A component in a schematic is an instance of a symbol from a symbol library. They can represent subcircuits to be included in the design, or discrete parts or devices to be used.

To add a component to a schematic page, press <I> or select Add→Component… to bring up the “Select Component…” window. The window has three main areas:

• The library area is on the left side of the window, and allows you to choose a symbol to place on the schematic page.
• The preview area is on the right side of the window. This shows a picture of the chosen symbol, and its attributes.
• The insertion mode menu at the bottom of the window controls how components are inserted.

By switching to the In Use tab of the component selector, you can view a list of the symbols that have already been used in the schematic. To select a symbol from the list, left-click on it.

If the list needs to be updated, click the Refresh button at the bottom of the “In Use” page.

To select a symbol from a symbol library, switch to the Libraries tab of the component selector. This shows a list of available libraries. To view the symbols in a library, double-click on the library's name, or left-click the arrow next to it. To select a symbol from the list, left-click on it.

Alternatively, you can search all available symbols by typing into the Filter box at the bottom of the Libraries page.

The list of libraries and symbols may need to be updated (for example, if you modified a symbol library while gschem was running). To update it, click the Refresh button at the bottom of the Libraries page.

When you have selected a component, left-click in the schematic view area of the main window to add it to the page. You can continue to click to place copies of the same component, or right-click to finish placing.

To hide the “Select Component…” window while you place components, click OK. When you right-click to finish placing components, the window will re-appear.

There are three ways that gschem can insert a symbol into a schematic:

1. As a component linked to a symbol in the symbol library (Default behavior - reference component). This is the default method, which ensures that when you update a library symbol, all the places it was used are updated too.
2. As a component with the symbol data copied into the schematic (Embed component in schematic). If you embed the symbol, it is easier to share your schematic with other users without having to set up the same symbol libraries.
3. As individual objects obtained by breaking the symbol apart (Include component as individual objects).

You can make a linked component embedded by selecting it and using Edit→Embed Component/Picture. To make an embedded component linked, use Edit→Unembed Component/Picture.

If you wish to update an embedded component after making changes to the original symbol file in the library, use Edit→Update Component.

To edit a component's symbol file, select the component and use Hierarchy→Down Symbol. gschem will open and display the symbol page for editing. When you are finished editing, save the file and use Hierarchy→Up to return to the schematic. You may need to use Edit→Update Component for your changes to be reflected in the schematic view.

If, when loading a schematic, one of the symbols it needs cannot be found in the available symbol libraries, a warning graphic will be displayed in its place.

A component may have a datasheet or other documentation associated with it. To view a component's documentation, select it and use Help→Component Documentation.