SOL 101 — Static Analysis

Simulation: Beam_sim1.sim Solver: NX Nastran SOL 101 (Linear Static) Status: Setup confirmed from KBS session (Gen 002). Baseline run needed.

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

Output	Method	Expression/Sensor	Status
Mass	NX expression	`p1` (NOT `p173`)	✅ Confirmed — 11.33 kg baseline
Tip displacement	❓ Sensor or .f06 parse	TBD	Gap G3, G6 — need baseline run
Von Mises stress	❓ Sensor or .f06 parse	TBD	Gap G4, G6 — need baseline run

⚠️ Mass expression changed: p1 confirmed in KBS session, replacing previous assumption of p173. Extractor config must be updated.

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:

Linear assumption: With 11.33 kg beam under 98 kN load, deflections may be significant relative to beam dimensions. L/δ ratio needs verification from baseline run.
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 estimate: Single beam, CQUAD4 thin shell → likely seconds per evaluation. 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 p1 (11.33 kg)
Baseline displacement measured (was 22 mm at old model state — needs re-verification G10)
Baseline stress measured (never had a value — G11)
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

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 p1. Material: AISI 1005.

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:

Open .sim file (loads chain)
Switch to Beam.prt — import .exp file, update expressions, rebuild geometry
Switch to Beam_fem1.fem — update FE model (remesh)
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

5.2 KiB Raw Blame History Unescape Escape