titulo
We use cookies from thirth parties to inprove your experience and our services. If you do not close this window we understand that you allow its use. For more information about cookies click here
Cerrar

In-plane bending with Shell elements

November , 20th 2019 | Author: Prontubeam (@Prontubeam_en) Read: 1015 times

Before downloading it... Share it!

| Download article | Times downloaded: 218

In this article we will study the bending when we model beams / lintels with shell elements. In particular, the number of elements to be used when modelling a lintel in order to capture the tractions correctly. A simple model of a wall with a lintel is used and it will be studied the degree of precision of bending as a function of the number of finite elements used in the lintel modelling

Finite Element model

For this article we are going to use the same finite element model as the one used in this article where we studied the difference of studying the same lintel but using beam elements instead of shell elements. If you are interested in this topic, we recommend you to read this article (click here). The following picture shows the geometry of the 0.5m thick wall:

Figure 1.Model geometry

As shown above, we are going to study different models varying the meshing size. In particular, 7 different mesh sizes are used: 1m, 0.5m, 0.375, 0.25m, 0.125m, 0.06m and 0.03m (edge size). The following pictures show the different models used:

Figure 2.Mesh sizes (1m, 0.5m, 0.375, 0.25m, 0.125m, 0.06m and 0.03m)

Loads

To study the mesh size effect, we will apply a vertical acceleration equal to the gravity, to simulate the self-weight. We could have used a more complex load but the best way to analyse a finite element model is to use an easy load case, as we know how the model should behave.

Materials

We have used concrete as the chosen material but the results can be extrapolated to other materials.

Young modulus: 200000MPa

Density: 2500 Kg/m3

Preliminary study

Before launching the finite element model, it is advisable to know “where we are” and “what result should we expect”. Thefore, before launching the model, we will calculate the bending moment in the middle of the lintel span and then we will compare it with the results from Ansys. We expect the result to be something between the bending moment of a simply supported beam and a fixed one.

Self-weight by meter length: 2500Kg/m3 x 1m x 0.5m x 9.81m/s2 / 1000 = 12.26kN/m

Figure 3. Bending moment in the middle of the lintel span. Pinned beam and fixed beam

The bending force in the middle of the span is between 3.44 kNxm if we consider it pinned and 1.15kNxm if we consider it embedded.

We compare these results with those returned by Ansys if we request it to calculate the bending moment in the middle of the span. I explain quickly the process and the commands in case the reader is interested. For this we select the nodes in the middle of the span, the elements connected to these nodes, located either on the left or on the right (the same result is obtained by symmetry) and we apply the following commands:

spoint ,, 3,3,5,0! It places the calculation point of the acting forces in the middle of the span at the section’s gravity center.

fsum! It calculates the acting forces and moments at the previously defined point

The following table shows the result in the different models. As we see they all give results similar to each other

 

Table 1. Bending force in the middle of the span in Ansys

As we can see, the results in Ansys do not change much depending on the mesh, it seems coherent. This will allow us to draw one more conclusion at the end of the article, in the Conclusions section.

Results in Ansys  - X direction

The following images show the axial forces Nx (forces following the horizontal direction in N / m (force per linear meter). With these images I have tried to show how the forces vary in the lintel as we are fine-tuning the meshing. All the images have the same scale to be easily compared.

Figure 4. Force FX (horizontal) in Newtons per meter calculated with Ansys

Right now, we can directly confirm that the case where the lintel has been modelled with 1 row of finite elements does NOT represent the reality. It is a result that we should NOT use to calculate the reinforcement. It does not capture the flexion in the lintel. Now, do 2 rows correctly represent the behaviour, or do you need three? We will try to analyse it below.

The following table summarizes the results shown in the previous images. That is, it shows the horizontal forces per vertical linear meter in the last element of the lower part of the lintel in Newtons. They correspond to the tensile forces that are generally used to calculate the reinforcements

Table 2. Forces according to X in N / m in the lower element of the lintel

As we see, as we fine-tune the mesh, the maximum traction is growing. It is normal. In fact, if we take the mesh to the limit, to an infinitesimal mesh, the result should be the tensile stresses according to Navier multiplied by the width of the lintel (0.5m).

