Abgabe (2).zip

1. Introduction

The structural analysis of spectator stands of large venues, such as stadiums, arenas, and concert halls, pose unique challenges for engineers. One of the main aspects to take into consideration are the crowd-induced vibrations that can appear when spectators walk, jump or cheer. These vibrations can significantly impact the structural integrity of the tribune stands and in most cases it is necessary to perform an accurate dynamic analysis of the structure in order to ensure safety, functionality and comfort for the spectators.

An effective approach for this dynamic analysis is to calculate the natural frequencies of the structure and compare them to the excitation frequency induced by the crowd. This is generally done, by sing finite element software to create the model and carry out the simulations.  

In our specific project we created a suitable FEM model of the structure, considering not just the reinforcement of the tribune girder, but also the fact that there will appear cracks in the concrete if it is subjected to tensile stresses. We performed a modal analysis for both scenarios, uncracked and cracked concrete and compared them to each other. Furthermore, we assumed a realistic loading scenario and conducted a time step series with complete nonlinear material behaviour.

2. System

The task of our project was to analyse a tribune girder that is part of the spectator stands of a multifunctional arena in Munich. These tribune girders are made of prefabricated parts with following materials:

• Concrete: C40/50
• Reinforcement: B500A

The tribune structure consists of several of these girders, that are allocated with a regular distance of 5.5 m between each other. On top of the beams, there are 15 cm thick prefabricated concrete steps, that span from one beam to the next one. Furthermore, there is a 70 cm high prefabricated falling protection on the front part of the beam, also spanning with a length of 5.5 m. Both are made from concrete C30/37 and must be taken into consideration in our analysis. On top of the beam there is a 30 cm thick layer of cast-in-place concrete, that has also to be considered.

In terms of support conditions, the beams are placed on concrete pillars as shown in the section below. Out of the plane it is hold by the prefabricated concrete steps on top of the beam and some horizontal plates that connect with the middle part of the beam.

Figure 1: Cross section of the tribune girderFigure 2: 3D - view of the girder

3. Modelling

Since we wanted to model the structure as close to reality as possible, modelling was a big part of our project task. The FEM software SOFISTIK suited very well to our task as it contains a large range of tools and modules, including the possibility to perform dynamic analyses by using the modules ase or dyna. We opted for a text based modelling by using the pseudo-programming language CADINP in the SOFISTIK Teddy – Editor. This workflow allows us to define every part of the structure by yourself and model the rather complicate reinforcement situation of the girder.

3.1.  Definition of materials and cross sections

The definition of materials is done in the module aqua by assigning a material number and define the mechanical properties of the material. In a first step there were defined two materials: concrete C40/50 for the volume elements, and steel B500A for the reinforcement.

To considerate the cracks of the concrete in the nonlinear time step series, there had to be defined another material for the volume elements, as SOFISTIK is not able to include the cracking of concrete for volume elements, when using the default concrete material. This material was defined as elasto-plastic material and the material properties were defined manually.

In addition, to create a realistic coupling of the reinforcement with the concrete, there was defined another elastic material that describes this relation. In section 3.3 Reinforcement there is described the definition of this material as well as the definition of the cross sections of the reinforcement.

3.2.  Volume modelling

Figure 3: Process of creating a structural volume in SOFISTIK

The volume mesh of our structure was created in the module sofimshc by using BRIC – Elements. To create this BRIC – Elements we needed to define the boundary of the volume. Every single part of the structure must be defined manually, starting from the structural points by specifying their number and the coordinates. Then there must be defined the structural lines and assigned a start and endpoint. Same must be done for the structural areas, by specifying the boundaries of the areas and setting the thickness of the elements to zero. In the end there must be defined the structural volume by selecting the boundary areas of the volume and the material, that was previously defined in the module aqua.

The following lines illustrate the input of the structural elements in sofimshc:

This workflow gives a lot of freedom when creating the model as everything is defined by yourself, but it also creates a high modelling effort if the structures become more complex. In our case the structure seems to be rather simple, but if you also consider the reinforcement this isn’t the case anymore.

The reinforcement bars connect properly with the volume, just if they lay in a previously defined structural area. This means that this area must be defined earlier when creating the volume model.  Thus, the whole girder had to be divided in total into 30 smaller “part-volumes” and later in the analysis, when there was defined an area with reduced stiffness, (Section 6.2) the “part-volumes” became 60. There were used loops and defined templates to reduce the modelling effort and get a shorter and cleaner CADINP – Code.

Figure 4: Cross sectionFigure 5: Division into "part-volumes"

 Figure 6: Division into "part volumes"

3.3. Reinforcement

 There are two main possibilities to model the reinforcement in a volume model in SOFISTIK.

