안녕하십니까? ED&C입니다.
MG510024의 내용을 전달 드립니다.
백업 후에, 아래 Solution 1과 Solution 2의 방법을 사용해 보시기 바랍니다.

Cell Name is not a valid cell for Part Numberd.
==================================================
Error while Packaging and Forward Annotation: Cell Name is not a valid cell for Part Number.
Have changed the cell name attached to a part, now I cannot Package.
Cell name has changed, how can I add the associated parts to schematics that already use this part?
==================================================
Cell Name property that is defined on the Symbol is not a valid cell as defined in the Part of the Central Library.
Either of the following will fix the problem:

Remove Cell Name on Symbol Properties in Schematic.
Replace Cell Name Property on the Symbol with a correct Cell Name from the Part in the Central Library

Solution 1

The following procedure may be useful for removing Cell Name properties from schematic symbol instances, where a high amount thereof exist:

For each schematic sheet in the design in turn:

Open the sheet.
Set the Selection Filter to only show symbols.
Drag-select the entire sheet contents.
In the Properties dialog, locate ‘Cell Name’, and on ‘Cell Name’ select Right Mouse Button (RMB) - Delete Instance Value.
NOTE:  If Back Annotation of Cells in the PCB to the Cell Name property in the schematic is not desired, then it can be turned off in PADS Professional Pulldown: Setup - Project Integration - Additional Options - Back annotate cell names to schematic.

Solution 2

The assumption is that the 'cell name' property is required and added to placed part symbols during instantiation.
In the following example the part number mg1234 originally used cell name C1206 and is placed and packaged.
The part has been changed in the library so part number mg1234 now uses cell name C1210. When a new version of the part mg1234 is placed in the schematic Packager fails because of the mis-match between cell names, old and new.
To correct the problem do the following:

Find the property 'cell name' with value 'C1206' for part number mg1234 and delete the property.
Package with any 'PDB Extraction' options except 'Only Extract Missing Library Data' i.e Do not use this option.
If using option 'Extract Missing with Selected Library Data' ensure to select the required part number from the 'pop up' GUI.
Open the associated PCB with PADS Professional and choose to run 'Project Integration'. Ensure the 'Forward Annotation Options' are set to 'Additional Options' - 'Back annotate cell names to schematic', and the 'Library Extraction Options' is set the same as was set with Packager in the schematic.
Run Forward Annotation by mouse clicking on the top forward annotation light/button.
To ensure changes are pushed back to the schematic run 'Back Annotation', Save the PCB.
If closed, re-open the schematic and check that instances of part number mg1234 now have the property 'cell name' with value 'C1210' attached.

감사합니다