Migrate to Parts Database

Project Library Migration to Parts

Altium > Project > Project Packager to backup the original project. (Recommened)

Altium > Schematics > Save Designators and Comments XY to Excel (Optional).

Altium > Disable Autoposition for all Designators and Comments. (Optional).

Altium > SCH > Parameter Manager > Add Mfr Part Number all Components.

Altium > SCH > Parameter Manager > Sort by Mfr Part Number to find missing Mfr Part Numbers.

Note: Unique Mfr Part Numbers are Required.

If needed Copy Library Reference or Comment to Mfr Part Number.

Or create a unique temporary part number using a description, i.e. R402 1K 1%

Note: If you are using Draftsman for Assembly Drawings then .designators are not needed.

Altium > PCB > Delete .designators from all Footprints before Making a PcbLib (Optional)

Altium > SCH > File > Run Script > MakeSymbolRefs.pas Script.

Altium > SCH > Design > Make Integrated Library > Review Messages Panel.

Altium > SCH > Extract Libs *.SCHLIB and *.PCBLIB from the Integrated Library.

Altium > PCBLIB > Scrub Whole PCBLIB. i.e. Change Mech Layer Usage (Optional)

Begin Symbol and Footprint Libraries Migration to Parts Database (DbLib)

Altium > Tools > Library Splitter Wizard > Libs WITH Models and Parameters.

Parts > Tools > Import Libs > Rename Libs Like Symbol Ref.

Altium > Open Renamed Libs >  Run > MakeLibRefs.pas Script, then Save Files.

Parts > Tools > Import Libs > Select Libs > Map Parameters > Import

Altium > Run Script CleanSymbols.pas to Remove Models and Parameters.

Altium > Save the Cleaned SchLib Files in the Parts Working Folder.

Parts > Verify Libs  > Select All > Fix LibRefs and Filenames as needed.

End Symbol and Footprint Libraries Migration to Parts Database (DBLib)

Project Migration to Parts

Altium > Generate a Project BOM.

Parts > Import The Project BOM > Tools > Import Excel.

Altium > Components Panel > Deactivate (UnCheck) All Install Database Libraries

Altium > Add a DbLink to the Project.  Connect to the Parts Library. (Tips below)

Altium > DbLink > Key > Mfr Part Number || Mfr Part Number (Only Update ID)

Altium > Tools > Update Parameters from Database. (Create Log and Review errors).

Altium > Tools > Parameter Manager > Verify all Components have IDs (fix as needed).

Altium > Remove Parts DbLink from the Project.

Parts > Update Parametric Data from Digi-Key or Mouser. (Recommended)

Altium > Components Panel > Install and Activate Parts DbLib Database Library.

Altium > Close and Open (Restart) Altium to clear Cached Libraries.

Altium > Use Find Similar Objects > Select All Parts in the Project.

Altium > Use Properties Panel > Set Source > Part.DbLib - Parts

Altium > Tools > Parameter Manager > Copy IDs to Library References > Accept Changes.

If needed  . . . 

Save Schematics > Close Schematics > Open Schematics !

Altium > Tools > Update from Libraries.

Altium > Tools > Update Parameters from Database. If Needed

Altium > Fix Variant Part Numbers. Project > Variants . . .

Altium > Fix XY location of Comments using saved Excel data.

Done - Review Changes (Compare BOM and Schematic with Original files).

Tips: 

DbLink Options:

Open or Create a DBLink in the Project that is pointing to the Parts database.

DbLink > Options > Do Not Update (Global)

DbLink > Options > Do Not Add (Global)

DbLink > Options > Do Not Remove (Global)

DbLink > Single Key Lookup = Mfr Part Number || Mfr Part Number 

DbLink > Options > ID Update (Parameter Option)

DbLink > Options > ID Add (Parameter Option)

DbLink > Options > ID Remove only if blank in database (Parameter Option)

To Disable Autoposition of Designators and Comments

Use Find Similar Objects > Uncheck Autoposition for all Designators

Use Find Similar Objects > Uncheck Autoposition for all Comments

To Remove the Parameter Position Dots

DXP Preferences > Schematic > Graphical Editing > uncheck 'Mark Manual Parameters'

That's it !

Migrate to Parts Using Tools > Import Excel

Take a Project Snapshot 

Backup (Zip the Project)

Output the Schematic and BOM (save for reference and change reports)

Create Project SCHLIB and PCBLIB Libraries.

Altium Parameter Manager:

Optional (not required)  - To identify Library Ref for parts placed from DBLIBs

Using the Parameter Manager create a parameter named Symbol Ref for all parts in the project schematic and copy the LIbrary Ref to the Symbol Ref parameter. Or run the Altium Script "MakeSymbolRefs" to create Symbol Ref from placed parts. The "MakeSymbolRefs" script is included in the Parts Download.

Altium Reports > Bill of Materials

Export Project BOM, group by Mfr P/N, include Footprint and Library Ref .

Optional Parts Application - User Defined Fields

Select Configuration > User Defined Fields

Add user defined fields:  RefDes, Qty

Required:

Place copies of the project libs in the DBLib working folders (footprints and symbols)

Parts FE > Import Project BOM

Parts FE > Set Library and Footprint Paths to saved Project Libs

Altium Components Panel:
Uninstall All Database Libraries, except for your DBLIB database.

Altium DBLink:
Add a File > Library > DBLink to your project linked to the Parts DBLIB database

DbLink > Options > Do Not Update (Global)

DbLink > Options > Do Not Add (Global)

DbLink > Options > Do Remove (Global)

DbLink > Single Key Lookup = Mfr Part Number || Mfr Part Number 

DbLink > Options > ID Update

DbLink > Options > ID Add only if not blank in database

DbLink > Options > ID Remove only if blank in database

Save and Add the DbLink file to your project

Open all schsoc files in the project, then Select
Tools > Update Parameters from Database

Altium > Remove Parts DbLink from the Project.

Altium > Components Panel > Install or Activate Parts DbLib Database Library.

Altium > Close and Open (Restart) Altium to clear Cached Libraries.

Altium > Schematic > Use Find Similar > Select All Components > Properties Panel > Source > Part.DbLib - Parts

Altium > Tools > Parameter Manager > Copy ID Column to Library Reference Column > Accept Changes

Save Schematics > Close Schematics > Open Schematics.

Tools > Update From Libraries

Review Schematic and BOM, fix as needed.

That's it !