I’ve noticed comments in the forums from users believing that you cannot use Ultra Librarian with CircuitStudio. I would like to set the record straight with this short tutorial, showing how to select and download a part from Ultra Librarian and then import as a library into CircuitStudio along with the associated 3D model.


What is Ultra Librarian?


An online website, Ultra Librarian's claim to fame is having “millions of parts at your fingertips” (around 8 million models I believe they have quoted), a library of component models that can be exported to a variety of CAD formats. Although CircuitStudio is not listed as a supported CAD package we will soon see that does not stop us making use of their components. The website does charge for downloads of its models but allows up to 30 per month on their free plan.


Why Use Ultra Librarian?


CircuitStudio comes with a claimed 300,000+ parts in the Altium Content Vault and an impressive number of downloadable libraries from the Altium Live Design Content resource.  Don’t forget you can use the search function within the Design Content area to find the component of interest, otherwise it can be difficult to decide which library to download as there are so many of them.


Even with all these impressive numbers you are still likely to encounter situations where you cannot find that component you need. Although component creation within CircuitStudio relatively easy and painless it can sometimes be a time saver to just download what's needed. The Ultra Librarian models are generally supplied with a symbol, footprint and basic 3D model.


Finding and Exporting Your Component


On the Ultra Librarian website select the ‘Models’ button and enter your search string, in our example this is a good old fashioned SN74LS00N (I'm sure a few readers will recall designing with such ancient technology).


On the results page use the arrows to expand the format boxes and select both “3D STEP Model” and “Altium PCAD v15”.


Tick the license agreement checkbox then click submit to download the ZIP file, typically named exports.zip. Store this somewhere convenient on your drive and extract the contents. If all is well you should have a few folders as highlighted below.


Importing into Circuit Studio


Start a new project or open an existing project in CircuitStudio. From the File menu choose Import..., select "P-CAD Libraries (*.LIA, *.LIB)" from the file type dropdown. Navigate to the AltiumV15a.lia file you extracted in the previous section (it will be in the AltiumV15 folder) and click Open.




The import process will run and will result in the creation of AltiumV15.PcbLib and AltiumV15.SchLib in your current project. These are standard CircuitStudio library files that you can manipulate and use as normal.


The next step is to add the 3D model to the PCB part. Invoke the library editor by double clicking on AltiumV15.PcbLib in the Projects panel (or use Right Click > Open). You should be presented with the 14 pin DIL footprint of the SN74LS00N. Select Home > 3D Body. In the dialog select "Generic 3D Model" and click "Embed Generic 3D Model". From the file chooser locate your STL folder (extracted earlier) and open the 3D model file.




Use the cursor to align the model to the footprint and then hit ESC to exit model placement. Check your work by viewing in 3D (View > Switch to 3D).




In the real world you would check grids, pin 1 location, mappings between schematic and PCB part just to make sure everything was present and correct. Nothing worse than using duff library parts and then having to write off a board production run. One point to beware of is the import of SMD parts can sometimes seem to generate multi-layer pads which will need adjusting to be just top layer. Also we have just got the one component is this library. You will most likely want to copy this component into one of your own custom libraries you manage.


Another Useful Tip for Adding to Your Component Collection


Some manufacturers offer downloadable symbols and footprints for their components, for an example see Analog Devices' footprints and symbols page. These are in BXL format, a format that can be converted to use with your CAD package with the Ultra Librarian Free Reader application (a free download from their website). It's a somewhat ugly application where the fonts don't really fit the space allocated (at least on my system), however it is simple to use. Select the checkboxes for the output format (Altium P-CAD v15 and STP) and then load the BXL file, by default the outputs are saved in C:\UltraLibrarian\Library\Exported. You will really want to rename the files. YMMV as they say.


Remember to always check the imported library components. Just because you did not get any errors messages does not mean that it is correct. CAD conversion programs have always been somewhat hit and miss so it is vital that you check the results before using on a real design. Look out for pin mappings, pad sizes, SMD pads ending up on wrong side of board, orientations and anything else you can think of. Unless you are paranoid you are not worrying enough!


Standard disclaimer: The Ultra Librarian website and associated tools are mentioned here for interest only, they are not officially endorsed or supported by Altium or Premier Farnell.


Have Your Say


Let us know what you think and how we can do things better with CircuitStudio.

  • Have you tried this yourself?
  • Were the results acceptable?
  • Do you have a better workflow for importing Ultra Librarian components?
  • Do you know of a better library to import components from?