TMM4175 Polymer Composites

Home About Python Links Table of Contents

Material models for composites¶

Thermo-elastic behaviour¶

The most relevant material models and/or material definitions for thermo-elastic behaviour available in Abaqus are:

Density: For any simulations that involves dynamics or body forces such as gravity, the density must be supplied.

Elastic - Linear elastic - Isotropic: Defined by the Young's modulus $E$ and the Poisson's ratio $\nu$.

Elastic - Linear elastic - Engineering Constants: Defined by the nine engineering constants for an orthotropic material, $E_1, E_2, E_3, \nu_{12}, \nu_{13}, \nu_{23}, G_{12}, G_{13}, G_{23}$

Elastic - Linear elastic - Lamina: Typically used for shells and layered shells. Includes the four engineering constants for plane stress, $E_1, E_2, \nu_{12}, G_{12}$, and additionally the shear moduli $G_{12}$ and $G_{13}$.

Elastic - Linear elastic - Orthotropic: Defined by the stiffness matrix components, as an alternative to using the Engineering Constants.

Expansion - Isotropic: The coefficient of linear thermal expansion $\alpha$.

Expansion - Orthotropic: The 3 coefficient of linear thermal expansion, $\alpha_1, \alpha_2, \alpha_3$.

Other material behaviors¶

Other models for material behaviors will be introduced for particular applications. These includes plasticity (relevant for matrix and adhesive layers) as well as failure and damage models for composites.

`Abaqus Python tips & tricks`¶

Abaqus Python script for importing UD materials from the course into Abacus CAE model database.

from abaqusConstants import *
import json
    
def materialProperties(model,m):
    matname=str(m['name'])
    model.Material(name=matname)
    model.materials[matname].Density(table=((2e-09, ), ))
    model.materials[matname].Elastic(type=ENGINEERING_CONSTANTS, 
        table=((m['E1'], m['E2'], m['E3'], m['v12'], m['v13'], m['v23'],
                m['G12'], m['G13'], m['G23']), ))
    model.materials[matname].elastic.FailStress(table=((
        m['XT'], m['XC'], m['YT'], m['YC'], m['S12'], m['f12'], 0.0), ))
    model.materials[matname].Expansion(type=ORTHOTROPIC, 
        table=((m['a1'], m['a2'], m['a3']), ))

def importMaterials(filename):    
    with open(filename, "r") as file:
        imported_materials = json.load(file)
    modelName = session.sessionState['Viewport: 1']['modelName']
    modelName = getInput('Model',modelName)
    model = mdb.models[modelName]
    for m in imported_materials:
        materialProperties(model,m)
        
importMaterials(filename='TMM4175Matlib.txt')

References and further readings¶

SIMULIA User Assistance 2017 - Abaqus - Materials - Density
SIMULIA User Assistance 2017 - Abaqus - Materials - Elastic Mechanical Properties - Elastic behavior - Linear elasticity - Linear elastic behavior
SIMULIA User Assistance 2017 - Abaqus - Materials - Elastic Mechanical Properties - Elastic behavior - Linear elasticity - Plane stress orthotropic failure measures
SIMULIA User Assistance 2017 - Abaqus - Scripting