KICAD TUTORIAL Make Your First Printed Circuit Board
In this KiCad tutorial for beginners, you'll learn to make your first Printed Circuit Board (PCB). You'll get simple step-by-step instructions on how to draw schematics, board layout, and getting your board made cheaply.
When I started building circuits as a teenager, I used different types of prototyping boards. I only built circuits with few components because of all the wires I had to solder here and there to get it working.
I remember finding cool projects with circuit diagrams included. Like guitar effect pedals. Or DIY weather stations. And I really wanted to build them.
But all of them needed at least 20-30 components. Usually much more. So I didn’t dare to try as I knew that I would end up with a big mess of wires, almost impossible to troubleshoot. And even if I’d be able to do it, I’d be afraid to use it in real life in case I would mess something up.
It wasn’t until my early twenties that I first tried to design my own custom Printed Circuit Board (PCB). And after that, I was hooked! The number of components for a project wasn’t a problem anymore. I felt I could build anything!
When you design your own custom PCB, you’ll draw the connections in peace and quiet on your computer. You can double and triple check your connections easily. You even get help from the design program to check for errors.
Next, you can get a few copies of your board made for just a few bucks.
Now you have a board in hand that you know have all the correct connections. No wires needed. All you need to do is to solder the components to the board, just like a soldering kit, and your circuit should work.
In this kicad tutorial, you’ll learn how to make your first PCB. I’ll show you by creating a super simple project in KiCad. After you’ve done one project, you’ll know the basics and can design more PCBs on your own.
But if you want more instructions, more projects to try, and a place to ask questions and discuss electronics projects – I also invite you to check out my electronics community Ohmify:
There are several software alternatives for designing PCBs. KiCad is a free and really good alternative. It’s used extensively by both hobbyists and professionals. That’s what we’ll use in this tutorial.
KiCad is available for Windows, macOS, Ubuntu, and many other platforms. Find the platform alternatives and download the installation files for KiCad here:
When you open up KiCad, you’ll see the window shown in Image 2.1. From here, you can open or create new projects.
To create a new project, click on the File menu and select New -> Project.
Choose where you want to save your project and type in a name for it. Then click on the Save button.
Image 2.1 The main KiCad window
Your new project will be empty. It’s now your job to first create a schematic, then later draw the board layout.
You create the schematic from the Schematic Layout Editor, also called Eeschema.
Open the editor by double-clicking on the schematic file on the left, or by clicking on the Schematic Layout Editor button (Image 2.2).
Image 2.2 Schematic layout editor button
When opening the editor for the first time, you might get asked to Configure the Global Symbol Library Table.
Just choose the recommended settings.
NOTE: If the recommended option is disabled, it most likely means
that you installed KiCad without the default libraries. In that case, you need to download and install the libraries manually. Learn more about that here: https://forum.kicad.info/t/library-management-in- kicad-version-5/14636
Your schematic is where you draw your circuit. First, you add the components you want. Then you add wires to show how to connect your components.
To add a component, click on the Place Symbol button on the toolbar on the right (or press A on your keyboard), then click anywhere in your work area. This brings up the component chooser.
Image 3.1 The place symbol button
From the component chooser, you can search for the component you want to add. Just type in what you’re looking for. For example, if you need a resistor, type in “resistor.” Look through the list of results and choose a good match *.
* What is a good match?
The most important thing is that you choose a symbol that represents the component you want to use in the best way possible.
For example, when you search for “resistor,” you’ll get several options like “thermistor,” “trimmable resistor,” and such. But you also get a symbol that is just a resistor, nothing more. So that’s the best representation.
Image 3.2 The component chooser window
Place the symbol
When you’ve chosen a component, place it in your schematic by clicking in your work area with your mouse.
If you later want to move the component, place your mouse pointer over it and press M on your keyboard. To rotate the component, press R. You can zoom in and out by using your mouse wheel – or F1 and F2 on your keyboard.
Image 3.3 A resistor, LED, and battery added to the schematic
Action Points:
Add a resistor, an LED, and a battery to your schematic
Move the components so that they are positioned the same way as in Image 3.3
Now you need to draw wires between the components to connect them. You can do this by clicking on the Place Wire button on the toolbar – or by pressing W on your keyboard.
