ProductsAbaqus/StandardAbaqus/ExplicitAbaqus/CAE Mechanical behaviorThe model is a continuum, plasticitybased, damage model for concrete. It assumes that the main two failure mechanisms are tensile cracking and compressive crushing of the concrete material. The evolution of the yield (or failure) surface is controlled by two hardening variables, ${\stackrel{~}{\epsilon}}_{t}^{pl}$ and ${\stackrel{~}{\epsilon}}_{c}^{pl}$, linked to failure mechanisms under tension and compression loading, respectively. We refer to ${\stackrel{~}{\epsilon}}_{t}^{pl}$ and ${\stackrel{~}{\epsilon}}_{c}^{pl}$ as tensile and compressive equivalent plastic strains, respectively. The following sections discuss the main assumptions about the mechanical behavior of concrete. Uniaxial tension and compression stress behaviorThe model assumes that the uniaxial tensile and compressive response of concrete is characterized by damaged plasticity, as shown in Figure 1. Figure 1. Response of concrete to uniaxial loading in tension (a) and
compression (b).
Under uniaxial tension the stressstrain response follows a linear elastic relationship until the value of the failure stress, ${\sigma}_{t0}$, is reached. The failure stress corresponds to the onset of microcracking in the concrete material. Beyond the failure stress the formation of microcracks is represented macroscopically with a softening stressstrain response, which induces strain localization in the concrete structure. Under uniaxial compression the response is linear until the value of initial yield, ${\sigma}_{c0}$. In the plastic regime the response is typically characterized by stress hardening followed by strain softening beyond the ultimate stress, ${\sigma}_{cu}$. This representation, although somewhat simplified, captures the main features of the response of concrete. It is assumed that the uniaxial stressstrain curves can be converted into stress versus plasticstrain curves. (This conversion is performed automatically by Abaqus from the userprovided stress versus “inelastic” strain data, as explained below.) Thus, $$\begin{array}{cc}\hfill {\sigma}_{t}& ={\sigma}_{t}\left({\stackrel{~}{\epsilon}}_{t}^{pl},{\dot{\stackrel{~}{\epsilon}}}_{t}^{pl},\theta ,{f}_{i}\right),\hfill \\ \hfill {\sigma}_{c}& ={\sigma}_{c}\left({\stackrel{~}{\epsilon}}_{c}^{pl},{\dot{\stackrel{~}{\epsilon}}}_{c}^{pl},\theta ,{f}_{i}\right),\hfill \end{array}$$
where the subscripts t and c refer to tension and compression, respectively; ${\stackrel{~}{\epsilon}}_{t}^{pl}$ and ${\stackrel{~}{\epsilon}}_{c}^{pl}$ are the equivalent plastic strains, ${\dot{\stackrel{~}{\epsilon}}}_{t}^{pl}$ and ${\dot{\stackrel{~}{\epsilon}}}_{c}^{pl}$ are the equivalent plastic strain rates, $\theta $ is the temperature, and ${f}_{i},(i=1,2,\mathrm{\dots})$ are other predefined field variables. As shown in Figure 1, when the concrete specimen is unloaded from any point on the strain softening branch of the stressstrain curves, the unloading response is weakened: the elastic stiffness of the material appears to be damaged (or degraded). The degradation of the elastic stiffness is characterized by two damage variables, ${d}_{t}$ and ${d}_{c}$, which are assumed to be functions of the plastic strains, temperature, and field variables: $$\begin{array}{cc}\hfill {d}_{t}& ={d}_{t}({\stackrel{~}{\epsilon}}_{t}^{pl},\theta ,{f}_{i});\mathrm{\hspace{0.25em}\hspace{0.25em}\hspace{0.25em}0}\le {d}_{t}\le 1,\hfill \\ \hfill {d}_{c}& ={d}_{c}({\stackrel{~}{\epsilon}}_{c}^{pl},\theta ,{f}_{i});\mathrm{\hspace{0.25em}\hspace{0.25em}\hspace{0.25em}0}\le {d}_{c}\le 1.\hfill \end{array}$$
