He is sponsored by and uses JLCPCB. (see around 5min).
He includes a USB to serial converter and uses a USB-C connector.
I already have a /home/tom/KiCAD directory. I navigate there and call this new project "emup". And I open the Schematic Editor. By default, this takes up my entire screen, but is easy to reduce in size.
The mouse wheel zooms in and out. Clicking specifies the center of the zoom. Right button hold drags things around. Left button hold gives a selector rectangle.
Top left, 3 over is page setting where you can specify paper size and fill in stuff for the title block.
On the right side is a thing that looks like an op-amp. (or click "a") This is "place symbols". I type 74LVC245 into the search entry (filter) at the top, and there it is!! However, it does not give a DIP footprint for this part, so I select a 74HCT245 instead, which has the same pinout.
Passive components are available (R for resistor, C for capacitor).
For his MSPM controller, he had the design the symbol, and he says not to be hesitant about this. He also says beware of downloading symbols that are not part of the standard KiCAD libraries as they often have errors or are not what they claim to be.
I also need some ribbon connectors, and I am surprised to find them easily. To go to my DB-25 I need a 26 pin ribbon (2x13) and I find "Conn_02x13_Odd_Even". There are many many footprints. I select IDC-Header_2x13_P2.54mm_Vertical.
And I need a 40 pin ribbon for the Orange-Pi connection. This is "Conn_02x20_Odd_Even". I select IDC-Header_2x20_P2.54mm_Vertical for the footprint.
I also want to use one of the 4 terminal green screw terminals for power. KiCAD calls these TerminalBlock in the PCB editor. In the Schematic Editor, look for Screw_Terminal_01x04. Again, a multitude of footprints are offered. My blocks are 0.2 (5mm) spacing so I select one of those.
The last thing I need is a 74HCT04. I select the dip footprint. When I place this, I get to place each of the 6 inverters. I will use just 4 of these.
While I am going on about the EMUP adapter board I plan to build, it seems completely reasonable to supply the Orange Pi with 5 volt power via the 40 pin cable. It also seems reasonable to use the 3.3 volt power it makes available to power the LVC245. This means I can avoid a 3.3 volt regulator on the board. I can also avoid supplying 5 volt power via a barrel connector.
On the right side, 3 down is a thing that looks like a ground. This gives you your power symbols. I can go in here, find ground, click OK and then I have the symbol to place where I like. I place it, then hit ESC and I am ready to start over. The "p" shortcut is another way.
This turns up a problem. Although I placed 6 individual inverters for my 7404, I have no place to connect power and ground. I delete this (use DEL on the keyboard). And I place it again. There are actually 7 things -- the last is a box that has the place for power and ground.
I type Ctrl-S to save every now and then. When I do this, the title at the top center had a "*" prior to the save to clue me in that I had unsaved work. When I save, this goes away.
Ctrl-Z is an undo. I use this after I place +5 where I wanted +3.3. Note that using 3V3 avoids the invisible "dot" in 3.3.
To move anything, select it, which causes it to "light up", then use "m" to move it. This works for part "designators" (part numbers and U1 and such) as they are their own object on the drawing. Use "r" to rotate a part. ESC to cancel or end these.
If you don't want to see the letters "GND" next to your ground symbols, double click on those letters to get a dialog and uncheck the "visible" checkbox.
Pressing ESC finishes or terminates a command.
When you have a lot of the same part, you can create the first (including the footprint). Then use copy to duplicate it with all of your customization. You may even want to create your own symbol library for parts you keep in stock and use over and over.
To make connections, hover over the tiny "ball" at the end of something you want to connect. When you see a "pen" appear, let go. Then do the same where you want it to connect to and there you are. To make the wire take a turn where you like, click at the spot along the way (as many times as you like). You can get silly with this.
To copy a part (or a selected subcircuit) use Ctrl-C Ctrl-V. C for copy, P for paste. One the new part appears you can use "r" to rotate it, "x" to flip it left-right, (along the X axis) "y" flips it up/down (along the Y axis).
He suggests labeling every single net in your design! Click on a wire to select it, and look at the lower left for the info. Use the keyboard shortcut "L" or the thing on the right column that looks like an A with a line under it. When you place the name, there is a tiny box at the lower left of the text that you must place on the wire.
To add a capacitor value, hover over the capacitor and type "V" to get a gadget to enter a value. You can also get a right click menu and go to properties.
You get more than you bargain for from the "Phil's Lab" videos, and in a good way. He talks about electronics and circuit design as much as just the mechanics of using KiCAD.
Also he does what I have already learned to do. Use Ctrl-C Ctrl-V to duplicate parts already on the schematic rather than pulling them from the big component selector menu. Then modify values as needed.
He adds a crystal using "crystal_gnd24". Look up ST Micros AN2867 which is a 60 page document all about using crystals in microcontroller designs.
He likes the spc3819 as a "jelly bean" 3.3 volt regulator.
If you find yourself wanting to make a connection where there are no dangling wires with little circles, use "w" to start the wire functionality.
Use shift - click - drag to extend a selection that didn't quite get everything.
He uses a clever thing, a TC2030 debug connection. The end on the board is free (there are 6 printed pads and 3 drilled holes). KiCAD knows about it. He likes to include reset in the debug signals, which is a good idea.
Use "t" to add text annotation anywhere you like. There is also a big "T" on the right to trigger the same feature.
You can create "net classes" (2nd icon from the left up top) that color lines on the schematic, but also may indicate things like trace thicknesses and such for PCB layout. If you select intelligent net names, you can select all the nets that apply with a wildcard like /USB*. This will be especially helpful when PCB layout is being done.
When you think you are done, run ERC (electrical rules check). There is an icon up top with a red circle and check inside. Or you can get to it from the "inspect" menu.
Some of the errors you can clear (for power and ground) by adding a "power flag" symbol to the relevant lines. You will find this in the "P" menu. Do this for all power sources.
To indicate a "no connect" pin, hover over the pin and type "Q" to place an X thing there. This is also available from the right side menu.
To avoid having difficult wires crossing others in the schematic, use global labels! These are the labeled boxes with pointers on the ends you see in all schematics. There used to be a little "A" with a pointed box around it on the right hand side for this. Now you type Ctrl-L to start the process. Actually the thing is just hidden. If you put the mouse on the A with underline below it and hold the mouse, a menu flies out with what you want.
This is easiest to do when you first place the symbol. Unless you know what libraries your part will be found in.
You can add mounting holes to the schematic (I would have thought this would entirely be part of the PCB layout), as well as to specify alignment marks. You need three fiducials minimum on each side of the board with components.
I add four 3.7mm mounting holes with pad, but no connection
#6 bolt is 3.45 inches #8 bolt is 4.12 inchesAnd we are at the end of video #1 !!
So you need to "get it right" the first time. One suggestion for sure is to zoom in when completing line connections. If you don't do this, it is easy to think a line has been connected, but there is actually a tiny gap.
The advice of sticking to a 100 mil grid comes into play here. If nothing else, it is easier to see 100 mil gaps that it is to see 50 or 25 mil gaps.
Note that the G command is very handy. Unlike M, it moves a component while keeping the wires attached. By using G, zooming in and squinting carefully, I was able to get my messy schematic nicely cleaned up.
Tips:
- Ask other people to review your schematic. - Do not cross wires - Use ground and power symbols - consider putting decoupling caps off to the side - be intelligent about where you place components - use grouping boxes with titles for complex schematics - use hierarchical sheets with a complex design - use KiCAD "inspect" -- "electrical rules checker"
For cleanup, see Part 4 below --
Tom's Electronics pages / tom@mmto.org