[0:00] I recently prototyped these I2S stereo amplifier boards using PCBWay.
[0:05] They work really well and I made a bluetooth speaker using them.
[0:07] But there’s a couple of improvements I want to make.
[0:10] The first is the size of the board.
[0:12] My original plan was to make them the same size as the Adafruit mono I2S amplifier.
[0:16] I’m not sure what happened, but somewhere in the excitement of PCB layout
[0:20] I ended up with much smaller boards.
[0:22] This has the knock on effect of things being a bit cramped.
[0:24] You can’t see the silk screen for the two speaker connections
[0:27] which is pretty poor for something that is supposed to be a nice friendly breakout board
[0:31] and the screw terminals are hanging off the edge of the board.
[0:33] Which frankly just looks a bit rubbish.
[0:35] Time to fix my mistakes and do a version 2.
[0:40] I’m going to take this opportunity to lear KiCad and see what it’s like.
[0:44] My first task is to learn how to pronounce it
[0:47] is KiCad or KeeCad - let me know in the comments.
[0:49] For now I’ll stick to KiCad as it’s easier for me to say.
[0:53] Why KiCad?
[0:54] Not only is it free
[0:56] it’s also open source.
[0:58] If there are any problems or things I really dislike about it, I can always dive into the code and try and fix them.
[1:02] It’s also very popular in the maker community
[1:05] and it’s good to learn new things
[1:07] I’ll let you know what I think of KiCad at the end of the video.
[1:12] I’ve already downloaded KiCad and installed it on my machine.
[1:15] I want to set it up with the right design rules and settings for PCBWay.
[1:20] On the PCBWay GitHub account there’s a link to a template project we can use.

[1:24] We can easily follow the instructions here. It’s pretty straightforward.
[1:27] We just create a templates folder and clone the repo into it
[1:31] With that done we just go to the KiCad preferences and update the paths
[1:34] so that the user templates path points at our new templates folder.
[1:38] Now, when we create a new project we can now select the PCBWay template.

[1:42] This should give us all the correct settings and DRC rules for PCBWay.
[1:47] To open up the schematic editor and start our design we just double click on this icon.
[1:52] I’ve made one change to the preferences that lets me use my trackpad to pan the design
[1:56] This makes navigation a lot easier
[1:59] as I can just use two finger swipes to move the canvas around. And I can pinch to zoom in and out.
[2:03] To place a symbol we either use this icon and click or use the ‘P’ keyboard shortcut.
[2:08] The first problem we have it that we don’t have a symbol for the MAX98357 in the symbol library.
[2:14] Let’s get that fixed.
[2:15] I’ve found the symbol on Octopart - so we just download it.
[2:18] I’ve created a libraries folder on my machine and unzipped the download into it
[2:22] I’m sure there will more symbols required over time.
[2:25] To add it to our symbol libraries we goto Preferences -> Manage Symbol Libraries.
[2:29] And then click the little folder icon to add our downloaded lib file.
[2:33] Going back to the schematic editor we can now find our symbol and place it.
[2:39] I’m just going to quickly recreate my original layout from EasyEDA
[2:43] I could just try and import it, but I want to learn how to use KiCad.
[2:47] I do have a complete video on the schematic for this project, but it is pretty straightforward.
[2:51] We need a 7 pin header for the input
[2:54] looking through the symbol library we can find a component for this by searching for Connectors.
[2:58] I’m going to use labels to hook things up to avoid wires going all over the place.

[3:02] You create a label using this menu icon
[3:05] and then just click where you want them.
[3:06] Double clicking lets you quickly modify the name.
[3:09] To rotate symbols use the “R” keyboard shortcut. Make sure you have the mouse pointer over the symbol you want to rotate.
[3:15] Similarly, we can duplicate using the “C” button
[3:18] again make sure the pointer is over the symbol you want to duplicate.
[3:22] To place the power ports we use this symbol and then click where we want the symbol.
[3:27] We can find and place the ground symbol we need.
[3:29] And we can also find and place the VCC symbol.
[3:31] To place a wire use the “W” keyboard shortcut.
[3:35] This does have some slightly weird behaviour where the wire starts wherever the cursor currently is
[3:39] but you get used to that after a while.
[3:41] Just place the cursor where you want the wire to start
[3:43] Once again I’m connecting up all the non connected pins to ground as I did in my previous layout.
[3:48] I also need a couple of decoupling capacitors
[3:51] so I’ll use the P key to place two generic capacitor symbols
[3:54] and hook them up to VCC and ground.
[3:56] The final thing we need is a screw terminal for the output.
[3:59] Once again it’s the P key and we just search through the component libary for screw terminals.
[4:04] And that’s the left channel done.
[4:06] We can just make a copy of this to create our right channel.
[4:09] If you just drag and select then you will start moving the components,
[4:12] so you need to shift+drag to make a copy.
[4:14] The right channel is the same as the left,
[4:16] but there’s now a resistor going to the SD line so the chip knows to only process the right channel.
[4:21] We’ve got a bunch of question marks on our components so I’ll just quickly fill these out.
[4:25] I’m not sure if this would be done automatically
[4:27] but I’ll do it now just to be sure.
[4:28] I’ll also put values on the symbols for the capacitors and the resistor.
[4:34] before we generate the PCB we need to assign footprints to our symbols
[4:39] KiCad works in a slightly different way from EasyEDA - the symbols are

