SCH Library

Parent page: Panels

Interactively browse, view and edit Schematic Library components and their pins.

Summary

The SCH Library panel enables you to browse through, and make changes to, the components stored in the active schematic library document. The panel also offers the ability to pass on any changes made to components in the library directly to the current schematic design document.

Panel Access

The SCH Library panel will automatically open when a Schematic library is the made active document in the editor. Otherwise, when a SCH Library is the active document in the editor, the SCH Library panel can be accessed from the menu's View | Schematic |  button.

Panels can be configured to be floating in the editor space or docked to sides of the screen. If the SCH Library panel is currently in the group of docked Workspace panels on the left, use the SCH Library tab located at the bottom of the panels to bring it to the front.

Library Browsing

The body of the SCH Library panel has two interactive list sections to access the components and their pins in the active SCH Library:

• Components – The list of all components in the active library document with the associated descriptions.
• Pins – A list of all the pins that have been placed and defined for the selected component.

As you click on a component entry in the Components list, it will become the active part in the design editor window. Selecting a Pin object in the panel causes the corresponding graphical object to be highlighted (and zoomed) in the editor workspace. In this way the SCH Library panel offers a fast and easy way to browse, view and access SCH library components and pins.

Filtering Content

The contents of the Components list can be filtered, enabling you to quickly find a particular component within the library. This is especially useful if the library contains a large number of items. Filtering can be applied using one of the following two methods:

Indirect Filtering

This method uses the field at the top of the panel to filter the contents of the list. The name masking is applied based on the entry in the field. Only those components in the list targeted by the scope of the entry will remain displayed.

The filtering feature is not case sensitive and supports 'type-ahead' functionality, meaning that the content of the Components list is filtered as you type.

Use the * wild card operator for more elaborate filtering. For example, typing MAX* will display only components whose names begin with MAX. Or as in the image below, typing *13 will display only components where the body of the name contains 13.

Direct Filtering

This method is available for both list regions in the panel and allows you to quickly jump to an entry by directly typing within the area of the list. Masking is not applied, leaving the full content of the list visible at all times.

To use the feature for quickly finding a component, click inside the Components section of the panel and type the first letter of the component you wish to jump to. For example, if you wanted to quickly jump to component entries starting with the letter F, you would press that letter on the keyboard. The first component in the list starting with F would be made active.

If there are multiple components starting with the same letter and especially if the library is particularly large, type further letters to target the specific entry you require - for example; MAX1112 as illustrated by image below which highlights the first of the MAX1112 series in the list.

Combination Filtering

In some situations it may be helpful to use Indirect and Direct filtering together. If for example, you recall that the component you want to locate has a sub-type variant of +T and a prefix of MAX1112, this information can be used as Indirect (Mask) and Direct entries respectively, as shown in the image below.

Zoom Controls

To the immediate right of the filtering field, is the  control. Clicking this gives access to a pop-up window presenting a choice of options to control the zoom behavior, when displaying a selected component in the main design window.

Control how components are zoomed in the main design window, as you switch components in the panel.

Choose from the following options:

• Do Not Change Zoom Between Components - choose this option to keep the same level of zoom between components as you browse. Whatever manual level of zoom you define while browsing one component will be adopted for all other components you subsequently browse.
• Remember Last Zoom For Each Component - choose this option to retain the zoom level applied to each component you have browsed. In other words, the view of a component will appear just as you last viewed it.
• Center Each Component in Editor - choose this option to zoom and center each browsed component, in the main design window.
  • Zoom Precision - use this slider to define the level of zoom. Slide to the right for a more zoomed-in view of a component.

Panel sections

Components list

As you click on an entry in the Components list, it will become the active part in the design editor window, and also for the four buttons directly beneath the list. These buttons provide the following commands that can be used with respect to the list of components:

• – Place the active component onto a schematic design document. When clicked, the schematic document that is used will depend on whether or not any schematic documents are currently open:
  • If there are no schematic documents open, clicking the button will cause a new schematic document to be created and made the active document in the design editor window. The active library component will appear floating on the cursor, ready for placement.
  • If one or more schematic documents are currently open, the last document to have been active (irrespective of the project it belongs to) will be made the active document in the design editor window and the active library component will appear floating on the cursor, ready for placement.
• – Add a new component to the library document. The New Component Name dialog will appear. Enter the required name for the new component and this will be added to the list, and a blank sheet will be opened in the design editor window ready for you to define the component.
• – Permanently delete the selected component(s) from the library document. A confirmation dialog will appear asking for verification of whether or not to proceed with the deletion
• – Open the Library Component Properties dialog, from where you can view/edit properties associated with the active component. The dialog also provides access for creating links to new models or editing existing ones. Double-clicking on a Component entry will also open the Library Component Properties dialog.

