DIANA FEA BV, hereafter just called DIANA, is a finite element analysis program used for predicting displacements in structural and geotechnical problems. The program is good for modelling reinforced concrete structures and for calculating heat transfer across the elements. DIANA also have the functionality of making the Young’s modulus dependent of temperature, which was the motivation for choosing DIANA in this project.
6.2.1 Creating the model
The dimension was set to 2D in DIANA, which means that the definition of the axis system was as shown in figure 6.2. The x-axis follows the longitudinal direction of the beam, while the y-axis follows the height of the beam. The z-axis is normal to the x-y plane.
Figure 6.2: Model shapes and axis-system
6.2.1.1 Defining shapes
The beam was created with a rectangular shape with the length and height of the beam as given in chapter 6.1.1. Two small plates were added at each end of the beam where the supports will be. These plates will be made of steel and are added to distribute the point force caused by the supports over a larger area on the concrete beam.
When two adjacent shapes have different material properties it is necessary to define a connection between them in DIANA. In this case, a structural interface element was required between the concrete beam and the steel plates at the supports. The interface material assigned to the elements was defined as a 2D line interface with high normal stiffness, 3.42e13 N/m2, and low shear stiffness, 3.42e5 N/m2.
For both the beam, the plates and the interfaces a geometry width of 12 meters into the x-y plane were added.
6.2.1.2 Defining material properties for the shapes
The beam shape was given a concrete material based on the material model in EC2, with the material properties given in table 6.1. The material uses a total strain crack model with creep and shrinkage effects included. When the total strain crack model is included, this means that the concrete will crack if the stresses in the beam reach the tensile
31
strength of the concrete, causing the material behaviour of the concrete to become nonlinear.
The ambient temperature is set to be 20°C. According to HB N400 7.2.3, the relative humidity for a bridge superstructure is 70%. The notional size of the member is as expressed equation (4.4); h0 = 0.923.
The curing period of the concrete is set to 1 day and the age at when the structure is loaded with self-weight, post-tensioning and a uniformly distributed load is set as 14 days. The strength and stiffness of concrete are varying with the aging time. In EC2, this effect is considered when the structure is loaded before 28 days after casting and this is accounted for automatically in DIANA.
6.2.1.3 Structural boundary conditions
Two structural boundary conditions were added to the structure. At the left support translation in both x- and directions were fixed. At the right support translation in y-direction were fixed. This can be seen in figure 6.3.
Figure 6.3: Boundary conditions at support
6.2.2 Loads
The structure is subjected to self-weight, post-tensioning and a uniformly distributed load.
In the early phases of the project, the structure was only exposed to self-weight and post-tensioning, and at that point it was desirable to have the self-weight and post-tensioning equivalent to each other. With the given density and dimensions of the concrete beam the self-weight can be calculated as 7063.2 kN, or 282.528 kN/m.
Equation (6.3) can be used to calculate the equivalent forces for a simply supported beam as shown in figure 6.4 for prestressing reinforcement with a parabolic form. In this case, the post-tensioning force is P = 55 181.25 kN.
𝑃 = 𝑞𝐿2
8𝑒 (6.3)
Later in the project, it turned out necessary to have a bigger bending moment in the structure, so that the temperature strain due to the beta-effect got a significant value.
Therefore, a uniformly distributed load of 300 kN/m was added to the model.
32
Figure 6.4: Equivalent forces [21].
6.2.3 Reinforcement
6.2.3.1 Passive reinforcement
The longitudinal reinforcement for the beam can be calculated by EC2 9.2.1.1 to be 𝐴𝑠,𝑚𝑖𝑛= 21934𝑚𝑚2, which satisfy the requirements for As,max. EC2 NA9.3.1.1 gives the maximum centre distance for longitudinal reinforcement as less than 250 mm while R668 3.1.3 suggests a practical (buildable) centre distance as 𝑠 = 150𝑚𝑚 for all passive reinforcement. The centre distance is therefore taken as 150 mm for both the longitudinal and the shear reinforcement. With a rebar dimension of Ø20 the values for the longitudinal reinforcement becomes 80Ø20s150 into the plane which results in a cross-sectional area of 𝐴𝑠 = 25133𝑚𝑚2. The longitudinal reinforcement is put in the top and bottom of the beam as shown in figure 6.5.
