Kicad 6.0 symbol for PIC16F887 (TQFP) does not exist

[newtekuser]

I have a Kicad 6 project that currently uses a PIC16F887 in DIP40 format that I'd like to convert to TQFP-44. I downloaded the footprint from mouser (I am well aware that footprints are not the same as symbols), put it in the 'KiCad\6.0\share\kicad\footprints\Package_QFP.pretty' directory and now I'd like to add the symbol for the TQFP package. How do I do that since no symbols exist for this type of package? Is there a place that I can get symbols for components that Kicad doesn't know about?

Kicad only knows about the DIP40 version with 40 pins.... is there any way around it, or should I move away from Kicad to something else more capable/polished? I'd be willing to spend up to $1000 for a CAD tool with a perpetual license that gives me a better user experience if someone can recommend one.

[newtekuser]

I found symbols and footprints on snapEDA for TQFN type, was able to make them show up, but Kicad is still not happy when I select the footprint on the Choose symbol screen. Very frustrating...

[julian1]

I'd like to convert to TQFP-44. I downloaded the footprint from mouser

tqfp-44 is unusual. Before associating the symbol with the footprint, check if kicad can view the downloaded footprint with the footprint editor?

Also, check the footprint quickly in a text editor, and verify it's not obviously corrupted and matches the expected syntax.

If the downloaded version is the issue, then it is possible to create the tqfp-44, by copying a modifying a tqfp-48 from the kicad library.

Otherwise if it can be viewed in the footprint editor ok, then recheck the path association/mapping from the symbol. It's more common to setup paths to manage your footprints and symbols separate from the kicad distribution libraries, although it shouldn't affect functionality.

[Doctorandus_P]

KiCad V7.0 has two TQFP-44 packages in it's default libraries. You can see them in the footprint editor when searching for tqfp and 44 (with a space in between).
If you want a custom footprint, there is also: Footprint Editor / File / Create Footprint / QFP**. These footprint wizards are python scripts, so you can also quite easily modify (copies of) these for more customization.

I don't know which file you got from Mouser. Why do you even think that file is compatible with KiCad?

In KiCad, schematic symbols are very loosely coupled with footprints. The schematic symbol just has a text string specifying which footprint to use. Any schematic symbol can be matched with any footprint, and KiCad has several tools to do this matching for single schematic symbols or in bulk. The Symbol Chooser only shows what is in the libraries. You add or modify footprint links after a symbol has been placed on the schematic.

And no matter which EDA suite you use, there will always be a need to create custom symbols and footprints. Creating custom footprints is just a part of the design process. And KiCad has quite good editors for both.

For your uC, you can just re-use the existing schematic symbol, but you will probably have to change the pin numbers, as it's unlikely pin assignments for a tqfp44 and a DIP40 are the same. To do this, first put the DIP 40 variant on your schematic, then hover the mouse cursor over it (no need to select it first) and press >[Ctrl + e] to load it in the Symbol editor. Then Symbol Editor / Edit / Pin Table gives you easy access to the pins to renumber them (and change other attributes) You can change the sort order by clicking on column headers. When finished, just close the Schematic symbol Editor, and it asks you whether you want to update the schematic with your changes.

If you want to do it "properly" you will also need some library management