Image 4.1 The Add Wire Button
Click on the pin of a component to start drawing a wire. Then click again on the pin where you want the wire to end.
Image 4.2 The components with wires connecting them
If you want to move a component now that they are connected, you have two options: Move and Drag
If you place your mouse pointer over a component and press M on your keyboard, you Move the component without the wires. But if you press G, you Drag the component with the wires attached.
If you start moving or dragging a component but then change your mind, just press the Escape key on your keyboard to release.
Action Points:
Draw wires between the components so that you connect them like in Image 4.2
Test out the two methods of moving a component (Move and Drag) after you’ve connected them
In most cases, a component should have a value. For example, a resistor should have a resistance value. A battery should have a voltage value, etc.
By pressing V on your keyboard, with your mouse pointer over the component, you can edit its value. You also find this option in the menu when right-clicking on the component.
Image 5.1 The window for editing the component value
To set a resistor value to 470 Ω, you’d normally write “470”. And to set the battery value to 9 volts, it’s normal to write “9V”. For the LED you could, for example, write “2V RED” or something similar to indicate that you want to use a red LED with 2V forward voltage.
Note that the value you set for a component does nothing to your circuit. It just serves as a reminder for you, so that you’ll remember what value to use when you build the circuit.
The next step is to Annotate your schematic, which means to give the components a unique identifier. For example, if you have several resistors, they will be named R1, R2, R3, and so on.
To do this, click on the Tools menu, then choose Annotate Schematic.
Leave the default options and click on the Annotate button. Then close the window.
Now you can see that the components have numbers: BT1, R1, and D1.
Before you can move on to drawing your board, there is one more thing you need to do; add footprints to your components.
The footprint is what will be printed onto the board for each component.
For example, for a through-hole resistor, you’ll choose a footprint with two holes, so that you’ll get two holes for soldering the resistor onto on your board.
Click on the Tools menu and choose Assign footprints…
Sometimes it takes a bit of time to load all the libraries, so be patient.
Image 7.1 The footprint selector
Image 7.1 shows the footprint selector. On the left side, you see all the footprint libraries you have available. In the middle, you have the components from your schematic. And on the right, you have a list of footprint options to choose from.
To see what a footprint looks like, right-click on it and select View Footprint.
Image 7.2 An example of a footprint for a resistor. The yellow circles represent holes.
Filters help you narrow it down
There are a lot of footprints in KiCad.
But on the toolbar, you have filters to choose from to help you narrow down your options:
Image 7.3 The Footprint Filter Selector
If you filter by pin count you’ll only see footprints that have the same number of pins as your component.
If you filter by library you’ll only see footprints from the library that you have selected on the left.
The schematic symbol footprint filter will filter based on filtering rules set by the symbol.
What footprint to choose for the battery?
There are many ways to connect a battery. You can use a battery holder that’s fixed onto the board. You can use a barrel connector. Or how about two pins?
For 9V batteries though, I prefer using a battery clip. It’s a clip you fasten to the top of the battery that has two wires going from it.
Image 7.4 A battery clip for connecting 9V batteries
Such a clip doesn’t exist in KiCad at the time of writing. But all you need is a couple of holes where you can solder the wires from the clip. If you add a pin header with two pins, the footprint will be two holes.
You can find pin headers for example in the Connector_ PinHeader_2.54mm library.
There are a few options here. Have a look at a couple of them by right-clicking and choosing View Footprint. Then click on the 3D Display button to see what it looks like in 3D.
Remember that it doesn’t matter which one you choose, as long as it adds two holes to your board. Double-click a footprint to choose it.
What footprint to choose for the resistor?
You’ll find two resistor libraries among the standard KiCad libraries: Resistor_THT and Resistor_SMD.
THT stands for Through-Hole Technology. That’s the type of component where you put the legs into holes on the board and solder on the other side as shown in Image 7.5. It’s the classic type of component, often used by hobbyists as it’s a bit simpler to solder.
Image 7.5 Through Hole Technology (THT)
SMD stands for Surface Mount Device. That’s the type of component that lies on top of the board. You solder them on the same side, as shown in Image 7.6. SMD is the standard component type for modern electronics. They are smaller and take up less space.
Image 7.6 Surface Mounted Device (SMD)
For this circuit, let’s use Through-Hole Components, so select the Resistor_THT library.
