ABAQUS Multiphysics Diffusion UEL

A coupled multiphysics finite element implementation for moisture diffusion in epoxy materials with stress-assisted transport mechanisms.

🔬 Overview

This project implements a User Element (UEL) for ABAQUS that simulates the coupled hydro-mechanical behavior of moisture diffusion in polymer materials. The element captures bidirectional coupling between mechanical stress fields and moisture transport phenomena, making it a multiphysics simulation.

Key Physics

• Stress-assisted diffusion: Hydrostatic stress influences moisture transport
• Coupled field equations: Simultaneous solution of mechanical and diffusion problems
• Nonlinear coupling: Stress gradients create preferential diffusion pathways

✨ Key Features

• 🔧 Multiphysics Coupling: Stress-assisted diffusion with hydrostatic stress influence
• 🧮 20-Node Elements: Quadratic hexahedral elements with 80 DOF (60 mechanical + 20 concentration)
• ⚡ Monolithic Solution: Simultaneous solution of mechanical and diffusion fields
• 🔗 ABAQUS Integration: Full integration with ABAQUS Standard
• 📊 Visualization Support: MATLAB tools for result post-processing
• 🧪 Material Flexibility: Configurable material properties for different polymers

📐 Governing Equations

Coupled Diffusion Equation

∂c/∂t = ∇·(D∇c) - (D·Vh)/(R·T) ∇·(σh∇c)
         ↑_______↑   ↑_________________↑
      Pure diffusion   Stress-assisted term

Mechanical Equilibrium

∇·σ = 0
σ = D:(ε - εswelling)

Coupling Parameter

κ = Vh/(R·T) = 8000/(8314.5 × 300) ≈ 3.2 × 10⁻³ MPa⁻¹

Where:

• c: Moisture concentration [mol/mm³]
• D: Diffusion coefficient [mm²/s]
• σh: Hydrostatic stress [MPa]
• Vh: Molar volume of water (8000 mm³/mol)
• R: Gas constant (8314.5 J/(mol·K))
• T: Temperature (300 K)

🚀 Quick Start

Prerequisites

• ABAQUS Standard 2020 or later
• Intel Fortran Compiler (part of ABAQUS installation)
• MATLAB R2018a or later (for visualization)
• Windows/Linux operating system

Basic Usage

1. Download the UEL

   git clone https://github.com/BBahtiri/ABAQUS-Multiphysics-Diffusion-UEL.git
   cd ABAQUS-Multiphysics-Diffusion-UEL

2. Run ABAQUS analysis

   abaqus -standard -job MyAnalysis -user Diffusion_3D.for

3. Generate visualization mesh (MATLAB)

   % Place your ABAQUS input file as 'CT.inp'
   run('VisualMesh.m')

4. Post-process results in ABAQUS/Viewer

Element Definition in ABAQUS Input File

*USER ELEMENT, NODES=20, TYPE=U1, PROPERTIES=3, COORDINATES=3, VAR=128
1,2,3
1,11

*ELEMENT, TYPE=U1, ELSET=SOLID
1, 1, 2, 3, 4, 5, 6, 7, 8, 9, 10, 11, 12, 13, 14, 15, 16, 17, 18, 19, 20

*UEL PROPERTY, ELSET=SOLID
210000., 0.3, 0.0127
! E [MPa], ν [-], D [mm²/s]

🔬 Physics and Theory

Multiphysics Coupling Mechanisms

1. Mechanical → Diffusion Coupling

• Tensile stress (σh > 0): Enhances diffusion by opening material microstructure
• Compressive stress (σh < 0): Reduces diffusion by closing pore networks
• Stress gradients: Create preferential diffusion pathways

2. Stress-Diffusion Interaction

The coupling term (Vh/RT)∇·(σh∇c) represents:

• Pressure-driven moisture transport
• Stress-concentration effects
• Hydrostatic stress influence on chemical potential

Element Implementation

• Element Type: 20-node quadratic hexahedral (C3D20-like)
• Integration: 8-point Gauss quadrature
• DOF: 80 total (3 displacement + 1 concentration per node)
• Time Integration: Backward Euler for diffusion
• Convergence: Monolithic Newton-Raphson

🏭 Applications

Aerospace Industry

• Composite laminates: Carbon fiber/epoxy moisture absorption
• Environmental certification: Hot/wet qualification testing
• Stress concentration: Bolt holes and cutouts in humid environments

