Tutorial: How to Design Your Own Custom STM32 Microcontroller Board – Part 1

Article Technical Rating: 7 out of 10

This is the first in a series of tutorials where you’ll learn how to design your own custom microcontroller board. To get the most out of this tutorial it’s critical that you read the article and watch the included video.

Initially, we’re going to focus on just the microcontroller itself so you can more easily understand the design process without getting overwhelmed with circuit complexity.

I’ll break down the design process into three fundamental steps:

STEP 1 – System Design
STEP 2 – Schematic Circuit Design
STEP 3 – PCB Layout Design

You’re going to learn how to design the system and the schematic circuit in this first tutorial. Then, in part two you’ll learn how to lay out the Printed Circuit Board (PCB) and order prototypes.

This will be an ongoing tutorial series and in the future we’ll greatly expand the capabilities of the design by adding advanced features such as: a rechargeable battery, a display, Bluetooth, WiFi, USB data, GPS, and an accelerometer.

NOTE: This is a long, very detailed tutorial so here's a free PDF version of part 1.



System / Preliminary Design

When developing a new circuit design the first step is the high-level system design (which I also call a preliminary design). Before getting into the details of the full schematic circuit design it’s always best to first focus on the big picture of the full system.

Designing the system consists mainly of two steps: creating a block diagram and selecting all of the critical components (microchips, sensors, displays, etc.). A system design treats each function as a black box

In engineering, a black box is an object which can be viewed in terms of its inputs and outputs but without any knowledge of its internal workings. With a system-level design the focus is on the higher level interconnectivity and functionality.

Block Diagram

Below is the block diagram that we’ll be working from in this tutorial series. As I mentioned, for this first tutorial we’ll focus just on the microcontroller itself. In future tutorials we’ll expand the design to include all of the functionality shown in this block diagram.

A block diagram should include a block for each core function, the interconnections between the various blocks, specified communication protocols, and any known voltage levels (input supply voltage, battery voltage, etc.).

Later, once all of the components have been selected and the required supply voltages are known I like to add the supply voltages to the block diagram. Including the supply voltage for each functional block it allows you to easily identify all of the supply voltages you’ll need as well as any level shifters.

In most cases when two electronic components communicate they need to use the same supply voltage. If they are supplied from different voltages then you’ll usually need to add in a level shifter.

Block Diagram

Figure 1 – System-level block diagram. Blocks in yellow are included in this initial tutorial. Other blocks/functions will be added in future tutorials.


Now that we have a block diagram we can better understand the necessary requirements for the microcontroller. Until you’ve mapped out everything that will connect to the microcontroller it’s impossible to select the appropriate microcontroller.

Select Microcontroller

When selecting a microcontroller (or just about any electronic component) I like to use an electronics distributor’s website like Newark.com. Doing so allows you to easily compare various options based on a variety of specifications, pricing, and availability. It’s also an easy way to quickly access the component’s datasheet.

If you regularly read this blog you’ll know that I’m a big fan of ARM Cortex-M microcontrollers. Arm Cortex-M microcontrollers are easily the most popular line of microcontrollers used in commercial electronic products. They have been used in tens of billions of devices.

Microcontrollers from Microchip (including Atmel) may dominate the maker market but Arm dominates the commercial product market.

Arm doesn’t actually manufacture the chips directly themselves. They instead design processor architectures that are then licensed and manufactured by other chip makers including ST, NXP, Microchip, Texas Instruments, Silicon Labs, Cypress, and Nordic.

The ARM Cortex-M is a 32-bit architecture that is fantastic choice for more computationally intensive tasks compared to what is available from older 8 bit microcontrollers such as the 8051, PIC, and AVR cores.

Arm microcontrollers come in various performance levels including the Cortex-M0, M0+, M1, M3, M4, and M7. Some versions are available with a Floating Point Unit (FPU) and are designated with an F in the model number such as the Cortex-M4F.

One of the biggest advantages of Arm Cortex-M processors is their low price for the level of performance you get. In fact, even if an 8-bit microcontroller is sufficient for your application you should still consider a 32-bit Cortex-M microcontroller.