The damage variables can take values from zero, representing the undamaged material, to one, which represents total loss of strength. If ${E}_{0}$ is the initial (undamaged) elastic stiffness of the material, the stressstrain relations under uniaxial tension and compression loading are, respectively: $$\begin{array}{cc}\hfill {\sigma}_{t}& =\left(1{d}_{t}\right){E}_{0}\left({\epsilon}_{t}{\stackrel{~}{\epsilon}}_{t}^{pl}\right),\hfill \\ \hfill {\sigma}_{c}& =\left(1{d}_{c}\right){E}_{0}\left({\epsilon}_{c}{\stackrel{~}{\epsilon}}_{c}^{pl}\right).\hfill \end{array}$$
We define the “effective” tensile and compressive cohesion stresses as $$\begin{array}{cc}\hfill {\overline{\sigma}}_{t}& =\frac{{\sigma}_{t}}{\left(1{d}_{t}\right)}={E}_{0}({\epsilon}_{t}{\stackrel{~}{\epsilon}}_{t}^{pl}),\hfill \\ \hfill {\overline{\sigma}}_{c}& =\frac{{\sigma}_{c}}{\left(1{d}_{c}\right)}={E}_{0}({\epsilon}_{c}{\stackrel{~}{\epsilon}}_{c}^{pl}).\hfill \end{array}$$
The effective cohesion stresses determine the size of the yield (or failure) surface. Uniaxial cyclic behaviorUnder uniaxial cyclic loading conditions the degradation mechanisms are quite complex, involving the opening and closing of previously formed microcracks, as well as their interaction. Experimentally, it is observed that there is some recovery of the elastic stiffness as the load changes sign during a uniaxial cyclic test. The stiffness recovery effect, also known as the “unilateral effect,” is an important aspect of the concrete behavior under cyclic loading. The effect is usually more pronounced as the load changes from tension to compression, causing tensile cracks to close, which results in the recovery of the compressive stiffness. The concrete damaged plasticity model assumes that the reduction of the elastic modulus is given in terms of a scalar degradation variable d as $$E=\left(1d\right){E}_{0},$$
where ${E}_{0}$ is the initial (undamaged) modulus of the material. This expression holds both in the tensile (${\sigma}_{11}>0$) and the compressive (${\sigma}_{11}<0$) sides of the cycle. The stiffness degradation variable, d, is a function of the stress state and the uniaxial damage variables, ${d}_{t}$ and ${d}_{c}$. For the uniaxial cyclic conditions Abaqus assumes that $$\left(1d\right)=\left(1{s}_{t}{d}_{c}\right)\left(1{s}_{c}{d}_{t}\right),$$
where ${s}_{t}$ and ${s}_{c}$ are functions of the stress state that are introduced to model stiffness recovery effects associated with stress reversals. They are defined according to $$\begin{array}{cc}\hfill {s}_{t}& =1{w}_{t}{r}^{*}\left({\sigma}_{11}\right);\mathrm{\hspace{0.25em}\hspace{0.25em}\hspace{0.25em}0}\le {w}_{t}\le 1,\hfill \\ \hfill {s}_{c}& =1{w}_{c}(1{r}^{*}\left({\sigma}_{11}\right));\mathrm{\hspace{0.25em}\hspace{0.25em}\hspace{0.25em}\hspace{0.25em}0}\le {w}_{c}\le 1,\hfill \end{array}$$
where $${r}^{*}\left({\sigma}_{11}\right)=H\left({\sigma}_{11}\right)=\{\begin{array}{ccc}\hfill 1\hfill & \hfill \mathrm{if}\hfill & \hfill {\sigma}_{11}>0\hfill \\ \hfill 0\hfill & \hfill \mathrm{if}\hfill & \hfill {\sigma}_{11}<0\hfill \end{array}$$
The weight factors ${w}_{t}$ and ${w}_{c}$, which are assumed to be material properties, control the recovery of the tensile and compressive stiffness upon load reversal. To illustrate this, consider the example in Figure 2, where the load changes from tension to compression. Figure 2. Illustration of the effect of the compression stiffness recovery
parameter ${w}_{c}$.