Marine Engineering

• Underwater structures: Pressure vessel moisture penetration
• Adhesive joints: Combined mechanical and environmental loading
• Fatigue analysis: Moisture-assisted crack growth

Electronics Packaging

• IC encapsulation: Moisture diffusion under thermal cycling
• Reliability testing: Combined thermal-mechanical-moisture effects
• Delamination prediction: Interface failure mechanisms

Infrastructure

• Bridge components: Moisture penetration under traffic loads
• Protective coatings: Mechanical damage accelerating moisture ingress
• Durability assessment: Long-term environmental degradation

📊 Material Properties

Typical Values for Epoxy Materials

Property	Symbol	Value	Unit
Young's Modulus	E	3000-4000	MPa
Poisson's Ratio	ν	0.35-0.40	-
Diffusion Coefficient	D	1×10⁻³ - 1×10⁻²	mm²/s
Molar Volume (Water)	Vh	8000	mm³/mol
Temperature	T	300	K

Property Variations

• Temperature dependence: D = D₀ exp(-Q/RT)
• Concentration dependence: D = D₀(1 + βc)
• Stress dependence: Implemented through coupling term

🔧 Advanced Usage

Custom Material Properties

*UEL PROPERTY, ELSET=MATERIAL_A
! E [MPa], ν [-], D_step1 [mm²/s], D_step2 [mm²/s]
3500., 0.37, 0.008, 0.012

Boundary Conditions

! Moisture flux boundary condition
*DFLUX
NodeSet_Surface, 11, 1.0E-6

! Concentration boundary condition  
*BOUNDARY
NodeSet_Exposed, 11, 11, 0.1

Multi-Step Analysis

*STEP, NAME=Drying
*COUPLED TEMPERATURE-DISPLACEMENT, STEADY STATE
! Use D = props(3)

*STEP, NAME=Loading  
*COUPLED TEMPERATURE-DISPLACEMENT
! Use D = props(4)

🧪 Validation and Testing

Analytical Benchmarks

• Pure diffusion (σ = 0) vs. Fick's law
• Stress-free moisture uptake
• Simple tension with diffusion
• Complex loading scenarios

Experimental Validation

• Moisture uptake curves
• Stress-strain response
• Coupled behavior validation

📈 Results and Visualization

Output Variables

Variable	Description	Access
U1, U2, U3	Displacements	Standard ABAQUS output
NT	Concentration (as temperature)	Field output
SDV1-SDV6	Stress components	State variables
SDV7-SDV12	Strain components	State variables
SDV14	Hydrostatic stress	State variables

Post-Processing Example

# Python script for ODB processing
from abaqus import *
from abaqusConstants import *

odb = openOdb('Analysis.odb')
step = odb.steps['Loading']
frame = step.frames[-1]

# Extract concentration field
concentration = frame.fieldOutputs['NT']
# Extract stress components  
stress_xx = frame.fieldOutputs['SDV1']
hydrostatic = frame.fieldOutputs['SDV14']

🤝 Contributing

Contributions are welcome! Please feel free to:

1. 🐛 Report bugs via Issues
2. 💡 Suggest features or improvements
3. 🔧 Submit pull requests with enhancements
4. 📖 Improve documentation
5. 🧪 Add validation cases

Development Guidelines

• Follow Fortran 90+ standards
• Include test cases for new features
• Update documentation accordingly
• Maintain backward compatibility

📜 Citation

If you use this code in your research, please cite:

@software{bahtiri2025abaqus,
  title={ABAQUS Multiphysics Diffusion UEL: Coupled Stress-Diffusion Analysis},
  author={Bahtiri, Betim},
  year={2025},
  url={https://github.com/BBahtiri/ABAQUS-Multiphysics-Diffusion-UEL},
  note={User Element for coupled hydro-mechanical analysis in ABAQUS}
}

📄 License

This project is licensed under the MIT License - see the LICENSE file for details.

📞 Contact and Support

• GitHub: @BBahtiri
• Issues: GitHub Issues
• Discussions: GitHub Discussions

🔗 Related Work

• ABAQUS User Subroutines
• Multiphysics Finite Element Methods
• Moisture Diffusion in Polymers

⭐ Acknowledgments

• ABAQUS User Community for documentation and examples
• Research community in computational mechanics
• Open source contributors and users

---

Made with ❤️ for the computational mechanics community

Star ⭐ this repository if you find it useful!