Back to Online Manuals

Is this page helpful?

5890x

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

Material Models

If the analysis add-on Nonlinear Material Behavior (license required) is activated in the Model Base Data, further options are available 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

If you use a nonlinear material model, 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 repeatedly adjusted in the course of the iterations until the stress-strain relation is complied with. The adjustment is always carried out for an entire surface or solid element. The smoothing type Constant on mesh elements should therefore always be used when evaluating stresses.

Result Smoothing

Some material models in RFEM are labeled as 'Plastic', others as 'Nonlinear Elastic'. If a structural component with a nonlinear elastic material is relieved of loads again, the strain decreases along the same path. When the load is completely removed, no strain remains.

Stress-Strain Diagram for Nonlinear Elastic

When a component is relieved of loads with a plastic material model, a strain remains after complete unloading.

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 Yield Laws in Isotropic Nonlinear Elastic Material Model.

The internal forces in plates with nonlinear material result from the numerical integration of the stresses over the plate thickness. 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

You can also specify the 'Number of integration points' from 3 to 99 via the plate thickness.

Info

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

Isotropic Plastic (Members)

When you select Isotropic | Plastic (Members) from the 'Material model' drop-down list, the tab for entering the nonlinear material parameters is activated.

Activating Nonlinear Material Model

Defining Nonlinear Material Parameters

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

Basic
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 diagram 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 '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 you select 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:

Distribution After Last Definition Point

Continuation 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 taken into account with this material model.

Isotropic Plastic (Surfaces/Solids)

When you select Isotropic | Plastic (Surfaces/Solids) from the 'Material model' drop-down list, the tab for entering the nonlinear material parameters is activated.

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

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, 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	Grenzspannung für Druck
σ_t	Grenzspannung für Zug

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. But in contrast to it, no plastic strain remains after the load is removed.

Isotropic Nonlinear Elastic (Surfaces/Solids)

The functionality largely corresponds to that of the Isotropic Plastic (Surfaces/Solids) material model. But in contrast to it, no plastic strain remains after the load is removed.

Isotropic Damage (Surfaces/Solids)

In contrast to other material models, the stress-strain diagram for this material model is not antimetric to the origin. This material model can therefore be used to model the behavior of steel fiber-reinforced concrete, for example. Detailed information on modeling steel fiber-reinforced concrete can be found in this technical article about 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 areas 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 zero, no scaling is performed. Thus, the material behavior of the steel fiber-reinforced concrete is modeled realistically.

You can find theoretical background information on the material model 'Isotropic Damage' in the technical article 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. A redistribution takes place depending on the stiffnesses that are present in the individual directions.

Material Model "Orthotropic | Plastic (Surfaces)"

Material Model "Orthotropic | Plastic (Solid)"

The elastic area corresponds to the material model Orthotropic Linear Elastic (Solids) . The following yielding condition according to Tsai-Wu applies to the plastic zone:

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 are to 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 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, plane stress state equation 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 behavior is ideal-plastic, which means there is no stiffening.

Orthotropic Plastic Weld (Surfaces)

This material model is used in analyses with the Steel Joints add-on to represent the behavior of welds in accordance with standards. Only stresses that correspond to the stress components σ_⊥, τ_⊥, and τ_|| of the weld occur in the equivalent surface. 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 plastic strain hardening for welds into account, such as the limit values f_ekv and f_x for the stress analysis according to the "Directional Method" as per EN 1993-1-8 [1] for welds, modified by a plastic component (see also the technical article Design of Fillet Welds).

Concrete

The nonlinear material models 'Anisotropic | Damage' and 'Isotropic | Damage (Surfaces/Solids)' are available for the 'Concrete' material type.

Material Models for Concrete

The two material models are described in the chapter Material Type and Material Model of the Concrete manual or above in the Isotropic Damage section.

Masonry

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

Material Models for Masonry

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

References

European Committee for Standardization. (2009). Eurocode 3: Design of Steel Structures – Part 1-8: Design of Joints; EN 1993‑1‑8:2005 + AC:2009. Berlin: Beuth Verlag GmbH.

Parent Chapter

Materials

Models

1200x

97x

Material Nonlinear Analysis

571x

33x

Tsai-Wu Material Model | Orthotropic Elastic-Plastic

1201x

111x

RF-MAT