Troubleshooting the Library Panel

Libraries Panel Not Displaying Symbols

click on image to view

Fix: 

Install a PCBLIB and a DBLib or SVNDBLiB.

Then with the PCBLiB selected, toggle Footprints off. Altium will close the PCBLib panel and open the DBLib or SVNDBLib Library Panel.

Next toggle the footprints on and now the both the DBLib and PCBLib Library Panels should be properly displayed.

Libraries Panel is not displaying symbols or footprints.

For DBLib (Not applicable to SVNDBLIB) there is a required folder structure.

The Altium *.DBLib file and the Symbols and Footprints folders need to be stored in the same parent folder, example shown below.

click on image to view

Verify Components, Footprints and Models are selected.




Your first step should be to open your DBLib or SVNDBLib file in Altium to check the mapping, and use the table browser to verify the database records are visible.

If you are using the Parts Frontend application use 'Verify Libs' to locate any missing library files of bad library references in the database.

Verify file locations, file names and model names (Refs) are good.

The Verify Libs button in the Parts Frontend can be used to verify the symbol and footprint files exist and are properly located relative to the Working Folder path.

Load the DBLib or SVNDBLIB file in Altium, connect to the data source, fix mappings, then use the table browser to verify the parametric data is displayed in the *DBLib.

DBLib:

Libraries Panel is empty, no symbols or footprint are displayed.

Fix:

Verify that the SVN Libraries Working Folder path is NOT pointing to your DBLib symbols and footprints parent folder. (this is a very sneaky bug).

This is a strange problem to comprehend when you don't have a SVNDBLIB installed. Then why is does the Library Panel go blank for an installed DBLIB Library ?

DXP > Preferences > Data Management > SVN Libraries > Edit Working Folder Path or move the footprint and symbols files out of the SVN Library Working Folder.

This strange event occurs if your DBLIB database is pointing to footprints and symbols that are in a SVN Library working folder.

One workaround is to point the SVN Library Working Path to a temp folder, i.e. C:\temp

SVNDBLIB Display Parts:

Problem:

Symbols and footprints are missing in all of the displayed records.

Fix:

Open the SVNDBLIB in Altium, set the Repository Server Connection and Model Location.




Problem:

Symbols or footprints are missing in some of the displayed records.

Fix:

In a SVNDBLIB Library you can have only one footprint per *.PCBLIB file. And the model name in the file should be exactly the same as the file name.

Example:

Filename = SOP50P490X110-10N.PcbLib
Footprint Ref = SOP50P490X110-10N

This also applies to symbols *.SCHLIB files.

You can use the 'Verify LIBs' command on the Parts Frontend menu to find any missing files or improperly referenced models.

Fix:

You may need to delete or move the existing symbols and footprint folders in the working folder. Restart Altium > Install SVNDBLib > Right Click and select Edit Symbol to rebuild the the SVN checkout folder for the Symbols. Then repeat these steps for the footprints.


SVNDBLIB Edit Parts:

Problem:

You right clicked on a part and selected edit in the Libraries Panel, however the part editor did not open with the symbol or footprint displayed.

Fix:

DXP > Preferences > Data Management > SVN Libraries > Edit Working Folder Path.

Verify that the SVN Library working folder exists, if it does not exist, then create a working folder and set the working folder path in DXP Preferences.

Fix:

Close Altium. Find and Delete the corrupted SVNDBLIB Cache Folder, typically located at:

C:\Users\xxx\AppData\Local\Temp\SVNDBlib Cache

Where xxx = windows machine user name.

Restart Altium and connect to the SVNDBLIB library. The deleted SVNDBlib Cache should be rebuilt.

Fix.

Verify drive letter mapping matches paths in DXP preferences and the *.SVNDBLIB options.

Libraries Panel Freezes

Note: To avoid Library Panel freezes users should not enter Footprint and Symbol file names into the database if the files do not exist.

Database entries pointing to non-existent library files will cause Altium's Library panel to freeze.

How long the Libraries Panel appears to be frozen is dependent on how many records in the backend database are pointing to non-existent library files.

After Altium is done looking for each of the non-existent library files the Libraries Panel will return to a functional state. (This can take few minutes)

Tip: Use the Verify command in the Parts Frontend to find records with non-existent library files or bad library references.

Related: Libraries Panel - Missing Symbols Fixed (Altium PCB Designer blog)

Libraries Panel - Missing Parametric Data.

As shown below the Libraries Panel is missing Parametric Data. Only the symbol and footprint are visible.

click on images to view



Open your DBlib and check the the Field Settings for the Tables.



If you see a red colored message The database underlying this library has changed . . .

This means that Tables in the database and the DbLib file are out of sync.

Fix:

Select each Table or Query displayed in the Table list.



In the Field Settings select ID = ID for each Table.



Select (0) use Connection String and select Reconnect.



That's It !

DBLIB or SVNDBLIB ?

In a DBLIB Library you can have multiple footprints stored in the file or a single footprint. The model name in the file can be anything as long as it is a unique name within the library file.

Filename = SOP50P490X110-10NC.PcbLib
Footprint Ref = any unique name.

DBLIB:

Pros:

• Simpler to implement and use than SVNDBLIB.
• Supports multiple and single part Library files.
• Good Choice for Single and Multiple Users

Cons:

• NO Version Control for Symbols and Footprints
• NO Right Click and Edit Symbols and Footprints from Library Panel.

Note: DBlib libraries support single or multiple part files, however, it is recommended that you create library files with one symbol or footprint per file. This will reduce locked file conflicts in multiple user environments.

SVNDBLIB:

In a SVNDBLIB you can have only one footprint per *.PCBLIB file. And the model name in the file must be exactly the same as the file name.

Filename = SOP50P490X110-10NC.PcbLib
Footprint Ref = SOP50P490X110-10NC

Note that the Footprint Ref (model name) matches the Filename for SVNDBLIB.

This also applies to symbols *.SchLib files.

Pros:

• Version Control for Symbols and Footprints
• Right Click and Edit Symbols and Footprints from Library Panel
• Good Choice for Single and Multiple Users

Cons:

• Occasional Corrupted SVNCaches.
• Performance, slower than DBLIB.
• Setup is more complicated than DBLib, may require technical support.

SVNDBLIB's slower performance is due to the SVNCaches which include a working folder and a system cache of footprints and symbols that are checked out from the SVN repository.

Choices:

Both DBLib and the SVNDBLIB are the good choices for library maintenance. 

When deciding which choice is best for your situation, you need to consider number of users and librarians that will be using the database.  

You should consider you team's experience with SVN when choosing SVNDBLIB.

Suggestion:

Start out with a DBLib, then convert to a SVNDBLIB if you need better version control (accountability for changes). 

Transitioning from DBlib to SVNDBlib will be easy if you have one model per file which is required for SVNDBlib.  

The sample symbols and footprints included in the 'Parts' download are one model per file.

Using a well designed Parts Frontend application can greatly simplify Altium CAD library maintenance.

That's It !

SVNDBLib Model

The SVNDBLIB library is little more complicated than the DBLIB.  It's a good choice if you need tighter control and change history for your symbols and footprints.

Click on Image to View

Tip: Get DBLIB working first !   Then setup SVNDBLIB

Related Links: PARTs and SVNDBLIB

That's It !