A set of user material constants are provided in the input file that can be modified to control certain features of the analysis. The user material constants are added to the input file during the export from Advanced Material Exchange.
Note: Autodesk strongly recommends that you do not modify the user material constants. Please consult Autodesk support before changing any of the user material constants.
Abaqus/Standard
When you export an Abaqus/Standard input file from
Advanced Material Exchange, a user material definition is created in the input file. The user material definition will take the following form:
*MATERIAL, NAME=Material_Name
*DEPVAR
11
*USER MATERIAL, CONSTANTS=4
n, sigma_0, sigma_max, degradation_paramater
The
Material_Name
parameter is the name of your material. This name will be set automatically to match the name of the material stored in the structural interface file (*.sif). You should not modify the material name.
The *DEPVAR keyword and associated data line define the number of solution dependent state variables to be tracked. All Advanced Material Exchange analyses should use the default value of 11 solution dependent state variables.
The four user material constants are defined as follows:
- n
- The Ramberg-Osgood n parameter. Refer to the Theory Manual for more information on the n parameter.
- sigma_0
- The Ramberg-Osgood sigma_0 parameter (σ0). Refer to the Theory Manual for more information on σ0.
- sigma_max
- The maximum effective stress for the von Mises failure criterion. The maximum effective stress is used to determine when matrix rupture occurs. Refer to The Rupture Model section of the Theory Manual for a complete description. If you are experiencing convergence issues in your analysis, you may choose to increase the maximum effective stress to a large value so that rupture will never occur. This can be useful for large models that experience a dramatic and widespread failure cascade. Consult Autodesk support before adjusting the maximum effective stress.
- degradation_parameter
- The degradation parameter represents the ratio of the degraded material stiffnesses to that of the original material stiffnesses. Once matrix rupture is predicted, the stiffness of the composite material is instantaneously reduced to a fraction of the original elastic stiffness of the composite. This percentage is determined by the degradation parameter. This stiffness reduction is applied to the stiffness matrix [C]. Once rupture is triggered, the stiffness of the composite material remains fixed at the reduced value for the duration of the analysis.
- The degradation parameter can have a large influence on a progressive failure solution. Consult Autodesk support before adjusting the degradation parameter.
If n, sigma_0, or sigma_max are omitted (zero) in the user material definition, the values stored in the structural interface file (*.sif) will be used. The degradation_parameter value is not stored in the *.sif file. If this value is omitted in the input file, a default value of 1.0E-06 will be applied.
Abaqus/Explicit
The user material constants for Abaqus/Explicit are the same as for Abaqus/Standard with one exception: the degradation parameter is not used in Abaqus/Explicit simulations. For an Abaqus/Explicit model, the user material definition would appear as follows:
*MATERIAL, NAME=Material_Name
*DEPVAR
11
*USER MATERIAL, CONSTANTS=3
n, sigma_0, sigma_max