There are tons of options. But note that it’s not very important which option you choose here. All of them will give you two holes on the board to solder your resistor into.
But if you want the perfect fit, measure the resistor you plan to use – or look at its size specification from the store where you plan to buy it. Then choose the closest match you can find.
What footprint to choose for the LED?
The last component is the LED. Choose the LED_THT library to add a through-hole LED.
A typical LED is 5mm in diameter. There are many 5mm options in the library. A lot of them have the same footprint but different 3D models. Have a look at the 3D version of a couple of them to get an idea of the difference. (Right-click and select View Footprint. Then click on the 3D Display button.)
Double-click to choose one. You can see my footprint selections in Image 7.7.
Image 7.7 My footprint selections for this circuit
Action Points:
Add footprints for the resistor, the LED, and the battery. See image 7.7 for my selections
It’s easy to make errors, like forgetting to connect a component. Especially when you are drawing large circuits. To help you find these errors, use the tool Electrical Rules Check (ERC).
Click on the Inspect menu and choose Electrical Rules Check. Or click on the Perform Electrical Rules Check button shown in Image 8.1.
Image 8.1 The Perform Electrical Rules check button
In the window that pops up, click on the Run button and look for error messages under Error List.
A typical error here is if you forgot to connect the pin of a component to another component. Or if you accidentally moved a component so that it’s no longer connected.
Image 8.2 The Electrical Rules Checker window
If there are no errors, you’ve finished the first phase of drawing the schematic. You can move on to the second phase – designing your board.
That’s it for drawing the schematic. To make it easier for your next design, here’s a checklist with all the action points you need to take before moving on to the board design:
Add all components to your schematic
Connect all components with wires
Add values to all components
Annotate your schematic
Add footprints to all components
Run the Electrical Rules Checker (ERC) and fix any errors
You have defined how you want to connect the components in the schematic editor, and now it’s time to put that onto your board. You need to decide where to place the components, then draw tracks to create the connections between them.
To start drawing your board layout (assuming you’re still in the Schematics Editor), click on the toolbar button that says Run Pcbnew to layout printed circuit board, as shown in Image 10.1. Or go to the Tools menu and select Open PCB Editor. This opens up the Board Editor window.
Image 10.1 The button to go from schematic design to board layout
The first thing you’ll see is just an empty area.
To get started, you need to retrieve information about footprints and connections from your schematic. You can do this by clicking on the toolbar button that says Update PCB from schematic… as shown in Image 10.2. You’ll also find this option in the Tools menu.
Image 10.2 The button to update PCB from schematic
A window will pop up.
Keep the default options and click on the Update PCB button. This will load your footprints. Then click on the Close button.
Click anywhere to place the components.
If you zoom in on the components, using either your mouse-wheel or F1/F2, you’ll see white straight lines between the pins. These are called air-wires and tell you which pins to connect – according to your schematic.
Image 10.3 The components imported from the schematic
Action Points:
Update your PCB from schematic, so that you see the three footprints you’ve chosen
Your next task is to position your components so that it becomes easy to connect the components according to your air-wires. If you’re able to place the components in a way that no air-wires cross, that’s the easiest.
I recommend positioning the components like the way you did in the schematic, if possible. It’s not very important for such a simple board, but for more complicated boards it can simplify troubleshooting.
To move a component, move your mouse over it and press M. If you already have a group selected, the whole group will move. To deselect the group, press ESCAPE. To rotate a component, press R.
If you accidentally place your mouse over the component name, you’ll move only the name. Just press ESCAPE to try again.
Image 11.1 The components placed so that no air-wires cross
Action Points:
Place the components in an orderly way, similar to the way you placed them in your schematic diagram
When you’re happy with the placement, the next step is to replace the air-wires by drawing tracks to connect the components. The tracks you draw will become copper traces on your finished board.
Start drawing tracks by clicking on the Route Tracks button on the toolbar on the right (shown in Image 12.1) – or press X on your keyboard.
Image 12.1 The button for routing tracks
You can choose if you want to draw on the front or the back of the board, by selecting a layer in the Layer Manager. The little blue triangle on the left shows the selected layer.
F.CU is the front (or top) side.
B.CU is the back (or bottom) side.
