Skill/references/schlib_parameters.md

Mandatory symbol parameters (.SchLib)

Vecmocon's Altium SOP (§5) requires every schematic-library symbol to carry a fixed set of parameters in its component properties (the panel shown in Altium: Properties → Parameters). This file defines that set, where each value comes from, and how the skill stamps them onto the .SchLib symbol.

How the parameters get in: the skill writes them directly into the .SchLib in pure Python via scripts/schlib_write.py — it rebuilds the OLE compound file around the enlarged component Data stream while preserving every other byte (all other streams, the directory tree, the Altium CLSIDs). It also removes the Ultra-Librarian default params Manufacturer_Name and Manufacturer_Part_Number (which duplicate the SOP Manufacturer / Manufacturer Part), the UL Copyright notice (Vecmocon symbols don't carry it), and the UL Component_Type (underscore) — replaced by Vecmocon's own spaced Component Type parameter (see below). The output is a ready .SchLib. Because this writes Altium's own format from outside Altium, the script self-checks that the result re-opens as a valid OLE with the params present — but always open the result in Altium once to confirm it loads before relying on it. (An older path, scripts/altium_params.py, instead emits an Altium DXP script to stamp the same parameters from inside Altium; keep it as a fallback if a particular file doesn't round-trip.)

The parameter set

Use these exact Altium parameter names (they must match the symbol, per the SOP screenshot). The Comment field is set to the MPN (SOP §4), and the Description field is the strict string from references/description_format.md — the same string as the part's Excel Description column. Both are written by schlib_write.py from the comment and description keys of params.json; neither is optional.

Parameter	Source	Notes
Component Type	derived	the part's Class — Resistor, Capacitor, Diode, Transistor, IC, … — from the taxonomy row for its typeid (scripts/common.py:class_folder(typeid))
Value	datasheet	the component value only (no package), in shorthand — e.g. 1u, 12p, 100n, 10k
Manufacturer Part	datasheet	the MPN; also the Comment field
Manufacturer	datasheet	manufacturer name as printed, e.g. YAGEO
Manufacturer Part 2	leave blank (for now)	second-source MPN — left empty by default; see optional note below
Manufacturer 2	leave blank (for now)	second-source manufacturer — left empty by default
Process	derived	assembly process from package: SMD → Reflow, through-hole → Wave/Manual; confirm
Vecmocon Part Code	engineer	internal code (e.g. VECESC2421) — not on the datasheet; ask
Operating Temperature	datasheet	full range, e.g. -55 °C to +125 °C
Tolerance	datasheet	e.g. 1% (or ±1%)
Datasheet	derived	Gitea link to the pushed <MPN>_data.<ext> — see below (SOP marks this optional)
ROHS	datasheet	RoHS compliance, Yes/No

Read the datasheet-sourced values from the actual datasheet — don't echo whatever text was handed to you. Open the PDF, find each real value (Value, Manufacturer Part, Manufacturer, Operating Temperature, Tolerance, ROHS, and Process by inference from the package), and fill them verified. An honest blank beats a guess — the SOP hides blank parameters, so a gap just stays empty until someone fills it. Only one field is purely internal and must come from the engineer: Vecmocon Part Code — ask for it.

The Datasheet field is a link, not a value read off the PDF. Point it at the datasheet this skill pushes into the part's Gitea folder (<MPN>_data.<ext>), so opening the symbol in Altium clicks straight through to the exact datasheet used. Build it from the config (GIT_HOST, LIBRARY_REPO in config/gitea.env) and the part's Class + tag:

https://<GIT_HOST>/<LIBRARY_REPO>/raw/branch/main/<Class>/<MPN>_<make>_<typeid>/<MPN>_data.<ext>

e.g. https://gitea.vecmocon.com/nitishKumar/library/raw/branch/main/Diode/BAT46WJ_Nexperia_SCH/BAT46WJ_data.pdf. Use the raw/branch/<default-branch> form (not src/…) so the URL opens the PDF directly; <Class> is class_folder(typeid) and <MPN>_<make>_<typeid> is the same tag the folder is pushed under, so the link always resolves to the file that lands in Gitea. Fill this link even on the first push of a new part — the push and the symbol write happen in the same run, so the URL is valid as soon as the part folder lands. (If for some reason the datasheet isn't being pushed to Gitea, leave Datasheet blank rather than writing a link that won't resolve.)