There are Cortex-M microcontrollers available with very comparable pricing to some of the older 8-bit chips. Basing your design on a 32-bit microcontroller gives you more room to grow should you want to add additional features in the future.

STM32 Microcontroller

Figure 2: The STM32 from ST Microelectronics is my favorite line of ARM Cortex-M microcontrollers.


Although numerous chip makers offer Cortex-M microcontrollers, my favorite by far is the STM32 series from ST Microelectronics. The STM32 line of microcontrollers is quite expansive with just about any feature and level of performance you would ever need. The STM32 line can be broken down into several subseries as shown in Table 1 below.

STM32 Series


Max clock (MHz)

Performance (DMIPS)













































Table 1: Comparison of various STM32 microcontroller variants


The STM32F subseries is their standard line of microcontrollers (versus the STM32L subseries which is specifically focused on lower power consumption). The STM32F0 has the lowest price but also the lowest performance. One step up in performance is the F1 subseries, followed by the F3, F2, F4, F7, and finally the H7.

For this tutorial I have selected the STM32F042K6T7 which comes in a 32-pin LQFP leaded package. I selected a leaded package primarily because it simplifies the debugging process because you have easy access to the microcontroller pins. Whereas with a leadless package, like a QFN, the pins are hidden away underneath the package making access impossible without test points.

A leaded package also allows you to more easily swap out the microcontroller if it were to become damaged. Finally, leadless packages cost more to solder on to the PCB so they increase both the prototyping and manufacturing costs.

I selected the STM32F042 because it offers moderate performance, a good number of GPIO pins, and various serial protocols including UART, I2C, SPI and USB. This is a fairly entry-level STM32 microcontroller with only 32 pins, but with a wide variety of features. More advanced versions come with as many as 216 pins which would be quite overwhelming for an introductory tutorial.

In this first video we won’t be using most of these features, but we will take advantage of them in future videos in this series.

Schematic Circuit Design


Schematic circuit diagram for microcontroller circuit

Figure 3: Schematic circuit diagram for this first tutorial showing the STM32 microcontroller, linear regulator, USB connector, and programming connector.


Now that we have selected the microcontroller it’s time to design the schematic circuit diagram. For these tutorials I’ll be using a PCB design tool called DipTrace.

There are dozens of PCB tools available but when it comes to ease of use, price, and performance I find that DipTrace is hard to beat, especially for beginners.

If you don’t have a PCB design package then you may want to consider downloading the free version of DipTrace so you can follow along closely with this tutorial. The best way to learn something is always to actually do it.

For this initial tutorial the free version of DipTrace is sufficient, but as we expand the functionality of this circuit in future tutorials you’ll need to upgrade to a paid version of DipTrace or their 30-day free trial.

DISCLOSURE: I’m an affiliate for DipTrace, but only after I used it to successfully design dozens of products. I’ve been using it now for almost 4 years, and I still love it. If you do decide to purchase DipTrace, I would really appreciate it if you would use this link so I get a commission at no extra cost to you.

Nonetheless, this tutorial will be focusing on the process for designing a custom microcontroller board, and not on how to use any specific PCB design tool. So regardless of which PCB software you end up using you’ll still find these tutorials are just as useful.

The first step in designing a schematic is to place all of the key components. For this initial design this includes the microcontroller chip, a voltage regulator, a microUSB connector, and a programming connector.

For more complex designs it usually makes more sense to completely design each sub-circuit first, then merge them all together. Depending on the design complexity (and personal preference) you may also want to place each sub-circuit on its own separate sheet. This keeps the schematic from becoming a huge, overwhelming monster on a single sheet.


Next, we’ll place all of the various capacitors. For the most part you can think of capacitors as tiny little rechargeable batteries that hold electrical charge and help to stabilize the voltage on a supply line.

We’ll start by placing a 4.7uF capacitor on the input pin of the linear regulator. This is the 5VDC input voltage supplied by an external USB charger. This voltage is fed into a TLV70233 linear regulator which steps the voltage down to 3.3V since the microcontroller can only be supplied by a maximum of 3.6V.

