Use this to change a component in a PCB or Schematics design to use a different part from the Parts Libraries.
If you simply want to replace the component with a newer version from the parts library, use the Reload From Library option.
If you only want to change the component to use a different footprint from the same part, use Component Properties.
If you want to change the component to an alternate part in the same part family, use the Alternate Part option.
Shortcuts
Default Keys: I or Alt+Enter
Default Menu: Edit
Command: Properties
Locating this option
Available from: Edit menu > Properties option
Available from: Context menu > Properties option
Available from: Shortcut key > I
How To Change A Part
Select the Component that you wish to change. Use the Properties option from the Edit menu, or from the shortcut menu. Now switch to the Component Properties Tab.
From this property page, select the Change button to the right of the current Part name. The following dialog will be displayed:
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.
If the Vault is use, the drop-down list will additionally include Vault 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 viewed.
Which Parts
Use the Filter box to enter a string containing the ”*” or ”?” wildcard characters to filter the list to only matching names e.g. “74*“.
Use the No. Pins box to limit the matching parts to those of a set number of pins (blank means any pin count). This box will be primed to contain the same number of pads as the part you are changing, so when you enter the dialog the list of parts all have the correct number of pads.
Use the Same Footprint checkbox to limit the matching parts to those that have the same footprint as the part you are changing. In schematic designs, use the ‘Specify Footprint’ option in Component Properties to specify which footprint is being matched when the Same Footprint checkbox is enabled.
Use the Same Symbol checkbox to limit the matching parts to those that have the same symbol as the part you are changing. This option is only available in schematic designs, and for parts with a single gate.
Press Apply to alter the list of parts names accordingly. 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.
Footprint
Only used for PCB designs. This shows the alternative footprints that the chosen part can use. Select the footprint required.
Keep attributes styles
Check this box if you do not want the attribute styles reset to their values in the footprint in the library.
Keep attributes positions
Check this box if you do not want the attribute positions reset to their values in the footprint in the library.
Keep local attribute values
Check this box if you want any attributes you have added to the component to be retained.
Replace nets assigned to ungated pins
Only used in Schematic designs. Check this box to reset the pins on the component that are not on gates, to be on the nets on the pin definitions in the part in the library. Leave unchecked to keep the component’s ungated pins on the nets already assigned to them in the design.
Preview
Use this to optionally display what the component will look like when added to the design.
Performing The Change
Press OK when you have selected the new part in the dialog. You will be returned to the properties dialog where you can change other properties of the component.
Connected Components
If your component was connected, you would normally change it to a component with the same number of pins in order to not affect the nets. The connections or tracks will be attached to the pads with the matching pin name in the new part.
If you choose a part with more pads, the extra pads will remain unconnected in the design. If you choose a part with less pads than on the component, any connection to a pad that does not exist on the new part will be removed, and any track in the same situation will be disconnected and left dangling for you to sort out in the design later.
For schematic components, as well as pins being matched up, gates are matched so that if you replace a four gate component with a single gate part , only pins on the first gate of the original component will retain their connectivity. All connections to pins on unmatched gates will be disconnected and left for you to sort out later.
Database Connection Extensions
These additional features are available as part of the Pulsonix Database Connection.
Change Database
Clicking this additional button displays the Database Bar in a special ‘Change Part’ mode to allow the part to which you wish to change, to be chosen via your database rather than from the Parts Library. The selected database part contains a reference to its equivalent part in the Pulsonix library which is used to represent it in your design and whose details will be displayed as normal in the Change Part dialog.
Note that if the part to change to is not chosen via the Database Bar any existing database information for affected components is lost and they will revert back to being ‘local’ components.
Database field
The database key field is displayed in the dialog rather than the Part Family field.
Related Topics
Alternate Part | Library Folders | PCB Footprint Library | Parts Library | Properties - Component | Reload From Library