# Nonlinear Calculation of a Floor Slab Made of Steel Fiber-Reinforced Concrete in the Serviceability Limit State with RFEM

### Technical Article

Describing the procedure for the serviceability limit state design of a floor slab made of steel fiber-reinforced concrete. This article shows how to perform the corresponding design for the SLS by means of the iteratively determined FEA results.

The design of a floor slab made of steel fiber-reinforced concrete consists of the ultimate limit state design and the serviceability limit state design. The procedure for performing the ultimate limit state design was explained in a previous Technical Article. The serviceability limit state design is now performed for the floor slab discussed in the previous article. This article shows how to perform the corresponding design for the SLS by means of the iteratively determined FEA results.

#### Enter the Topology and Loads

The plate geometry and imposed loads are transferred from the ultimate limit state design (see the technical article mentioned above).

Image 01 - Floor Slab with Racking Loads

For the serviceability limit state designs, the positive effects from shrinkage must also be taken into account. When shrinking, the floor slab tends to contract. Due to the interconnection or friction of the floor slab on the subsoil, tensile stresses occur that have to be considered. The base plate is embedded on the following layer structure (from top to bottom): Base plate, foil as a separating layer, perimeter insulation, bottom concrete layer, soil. According to [3], Table 4.19, a friction coefficient μ_{0} of 0.8 is recommended for this layer structure. For the design value μ_{0,d}, the authors of [3] recommend a partial safety factor of γ_{R} = 1.25.

μ_{0,d} = γ_{R} ⋅ μ_{0} = 1.25 ⋅ 0.8 = 1.0

In RFEM, the friction coefficient μ_{0,d} can be defined as the nonlinearity of the surface elastic foundation. Figure 02 shows the setting option in the program.

Image 02 - Evaluation of the strains for the crack width calculation with restraint

In the case of industrial floor slabs, the vertical load is of great importance for the formation of the positive action due to shrinkage strain. Before applying the rack loads and the stored goods, only the self-weight of the floor slab is available. As a result, the friction resistance of the bottom floor slab is relatively small. The tensile force N_{ctd} resulting from the friction (referred to a 1-meter-wide strip) in the floor slab is determined as follows.

N_{ctd} = μ_{0,d} ⋅ σ_{0} ⋅ L/2

where

N_{ctd}... Design value to determine the tensile stress in the floor slab when the friction force is reached

μ_{0,d}... Design value of friction

σ_{0}... Soil contact stress

L... Length of the base plate for the displacement on the soil

σ_{0} = 0.19 m ⋅ 1.0 m ⋅ 25 kN/m² = 4.35 kN/m² (self-weight of the slab)

N_{ctd} = 1.0 ⋅ 4.75 kN/m² ⋅ 24.40 m/2 = 57.95 kN/m

The maximum resulting tensile stress σ_{ct,d} resulting from friction thus results in

σ_{ct,d} = N_{ctd }/ A_{ct} = 57.95 kN/m / 0.19 m = 305 kN/m² = 0.305 MN/m² <f ^{f}_{ctm,fl} = 2.9 MN/m².

The concrete tensile stress resulting from friction under the self-weight of the floor slab is smaller than the concrete tensile strength f^{f}_{ctm,fl}. As a result, the shrinkage strain can be set free of cracks under the self-weight of the plate.

After applying the shelf loads/support reactions, however, due to the increased friction forces under the higher shelf supports, restraint forces occur that have to be considered in the calculation. In this project, the time of applying the shelf loads is assumed to be t = 180 days after concreting the floor slab. To calculate the shrinkage strain, t_{s} = 7 days is used as the start of the shrinkage and t = 18,250 days as the end of use. Furthermore, a relative humidity of 50% is assumed. The shrinkage strain is applied as an external surface load by means of the axial strain load type. At this point, we would like to point out that you can use a help tool in the Surface Load dialog box that allows you to determine the shrinkage strain easily.

Image 03 - Floor slab with shelf loads

When applying the shrinkage strain, it must be taken into account that shrinkage does not cause any restraints in the plate up to the point of time t = 180 days. Therefore, only the positive shrinkage strain ε_{cs,wk }has to be applied for the design at time t = 18,250 days. This is calculated as the difference of the shrinkage strains at t = 18,250 and t = 180 days. A detailed calculation of the individual shrinkage strains is not described in this article.