Another 4.7uF capacitor is placed on the output of the regulator as close to the pin as possible. This capacitor serves to store charge to supply transient loads and it acts to stabilize the internal feedback loop of the regulator. Without an output capacitor most regulators will begin to oscillate.

Decoupling capacitors must be placed as close as possible to the microcontroller supply pins (VDD). It’s always best to refer to the microcontroller datasheet in regards to their recommendations for decoupling capacitors.

The datasheet for the STM32F042 recommends a 4.7uF and a 100nF capacitor be placed next to each of the two VDD pins (input supply pins). It also recommends 1uF and 10nF decoupling capacitors be placed near the VDDA pin.

The VDDA pin is the supply for the internal analog-to-digital (ADC) converter and must be especially clean and stable. We’re not using the ADC in this first tutorial but we will in a future one.

Note that you’ll commonly see two capacitor sizes specified together for decoupling purposes. For example, 4.7uF and 100nF capacitors.

The larger 4.7uF can store more charge which helps stabilize the voltage when large spikes in load current are required. The smaller capacitor serves mainly to filter out any high-frequency noise.

Microcontroller pinout

Although the STM32F042 offers a wide variety of functions such as UART, I2C, SPI, and USB communication interfaces, you won’t find any of these functions labeled on the microcontroller pinout. This is because most microcontrollers assign a variety of functions to each pin so as to reduce the number of pins required.

Figure 4: Pinout for the STM32F042 microcontroller in a 32-pin LQFP leaded package.


For example, on the STM32F042 pin 9 is labeled as PA3 which means it is a GPIO pin. Upon startup this function is automatically assigned to this pin. But it also has alternative functions that can be specified in the firmware program.

Pin 9 can be programmed to serve the following functions: receive input pin for UART serial communication, an input to the Analog-to-Digital Converter (ADC), a timer output, or an I/O pin for the capacitive touch sensor controller.

Refer to the pin definition table in the microcontroller datasheet (page 33 for the STM32F042) which shows all of the various functions available for each pin. Always be sure to confirm that two functions required for your product don’t overlap on the same pins.


All microcontrollers require a clock for timing purposes. This clock is just an accurate oscillator. Microcontrollers execute programmed commands sequentially with each tick of the clock.

The simplest option, if available on the selected microcontroller, is to use the internal clock. This internal clock is known as an RC oscillator clock because it uses the timing characteristics of a resistor and capacitor.

The major downside to an RC oscillator is accuracy. Resistors and capacitors (especially those embedded inside a microchip) vary significantly from unit to unit causing the oscillator frequency to vary. Temperature also significantly impacts the accuracy.

An RC oscillator is fine for simple applications, but if your application requires accurate timing then it won’t be sufficient. For this initial tutorial we’re going to use the internal RC clock to keep things simple. In future tutorials we’ll improve the design by adding a much more precise, external crystal-based oscillator.

Programming Connector

Programming an STM32 is done via one of two protocols: JTAG or Serial Wire Debug (SWD). More advanced versions of the STM32 (STM32F1 and higher) offer both JTAG and SWD programming interfaces. The STM32F0 subseries offers only the simpler SWD programming interface so that is what we will focus on for this tutorial.

The SWD interface requires only 5 pins. They are SWDIO (data input/output), SWCLK (clock signal), NRST (reset signal), VDD (supply voltage) and ground.

Unfortunately the ST-LINK programmer device that you’ll use to program the STM32 uses a 20-pin JTAG connector (with SWD functionality). This connector is quite large and is not practical for smaller board designs.

Instead, you can use a 20-pin to 10-pin adapter board such as this one from Adafruit so you can use a smaller 10-pin connector on your board.

For this tutorial we will use the 10-pin connector. If that is still too large for your project then you can always use a 5-pin header and jumper wires from the 20-pin programmer output to connect only the 5 lines required for SWD programming.


The last part of the schematic we’ll cover is the power section. The STM32 microcontroller can be powered with a supply voltage from 2.0 to 3.6V. Unless you have a variable power supply, you’ll need an on-board regulator to provide the appropriate supply voltage.

