In order to link your DxDatabook database with DxDesdigner Schematics, you must first configure your ODBC Driver settings. In the Control Panel>Administrative Tools> Data Sources ODBC, setup the Name and Location of your SQL database. This should point at your database, and when your Proper .DBC file is chosen in DxDatabook you should be linked. This will allow for placement from Databook and Verification to it.
I always place from Databook and allow the database to push the properties into the schematic. It is more consistent this way and allows for the Database to be the control. In an Enterprise organization, you really do not want the users editing properties in the schematics - let the database placement provide the correct info that can be verified to. But if you do have user Properties that you wish to be editable within the schematic after placement, then you must make sure that those Properties are listed in the Central Library Properties file. These properties are added and edited within the Central Library Manager.
You said local symbols, this would normally mean that the symbols are not in a central library. A first step would be to export the symbols into the Central Libary.
For the schematic, make a backup and there should be very little risk in updating the schematic, backup the original first, and experiment. You may also want to use search and replace in combination with using DxDatabook. Compare your outputs by using creating a BOM of the original and revised versions.
For example, I once I had a design with 0402 resistors, and when we changed manufacturers we wanted to go to 0603. I first replaced all 0402 cells with 0603.
I then made a .dbc that would compare "load" values that matched cell name = 0603, and the current resistor value. After reviewing the matches, only a few new part numbers were required, which I added. Then I used databook to search, and replace the part numbers using Live or New Hierarchical Verification window and the schematic was quickly updated.
On success, you will have learned the real power of DxDatabook!
Thanks for your answers.
But it's still a little fuzzy for me.
If i put a component in my schematic using DxDatabook and after a while i want to modify in my personnal Database a property of this component.
How can i update my component properties who is placed in my schematic ?
I know that i can replace all properties of one component in my schematic with properties of one component in my personal database (, but how can i do that with more than one component and without having to find them one by one in the schematic.
If i do that with the verification menu, he replaces component in function of Part Number, but in my case, all resistors have the same Part Number. Maybe he compares also with Value/Tolerance property and find right one like this !?
Thanks in advance,
In my situation, I have DxDatabook setup to verify to all important properties in my database that I do not want the users to change by hand in the schematic. IE: Part Number, Valu, Tolerance, Description, ETC. This can be whatever you want it to be. In my past experience, the more the better. This allows the Library to control the properties once, to be used by many engineers - and to keep the chances of property errors from being incorporated into the schematic. You setup these Verifyable properties in the DBC file. Once setup, use the Heirarchal Verification to find any parts in the entire schematic that do not match the properties in the Database. You will get "Red Lights" lights for each of these, with Conditions that do not match the database. Update for the correct properties in DxDatabook and your properties will be matched with a "Green Light"
In your schematic you state that all of the Parts have the same part number. When placing from DxDatabook a 10 ohm resistor, and a 22 ohm resistor should not have the same part number. Also, there would be several specific properties that would be different that could be verified to. If you setup your DxDatabook database correctly, and place only from DxDatabook, you will have very few issues to address at point of verification.
I hope this can help...
In your schematic you state that all of the Parts have the same part number. When placing from DxDatabook a 10 ohm resistor, and a 22 ohm resistor should not have the same part number.
It's interesting ! I think, one of the best advantages of DxDatabook (and to use an external database) is to have a clean, smart and small Part library. It's why i built my resistor partition with approximatively 5 differents parts.
(Gen = Generic)
The value/tolerance and others properties are added when i drag and drop a component from DxDatabook.
I'm alone to think that it will be very interesting to have a link (=key) between my component in the schematic and my database ?
With a unique key, it will be very easy to update a specified component.
This is the right approach. The link between DxD and DxDB is a component property defined as UniqID in DxDB. Quite often a special user property is used for that (e.g. "Corporate Partnumber"). DxDB manual describes it in details.
In such case your Central Library contains only symbols, cells and the mapping between them (part), but almost all properties are retrieved from DxDB
You are correct in your thinking, and I may have confused you. With DxDatabook you link what can be 1 Resistor Symbol with thousands of Database Records in DxDatabook - these would be your Update Keys as you state - but a resistor library for example may only have a few symbols in it. In the past I have had a library of approximately 1500 symbols, but with over 30K Dxdatabook records within my database. The symbols and footprints are generic, the DxDatabook database is specific to each individual manufactured part.
We understand the fuzzyness; this question is difficult to answer in a community forum and is much easier in a one on one environment where the data can be viewed and queried.
Have you contacted your account manager for support and/or training opportunities?