Image 12.2 The layers manager
Click at the beginning of an air-wire to start drawing a track. Click again where the air-wire ends to finish drawing the track.
When there are no more white lines, you’re done routing the tracks.
Image 12.3 The board with all its tracks routed
Action Points:
Draw all the tracks so that you have no more air-wires left
To check if you’ve made any errors, you need to run the Design Rules Checker – also called the DRC. Typical errors are placing two components too close to each other, or forgetting to draw a track.
Image 14.1 The button for running the Design Rules Checker (DRC)
Select the Edge.Cuts layer.
Click on the Design Rules Checker button, shown in Image 14.1, or find it under the Inspect menu. Leave the default options and click on Run DRC button.
Check both the Problems tab and the Unconnected Items tab. The Problems tab will list any design issues, such as a track being too close to another track. The Unconnected Items tab will list any air-wires that you have not yet connected by drawing a track.
Image 14.2 The Design Rules Checker window without any errors
If you see any items on any of these tabs, make sure you fix them before moving on.
If you have a lot of errors, do not despair. Often one little mistake can result in lots of messages. Just focus on one message and try to figure out what it says. Then fix it and run the DRC again.
When you have zero errors listed here, you are done. Your board is finished!
Click on the View menu and select 3D Viewer to see your finished board.
Image 14.3 3D view of the finished board
Action Points:
Run the Design Rules Checker (DRC) and fix any errors that you might have
That’s it for drawing the board layout. To make it easier for your next design, here’s a checklist for all the action points you need to take to complete the board design:
Open the Board Layout Editor and run Update PCB from schematic
Place your components in an orderly way
Draw all the tracks so that you have no more air-wires left
Create your board edges by adding a polygon in the Edge. Cuts layer that encloses all your components and tracks
Run the Design Rules Checker (DRC) and fix any errors that you might have
You’re now ready to get your board made. This is something that many think is hard and expensive. But that couldn’t be farther from the truth!
These days, PCB manufacturing is available at low cost to anyone who wants to get their circuit boards made. You can find companies that will make a few copies of your boards for only $5-10 (USD).
And it’s become so easy to order that even the most computer-challenged among us can do it.
Image 16.1 The finished board from Make Your First PCB at https://ohmify.com
The Easiest Way
The US manufacturer OSH Park allows you to drag and drop your KiCad PCB file onto their website. That’s it! They process the file in real-time and show you the details of your board so that you can double-check for errors.
Check the file, make the payment, then all you need to do is to sit back and let them make the board for you. The whole process takes less than 5 minutes.
I think we’ll see more manufacturers offering this in the future.
Congratulations, you’ve made it to the end! I really hope this has been helpful. If you have any questions, doubts or feedback, please let me know in the comment section below.
PS! KiCad is constantly being improved upon. Screenshots, library names, or other things from this KiCad tutorial might change over time. If you see something that is no longer as explained in this tutorial, please let me know!
Hey, I’m Oyvind Dahl and I run an electronics membership site for people like you to get really good at building electronics projects. Everything is explained in simple ways and my students learn by doing – not by being swamped with complicated jargon and maths.
I need info on creating a schematic symbol. The instructions/tutorial supplied does not match the current version of software so I have finally hit an impasse trying to figure out how to do it. Help?
Thanks for this tutorial! Recent grad firmware/software engineer here, thought I'd try to fix up my weakness in the hardware area. This was a great tutorial for quickly getting the broad strokes of schematic capture and PCB layout, and a good intro to KiCad.
When designing the PCB layout at the stage with the red and green traces, why is the trace connecting the LED and the battery on the bottom of the board instead of the top like the other traces?
I would really like some help in building a capacitor circuit for a dpdt switch on a guitar preamp. I have no experience in electronics so I don't know my head from my toe here. Can you help?
I do have an example to show you if you wouldn't mind looking at it.
I downloaded different version of KiCad 5 and plus several times , but each time it doesn t include default foot print table and won't let me let me import it by different paths!
Can anybody direct me to any full version download that include the default symbol table please?
You can download the complete version of KiCad here:
https://kicad-pcb.org/download/
If you're having problems with the libraries I recommend you explain your problem in the KiCad forum and you'll likely get some help:
https://forum.kicad.info/
It sounds like you're not able to complete the polygon when drawing edge cut. Try zooming in for the last point. It's important to end the polygon exactly where you started it.
