Working with Reuse Blocks

If your designs often include common 'sections' of schematic and PCB circuitry, Altium Designer provides simple and easy ways to save and reuse these sections, eliminating the need to create them from scratch each time.

When connected to a Workspace, you can create a reuse block that can contain both schematic circuitry and its physical representation for the PCB. When such a reuse block is placed on a schematic sheet, its physical representation will be placed automatically in the PCB document during the ECO process.

The Design Reuse panel allows you to quickly access all of the controls needed to work with and manage your reuse blocks.

To work with reuse blocks through the Design Reuse panel, make sure that the panel is configured to browse Workspace resources. To do this,  click the left-most icon in the address bar at the top of the panel and select the entry of your connected Workspace. The icon will be shown as .

Creating a Reuse Block

A new reuse block can be created as described below.

1. Click the  button at the top-right of the Design Reuse panel. Alternatively, select the File » New » Reuse Block command from the main menus.

2. A temporary editable PCB project-like structure of the reuse block will open in the Projects panel (under an entry for the connected Workspace), and the temporary Schematic editor will open, ready for defining the schematic document of the reuse block. Use the standard placement commands and techniques to define the schematic document of the reuse block.

   If you would like to create a schematic-only or PCB-only reuse block, you can remove the PCB or schematic document from the structure of the snippet by right-clicking the PCB or schematic document, respectively, in the Projects panel and selecting the Remove from Project command.

3. Use the Design » Update PCB Document command and the ECO process to transfer the captured schematic to the PCB document of the reuse block, then apply the changes needed to that document (defining component locations, routing, etc.).

   Multiple PCB documents can be added to the reuse block being defined. To do this, use the Add New to Project » PCB command from the right-click menu of the reuse block's entry in the Projects panel.

   

   Use the Rename command from the right-click menu of the added PCB document's entry in the Projects panel to define a meaningful name for it. Use a Design » Update command from the schematic editor main menu to update the required PCB document.

4. When both schematic and PCB documents of the reuse block are defined, save the reuse block to the Workspace using the Save to Server command from the right-click menu of the reuse block's entry in the Projects panel or the Save to Server control at the right of the entry.

   Because reuse blocks are stored in the connected Workspace, it is recommended to use components from that Workspace in the reuse block. That way, you get the full benefit of the content system the Workspace provides.

   • Both schematic and PCB documents of the reuse block must contain at least one component in order to be saved to the Workspace.

   • If the reuse block's schematic and PCB documents are not synchronized (differences between the schematic and PCB documents are detected), a warning dialog will be shown when you attempt to save the reuse block to the Workspace. You can cancel saving to return to the reuse block and address the differences or proceed with saving.

5. The Create New Reuse Block dialog will appear, in which you can define Name, Description, and the Workspace Folder into which the new reuse block will be saved.

   

6. After clicking OK in the Create New Reuse Block dialog, the reuse block will be saved to the Workspace, and its temporary structure will be closed.

Searching for and Placing a Reuse Block

Reuse blocks stored in your connected Workspace can be browsed and used from the Design Reuse panel when it is set to display Workspace resources (). In this mode, the panel presents the folder structure of your Workspace so you can browse folders where your reuse blocks are stored. Each folder and reuse block are presented in the list at the top of the panel by its name and description.

To find the required reuse block, you can navigate through the folders or use the Search field at the top of the Design Reuse panel to search for a reuse block by its name or description ().

Click the Details control at the bottom of the panel to expand the Details pane that displays details for the selected reuse block, including:

• Reuse block name.

• The lifecycle state icon and revision (click the link to open the detailed History view of the Reuse Block Item with the latest revision selected).

• Reuse block description.

• Reuse block general information and its parameters.

• Preview images of the reuse block's schematic and PCB documents.

• List of projects () and project releases () where the reuse block is used (the Where Used region).

To place a reuse block in a design,  hover the cursor over its entry in the Design Reuse panel, click the  button (or right-click the entry), and select one of the following commands from the menu:

• Place – select to place the reuse block directly on the active schematic or PCB document. Depending on the type of document that is active when running the command, the schematic or PCB document of the reuse block will be placed.

  

  

   

• Place as Sheet Symbol – when a schematic document is active, select to place the reuse block as a sheet symbol on the schematic sheet. The placed sheet symbol will include sheet entries corresponding to ports in the reuse block. The content of the reuse block will be placed on an automatically created child schematic sheet referenced by the sheet symbol. The sheet symbol of a placed reuse block will have a distinctive icon.

  

After placing the schematic document of a reuse block, its PCB document can be placed in the PCB document through the ECO process. From the Schematic editor, use the Design » Update PCB Document command from the main menus, then validate and execute changes using the Engineering Change Order dialog.

Editing a Reuse Block

To edit a reuse block, hover the cursor over its entry in the Design Reuse panel and click the  button (or right-click the entry) and select the Edit command from the menu.

The temporary project structure of the reuse block that contains the latest revision of the Reuse Block Item will open for editing. Make changes as required, then save the reuse block into the next revision of the reuse block (File » Save to Server).

Other Reuse Block Actions

The  button menu (and the right-click menu) of a reuse block entry in the Design Reuse panel also provides access to the following commands:

• Rename – use to change the name of the reuse block. After selecting the command, enter the desired new name in the Rename Reuse Block dialog that appears, then click OK.

• Move – use to change the location of the Reuse Block Item in the Workspace folder structure. Launching a command will give access to the Move Item dialog in which to select the target folder under which the Item should be placed into.

• Share – use to define the sharing permissions for the reuse block. After selecting the command, the Share For Item dialog will open in which you can configure sharing as required. Learn more about Item-level sharing.

• Operations – use to access a drop-down menu of additional functions for reuse blocks as described below.

  • Make a Copy – use to copy the reuse block. A temporary project structure of the reuse block will open, with the same content as in the original reuse block. Make required changes and save the reuse block to the Workspace. 

  • Change Revision State – use to change the revision state of the reuse block's latest revision. After selecting the command, the Batch state change dialog opens, which allows you to change the revision state of the reuse block.

  • Download – use to download data stored in the reuse block (its schematic and/or PCB documents). The associated data will be downloaded into a sub-folder under the chosen directory, named using the Reuse Block Item Revision ID. The files can be found in the Released folder(s) therein.

• Delete – use to delete the reuse block from your connected Workspace. After selecting the command, the Delete Items dialog will appear, in which to confirm the deletion. You can also opt to delete the reuse block's related content (i.e., schematic and PCB snippets).

  The action is actually a 'soft delete', whereby the reuse block will be moved into the Trash area of the Workspace. Learn more about soft deletion.

• History – use to access a detailed view for the reuse block, opened as a new tabbed view within Altium Designer.