Assume that there was no previous compressive damage (crushing) in the material; that is, ${\stackrel{~}{\epsilon}}_{c}^{pl}=0$ and ${d}_{c}=0$. Then $$\left(1d\right)=\left(1{s}_{c}{d}_{t}\right)=\left(1\left(1{w}_{c}\left(1{r}^{*}\right)\right){d}_{t}\right).$$
Multiaxial behaviorThe stressstrain relations for the general threedimensional multiaxial condition are given by the scalar damage elasticity equation: $$\mathit{\sigma}=\left(1d\right){\mathbf{D}}_{0}^{el}:\left(\mathit{\epsilon}{\mathit{\epsilon}}^{pl}\right),$$
where ${\mathbf{D}}_{0}^{el}$ is the initial (undamaged) elasticity matrix. The previous expression for the scalar stiffness degradation variable, d, is generalized to the multiaxial stress case by replacing the unit step function ${r}^{*}\left({\sigma}_{11}\right)$ with a multiaxial stress weight factor, $r\left(\widehat{\mathit{\sigma}}\right)$, defined as $$r\left(\widehat{\mathit{\sigma}}\right)=\frac{{\sum}_{i=1}^{3}\u27e8{\widehat{\sigma}}_{i}\u27e9}{{\sum}_{i=1}^{3}\left{\widehat{\sigma}}_{i}\right};\mathrm{\hspace{0.25em}\hspace{0.25em}\hspace{0.25em}0}\le r\left(\widehat{\mathit{\sigma}}\right)\le 1,$$
where ${\widehat{\sigma}}_{i}\mathit{}(i=1,2,3)$ are the principal stress components. The Macauley bracket $\u27e8\cdot \u27e9$ is defined by $\u27e8x\u27e9=\frac{1}{2}\left(\leftx\right+x\right)$. See Damaged plasticity model for concrete and other quasibrittle materials for further details of the constitutive model. ReinforcementIn Abaqus reinforcement in concrete structures is typically provided by means of rebars, which are onedimensional rods that can be defined singly or embedded in oriented surfaces. Rebars are typically used with metal plasticity models to describe the behavior of the rebar material and are superposed on a mesh of standard element types used to model the concrete. With this modeling approach, the concrete behavior is considered independently of the rebar. Effects associated with the rebar/concrete interface, such as bond slip and dowel action, are modeled approximately by introducing some “tension stiffening” into the concrete modeling to simulate load transfer across cracks through the rebar. Details regarding tension stiffening are provided below. Defining the rebar can be tedious in complex problems, but it is important that this be done accurately since it may cause an analysis to fail due to lack of reinforcement in key regions of a model. See Defining rebar as an element property for more information regarding rebars. Defining tension stiffeningThe postfailure behavior for direct straining is modeled with tension stiffening, which allows you to define the strainsoftening behavior for cracked concrete. This behavior also allows for the effects of the reinforcement interaction with concrete to be simulated in a simple manner. Tension stiffening is required in the concrete damaged plasticity model. You can specify tension stiffening by means of a postfailure stressstrain relation or by applying a fracture energy cracking criterion. Postfailure stressstrain relationIn reinforced concrete the specification of postfailure behavior generally means giving the postfailure stress as a function of cracking strain, ${\stackrel{~}{\epsilon}}_{t}^{ck}$. The cracking strain is defined as the total strain minus the elastic strain corresponding to the undamaged material; that is, ${\stackrel{~}{\epsilon}}_{t}^{ck}={\epsilon}_{t}{\epsilon}_{0t}^{el}$, where ${\epsilon}_{0t}^{el}={\sigma}_{t}/{E}_{0}$, as illustrated in Figure 3. To avoid potential numerical problems, Abaqus enforces a lower limit on the postfailure stress equal to onehundreth of the initial failure stress: ${\sigma}_{t}\ge {\sigma}_{t0}/100$. Figure 3. Illustration of the definition of the cracking strain
${\stackrel{~}{\epsilon}}_{t}^{ck}$
used for the definition of tension stiffening data.
