Non-standard Component Generation

[logmeintoautodesk]

Hi all,

I'm new to F360 electronics (but I have some long-ago Eagle experience).

I'm starting on a design that uses a chip with a somewhat unusual QFN package: TI BQ25792, a Li-Ion charger IC housed in a 29-pin VQFN-HR that has 9 pins left and right, 8 top and 7 bottom, plus it connects all corner pins. This is a little beyond the capabilities of the (very nice!) component generator, unfortunately.

What's the best strategy to efficiently create components like this, so that symbol, footprint and 3D component play nice?

• I've included the "texas" managed library, but it does not include this chip - possibly as it is very new. Are there more up to date fusion-compatible manufacturer libraries?
• Maybe create a 8x9 QFN with the package generator and modify the package? Does this auto-generate a matching footprint from the "Pad" sketch, or is the footprint generated to the pre-modification auto-generated package's specs? Are the physically modelled pins somehow connected up, eg for Electronics Cooling Simulation, or do they just need to line up with the Pads sketch?
• TI has symbol, footprint and 3D-models of the component for download at ultralibrarian.com. Downloading in Eagle format generates a .scr. Running this as script does create a component, but there's a ton of errors so I'm not sure all is well. Importing the step as 3D model works well, but I'm not sure how to link that as a 3D component.  One can also download as Autodesk 2D & 3D DXF, but I found no way to import this into fusion electronics design.
• TI offers a reference design including CAD files for Altium. This includes a library component of the BQ25792. Is there any way to import this into Fusion? Library.io apparently only imports from Eagle.
• Create everything by hand based on the schematic. Tedious, would like to avoid this if at all possible

I'd be grateful for pointers helping to not have to generate everything from scratch.

Best,

Alex

[AutomaticRock · Accepted solution]

Hi @logmeintoautodesk,

You can create the part using the files you downloaded.

I've done this a few times last week with some 3d packages so I tell you what I remember. At the moment I can't do the steps myself, so i might forget something. I'm also not sure if it works the same with the symbol and footprint. But I hope this will get you in the right direction.

For the 3d model:

• Have you uploaded the files to your project? If not use the upload button in your data panel.
• Open your library with your device. This is assuming you already have a device with symbol and footprint.
• Right click on your footprint and select Create new 3d model
• Now go to your data panel where you have uploaded your 3d model. Right click on it and select Insert in current design. Then move it around so it's aligned with the footprint.

I hope I have it right, this is what I remember doing. Let me know if it was helpful!

Best regards,

Benno

[logmeintoautodesk]

Hi @AutomaticRock, thanks a lot for the pointers, they were very helpful. Here's the steps I followed:

• I've downloaded the step file and eagle library from utralibrarian.com, and ran the .scr in the eagle library zip file. This created the device, symbol and footprint, but threw a bunch of errors. The symbol was empty, the footprint had the texts at wrong locations, and since the symbol was empty, the pin connections of course didn't work either.
• I've then Created a New Package, which already contained the footprint from the .scr in a sketch called Pad. (This also explains why changing the Pad sketch in an autogenerated 3D Package does not change the auto-generated 2D footprint - it's the other way round!). I inserted the step file downloaded from ultralibrarian, which fit the footprint perfectly. Phew.
• I then created the symbol and connected the pins by hand, easy enough.
• Finally, added some nice text with hyperlinks pointing to the TI datasheets and ultralibrarian for future reference as description

Presto! Easy when you know how.

There's some idiosyncrasy in the footprint with pins that connect on two edges of the QFN package, for which the ultralibrarian part has blocked the net to one pin and reduced the solder mask to the size of the copper layer. (See attached screenshot)

Not sure this is proper, the datasheet makes no mention of this. However, adjusting this by hand in ye olde eagle style of drawing footprints is very tedious, as the pins are on a wonky grid, and you apparently can't use dimensioned sketches for generating footprints yet. Anyway it's not an import issue, as the same idiosyncrasy also is visible in the ultralibrarian.com preview. So all good for now.

Cheers,

Alex