Bad news (for me).
Autodesk's Eagle is the schematic capture/PCB layout application--"Electronics Design Automation" or "EDA"--I've been using forever.
But starting in 2026 Autodesk wants $749 USD a year for a Fusion 360 integrated version--and I confirmed with their sales team: my existing $100/year Eagle/Fusion 360 license is going away.
Time to say goodbye to Eagle.
Say Hello to KiCad.
The guys in my geeky synth meetup group have been telling me to use Kicad for years. Now, everyone will be be happy?
This post captures notes written during my initial exposure to KiCAD 7.
As usual this blog post is my own trail of breadcrumbs. If you are thinking of switching to Kicad from another EDA, or are a Kicad newbie like me, the post may be of some use.
Otherwise, you may want to skip this one.
GET KICAD
$749? Nope. KiCAD is free. Download it here.
I got the Windows version--not sure how transparent going between OS's will be, cross platform compatibility was poorly implemented in Eagle. Kicad docs say it's transparent; no reason to doubt them. I will try opening PC created projects on Linux and Mac down the road. I had no problem installing it on a few Windows 10 systems.
PROJECTS
Eagle and Kicad allow me to create a "project"; I never used projects in Eagle. Instead, I created a folder using my OS and put Eagle schematics and boards in there--as many schematics and PCB files in a single folder as I wanted; it was easy to have many schematic revisions in a single folder as long as each had a unique filename and the correct file extension....it all worked.
KiCAD is different; it is designed around a single project/single schematic/single board paradigm. However, a single schematic can have "subsheets" (details here--I have not tried subsheets yet).
Creating a new Kicad project creates new helper files and folders, so if I want to create a revised PCB for a given project, or create an additional board (a "revision 2.0" for example) I have to:
- Use Windows Explorer to create a new folder
- Copy the original project (.pro), schematic (.sch), and PCB (.pcb) files into the new folder
- Rename the project, PCB, and schematic files to a matching filename (with their original .kicad* extensions intact)
Automating these steps should be easy using something like
Python and
Powershell. I will look around for a script or macro for this. I'd be surprised if someone hasn't already created a utility for spinning off versions of Kicad projects, but so far I can't find it.
Update 5-15-25: Kicad V9 has a "save as" under "file"....which creates a duplicate of the current project. You can see the save as menu item when you open a Kicad project, before you open your schematic or PCB. KICAD LIBRARIES: SYMBOLS AND FOOTPRINTS
Eagle has a devilishly confusing "device/symbol/footprint" paradigm that makes you pick a symbol and footprint while choosing a component for your schematic. Eagle "device libraries" contain all the necessary elements--the symbol, the footprint, and how the two interconnect.
After using Eagle EDA for over 20 years I still find creating and managing custom or modified devices confusing, frustrating, and teeth-gnashingly counterintuitive.
KiCAD is a HUGE improvement--symbols and footprints have their own libraries and each is managed separately. The user has to make sure pins and pads are laid out correctly, but that's the case in Eagle as well.
For a good primer on Kicad symbol creation the video here; footprint creation here. The same ideas are used to modify existing objects as creating new ones. It's easy!
Elton from OtterMods, the resident KiCAD expert in my synth MeetUp group, suggested creating a custom personal library composed of symbols and footprints to be used over and over. Some are made "from scratch", some are brought in from snapEDA, some from obscure libraries found on the Internet, some are existing KiCAD library objects with minor modifications.
Following Elton's lead, I created, and will maintain, custom Kicad symbol and footprint repos. I have posted that on GitHub; go here and here.
Update 3-2-25: All hail smisioto.no--you can find most every Kicad symbol/footprint/3d model you could ever think of, and a lot you never thought of: here. Wow!
SCHEMATIC CAPTURE
After only using Kicad for a few hours, I found its schematic capture ability (well documented here) to be really easy!
A few shortcuts proved helpful:
- A for adding new symbols; basics like resistors and capacitors are in the folder called "devices". Shortcut: type "C" for a generic cap symbol and "R" for a generic resistor symbol.