Tension stiffening data are given in terms of the cracking strain, ${\stackrel{~}{\epsilon}}_{t}^{ck}$. When unloading data are available, the data are provided to Abaqus in terms of tensile damage curves, ${d}_{t}{\stackrel{~}{\epsilon}}_{t}^{ck}$, as discussed below. Abaqus automatically converts the cracking strain values to plastic strain values using the relationship $${\stackrel{~}{\epsilon}}_{t}^{pl}={\stackrel{~}{\epsilon}}_{t}^{ck}\frac{{d}_{t}}{\left(1{d}_{t}\right)}\frac{{\sigma}_{t}}{{E}_{0}}.$$
Abaqus will issue an error message if the calculated plastic strain values are negative and/or decreasing with increasing cracking strain, which typically indicates that the tensile damage curves are incorrect. In the absence of tensile damage ${\stackrel{~}{\epsilon}}_{t}^{pl}={\stackrel{~}{\epsilon}}_{t}^{ck}$. In cases with little or no reinforcement, the specification of a postfailure stressstrain relation introduces mesh sensitivity in the results, in the sense that the finite element predictions do not converge to a unique solution as the mesh is refined because mesh refinement leads to narrower crack bands. This problem typically occurs if cracking failure occurs only at localized regions in the structure and mesh refinement does not result in the formation of additional cracks. If cracking failure is distributed evenly (either due to the effect of rebar or due to the presence of stabilizing elastic material, as in the case of plate bending), mesh sensitivity is less of a concern. In practical calculations for reinforced concrete, the mesh is usually such that each element contains rebars. The interaction between the rebars and the concrete tends to reduce the mesh sensitivity, provided that a reasonable amount of tension stiffening is introduced in the concrete model to simulate this interaction. This requires an estimate of the tension stiffening effect, which depends on such factors as the density of reinforcement, the quality of the bond between the rebar and the concrete, the relative size of the concrete aggregate compared to the rebar diameter, and the mesh. A reasonable starting point for relatively heavily reinforced concrete modeled with a fairly detailed mesh is to assume that the strain softening after failure reduces the stress linearly to zero at a total strain of about 10 times the strain at failure. The strain at failure in standard concretes is typically 10^{−4}, which suggests that tension stiffening that reduces the stress to zero at a total strain of about 10^{−3} is reasonable. This parameter should be calibrated to a particular case. The choice of tension stiffening parameters is important since, generally, more tension stiffening makes it easier to obtain numerical solutions. Too little tension stiffening will cause the local cracking failure in the concrete to introduce temporarily unstable behavior in the overall response of the model. Few practical designs exhibit such behavior, so that the presence of this type of response in the analysis model usually indicates that the tension stiffening is unreasonably low. Input File Usage CONCRETE TENSION STIFFENING, TYPE=STRAIN (default) Abaqus/CAE Usage Property module: material editor: MechanicalPlasticityConcrete Damaged Plasticity: Tensile Behavior: Type: Strain Fracture energy cracking criterionWhen there is no reinforcement in significant regions of the model, the tension stiffening approach described above will introduce unreasonable mesh sensitivity into the results. However, it is generally accepted that Hillerborg's (1976) fracture energy proposal is adequate to allay the concern for many practical purposes. Hillerborg defines the energy required to open a unit area of crack, ${G}_{f}$, as a material parameter, using brittle fracture concepts. With this approach the concrete's brittle behavior is characterized by a stressdisplacement response rather than a stressstrain response. Under tension a concrete specimen will crack across some section. After it has been pulled apart sufficiently for most of the stress to be removed (so that the undamaged elastic strain is small), its length will be determined primarily by the opening at the crack. The opening does not depend on the specimen's length. This fracture energy cracking model can be invoked by specifying the postfailure stress as a tabular function of cracking displacement, as shown in Figure 4. Figure 4. Postfailure stressdisplacement curve.
