Atomizer/projects/hydrotech-beam/kb/fea/models/sol101-static.md

SOL 101 — Static Analysis

Simulation: Beam_sim1.sim Solver: NX Nastran SOL 101 (Linear Static) Status: ✅ Running — first real results obtained 2026-02-11. Automated DOE pipeline operational.

---

Setup — Confirmed

Item	Value	Source	Notes
Solution type	SOL 101 (Linear Static)	KBS session	"Solution 1 — static subcase"
Element type	CQUAD4 (4-node quad shell)	KBS session	✅ Confirmed — thin shell collectors
Property type	Thin shell	KBS session	Material inherited from "beam material"
Mesh density	Element size = 33.7 mm (67.4 / 2)	KBS session	Subdivision-based. Future refinement planned.
Idealization	Promote body → mid-surface extraction	KBS session	Pair mid-surface function

Boundary Conditions — Confirmed

BC	Location	Type	Value	Source
Fixed constraint	Left side of beam (full edge)	SPC (all 6 DOF)	Fixed	✅ KBS session — "left side fixed"
Applied force	Right side of beam (free end)	Point/edge force	10,000 kgf downward (−Y)	✅ KBS session — "project requirement"

Loading Details

• Force magnitude: 10,000 kgf = 98,066.5 N (≈ 98.1 kN)
• Direction: Downward (−Y in model coordinates)
• Application: Right side (free end) of beam
• Type: This is a cantilever beam with end loading — classic bending problem

Result Extraction — Confirmed (Gen 003)

Output	Method	Expression/Sensor	Status
Mass	NX expression	p173 (body_property147.mass in kg)	✅ Confirmed — journal extracts to _temp_mass.txt
Tip displacement	OP2 parse via pyNastran	Max Tz at free end	✅ Working — 17.93 mm at baseline-ish DVs
Von Mises stress	OP2 parse via pyNastran	CQUAD4 shell max VM	✅ Working — 111.9 MPa at baseline-ish DVs

Mass extraction: Journal extracts p173 expression after solve and writes _temp_mass.txt. Python reads this file. Expression p1 from KBS session was incorrect — p173 confirmed via binary introspection.

pyNastran note: Warns "nx version 2512 not supported" but reads OP2 files correctly. Stress output from pyNastran is in kPa — divide by 1000 for MPa.

Mesh Details

Property	Value	Notes
Element type	CQUAD4	4-node quadrilateral, first-order
Element size	33.7 mm	67.4 / 2 — Antoine says refinement is "not for now"
Mesh method	Subdivision-based	Auto-mesh with size control
Shell formulation	Thin shell	Mid-surface extracted from solid
Convergence	❓ NOT VERIFIED	Gap G8 partially closed (type known), but convergence check still needed

Mesh Estimate

• Beam length 5,000 mm / 33.7 mm ≈ 148 elements along length
• Perimeter of I-beam cross-section ≈ varies — but total mesh likely 10K–50K elements
• Expected DOF: 60K–300K → SOL 101 solve time: seconds to low minutes

Solver Considerations

From Technical Breakdown (Gen 001), updated with KBS data + Gen 003 run data:

• Linear assumption: With 1,133 kg beam under 98 kN load, deflections are ~18 mm at 5,000 mm span. L/δ ≈ 280 — linear assumption is reasonable.
• Mesh sensitivity: Stress at hole edges is mesh-dependent. CQUAD4 at 33.7 mm may not fully resolve SCF at 300 mm diameter holes (~28 elements around circumference — probably adequate but needs verification).
• Mesh morphing vs remesh: Parametric NX models typically remesh on update. Need to confirm behavior across DV range (Gap G7).
• Runtime: ✅ Confirmed ~12 seconds per evaluation (single beam, CQUAD4 thin shell on dalidou). Very fast.
• Unit system: NX model uses kg-mm-s (kgf for force). Nastran output stress in kPa → divide by 1000 for MPa.