- M for move
- D for drag. This is the same as "moving" in Eagle--you can move a part and the wires won't break.
- R, X or Y for rotating and mirroring
- W for wiring; / (slash) changes if you want to allow 90 degree bends in your wiring, 45 degrees, etc.
- E for modifying a symbol's properties....tap this and a dialog pops up when you can change things like values, display characteristics, fonts, and whatnot--this "E" behavior seems universal to many objects in Kicad. You also see options for changing symbols for your entire schematic through the "E" shortcut.
Right click > change symbol brings up a dialog to replace one symbol with another. This is the same as right click > replace in Eagle.
Synchronizing modified or updated "devices" in Eagle into my design was always cumbersome and confusing. Thank goodness it's much easier in Kicad--edit a custom symbol using the "symbol editor", save, open the schematic, then issue Tools -->update symbols from library. This brings up a dialog where you can find and replace symbols found in the entire schematic or a subset. This synch process has to be done manually; fine with me.
Tools > assign footprints brings up the dialog where you can assign footprints for your symbols. Again I found this pretty straightforward with one space oddity: to make your choices "stick" you have to click the "Apply, Save Schematic and Continue" button after making your edits--just clicking OK won't do it.
Another Kicad feature: You can modify a PCB and have the changes brought back into the schematic. Tools > update schematic from PCB. Eagle can't do this.
There are a lot more options and features of course. Thankfully Kicad's documentation is really good--find it here.
Update: I see this schematic layout elements of Kicad called "EESCHEMA". I am not an EE, but I occasionally have a SCHEMA.
LAYING OUT PCB's
Eagle automatically creates a PCB from your schematic; with Kicad, you have to start up the PCB editor then issue the command tools > update schematic from PCB to see footprints.
The PCB creation documentation (here) has a lot of detail, but I found the basics to be pretty easy once I learned some shortcuts:
- D drag a part, moving its traces along with it. If a trace turns green during the attempt it means it conflicts with your relocated footprint--edit conflicting trace(s) and try again. Otherwise--if you don't remember to hit D--the footprint will move but not its traces and you are left with a mess. Is there a way to make D the default behavior?
- X turns on the "trace route" tool
- Page up/page down toggles between layers (front and rear copper for instance)
- V places a via
- For 2 layer boards, the quick way to switch between placing front and back traces: create your trace, click "V" on your keyboard, placing a via, and then left click with your mouse to continue running a trace on the opposite side of your PCB. Don't click any other keys (no shift, no control, no enter) or this workflow may be interrupted.
- Alt + 3 shows a 3D view of the PCB (cool!!!)
- There are many more shortcuts documented here.
right click -- drag from bottom to top selects everything; right click -- drag top to bottom selects only items fully enclosed. Useful! Video here.
To change trace width, it's easy with Eagle--type in "change width 10 mil" or whatever in the uppermost text box then click on a trace that you want to fatten.
A few more steps with Kicad, but still not hard:
In the PCB editor, choose Track: use netclass width > edit predefined sizes.
Next, hit the + below then add some sizes to the dialog. (By the way: 40mm-75mm are really big trace sizes--I was messing around with DRC--you probably want smaller traces...)
Hit OK, now you can dial in the track width you want from the same "Track: use netclass width" when creating traces.
IMPORTING FROM EAGLE
Update: 3-3-25 I have removed this section re: the Eagle > Kicad update process for Kicad 7 since it's changed and is much improved in Kicad 8 and 9.
If interested, please read the dedicated post--Kicad >= 8 imports from Eagle--here.
BLOCKS AND HIERARCHICAL SHEETS
Modularity and reuse in Kicad? You bet! I removed that from this post because after many edits the section was getting too long; dedicated post on these features is
here.
