ltspice-to-kicad-workflow

name

ltspice-to-kicad-workflow

description

Use when taking a power-supply or analog-circuit idea all the way from LTspice simulation to a verifiable KiCad project (schematic + PCB + footprints + ERC/DRC). Covers ADI/LTC µModule demo-board adaptation, ASC → KiCad conversion, BGA functional-pad footprints, 4-layer stackup conversion, input protection hardening, datasheet-driven pin verification, kicad-cli-driven verification, and the structural ASC ↔ KiCad netlist cross-check. Companion to any project-specific LTspice skill — use that one for simulation, this one for everything between sim and a clean DRC pass. Out of scope: gerber generation as an acceptance artifact, certification/compliance, mechanical/thermal proof, custom IC design.

LTspice → KiCad Workflow

End-to-end recipe for going from a circuit idea through LTspice validation to a KiCad project that loads cleanly, passes ERC and DRC under kicad-cli, and is honest about what is verified vs. inferred. Distilled from a 48V → 5V → 1V/10A two-stage µModule design (LTM8064 + LTM4658) and the bugs that surfaced along the way.

When to use this skill

Trigger this skill when the user:

• Has an LTspice .asc (or wants to create one) for an analog / power circuit and intends to fabricate a board.
• Asks to generate, fix, or review a KiCad project derived from an LTspice schematic.
• Asks to harden a prototype-review board for production: cap derating, input protection, layer-count upgrade, real footprints.
• Wants to verify a KiCad project against the source .asc topology.
• Hits "Failed to load board" or DRC violations on a hand-edited .kicad_pcb.

If the user is only doing simulation work (no PCB), hand off to whatever LTspice-only skill they already have. If they want gerbers, certification, or thermal/mechanical analysis, those are out of scope.

High-level flow

1. Idea / specs              → V_in, V_out, I_load, transient targets
2. Part selection            → ADI / LTC µModule catalog, demo-board match
3. LTspice schematic         → copy demo values; add load; .tran startup
4. Sim validation            → vbus_avg, vcore_avg, iload_avg within tol
5. KiCad generation          → symbols, footprints, sch, pcb, netlist
6. Hardening pass            → cap V ratings, input protection, layer count,
                                real footprints
7. kicad-cli verification    → erc, drc (--refill-zones --save-board),
                                jumper-strip drc gate, netlist re-export
8. Structural cross-check    → netlist_comparison.py (ASC ↔ KiCad nets)
9. Document deferred work    → README + drc.rpt / erc.rpt match reality

Each stage below lists the artefacts to produce, the gotchas to avoid, and the verification check that gates moving to the next stage.

Stage 1 — Specs

Pin down before touching tools:

• Input voltage range and worst-case transient
• Output voltage(s) and per-rail load current
• Switching frequency target (sets external R_T values)
• Protection envelope (fuse rating, max V on TVS, expected ESD class)
• Layer count and copper weight constraints (cost vs. current density)

For high-current rails write down the load resistance you'll simulate with (V_out / I_load, e.g. 1V / 10A = 0.1 Ω) — this is the Rload that must be deleted from the PCB later.

Stage 2 — Part selection

For ADI/LTC µModules:

• Match the demo board (e.g. DC2237A for LTM8064 5V output, DC2861A for LTM4658) — copy its component values verbatim into the ASC. The feedback resistor formulas vary by part; the demo's RFB / RT values encode the right answer and the LTspice model agrees.
• Note the package: BGA-25 / BGA-108 / LGA / etc. and the ball pitch. Used in Stage 5 footprint work.

Stage 3 — LTspice schematic

Conventions that pay off downstream:

• Name every instance after its role with the part prefix, e.g. C8064_OUT1, R4658_FB_TOP. This carries through as the KiCad ASC_REF property and makes the netlist cross-check trivial.
• Place a single voltage source V1 for the input — it becomes the input connector J1 on the PCB.
• Include a load resistor with a clearly review-only name (e.g. Rload, value 0.1). It is for sim only.
• Add .save, .tran startup, and at least three .meas lines:

  .meas TRAN vbus_avg  AVG V(BUS5)  FROM=0.7m TO=1m
  .meas TRAN vcore_avg AVG V(OUT1V) FROM=0.7m TO=1m
  .meas TRAN iload_avg AVG I(Rload) FROM=0.7m TO=1m
  

• Cap voltage ratings on the ASC SpiceLine (V=6.3 Rser=5m) are the values that will get carried over to the PCB BOM. They are usually too tight — the demo board uses 6.3V rated parts on 5V rails because the demo isn't a product. Note these for the hardening pass.

