schematic? Thank you so much!
The STM32 min. systems is supposed to blink an LED, with the function of USB-TTL.

Looks good and neat.

NRST should be 100nF not 100pF, but its optional like you said.
What is the purpose of the diode on RxD line?

[bjdhjy888]

I re-drew my schematic from scratch, correcting all my previous mistakes.
Would you please help me review my latest schematic? Thank you so much!
The STM32 min. systems is supposed to blink an LED, with the function of USB-TTL.

Looks good and neat.

NRST should be 100nF not 100pF, but its optional like you said.
What is the purpose of the diode on RxD line?

Thanks for your help.
As far as the diode is concerned, I previously copied it from another schematic from the Internet, and now it's been removed from my latest schematic.
I've also fixed some minor mistakes today.
Here's my current schematic and layout. Any suggestions would be highly appreciated.
I will get the PCB manucfactured once it's free of mistakes. (The GPIO is left out doing nothing on purpose. I will wire it to STM32 in my next design. And I will pour some copper once the schematic is free of mistakes.)
Bless you.

[profdc9]

If it would help, I have a kicad project with my own version of the bluepill STM32F103C8T6 you could start with if you want to make your own development board.

https://github.com/profdc9/STM32alt

I also made one for the STM32F4 as well

https://github.com/profdc9/STM32F4ThruPill

I made these so that generic through-hole parts can be used, but you can change the footprints if you choose.

[thm_w]

Thanks for your help.
As far as the diode is concerned, I previously copied it from another schematic from the Internet, and now it's been removed from my latest schematic.
I've also fixed some minor mistakes today.
Here's my current schematic and layout. Any suggestions would be highly appreciated.
I will get the PCB manucfactured once it's free of mistakes. (The GPIO is left out doing nothing on purpose. I will wire it to STM32 in my next design. And I will pour some copper once the schematic is free of mistakes.)
Bless you.

http://chuantu.xyz/t6/702/1565913407x2073530527.png
http://chuantu.xyz/t6/702/1565913446x2073530527.png
http://chuantu.xyz/t6/702/1565913459x2073530529.png

- I normally like to see some outlines around the capacitors/resistors in the silkscreen to make it clear where to place it (like C9 has). But that is more for convenience when building, you dont have to have it. I wonder why yours do not show up.
- The placement of C6 is not bad, but C7 and C8 can be improved. They can be closer to pins 24, 36, 48, and two do not share the same pin. So you have one at 24 one at 36, etc.
- TX1 and TX2 should be closer to the microcontroller. For example, TX1 you have long traces traveling to the left, what you can do is move TX1 into the space to the left of the chip, so the traces will be a lot shorter.
- I would put your name and date on the PCB as well on the silkscreen, if you ever want to show someone.

[mariush]

The board's a bit of a mess...
Get your oscillators closer to the ICs ... get your capacitors closer to the oscillators/crystals.
I'd leave space to lay the 32kHz crystal flat on the board... maybe solder it to a third pad with a bit of solder, or have a loop of wire keep it from vibrating or hitting the board.
careful with 1117 regulators.... some are unstable if the output capacitance has too low ESR ... some 1117 linear regulators require ESR on output between 0.1 and 1 ohm ... a ceramic capacitor on output will have too low esr... so either add a tiny resistor in series with the output capacitor , something like 0.22... 0.47 ohm or whatever, or just use a regular electrolytic capacitor (ex a 10..100uF 10v electrolytic )
or just use a better linear regulator.
add some decoupling capacitors between vin and ground on your micro ... a 100nf ceramic (0.01uF)
200 ohm is kinda non standard value... no need for such value for a status led... i'd say just use 330 ohm or even 470 ohm... more common value.
I wouldn't use surface mounted electrolytics (c9)... i'd suggest plain boring through hole, or polymer surface mount