For this design we’ll power the board using an external USB charger which outputs 5 VDC. This voltage will then feed into a linear voltage regulator (TLV70233 from Texas Instruments) which steps it down to a stable 3.3V.

The STM32 requires a maximum of only 24mA assuming none of the GPIO pins are sourcing any current (each GPIO pin can source up to 25mA). The absolute maximum current the STM32 will ever require is 120mA assuming various GPIO pins are sourcing current.

The TLV70233 is rated for up to 300mA which should be more than sufficient for this initial design. In future tutorials, as we add additional functions, we may need to revisit this to ensure the regulator can handle the required system current.

Electrical Rules Check

The final step of designing the schematic circuit diagram is to perform a verification step called an Electrical Rules Check (ERC). This verification step checks for errors such as shorts between nets, nets with only one pin, superimposed pins, and unconnected pins.

You can also setup various pin type errors. For example, if an output pin is connected to another output you will get an error. Or if an output pin is connected to a power supply line you will get an error. DipTrace uses a colored grid matrix that allows you to define which pin type connections will give you errors or warnings.


In this first tutorial we’ve designed the system block diagram, selected all of the critical components, and designed the full schematic circuit diagram.

In part 2 of this tutorial series we’ll focus on designing the actual printed circuit board (PCB) layout and ordering board prototypes.

Are you ready to discover the smart way to develop a new electronic hardware product? If so then check out the Predictable Hardware Report.

Leave a Reply 37 comments

Kevin Vo Reply

Thank you John for the great content,
When is part 2 and 3 come out?

    John Teel Reply

    Thanks Kevin, I’m glad it was helpful. Part 2 is already published here. I’m not sure yet when part 3 will come out, so please keep checking back in.

paul Reply

Thank you for this article . I am new to micro controllers and found this article very well written and in a language I could understand. After looking at many websites and feeling like I was going in circles and swamped by tech specs and jargon . I found your article and learnt more in 15mins than I had in hours. i like the ground up approach of your tutorials.

    John Teel Reply

    Hi Paul, that is so awesome to hear!! I do enjoy explaining complex topics in a way that people can actually understand. So thank you for this comment.


Brendan Reply

Thank you so much for this tutorial! It’s what my electrical engineering degree program was missing, honestly. Regarding the Power Scheme for “2 x VDD”, I saw it said “2 x 100 nF + 1 4.7 uF”. I think I understand it correctly: there are 2 VDD pins on opposite sides of the chip, they both require a 100 nF and 4.7 uF cap separately. However order of operations (2 x large cap+1 x small cap) and the drawing leave a lot up to interpretation. Can you please clarify how I should read that? Thank you.

    John Teel Reply

    Thank you Brendan, I’m glad it was helpful. On the particular MCU version I’ve used there is one VDD pin and one VDDIO pin (for I/O). Each of those pins should have a 100nF and a 4.7uF capacitor, although if each is tied to the same supply voltage you could also just do a 100nF on each pin and a single 4.7uF that is shared between them. I hope that clarifies your question, if not just let me know.


Vimal Kumar CR Reply

Hi John teel.
Thank you very much for helping all the electronics hungry people around the globe. Your data and articles are a great frame for my startup.

Thank you once again. Gratitude !!

Taofeek Reply

Your articles are always great and light up my Hardware career. Thanks for the great work.
Also I saw a guy that program STM32 directly USB without St link. Also some people program STM32 series with Arduino IDE. Is there any best IDE to program STm. Because I know some people use open system workbench, True studio, Keil etc

Chandra Reply

Thanks John, I have been following your newsletters for a long time. This is a wonderful vlog. Looking forward for more.

    John Teel Reply

    Thank you Chandra, I really appreciate that!

Simon Robb Reply

Thank you for all your hard work John.

I’m so impressed with your content. I come from a software background and started tinkering with hardware about 18 months ago, in order to develop precision agriculture sensors for my (aspiring) startup. It was a slow and – at times – frustrating experience. It seems every paragraph of yours I read, I recognize it as a hard-won lesson from my first six months.