[4:42] independent from footprints, so we need to assign a footprint for each component in our schematic.
[4:47] This is done from the Tools -> Assign Foorprints menu item.
[4:50] This is pretty straightforward for most of our components the

[4:52] filter works quite well and they have footprints for everything.
[4:55] However, we don’t have a footprint for the MAX98357 chips.
[4:59] We could use a standard footprint from the existing library
[5:02] but I’m going to use the specific foot print that we got from Octopart.
[5:05] To import the footprint we use the Preference -> Manage Footprint Libaries.
[5:09] We click on the folder icon and navigate to the folder that contains the footprint file.
[5:13] We can now go back to our schematic editor and finish off assigning our footprints.
[5:19] To convert the schematic to a PCB we need to generate the netlist.

[5:23] We do that using the netlist icon.
[5:25] We can now open up the PCB tool by double clicking on this icon and import the netlist.
[5:30] That’s brought in all our components ready to layout.
[5:34] I want to have a custom board outline that has curved corners
[5:38] and I’ve done some playing around and some research on KiCad
[5:42] and it seems the consensus is that to do any that to do anything more complex than basic rectangles
[5:46] you should use a different tool and generate a DXF file.
[5:49] So I’m going to use Fusion 360 to create a sketch of the board outline and give it rounded corners.
[5:54] I can then export this as a DXF file and import it for the board outline.
[5:58] What’s interesting is the construction lines from the sketch have also come through
[6:02] so maybe worth deleting them before doing the export from Fusion360
[6:09] To move components around you hover over them and hit the “M” key
[6:12] Rotate is the same as in the schematic editor - just use the “R” key.
[6:16] With our components in the correct positions,

[6:18] we can do the wiring up. To start a track push the “X” key. You can insert a via as

[6:23] you are drawing a wire using the “V” key and carry on drawing on the opposite layer.
[6:26] To quickly switch between layers you can use the “+” and “-“ key.

[6:30] I found this quite helpful when placing tracks on the back and front of the board.
[6:34] With the signal tracks all done I just need to add some thick

[6:36] tracks for the power and the speaker outputs. There’s a handy track width

[6:40] calculator built in that we can use to work out what size we need to use.
[6:44] We can add our new track width to the available options.
[6:46] And then add our wide tracks for the power and speaker connections.
[6:52] I’m going to add a copper pour connected to the ground net on both the top and bottom

[6:57] of the boards. This will give us some good thermal dissipation for the amplifier chips.
[7:00] The chips are very efficient, but let’s give them a bit more help.
[7:03] This works pretty well, the only thing I needed to change was the

[7:06] clearance to match the capabilities of PCBWay.
[7:08] I’ve also stitched the front and back ground pours together using vias.
[7:14] One of the things that I was keen to try out on

[7:16] KiCad was the 3D view of the PCB and in particular the 3D export.
[7:21] Opening up the 3D view it works nicely, but the models for the amplifier ICs are missing.
[7:25] To fix this we need open up the footprint properties and associate the 3D model.

