As I promised a few weeks ago, I’m back with a tutorial! In this occasion, a cantilever beam will be modelled in Abaqus/Standard. What is more, the importance of defining a good mesh (not only the element size matters!) will be illustrated with several examples.

So, first things first. A cantilever beam is a structure which has one of its ends fully constrained. This means that all degrees of freedom are restricted. An example is presented in the following figure:

A similar case as the one presented above will be modelled using the Finite Element package Abaqus/Standard. The structure can be created using different types of elements: beam, bar, solid or shell. I have decided to model it using shell elements, since it will allow me to show the influence of the element size and type in a very simple way.

In order to create the component we need to be in the **Part** module. We should select the **3D deformable shell** **(planar) **option. Then we will be able to create the geometry. In this case a simple rectangle of 20mm x 100mm will be enough. Please bear in mind that Finite Element codes are unitless and all the parameters need to be defined in a consistent system of units. I have decided to use mm, GPa and kN.

After that, we need to change the module from **Part **to **Property**. To make things easy, let’s consider a perfectly elastic material model. Therefore, we just need to define the **Mechanical** property called **Elastic**. That material model, in its isotropic version, only requires the definition of the Young’s modulus and the Poisson’s coefficient. For instance, we could introduce an elastic modulus of 210GPa and a Poisson’s ratio of 0.3. Then, in the same module, a **section** has to be created: based on the type of our part, **Homogeneous Shell**. Then a dialog box will allow us to input the shell thickness, let´s say 5mm. Finally, the section needs to be **assigned** to the component.

For the first analysis, a coarse mesh will be used. Hence, changing to the **Mesh** module, **10 elements ** should be created. By default, the element type is set to **S4R**. This means that **reduced integration** will be considered or, in other words, only one integration point will be used for each element, i.e. the central point. Moving to the **Assembly**, **Dependent Instance** should be included, since the part has been already meshed.

For the **Step**, a **Static, General** with all the default options can be created. Before changing to the **Load **module, we can modify the** Field Output**, so that the **Contact** variables are not included in the analysis.

The last things to define are the **boundary conditions**. For the left end, all degrees of freedom should be constrained. Thus, the first boundary condition will be **Symmetry/Antisymmetry/Encastre** in the **Initial Step**. Then a **Concentrated Load** will be defined the the top right corner in **Step-1**. We can input a value of **-1kN**, acting along the vertical axis.

Now we are ready to run the simulation. Once it is completed, by default, the results are shown as follows:

From the image, you can tell that there is a variation of the colour within each element. That would suggest that the stress is changing along the element. However, as we defined the mesh with **reduced integrated elements**, only one value has been calculated for each element. In order to avoid any confusion, we need to change the **Results Options**. In the dialog box we should uncheck the **“Average element output at nodes” **option. Then, the results will be plotted in a more coherent way:

It is quite obvious that the results are not very reliable. When we face a problem like this, before remeshing, the first thing to do is to use **fully integrated elements (S4)**. This type of elements have four integration points instead of just one. Therefore, four values will be calculated for each element. Rerunning the simulation, the results do not show any remarkable improvement.

Hence, a refinement of the mesh seems to be necessary, right? Let’s see what happens when we double the number of elements using reduced integration:

This time, the results with reduced integrated elements show a very similar stress distribution if we compare it with the model with a coarse mesh and full integration. This highlights the fact that using full integration is quite a good option, even though the results still look quite inaccurate. Now it’s time to rerun the model using S4 elements intead of S4R.

Finally we are able to see some kind of stress distribution! The difference between reduce and full integration is quite remarkable now. In this case, we can see how the quality of the results has improved. Nevertheless, in order to confirm that we are on the good path for getting reliable results, we should simulate another finer mesh, let’s say 80 elements. As usual, we’ll start using S4R elements.

From the previous figure, we can see that there is going to be some localised stress areas in the structure. What is more, if we compare it with the 20 element model with full integration, we can observe how this new model is kind of calculating something similar, but obviously with only one value for each element. Thus, for the last time, we should run the same model with fully integrated elements.

Well, this is something interesting! Now we have a clear distribution and it is very similar to the one from the previous model that was simulated with S4 elements. This means that for a very rough estimation, the previous model with full integration would be more or less okay.

If we have a look at the results, we can see how if we kept refining the mesh, we would eventually get a similar stress distribution. This would also result in a model which would require much greater resources to calculate the response of the structure. Obviously, the finer the mesh, the more accurate the results, but what I wanted to show is that before remeshing, we should always consider using full integration. By doing this, we would be simulating a more precise model without increasing the computational effort that much.

I really hope you’ve found this “tutorial” useful. Very soon I’ll be back with some new posts! However, the next two articles won’t be part of this particular “dictionary”… Why is that? First of all, because I want to write a bit about how carbon fibre composites are currently being recycled. Furthermore, I will also write a post about… wait for it… The 87th Geneva Motor Show! I’ll be attending the event and hopefully I will take some good photos to share with you!