...
And that's how you place a part! Super easy! Now go ahead and choose a different colour button for your second one, and place it on. (It's important that your schematic is aesthetically clear. So place things nicely, and feel free to move things around). Now to make connections, you can select 'Place → Wire" or ctrl+w, then press to begin laying a wire. Altium will show you if a new connection is being made by showing a thin large red 'X' over your cursor when you hover over a possible connection. Go ahead and place wires before and after the buttons:
Connections:
As we just did, connections in Altium can be done using a physical wire connection between the two components we wish to connect. However, this is not the only way! A lot of times, for aesthetic reasons or otherwise, we cannot make a physical connection between the two components. In this case, we can use 'NetLabels'. A NetLabel allows us to make connections without using a physical wire. In fact, you've already seen NetLabels! On the connector, you see red text that describes the pin - that's a NetLabel! Not only that, but power/ground indicators (+12V, 3V3, GND) are also all NetLabels.
For instance, we know we want to connect the left side of the button to power (3V3), we also want to connect the right side of the button to an input on the MCU connector (Ignore filtering for now). We can do the following:
To place a NetLabel go to 'Place → NetLabel' or 'pn' on your keyboard. The NetLabel must be properly connected to a pin or an existing wire to properly function. All wires or pins that you want to connect using a NetLabel MUST have the same NetLabel on all of them.
Note: In Altium, any connection falls under a 'Net'. If multiple things are connected to the same connection (i.e. Ground or PA10), then they belong to the same Net.
Now in the photo above, as far as Altium is concerned, the buttons are both connected to power, 3V3 (In parallel), and to PA10 and PA09 respectively. Even if there's no physical wire connection, the connection is there and Altium is happy.
But these aren't the right connections... We need filters between the buttons and MCU. We also need to decide which pins to connect the buttons to. I'll leave it up to you to go into the datasheet and decide which pins to use (Starting page 33. We're using the LQFP48 package).
At this point you should have enough information to complete our block diagram, except for one thing: the Schmitt Trigger. We have 1-channel Schmitt Triggers in our library, but I wanna take this time to introduce you to another very important step in our development: Adding parts to our library. So, let's find and add a 2-Channel Schmitt Trigger to our library, so we can use it for our buttons.
Since finding a part can be intimidating on Digikey, we'll go ahead and find the part for you, but be sure to ask one of our leads about how we choose parts because it's very important!
We'll go ahead and use this part: https://www.digikey.ca/product-detail/en/nexperia-usa-inc/74LVC2G14GW-Q100H/1727-2072-1-ND/5221591 with the following datasheet. Now, to add this part to our library, have to do a few things:
Let's start with adding the schematic symbol. Navigate to our Schematic Library from the project finder 'Libraries → Schematic Library Documents → Schematic Documents.SchLib' and double click to open. Choose 'SCH Library' from the bottom panel, and you should see a list of all the schematic symbols for all our parts in our library.
To add a new schematic symbol, press 'Add' and put the name thats under the Description of the part on Digikey - in our case it's 'IC INVERTER SCHMITT 2CH 6TSSOP'. Then navigate to your new part and click one part, and click 'Edit'.
For the designator, input 'U?' (U is for all ICs, and the '?' tells Altium that it can be annotated with a number later in the schematic). For the description, input the 'Detailed Description' of the part as found on Digikey: "Inverter IC 2 Channel Schmitt Trigger 6-TSSOP" in our case.
Now it's time to actually draw the schematic symbol that we'd see in our schematic diagrams. We can use a simple rectangle with 'pins' to denote the different pins on our IC.
To place a rectangle shape, go to 'Place → Rectangle' and click to set the start and finish of the shape. Then to place pins, go to 'Place → Pin' and place it to look like the following (you'll have to play around with orientation and such)
(we like to keep Vcc at the top, and GND at the bottom; inputs on the left and outputs on the right)
So now this is what it'll look like on our schematic sheet when we use it. Another important step is adding the manufacturer details and supplier information to the library. Here's how we do that:
Click on 'Panels' on the bottom right of your screen and select 'Manufacturer Part Search'. This will bring up a panel on the left that you can use to link the part we found on Digikey, to the part in the Library (This is very important when we're creating our BOM when we buy the parts for the board). Copy and paste the digikey part number and paste it in the 'search' bar.
Click on the little arrow to expand the parts, then right click the part number and choose 'Add Supplier Link and Parameters to ... ". You should now see the supplier link on the bottom left panel of your SCH Library panel. Be sure to save the Schematic Diagrams.SchLib file as you make changes.- Let's now go and add a footprint for this part so we can link it to our schematic. To add a footprint, open the 'Libraries → PCB Library Documents → Footprints.PcbLib'. Open the PCB Library panel on the bottom left, and you'll see a familiar panel. We're going to use a tool to help us create the footprint easily just by inputting parameters. Go to 'Tools → IPC Compliant Footprint Wizard'.
This is a Wizard tool that we generally use for more complicated ICs and such. It's pretty easy to follow: the only thing you need is the part datasheet. Choose the SOP/TSOP option, and hit next
You'll now notice that it's asking you about measurements for the part. To find these exact values, go to page 12 (the package we chose), and fill the parameters accordingly. Be very careful and precise!
For this part, it's ok to use calculated values for most of the parameters following the initial form. However, select 'Rectangle' when presented with the pad layout (instead of Rounded). Also be sure to select 'Generate STEP Model Preview' on the bottom left corner of the wizard.
Input the same name and description as for the schematic, and click 'Finish'. The footprint is now complete, we now need to go back to our schematic, and 'Add Footprint' and choose our newly created footprint.
Our part has now been successfully added, and we can now import our library changes by going back to our schematic document, select 'Tools → Update from Libraries'. Now when we place a new part, it will show up.
Now that we've added the new Schmitt Trigger, we can finish our schematic. Do so on your own, and show one of our leads once you're finished, or ask them for help if you get stuck at any point in the process - I know that was a lot!!