Alternatively, the fracture energy, ${G}_{f}$, can be specified directly as a material property; in this case, define the failure stress, ${\sigma}_{t0}$, as a tabular function of the associated fracture energy. This model assumes a linear loss of strength after cracking, as shown in Figure 5. Figure 5. Postfailure stressfracture energy curve.
The cracking displacement at which complete loss of strength takes place is, therefore, ${u}_{t0}=2{G}_{f}/{\sigma}_{t0}$. Typical values of ${G}_{f}$ range from 40 N/m (0.22 lb/in) for a typical construction concrete (with a compressive strength of approximately 20 MPa, 2850 lb/in^{2}) to 120 N/m (0.67 lb/in) for a highstrength concrete (with a compressive strength of approximately 40 MPa, 5700 lb/in^{2}). If tensile damage, ${d}_{t}$, is specified, Abaqus automatically converts the cracking displacement values to “plastic” displacement values using the relationship $${u}_{t}^{pl}={u}_{t}^{ck}\frac{{d}_{t}}{\left(1{d}_{t}\right)}\frac{{\sigma}_{t}{l}_{0}}{{E}_{0}},$$
where the specimen length, ${l}_{0}$, is assumed to be one unit length, ${l}_{0}=1$ ImplementationThe implementation of this stressdisplacement concept in a finite element model requires the definition of a characteristic length associated with an integration point. The characteristic crack length is based on the element geometry and formulation: it is a typical length of a line across an element for a firstorder element; it is half of the same typical length for a secondorder element. For beams and trusses it is a characteristic length along the element axis. For membranes and shells it is a characteristic length in the reference surface. For axisymmetric elements it is a characteristic length in the r–z plane only. For cohesive elements it is equal to the constitutive thickness. This definition of the characteristic crack length is used because the direction in which cracking occurs is not known in advance. Therefore, elements with large aspect ratios will have rather different behavior depending on the direction in which they crack: some mesh sensitivity remains because of this effect, and elements that have aspect ratios close to one are recommended. Alternatively, this mesh dependency could be reduced by directly specifying the characteristic length as a function of the element topology and material orientation in user subroutine VUCHARLENGTH (see Defining the characteristic element length at a material point in Abaqus/Explicit). Input File Usage Use the following option to specify the postfailure stress as a tabular function of displacement: CONCRETE TENSION STIFFENING, TYPE=DISPLACEMENT Use the following option to specify the postfailure stress as a tabular function of the fracture energy: CONCRETE TENSION STIFFENING, TYPE=GFI Abaqus/CAE Usage Property module: material editor: MechanicalPlasticityConcrete Damaged Plasticity: Tensile Behavior: Type: Displacement or GFI Defining compressive behaviorYou can define the stressstrain behavior of plain concrete in uniaxial compression outside the elastic range. Compressive stress data are provided as a tabular function of inelastic (or crushing) strain, ${\stackrel{~}{\epsilon}}_{c}^{in}$, and, if desired, strain rate, temperature, and field variables. Positive (absolute) values should be given for the compressive stress and strain. The stressstrain curve can be defined beyond the ultimate stress, into the strainsoftening regime. Hardening data are given in terms of an inelastic strain, ${\stackrel{~}{\epsilon}}_{c}^{in}$, instead of plastic strain, ${\stackrel{~}{\epsilon}}_{c}^{pl}$. The compressive inelastic strain is defined as the total strain minus the elastic strain corresponding to the undamaged material, ${\stackrel{~}{\epsilon}}_{c}^{in}={\epsilon}_{c}{\epsilon}_{0c}^{el}$, where ${\epsilon}_{0c}^{el}={\sigma}_{c}/{E}_{0}$, as illustrated in Figure 6. Figure 6. Definition of the compressive inelastic (or crushing) strain
${\stackrel{~}{\epsilon}}_{c}^{in}$
used for the definition of compression hardening data.
Unloading data are provided to Abaqus in terms of compressive damage curves, ${d}_{c}{\stackrel{~}{\epsilon}}_{c}^{in}$, as discussed below. Abaqus automatically converts the inelastic strain values to plastic strain values using the relationship $${\stackrel{~}{\epsilon}}_{c}^{pl}={\stackrel{~}{\epsilon}}_{c}^{in}\frac{{d}_{c}}{\left(1{d}_{c}\right)}\frac{{\sigma}_{c}}{{E}_{0}}.$$
