Kicad 5 recipe: How to create a new component (symbol)

This is a recipe from my new book “Kicad Like a Pro” , 2nd edition. This book should be available in late 2018 in print and ebook editions. A video course is also in the works.

In this recipe, you will learn how to create a custom component (or symbol as it is also known). You use symbols in schematic diagrams that you can create in Eeschema. Much of what you will learn in this recipe you will be able to reuse for modifying existing symbols. There is a separate recipe in this book that explains how to do that.

Most likely, you want to create a custom schematic symbol because you have a physical component but can’t find an existing symbol to represent it. Perhaps you have searched through the symbols that come with Kicad, and Googled for suitable third-party symbols, but couldn’t find any.

It is also likely that you will want to associate your new symbol with a footprint. If your physical component has a standard package, like DIP, for example, then you will be able to associate an existing footprint with your custom symbol. If not, you will also need to create a custom footprint. You can learn how to do this in the relevant recipe, also available in this book.

In this recipe, you will learn how to create a custom symbol by creating a symbol for the 555 timer integrated circuit. There are plenty of libraries for Kicad that contain this symbol, but for the sake of learning, let’s pretend that we can’t find it.

What we want to create is a symbol like the one in Figure 1.

Figure 1: A custom-made symbol for the 555 IC

Figure 1: A custom-made symbol for the 555 IC 

Our objective is to create a symbol that complies with convention. In regards to IC symbols:

  1. We arrange pins around a rectangle.
  2. We group pins according to function (like inputs, outputs, power etc.)
  3. We place the Vcc pin on the top of the rectangle.
  4. We place the GND pin on the bottom of the rectangle.
  5. We choose an appropriate name and designator for the symbol. Symbol designators are standardised; you can learn more about them here.

The physical component that we are working with is in Figure 2. This component comes in a standard DIP package with 8 pins.

Figure 2: The physical component is a 555 timer in a DIP package with 8 pins

Figure 3: The physical component is a 555 timer in a DIP package with 8 pins 

Because we are working to create a symbol, we don’t need to know anything about the physical characteristics of the physical component other than the total number of pins that its package contains. You need to know details about the physical characteristics are essential when you are working on the footprint of the component.

However, it is beneficial if you have access to the components data sheet. The data sheet contains information that you need: The names, numbers, and roles of each pin, whether they are input, output, bidirectional, power, signals, etc. All this is useful information, and the more you have on hand, the better.

The data sheet for the example component is available from its manufacturer. The information you need is on page 6, and I have included it in Figure <$n:figure:P5_symbol_datasheet> for your convenience.

Figure 3: Pin configuration and functions from the IC’s datasheet

Figure 4: Pin configuration and functions from the IC’s datasheet 

Let’s start the process of creating a new symbol. In the main Kicad window, click on the Symbol Library Editor button.

Figure 4: Start the Symbol Editor

Figure 5: Start the Symbol Editor 

You must store each symbol inside a library file, so before you start creating the symbol create a new library. Create a new library by clicking on the “New library” button or through the File menu.

Figure 6: Create a new symbol library; I have placed mine in a directory named “Custom libraries

Figure 6: Create a new symbol library; I have placed mine in a directory named “Custom libraries

Kicad will ask you if you would like this library to be available to all projects (“Global”) or only to the current project (“Project”). Choose the most appropriate one for your circumstances (I chose “Global”). You are now working in the new library, and you will store the new symbol in it. You can confirm this by looking at the header of the Editor window. The path and name of the library you just created must be showing there.

Next, click on the “Create new symbol” button in the top toolbar.

A prompt will ask you to select the library in which you will store the symbol. The library you just created should be listed. Click on it to select it and click “ok” to continue. The Symbol Properties window will show up. The most important values that you need to complete are the symbol name and designator. The name typically consists of the physical component’s model name and any other information that helps to identify it. When you use it later, you have to search for it in the symbol library and having a good name will help you find it quickly. In my example, because I want to differentiate my 555 symbol to those that exist in other libraries, I add my initials “PD” at the end of the name.

For the designator, you should not guess. Visit Wikipedia to see the Reference Designators table. You can see a section of this table in Figure 7. The designator for integrated circuits is “U,” so type this in the Default Reference Designator field.

Figure 7: A section of the reference designators standard IEEE 200-1975/ANSI Y32.16-1975

Figure 7: A section of the reference designators standard IEEE 200-1975/ANSI Y32.16-1975

Figure 8, below, shows the values I have entered in the Symbol Properties window. Other than the symbol name and the designator, everything else remains as per the default.

Figure 8:The properties for the new symbol

Figure 8:The properties for the new symbol

Click Ok to commit and continue. Kicad will place the designator and symbol name in the middle of the sheet, on top of the other. Use the “M” hotkey to relocate the two blocks of text. You should have something similar to the example in Figure 9.

