Online manuals, introductory examples, tutorials, and other documentation.
Materials are required to define surfaces, cross-sections, and solids. The material properties affect the stiffnesses of these objects.
A Color is assigned to each material, which is used for the display of objects in the rendered model (see Chapter 11.1.9).
For new models, RFEM presets the two materials that were last used.
Any name can be chosen as a Description of the material. When the entered name corresponds to an entry of the library, RFEM imports the material properties.
The import of materials from the library is described in the Opening the library section.
The modulus of elasticity E describes the ratio between normal stress and strain.
To adjust the settings for Materials, click Edit → Units and Decimal Places on the menu or use the corresponding button.
The shear modulus G is the second parameter for describing the elastic behavior of a linear, isotropic, and homogenous material.
The shear modulus of the materials listed in the library is calculated from the modulus of elasticity E and Poisson's ratio ν according to Equation 4.1. Thus, a symmetrical stiffness matrix is ensured for isotropic materials. The shear modulus values determined in this way may slightly deviate from the specifications in the Eurocodes.
The following relation exists between modulus E and G, as well as Poisson's ratio ν:
When you manually define the properties of an isotropic material, RFEM automatically determines Poisson's ratio from the values of the E and G modulus (or the shear modulus from E modulus and Poisson's ratio).
Generally, Poisson's ratio of isotropic materials is between 0.0 and 0.5. Therefore, for a value of 0.5 or higher (e.g. rubber), we assume that the material is not isotropic. Before the calculation starts, a query appears asking if you want to use an orthotropic material model.
The specific weight γ describes the weight of the material per volume unit.
The specification is especially important for the load type 'self-weight'. The automatic self-weight of the model is determined from the specific weight and the cross-sectional areas of the used members or the surfaces and solids.
This coefficient describes the linear correlation between changes in temperature and axial strains (elongation due to heating, shortening due to cooling).
The coefficient is important for the 'temperature change' and 'temperature differential' load types.
This coefficient describes the safety factor for the material resistance; therefore, the index M is used. Use the factor γM to reduce the stiffness for calculations (see Chapter 7.3.1).
Do not confuse the factor γM with the safety factors for the determination of design internal forces. The partial safety factors γ on the action side take part in combining load cases for load and result combinations.
Twelve material models are available for selection in the list. Use the [Details] button in the dialog box or table to access dialog boxes where you can define the parameters of the selected model.
If the add-on module RF-MAT NL is not licensed, you can only use the Isotropic Linear Elastic and Orthotropic Elastic 2D/3D material models.
The linear-elastic stiffness properties of the material do not depend on directions. They can be described according to Equation 4.1. The following conditions apply:
- E > 0
- G > 0
- –1 < ν ≤ 0.5 (for surfaces and solids; no upper limit for members)
The elasticity matrix (inverse of stiffness matrix) for surfaces is the following:
You can define the nonlinear elastic properties of the isotropic material in a dialog box.
You have to define the yield strengths separately for tension (fy,t) and compression (fy,c) of the ideally or bilinearly elastic material. You can also define a stress-strain Diagram to display the material behavior realistically (see Figure 4.44).
If you have set the 3D model type (see Figure 12.23), you can define the plastic properties of the isotropic material in a dialog box. RFEM takes these properties for member elements into account, for example for the plastic calculation of a kinematic chain.
The nonlinear material behavior is only determined correctly in the calculation if a sufficient number of FE nodes are created on the member. For this purpose, the following options are available:
Define the parameters of the ideally or bilinearly plastic material. You can also define a stress-strain Diagram to display the material behavior realistically.
The material properties can be defined separately for the positive and the negative zone. The Number of steps determines the number of definition points respectively available. Enter the strains ε and the corresponding normal stresses σ into the two lists.
You have several options for the Diagram after last step: Tearing for material failure when exceeding a certain stress, Yielding for restricting the transfer of a maximum stress, Continuous as in the last step, or Stop for restricting to a maximum allowable deformation.
It is also possible to import parameters from an [Excel] worksheet.