I annotated all my board couponents except caps and one resistor wont accept foot print after different footprint assignments?
Any guideline direction ? Thanks
Tough , I updated the library, but the caps and resistor wont accept footprint assignment after different ..
I got stuck at the footprint assignment step...
Any help gays?
After runing Electrical Rule Check , it shows an error some circuit connection in the schematic and how to fix it by using" Power Flag tool " ?!
How this tool repairs the above circuit disconnection and make the schematic ready for the following steps?
The Power Flag tells the schematic what it is that powers the circuit. For example if you've added a connector that you plan to connect power to, you might need to explicitly add the power flag to the supply lines of the connector.
Thanks for make it simple and clear for beginners.
Except for some steps : if u can explain the DRC of some errors fix like
POWER FLAG ? how it can fix the power pin connection of vac or vdc terminal disconnection errors for ex.?
I did used it to clear errors on my project but didn t understand how?
Second question, I couldn t find in the library some couponents like one package bridge rectifier for ex.? How to foot print a transformer on the schematic ?
Would ad some clearance ,thanks
Thanks for sharing excellent informations. Your website is so cool. I am impressed by the details that you have on this website. It reveals how nicely you perceive this subject. Bookmarked this web page, will come back for extra articles. You, my pal, ROCK! I found simply the info I already searched all over the place and simply couldn’t come across. What a great web-site.
I've been struggling to learn KiCad for months! I'm really glad I found your website, this tutorial breaks it down and makes it real simple and understandable. Gives me a solid foundation to build my KiCad experience and skill on. One question though, It looks like KiCad supports running simulations of circuits, can it output things like simulated oscilloscope readings, multimeter type readings at various test points, etc?
Hi,
How can I tell KiCad to place a straightforward hole? I want to mount a potentiometer on the board with the shaft perpendicular to the board surface. I could place a pad and then open up the hole, but it would be better to specify a plain hole with no pth.
Regards
Keith
Normally, you'll choose a component with the footprint that matches your component so that all the holes you need appear automatically.
But if you're in the PCB editor and just want to add a hole, you can do that by choosing Place->Footprint, then choosing a footprint that is just a hole.
If the hole isn't the correct size, you can customize it via it's properties after having added it.
Useful tutorial - but what about if (like me), you want to make the board yourself?
By this I mean by taking a print of the PCB layout in order that the pattern can be transferred to a copper laminate board?
It would be nice for the above to have been included, as the method would have captured an audience for those who are already conversant with the process of track transference and etching etc?
Thank you for this incredibly helpful tutorial! It truly has everything and more that a beginner needs to get thru first project. More over, it's very detailed in all necessary steps to accomplish that and written in easy-to-understand language. The examples in the tutorial put a cherry on 'the cake'. Really outstanding help.
Jan
Ground and power fills/planes?
Hi Pb, Are you asking how to do it? Or are you suggesting it should be added?
Best,
Oyvind
I need info on creating a schematic symbol. The instructions/tutorial supplied does not match the current version of software so I have finally hit an impasse trying to figure out how to do it. Help?
Here's how to edit a symbol: https://www.build-electronic-circuits.com/how-to-edit-symbol-in-kicad/
Hi Oyvind,
Thanks for this tutorial! Recent grad firmware/software engineer here, thought I'd try to fix up my weakness in the hardware area. This was a great tutorial for quickly getting the broad strokes of schematic capture and PCB layout, and a good intro to KiCad.
Will check out Ohmify!
Hi Huan, glad to hear!
When designing the PCB layout at the stage with the red and green traces, why is the trace connecting the LED and the battery on the bottom of the board instead of the top like the other traces?
Thanks!
Hi Jonathan!
It's just to show that you can draw the traces on both sides. It could just as well have been on the top like the other ones.
Best,
Oyvind
I would really like some help in building a capacitor circuit for a dpdt switch on a guitar preamp. I have no experience in electronics so I don't know my head from my toe here. Can you help?
I do have an example to show you if you wouldn't mind looking at it.
Hi Kohl,
Could you post a link to the schematics and what you are struggling with?
I downloaded different version of KiCad 5 and plus several times , but each time it doesn t include default foot print table and won't let me let me import it by different paths!