Stage 4 — Sim validation

Two passes:

1. Smoke — .tran 1m startup, just confirm convergence and no model errors.
2. Steady-state — extend to 2.5m, measurement window 2m–2.5m so the averages reflect settled operation. Compare vbus_avg, vcore_avg, iload_avg against spec; ±2% is typical.

Save the validation .asc separately (don't overwrite the source) so the "this design simulates to spec" evidence is traceable.

Stage 5 — KiCad generation

The artefacts you need:

• *.kicad_pro, *.kicad_sch, *.kicad_pcb (project, schematic, board)
• <lib>.kicad_sym with symbol definitions for each unique part
• <lib>.pretty/<footprint>.kicad_mod for any custom footprints (the µModule BGAs typically)
• sym-lib-table, fp-lib-table listing the local libs + any KiCad standard libs the project uses (Capacitor_SMD, Resistor_SMD, Diode_SMD, Fuse, TestPoint, TerminalBlock_Phoenix)

Decisions to make up front:

• Pad numbering for BGAs. Two schemes, with a hard boundary between them:
  1. Function-named pads. Pad number is "VIN" / "GND" / "VOUT" / etc., so the schematic symbol can use the same names as pin numbers and net-mapping is automatic. Requires duplicate_pad_numbers_are_jumpers yes on the footprint. Review-grade only — the result is NOT fabricable. The jumper flag asserts the component itself bridges same-numbered pads, so DRC passes with no physical copper between them (the rev A reference board hid 94 unconnected pads this way — every GND return, the 10A output, both feedback balls). The Stage 7 jumper-strip gate exposes this.
  2. Ball-numbered pads. Pad number is "A1" / "M9" / etc. — one pad per ball, real fanout, no jumper flags. Required for production. The working pattern (from the rev B reference board):
     • Symbol: one visible pin per function, plus hidden passive duplicates stacked at the same coordinates — every ball gets its net assignment while wires stay attached to the single visible pin.
     • BGA power/ground: strap mesh across same-net ball clusters plus dogbone vias into the inner planes (the GND via field doubles as the thermal path).
     • Fine-pitch interior balls (e.g. 0.65 mm): escape between balls with 0.12 mm track / 0.1 mm clearance rules — confirm the fab can hold them before ordering.
     • Where the F.Cu fill would split into islands, add explicit B.Cu bridges. KiCad's DRC does not credit "the inner plane will carry it" unless the connecting copper is actually drawn and stitched. Start with scheme 2 unless the board is explicitly a throwaway review; converting 1 → 2 later is a full footprint + symbol + fanout rebuild, not an edit (the rev A → rev B transition was a scripted rebuild).
• Layer count. 2-layer is fine for low-power. For ≥5 A rails on a small board, default to 4-layer (signal / GND / power / signal). The hardening pass converts 2 → 4 if needed.

Stage 6 — Hardening pass (the part most generators skip)

Six checks. Walk them every time.

6a. Cap voltage ratings

Aim for ≥2× the DC working voltage on MLCC, more if you care about de-rating under DC bias. Bulk caps need transient margin too.

Common mistakes inherited from demo boards:

• 6.3V cap on a 5V rail → bump to 16V.
• 100V cap on 48V → marginal; add a 100V/22µF aluminum-polymer bulk.

6b. Remove sim-only parts

Rload (the load resistor) must come out of:

• the KiCad schematic instance
• the PCB footprint instance and any routes that only go to it
• the static schematic.net export

Keep it in the ASC if you want re-runnable simulation evidence.

6c. Input protection

For 48V inputs add (at minimum):

Part	Footprint	Net wiring
F1	Fuse:Fuse_1206_3216Metric	series J1 → F1 → IN48
D1	Diode_SMD:D_SMB (SMBJ58A)	K=IN48, A=GND
C8	Capacitor_SMD:CP_Elec_10x10	+ = IN48, − = GND, 22µF/100V

A new net IN48_RAW sits between J1 and F1; everything else stays on IN48. Update the symbol library if you didn't have a Fuse or D_TVS symbol — examples in references/protection_symbols.kicad_sym.

6d. Layer-stack conversion (2 → 4)

In the PCB (layers …) block, add inner layers between F.Cu and B.Cu. Use this exact form (signal type, IDs in the free even-number range):

(layers
    (0 "F.Cu" signal)
    (4 "In1.Cu" signal)
    (6 "In2.Cu" signal)
    (2 "B.Cu" signal)
    ; … user layers unchanged
)

Do not use power as the layer type — KiCad 10's PCB loader rejects it with a generic "Failed to load board" error.

For each via, the (layers …) field is start-layer end-layer, NOT a list of every layer touched. A through-via stays (layers "F.Cu" "B.Cu") even on a 4-layer board; the copper rings on inner layers are implicit. Writing (layers "F.Cu" "In1.Cu" "In2.Cu" "B.Cu") makes the file unloadable.

