Conversation
…atic Working on a real multi-part MCU node board (STM32G474VETx, LQFP100) surfaced a few things worth capturing: - kicad-python's IPC API is broken against KiCad 10.0.5's own server in practice (import succeeds, get_open_documents() doesn't); documented a script-the-.kicad_sch-directly-and-verify-with-ERC fallback workflow, plus the coordinate transform that makes that tractable instead of guesswork. - Labels need to land on the exact wire/pin coordinate or ERC reports label_dangling/unconnected_wire_endpoint even though the render looks fine -- easy mistake when a script nudges a label for "readability". - Decoupling caps wired in series between a pin and its rail (instead of a parallel branch to ground) render identically to correct wiring but leave the pin floating at DC; ERC's power_pin_not_driven / ground_pin_not_ground is what actually catches it. - A PWR_FLAG placed near a rail but not actually wired onto it still trips power_pin_not_driven. - A practical tip for reviewing large schematics when an image tool chokes on a big SVG: temporarily shrink the page to a custom size that wraps just the review area, for more effective detail per pixel. - kicad-symbol: symbols using (extends "Base") -- common in ST's own KiCad MCU libraries -- need flattening into a standalone symbol before they can go in a schematic's lib_symbols block; noted the approach.
… a Value override Follow-up finding from the same OMNI-SENSE node schematic work: went to add a second isolated-domain power net (OMNI_+3V3_ISO etc.) by copying the existing "just rename a power symbol" advice -- overrode the instance's Value property while leaving lib_id pointed at +3V3/GND (or, worse, pointed lib_id straight at the new name with nothing defining it). Every instance came back as its own single-node net instead of merging, confirmed by exporting a netlist and reading it directly. The actual fix is a real duplicated symbol *definition* under the new name in lib_symbols. Also note the annotation-check gotcha discovered along the way (kicad-cli sch export netlist warns and continues on an unannotated schematic -- easy to miss since nothing fails loudly).
Third follow-up from the same OMNI-SENSE LTC2984 interface work: two decoupling/bypass nets (LDO output, VREF bypass) sat on pins only 5.08mm apart on the same IC edge. Both used the same fixed stub distance to clear the body, landing their vertical wire runs at the identical x. Since one run's y-range overlapped the other's, they touched at a coincident point and merged into one net -- caught via netlist export showing a 2-pin capacitor's own two pins sharing a net (shorted). Different stub lengths per net avoids it.
Document KiCad 10 + Windows agent pitfalls: kicad-cli full path, annotation warnings on netlist export, pcbnew Remove/SWIG crashes, pad+copper remapping after schematic net renames, and MCP footprint parity false positives when instance Footprint fields are blank. Co-authored-by: Cursor <cursoragent@cursor.com>
…umber Fourth follow-up from the OMNI-SENSE work: a hand-authored PCAL6524 symbol had its INT pin typed "output" (push-pull) when NXP's datasheet specifies open-drain. Wiring it to another chip's genuinely open-drain alert pin on the same net produced ERC's pin_to_pin type-conflict warning, which is what actually caught the mistake -- the wiring was fine, the symbol's declared pin type was wrong.
…-vs-content sizing Findings from OMNI-SENSE's I2C sensor cluster + isolation barrier layout pass (2026-09-07), driven by a user-reported "net names overlapping pins" bug, fixed via mechanical SVG text-bbox overlap detection rather than visual inspection alone: - A label's text anchors at the stub's far end and reads back toward the pin (verified from the exported SVG's own text-anchor position), so a long net name on a short stub overshoots into the IC's own pin-name text or a neighbour's label -- stub length needs to scale with name length, not use one fixed default for every label on a sheet. - Multiple pins at the exact same local (x, y) in a symbol's pin table (vendor-ganged IN/GND/OUT pins) are already electrically joined by one wire touching that point -- drawing a separate wire+symbol per duplicate pin adds visual clutter, not connectivity. - A block's own bounding box has to fit inside the sheet's declared paper size, or it lands off-page or under the auto-placed title block -- checked incrementally as content grows, not just visually at "fit whole page" zoom. - A shared decoupling branch off a pin at the edge of a tight pin column should extend away from the column (into open space), not further along the same axis parallel to the other pins it needs to clear. - A reusable technique for actually verifying "no overlapping text" on a dense sheet: parse the exported SVG's own <text> x/y/textLength/ font-size/text-anchor into real bounding boxes and check pairwise intersection, instead of eyeballing a render. Co-Authored-By: Claude Sonnet 5 <noreply@anthropic.com>
From OMNI-SENSE's relay-driver subcircuit (4x identical relay+TVS+ connector blocks stacked in a column, 2026-09-07): fixing a same-block label collision by lengthening one pin's stub repeatedly pushed the fix into colliding with the *next* repetition's own labels instead -- a whack-a-mole loop the stub-length lesson from the previous commit doesn't by itself warn against. Widening the inter-block pitch first (so no stub length, however long, can reach the next repetition) turned out to be the actual fix, with per-pin stub tuning only needed for collisions within a single repetition after that. Co-Authored-By: Claude Sonnet 5 <noreply@anthropic.com>
Document moving passives when corridors fail structural DRC, and the correct kicad-cli --severity-all JSON gate used on Omni-Harvester Phase1. Co-authored-by: Cursor <cursoragent@cursor.com>
This file contains hidden or bidirectional Unicode text that may be interpreted or compiled differently than what appears below. To review, open the file in an editor that reveals hidden Unicode characters.
Learn more about bidirectional Unicode characters
Sign up for free
to join this conversation on GitHub.
Already have an account?
Sign in to comment
1 participant
Add this suggestion to a batch that can be applied as a single commit.This suggestion is invalid because no changes were made to the code.Suggestions cannot be applied while the pull request is closed.Suggestions cannot be applied while viewing a subset of changes.Only one suggestion per line can be applied in a batch.Add this suggestion to a batch that can be applied as a single commit.Applying suggestions on deleted lines is not supported.You must change the existing code in this line in order to create a valid suggestion.Outdated suggestions cannot be applied.This suggestion has been applied or marked resolved.Suggestions cannot be applied from pending reviews.Suggestions cannot be applied on multi-line comments.Suggestions cannot be applied while the pull request is queued to merge.Suggestion cannot be applied right now. Please check back later.
Found while using kicad-schematic/kicad-symbol to build a real STM32G474VETx (LQFP100) node-controller schematic for an unrelated project. Everything here is a thing that actually went wrong once and cost time to diagnose:
get_open_documents()doesn't) — documented a fallback: script the.kicad_schS-expression text directly, validate withkicad-cli sch erc+ renders. Included the coordinate transform (abs = inst + local_x, inst - local_yat rotation 0) that makes hand/script-authored placement tractable instead of guesswork — verified empirically via an ERC report rather than assumed.label_dangling/unconnected_wire_endpoint, even though the rendered image looks completely fine. Cost 22 dangling labels in one pass from a 0.5mm "just for readability" offset.power_pin_not_driven/ground_pin_not_groundis what actually catches it — worth calling out since it's easy to get backwards when a script is drawing wires without a live visual editor giving instant feedback.power_pin_not_driven— proximity isn't the same as connectivity.(paper "User" w h)) that tightly wraps just the review area, so the same fixed image resolution shows more detail.(extends "Base")symbols — e.g. KiCad's ownMCU_ST_*libraries — need flattening into a standalone symbol before they can go in a schematic'slib_symbolsblock, with a short description of the approach (parse both symbols, merge properties with the derived symbol's overrides winning, rename the base's sub-units).🤖 Generated with Claude Code