Validation Checklist

• Baseline mass matches NX expression p173 (1,133.01 kg)
• Displacement measured — 17.93 mm at baseline-ish DVs (G10 closed)
• Stress measured — 111.9 MPa at baseline-ish DVs (G11 closed)
• Mesh convergence verified at baseline
• Mesh quality acceptable at DV range extremes
• Model rebuilds cleanly at all 4 corners of design space (Gap G7)
• Stress at hole edges resolved with current mesh density

NX Version & Environment — Confirmed (Gen 003)

Item	Value	Notes
NX Version	DesigncenterNX 2512	Siemens rebranded NX to "DesigncenterNX"
Install path	C:\Program Files\Siemens\DesigncenterNX2512	On dalidou (Windows solver node)
Previous config	NX 2412	❌ Failed — "Part file is from a newer version"
pyNastran compat	Warns "nx version 2512 not supported"	✅ But reads OP2 files correctly

⚠️ Critical lesson (2026-02-11): Solver was originally configured for NX 2412 but model files are from DesigncenterNX 2512. NX refuses to load with "Part file is from a newer version." Must match version exactly.

Path Resolution on Windows — Critical

Bug discovered: Path.absolute() on Windows does NOT resolve .. components (unlike Path.resolve()).

# WRONG — leaves ".." in path, NX can't find referenced parts
path = Path("../../models/Beam_sim1.sim").absolute()
# → C:\Users\antoi\Atomizer\projects\hydrotech-beam\studies\01_doe_landscape\..\..\models\Beam_sim1.sim

# CORRECT — fully resolves path
path = Path("../../models/Beam_sim1.sim").resolve()
# → C:\Users\antoi\Atomizer\projects\hydrotech-beam\models\Beam_sim1.sim

Rule: Use .resolve() everywhere when constructing paths for NX. NX cannot follow .. references in paths.

NX File References — In-Place Solving Required

NX .sim files store absolute internal references to .fem and .prt files. Copying model files to iteration folders breaks these references (Parts.Open returns None).

Solution: Solve on master model in-place (in the models/ directory) with backup/restore for isolation:

1. Backup master model files before each trial
2. Write expressions, rebuild, solve in models/
3. Archive outputs (OP2, F06, params, results) to iteration folder
4. Restore master from backup

See DEC-HB-008 in DECISIONS.md.

History

• Gen 001 (2026-02-09): Initial documentation from technical breakdown. All solver details pending gap resolution.
• Gen 002 (2026-02-10): Confirmed from KBS session — CQUAD4 thin shell, 33.7 mm element size, cantilever BCs (left fixed, right 10,000 kgf down), mass via p173. Material: AISI 1005.
• Gen 003 (2026-02-11): First real results! DesigncenterNX 2512 version confirmed, path resolution bugs fixed, backup/restore in-place solving architecture, mass extraction via journal. Displacement=17.93mm, Stress=111.9MPa, Solve time ~12s/trial.

NX Automation Workflow

This model uses the SIMPLE workflow (single-part, no assembly FEM).

Simple Workflow Chain

Beam.prt (geometry) → Beam_fem1_i.prt (idealized/mid-surface) → Beam_fem1.fem (mesh) → Beam_sim1.sim (solve)

Steps:

1. Open .sim file (loads chain)
2. Switch to Beam.prt — import .exp file, update expressions, rebuild geometry
3. Switch to Beam_fem1.fem — update FE model (remesh)
4. Switch back to .sim — solve SOL 101

Assembly FEM Workflow (NOT used here)

For multi-part models with .afm files (e.g., SAT3 mirror):

• Additional steps: load all components, update each FEM, merge duplicate nodes, resolve label conflicts
• Detected automatically by presence of .afm files in working directory

Key Automation Notes

• hole_count expression unit = Constant (not MilliMeter)
• All length DVs = MilliMeter
• FEM part is Beam_fem1 — NOT Beam_fem1_i (idealized)
• Journal: solve_simulation.py handles both workflows