In the Models area of the dialog, click the Edit button to open the PCB Model dialog, which provides access to the PCB model linking for the current schematic component. Select the Add button to add a new PCB model.

Pins list

The Pin List section of the panel lists all of the pins that have been placed and defined for the active component. Each entry in the list contains the pin number, any name that has been defined for the pin, its electrical type and, where footprint models have been linked to the component, the corresponding pin in the model that this pin maps to.

As you click on an entry in the list, the corresponding pin graphic will be centered and selected in the design editor window.

Double-clicking on a pin entry in the list, or selecting the entry and clicking the button below the list, will open the Pin Properties dialog, from where you can view/modify the properties of the pin as required.

To add a new pin from the panel, click the button beneath the pin list. The pin will appear floating on the cursor within the design editor window. Position the pin as required and click to effect placement. Continue placing additional pins or right-click or press ESC to exit pin placement mode.

To delete one or more pins, select the required entries in the list and press the button. The pins will be removed from the list and deleted from the symbol's graphic.

Changing the Panel Display

The Components section of the panel is always displayed, however the Pins section can be set to be displayed or hidden. This is achieved using the associated button located to the right of a panel section:

• When the Pins section is currently displayed, the button will appear as – which will hide the section when clicked.
• When the Pins section is currently hidden, the button will appear as  – which will display the section when clicked.

Right-Click Menus

Right-clicking on an entry in the Components list will pop-up a menu of commands.

The commands are as follows:

• Select all - quickly select all component entries in the list.
• Update Schematic Sheets - pass on all changes made to components within the active library document to all open schematic design documents. All instances of changed components that exist on the design documents will be updated.
• Copy - place a copy of the selected component(s) onto the Schematic Library Editor's internal clipboard
• Cut - place a copy of the selected component(s) onto the Schematic Library Editor's internal clipboard and then permanently delete the component(s) from the library. A confirmation dialog will appear asking for verification to proceed with the deletion
• Paste - paste a component from the Schematic Library Editor's internal clipboard into the active library document
• Delete - permanently delete the selected component(s) from the library document. A confirmation dialog will appear asking for verification of whether or not to proceed with the deletion.

Notes

• Options for the library workspace can be configured in the Library Editor Workspace dialog: Home | Library » Options.
• Standard Ctrl+click and Shift+click functionality is supported for selection of multiple entries in a list.
• The active component is that whose symbol is currently displayed in the design editor window.
• Ctrl+click over a selected entry in a list to deselect it.
• The keyboard shortcuts Up Arrow, Home, End and Down Arrow, can be used to display the previous, first, last and next entry in a list region, respectively.
• Multi-part components appear in the list with a + symbol (expandable) next to them. Each part is listed as a sub-entry below.
• Data may be sorted by any column by clicking on the header for that column. Clicking once will sort in ascending order. Click again to sort by descending order.
• You can change the order in which columns of data are displayed. To move a column, click on its header and drag it horizontally to the required position. A valid position is indicated by the appearance of two green positional arrows.
• The component that you paste into the active library document can originate from either a schematic design document or another schematic library document.
• If multiple components have been copied to the clipboard from the main design in the Schematic Editor, all components in the selection will be pasted into the library document.
• If the same component is pasted into the library more than once, or if more than one new component is added to the library without renaming, the copies are distinguished by the suffix _1, _2, _3, and so on.
• A schematic design document must be open in order to pass on changes made to components in the library document.
• For a multi-part component, the corresponding pins for the active part will be highlighted with a white background in the Pin List section of the panel. All pins of other parts will be lowlighted with a grey background. You are, however, still able to edit the pins of these non-active parts.
• As you select pins in the design editor window, the corresponding pin entries will be selected in the panel.
• The attributes of pins and other graphical objects used to define the component can be edited using the SCHLIB Inspector panel. Objects must be selected first in order for the panel to display the attributes.
• When a new schematic library document is created the panel will, by default, contain a single, blank component - Component_1.