Figure 9: An empty new symbol

Figure 9: An empty new symbol

Continue by drawing the outline of the symbol. You can either use the polygon tool:

… or the rectangle tool:

… to do this. Your outline should like like the example in Figure 10.

Figure 10:The outline of the footprint

Figure 10:The outline of the footprint 

Add the background color that is consistent with other IC symbols by opening the drawing properties window for the rectangle (place your mouse pointer on the rectangle line and type “E”). Under “Fill Style”, check the “Fill background” radio button (Figure 11).

Figure 11: Fill the rectangle backgroundFigure 11: Fill the rectangle background 

Next, work on the pins. Keep the datasheet open because you need the information in it. For your convenience, refer to the excerpt in Figure 4. Click on the pin button in the right toolbar:

Place the 8 pins around the perimeter of the symbol outline, as in the example of Figure 1. The thing to remember here is that the convention is to group similar pins together and place the two power pins to the top and bottom of the rectangle. Let’s start with the Vcc pin. According to the datasheet, the Vcc pin is number 8, and according to the convention, it should go to the top edge of the rectangle. Click on the pin tool, and then click in the middle of the top edge. The Pin Properties window will come up. Fill it as you can see in the example in Figure 12.

Figure 12:The Vcc pin properties

Figure 12:The Vcc pin properties 

In Figure 12, the fields inside the box are the ones that you need to focus on. The pin name is arbitrary, but of course, you should use a name that is appropriate. I usually use the same name that I see in the documentation for this pin. The Pin number, on the other hand, is very important. The Pin number is how schematic symbols and footprints can associate physical and symbolic pins. When you design the custom footprint for this physical component in the “Creating new footprint” recipe, it is the number that you put in the Pin number field that dictates which net in the schematic diagram connects to the correct pad in the footprint. Take the pin number for the Vcc pin from the documentation (“8”) and type it in this field.

In the orientation drop-down, select the option that matches the side of the rectangle where you are attaching the pin. The Vcc pin should go on the top of the rectangle and should have its circular connector pointing away from the rectangle. The horizontal line of the pin orientation icon represents the rectangle. If you wanted to place the pin on the left of the rectangle, you would choose the icon with the circular connector printing towards the left.

Finally, because the Vcc pin is a power pin, I have selected the “Power input” electrical type. You should choose the same type for the GND pin.

Click Ok to commit the changes. Please the pin in the middle of the top side of the rectangle, as you can see in Figure 13. I have moved the text block so that they don’t overlap with the pin.

Figure 13: The Vcc pin, in place

Figure 13: The Vcc pin, in place

Follow the same process to add the GND pin (pin 1) in the bottom edge of the rectangle. Copy the pin name and number from the datasheet, and mark it also as a Power Input.

Continue with the left side of the rectangle where you should place the input pins. According to the datasheet, the input pins are RESET, THRES, TRIG. There is one bidirectional pin, “CONT,” which you can place either on the left or the right of the rectangle. I have placed it on the left. Your symbol should look like the example in Figure 14.

Figure 14: Input pins are placed on the left side

Figure 14: Input pins are placed on the left side

The pin attributes for the input pins on the left of the symbol look like the example in Figure 15. Remember that pin 5 is bi-directional so its electrical type should be “bidirectional”.

Figure 15: The input pin attributes

Figure 15: The input pin attributes

Continue in the same way to create the last two pins. Those are output pins, as per the datasheet. Use the pin names and numbers as those appear in Figure 4 for pins 7 and 3. When completed, you should have a symbol that looks like the example in Figure 16.

Figure 16: The datasheet is very useful to have readily availableFigure 16: The datasheet is very useful to have readily available

Your work is complete. Save the symbol to the selected library by clicking on the Save Current Symbol button:

Then, test that you can use it in Eeschema. Open Eeschema. Go into Symbol Libraries from the Preferences menu and add the new library (read the relevant recipe if you don’t know how to do this). Place your cursor on the Sheet and type “A” to add a new symbol. Search for the name of your library by typing part of its name in the filter field (Figure 17). The library should appear. Double-click on the symbol to drop it on the sheet.

Figure 17: Find your new library and symbol

Figure 17: Find your new library and symbol

The custom 555 symbol should now be in place inside Eeschema, and you can go ahead to use it as you do with any other symbol ( (Figure 18).

Figure 18: Your new custom symbol in Eeschema

Figure 18: Your new custom symbol in Eeschema

In this recipe, you learned how to create a brand-new symbol. What if you have found a symbol that is close to what you want, but could be perfect with a bit of tweaking? In other words, what if you want to modify an existing symbol? You can learn how to do this in the “Modifying an existing component (symbol)” recipe, also available in this book.

Related Articles

>