Back to Online Manuals

5271x

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

Calculation

Results

Guide Objects

Program Functions

Result Evaluation

Printout Reports

Nonlinear Material Behavior

If activating the Nonlinear Material Behavior analysis add-on (requires a license) in the Model – Base Data, there are further options for selection in the list of material models in addition to the "Isotropic | Linear Elastic" and "Orthotropic | Linear Elastic" material models.

Material Models for Analysis Add-on "Nonlinear Material Behavior"

If you use nonlinear material models in RFEM, an iterative calculation is always performed. Depending on the material model, a different relation between the stresses and strains is defined.

The stiffness of the finite elements is adjusted again and again in the course of the iterations until the stress-strain relation is met. The adjustment is always carried out for an entire surface or solid element. Therefore, we recommend always using the Constant on mesh elements smoothing type when evaluating stresses.

Result Smoothing

Some material models in RFEM are indicated by "Plastic", others by "Nonlinear Elastic".

If a structural component with a nonlinear elastic material is released again, the strain goes back on the same path. When completely unloaded, there is no strain left.

Stress-Strain Diagram for Nonlinear Elastic

When unloading a structural component with a plastic material model, the strain remains after it has been completely unloaded.

Stress-Strain Diagram for Plastic

Loading and unloading can be simulated using the Construction Stages Analysis add-on.

Background information about nonlinear material models can be found in the technical article describing the yield laws in isotropic nonlinear elastic material model.

The internal forces and moments in plates with nonlinear material result from the numerical integration of the stresses over the thickness d of the plate. To define the integration method for the thickness, select the Specify integration method option in the "Edit Thickness" dialog box. The following integration methods are available:

Gauss-Lobatto quadrature
Simpson's rule
Trapezoidal rule

Defining Integration Method for Surface Thickness

Furthermore, you can specify the "Number of integration points" from 3 to 99 by the plate thickness.

Info

You can find a theoretical explanation of the individual integration methods in the Multilayer Surfaces manual.

Isotropic Plastic (Members)

If selecting the Isotropic | Plastic (Members) entry in the "Material model" drop-down list, the tab for entering nonlinear material parameters is enabled.

Activating Nonlinear Material Model

Defining Nonlinear Material Parameters

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

Standard
Bilinear
Diagram

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

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

Activating User-Defined Material

For a bilinear definition, you can also enter a value for E_p.

More complex relations between stress and strain can be defined by means of the Stress-strain diagram. If selecting this option, the "Stress-Strain Diagram" tab is displayed.

Entering User-Defined Stress-Strain Diagram

Define a point for the stress-strain relation in each table row. You can select how the diagram continues after the last definition point in the "Diagram end" list below the diagram:

Run After Last Definition Point

In the case of "Tearing", stress after the last definition point jumps back to zero. "Yielding" means that stress remains constant when strain increases. "Continuous" means that the graph continues with the slope of the last section.

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 considered by this material model.

Isotropic Plastic (Surfaces/Solids)

If selecting the Isotropic | Plastic (Surfaces/Solids) entry in the "Material model" drop-down list, the tab for entering nonlinear material parameters is enabled.

Selecting Plastic Material Model

First, select the "Stress failure hypothesis". The following hypotheses are available for selection:

von Mises (von Mises yield criterion)
Tresca (Tresca yield criterion)
Drucker-Prager
Mohr-Coulomb

Defining Stress Failure Hypothesis

When selecting von Mises, the following stress is 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, the following stress is 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, the following 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. The difference is that no plastic strain remains after the unloading.

Isotropic Nonlinear Elastic (Surfaces/Solids)

The functionality largely corresponds to that of the isotropic plastic (surfaces/solids) material model. The difference is that no plastic strain remains after the unloading.

Isotropic Damage (Surfaces/Solids)

In contrast to other material models, the stress-strain diagram for this material model is not antimetric to the origin. Thus, the behavior of steel fiber-reinforced concrete can be displayed with this material model, for example. Find detailed information about modeling steel fiber-reinforced concrete in the technical article about determining the material properties of steel-fiber-reinforced concrete.

Material Model "Isotropic | Damage"

In this material model, the isotropic stiffness is reduced with a scalar damage parameter. This damage parameter is determined from the stress curve defined in the Diagram. This does not take the direction of the principal stresses 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 area of the stress tensor is 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 zero, no scaling is performed. Thus, the material behavior of the steel fiber concrete is modeled realistically.

Find more information about the theoretical background of the "Isotropic Damage" material model in the technical article describing the Nonlinear Material Model Damage.

Orthotropic Plastic (Surfaces) / Orthotropic Plastic (Solids)

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

If the material is plastified, the stresses remain constant. The redistribution is carried out according to the stiffnesses available in the individual directions.

Material Model "Orthotropic | Plastic (Surfaces)"

Material Model "Orthotropic | Plastic (Solid)"

The elastic area corresponds to the material model. The following yielding condition according to Tsai-Wu applies to the plastic zone:

Surfaces (2D):

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 (3D):

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 has to be defined positively.

You can think of the stress criterion as an elliptical surface in a six-dimensional stress space. If one of the three stress components is applied as a constant value, the surface can be projected onto a three-dimensional stress space.

If the value for f_y(σ) according to the Tsai-Wu equation, plane stress condition, is smaller than 1, the stresses are in the elastic zone. The plastic zone is reached as soon as f_y(σ) = 1. Values higher than 1 are not allowed. The model behavior is ideal-plastic, which means there is no stiffening.

Masonry

If the Masonry Design design add-on is activated (a license is required) in the Model – Base Data, the "Isotropic | Masonry | Plastic (Surfaces)" and "Orthotropic | Masonry | Plastic (Surfaces)" material models are available for the "Masonry" material type.