Abaqus will issue an error message if the calculated plastic strain values are negative and/or decreasing with increasing inelastic strain, which typically indicates that the compressive damage curves are incorrect. In the absence of compressive damage ${\stackrel{~}{\epsilon}}_{c}^{pl}={\stackrel{~}{\epsilon}}_{c}^{in}$. Input File Usage CONCRETE COMPRESSION HARDENING Abaqus/CAE Usage Property module: material editor: MechanicalPlasticityConcrete Damaged Plasticity: Compressive Behavior Defining damage and stiffness recoveryDamage, ${d}_{t}$ and/or ${d}_{c}$, can be specified in tabular form. (If damage is not specified, the model behaves as a plasticity model; consequently, ${\stackrel{~}{\epsilon}}_{t}^{pl}={\stackrel{~}{\epsilon}}_{t}^{ck}$ and ${\stackrel{~}{\epsilon}}_{c}^{pl}={\stackrel{~}{\epsilon}}_{c}^{in}$.) In Abaqus the damage variables are treated as nondecreasing material point quantities. At any increment during the analysis, the new value of each damage variable is obtained as the maximum between the value at the end of the previous increment and the value corresponding to the current state (interpolated from the userspecified tabular data); that is, $$\begin{array}{cc}\hfill {{d}_{t}}_{t+\mathrm{\Delta}t}& =max\left\{{{d}_{t}}_{t},{d}_{t}\left({{\stackrel{~}{\epsilon}}_{t}^{pl}}_{t+\mathrm{\Delta}t},{\theta }_{t+\mathrm{\Delta}t},{{f}_{i}}_{t+\mathrm{\Delta}t}\right)\right\},\hfill \\ \hfill {{d}_{c}}_{t+\mathrm{\Delta}t}& =max\left\{{{d}_{c}}_{t},{d}_{c}\left({{\stackrel{~}{\epsilon}}_{c}^{pl}}_{t+\mathrm{\Delta}t},{\theta }_{t+\mathrm{\Delta}t},{{f}_{i}}_{t+\mathrm{\Delta}t}\right)\right\}.\hfill \end{array}$$
The choice of the damage properties is important since, generally, excessive damage may have a critical effect on the rate of convergence. It is recommended to avoid using values of the damage variables above 0.99, which corresponds to a 99% reduction of the stiffness. It is strongly recommended that you specify the tabular definition of tensile and compressive damage variables for the same values of cracking and inelastic strains/displacements as those used in the tabular definitions of tension stiffening and compressive behavior, respectively. When the tensile stiffening response is defined directly in terms of failure stress and fracture energy (${G}_{f}$), the definition of the tension damage variable should be such that it increases linearly as a function of the cracking displacement. Tensile damageYou can define the uniaxial tension damage variable, ${d}_{t}$, as a tabular function of either cracking strain or cracking displacement. Input File Usage Use the following option to specify tensile damage as a function of cracking strain: CONCRETE TENSION DAMAGE, TYPE=STRAIN (default) Use the following option to specify tensile damage as a function of cracking displacement: CONCRETE TENSION DAMAGE, TYPE=DISPLACEMENT Abaqus/CAE Usage Property module: material editor: MechanicalPlasticityConcrete Damaged Plasticity: Tensile Behavior: SuboptionsTension Damage: Type: Strain or Displacement Compressive damageYou can define the uniaxial compression damage variable, ${d}_{c}$, as a tabular function of inelastic (crushing) strain. Input File Usage CONCRETE COMPRESSION DAMAGE Abaqus/CAE Usage Property module: material editor: MechanicalPlasticityConcrete Damaged Plasticity: Compressive Behavior: SuboptionsCompression Damage Stiffness recoveryAs discussed above, stiffness recovery is an important aspect of the mechanical response of concrete under cyclic loading. Abaqus allows direct user specification of the stiffness recovery factors ${w}_{t}$ and ${w}_{c}$. The experimental observation in most quasibrittle materials, including concrete, is that the compressive stiffness is recovered upon crack closure as the load changes from tension to compression. On the other hand, the tensile stiffness is not recovered as the load changes from compression to tension once crushing microcracks have developed. This behavior, which corresponds to ${w}_{t}=0$ and ${w}_{c}=1$, is the default used by Abaqus. Figure 7 illustrates a uniaxial load cycle assuming the default behavior. Figure 7. Uniaxial load cycle (tensioncompressiontension) assuming default
values for the stiffness recovery factors: ${w}_{t}=0$
and ${w}_{c}=1$.