"LIVE AND LEARN"
....solutions to things I had to figure out, not immediately obvious to me
Changing footprint descriptions; matching a footprint to its 3D image Surprisingly--neither are available via the "e" shortcut. With the footprint open and ready to edit: file > footprint properties. The "General" tab allows you to change the description; "3D Models" lets you select then position 3D images for the footprint. 11-20-23
Changing "drawing sheet" size (the border with title block etc): open EESCHEMA editor or PCB editor, then > file > page settings. Adjust width and height. 11-25-23
Creating ground pours: I always forget how to do this...we will start with the front layer:
- open your PCB
- In the top right, under "Appearance", left click on "F. Cu":
- to the right of your PCB, click on this icon:
- Left click somewhere outside your PCB's edgecut
- Select "F.Cu" and "GND" (or whatever designation you are using for ground) in the dialog that appears:
- Draw a rectangle around your entire PCB, doesn't matter where, but make it bigger than your edge cuts
- Hint: when closing your rectangle right click + "close outline" to complete the rectangle
- Click B on your keyboard to fill.
- Run Inspect > Design Rules Checker to make sure the pour is OK.
Repeat the process for the B.cu (bottom layer).
Cool, but how to turn the damn pours off when you want to edit your PCB?
The "toggle your pours on and off" icons are on the left side of the PCB:
Good video for this is
here.
2-9-24
Making imported footprints work with Kicad symbols: This is an obvious one that I missed for several weeks.
Eagle allows you to name device pins--"Tip", "Ground", and "Sleeve" for a 3.5mm jack, for instance. I figure all EDA programs do this.
But! Corresponding Kicad pins have numbers, not names; pin numbers in Kicad may not match those imported from Eagle,
When importing Eagle devices into Kicad custom libraries: edit pin numbers to make them Kicad-like.
"Kicad-like?"
Here is what I mean: Kicad symbols often follow a pattern: for instance, for diodes, it's usually 2-anode and 1-cathode. So if you are importing an Eagle diode into a custom Kicad library, edit your imported footprint to change pin names "Anode" to "2" and "cathode" to "1".
If there is any doubt open a factory symbol in Kicad and note its pin numbers. Then, edit the Eagle component before adding to your custom libraries so it will work in future designs. 5-26-24
Constraining lines to H/V/45 degrees: when drawing silkscreen lines for boards for instance, right click as you are drawing and choose "H/V/45". This constrains the line to Horizontal, Vertical, and 45 degrees. Nice! To undo, right click again as you are drawing and deselect this feature. 5-31-24
Placement Constraint: This assumes Preferences > Preferences > Schematic Editor (or) Footprint Editor > Grid Display >Snap to Grid is set to "Always" or "when grid is shown":
Use the UI element boxed in red below to constrain line endpoints, parts placements, text locations, etc.
This setting does not impact the density and frequency of visible cross hatches/dots/lines as you zoom in and out; instead, it determines where by default you can place things.
Holding down "control" while placing an object overrides this setting. 9-1-24
Importing 3D models into Kicad: Save your 3D file in "STEP", "STP". or ".WRL" format--most 3D software can do this. Then: open the footprint editor in Kicad, choose the footprint that needs a 3D model, then file > footprint preferences > 3D tab. Click the folder icon at the top of the dialog and choose your WRL or STP file you just saved; use the various +/- buttons to scale and position your model. When you're happy, click OK. Good video for this can be found
here.
9-14-24
Importing .lib symbol libraries into Kicad: seems <= Kicad 5.0 (?) used ".lib" as an acceptable extension for a symbol library. If you are importing from the outside world (
e.g. the useful library
here) you might find 2 files: .dcm and .lib. Leave .dcm alone but rename the extension of the .lib file to
.kicad_sym; open symbol editor in Kicad > import the library > find the .kicad_sym file > OK
9-30-24
Importing symbols into Kicad: You can't overwrite the symbol libraries that shipped with Kicad, so you'll need to save imported symbols into their own symbol library then import it into your project (how-to
here).
Better yet, extract the symbols you care about into your own custom symbol (*.kicad_sym) file.
How to do the latter.
Create a custom library if you don't already have one (symbol editor > file > new library), or get my custom symbol library from Github
here, save it to your hard drive, then add your cool symbols to it.
To import a single symbol into your custom symbol library:
- Save your newly acquired .kicad_sym file somewhere.