The shear reinforcement can be calculated with EC2 9.2.2(9.4) and 9.2.2(NA.9.5.N) which gives 𝐴𝑠𝑤 = 2416𝑚𝑚2. The shear reinforcement will be placed in u-forms around the longitudinal reinforcement and with a rebar dimension of Ø20 this gives a shear reinforcement of 167Ø20s150 in the plane. This results in a cross-sectional area of 𝐴𝑠𝑤= 2513𝑚𝑚2.
Since this is a 2D model where the goal is to study the long-term effects and thermal effects with no eccentric loading, it is assumed that the torsional moment and also transversal reinforcement will have little to no effect on this problem. Hence the transversal reinforcement has not been considered.
Figure 6.5: Beam model showing only the longitudinal reinforcement.
33
Figure 6.6: Beam model showing only the shear reinforcement.
6.2.3.2 Prestressing reinforcement
HB N400 2.3.5 and 2.3.6 lists the standard cable types and cable pipes in accordance with the European Technical Approval. In the model, a 12-strands cable with an outer pipe diameter of 90 mm is used. The strands have a cross-section of 150 mm2, which makes the cross-sectional area of the cables 𝐴𝑝 = 1800𝑚𝑚2.
EC2 5.10.2.1 defines the maximum stressing force applied to a tendon as;
𝑃𝑚𝑎𝑥 = 𝐴𝑝∙ 𝜎𝑝,𝑚𝑎𝑥 (6.4)
Using the material properties from table 6.3 and the cross-sectional area for the cables, equation (6.4) gives the maximum stressing force as 2656.8 kN. Dividing the prestressing force P calculated in 6.2.2 with Pmax shows that the beam needs 21 cable pipes for sufficient capacity. This gives a total prestressing area of 𝐴𝑝 = 37800𝑚𝑚2.
Figure 6.7: Beam model showing only the post-tension cable.
6.2.4 Load combination
For this project, only one load combination has been considered with all the loads, self-weight, post-tensioning and the uniformly distributed load, acting together. Table 6.4 shows the time-dependent factors defined in DIANA for the load combination. The factors are multiplied with the loads at the given time steps. Here, all of the loads are applied at the same at day 14.
Table 6.4: Time-dependent factors.
Time [days] Factor
0 0 Zero loading
14 0
All loads are applied at day 14
14 1
3650 1 Period of interest is 10 years
34
6.2.5 Meshing
The beam and support plates were meshed with Q8MEM elements with a size of 0.1 meters. These are quadrilateral isoperimetric plane stress elements with four degrees of freedom, that uses linear interpolation [28]. Figure 6.8 shows the node numbering for Q8MEM elements. L8IF interface elements were used between the concrete beam and the steel plates.
Figure 6.8: Q8MEM element [28].
The nodes along the y-axis at the middle of the beam and the node above the support is of interest later when looking at the strains. Figure 6.9 shows the relevant node numbers where node 6 is at the bottom at the middle section and node 3 is at the top. Node 18 is at the support.
Figure 6.9: (a) Node number at the support, (b) Node numbers at the mid-section.
6.2.6 Heat transfer
Originally, the intention with using DIANA was to model the heat transfer problem in the program. DIANA has the option of having a temperature dependent concrete material, which means the Young’s modulus varies with the temperature as described in chapter 3.2.2. Therefore, conduction, convection and radiation were defined for the model as well as a temperature variation. The model worked well when it was tested for temperature variation data for a few months.
However, in this project, it was necessary to have strain data for several years with temperature variations every day like the variations in figure 6.10. As mentioned, the strain is varying with the temperature. Since the temperature varies every day, this means
35
that the strain will vary every day as well. Hence, to get accurate strain results from the analysis, the time steps must be very small. This leads to a huge amount of time steps, which proved to make it very problematic to run the analysis. With further work, there might be a solution to this problem, but with the limited time and resources of this project, it was decided to move on and not use DIANA for the thermal problem. Instead, MATLAB was used to calculate the heat transfer in the beam.