Back to Online Manuals

9270x

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

Layout and Drawing (CAD)

Digital Twins

Program Functions

Result Evaluation

Printout Reports

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

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

The stiffness of the finite elements is continuously adjusted during the iterations until the stress-strain relationship is met. The adjustment always applies to an entire surface or solid element. Therefore, when evaluating stresses, the smoothing type Constant in Mesh Elements should always be used.

Result Smoothing

Some material models in RFEM are designated as 'plastic', others as 'nonlinear elastic'. If a component with a nonlinear elastic material is unloaded, the strain returns along the same path. Upon complete unloading, 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 Construction Stages Analysis add-on.

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 material result from the numerical integration of stresses over the slab thickness. To specify the integration method for the thickness, check the Specify integration method option in the 'Edit Thickness' dialog box. The following integration methods are then available for selection:

Gauss-Lobatto quadrature
Simpson's rule
Trapezoidal rule

Defining Integration Method for Surface Thickness

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

Info

A theoretical explanation of 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 this:

Standard
Bilinear
Diagram

If Standard is selected, RFEM uses a bilinear material model. The values for the modulus of elasticity E and the yield strength f_y are taken from the material library. For numerical reasons, the branch does not run exactly horizontally 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 'Base' tab.

Activating User-Defined Material

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

More complex relationships between stress and strain can be defined using the Stress-Strain Diagram. If you select this option, the 'Stress-Strain Diagram' tab is displayed.

Enter User-defined Stress-strain Diagram

Enter Custom Stress-Strain Diagram

Define a point for the stress-strain relationship in each row. You can select how the diagram is to continue after the last definition point in the 'Diagram end' list below the diagram:

Progression After Last Definition Point

With 'Failure', the stress jumps back to zero after the last definition point (for example, if 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 considered 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. In contrast to this, however, 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. In contrast to this, however, no plastic strain remains after 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, this material model can be used, for example, to represent the behavior of steel-fiber-reinforced concrete. 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 considered; rather, the damage occurs in the direction of the equivalent strain, which also captures the third direction perpendicular to the plane. The tension and compression ranges 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 zone is scaled to the length of the element. With the preset value of zero, no scaling is performed. This realistically represents the material behavior of steel-fiber-reinforced concrete.

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

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 plastic or timber.

When the material yields, the stresses remain constant. Redistribution occurs 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 material model Orthotropic Linear Elastic (Solids). The following yield condition according to Tsai-Wu applies to 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, plane stress state is less than 1, the stresses lie 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 ideally plastic, meaning no stiffening occurs.

Orthotropic Plastic Weld (Surfaces)

This material model is used in analyses with the Steel Joints add-on to represent the behavior of welds according to standards. In the equivalent surface, only stresses corresponding to the stress components σ_⊥, τ_⊥, and τ_|| of the weld occur. 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 considering the plastic material hardening of welds, 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

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 Design 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 selection for the 'Masonry' material type.