Back to Online Manuals

7661x

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 non-linear material behavior Analysis Add-on Non-linear Material Behavior is activated (license required) in the Model Basic Settings, additional options become available in the list of material models alongside 'Isotropic | Linear Elastic' and 'Orthotropic | Linear Elastic'.

Material Models for Nonlinear Material Behavior Add-on

Calculation Methods

When using a non-linear 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 adjusted throughout the iterations until the stress-strain relationship is satisfied. The adjustment is always made for an entire surface or volume element. Therefore, the type of smoothing Constant in Mesh Elements should always be used when evaluating the stresses.

Result Smoothing

Some material models in RFEM are labeled as 'plastic,' while others are 'non-linear elastic'. When a component with a non-linear elastic material is unloaded, the strain returns along the same path. No strain remains upon complete unloading.

Stress-Strain Diagram for Nonlinear Elastic

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

Stress-Strain Diagram for Plastic

The process of loading and unloading can be simulated with the Construction Stages Analysis Add-on.

Background information on non-linear material models can be found in the technical article Flow Laws in the Material Model Isotropic Non-linear Elastic.

The internal forces in plates with non-linear material result from the numerical integration of the stresses over the plate thickness. To set the integration method for the thickness, check the option Specify Integration Method in the 'Edit Thickness' dialog. 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 provide the 'Number of Integration Points' across the plate thickness from 3 to 99.

Info

A theoretical explanation of the individual integration methods can be found in the manual Multi-layer Surfaces.

Isotropic Plastic (Members)

If you select Isotropic | Plastic (Members) in the 'Material Model' dropdown list, the register for entering the non-linear material parameters becomes active.

Activating Nonlinear Material Model

Defining Nonlinear Material Parameters

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

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 database. For numerical reasons, the branch is not exactly horizontal but has a slight increase E_p.

To change the values for the yield strength and the modulus of elasticity, activate the Custom Material checkbox in the 'Basic' register.

Activating User-Defined Material

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

To define more complex relationships between stress and strain, use the Stress-Strain Diagram. When you select this option, the 'Stress-Strain Diagram' tab appears.

Entering User-Defined Stress-Strain Diagram

Define a point for the stress-strain relation in each row. You can choose how the diagram should continue after the last definition point in the 'Diagram End' list below the diagram:

Distribution After Last Definition Point

Continuation After Last Definition Point

With 'Tearing,' the stress jumps back to zero after the last definition point. 'Flowing' means the stress remains constant with increasing strain. 'Continuous' means 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 limits for tension and compression cannot be considered with this material model.

Isotropic Plastic (Surfaces/Volumes)

Selecting Isotropic | Plastic (Surfaces/Volumes) in the 'Material Model' dropdown list activates the register for entering the non-linear material parameters.

Selecting Plastic Material Model

First, choose the 'Stress Failure Hypothesis'. The following hypotheses are available:

von Mises (Distortion Energy Hypothesis)
Tresca (Shear Stress Hypothesis)
Drucker-Prager
Mohr-Coulomb

Defining Stress Failure Hypothesis

If von Mises is selected, 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

Volumes

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 stresses are used:

Surfaces

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

Equivalent Stress According to Tresca

Volumes

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 volumes:

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 volumes:

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 Non-linear Elastic (Members)

The operation is similar to the material model Isotropic Plastic (Members). However, no plastic strain remains after unloading in contrast to the said model.

Isotropic Non-linear Elastic (Surfaces/Volumes)

The operation is similar to the material model Isotropic Plastic (Surfaces/Volumes). However, no plastic strain remains after unloading in contrast to the said model.

Isotropic Damage (Surfaces/Volumes)

Unlike other material models, the stress-strain diagram for this material model is not antisymmetric to the origin. Hence, the behavior of, for example, steel fiber concrete can be modeled with this material model. Detailed information on modeling steel fiber concrete can be found in the technical article Material Properties of Steel Fiber Concrete.

Material Model "Isotropic | Damage"

The isotropic stiffness is reduced with a scalar damage parameter. This damage parameter is determined by the course of the stress defined in the diagram. The direction of the principal stresses is not considered; instead, the damage occurs in the direction of the equivalent strain that also captures the third direction perpendicular to the plane. The tension and compression areas of the stress tensor are treated separately. Different damage parameters apply to each.

The 'Reference Element Size' controls how the strain in the crack area is scaled to the element length. No scaling occurs with the set value of zero. Thus, the material behavior of steel fiber concrete is realistically depicted.

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

Orthotropic Plastic (Surfaces) / Orthotropic Plastic (Volumes)

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

When the material yields, the stresses remain constant. Redistribution depends 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 (Volumes). For the plastic range, the following yield condition according to Tsai-Wu applies:

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

Volumes

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 positively.

The yield condition can be imagined as an ellipsoidal 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 the equation Tsai-Wu, Plane Stress State 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 inadmissible. The model behaves ideally plastic, meaning there is no hardening.

Orthotropic Plastic Weld (Surfaces)

This material model is used in analyses with the Steel Joints Add-on to accurately represent the behavior of welds according to standards. Only stresses corresponding to the stress components σ_⊥, τ_⊥, and τ_|| of the weld occur in the substitute surface. In the other stress directions, the stiffness of the substitute surface approaches zero.

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

In the 'Orthotropic | Plastic | Weld (Surfaces)' register, you can define the parameters for considering the plastic strain hardening in welds, such as the limit values f_ekv and f_x for the stress check according to the "directional method" based on EN 1993-1-8 [1] for welds, modified to include a plastic component (see also the technical article Verification of Fillet Welds).

Concrete

For the material type 'Concrete,' non-linear material models such as 'Anisotropic | Damage' and 'Isotropic | Damage (Surfaces/Volumes)' are available.

Material Models for Concrete

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

Masonry

If the Masonry Design Add-on Masonry Design is activated (license required) in the Model Basic Settings, non-linear material models 'Isotropic | Masonry | Plastic (Surfaces)' and 'Orthotropic | Masonry | Plastic (Surfaces)' are available for the material type 'Masonry'.