1 - Introduction

Schematics are the basis of any kind of circuit design. Schematics define the components in your circuit and their connections to each other. In PCB design, schematics are necessary before moving onto the PCB layout, as the CAD software (i.e. Altium) will use your schematic to make sure you’ve connected your circuits on the layout exactly as you specified in the schematic.

Before you can actually start drawing your schematic, you need to figure out how your circuit will work.

2 - Schematic Theory and the Datasheet

Figuring out how your components are connected will require reading through the datasheet for your non-passive components (i.e. your ICs) and understanding how they work. You won’t have to read through the entire datasheet page-by-page, but there are a few sections you should read carefully and understand as much as possible to ensure you implement the circuit correctly. Here are some sections in the datasheet to look for:

• Typical Application Circuit: Most datasheets will have this at the very beginning or in various parts of the Application Information section. These schematics are good to use as a general reference, but do not simply copy these circuits. You need to understand why components are selected and connected the way they are, which will require reading through other sections of the datasheet

• Pin Descriptions/Configurations/Functions: The name can vary depending on the manufacturer. You probably will have already gone through this while designing the symbol and footprint. This section describes the function of each pin, and will usually label specific requirements for some of the pins. Reading through this section will help you figure out what connections are a must for a good portion of the pins

• Absolute Maximum Ratings and Typical Operating Conditions: Every datasheet should have this. It is extremely important to ensure that your circuit does not violate the absolute maximum ratings, and it should be used within the typical operating conditions. The typical operating conditions can also provide a picture of the typical outputs and power requirements of a component, which can help in determining the capabilities of the circuit and if it’s suitable for your project

• Application Information: Every datasheet should have a section titled something similar to this. This section explains all the different functions and behaviors for the component. It’s important to read through this to understand what your component can do and what features you want/need to implement, as well as how to implement them

Most datasheets will have a table of contents near the beginning that will outline where to find these sections. To provide an example, a screenshot from a Texas Instruments datasheet with some of the relevant sections highlighted is shown below.

Open

It’s a good idea to make rough notes and calculations somewhere, such as an Excel sheet, when figuring out the required component values and connections. This way you can keep track of your thought process and also more easily explain to those reviewing your schematic what your design decisions were.

After you’ve understood the datasheet and figured out how to wire up your components, it’s time to actually create the Altium schematic.

3 - Creating a Schematic File

Schematics are made up of one or more schematic files (or schematic sheets). At WARG, we have templates available for schematic sheets that include the WARG logo, address, and other information so that all our projects have a consistent style once you are done with the bootcamp. To create a new schematic file, click File > New > Schematic.

4 - Placing Components

Now it’s time to place the components you selected previously. From the hotbar at the top, click on the Place Part button. The Components pane should open up on the right with all the parts in your schematic symbol library. Scroll through the list of parts or search for the components you created from the top, double click on a component to grab it and then click somewhere on the schematic to drop it in.

Open

You can follow the guide below to make your own custom components as well!

Schematic Symbol and Footprint Guidelines

You’ll notice that each part you place has a symbol on top of it that looks something like U?, R? , C?, etc. This is the designator, which is a short text string to identify each component. Every component needs a unique designator, so you’ll need to modify all the designators to replace the question mark with a unique number. This is done by double-clicking a designator to modify its value. Alternatively, you can use Altium’s Annotation tool to automatically do it for you (Tools > Annotation > Annotate Schematics, then click Accept Changes (Create ECO)).

5 - Wiring up your Schematic

With your components placed and annotated, you can begin wiring everything up according to the circuit you figured out from the datasheet. There are a couple of tools you have available to wire things together:

• Wire: Click the Wire button from the hotbar or use Ctrl + W, then click to draw wires to connect different pins and things together. A wire is the simplest way of indicating two pins or nets are connected to each other.

• Power Ports: Use Place > Power Port, or click the Place GND Power Port button from the hotbar. Power ports are special symbols that should be reserved for voltage rails (i.e. 3.3V, 5V) and GND. All pins and wires that connect to a power port will be considered by Altium as connected to all other pins and wires that connect to a power port with the same name. This makes it easier to wire up your voltage rails and GND connections. Keep your power port names very short and to the point. Also note that you cannot use decimals for global port names, use a V instead as the decimal point (i.e. for 3.3V, write it as 3V3). For voltage rails, use the Bar symbol and for GND, use the Power Ground or Signal Ground symbol.

• Net Labels: Use Place > Net Label. Net labels do exactly as they say: they label a net with the name of your choosing, making it clearer what each specific connection is. However, you can also use net names to connect pins and ports without wires. By placing a Net Label on your wires, all wires with the same Net Label will be considered as connected to each other by Altium. This can help reduce the number of wires crossing over everywhere in your schematic, making it more organized and easier to read. Be sure to use clear, descriptive net names using snake case and capital letters (i.e. EN_INPUT, PWM_OUT, etc.). The full guidelines that WARG uses for labeling nets can be found here Net Naming Guidelines . Please use this for all nets.

• Ports: Use Place > Port or click the Place Port button from the hotbar. Ports are used to make connections between different schematic sheets, since wires cannot cross over into other schematic files. Ports with the same name will be considered by Altium as connected. Use the same naming convention as the Net Labels, and if possible use the same name as the Net Labels. Note that the bootcamp schematic is simple enough to fit on a single schematic page, so you shouldn’t need to use ports here, but it is still important to know how to use them for future projects.

• Generic No ERC: Use Place > Directives > Generic No ERC. This tool has multiple uses, but the main one you’ll be using it for is to indicate unconnected pins. It is important to do this in order to indicate both to Altium and design reviewers that you intentionally left certain pins unconnected, if it is necessary to leave a pin floating. You will see why it is important to flag this for Altium in the next section.

There are other tools available for wiring up schematics in your hotbar and Altium menus, but these aren’t necessary for the bootcamp and typically aren’t necessary until you start working on more intermediate or advanced projects.

6 - Validating your Schematic

The final step for making your schematic is to have Altium check your schematic for errors. This won’t guarantee that your schematic is 100% correct, but it can be used to catch some easy-to-fix mistakes. To run Altium’s error-checking, click Project > Validate PCB Project <name of your project>.PrjPcb. Altium will then display all the errors and warnings it found for your schematic in the Messages panel. Some examples of the errors and warnings it can find are:

• Unconnected pins/nets with only one pin (if they don't have the Generic No ERC symbol on them)

• Multiple net names on one net

• Duplicate designators for components

• Multiple input/output pins on a single net

Although you should fix all the errors that Altium finds, you probably will not have to fix every single warning that it finds. Some warnings (such as multiple input/output pins on a single net) may be intentional and required by your design, and as long as you can justify and are reasonably sure that the connections are correct, you do not need to worry about fixing every single warning. If you’re ever unsure what an error/warning means, how to fix it, or whether you need to fix something or not, ask!

Once you’re happy with your schematic, it’s time to move on to routing and layout!