Part-DB.Part-DB-server/docs/usage/eda_integration.md

layout	title	parent
default	EDA / KiCad integration	Usage

EDA / KiCad integration

Part-DB can function as central database for EDA or ECAD software used to design electronic schematics and PCBs. You can connect your EDA software and can view your available parts, with the data saved from Part-DB directly in your EDA software. Part-DB allows to configure additional metadata for the EDA, to associate symbols and footprints for use inside the EDA software, so the part becomes directly usable inside the EDA software. This also allows to configure available and usable parts and their properties in a central place, which is especially useful in teams, where multiple persons design PCBs.

Currently only KiCad is supported!

KiCad Setup

{: .important }

Part-DB uses the HTTP library feature of KiCad, which is experimental and not part of the stable KiCad 7 releases. If you want to use this feature, you need to install a KiCad nightly build (7.99 version). This feature will most likely also be part of KiCad 8.

Part-DB should be accessible from the PCs with KiCAD. The URL should be stable (so no dynamically changing IP). You require a user account in Part-DB, which has the permission to access Part-DB API and create API tokens. Every user can has its own account, or you setup a shared read-only account.

To connect KiCad with Part-DB do following steps:

1. Create an API token on the user settings page for the KiCAD application and copy/save it, when it is shown. Currently KiCAD can only read Part-DB database, so a token with read only scope is enough.
2. Create a file partd.kicad_httplib (or similar, only the extension is important) with the following content:

{
    "meta": {
        "version": 1.0
    },
    "name": "Part-DB library",
    "description": "This KiCAD library fetches information externally from ",
    "source": {
        "type": "REST_API",
        "api_version": "v1",
        "root_url": "http://kicad-instance.invalid/en/kicad-api",
        "token": "THE_GENERATED_API_TOKEN"
    }
}    

3. Replace the root_url with the URL of your Part-DB instance plus /en/kicad-api replace the token field value with the token you have generated in step 1.
4. Open KiCad and add this created file as library in the KiCad symbol table under (Preferences --> Manage Symbol Libraries)

If you then place a new part, the library dialog opens and you should be able to see the categories and parts from Part-DB.

How to associate footprints and symbols with parts

Part-DB dont save any concrete footprints or symbols for the part. Instead Part-DB just contains a reference string in the part metadata, which points to a symbol/footprint in KiCads local library.

You can define this on a per-part basis using the KiCad symbol and KiCad footprint field in the EDA tab of the part editor. Or you can define it at a category (symbol) or footprint level, to assign this value to all parts with this category and footprint.

For example to configure the values for an BC547 transistor you would put Transistor_BJT:BC547 on the parts Kicad symbol to give it the right schematic symbol in EEschema and Package_TO_SOT_THT:TO-92 to give it the right footprint in PcbNew.