The second-source pair (Manufacturer 2 / Manufacturer Part 2) is left blank for now — don't populate it by default. It simply stays hidden in Altium until someone fills it later.

Optional: second-source cross-reference (currently off)

House preference right now is to leave Manufacturer 2 / Manufacturer Part 2 blank, so do not do this unless the engineer explicitly asks you to find a second source. It's documented here so it can be switched on later without redesigning anything.

If asked to find a second source, it is an equivalent part from a different manufacturer that could drop into the design unchanged:

1. Pull the original's form-fit-function specs from the datasheet — capacitance, voltage, tolerance, dielectric/temp class, package (for a cap); resistance, power, tolerance, package (for a resistor); and so on per type.
2. Search for an equivalent from a different manufacturer (distributor/parametric cross-reference, "equivalent to <MPN>", or another reputable maker's matching series). It must match every form-fit-function spec and be at least as good on tolerance / voltage / temperature — never worse.
3. Fill Manufacturer 2 = its maker, Manufacturer Part 2 = its exact MPN.

Two hard rules if this is ever used: never invent an MPN (only a part number you verified exists; else leave blank), and always flag the chosen second source for the engineer to confirm with the specs you compared.

Building the parameter set

Collect the values into a params.json (same spirit as part.json). component is the symbol's Library Ref (from altium_refs.py); omit it to apply to every component in the lib.

Two top-level fields sit alongside parameters and are both mandatory:

• description → the symbol's ComponentDescription. This must be byte-identical to the part's Excel Description column — the same strict Class_TYPEID_… string built to references/description_format.md. Build it once, use it in both places; never let the two drift. A symbol must never ship carrying Altium's No Description Available placeholder.
• comment → the Comment record's Text, which per SOP §4 is always the exact MPN.

Both are patched in place, so the records keep their other fields (Comment keeps its Location/Color/FontID); only the parameter block is dropped and re-added.

{
  "component": "CC0402FRNPO9BN120",
  "description": "Capacitor_CER_12pF_50V_±1%_0402_c0g",
  "comment": "CC0402FRNPO9BN120",
  "parameters": {
    "Component Type": "Capacitor",
    "Value": "12pF_0402",
    "Manufacturer Part": "CC0402FRNPO9BN120",
    "Manufacturer": "YAGEO",
    "Manufacturer Part 2": "0402N120F500CT",
    "Manufacturer 2": "Walsin Tech Corp",
    "Process": "Reflow",
    "Vecmocon Part Code": "VECESC2421",
    "Operating Temperature": "-55 °C to +125 °C",
    "Tolerance": "1%",
    "Datasheet": "https://gitea.vecmocon.com/nitishKumar/library/raw/branch/main/Capacitor/CC0402FRNPO9BN120_YAGEO_CER/CC0402FRNPO9BN120_data.pdf",
    "ROHS": "Yes"
  }
}

Writing them into the symbol

Write the parameters straight into the .SchLib, producing a new file:

python scripts/schlib_write.py --schlib <in>.SchLib --params params.json --out <out>.SchLib

params.json may carry a "remove" list (defaults to ["Manufacturer_Name", "Manufacturer_Part_Number", "Copyright", "Component_Type"]); those Ultra-Librarian defaults are stripped and the SOP params — including the spaced Component Type = Class — added. The script also sets ComponentDescription from "description" and the Comment Text from "comment", and warns on stderr if "description" is missing — treat that warning as an error and re-run with the Description rather than shipping the symbol. It targets the component named in "component" (its Library Ref / storage name), or every component if omitted, and self-checks the output re-opens as a valid OLE with the params and Description present. Deliver the resulting .SchLib, and have the engineer open it in Altium once to confirm it loads, then Save to Server with a revision note per the SOP.

The script needs the olefile package (pip install olefile) — its only non-stdlib dependency. Install it if the import fails.

Scope note: the d