Eccentrically loaded gusseted equipment bracket

The primary engineering regression example with two rounded ribs, eight mounting holes, an eccentric bearing pad, multiaxial force, pressure, and self-weight. The simulation brief defines dimensions, assumptions, and acceptance criteria.

The 2026-09-06 test report (简体中文) records five passed integration tests across five real study solves in 208.16 seconds. The fine mesh has 27,980 nodes and 15,508 elements; maximum displacement is 0.019348617 mm and reported global stress maximum is 9.040418 MPa. Force/moment balance, mesh-change criteria, and full-field gravity-corrected linearity passed. The engineering aggregate remains WARN for the stated stress-review limitations. The static demonstration displays all five cases, both mesh-refinement steps, and three unchanged result views from mixed_5mm, with optional geometry and underside views.

The 252 passed / 20 skipped offline baseline belongs to the preceding validation round. Replacing the public example does not create a new test or solve record. Public evidence remains available at the stable summary, cases, and provenance paths.

This is one continuous solid. The ideal backing excludes bolt preload, slip, contact, and mounting compliance. Ribs and plates transfer load continuously; individual weld stresses are not modeled.

Inputs and dry-run

The committed STEP and its generated CAD properties are ready to use. CAD dependencies are required only to regenerate them. On the tested Windows host, use build123d==0.9.1 for regeneration (0.11.1 encountered a local system-font import error):

./.venv/Scripts/python.exe -m pip install "build123d==0.9.1"
./.venv/Scripts/python.exe examples/gusseted-bracket/generate_geometry.py

From the repository root:

./.venv/Scripts/python.exe -m ansys_skill.cli validate examples/gusseted-bracket/simulation.yaml --json
./.venv/Scripts/python.exe -m ansys_skill.cli run examples/gusseted-bracket/simulation.yaml --out build/bracket-dry-01 --json

The specification explicitly selects local Windows mechanical_batch. The command above remains DRY_RUN. After reviewing inputs and explicitly choosing to solve on an installed, licensed host:

./.venv/Scripts/python.exe -m ansys_skill.cli run examples/gusseted-bracket/simulation.yaml --out build/bracket-real-01 --execute --json

Five-solve engineering study

Install the project's dev and ansys extras as described in Windows testing. The development extra includes Pillow for complete PNG structure verification and pixel decoding.

The integration study performs three combined-load solves on 12, 8, and 5 mm quadratic meshes, then gravity-only and doubled force/pressure solves on the 5 mm mesh. Gravity stays constant.

It checks CAD-based force and moment balance, displacement convergence, pad stress statistics, whole-field linear superposition, native images, solver element/material settings, and input hashes. Force and moment relative tolerances are 0.5% and 1%. Both consecutive mesh refinements must meet 5% displacement and 10% pad stress-statistic thresholds. Pad mean and percentile statistics weight nodes equally, not by area. The 8 → 5 mm maximum-displacement change is 0.6556%. Full-field relative L2 error is 1.8077 × 10^-11, with no failing nodes at the stated per-node 1e-12 m + 1e-6 × ||predicted displacement|| tolerance.

Run serially with explicit opt-in and a fresh --basetemp directory:

$previousAvailable = $env:ANSYS_AVAILABLE
$previousBackend = $env:ANSYS_TEST_BACKEND
try {
    $env:ANSYS_AVAILABLE = "1"
    $env:ANSYS_TEST_BACKEND = "mechanical_batch"
    ./.venv/Scripts/python.exe -m pytest -q tests/integration/test_engineering_bracket.py --basetemp build/bracket-study-01 --junitxml=build/bracket-study-01.xml
}
finally {
    $env:ANSYS_AVAILABLE = $previousAvailable
    $env:ANSYS_TEST_BACKEND = $previousBackend
}

Pytest owns its temporary directory; choose a new path for each study. Each run retains engineering-checks.json, ordinary CLI reports, RST, saved Mechanical project, and solver logs. The study directory contains study-summary.json. An ordinary offline pytest -q skips real integration tests and starts no solver.

The general CLI still reports pressure/gravity reaction_balance: NOT_RUN; this fixture's separate checks supply the independently calculated resultants. safety_factor and automatic visual_review remain NOT_RUN; the recorded manual image review is separate. Global peak stress retains a review warning and is not a strength acceptance criterion. Compare the entire displacement field as u(2P+G) = 2u(P+G) - u(G); do not simply double displacement maxima that include self-weight.

export_views.py is an optional fixed Mechanical script for reopening a solved project and exporting Z-up and underside views. It requires ANSYS_AVAILABLE=1, BRACKET_VIEW_PROJECT (absolute saved project path), and BRACKET_VIEW_OUTPUT (new directory). It neither solves nor saves the project.