Library Management / Local Library and Symbol Creation
Click if you find this content useful

Library Management

Local Library and Symbol Creation

In a previous chapter, we started to create a component that can be used with Altium 365 technology. We understand that you might want to use local libraries as you used to, but we strongly recommend that you use Altium 365 because it gives you a wide range of new features when working with components. This chapter shows an example of how to create a symbol and footprint in a local library. In the scope of this chapter, we will create a SchLib with a symbol for our component and in chapter 5.4 we will create a PcbLib with a footprint for it and complete the component creation. 

We will create a transistor pack MBT3904DW1T1G consisting of two transistors in one 6-TSSOP package. It is best to make a symbol for this component using the multi-part feature.

Select File > New > Library > Schematic Library from the main menus to create a new local schematic library. The symbol editor will open in your design space. Open the Properties and SCH Library panels if they are not already open.

Creating a schematic library
Fig. 1 - Creating a schematic library

We need to define a name for the symbol and component. In the Design Item ID field (the name of the symbol) of the Properties panel, enter MBT3904DW1T1G. This name will be used when searching for the component in the Components panel.

Enter Q? in the Designator field. This field is used when annotating components and differs for each component type. The first letter represents a common component type, such as C for Capacitors, R for Resistors, etc. A question mark after the letter is used to define the variable numeric part of the component. After annotation, the question mark becomes the unique component identifier number, such as Q5, which is mandatory for the next steps of the design process.

Enter Dual General Purpose NPN Transistors, 40V, 0.2A, SOT-363 in the Description field. This field is shown by default while searching for components in the Components panel so it can be helpful to enter all the important values to make searching more precise.

Properties of the component being created
Fig. 2 - Properties of the component being created

When a component has different functional groups or repeating identical parts (e.g., resistor and transistor packs), it is more convenient to implement it with a multi-part component. In this case, the component MBT3904DW1T1G consists of two NPN transistors, which are more convenient to present in the form of such a symbol. Let's add the second functional part of the symbol.

In the SCH Library panel, select the MBT3904DW1T1G component then select Tools > New Part from the main menus. An Arrow Icon icon appears at the left of the part name in the Design Item ID column. Click on it to expand the symbol and show all its parts. Select Part A to make that part active.

A new part has been added for the symbol
Fig. 3 - A new part has been added for the symbol

Select Place > Pin from the main menus to start pin placement. Press the Tab key to open the Properties panel to edit the properties of the pin being placed. In the Properties panel, define the Designator as 1 and Name as E. Click the visibility icon to the right of the Name field to hide the name. In the Electrical Type drop-down, select Passive then enter 200 mils for the Pin Length. In the Font Settings region, enable Custom Settings in the Designator region then use the drop-down to select Arial for the Designator. Click the pause button in the design space then place the pin as shown in the figure below using the Spacebar to rotate the pin.

The first pin is placed in the center of the crosshair by the wire connection point.
Fig. 4 - The first pin is placed in the center of the crosshair by the wire connection point.

Warning: Always pay attention to the direction of a placed pin. The connection point of a pin is determined by a small gray crosshair attached to the mouse cursor and by four small white points on the placed pin. If you place the pin with the wrong connection point direction, it will be impossible to connect a track to it.

Connection point of the placed pin
Fig. 5 - Connection point of the placed pin

Place two more pins as shown in the figure below. Set B as the name for pin number 2 and C as the name of pin number 6. Hide both names using the approach described above.

Tip: You can place pins with the same properties quickly by copying and placing pin 1 twice then changing the designator and name values of the copied pin(s).

Pins 1, 2 and 6 are placed.
Fig. 6 - Pins 1, 2 and 6 are placed.

The graphic part of the symbol can be formed by the placement of any graphical primitives, such as lines, rectangles, arcs, and polygons. Using Place > Line from the main menus, draw three lines as shown in the figure below. To place the lines at an angle, use the Spacebar to change the drawing mode.

After placement, select all drawn lines and define their color as blue using the Properties panel. Right-click to finish line placement.

Tip: Grid size can be switched by pressing the G key.

Lines for transistor symbol are drawn.
Fig. 7 - Lines for transistor symbol are drawn.

Now we will add the last detail - an arrow indicating the type of transistor. In this case, it is an NPN transistor, so the arrow must be placed in the direction of the emitter, which is represented by pin 1. Select Place > Polygon from the main menus. Press Tab to open the Region mode of the Properties panel then define the parameters as shown in the figure below.

Properties of the created polygon
Fig. 8 - Properties of the created polygon

Using the G shortcut key, change the grid to 10 mil then draw an arrow as shown in the figure below.

Part A of the symbol has been created.
Fig. 9 - Part A of the symbol has been created.

The first part of the symbol is finished and now we need to finish Part B to make the symbol complete. Select all primitives in Part A and copy them. Select Part B in the SCH Library panel and place the copied primitives. To complete the symbol, do the following in Part B:

  • Change Pin 1 designator to Pin 4
  • Change Pin 2 designator to Pin 5
  • Change Pin 6 designator to Pin 3
Part B of the symbol should now look like the figure below.
Part B of the symbol has been created.
Fig. 10 - Part B of the symbol has been created.

 

Symbols for our component have been completed, so we can save the schematic library. Select File > Save from the main menus and save your library to a convenient location. Our component is not complete yet since we have no footprint for it. A footprint with the corresponding PCB library for this component will be created in Chapter 5.4. Leave this tab open in order to have quick access to it in Chapter 5.4.

Tip: You can add new symbols to your library by clicking the Add button below the footprint list in the SCH Library panel.

Was this article useful?
Yes No
Thank you Glad to hear it