1 of 1 people found this helpful
You would need to put a Cell Name property on the Part in order for Packager to put the property on the schematic.
In order to do this, you would need to modify the Cell Name property as follows:
1. Check the "Place property in schematic..." option
2. Click the Advanced button, and check the "Symbol" option in the "Attach selected property to" group
3. Check the "Part Editor" option in the "Include selected property in property lists for" group
And now you will need to add the Cell Name property to each PDB Part. This is not automatic, but it can be automated. I have attached a script form that can add a Cell Name property to every part in the library, whose value is the name of the top cell for that part. You can run the script by opening the central library in Library Manager, and choosing the File -> Open Script Form menu. Click the "Add Cell Name Property to all parts" button to add or update the Cell Name property on all parts.
The Cell Name property can be overridden at the schematic level using the "Select Alternate Cell" context menu. Unfortunately, I am seeing cases where you can end up with 2 Cell Name properties, one added by the Place Device command, and one added by the Select Alternate Cell. Please try this out in your environment, and see if you encounter the same behavior.
Then finally, you can alter the Part Lister configuration (ipl file) to use the Cell Name property instead of PKG_TYPE.
Let me know if you have any questions.
I did try adding the Cell Name property to a resistor in the PDB with Library Manager besides adding the property to the symbol. That was my first choice. I must not have followed through to Packager? I will give this a try again when I get back to work on Monday.
I guess that it is not that simple for EE2007.5 update 2. What you describe is the first thing that I tried. After filling the Property Editor setup for Cell Name I did try to add the Cell Name property in the PDB Editor. The Cell Name property shows up in the drop down list of properties that can be added to the part. In order for the Part Editor to save the Cell Name property on a part one has to add a value. That done, yes it will be added to the schematic part by Packager with the value that is typed in. But that is no better than to continue using PKG_TYPE attribute on the DxD symbol. Only now one has more parts than having more symbols.
The Cell Name is already added to the PDB when one does Pin Mapping. Adding in the Cell Name property under Component properties: duplicates the effort. If one were to place "XXX" as the Cell Name value under PDB Component properties, then Packager will not replace "XXX" the default cell for the footprint used in Pin Mapping even though the Pin Mapping footprint cell is passed on the layout. So I need to know what property I need to place in my *.ipl file that will pass the footprint cell to the BOM?
The Cell Name property in the PDB is duplicate data, but with the script is should not be any duplicate effort - just run the script and all Cell Name properties will be added or updated based on the default cell in the Pin Mapping dialog.
There are several benefits of using the Cell Name property instead of a PKG_TYPE property on the symbol, the most important is that alternate cells selected in the schematic will be shown in the BOM.
At this point there have been two paths presented to follow. The first was to go into the PCB editor and place the Cell Name property with the property value filled in using the drop down list under Component Properties. This procedure can be automated with a script to use the Cell Name that has already been added through the Pin Mapping window. Doing this will place the Cell Name property into DxDesigner and icdbPartsLister.exe can report the DxDesigner Cell Name property. But back annotation from Expedition will not change the contents of the DxDesigner Cell Name property and that could lead to multiple Cell Name properties in the CBD filled with different names; the BOM will not reflect what is on the board.
The second path is not to place the Cell Name property with the PCB editor into the Component Properties list but to only call out the Cell Name in the Pin Mapping window. In the Property Editor, put check marks in the boxes that tell the software to place the Cell Name into DxDesigner. You can build the DxDesigner schematic and package but you will not see the Cell Name property populated until the PCB is placed and back annotation is run. After back annotation is completed to DxDesigner, you will see the Cell Name property filled in with the footprint cell placed onto the PCB. icdbPartsLister.exe will now produce a BOM containing the footprint cell names for all of the parts.
There is a problem that is not addressed and that is that the BOM is drawn from the schematic and used to buy parts long before the PCB layout is started. So the footprint cell names will not be populated and the purchasing checking of the manufacturer’s part number vs. the footprint to be used can not happen. The schematic engineer may well build the symbol but the footprint cell may not be created until much later. So doing a quick and dirty dump of the parts into a PCB layout file using the pr –dist keyin command and back annotating to the schematic can not happen. Most of the part descriptions in our library end with a footprint name, so I guess we will have to rely on those for early BOM purchasing and checking.
Can i have the script file?