Insert Component (SCM)

Use this option for adding new components or gates to a Schematics design from a library.

Shortcuts

Default Keys: None

Default Menu: Insert

Command: Insert Component

How To Insert A Component

1. Select the Component option on the Insert menu, or use one of the above shortcuts.

2. Setup the Insert Component Dialog:

   • Set which parts library you wish to add from. A list of part names will appear in the dialog. Use the filter to reduce this list to the parts that you are interested in.
   • Choose which part you wish to add from the list or use the Find button to locate the part based on more advanced criteria.
   • Select which of the part’s footprints you require (if more than one available). If possible, this footprint will be used when using Translate To Pcb at a later stage. The chosen footprint may be reviewed if you have enabled the dual Schematic & PCB preview option.
   • Change the component name (if the default provided is not suitable).
   • If the part has multiple gates, the gate to be added is highlighted in the select colour and its gate identifier is shown in the dialog. If it is not the one you want to add, choose an alternative from the dropdown list.
   • Select which of the part’s schematic symbols you require (if more than one available). Optionally the chosen symbol may be reviewed if the Preview option is enabled.
   • Choose to add the part (or a number of copies of it) straight to the Component Bin, or to add a component or gate interactively into the design.

3. Use the Add button to add the component(s) to the design. If adding to the bin then you are returned immediately to the dialog, else follow these next steps.

4. Using the mouse, move the component or gate to the desired position and click to place it into the design.

5. Continue to place components or gates using the same part. Each next component’s name is auto incremented to the next free name in the design, or if adding a gate to the next free gate in the design.

   Press the Esc key, or cancel using the shortcut menu, to return to the add component dialog.

How To Use The Insert Component Dialog

Look In

Use this to choose a parts library to search for the required part. The library list is set up in Library Folders in the library manager. Two special entries exist:

Use [All Libraries] to choose from parts in all of the parts libraries. If the same part is in more than one library, the first found will be used, so library order is important.

Use [Current Design] to choose from the parts already added to the design.

Which Parts

Use the Filter box to enter a string containing the wildcard characters to filter the list to only match certain names e.g. “74LS*“. Use the No. Pins box to limit the matching parts to those of a set number of pins (blank means any pin count). press Apply to alter the list of parts names accordingly. By checking the Include Connectors box, you can also use this dialog to add connectors (as an alternative to using the Insert Connector Pin command). The number that matched the filters is shown in the dialog.

Part

This listbox contains the part names to choose from. Select the one required. The number of pins on the selected part is displayed in the Pins box.

Pins

This is a non-editable field that informs you as to the number of pins that selected part contains.

Desc (Description)

Displays the full description of the selected part.

Find

If you do not know exactly the name of the part to use but know some of it, or know the values of some of its attributes, use the Find button to locate it. The Find dialog will be displayed allowing you to search all libraries in the library folders for the required part. This dialog allows you to search using several different criteria. You can search by part name, including wildcard characters. You can search on the number of pins on the part. You can also search for parts containing a particular named attribute, again using wildcard characters on the value. A list of parts matching the search criteria will be shown in the dialog. Selecting the required part will change the Insert Component dialog to show the chosen part.

See the help section Find Library Item for details on how to use the Find dialog.

Family

Displays the name of the part family that the selected part is a member of. If the part is a member of a family it can be changed to any of the alternate family members easily using the Next Part Alternate command.

Footprint

This lists the alternative footprints that the chosen part can use when added to the PCB design. Select the footprint required.

Name

Enter the unique name for the component. The default name is created by adding a unique number to a stem taken from the part. This default name will not already exist in the design, or if adding gates it will not have all of its gates used in the design.

Name Ranges It is possible to add a set of similar components to be used, for example, as decoupling capacitors. This is done using the name range syntax defined in the Design Settings dialog. When such a component is converted to the PCB it is expanded to the correct number of components.

Symbol

This lists the symbols that can be used to represent the component or gate in the schematic design. If an alternative to the default is required, select it from the dropdown list. If the part has multiple gates the symbol selection applies to the currently selected (and highlighted) gate.

Gate

Only shown if the chosen part has multiple gates and you are not adding to the component bin (only whole components may be added to the bin).
The default gate identifier is the next free gate of this type that is not yet used in the design. For example, if U1-A and U1-B are already placed on a sheet in the design, then U1-C will be the default name. The listbox will contain the names of unused gates on the component using the typed name.

Component Name Buttons

If the chosen part has multiple gates you will see three buttons to the right of the name. These are to help you easily choose between using free gates on existing components, or adding new components. If you hover the cursor over the buttons, a tooltip will be shown describing their use and showing what component name will be used if they are pressed.

First Unused Gate - Use this button to set the dialog up to add the first unused gate on any component using this part in the design. The button will be disabled if there are no free gates in the design. Next Component name - Use this button to set the dialog up to add the next component using this part with free gates in the design. First Free Component Name - Use this button to set the component name to the first free name that does not yet exist in the design.

Preview

Use this to optionally display what the component or gate will look like when added to the design. If adding a gate the appropriate gate is highlighted in the select colour.

Schematic & PCB

If Preview is enabled, this switches between a Schematic Symbol preview and a dual preview allowing both the Schematic Symbol and PCB Footprint to be reviewed.

Attributes

As well as previewing Symbols for the Part, you can also preview Attributes associated with that Part by selecting the Attributes check box.

Add To Comp Bin

Use this to add the component(s) to the Component Bin. These components can then be dragged from the bin into the design at a later stage. The Number Of Copies box allows you to add multiple parts to the bin in one operation.

Vault

Checking the Vault button will show the Vault IID and Version reference information for the Part, Symbol and Footprint, alongside other enabled Preview information.

If the Vault is in use, Look In will additionally include Vault library entries. Each Vault folder that contains part items will be listed and the special entry [Vault Only] allows all parts from the Vault to be exclusively chosen.

Also, additional controls are shown on the dialog, below the Symbol field.

By default, Vault Revision shows the of the part, but other versions may be selected by choosing from the drop-down list.

Interactively Positioning A Component

Whilst using the mouse to position the component or gate, you can use the shortcut menu to change its angle and mirror it, amongst other things. This is explained in detail in the Move operation.

Use Next Alternate Part from the shortcut menu to change the component to use the next part that is a member of the same part family. This option is only available if the part is a member of a family.

Use Insert Multiple Items to switch from adding a single component to adding multiple copies of the selected part at the same time. An Insert Multiple Components dialog will be displayed for you to specify how many components in each direction and the gap between them.

Use Next In Sequence option from the shortcut menu to increment the component name and gate identifier to the next free component or gate not used in the design.

The Next Symbol option will be available from the shortcut menu when there are more than one schematic symbols assigned to the gate being added. Use this to change the symbol to the next alternate symbol defined for the gate in the part.

Click to position the component or gate at the required position.

Related Topics

Component Bin | Find Library Item | Libraries | Insert Connector Pin | Move | Translate To Pcb | Design Settings - Name Ranges