View All Posts
Want to keep up to date with the latest posts and videos? Subscribe to the newsletter
HELP SUPPORT MY WORK: If you're feeling flush then please stop by Patreon Or you can make a one off donation via ko-fi

Learn how to create custom footprints, symbols, and 3D models in KiCad 6 with this step-by-step guide. Design your own LED filament for a PCB project and watch it come to life in a 3D preview!

Related Content

[0:00] KiCad comes with a huge library of symbols and footprints.
[0:03] But what if you can’t find what you’re looking for?
[0:05] Let’s make a custom footprint, symbol and 3d model.
[0:08] right after this quick plug for the channel sponsor PCBWay.
[0:12] Do you like PCBs?
[0:14] Do you want to make a PCB and a weird and wacky colour like purple?
[0:17] Maybe you’d like a flexible PCB?
[0:19] Or maybe you’d like someone to do some CNC work for you?
[0:23] Check out the link to PCBWay in the description.
[0:31] I’m doing a project with these LED filaments.
[0:34] I’ve measured them up and the body of the filament is 33mm long with a 2.5mm diameter.
[0:41] The leads are about 4mm long giving us a total length of 41mm.
[0:46] To create a new footprint in KiCad we click on the footprint editor icon.
[0:51] I’m going to create a new library for my footprints so let’s create

[0:54] a new library and we’ll call it “LED_Filaments”
[1:00] Once that’s done we just right click and create a new footprint.
[1:04] So we’ll call this Led_Filament_4mm.
[1:07] I’ll just move these auto-generated bits of text out the way slightly

[1:11] and then add a rectangle for the filament body.
[1:14] I don’t actually want this to show up in my final PCB

[1:17] so instead of using a silkscreen layer I’ll use the user drawing layer.
[1:21] To make sure it’s nicely centred I’m going to edit

[1:24] the numbers directly instead of trying to draw it freehand.
[1:27] We now need to add two pads.
[1:28] I’m going to need one for positive and one for negative.
[1:32] Once again I’m going to adjust the numbers to get

[1:34] them exactly where I want them and the size I want.
[1:37] So we’ll do this for both paths so this is the negative pad and that’s done.
[1:42] So that’s pretty much it for what we need for my LED filament.
[1:45] But what I really want is a 3d model to go with it.
[1:48] So let’s jump into fusion 360 and knock one up
[1:54] Adding a 3d model will also let me check that everything lines up.
[1:58] As always in Fusion360 we start off with a sketch.
[2:02] I’ll make one for the connectors that stretch the whole length of the device

[2:05] and just extrude it by a very small amount.
[2:08] To position the body of the filament in the correct place

[2:10] I’m creating an offset plane from each end of the connector.
[2:13] I can now create a sketch on one of these planes with a circle at the required diameter.
[2:18] We can then just extrude this to the other plane and that’s our body
[2:25] I’m creating it as a new body so that I can apply appearance to it

[2:28] and we just need to do a quick bevel so it looks nice.
[2:32] Now we just need to apply some appearances.
[2:34] For the connector, I’m going to use some polished aluminium.
[2:40] And then for the actual body, I’m going to use a glossy yellow.
[2:44] So that looks pretty good we can now export this as a step file

[2:48] and head back into KiCad to assign it to our footprint.
[2:54] So we load up our step file and now we can preview it here.
[2:58] Now having a look at this I think I’m going to move the pads out

[3:01] by just a maybe half a millimetre just to give a bit more space for soldering.
[3:06] So if we go back and adjust the pads we could just use the numbers to do that.
[3:10] So 19.5.
[3:14] And 19.5 on this one as well.
[3:17] So if we now check our 3d model I feel it looks a bit better

[3:21] and there’s more room to get the soldering iron in.
[3:30] So with that done let’s create the symbol.
[3:32] So we go back to the main screen of KiCad and click on the symbol editor.
[3:36] Once again I’m going to create a new library to hold my symbols.
[3:40] So we’ll click new library and I’ll call it LED_Filaments
[3:46] And with that done we right click and create a new symbol.
[3:49] So let’s do LED_Filament_41mm.
[3:53] I’ll just move this text out of the way

[3:55] and then we’ll design some nice graphics for our led filament.
[3:59] So I’m going to draw a bunch of LEDs just to indicate there are multiple LEDs in this package.
[4:04] So we’ll draw one and then make a bunch of copies.
[4:09] And that looks pretty nice we’ll just put a box around

