I would like to make a self contained design pointing to its own local Library.lmc file that only has the parts that are in this design. What is the easiest way to accomplish this? Thanks.
Create an new Empty Library and using Libriary Services to import part from your main design.
Thanks! But now I am curious as to Why I do not get the File>Export EDX option when I open this library in xDM Library Tools?
Never mind follow up question. I found that If I create and use with xDM Librarian 100 license (instead of 200 or 300) I get the export File>Export EDX option.
This method given by pbo does not include schematic symbols. Do you know how to get a local library that includes schematic symbols?
In DxD create export EDIF Schematic from your project after that import that EDIF in empty project, open databook symbol view tab and look at [local symbols] listed here. You can select all of local symbols RMB->export symbol(s).
Open library tools and go to file->import symbols...
They're not automatically associated to the parts they were associated to in the design which makes this not very useable.
You need firstly import symbols on your library after that using library services to import parts.
Symbols wiil automaticaly associated with parts. Because when you import part via library services information about symbols already included in pdb.
If you do vice verca and firstly import part data, symbols can't link to the part because symbols associated with part does not exist in your library
The parts still do not get a symbol association under the Parts after doing this
Look at step by step manual that i recorded for you
Could the difference in results be due to different flows? I see that you are using PADS Library Tools and I am using xDM Library tools.
These are the steps I wrote following your video and previous instructions and it still did not work to associate the parts with symbols:
I used PADS Professional it is very similar to Expedition, but I did it in Expedition too.Very strange steps described above look rightAfter you import the part using library Services, open any part using the part editor, click on the pin mapping button and look at the section Symbol and symbol property list and check the symbol name, for example Capacitor: CAP_SMALL, where Capacitor is the symbol partition.
When you create a new symbol partitions they must match those specified here otherwise the symbols are not automatically assigned. After you do export local symbols, a folder is created in which all these symbol partitions are listed, and you need to create them in the partition editor (symbol tab)
The problem I was having was with the EDIF Schematic export. I was not checking this box for Generate edif cells based on Symbols instead of Parts. After doing this in step 1 in my detailed steps above, I was then able to see symbols associated to the parts. Thanks!
Retrieving data ...