ε_{cs,wk} = ε_{cs} (18,250, 7) - ε_{cs} (180, 7) = -0.515‰ - (-0.258‰) = 0.257‰

The positive shrinkage strain is defined as an additional load and taken into account in the load combinatorics for the time t = 18,250 days.

Image 04 - Definition of the friction coefficient in the parameters of the surface foundation

For the serviceability limit state design, the "Quasi-permanent" design situation is required. The variable load for storage spaces with the combination factor ψ_{2} = 0.8 is taken into account. These load combinations are used for the design of stresses as well as the limitation of crack widths caused by a load action.

In order to consider the imposed action from shrinkage at the end of use (t = 18,250 days), the previously created load combinations are copied and the "Shrinkage" load case is added to the positive shrinkage strain ε_{cs,wk}. These load combinations are used later for the crack width analysis under load action with restraint.

#### Define the Material Properties for Serviceability Limit State Design

Use the "Isotropic Damage 2D/3D" material model of the RF-MAT NL add-on module to display the material behavior of steel fiber-reinforced concrete in RFEM. We use C30/37 L1.2/L0.9 concrete as steel fiber-reinforced concrete according to DIN EN 1992-1-1 [2] and the guideline by the German Committee for Reinforced Concrete (DAfStb) about steel fiber-reinforced concrete [1] 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 [2] on the compression side of the stress-strain diagram. Figure 05 shows the characteristic distribution of the working line of the aforementioned steel fiber-reinforced concrete.

Image 05 - Generate surface load due to shrinkage

We have to use the characteristic stress-strain curve for the serviceability limit state. As input help or help for the calculation of the diagram points, you can download an Excel file at the end of this technical article. You can transfer these diagram points to the RFEM input dialog box using the clipboard (see also the recommendations in the article about the ULS design).

#### Sserviceability Limit State Design

When performing the serviceability limit state design, you have to design the maximum allowable

- limit stresses according to 7.2, DIN EN 1992-1-1 [2],
- crack widths according to 7.3, DIN EN 1992-1-1 [2], and
- deformations according to 7.4, DIN EN 1992-1-1 [2].

After a successful nonlinear calculation of the base plate, the strains and stresses on the top and bottom sides are evaluated and used for the individual designs.

A) Design of Limit Stresses

The design of the maximum concrete compressive stress according to 7.2 (3) [2] is fulfilled if the maximum concrete compressive stress remains less than 0.45 ⋅ f_{ck} under quasi-permanent load action. For this purpose, the minimum stresses on the top and bottom sides are checked from the FEM calculation and compared to the limit value.

Top side:

maximum compressive stress σ_{2-} = | - 8.5 | N/mm² <0.45 ⋅ f_{ck} = 13.5 N/mm²

Bottom side:

maximum compressive stress σ_{2+} = | - 3.1 | N/mm² <0.45 ⋅ f_{ck} = 13.5 N/mm²

Figure 06 shows the maximum compressive stress on the top side (-z) of the foundation plate.

Image 06 - Definition of the forced shrinkage strain

Maintaining the maximum concrete compressive stress is successfully verified.

The design of the limitation of the maximum reinforcing steel stress according to 7.2. (4) and (5) [2] is not performed here because there is no reinforcing steel reinforcement.

B) Crack Width Analysis from Load Action

The crack width analysis is performed for the pure load action (at the point of time t = 180 days) and with additional consideration of the restraint due to shrinkage at the end of use (t = 18,250 days). See also the explanations above regarding shrinkage.

The existing crack width is determined on the basis of the quasi-permanent action combination. The existing crack width results from the integration of the governing strains over the crack bandwidth. The crack bandwidth is different for each load situation, and you have to take it manually from the results of the FEM calculation. The crack bandwidth is perpendicular to the considered strain direction and includes the strains that are greater than the crack strain ε_{cr} = 0.1‰.

${\mathrm{w}}_{\mathrm{k},\mathrm{vorh}}=\int {\mathrm{\epsilon}}_{\mathrm{wk}}\mathrm{dl}$

where

ε

_{Wk}... Tensile strain within the crack band

dl... Differential of the crack bandwidth

To display the limits of the crack bands in RFEM, you can also control the color panel in a way so that only strains greater than the crack strain are displayed (see Figure 07).

Image 07 - Characteristic working line of C30/37 L1.2/L0.9

For the evaluation of strains and crack bandwidth, we recommend creating a section for each considered crack band in RFEM. From this section, you can easily find the mean tensile strain and the crack bandwidth. The section must be defined parallel to the displayed strain direction. The crack width perpendicular to the x-axis on the bottom side governs in the analyzed slab. Figure 08 shows the created section with the average value for the tensile strains and the integration length.

