Nonlinear Calculation of a Floor Slab Made of Steel Fiber Reinforced Concrete in the Ultimate Limit State with RFEM
Steel fiber reinforced concrete is nowadays mainly used for industrial floors or hall floors, for foundation plates with low loads, basement walls and basement floors. Since the publication of the first guideline by the German Committee for Reinforced Concrete (DAfStb) about steel fiber reinforced concrete in 2010, the structural engineer can use standards for the design of the composite material steel fiber reinforced concrete, which makes the use of fiber reinforced concrete increasingly popular in construction. This article describes the nonlinear calculation of a foundation plate made of steel fiber reinforced concrete in the ultimate limit state with the FEA software RFEM.
An earlier technical article describes how to determine the material properties of steel fiber reinforced concrete and convert these material parameters in the FEA software RFEM. Pure steel fiber reinforced concrete is mainly used for industrial floors and moderately loaded foundation plates. A linear elastic determination of internal forces does not provide any economical results for purely fiber reinforced structural components. Therefore, plastic methods are usually used for the ultimate limit state. However, these plastic approaches are rather unsuitable for the serviceability limit state. A nonlinear FEM calculation is always possible regardless of the analyzed limit state. Based on the iteratively determined internal forces, we perform the design manually.
Entering the Topology and Loads
The floor slab is entered as a foundation surface. For the foundation slab of this technical article, the foundation is realized with the method of the "effective soil" according to Kolar and Nemec . The adjacent soil is taken into account by additional line springs and single springs in the corners (see also this article). You can also calculate the surface elastic foundation with the RF-SOILIN add-on module.
The ultimate limit state design is shown by the loads from the shelf supports and the load under the shelves. The shelf support loads are defined as free rectangular loads. Additionally, points with mesh refinements have been arranged on the shelf supports so that the load is distributed into the base plate distributed over several elements.
Defining Material Properties
Use the material model "Isotropic Damage 2D/3D" of the RF-MAT NL add-on module to display the material behavior of steel fiber reinforced concrete in RFEM. We use as steel fiber reinforced concrete a concrete C30/37 L1.2/L0.9 according to DIN EN 1992-1-1  and the guideline by the German Committee for Reinforced Concrete (DAfStb) about steel fiber reinforced concrete  with the two performance classes L1/L2 = L1.2/L0.9. For a nonlinear calculation, we apply the parabolic distribution according to 3.1.5  on the compression side of the stress-strain diagram. The following figure shows the characteristic distribution of the working line of the above mentioned steel fiber reinforced concrete.
We have to use the characteristic stress-strain curve for the serviceability limit state. For the nonlinear calculation of the ultimate limit state, you have to apply the following according to Chapter 5.7 of the guideline by the German Committee for Reinforced Concrete (DAfStb) about steel fiber reinforced concrete :
Rd = R (fcR; 1.04 ⋅ ffcrLi; fyR, ftr) / γR
1.04 ⋅ ffcrLi ... is the calculated mean value of the tensile stress that can be absorbed by the steel fiber reinforced concrete after cracking according to the performance classes L1 or L2
fcR, fyR, ftR ... is the respective mean value of concrete strength according to NA.10, DIN EN 1992-1-1 
γR ... is the partial safety factor for the system resistance. For pure steel fiber reinforced concrete components, γR is assumed to be 1.4.
The partial safety factor γR can be considered either on the resistance side when entering the material properties or on the action side. In this article, we apply the global partial safety factor γR directly when defining the nonlinear working line. Figure 03 shows the reduced stress-strain curve for the ultimate limit state design in comparison to the characteristic working line for the SLS.
For nonlinear calculations, you have to apply the load step by step. If the calculation of a load increment does not converge within the preset maximum number of iteration steps, increase the maximum number of iteration steps in the calculation parameters. In addition, a better convergence can be achieved when using a nonlinear material model by selecting the asymmetrical equation solver in the calculation parameters.
Ultimate Limit State Design
The ultimate limit state is considered to be reached if
- the critical ultimate strains of the steel fiber reinforced concrete, εcu1 on the compression side, εfct,u on the tension side, are reached.
- the critical state of the indifferent equilibrium is reached in the entire system or in parts of it.
After successful nonlinear calculation of the base plate, the maximum and minimum strains on the top and bottom side are checked. If the critical ultimate strains are not exceeded, the ultimate limit state design is performed.
Subsequent strains were calculated for the ultimate limit state.
- maximum compression strain εmin- = -1.9 ‰ < 3.5 ‰
- maximum tensile strain εmax- = 4.2 ‰ < 25.0 ‰
- maximum compression strain εmin+ = -1.05 ‰ < 3.5 ‰
- maximum tensile strain εmax+ = 9.9 ‰ < 25.0 ‰
Figure 05 shows the maximum distortion at the top (-z) of the foundation plate.
By adhering to the limit strains, it was possible to successfully determine the ultimate limit state subjected to bending. We have to perform additional designs in the ultimate limit state, for example punching.
Recommendations for Nonlinear Calculation with the "Isotropic Damage 2D/3D" Material Model
Based on the polygonal definition of the stress-strain curve as a diagram, RFEM expects the tangent modulus at the origin of the stress-strain curve as the modulus of elasticity of the steel fiber reinforced concrete. This means that you have to adjust the preset secant modulus for concrete as well when entering the steel fiber reinforced concrete work line. The first polygonal point on the compression or tension side of the work line expects the modulus of elasticity of the material as the slope.
An Excel file is attached to this technical article to support you during the input and calculation of the diagram points. In this Excel file, depending on the analyzed limit state, ULS or SLS, you can determine the stress-strain curve to be used and transfer it to the RFEM input dialog box by using the clipboard. This approach is also shown in the attached video.
You can save the defined stress-strain diagrams in RFEM and reuse them in other projects. Thus, you can create your own material library of steel fiber reinforced concrete in RFEM.
Due to the significant nonlinearity, the load should be applied in several load increments. The number of load increments should be selected so that the system remains in the linear elastic state in the first load increment. This improves the convergence behavior of the calculation. You can control the number of load increments globally in the calculation parameters and locally for each load combination or load case. For the design load in the ultimate limit state for the floor slab shown above, 20 load increments have proven to be advantageous for the iteration. We defined the 20 load increments locally for the load combination (Figure 08).
Dipl.-Ing. (FH) Alexander Meierhofer
Head of Product Engineering Concrete & Customer Support
Do you have questions or need advice?
Contact our free e-mail, chat, or forum support or find various suggested solutions and useful tips on our FAQ page.
Structural engineering software for finite element analysis (FEA) of planar and spatial structural systems consisting of plates, walls, shells, members (beams), solids and contact elements
Consideration of nonlinear material laws