It's sounding to me like you have unintentionally set the library up as a netlist flow. The parts database needs to be defined in the central library and the access database is used purely for parametric data not part mapping. Perhaps you can figure out some tricks to convert things over to a netlist library and then use the migration tool to convert it to a central library (I know this seems like a backwards approach). Not sure how else you can do it without manually creating your parts...
OK... I will go back to the documentation to see how the netlist flow verses integrated flow impacts me. Thanks for the reply.
The first time through creation of libraries in any tool is always where the most pain occurs.
In answer to yours and Travis' post, you have set this up correctly, but not quite completely. As Travis mentions, you need to map the symbols to the PCB Decals in the central library, this maps the logical to the physical, the parametric database just adds properties and allows searching on other data that may not be used in the schematic or on the PCB (Price for example).
The long and the short of it is that the Part Number (equivalent to DEVICE in the netlist flow) is the unique identifier in the central library and therefore there needs to be a one-to-one correspondence between the parametric data in the Access database and the part data in the central library . If you use the 'Edit parametric data' from the Central Library when creating a new part you will notice that for each part in the central library it will create a new line in the database showing the one-to-one relationship.
You now have two choices as you have come at this from the database side of things. Use the migrator to build a new version of the library whilst pointing to the access database (and Databook configuration), this will create a part for each entry in the database, you will then probably have to map the decals once more. Alternatively you can just create a new part manually for each entry as you have identified in your original post.
A couple of ideas you can use though; firstly you don't need to map pin numbers to symbols directly, you can share basic symbols across all parts without pin numbers and let the packager assign them when it is run. To ensure this works you will need to always use Databook to place parts into the schematic as it will assign the correct part number and other properties to allow successful packaging.
If you have VX.1.2 or VX.2 then it comes with a 'StarterLibrary' in SDD_HOME\Libraries\xDX_Designer\StarterLibrary. This is not to be confused with the ODA library, but is a small library that users can get started with straight away, the structure is the same as the ODA library, but it uses a few tricks to limit the amount of data that was needed to create it. As an example all of the resistors listed in the associated Access database use the same symbol so that should you need to change the symbol or pin mapping you need only do it once in the central library. But there are a large number of parts referencing this symbol. You can also use symbols without pin numbers, just give them placeholder properties and packager will annotate the pin numbers as necessary. This library doesn't have an example of this trick as the parts were generated using the migrator, having started with the equivalent netlist library found at SDD_HOME\Libraries\xDX_Designer\SymbolLibrary. These two share the same Access database but use different Databook configuration files to ensure the required properties are added during part instantiation.
This is a big topic and I hope I've pointed you in the right direction, if you need further help or advice contact your usual support rep or get in touch with me via the community.