Image 08 - Maximum compressive stress on the top of the plate

The existing crack width w_{k,prov} from pure load action (t = 180 days) results in

w_{k,prov,x} = 0.219‰ ⋅ 1.172 m = 0.26 mm <0.3 mm (for exposition class XC 2).

C) Crack Width Analysis from Load Action and Effects Due to Restraint

The crack width analysis due to load action with restraint from shrinkage results at the end of the working life. When calculating the crack width using the strains from the FEM calculation, it is important to ensure that the strain causing stress is determined in a simple recalculation. This can be explained by the shrinkage behavior of the plate up to the time t = 180 days. If the plate can contract without constraint, the FEM calculation results in a distortion that is equal to the shrinkage strain. The resulting stress is equal to zero. A tensile stress only arises when a strain causing stress ε_{wk, restraint} occurs.

ε_{wk,restraint} = ε_{FEM} + | ε_{cs,wk}|

where

ε_{wk,restraint}... strain causing stress

ε_{FEA}... strain from FEM calculation

ε_{cs,wk}... shrinkage strain

In order to determine the crack bandwidth in RFEM, it is necessary first to determine the strain of the finite element at which the element cracks under the applied restraint.

ε_{cr,FEM,}restraint = ε_{cs,wk} + ε_{cr} = -0.257‰ + 0.1 ‰ = -0.157‰

Figure 09 shows the governing section for the crack width calculation with load action and effects due to restraint. To integrate the strains across the crack bandwidth, the section must be divided into several areas.

Image 09 - Display of crack widths for cracks perpendicular to the x-axis

The existing crack width is calculated as follows:

${\mathrm w}_{\mathrm k,\mathrm{prov}}\;=\;\int{\mathrm\varepsilon}_{\mathrm{wk},\mathrm{zwang}}\mathrm{dl}$.

w_{k,prov,y} = (-0.089‰ + 0.257‰) ⋅ 0.335 m + (0.059‰ + 0.257‰) ⋅ 0.450 m + (-0.093‰ + 0.257‰) ⋅ 0.402 m = 0.27 mm < 0.30 mm (for exposition class XC 2)

The crack width could be verified.

D) Deformation Analysis

The maximum deformations can be taken directly from the RFEM results. The total displacement under the quasi-permanent load is 32.8 mm. The deformation difference of the base plate results from the difference between the minimum and maximum deformations and amounts to 32.8 mm - 9 mm = 23.8 mm (see Figure 10).

Image 10 - Section along the crack strip width

The allowable limit values and the associated system compatibility for the rack must be agreed with the rack manufacturer.

Finally, we would like to point out the very helpful recommendations for performing nonlinear calculations with the "Isotropic Damage 2D/3D" material model in the technical article about the ultimate limit state design.

#### Author

#### Dipl.-Ing. (FH) Alexander Meierhofer

Head of Product Engineering Concrete & Customer Support

#### Keywords

Steel fiber-reinforced concrete Foundation plate Floor slab High-bay warehouse Industrial floor Fiber concrete Post-cracking tensile strength Performance class

#### Reference

#### Downloads

#### Links

Write Comment...

Write Comment...

Contact Us

Do you have further questions or need advice? Contact us via phone, email, or chat or find suggested solutions and useful tips on our FAQ page available 24/7.

Steel fiber-reinforced concrete is mainly used nowadays for industrial floors. The use of fiber-reinforced concrete is becoming increasingly popular in construction.

New

The shear and longitudinal reinforcement can be specified individually for each member. Various templates are available for entering the reinforcement.- What is the maximum number of reinforcement groups that can be created in a design case in RF‑CONCRETE Surfaces?
- I would like to perform punching design of a floor slab. I have selected nodes for the design, but they are marked as invalid. Where did I make a mistake?
- Is the deformation analysis in state II included in the concrete design in RFEM 6?
- How can I open the interaction diagram from Concrete Design?
- Where can I activate creep for concrete design?

- Is it possible to design single-layer reinforced surfaces with RFEM 6?
- Why are the members invalid for the Concrete Design add-on?
- How do I perform stability analysis to determine the critical load factor in RFEM 6?
- What is the meaning of the two terms "Factorize provided reinforcement" and "Optimize provided reinforcement" in the concrete design?
- Can I switch the required reinforcement in the result tables from "mesh nodes" to "grid points?"

Associated Products