Watch the dynamic graphic in the Stress-Strain Diagram dialog section to check the material properties. The dialog field Ei below the graphic shows the modulus of elasticity E for the current definition point.
Use the button in the dialog box to save the stress-strain diagram so that you can apply it to different models. To import user-defined diagrams, click the button.
For members with isotropic plastic material properties, the Activate shear stiffness of members (cross-sectional areas Ay, Az) check box in the Calculation Parameters dialog box (see Figure 7.27) has no effect. This material model uses the beam theory according to Euler-Bernoulli where shear distortions are neglected.
With this material model, you can display the properties of nonlinear materials for surfaces and solids. No energy is delivered to the model (conservative analysis). As the same stress-strain relations apply for loading and relief of load, no permanent plastic distortions are available after a relief.
You have to define the yield strengths fy,t of the ideally or bilinearly elastic material. For the hypotheses according to von Mises and Tresca, they are equally applicable for tension and compression. For an authentic display of the material behavior, you can also define a stress-strain Diagram (see Figure 4.44).
The elasticity matrix is damped isotropically in order for the stress-strain relations of the equivalent stresses and distortions to be fulfilled.
Four calculation theories are available in the Distortion-Hypothesis dialog section:
- von Mises:
- A criterion that tends to 1 is analyzed (in the plastic sense). Tension and compression stresses interact in the equations. During the evaluation, you should pay attention to the design ratio under the Criteria, not to the stresses.
- Similar to the Drucker-Prager model, a stress circle is analyzed, though it is based on the Tresca hypothesis.
Generally, many iterations are required for this material model until convergence is reached. Therefore, it is recommended to specify a minimum value of 300 as the Maximum number of iterations in the calculation parameters (see Chapter 7.3.3).
With the Only linearly elastic option, it is possible to deactivate the nonlinear material properties, for example for comparative analyses.
The following technical article provides further explanations on the yield laws of this material model:
This material model shows an isotropic material behavior in the elastic zone. The plastic zone is based on the yielding according to different distortion hypotheses with a user-defined Yield strength of the equivalent stress for surfaces and solids.
Specify the parameters of the ideally or bilinearly plastic material. You can also define a stress-strain Diagram to realistically display the material behavior (see Figure 4.44). According to von Mises and Tresca, the same yield strengths apply for tension and compression.
The yield conditions for 2D elements according to von Mises, for example, are mentioned in Equation 4.3. For 3D elements, they are as follows:
For plastic material properties, calculations are carried out iteratively and with load increments (see Chapter 7.3). If the stress is exceeded in a finite element, the modulus of elasticity is reduced there and a new calculation run starts. The process is repeated until a convergence is reached. When the calculation is done, stiffness reductions can also be checked graphically (see Chapter 9.3.2).
When evaluating results, it is recommended to use the smoothing option Constant on Elements (see Figure 9.31). The setting ensures that the defined yield strength is displayed as a maximum in the results panel: In the calculation, plastic effects can only be considered element by element. For the remaining smoothing options, however, RFEM interpolates or extrapolates the results. This may lead to distortions that are more or less pronounced depending on the mesh.
In the elastic-plastic calculation, the total strain ε is divided into an elastic component εel and a plastic component εpl.
However, this breakdown is only valid when assuming that the plastic strains are small (εpl < 0.1). If the plastic strains exceed this limit value, the plastic results should be evaluated with caution. This has to be taken into account in particular for calculations according to the large deformation analysis.
You can define stiffness properties that appear differently in both surface directions x and y. This way, you can model ribbed floors or stress directions of reinforced ceilings, for example. The surface axes x and y are perpendicular to each other in the surface plane (see Figure 4.75).
The RFEM 4 material models Orthotropic and Orthotropic Extra are converted into this model.
With this material model, you can globally assign an orthotropic property to all surfaces that consist of a particular material. Alternatively, it is possible to individually define the parameters for each surface (see Chapter 4.12).
