Back to Online Manuals

10296x

000076

Dipl.-Ing. Frank Faulstich

2023-12-14

Select Manual

Overview

Graphical User Interface and Settings

Dlubal Center

Model Base Data

Structure

Imperfections

Load Cases and Combinations

Load Wizards

Loads

Result Objects

Costs and Emissions

Calculation

Results

Guide Objects

Digital Twins

Program Functions

Result Evaluation

Printout Reports

Drawing Sheets

Nonlinear Material Behavior

Material models

If the analysis add-on Nonlinear material behavior is activated in the Model base data (license required), further options are available for selection in the list of material models in addition to the Isotropic | Linear elastic and Orthotropic | Linear elastic material models.

Material Models for Nonlinear Material Behavior Add-on

Calculation method

When using a nonlinear material model, an iterative calculation is always performed. Depending on the material model, a different relation between stresses and strains is defined.

The stiffness of the finite elements is adjusted repeatedly during the iterations until the stress-strain relation is fulfilled. The adjustment is always applied to an entire surface or solid element. Therefore, the smoothing type Constant in mesh elements should always be used for the stress analysis.

Result Smoothing

Some material models in RFEM are labeled 'plastic', others 'nonlinear elastic'. If a component with a nonlinear elastic material is unloaded again, the strain returns along the same path. After complete load relief, no strain remains.

Stress-Strain Diagram for Nonlinear Elastic

When unloading a component with a plastic material model, a strain remains after complete unloading.

Stress-Strain Diagram for Plastic

Loading and unloading can be simulated with the add-on Construction stages analysis.

Background information on the nonlinear material models can be found in the technical article Yield laws in the isotropic nonlinear elastic material model.

The internal forces in slabs with nonlinear materials result from the numerical integration of the stresses over the plate thickness. To define the integration method for the thickness, check the option Specify integration method in the 'Edit Thickness' dialog. This provides the following integration methods for selection:

Gauss-Lobatto quadrature
Simpson's rule
trapezoidal rule

Defining Integration Method for Surface Thickness

Furthermore, you can define the 'number of integration points' over the plate thickness from 3 to 99.

Tip

Theoretical background on the individual integration methods can be found in the manual Multilayer Surfaces.

Isotropic plastic (members)

If you select the entry Isotropic | Plastic (members) in the 'Material model' drop-down list, the tab for entering the nonlinear material parameters becomes active.

Activating Nonlinear Material Model

Defining Nonlinear Material Parameters

In this tab, you define the stress-strain diagram. The following options are available for selection:

Standard
Bilinear
Diagram

If Standard is selected, RFEM uses a bilinear material model. For the modulus of elasticity E and the yield strength f_y, the values from the material library are used. For numerical reasons, the branch is not exactly horizontal but has a small slope E_p.

If you want to change the values for the yield strength and the modulus of elasticity, activate the User-defined material check box in the 'Basic' tab.

Activating User-Defined Material

With the bilinear definition, you can also enter the value for E_p.

You can define more complex relations between stress and strain using a stress-strain diagram. If you select this option, the 'Stress-Strain Diagram' tab is displayed.

Entering a user-defined stress-strain diagram

Entering User-Defined Stress-Strain Diagram

Define a point of the stress-strain relation in each row. How the diagram should continue after the last definition point can be selected in the 'Diagram end' list below the diagram:

Distribution after the last definition point

Distribution After Last Definition Point

With 'Failure', the stress jumps back to zero after the last definition point (for example, when the material tears). 'Yielding' means that the stress remains constant with increasing strain. 'Continuous' means that the curve continues with the slope of the last segment.

Info

In this material model, the stress-strain diagram refers to the longitudinal stress σ_x. Different yield strengths for tension and compression cannot be taken into account with this material model.

Isotropic plastic (surfaces/solids)

If you select the entry Isotropic | Plastic (surfaces/solids) in the 'Material model' drop-down list, the tab for entering the nonlinear material parameters becomes active.

