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:
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:
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.