So, well done on so carefully curating these lessons. I would not be at all surprised if this syllabus enables a new wave of makers!

    John Teel Reply

    Thank you so much Simon for your fantastic comment. It always mean so much to hear from those learning from all the hard work I put into creating this content.

    Best wishes,

DApo Reply

Very educative

Stevie Reply

As a beginner to microcontrollers I am finding your articles informative…

Thanks you for helping me to understand the basics of this gigantic topic.

    John Teel Reply

    That’s awesome to hear Stevie! Thank you for the positive feedback, I really appreciate it.

Magnus Olsson Reply

I am at medium beginners level ….and due to English not being my native language some (quite a lot) went over my head in this fast fast video. But I’m learning step by step and it’s always nice to see a pro in action.

Qandeel Reply

Great article !

Santosh Reply

Thanks , I am new to this field , the way u r explaining is really very exciting.Waiting to see ur next tutorial.

Stefano Reksten Reply

Thanks John! I really appreciate all the knowledge you share with us!

    John Teel Reply

    You are welcome, and I truly do enjoy sharing it. Thanks for the comment.


Ruben Tjade Reply

Thank You John, it is really a pleasure again to read your article.
I have really learned so many thing.
I will like to know if all the microcontroller needs a Bootloader to operate like Arduino series?

    John Teel Reply

    Thanks Ruben! Yes, you would need a bootloader to program it via the USB port like an Arduino. In most cases when programming a custom MCU board its best to use the in-circuit programming/debugging port which for the STM32 is either SWD or JTAG. You’ll need an ST-LINK programmer to program via SWD.

Mes Reply

Good one John. It is one of the few Blog/vlogs that I follow regularly. I have two simple questions if possible; 1. Is that ok to mix the two grounds supplies (Analogue and Digital) for mixed signal boards: 2. what do you recommend to use where an IC has two different VDDs like 3V and 1.8V?


    John Teel Reply

    Thank you and that is great to hear!

    1) Yes, ideally you want to keep the digital and analog grounds separate and then connect them together at the ground plane. But for this first simple design this wasn’t necessary, especially since we’re not yet using the Analog-to-Digital Converter. This is something I’ll discuss further in a future tutorial

    2) I’m not quite sure I understand this question. But if you use an IC that requires two supply voltages then you’ll need two regulators (or a single dual-output regulator) to provide those voltages. If the 1.8V supply has to only supply small amounts of current then a linear regulator is best. But if the 1.8V supply has to source high current then a switching regulator is best. Whenever you have a situation where there is high current draw and a big difference in the input voltage to output voltage then a switching regulator will be much more efficient. So if you take a 5V supply and step it down to 1.8V and supply hundreds of milliamps then a switching reg is probably the best choice.

    Okay, I hope I answered your questions. Please let me know if I didn’t and I’ll be happy to try again:)

    Best wishes,

Rob Reply

This is just what we needed! Looking forward to the next installment!

Johan Reply


Jorge Reply

Congratulations!! I think that your newsletter / mail is the only that I always read. You’re not spam. that’s a great compliment!! Keep going!!

    John Teel Reply

    That’s awesome to hear Jorge! Thanks for the comment.


    Nick Reply

    I am really loving your site John. This micro controller series is just what I needed. Thank you and I hope to see more.

    Chris Reply

    The only newsletter I look forward to opening, knowing I’ll get something useful out of it. Thank you for the great content, John!

      John Teel Reply

      Thank you Chris that means a lot to me to hear.


Gabriel Cataldi Reply

Really good!!!

Craig Ross Reply

Enjoyed the tutorial, looking forward to the next two installments!

Leave a Reply:

Predictable Designs LLC, 10645 N. Oracle Rd, Suite 121-117, Oro Valley, AZ 85737 USA
[email protected], Phone: (520) 261-1844 (for fastest repsponse please email instead of call)
Copyright 2018 by Predictable Designs LLC

This website uses cookies. By continuing you consent to the use of cookies and the collection of your IP address. See our privacy policy for more information.