Can anybody direct me to any full version download that include the default symbol table please?
You can download the complete version of KiCad here:
https://kicad-pcb.org/download/
If you're having problems with the libraries I recommend you explain your problem in the KiCad forum and you'll likely get some help:
https://forum.kicad.info/
Hi Oyvind,
Thanks for a well written, easy to follow tutorial. I will shortly be embarking on my first PCB design.
Cheers!
Ravi
Great to hear! =)
i have a footprint and interconnect layout for front copper. i can't do edge cut.
it's SMT, no holes. polygon won't stay. esc makes it go away....
It sounds like you're not able to complete the polygon when drawing edge cut. Try zooming in for the last point. It's important to end the polygon exactly where you started it.
I annotated all my board couponents except caps and one resistor wont accept foot print after different footprint assignments?
Any guideline direction ? Thanks
Hi Ahmed, you won't be able to set footprints until you have annotated all components.
Tough , I updated the library, but the caps and resistor wont accept footprint assignment after different ..
I got stuck at the footprint assignment step...
Any help gays?
Have you annotated all the components? If yes, please let me know what the error says.
After runing Electrical Rule Check , it shows an error some circuit connection in the schematic and how to fix it by using" Power Flag tool " ?!
How this tool repairs the above circuit disconnection and make the schematic ready for the following steps?
The Power Flag tells the schematic what it is that powers the circuit. For example if you've added a connector that you plan to connect power to, you might need to explicitly add the power flag to the supply lines of the connector.
Thanks for make it simple and clear for beginners.
Except for some steps : if u can explain the DRC of some errors fix like
POWER FLAG ? how it can fix the power pin connection of vac or vdc terminal disconnection errors for ex.?
I did used it to clear errors on my project but didn t understand how?
Second question, I couldn t find in the library some couponents like one package bridge rectifier for ex.? How to foot print a transformer on the schematic ?
Would ad some clearance ,thanks
Thank you very much for your tutorial, that's very helpful to understand the basics, and workflow. Cheers
Thank you for this perfectly written guide. I just have to close other browsing tabs I opened for this same purpose.
Keep up the good work, bro.
I hope to see more tutorials on autorouting and creating mounting holes. Thanks.
Thank you for your guide. It is helpfull for me.
Thanks for walking me through this.
It's not particularly intuitive, but OK when you get used to it!
Best wishes.
i really enjoy this thank
Thanks for sharing excellent informations. Your website is so cool. I am impressed by the details that you have on this website. It reveals how nicely you perceive this subject. Bookmarked this web page, will come back for extra articles. You, my pal, ROCK! I found simply the info I already searched all over the place and simply couldn’t come across. What a great web-site.
Poker88 menawarkan pilihan game judi online terlengkap dan terbaik.
I've been struggling to learn KiCad for months! I'm really glad I found your website, this tutorial breaks it down and makes it real simple and understandable. Gives me a solid foundation to build my KiCad experience and skill on. One question though, It looks like KiCad supports running simulations of circuits, can it output things like simulated oscilloscope readings, multimeter type readings at various test points, etc?
Great=) Yes, that should be possible as far as I know.
Hi,
How can I tell KiCad to place a straightforward hole? I want to mount a potentiometer on the board with the shaft perpendicular to the board surface. I could place a pad and then open up the hole, but it would be better to specify a plain hole with no pth.
Regards
Keith
Normally, you'll choose a component with the footprint that matches your component so that all the holes you need appear automatically.
But if you're in the PCB editor and just want to add a hole, you can do that by choosing Place->Footprint, then choosing a footprint that is just a hole.
If the hole isn't the correct size, you can customize it via it's properties after having added it.
Greetings;
Useful tutorial - but what about if (like me), you want to make the board yourself?
By this I mean by taking a print of the PCB layout in order that the pattern can be transferred to a copper laminate board?
It would be nice for the above to have been included, as the method would have captured an audience for those who are already conversant with the process of track transference and etching etc?
Good point! I'll add some info about that when I get to it.
Thank you for this incredibly helpful tutorial! It truly has everything and more that a beginner needs to get thru first project. More over, it's very detailed in all necessary steps to accomplish that and written in easy-to-understand language. The examples in the tutorial put a cherry on 'the cake'. Really outstanding help.
Jan