Adding Components to a Schematic
You can keep working with your project or open it from the Workspace and continue from where the previous step is completed.
To download the project, use the buttons shown in the figure below.
The schematic sheet that we will create will look like this.
It consists of a small number of elements. Here is the whole list, in respect of their manufacturer part numbers and designators:
C1005X7R1H104K050BB - C1, C2, C3, C4, C5, C8, C9, C12;
GRM21BR61C475KA88L - C6;
04025A120JAT2A - C7, C10;
TAJA106K016RNJ - C11;
LTST-C190GKT - D1;
1N5819HW-7-F - D2;
629004113921 - J1;
RT0402BRD072K2L - R1, R2;
ERJ-2GEJ331X - R3;
ERJ-3GEY0R00V - R4;
RC0402J330CS - R5;
CY7C68023-56LTXC - U1;
MT29F8G08ABACAWP-IT:C - U2;
TPS78833DBVR - U3;
ABM3B-24.000MHZ-B2-T - X1.
All these components are already at your disposal. In order to place them, you need to open the Components or Manufacturer Part Search panel. They are opened using the Panels button at the bottom right of the application window.
In order to search for a component, it is enough to enter its part number (as listed above) in the Search field. Right-click on the found component and place it on the schematic sheet using the Place button.
When positioning a component, you may need to use the following shortcuts:
- Spacebar to rotate the component by 90 degrees.
- X or Y (at the time of component movement!) to mirror the component on the corresponding axis.
Note: If you need to add a component that is already in your schematic, there is no need to search for it in the library. Clone an existing component as follows: select and hold the component with the mouse, press the Shift key and start moving it.
All the component properties can be found in the Properties panel when the component is selected in the design space. The panel can be accessed as described above. Place the components on the schematic sheet as shown on the image above. After completing this step, save the changes locally (File » Save All) and to the Workspace (Save to Server).
Note: Do not spend time aligning components manually. Select components and use the Align function ( A button on the keyboard) to align them quickly, or place them on the grid!
Now we need to assign designators to the components to complete the schematic. To do this, use the Tools » Annotation » Annotate Schematics command. You can learn more about this tool here.
Click Update Changes List followed by Accept Changes (Create ECO). Then the dialog appears, where you need to Validate Changes, then to Execute Changes.
Note: In case you have deleted or added new components after the numbering of components in the schematic, it is not necessary to enter the Tools » Annotation » Annotate Schematics settings. The program remembers all the last settings applied to the current schematic sheet and it is enough to apply the following commands:
- Tools » Annotation » Reset Schematic Designators – if necessary, reset all values of Designators
- Tools » Annotation » Annotate Schematics Quietly – to quickly assign Designators to components that do not have a number, according to the settings previously applied to this sheet.
Save the changes locally (File » Save All), and then to the Workspace (Save to Server).
