Concrete
The Concrete subnode includes three different material models for modeling concrete and other quasibrittle materials with similar properties:
•
Coupled Damage–Plasticity
•
Mazars Damage
•
Perfect Plasticity
These material models can be used together with Linear Elastic Material and Nonlinear Elastic Material. It is available with the Geomechanics Module. Concrete is available for 3D, 2D, and 2D axisymmetry.
Concrete Model
Use this section to define properties of the concrete material.
Select a Material model — Coupled damage–plasticity, Mazars damage, or Perfect plasticity, then follow the instructions below.
Coupled Damage–Plasticity
The Coupled damage–plasticity material model combines damage mechanics with a plasticity model to describe important characteristics of the mechanical response and failure of concrete subjected to multiaxial and cyclic loading conditions.
See also:
•
Coupled Damage–Plasticity in the Structural Mechanics Theory chapter.
•
Modeling Damage in the Structural Mechanics Modeling chapter.
Enter the uniaxial Tensile strength σts, and Compressive strength σcs. These parameters are by default taken From material. When User defined, enter other values or expressions.
The Biaxial compressive strength σbc is defined as σbc = 1.16σcs when set to From default suggestion. Other values can be used if set to From Material or User defined.
The Compressive yield stress σcy controls when plastic deformation starts. It is defined σcy = 0.3σcs when set to From default suggestion. Other values can be used if set to From Material or User defined.
Tension softening
The settings in the Tension softening section controls the post-peak response of the model when loaded in tension. Select the type of softening function — Linear, Bilinear, Cornelissen, Exponential, User–defined strain, User–defined displacement, or None. Selecting None disables the tensile damage model. The Bilinear curve is used by default.
When Linear, Bilinear, Cornelissen, or Exponential is selected, specify how to set the Tensile fracture energy Gft— From material, From strain limit, From displacement limit, or User defined. If necessary, also enter a value for the Characteristic length lct.
Using the Cornelissen, Exponential, or a User defined softening function requires solving an extra nonlinear equation to determine the tensile damage variable.
Compression Softening
The settings in the Compression softening section controls the post-peak response of the model when loaded in compression. Select the type of softening function — Linear, Bilinear, Exponential, User–defined strain, User–defined displacement, or None. Selecting None disables the tensile damage model. The Linear curve is used by default.
When Linear, Bilinear, or Exponential is selected, specify how to set the Compressive fracture energy Gfc— From material, From strain limit, From displacement limit, or User defined. By default From strain limit is used with a value equal to 1e-4. If necessary, also enter a value for the Characteristic length lcc.
Enter a value for the Ductility parameter As. The parameter affects the softening response under multiaxial stress states. The default is 10.
Using the Exponential, or a User defined softening function requires solving an extra nonlinear equation to determine the compressive damage variable.
Spatial Regularization Method
Select a spatial regularization method for the tensile damage model — Crack band or None. By default the Crack band method is used for the tensile response.
Select a spatial regularization method for the compressive damage model — Crack band or None. By default the no regularization is used in compression.
If the Crack band method is used in either tension or compression, specify the Crack band calculation — Element volume/area or Element size. The Element volume/area setting computes a representative crack band based on the mesh element type, whereas the Element size always picks the longest edge of the mesh element. See Spatial Regularization for details.
Mazars Damage
The Mazars damage model defines a strain–based scalar damage model that is a computationally lean alternative for modeling the failure of concrete during monotonic loading.
Select the type of Equivalent strain — Mazars, Modified Mazars, or User defined. See Mazars Damage for Concrete for details.
Enter the Shear exponent β, the default is set to 1.06.
Select the Tensile damage evolution — Linear, Exponential, Polynomial, Multilinear, Mazars function, or User defined.
•
For Linear, Exponential, Polynomial, and Multilinear, enter the Tensile strength σts, the default is to take the value From material. Also specify how to define the Tensile fracture energy Gft — From material, From strain limit, From displacement limit, or User defined. The default is to take the value From material.If necessary, also enter a value for the Characteristic length lct. For the Multilinear option, also enter a value for the Shape factor λ, the default is set to 0.5.
•
For Mazars function, enter the Tensile strain threshold ε0t, and the Tensile damage parameters At and Bt.
•
For User defined, enter an expression for the Tensile damage evolution function dt(κ).