The first thing we check is that the Navier-Stokes hypotheses are fulfilled. That is, we expect a linear flat distribution of tensile stresses. The following image shows that it seems that this is quite real in our case.

Figure 5. Section force distribution - Verification of Navier's hypothesis

The second thing we check is that if we apply the Navier-Stokes equations and multiply this tension by the thickness of the lintel (0.5m) we obtain the same result as it is obtained in Ansys with the refined mesh.

The following table summarizes the Ansys results and those obtained analytically with the Navier-Stokes formulae:

Table 3. Forces in the lower/upper face of the lintel calculated with Navier and obtained with Ansys

It seems that we are quite close so we accept everything we have assumed. We see that there is a slight difference between the theory and the reality. This is normal. It is not a theoretical beam and also the span / height ratio (1.5 / 1) is not big enough to consider it to behave totally as a beam. The recommendation is that values below 3/1 (light / edge) should be studied as deep beams, using a strut-and-tie model. Additionally, between the theory and the calculation of finite elements, a certain difference can be expected.

As we see, as we refine the mesh, the horizontal force according to X is growing, but what is interesting is to know how much force there is per element, as the force per linear meter increases but the size of the element decreases. We are also interested in knowing how much the total force is in the tensioned area where we will place the reinforcement bars.

The following table shows the load in the las element, the most tensioned one, in Newtons (N):

Table 4. Load in the lower element of the lintel (the most tensiled one)

As expected, as we mesh finer, the force per element is decreasing despite the force per linear meter grows. This tells us that in reality there will be no more demand for reinforcement bars. We can confirm it in the following table.

The following table shows the total force for the lower 0.25m from the bottom face of the lintel, this means that we assume that our reinforcement will be placed in a distance of 0.25m from the lower part of the lintel.

(*) In these two cases the element (0.5m and 0.33m) is greater than the 0.25 m distance that we are studying. The fact of finding smaller values is telling us that there is already a compressed zone in the distribution of stresses.

Table 5. Total tensile force at 0.25m from the bottom of the lintel

As we can see, starting from 0.25m in the size of the element (which is equivalent to modelling four rows of elements in the lintel) the total force remains constant.

In the following section we try to sum up these results in the form of conclusions.

Conclusions

After this study we can reach the following conclusions. The reader is reminded that this is the study of a particular simple case. To ensure its validity to other cases, the engineer must perform his own calculations in each particular case and validate these conclusions.

- To capture the bending on a beam using Shell elements, at least 2 rows of elements must be used at the edge. One row only is not acceptable

- Two rows of elements is the minimum that should be used. However, it is very likely that we underestimate the tensile forces to calculate the reinforcement. In our particular case, we would have underestimated them.

- From 4 rows the result seems to be acceptable, in our case we can see an error of 5% with respect to modelling with 32 rows of elements.

- The fact of using 8 or more rows does not alter the result but significantly increases the calculation time.

- If we are going to model with a single line of elements, we know that the results will not show bending stresses but we do know that we can properly get from Ansys the moments and forces to make a calculation of the section separately.

References

[1] Ansys v15.0 – Calculation program through finite elements

| Download article | Times downloaded: 218

If you like it, share it!

Share in Facebook
Share in Google+
Cargando comentarios...
¿Do you want to publish in Prontubeam? Send us your name, mail and subjet of the article. We will get in touch with you as soon as possible
Full name:
Email adress:
Subjet of the article:
Subscribe: Prontubeam in your mail
Name:
Email:
I accept the privacy policy
About the author
foto_quienes_somos
Carlos Corral . MEng Civil Engineering from the Politécnica university of Madrid. Speciality: Structural engineer. Owner and programer of Prontubeam.com and Prontubeam.com/en.
Vote the article
vote
Puntuación de artículo: 0/5 (basado en 0 votos)
Top of the month
Read 364 times this month
Read 324 times this month
Read 312 times this month
Prontubeam - Verify, calculate, check... the Civil Engineering starts here.
This website has been created by Carlos Corral. More information about cookies click here
The author of this website is not responsible for any possible error in the formulation used. The user has to verify all the results by his own.