3.3.1.  Rigid connection

The reinforcement bars are coupled rigidly with the concrete of the volume elements in all directions. There must just be defined a second structural line, with a given cross section, on the same location of a previously defined one. This previously defined structural line must be part of the structural volume, otherwise the reinforcement doesn’t couple with the volume elements. SOFISTIK does then automatically couple the two lines with a rigid connection.

The cross sections of the reinforcement must be defined in the module aqua.

3.3.2. Elastic connection

In real life there isn’t a rigid connection between reinforcement bars and concrete, but an elastic one. We decided to take this into account in our project to get more accurate results. The procedure to create such a coupling is the following:

1. Create a new structural line (same as in section 3.3.1)
2. Define elastic coupling in longitudinal direction
3. Define rigid coupling in transverse direction

The elastic coupling in longitudinal direction is obtained by creating longitudinal springs with a material behaviour that must be specified in the module aqua, by defining a force-displacement curve. This material describes the coupling conditions of the reinforcement bars with the concrete.

Figure 7: Elastic coupling of reinforcement with volume elements

3.4. Modelling Assumptions

 In modelling it is usual to make modelling assumption to simplify complex systems, improve computational efficiency and reduce the modelling effort.

In this project following modelling assumptions were made:

Reinforcement:

There were considered only longitudinal reinforcement bars and there wasn’t considered the constructive reinforcement. This leads to a total of 20 reinforcement bars, distributed on three bottom layers and two top layers.

Additional dead loads:

The prefabricated concrete steps on top of the beam and the falling protection were not modeled as volume elements but are taken into consideration as additional dead loads. The cast-in-place concrete on the upper part of the beam was modeled as volume element, as the reinforcement bars connect to this structure. Simplifying it was assumed that this part is made of the same concrete C40/50 as the girders.

Support conditions:

The girder has complex support conditions that are difficult to model in a realistic way. For this project we decided to simplify these supports, by using fixed and movable area supports in plane and add some more fixed point supports to avoid deformations perpendicular to the plain, as in reality the movement in this direction is limited by the concrete steps on top of the beam and the horizontal plates that connect with the middle part of the beam.

Figure 8: FEM Model of the tribune girder including support conditions

4. Loads

Following loads were applied on the structure:

Beam dead load:

The dead load of the beam is considered automatically in SOFISTIK

Dead load of prefabricated concrete parts on steps:

- Width (Lasteinzugsbreite):  5.5 m

- Thickness: 0.15 m

- Specific weight: 25 kN/m³

- Beam width: 0.5 m

Dead load of of falling protection:

- Width:  5.5 m

- Cross section: 0,18 x 0,70 [m]

- Specific weight: 25 kN/m³

- Beam width: 0.5 m

Live load:

There was assumed a live load of 5 kN/m², according to DIN-EN 1991-1-1, Kat. C5 (Areas susceptible to large crowds, e.g. in buildings for public events like concert halls, sports halls including stands, terraces and access areas and railway platforms).

This assumption lays on the safer side, as it implicates around 6 persons/ m² on the tribune stands.

- Assumption: q = 5 kN/m²,      (DIN-EN 1991-1-1, Kat. C5)

- Width:  5.5 m

- Beam width: 0.5 m

Figure 9: Dead load prefabricated parts on steps + falling protectionFigure 10: Live load

5.  Overview of loadcases 

-

Notes: primary load case (Primärer Lastfall - PLF) refers to the laod case that is already applied to they system before the new loadcase is calculated. So the system can already be deformed or if calculated with nonlinear material have plastic strains or cracks.

6. Modal Analysis

6.1. Modal Analysis of uncracked beam

Firstly, we did a modal analysis using Sofistik modul ASE and the function eige. This was done for the structure with and without the additional dead load from the prefabricated parts, the steps and the falling protection. The additional dead load defined as a load and with the function mass the load can be added as mass to the system. The frequencies for the first 4 eigenmodes are shown in the following table.

Eigenfrequencies f for complete dead load with steps and falling protection (center) and only the dead load of the beam (right)

Figure 11: 1st eigenmodeFigure 12: 4th eigenmode

6.2. Modal analysis of cracked beam

The modal analysis of the cracked beam was done by reducing the stiffness in the cracked area. It was assumed that the cracked area had a remaining stiffness (youngs modulus) of 30%. To estimate the cracked area of the beam a static analysis was performed with twice the live load. The reasoning for this approximation was that a unit step excitation has a maximum deformation of twice the static deformation. Subsequently the area that we reduced the stiffness in is shown in figure 14. As the modelling effort was already exteremely high, we assumed to only have a cracked material in the section of positive bending moment and not over the support.

Figure 13: Stresses for load case: 12 (g1 + g2 +g3 + 2*q)

Figure 14: Area with reduced stiffness shown in a different colour.

The eigenfrequencies f for the beam with a reduced stiffness and the deviation compared to the "uncracked" beam are show in the following table. 