Input File Usage Use the following option to specify the compression stiffness recovery factor, ${w}_{c}$: CONCRETE TENSION DAMAGE, COMPRESSION RECOVERY=${w}_{c}$ Use the following option to specify the tension stiffness recovery factor, ${w}_{t}$: CONCRETE COMPRESSION DAMAGE, TENSION RECOVERY=${w}_{t}$ Abaqus/CAE Usage Property module: material editor: MechanicalPlasticityConcrete Damaged Plasticity: Tensile Behavior: SuboptionsTension Damage: Compression recovery: ${w}_{c}$ Compressive Behavior: SuboptionsCompression Damage: Tension recovery: ${w}_{t}$ Rate dependenceThe ratesensitive behavior of quasibrittle materials is mainly connected to the retardation effects that high strain rates have on the growth of microcracks. The effect is usually more pronounced under tensile loading. As the strain rate increases, the stressstrain curves exhibit decreasing nonlinearity as well as an increase in the peak strength. You can specify tension stiffening as a tabular function of cracking strain (or displacement) rate, and you can specify compression hardening data as a tabular function of inelastic strain rate. Input File Usage Use the following options: CONCRETE TENSION STIFFENING CONCRETE COMPRESSION HARDENING Abaqus/CAE Usage Property module: material editor: MechanicalPlasticityConcrete Damaged Plasticity: Tensile Behavior: Use strainratedependent data Compressive Behavior: Use strainratedependent data Concrete plasticityYou can define flow potential, yield surface, and in Abaqus/Standard viscosity parameters for the concrete damaged plasticity material model. Input File Usage CONCRETE DAMAGED PLASTICITY Abaqus/CAE Usage Property module: material editor: MechanicalPlasticityConcrete Damaged Plasticity: Plasticity Effective stress invariantsThe effective stress is defined as $$\overline{\mathit{\sigma}}={\mathbf{D}}_{0}^{el}:\left(\mathit{\epsilon}{\mathit{\epsilon}}^{pl}\right).$$
The plastic flow potential function and the yield surface make use of two stress invariants of the effective stress tensor, namely the hydrostatic pressure stress, $$\overline{p}=\frac{1}{3}\mathrm{trace}\left(\overline{\mathit{\sigma}}\right),$$
and the Mises equivalent effective stress, $$\overline{q}=\sqrt{\frac{3}{2}(\overline{\mathbf{S}}:\overline{\mathbf{S}})},$$
where $\overline{\mathbf{S}}$ is the effective stress deviator, defined as $$\overline{\mathbf{S}}=\overline{\mathit{\sigma}}+\overline{p}\mathbf{I}.$$ Plastic flowThe concrete damaged plasticity model assumes nonassociated potential plastic flow. The flow potential G used for this model is the DruckerPrager hyperbolic function: $$G=\sqrt{{\left(\u03f5{\sigma}_{t0}\mathrm{tan}\psi \right)}^{2}+{\overline{q}}^{2}}\overline{p}\mathrm{tan}\psi ,$$
where
This flow potential, which is continuous and smooth, ensures that the flow direction is always uniquely defined. The function approaches the linear DruckerPrager flow potential asymptotically at high confining pressure stress and intersects the hydrostatic pressure axis at 90°. See Models for granular or polymer behavior for further discussion of this potential. The default flow potential eccentricity is $\u03f5=0.1$, which implies that the material has almost the same dilation angle over a wide range of confining pressure stress values. Increasing the value of $\u03f5$ provides more curvature to the flow potential, implying that the dilation angle increases more rapidly as the confining pressure decreases. Values of $\u03f5$ that are significantly less than the default value may lead to convergence problems if the material is subjected to low confining pressures because of the very tight curvature of the flow potential locally where it intersects the paxis. Yield functionThe model makes use of the yield function of Lubliner et. al. (1989), with the modifications proposed by Lee and Fenves (1998) to account for different evolution of strength under tension and compression. The evolution of the yield surface is controlled by the hardening variables, ${\stackrel{~}{\epsilon}}_{t}^{pl}$ and ${\stackrel{~}{\epsilon}}_{c}^{pl}$. In terms of effective stresses, the yield function takes the form $$F=\frac{1}{1\alpha}\left(\overline{q}3\alpha \overline{p}+\beta \left({\stackrel{~}{\mathit{\epsilon}}}^{pl}\right)\u27e8{\widehat{\overline{\sigma}}}_{\mathrm{max}}\u27e9\gamma \u27e8{\widehat{\overline{\sigma}}}_{\mathrm{max}}\u27e9\right){\overline{\sigma}}_{c}\left({\stackrel{~}{\epsilon}}_{c}^{pl}\right)=0,$$
with $$\begin{array}{cc}\hfill \alpha & =\frac{\left({\sigma}_{b0}/{\sigma}_{c0}\right)1}{2\left({\sigma}_{b0}/{\sigma}_{c0}\right)1};\mathrm{\hspace{0.25em}0}\le \alpha \le 0.5,\hfill \\ \hfill \beta & =\frac{{\overline{\sigma}}_{c}\left({\stackrel{~}{\epsilon}}_{c}^{pl}\right)}{{\overline{\sigma}}_{t}\left({\stackrel{~}{\epsilon}}_{t}^{pl}\right)}\left(1\alpha \right)\left(1+\alpha \right),\hfill \\ \hfill \gamma & =\frac{3\left(1{K}_{c}\right)}{2{K}_{c}1}.\hfill \end{array}$$
Here,
Figure 8. Yield surfaces in the deviatoric plane, corresponding to different
values of ${K}_{c}$.
Typical yield surfaces are shown in Figure 8 on the deviatoric plane and in Figure 9 for plane stress conditions. Figure 9. Yield surface in plane stress.