- Unzip the symbol file if needed
- In KiCad, go to Preferences.
- Click on Manage Symbol Libraries.
- On the Global Libraries tab, click on Browse Libraries (the small folder icon)
- Select the .kicad_sym file you just imported, then click Open.
- The library will appear, click OK.
- From the main Kicad screen, click on Symbol Editor.
- Type on the filter search field and navigate to the symbol in the library you just imported.
- Double-click it to open the file.
- Edit the symbol as needed
- Optional: File > symbol properties > footprint and assign the symbol a default footprint
- File > save copy as
- Save the symbol, extracted from the imported library, into your custom symbol library. 10-28-24
Kicad Symdirs: In kicad10, you can create a folder called [foldername].kicad_symdir and save your custom symbols there. This makes editing them the same mindset as editing as footprints: edit a single custom symbol and not have to resave the entire symbol library, rather, just your newly modified symbol. Nice! Get my custom symdir content from github
here.
5-21-26
Setting Grid Origins for your PCB: (tried this with Kicad V9, not sure about older versions) By default 0,0 of my grid is the top left corner the large purple box that holds your PCB drawing--the "drawing sheet"? Sorry still don't know what to call the purple box thing.
I don't want 0,0 to be there since it has nothing to do with my PCB. I want it to be the bottom left corner of my PCB. How to change this?
- In the PCB editing tool, set your grid--say 100 mils--from the pull down at the top:
- Select then move your entire PCB so the bottom left corner of the edge cut lines up with a sensible spot on the grid.
- Preferences > Preferences > PCB Editor > Origins & Axis
- Go back to your PCB, and from the menu along the top: Place > Grid origin
- left click on bottom left corner of edge cut. You will see a cross on the new origin. 5-17-25
Getting started with NGSpice Simulations and Kicad: C
omplex enough that it needs its own post; go here. 2-10-25
Why can't I select a @#$% symbol library to import things into? Simple! make sure this icon is selected on one of the left columns. Your list of available symbol libraries appears...left-click on to select a symbol library to import things into. Remember! you can't import anything nor edit the "stock" libraries that come with Kicad--you have to use a 3rd party library or create your own. 4-25-26 (Kicad 10)
Avoid using absolute paths for things like custom 3D models. Use "Environment Variables" instead.
A path like this maps to a windows D:\ drive and will work on a single system:
But as soon as you go to any system that has "Dropbox" mapped to somewhere else on its local storage devices this will break.
Instead, use a Kicad Environment variable:
Notice the syntax here: ${env_variable_name}
You can create as many custom variables as you want, configure this through Preferences > Configure paths:
You can then drop these variables into things like "where does the 3D file for this live"? This will allow a computer with different directory locations to still find things you create in Kicad.
4-26-26 OUTRO: GERBERS n' PCBWAY
In case you haven't noticed by now, Kicad kicks Eagle's butt. Small wonder Autodesk is moving on.
After a few evenings with Kicad, I feel I know enough to create a baptism-by-fire schematic and PCB. Probably a retread of something I made in Eagle? Why not....coming soon.
HA!!--it works--"KicADSR". My first Euro module created with Kicad. Post is here.
 |
| Not that kinda gerber.... |
....I checked out a Kicad gerber creation how-to on my sponsor PCBWAY's site--here.
Check that! Shout out to Serene at PCBWAY, she told me I could get PCBWAY's add-on for Kicad--for uploading designs to PCBWAY for fabrication using a single click.
Instructions for setting up the plug-in are here.
A useful video going over other cool Kicad add-ons is here.
After installation the plug-in made uploading files to PCBWAY a breeze: I logged into the PCBWAY website, ran Kicad, opened the test PCB, the in Kicad went to tools > plug-in > "PCBWAY Plug-in for Kicad".
This gerber-ized my file and everything looked to be good to go.
Finally I picked which color PCB I wanted, how many I wanted fabricated, any a few other options; then hit "add to cart".....
Enough for now, this is getting to be long post. Much more KiCAD on the way. Don't breathe the fumes....
