There could be several reasons why the migration stopped, do the log files give any clues? It is possible that there are WIR files that are no longer used in the design, the migration checks for this but is not very informative if this is the problem. I would suggest you contact Customer Support for help in this instance.
Thanks for answer. I opened the file migration.log and it seems that there's a problem with WIR file of symbol CONN5PER1.1
Here below the section of log where the error is visible:
00:00:00 The following schematics found in I:\Tc-pe\MassimoM\progetti_dxdesigner\se_pow\:
00:00:00 'scheda_sup.1' 'scheda_sup.2'
00:00:00 Adding block scheda_sup.1
00:00:00 Adding block scheda_sup.2
00:00:01 Error: Default configuration for scheda_sup.1 cannot be created:
viewbase: Warning 221: is newer than the wir file symbol.
viewbase: Error 222: Error - Could not find WIR file CONN5PER1.1.
00:00:01 Migration stopped because schematics cannot be migrated to iCDB
How can I proceed? Maybe it's enough to modify something in wir file or schematic file, isn't it?
Thanks in advance.
The error is about a missing WIR file for CONN5PER1.1. This could be because this particular schematic is not needed or used in the design, in which case ePD3.0 would ignore it and not create a WIR file. The migration process on the other hand checks all schematics and looks for a corresponding WIR file. If this is the case you could move the schematic to a backup folder and re-run the migration and see if it completes. If this is not successful please call Customer Support.
I found the solution!!!!!!!
I tried to edit the symbol file CONN5PER1.1 and also the schematic and wir file in which there were the references of CONN5PER1. Then, I compared these wiht ones of another "correct" symbol.
I discovered the following 2 differences between "wrong" symbol (CONN5PER1) and "correct" symbol:
1) COMPOSITE insted MODULE in the symbol attributes (I used "Symbol Editor tool" to modify it)
2) At the beginning of the declaration instance in the wir file, there was letter W instead M (I used notepad to modify wir file)
Then, starting DxDesigner and opening the project file .dproj, the migration returned 0 errors and the root project with all schematics is now visible.
I used the 2 steps with some "old" projects that returned migration error about ICDB, they are useful.
please i need your help.
i have this problem, the migration file is:
00:00:09 Error: Default configuration for sp605.1 cannot be created:
viewbase: Error 222: Error - Could not find WIR file SFP_FLOW.1.
00:00:10 Migration stopped because schematics cannot be migrated to iCDB
i try follow your steps, but i don't understand how change COMPOSITE instead MODULE, and where change W instead M.
please help me.
Migration.log.zip 1.5 KB
In this case Massimo is talking about the symbol ascii file in the sym folder, if the symbol is a 'composite' it means it is a block/FUB and has an underlying schematic which requires a corresponding WIR file. If the symbol is for PCB layout then it should be a 'module' type and doesn't require a WIR file. Be careful when modifying the SFP_FLOW.1 file, if it is in the schem folder it wil most likely be a composite, but see my other post as it may not be required in the design. If it is a PCB symbol (module) then you'll need to change the symbol file and the WIR file where the symbol is instantiated (the sheet of the schematic where the symbol has been placed). You will need to search all of the WIR files for the reference to the SFP_FLOW 'symbol' to figure out what to change.
You should call customer support, they can give a quicker response than trying to use these forums.