[4:11] it so that it encapsulates the whole component.
[4:14] So now we just need to add our pins.
[4:16] So we need a pin for the positive connection.
[4:19] One thing you do have to remember is to set the pin number if you don’t

[4:22] do this then it won’t connect up to the footprint properly.
[4:26] So that’s the positive connection and now we just need to add the negative connection.
[4:34] And with a final bit of tweaking of positions, we’re done with our symbol.
[4:38] So let’s try it out.
[4:42] I’ve started a new schematic.
[4:44] Let’s make a seven-segment display.
[4:47] So I’ll add in seven of our new led filaments

[4:50] and I’ll just arrange them in a particular pattern for a seven-segment display.
[4:56] So I’ve added all seven.
[4:57] I’m going to use a common anode so all the positive pins will be connected together.
[5:02] And I’ll be switching on the negative pins.
[5:04] I’ll add in a pin header for all the connections and I’ll use

[5:07] labels to connect everything together.
[5:09] This will just make this schematic slightly easier to read as there won’t be wires going everywhere.
[5:15] So that’s it all wired up we now need to assign the footprints.
[5:19] So we click the assign footprints KiCad will prompt us to annotate the schematic.
[5:24] So that just adds numbers where you currently see question marks.
[5:27] So if we select all the LED filaments and then we search for our custom footprint

[5:32] we just need to double click on it and that will assign it to our symbol.
[5:39] And now we just need the footprint for our header.
[5:42] I’m going to use a horizontal header because I’m going to plug these PCBs into a motherboard.
[5:49] So that’s that done let’s design the PCB for this
[5:58] So we switch over to the PCB tool and we update it from the schematic
[6:07] So that’s added our components to the PCB.
[6:10] I’ll position them in approximately the correct position.
[6:16] So that’s done and if we look at the 3d preview we can see

[6:19] our nice LED filament model is being pulled in.
[6:23] But i want quite a complex board outline for my project.
[6:26] I’ve designed how I want it to look in Fusion360.
[6:30] But if you look at the underlying sketch for the board outline

[6:33] you can see that it’s pretty complex with lots of construction lines.
[6:36] We can’t use this board outline in KiCad.
[6:39] But what we can do is create a new sketch and we can project the board geometry onto it.
[6:45] This will give us a really nice clean sketch that we can export as a DXF file

[6:49] and then import directly into KiCad as our edge cuts.
[6:53] So let’s export this as a DXF file.
[6:56] So I’ve turned off everything else.
[6:57] You can see it’s nice and clean.
[6:59] So we right-click and we do save as DXF.
[7:03] So then back in KiCad we can import this as graphics and set it as the edge cuts layer.
[7:13] So we just need to rotate it and then we’ll just tweak all the positions

[7:18] so they line up nicely with our new board outline.
[7:26] That’s done - let’s look at the 3d model.
[7:30] So I think this is going to look pretty cool.
[7:32] I just hope it can actually be manufactured but we’ll see when we send it off for processing.
[7:38] So I finished all the routing.
[7:40] We do have some design rule warnings from the connector

[7:43] as it has a bunch of silkscreens that we don’t need that overlaps the edge cuts.
[7:50] What we can do is we can go in and edit

[7:52] the footprint and remove all of this stuff we don’t need.
[7:56] So we go and update the footprint and now we can just delete the bits that we don’t want.
[8:03] Now one thing to remember is this only affects the footprint in this PCB.
[8:07] It’s not going to affect the global footprint.
[8:10] Now when we run the DRC again all of our warnings have disappeared.
[8:14] There’s just a final bit of cleanup to do and adding some pin labels.
[8:19] I’ve hidden all the user graphics and it looks very nice and the 3d model looks great as well.
[8:24] So these PCBs are going to plug into my main control board

[8:27] so I might make a custom symbol footprint and 3D model for them later.
[8:31] I hope you enjoyed this video.
[8:33] If there’s anything in my workflow that could be better or is just plain wrong

[8:36] then let me know in the comments.
[8:37] I am still learning KiCad 6 so any advice would be much appreciated.
[8:42] I’ll see you all in the next video

HELP SUPPORT MY WORK: If you're feeling flush then please stop by Patreon Or you can make a one off donation via ko-fi
Want to keep up to date with the latest posts and videos? Subscribe to the newsletter
Blog Logo

Chris Greening

> Image


A collection of slightly mad projects, instructive/educational videos, and generally interesting stuff. Building projects around the Arduino and ESP32 platforms - we'll be exploring AI, Computer Vision, Audio, 3D Printing - it may get a bit eclectic...

View All Posts