Unsurprisingly, a reduced stiffness leads to a lower eigenfrequency f. Although one can observe that the reduction is not the same across different eigenmodes. 

Figure 15: Mode 1Figure 16: Mode 2

In the first mode we can see a significant deformation is happening in the area where the youngs modulus is reduced, while for the second mode most of the deformation is happning around the tip of the structure on the right side. So changing the stiffness in a specific area only impacts an eigenfrequency signficiantly if that area also is deformed notabely.

7. Time step analysis

For the timestep analysis we analysed the displacement in global z-direction of the point 412, that is located roughly in the middle of the first field of the beam.

Figure 17: location of point 412.

The eigenfrequency was determined by the counting the number of cycles completed in a specific time:

Figure 18: Illustrate the method of determining the eigenfrequency

7.1. Time step analysis of uncracked beam with full linear analysis

For the uncracked analysis, we first ran the simulation with a load impulse duration of 0.05 s with a$//<![CDATA[ \begin{array}{l}\Delta t = 0.01s\end{array} //]]>$ and 0.01 s with a $//<![CDATA[ \begin{array}{l}\Delta t=0.005s\end{array} //]]>$ while selecting different mass and primary load case configurations. The plots for this analysis can be found in the pdf documents "v1_implus_0.05_page_page_388ff" on the pages 388 to the end and "v2_impuls_0.01_page_397ff" on the pages 397 to the end. For the final presentation the load cases 4000+ and 5000+ were included, but the material definition for a nonlinear material was incorrect and are therefore excluded in the following. The measured frequencies were:

We can see that the simulation with a short impulse delivers better results on average. This is likely due to the shorter time step and therefore more precise displacement plot.

7.2.  Additional simulation runs 

7.2.1.  Impulse loading

A few additional simulations were. And the load cases 1100+ - 1400+ were done to confirm the results that were done in section 7.1. 

• Load case 10: static linear loadcase → no pre-cracking 
  • As can be seen in the figure 20
• Load case 20: static material nonlinear loadcase → pre-cracking
• Load case 21:static material nonlinear loadcase → pre-cracking.
  • As can be seen in the figure 21 below there is damage due to tension at location where first principle stresses have a sudden change in direction along the bottom part of the beam

Figure 20: Load case 10 - first principle stresses - no crackingFigure 21: Load case 21 - first principle stresses - cracking

Load cases series 2000+, 3000+ and 6000+ were excited by an impulse load but had different primary load cases applied to them. Unfortunately the free vibration had the same frequency as the uncracked load cases, despite the structure the Sofitstik output showing the formation of cracks.

For example for load series 2000+ after the first step only damage above the support could be observed. Until the first peak at 0.065 (load case 2012) we can observe the creation of additional cracks especially along the bottom side of the beam. Despite this immediate crack formation no change in oscillating behavior could be observed with regards to frequency.

Figure 22: Tension damage for load case 2001 (top) and 2012 (bottem)Figure 23: Displacement plot for load series 2000+

Now the idea was to impose a primary load cases that already included damage like load case 3000+ or  6000+. But those also showed no difference in frequency despite.

Figure 24: Displacement plot for load series 6000+

7.2.2.  Sinusoidal loading

Applying a sinusoidal load to the load case series 1500+, an increase in amplitude can be observed as we are close to resonance.

Figure 25: displacement plot for load series 1500+

8. Loading from jumping fans

Generally the loading from jumping fans can approximated by a fourier series with 3 terms (1-3). With the lowest frequency being between 2 and 2.3 Hz for an active crowd. This corresponds roughly to the peaks from the fourier spectrum.

Figure 26: Fourier amplitude spectrum for crowd jumping behavior (3)

9. Conclusions

In conclusion, this work has provided significant insights into the dynamic behavior of spectator stands, particularly regarding crowd-induced vibrations in a Munich arena. Through Finite Element modeling, several key findings emerged. Modal analysis revealed different eigenfrequencies for both uncracked and cracked beam configurations, highlighting the impact of crack-induced stiffness alterations. Time step analysis deepened our understanding of dynamic behavior under various loading conditions.

In our specific scenario, it appears that under the assumptions made, both uncracked and cracked structure have sufficiently high eigenfrequencies to avoid resonance under fan-induced loading scenarios.

10. References

(1) Ellis, B R., Ji, T. (2004). Loads generated by jumping crowds: numerical modelling. The Structural Engineer, 82(17), 35-40.

(2) Institution of Structural Engineers. (2008). Dynamic performance requirements for permanent grandstands subject to crowd action. IStructE Ltd.

(3) Li, G., Ji, T., Chen, J. (2018). Determination of the dynamic load factors for crowd jumping using motion capture technique. Engineering Structures, 174, 1-9. https://doi.org/10.1016/j.engstruct.2018.07.056.