Selecting Plastic Material Model

First, select the 'stress failure hypothesis'. The following hypotheses are available for selection:

von Mises (distortion energy hypothesis)
Tresca (shear stress hypothesis)
Drucker-Prager
Mohr-Coulomb

Defining Stress Failure Hypothesis

If you select von Mises, the following stresses are used in the stress-strain diagram:

Surfaces

σ_{v} = \sqrt{σ_{x}^{2} + σ_{y}^{2} - σ_{x} σ_{y} + 3 (τ_{xy}^{2})}

Equivalent Stress from Basic Stresses According to von Mises

Solids

σ_{v, Mises} = \sqrt{σ_{x}^{2} + σ_{y}^{2} + σ_{z}^{2} - σ_{x} σ_{y} - σ_{x} σ_{z} - σ_{y} σ_{z} + 3 (τ_{xy}^{2} + τ_{xz}^{2} + τ_{yz}^{2})}

Equivalent Stress σ_v,Mises from Basic Stresses

σ_{v, Mises} = \sqrt{\frac{1}{2} [(σ_{1} - σ_{2})^{2} + (σ_{1} - σ_{3})^{2} + (σ_{2} - σ_{3})^{2}]}

Equivalent Stress σ_v,Mises from Principal Stresses

According to the Tresca hypothesis, these stresses are used:

Surfaces

σ_{v} = \sqrt{{(σ_{x} - σ_{y})}^{2} + 4 {τ_{xy}}^{2}}

Equivalent Stress According to Tresca

Solids

σ_{v, Tresca} = max (|σ_{1} - σ_{2}|; |σ_{2} - σ_{3}|; |σ_{3} - σ_{1}|)

Equivalent Stress σ_v,Tresca

According to the Drucker-Prager hypothesis, this stress is used for surfaces and solids:

σ_{v} = \frac{m - 1}{2} (σ_{1} + σ_{2} + σ_{3}) + \frac{m + 1}{2} \sqrt{\frac{1}{2} [{(σ_{1} - σ_{2})}^{2} + {(σ_{2} - σ_{3})}^{2} + {(σ_{3} - σ_{1})}^{2}]}

m = \frac{σ_{c}}{σ_{t}}

σ_c	Limit stress for compression
σ_t	Limit stress for tension

Yield Criterion According to Drucker-Prager

According to the Mohr-Coulomb hypothesis, the following stress is used for surfaces and solids:

σ_{v} = \frac{m + 1}{2} \max \{|σ_{1} - σ_{2}| + K (σ_{1} + σ_{2}), |σ_{2} - σ_{3}| + K (σ_{2} + σ_{3}), |σ_{3} - σ_{1}| + K (σ_{3} + σ_{1})\}

K = \frac{m - 1}{m + 1}

m = \frac{σ_{c}}{σ_{t}}

Mohr – Coulomb

Isotropic nonlinear elastic (members)

The functionality largely corresponds to that of the Isotropic plastic (members) material model. However, unlike this model, no plastic strain remains after unloading.

Isotropic nonlinear elastic (surfaces/solids)

The functionality largely corresponds to that of the Isotropic plastic (surfaces/solids) material model. However, unlike this model, no plastic strain remains after unloading.

Isotropic damage (surfaces/solids)

Unlike other material models, the stress-strain diagram for this material model is not antimetric to the origin. Thus, for example, the behavior of steel fiber reinforced concrete can be modeled with this material model. Detailed information on modeling steel fiber reinforced concrete can be found in the technical article Material properties of steel fiber reinforced concrete.

Material Model "Isotropic | Damage"

The isotropic stiffness is reduced by a scalar damage parameter. This damage parameter is determined from the stress curve defined in the diagram. The direction of the principal stresses is not taken into account; rather, the damage occurs in the direction of the equivalent strain, which also covers the third direction perpendicular to the plane. The tension and compression zones of the stress tensor are treated separately. Different damage parameters apply in each case.

The 'reference element size' controls how the strain in the crack area is scaled to the length of the element. With the default value of zero, no scaling takes place. This realistically represents the material behavior of steel fiber reinforced concrete.

Tip

Theoretical background on the 'Isotropic damage' material model can be found in the technical article Nonlinear damage material model.

Orthotropic plastic (surfaces) / Orthotropic plastic (solids)

The material model according to Tsai-Wu combines plastic and orthotropic properties. This allows special modeling of materials with anisotropic characteristics such as fiber-reinforced plastics or timber.

When the material yields, the stresses remain constant. A redistribution takes place depending on the stiffnesses present in the individual directions.