Add these zones (declare polygons, skip (filled_polygon …) — let kicad-cli pcb drc --refill-zones --save-board compute them):

• In1.Cu / GND / full-board rectangle
• In2.Cu / GND / full-board rectangle (priority 0 — gets overridden by power islands)
• In2.Cu / IN48 / island enclosing input components, priority 1
• In2.Cu / BUS5 / island enclosing stage 1 output, priority 2
• In2.Cu / OUT1V / island enclosing stage 2 output, priority 3

6e. Real BGA land patterns

Replace any "functional pads" / "review" footprint with the datasheet-accurate one:

• Ball pitch and body size exactly per ADI datasheet.
• Pad diameter: NSMD, 75–80% of ball diameter (e.g. 0.30 mm for the 0.40 mm balls of an LTM4658, 0.60 mm for the ~0.75 mm balls of an LTM8064).
• Annotate ball positions (A1, B2, … M9) on F.Fab so reviewers can cross-check the datasheet.
• Retain perimeter SMD "fan-out" rectangles if the original footprint had them. They are not visual review aids — they are bridging copper that PCB routes terminate on, and duplicate_pad_ numbers_are_jumpers merges them with the same-name balls. Removing them silently breaks ~17 same-net connections per part.
• Verify the GND fill convention by web-sampling at least one ball per bank against the datasheet pin table.

6f. Schematic & PCB consistency

If you renamed a net (e.g. IN48 → IN48_RAW for the section ahead of the fuse), update all four places:

• the schematic label (label "IN48_RAW" on the J1-side wire)
• the PCB pad (net "…") field on J1.1
• the netlist export (schematic.net)
• the validation script's expected-net table

Stage 7 — kicad-cli verification

This is the difference between "looks right" and "actually loads".

$cli = 'C:\Program Files\KiCad\10.0\bin\kicad-cli.exe'
$proj = '<path to project>'

# Hard checks
& $cli sch erc --severity-error --output "$proj\erc.rpt" "$proj\*.kicad_sch"
& $cli pcb drc --refill-zones --save-board --severity-error `
        --output "$proj\drc.rpt" "$proj\*.kicad_pcb"

# Regenerate the netlist
& $cli sch export netlist --output "$proj\schematic.net" "$proj\*.kicad_sch"

# Optional: broader inspection
& $cli pcb drc --schematic-parity --severity-all `
        --output "$proj\drc_full.rpt" "$proj\*.kicad_pcb"

Expectation after the hardening pass: 0 ERC errors, 0 DRC errors, 0 unconnected pads — and 0 unconnected items in the jumper-strip run below, if it applies. Schematic-parity warnings about stale Value / ASC_REF strings on inline PCB footprints are cosmetic; the user can clear them with Tools → Update PCB from Schematic in the GUI. Treat net_conflict parity warnings as real until each one is individually read — they can hide pad-number swaps (see pitfalls table).

Jumper-strip gate (mandatory if any footprint uses duplicate_pad_numbers_are_jumpers)

Normal DRC is blind to missing copper on these footprints: the jumper flag asserts the component bridges same-numbered pads even when the "bridge" pads lie outside the package body. Test the physical copper by stripping the flag from a copy of the board:

$strip = "$proj\drc_strip_check.kicad_pcb"
$text  = Get-Content "$proj\<project>.kicad_pcb" -Raw
$text  = $text -replace '(?m)^[ \t]*\(duplicate_pad_numbers_are_jumpers yes\)[ \t]*\r?\n', ''
# UTF-8 WITHOUT BOM — Set-Content writes a BOM and KiCad then fails
# with "Failed to load board"
[System.IO.File]::WriteAllText($strip, $text, [System.Text.UTF8Encoding]::new($false))
& $cli pcb drc --refill-zones --output "$proj\drc_strip.rpt" $strip
Remove-Item $strip   # or it gets swept up by later *.kicad_pcb wildcards

The unconnected-items count in drc_strip.rpt is the physical-copper truth. The rev A reference board passed normal DRC clean and showed 94 unconnected pads here (all GND returns, the 10A output, both feedback balls). Anything non-zero means the board relies on virtual bridging and is not fabricable — go back to Stage 5 and build scheme 2 footprints. On a scheme-2 board the flag doesn't exist and this gate is a no-op.

If pcb drc fails with "Failed to load board" and no line number, work backward through the recent edits — most often the via (layers …) mistake from 6d, or a layer type other than signal / user. Bisect by reverting commits or by progressively removing recent additions.