[7:30] For some reason this didn’t work properly when we imported the footprint originally,

[7:33] but we just need to fix up the file paths.
[7:35] Back on the PCB we can now just update the footprints and our 3D model is fixed.
[7:42] The 3D export is one of the main reasons for me to start using KiCad - I 3D print

[7:47] a lot of boxes for my custom PCBs and having an accurate model is priceless.
[7:51] Exporting the step file and importing it into Fusion360

[7:55] seems to work really well. For my workflow this is a bit of game changer. Having an

[7:59] accurate model of your PCB along with the components on it makes desiging

[8:02] enclosures considerable easier - it should eliminate a lot of guesswork.
[8:08] The final thing to complete our PCB is the mounting holes. I need to move the screw terminals

[8:13] closer together to fit these on and hit a problem with the DRC - there’s a rule in the DRC around

[8:18] overlapping courtyards. The footprints for the connectors in KiCad have very generous

[8:22] courtyards which makes it hard to put the terminal blocks close together without breaking the rules.
[8:27] For my design I’m turning off these rules as they aren’t really relevant

[8:30] and I know the screw terminals will fit without any problems. It took a

[8:34] bit of poking around to find the option for this, but I found it eventually.
[8:37] Re-running the DRC we just need to fix up a track from when I moved the screw terminals.
[8:41] We’ve got our mounting holes and I can reload the model in Fusion360 to have a good look at it.
[8:49] Labelling the pins is a pretty mechanical process.

[8:51] Once again I’m labelling both top and bottom layers to make it easy to use.
[8:55] And I’m sticking my board label and revision number on the bottom of the board.
[8:59] I’m pretty happy with that, we’re good to go.
[9:04] To export the Gerber and drill files I’ve followed the instructions from the PCBWay website.
[9:09] You use the File->Plot menu option and select the required layers. For a two

[9:14] layer board we need the Top and Bottom copper layers and then the Solder Paste,

[9:18] Silk and Solder Mask for both layers. We also need the Edge Cuts to give our board outline.
[9:24] You need to make sure to check the “Use Protel Filename Extensions as well”
[9:29] You also need to generate the drill files so the

[9:31] PCB manufacturer knows where to make holes in your PCB.
[9:35] Follow the instructions on the PCBWay website and you should be ok.
[9:39] We just need to zip up the results of this export to have something we can submit to

[9:43] PCBWay. We can also use an online Gerber viewer to double check the results of the export.
[9:47] And it looks pretty good
[9:51] I’m going to be doing SMT assembly with PCBWay. So I need to create a Bill of Materials File
[9:56] We just go to File -> Farication Outputs and click on BOM

[10:00] file. This will create a CSV file that lists our components along with their designators.
[10:04] I’ve opened this file up in Excel along with the BOM file from my previous version that

[10:08] PCBWay sent me and the template Excel file that PCBWay suggest.
[10:12] Let’s try and get out file to match what PCBWay would like. The first thing I’m

[10:16] going to do is remove the mounting holes, pin header and terminal blocks.
[10:20] As the won’t be assembled by PCBWay. I’m not sure why the mounting holes are inclued.
[10:26] I’m going to get PCBWay to supply the components
[10:29] so I just need to let them know the manufacturer and the manufacturers code.
[10:33] Fortunately I can copy and paste these from the original BOM and I can look them up on LCSC
[10:41] We also need the footprint positions for our board, one thing that I did need to do was include

[10:46] footprints even if not marked for surface mount - if I didn’t do this my ICs we not

[10:50] included - hopefully this would have been caught by PCBWay before it got to manufacture,

[10:54] but I’m happy that I caught this error.
[10:58] With all the files generated,

[10:59] we’re now ready to submit the files to PCBWay and get our boards ordered.
[11:03] To do this we use the quick order process and upload our Gerber files. All the defaults

[11:07] should be fine for us and we can fill out the details for the SMT assembly.
[11:11] On the following screen we upload the BOM file

[11:14] and the position files. PCBWay will take our BOM and work out the costs for the parts and

[11:18] we’ll be good to go.
[11:21] After 12 hours or so
[11:23] I’ve received the final quote for the parts. PCBWay have filled in the costs.
[11:29] We can go onto LCSC and check the prices to

[11:32] see if they are reasonable and they all look pretty sensible.
[11:35] I’ve approved the order so we’ll see the fruits of our labour in a couple of weeks. I can’t

[11:38] wait to see how they come out. Fingers crossed we’ve not messed anything up!
[11:44] So, what do I think of KiCad having done an end to end project with it.
[11:48] I found it surprisingly pleasant to use. Symbol and footprint management is a bit confusing,

[11:52] it took a few tries to understand how to do it. But, this seems to

[11:55] be the case of all the software I’ve used
[11:58] they all seem to make symbol and footprint management amazingly complicated.
[12:01] The UI is a bit 90s, it doesn’t look that nice an there’s other software that looks nicer
[12:06] but it is functional. And the icons are fairly easy to understand
[12:09] There are a few quirks and weird things, but I got used to it pretty quickly.
[12:12] I give it a solid 8 out of 10 - I would recommend giving it a go.