Nonassociated flowBecause plastic flow is nonassociated, the use of concrete damaged plasticity results in a nonsymmetric material stiffness matrix. Therefore, to obtain an acceptable rate of convergence in Abaqus/Standard, the unsymmetric matrix storage and solution scheme should be used. Abaqus/Standard will automatically activate the unsymmetric solution scheme if concrete damaged plasticity is used in the analysis. If desired, you can turn off the unsymmetric solution scheme for a particular step (see Defining an analysis). Viscoplastic regularizationMaterial models exhibiting softening behavior and stiffness degradation often lead to severe convergence difficulties in implicit analysis programs, such as Abaqus/Standard. A common technique to overcome some of these convergence difficulties is the use of a viscoplastic regularization of the constitutive equations, which causes the consistent tangent stiffness of the softening material to become positive for sufficiently small time increments. The concrete damaged plasticity model can be regularized in Abaqus/Standard using viscoplasticity by permitting stresses to be outside of the yield surface. We use a generalization of the DuvautLions regularization, according to which the viscoplastic strain rate tensor, ${\dot{\mathit{\epsilon}}}_{v}^{pl}$, is defined as $${\dot{\mathit{\epsilon}}}_{v}^{pl}=\frac{1}{\mu}\left({\mathit{\epsilon}}^{pl}{\mathit{\epsilon}}_{v}^{pl}\right).$$
Here $\mu $ is the viscosity parameter representing the relaxation time of the viscoplastic system, and ${\mathit{\epsilon}}^{pl}$ is the plastic strain evaluated in the inviscid backbone model. Similarly, a viscous stiffness degradation variable, ${d}_{v}$, for the viscoplastic system is defined as $${\dot{d}}_{v}=\frac{1}{\mu}\left(d{d}_{v}\right),$$
where d is the degradation variable evaluated in the inviscid backbone model. The stressstrain relation of the viscoplastic model is given as $$\mathit{\sigma}=\left(1{d}_{v}\right){\mathbf{D}}_{0}^{el}:\left(\mathit{\epsilon}{\mathit{\epsilon}}_{v}^{pl}\right).$$
Using the viscoplastic regularization with a small value for the viscosity parameter (small compared to the characteristic time increment) usually helps improve the rate of convergence of the model in the softening regime, without compromising results. The basic idea is that the solution of the viscoplastic system relaxes to that of the inviscid case as $t/\mu \to \mathrm{\infty}$, where t represents time. You can specify the value of the viscosity parameter as part of the concrete damaged plasticity material behavior definition. If the viscosity parameter is different from zero, output results of the plastic strain and stiffness degradation refer to the viscoplastic values, ${\mathit{\epsilon}}_{v}^{pl}$ and ${d}_{v}$. In Abaqus/Standard the default value of the viscosity parameter is zero, so that no viscoplastic regularization is performed. Material dampingThe concrete damaged plasticity model can be used in combination with material damping (see Material damping). If stiffness proportional damping is specified, Abaqus calculates the damping stress based on the undamaged elastic stiffness. This may introduce large artificial damping forces on elements undergoing severe damage at high strain rates. Visualization of “crack directions”Unlike concrete models based on the smeared crack approach, the concrete damaged plasticity model does not have the notion of cracks developing at the material integration point. However, it is possible to introduce the concept of an effective crack direction with the purpose of obtaining a graphical visualization of the cracking patterns in the concrete structure. Different criteria can be adopted within the framework of scalardamage plasticity for the definition of the direction of cracking. Following Lubliner et. al. (1989), we can assume that cracking initiates at points where the tensile equivalent plastic strain is greater than zero, ${\stackrel{~}{\epsilon}}_{t}^{pl}>0$, and the maximum principal plastic strain is positive. The direction of the vector normal to the crack plane is assumed to be parallel to the direction of the maximum principal plastic strain. This direction can be viewed in the Visualization module of Abaqus/CAE. Abaqus/CAE Usage Visualization module: ResultField Output: PE, Max. Principal PlotSymbols ElementsAbaqus offers a variety of elements for use with the concrete damaged plasticity model: truss, shell, plane stress, plane strain, generalized plane strain, axisymmetric, and threedimensional elements. Most beam elements can be used; however, beam elements in space that include shear stress caused by torsion and do not include hoop stress (such as B31, B31H, B32, B32H, B33, and B33H) cannot be used. Thinwalled, opensection beam elements and PIPE elements can be used with the concrete damaged plasticity model in Abaqus/Standard. For general shell analysis more than the default number of five integration points through the thickness of the shell should be used; nine thickness integration points are commonly used to model progressive failure of the concrete through the thickness with acceptable accuracy. OutputIn addition to the standard output identifiers available in Abaqus (Abaqus/Standard output variable identifiers and Abaqus/Explicit output variable identifiers), the following variables relate specifically to material points in the concrete damaged plasticity model:
References