Material Model "Orthotropic | Plastic (Surfaces)"

Material Model "Orthotropic | Plastic (Solid)"

The elastic range corresponds to the Orthotropic linear elastic (solids) material model. The following yield condition according to Tsai-Wu applies for the plastic range:

Surfaces

σ_{x} [\frac{1}{f_{t, x}} - \frac{1}{f_{c, x}}] + \frac{{σ_{x}}^{2}}{f_{t, x} f_{c, x}} +

σ_{y} [\frac{1}{f_{t, y}} - \frac{1}{f_{c, y}}] + \frac{{σ_{y}}^{2}}{f_{t, y} f_{c, y}} +

\frac{{τ_{xy}}^{2}}{{f_{v, xy}}^{2}} - {[\frac{1}{f_{t, x}} + \frac{1}{f_{c, x}}]}^{2} \frac{E_{x} E_{p, x}}{E_{x} - E_{p, x}} α \leq 1

α = \sum_{i} ∆ γ_{i}

Tsai-Wu, State of Plane Stress

Solids

σ_{x} [\frac{1}{f_{t, x}} - \frac{1}{f_{c, x}}] + \frac{{σ_{x}}^{2}}{f_{t, x} f_{c, x}} +

σ_{y} [\frac{1}{f_{t, y}} - \frac{1}{f_{c, y}}] + \frac{{σ_{y}}^{2}}{f_{t, y} f_{c, y}} +

σ_{z} [\frac{1}{f_{t, z}} - \frac{1}{f_{c, z}}] + \frac{{σ_{z}}^{2}}{f_{t, z} f_{c, z}} +

\frac{{τ_{yz}}^{2}}{{f_{v, yz}}^{2}} + \frac{{τ_{xz}}^{2}}{{f_{v, xz}}^{2}} + \frac{{τ_{xy}}^{2}}{{f_{v, xy}}^{2}} -

{[\frac{1}{f_{t, x}} + \frac{1}{f_{c, x}}]}^{2} \frac{E_{x} E_{p, x}}{E_{x} - E_{p, x}} α \leq 1

α = \sum_{i} ∆ γ_{i}

Tsai-Wu, Spatial State of Stress

All strengths must be defined as positive.

The yield condition can be imagined as an elliptical surface in the six-dimensional stress space. If one of the three stress components is set as a constant value, the surface can be projected onto a three-dimensional stress space.

If the value for f_y(σ) according to equation Tsai-Wu, state of plane stress is less than 1, the stresses are in the elastic range. The plastic range is reached as soon as f_y(σ) = 1. Values greater than 1 are not allowed. The model behaves in an ideally plastic manner, that is, no stiffening takes place.

Orthotropic plastic weld (surfaces)

This material model is used for analyses with the add-on Steel joints in order to represent the behavior of welds in accordance with the standards. In the equivalent surface, only stresses occur that correspond to the stress components σ_⊥, τ_⊥, and τ_|| of the weld. In the other stress directions, the stiffness of the equivalent surface approaches zero.

Material Model "Orthotropic | Plastic | Weld (Surfaces)"

In the 'Orthotropic | Plastic | Weld (Surfaces)' tab, you can define the parameters for taking into account the plastic material hardening of welds, for example the limit values f_ekv and f_x for the stress analysis according to the "directional method" according to EN 1993-1-8 [1] for welds, modified by a plastic component (see also the technical article Design of fillet welds).

Concrete

For the 'Concrete' material type, the nonlinear material models Anisotropic | Damage and Isotropic | Damage (surfaces/solids) are available for selection.

Material Models for Concrete

These material models are described in the chapter Anisotropic | Damage of the Concrete manual or above in the section Isotropic Damage.

Masonry

If the design add-on Masonry Design is activated in the Model base data (license required), the nonlinear material models Isotropic | Masonry | Plastic (surfaces) and Orthotropic | Masonry | Plastic (surfaces) are available for the 'Masonry' material type.

Material Models for Masonry

Both material models are described in the chapter Materials of the Masonry manual.

Fabric

For the 'Fabric' material type, the nonlinear material model Orthotropic | Fabric | Nonlinear elastic (surfaces) is available in addition to the orthotropic linear material model.

Material Models for Fabric

This material model allows for a realistic representation of the orthotropic behavior of prestressed fabric membranes in which the stiffnesses in warp and weft are different. It describes the fabric using a representative volume element (RVE) of its microstructure. By taking the fabric geometry into account, the model captures the associated transverse strain effect for all force states in the membrane. The load-dependent stiffness development of the fabric is also taken into account, which is essential for the accurate analysis of membrane structures.

The description is in progress.

References