Select the Compressive damage evolution — Mazars function or User defined.
•
For Mazars function, enter the Compressive strain threshold ε0c, and the Compressive damage evolution parameters Ac and Bc.
•
For User defined, enter an expression for the Compressive damage evolution function dc(κ).
Select the type of Spatial regularization method — None, Crack band, or Implicit gradient. See Spatial Regularization for details.
•
For the Crack band method select the type of Crack band calculation — Element volume/area or Element size.
•
For the Implicit gradient method enter the Length scale lint. If the Fracture energy per area was selected as Strain softening input, enter also the Characteristic size of the damage dissipation zone hdmg. The Implicit gradient method is available in the Solid Mechanics and Layered Shell interfaces.
Select the type of Viscous regularization method — None or Delayed Damage.
For the Delayed damage method, enter the Characteristic time τ. The Delayed damage method is intended for time-dependent studies, and adds no contributions for other study types. See Viscous Regularization for details.
Perfect Plasticity
The Perfect plasticity material model defines a yield surface suitable to capture the failure of concrete under multiaxial loading conditions. As the name implies, no hardening is included and the purpose of the model is thus mainly to identify if the strength of the material is reached.
Select a Yield function— Bresler–Pister, Willam–Warnke, or Ottosen. The default values for the material parameters are taken From material. For User defined choices, enter other values or expressions.
When Bresler–Pister or Willam–Warnke is selected, enter the Tensile strength σts, Compressive strength σcs, and Biaxial compressive strength σbc.
When Ottosen is selected enter he Compressive strength σcs, Ottosen parameters a and b, Size factor k1, and Shape factor k2.
The failure criteria are described in the theory section:
•
The Bresler–Pister Yield Criterion
•
The Willam–Warnke Criterion
•
The Ottosen Criterion.
Tension Cutoff
This section is available for the Perfect plasticity material model. If required, select either None or Principal stress cutoff.
When Principal stress cutoff is selected from the list, enter a value or expression for the Maximum tensile stress σt. Use this to constrain the concrete model with an extra yield surface, which limits the maximum principal tensile stress.
See also Tension Cutoff in the Structural Mechanics Theory chapter.
Advanced Parameters
This section is available for the Coupled damage–plasticity and Mazars damage material models.
For both material models, enter the Maximum damage. This settings controls the residual stiffness of the material when fully damaged kept for numerical stability. The default is 1-1e-5.
When the Coupled damage–plasticity model is selected, this section allows you to enter values for several advanced model parameters modify the behavior of the model. In the majority of cases the default values results in a good prediction.
•
The Dilatancy parameter Df controls the amount of volumetric plastic deformation during compressive loading. It can be considered as the ratio of the absolute values of lateral and axial plastic strains during uniaxial compression. The default value is 0.85.
•
The Hardening modulus Hp controls the evolution of the yield surface during plastic flow. Its value must be set between 0 and σcy / σcs. The default value is 0.05.
•
The Hardening ductility parameter Ah, Bh, Ch, and Dh controls the evolution of the scalar hardening variable and can be used to adjust the ductility of the yield surface for different loadings. The default values are 0.08, 0.003, 2, and 1e-6.
To display this section, click the Show More Options button () and select Advanced Physics Options in the Show More Options dialog box
Advanced Settings
Select the Local method to solve the plasticity problem — Automatic or Backward Euler. When Backward Euler is selected, it is possible to specify the maximum number of iterations and the relative tolerance used to solve the local plasticity equations. Enter the following settings:
•
Maximum number of local iterations. To determine the maximum number of iteration in the Newton loop when solving the local plasticity equations. The default value is 25 iterations.
•
Relative tolerance. To check the convergence of the local plasticity equations based on the step size in the Newton loop. The final tolerance is computed based on the current solution of the local variable and the entered value. The default value is 1e-6.
To display this section, click the Show More Options button () and select Advanced Physics Options in the Show More Options dialog box.
See also Numerical Solution of the Elastoplastic Conditions in the Structural Mechanics Theory chapter.
Location in User Interface
Context Menus
Solid Mechanics>Linear Elastic Material>Concrete
Solid Mechanics>Nonlinear Elastic Material>Concrete
Ribbon
Physics tab with Linear Elastic Material or Nonlinear Elastic Material node selected in the model tree:
Attributes>Concrete