An orthotropic elastic material is characterized by the moduli of elasticity Ex and Ey, the shear moduli Gyz, Gxz, and Gxy, as well as Poisson's ratio νxy and νyx. The elasticity matrix (inverse of stiffness matrix) is defined as follows:
The following correlation exists between principal Poisson's ratio νxy and secondary Poisson's ratio νyx:
The following conditions must be met for a positively definite stiffness matrix:
- Ex > 0; Ey > 0
- Gyz > 0; Gxz > 0; Gxy > 0
In a three-dimensional material model, you can define elastic stiffnesses separately in all directions of the solid. This way, you can display the strength properties of wood-based materials, for example.
The elasticity matrix is defined as follows:
The following correlations exist between principal Poisson's ratios νyz, νxz, νxy and secondary Poisson's ratios νzy, νzx, νyx:
The following conditions must be met for a positively definite stiffness matrix:
- Ex > 0; Ey > 0; Ez > 0
- Gyz > 0; Gxz > 0; Gxy > 0
The material model according to Tsai-Wu unifies plastic with orthotropic properties. This way, you can enter special modelings of materials with anisotropic characteristics such as plastics or timber. When the material is yielding, stresses remain constant. A redistribution is carried out according to the stiffnesses available in the individual directions.
The elastic zone corresponds to the Orthotropic Elastic - 3D material model (see above). For the plastic zone, the yielding according to Tsai-Wu applies:
ft,x, ft,y, ft,z : Plastic ultimate tensile strength in direction x, y, or z
fc,x, fc,y, fc,z : Plastic ultimate compressive strength in direction x, y, or z
fv,yz, fv,xz, fv,xy : Plastic shear strength in direction yz, xz, or xy
Ep,x : Hardening modulus
α : State variable of hardening
All strengths must be defined positively.
The stress criterion can be imagined as an elliptical surface within a six-dimensional space of stresses. If one of the three stress components is applied as a constant value, the surface can be projected onto a three-dimensional stress space (see Figure 4.51).
If the value for fy (σ) according to Equation 4.11 is lower than 1, stresses lie in the elastic zone. The plastic zone is reached as soon as fy (σ) = 1. Values higher than 1 are not allowed. The model behavior is ideal-plastic, which means no stiffening takes place.
Equation 4.11 is only valid for the local FE coordinate system. If this local coordinate system does not match the solid's coordinate system used for the stress output in RFEM, the values must be transformed accordingly.
Temperature-dependent stress-strain properties of an elastic isotropic material can be defined in a diagram or imported from [Excel]. These properties are considered for member and surface elements subjected to thermal load (changes or differences in temperature).
The Reference temperature defines stiffnesses for the members or surfaces that have no temperature loads. For example, if a reference temperature of 300 °C is set, the reduced elastic modulus of this point of the temperature curve is applied to all members and surfaces.
The Options dialog section allows you to control if the Poisson's ratios that are applied to the complete temperature diagram are identical. Clear the check box to access the Poisson's Ratio table column for individual entries.
Use the [Load] button to import predefined temperature diagrams for different steel alloys (see Figure 4.45).
Click the [Save] button to save user-defined temperature diagrams so that you can use them for other models.
Use this material model to consider masonry walls not able to bear tension forces and reacting with formation of cracks.
The dialog box allows you to define the Limit tension stresses in direction of the surface axes x and y, which means parallel and perpendicular to the support interstices. In several iterations during calculation, RFEM then finds out, which finite elements become stress-free due to the failure criterion.
When the limit tension stress is set to zero, RFEM applies a value of 1⋅10-11 N/mm2 in calculations for stability reasons. Thus, minor tensile stresses are not completely excluded.
If numerical problems occur during calculation, you can try to reach convergence by increasing the Hardening factor CH.
If the masonry material has already been defined in the library before you open the Material Model dialog box, the following limit values are preset:
The following article describes how materials can be created for masonry:
Another technical article provides information on the assessment of structural behavior of masonry in RFEM:
With this material model, you can model the material behavior of steel fiber concrete where a continuous reduction of strength occurs due to cracking.