Stage 8 — Structural cross-check (ASC ↔ KiCad)

Behavioral sim says "the values work." Structural check says "the KiCad net topology matches the ASC." Both are needed because either can silently break without the other noticing.

validation/netlist_comparison.py (template in references/netlist_comparison.py):

• Parses ASC SYMATTR InstName lines to enumerate the ASC's components.
• Parses the KiCad-exported schematic.net for component refs and net membership.
• Uses a hardcoded EXPECTED_ASC_TO_KICAD map (ASC name → KiCad ref) and EXPECTED_NETS table (key nets → expected member refs) to do the comparison.
• Tolerates a KICAD_ONLY_REFS set for KiCad-only additions (J1 replacing V1, J2/J3 monitors, TP1–TP9, F1/D1/C8 protection).

Do not try to parse LTspice net connectivity geometrically — the ASC format requires symbol library pin offsets that aren't reliably shipped with the project. The hardcoded expected-net table is the honest approach.

Stage 9 — Document deferred work

If something can't be auto-checked here, write it down. README sections that pay off:

• Verification log — exact kicad-cli invocations, the numerical results, and the date / KiCad version.
• Important limitations — what's verified vs. inferred (e.g. "67 GND-by-convention balls sampled across 9 of 12 banks").
• Remaining work — what the user must do in the GUI before fab (typically: Update PCB from Schematic for parity hints, then cross- check footprints against the latest ADI mechanical drawing for the ordering code).

Common pitfalls & fixes

Symptom	Cause	Fix
kicad-cli pcb drc → "Failed to load board"	Via (layers …) lists all 4 layers instead of start/end	Revert to (layers "F.Cu" "B.Cu") for through-vias
Same error after layer-type change	Used power or mixed instead of signal / user in (layers …)	Use only signal or user
17+ unconnected pads after BGA footprint "cleanup"	Removed perimeter fan-out rectangles	Restore them; they're bridging copper, not visual decor
DRC reports clearance violations on existing pads after refill	Stale filled_polygon from before the recent additions	Run pcb drc --refill-zones --save-board once
"Via dangling" warnings on new vias inside an inner-layer zone	Zone fill hasn't anchored to the via	Cosmetic; F.Cu zone of same net provides the load-bearing path
259 schematic-parity warnings on Value / ASC_REF mismatches	PCB inline footprint properties stale vs. schematic	Tools → Update PCB from Schematic in the GUI
Netlist comparison flags IN48_RAW missing	Forgot to update one of: schematic label, PCB pad net, schematic.net, expected-table	Update all four
ERC reports 100+ endpoint_off_grid warnings	Generator emitted pins on a non-100mil grid	Filter with --severity-error; the warnings are cosmetic
Schematic-parity net_conflict warnings dismissed as net-name noise	Real pad-number swaps buried in the noise (rev A: J1/J2/J3 power and GND pads swapped vs. schematic pins, under 199 net-name-prefix warnings)	Sync net-name forms (/NET vs NET) first, then re-read every remaining net_conflict individually

Folder layout

project_root/
├─ <project>.kicad_pro
├─ <project>.kicad_sch
├─ <project>.kicad_pcb
├─ <project>.kicad_prl
├─ <lib>.kicad_sym
├─ <lib>.pretty/
│  ├─ <bga1>.kicad_mod
│  └─ <bga2>.kicad_mod
├─ sym-lib-table
├─ fp-lib-table
├─ schematic.net           ; KiCad-exported, do not hand-edit if possible
├─ erc.rpt                 ; from kicad-cli sch erc --severity-error
├─ drc.rpt                 ; from kicad-cli pcb drc --refill-zones --save-board
├─ README.md               ; verification log, limitations, deferred work
└─ validation/
   ├─ <project>_validation.asc      ; extended .tran for measurements
   ├─ ltspice_validation_summary.md ; sim numbers + cross-check approach
   └─ netlist_comparison.py         ; ASC ↔ KiCad structural diff

References

• references/netlist_comparison.py — template for stage 8
• references/protection_symbols.kicad_sym — Fuse + D_TVS symbol snippets
• references/four_layer_zones.kicad_pcb_snippet — In1.Cu / In2.Cu zone declarations
• ADI demo board manuals (DC22…, DC28…) carry the canonical RFB / RT values
• KiCad 10.0 documentation for the kicad-cli subcommand surface

What to hand back

When this skill finishes, the user should have:

1. A KiCad project that loads cleanly under kicad-cli.
2. erc.rpt and drc.rpt documenting 0 errors and 0 unconnected pads (plus drc_strip.rpt if any footprint carries the jumper flag).
3. A validation/ directory whose Python script passes against the project's own ASC.
4. A README that names every revision and the date / KiCad version that verified it.