# Refining the Metal Bar Model

In the last episode we seen that our model solution for the modes of vibration of a metal bar wasn’t looking particularly good for the highest mode. In fact, when we clipped into the bar, we seen few bubbles of discontinuity in the displacement field that are not expected for linearly elastic homogeneous and isotropic bodies. To understand this we have to step back a little and think about FEM some more.

As we discussed in the FEM in a Nutshell episode, FEM does not actually solve the PDEs that govern our model. That is too complicated. Instead, FEM sets up a simplified problem. One thing we can say, though, is that for single physics problems, that is, problems described by a single PDE, FEM is guaranteed to converge to the PDE solution as the meshing is made denser and/or the higher the order of the mesh is.

So, the first port of call when our solution looks dodgy is the mesh: is it fine enough to model the system properly? In our case the model seemed to face some issues when solving for the twisting mode of the metal bar. If we look at our mesh, we will see that the cross-section of the bar is tiled by only $8$ elements, the edges being fairly long (one quarter of the cross-section edge). In reality, we would like to have at least $10$ elements along the cross-section edge, so that we can capture well all sorts of motions that involve the cross-section *as a whole* (to solve for displacement field that show more than one local maximum along the cross-section we will need more elements).

The more the better. However, keep in mind that the computational requirements of the model will go up the denser the mesh and the higher the order. Also, Elmer (but also any other solver) will face numerical issues for very high density meshes, especially if they aren’t linear elements. So, in reality, we need to compromise.

# Project Files

All the files used for this project are available here.

# Let’s Remesh!

We can open up our Salome study from the previous episode. Then, let’s go to the Mesh Module. If this seems strange, just re-watch the meshing video from the previous episode, **Meshing** section.

If you are editing the old Salome study, you can create a mesh alongside the old one. Otherwise just create a new study as in the video, but when you get to the point of creating the mesh, follow the procedure below.

We will be using a different mesh: a hexahedral mesh. We do this because our solid is a big hexahedron itself, and the nature of linear elasticity makes regular meshing of regular objects quite appropriate. Also, by selecting as a meshing parameter the segments per edge we will get a mesh that is denser in the cross-section than on the sides of the bar, meaning that our mesh will be refined to tackle our particular problem: no need to raise the computational costs by making the mesh denser everywhere! Finally, hexahedral meshes are very easy and fast to compute, so we get our improvements without needing to sit $15$ minutes or more staring at Salome’s meshing progress bar.

Once you are in the *Mesh* Module in Salome, do the following:

- Select the
*Solid_1*Geometry item from the*Object Browser*on the left. - On the upper Menu, select
*Mesh*and then*Create Mesh*. A window will popup. - On the
*3D*tab, select*Hexahedron (i,j,k)*. - On the
*2D*tab, select*Quadrangle Mapping*. - On the
*1D*tab, select*Wire Discretization*. Click the gear wheel to the right of*Hypothesis*and select*Number of Segments*. Type*20*in the the*Number of Segments*edit box and select*Equidistant distribution*in the*Type of distribution*list box. Click*OK*. - Click
*Apply and Close*. - Now, right click your newly created mesh, which is sitting in the
*Object Browser*and select*Create Groups from Geometry*. This will open up a new window. - While the new window is still open, select
*Solid_1*and all the faces (*Face_1*,*Face_2*, …) from the*Object Browser*. These will now appear in the*Elements*list in the new window. Click*Apply and Close*. - You can now right click the your mesh from the
*Object Browser*and select*Compute*. - A window will pop up after the mesh computation has finished. Dismiss it.
- Now, save your study (
*File*>*Save*) and export your mesh. Right click on it from the*Object Browser*and select*Export*and then*UNV File*.

Our new mesh will look like the one in the figure below (which is made with ParaView), left side. The mesh from the previous episode is also reported on the right, for comparison. We can see that the new *Fine Mesh* is indeed way more dense.

At this point you can use your newly exported mesh into Elmer just like explained in the previous episode, in the **Solver Setup and Solution** section.

Note that the mesh we calculated is **linear**, that is, the basis functions are linear. You can convert it to quadratic by right clicking on it from the Salome *Object Browser* and selecting *Convert to/from quadratic*. However, I found that once the mesh gets a bit dense Elmer will struggle and fail to find a solution due to denormal floating point values being generated by the calculation. So, I recommend keeping the meshes linear after a certain density, unless the particular solver actually works better with other kind of element orders (this is normally reported in the Elmer Models Manual).

Also, as mentioned, note that it is not universal that hexahedral meshes are better. Here, they are made better by the simplicity of both the domain and the PDE we are solving for. In general, tetrahedral meshes are the most flexible, allowing even mesh optimisation. So, if in doubt, go with tetrahedral.

# The Result

You can now follow along the previous episode’s **Visualization and Post-processing** section to load the simulation results into ParaView and check them out. Let’s compare the fifth eigenmode of our new solution with the fifth eigenmode of the previous solution. In the figure below we compare the new solution (left) to the old solution (right). We cut the bar in half with ParaView, so that we can see the displacement field magnitude inside the bar.

Looks like we were successful! In our refined mesh results we do not see any nasty unexpected displacement field discontinuity, or dodgy bubbles in the middle of the domain, a sign that now that we have way more than $10$ elements across the edges of the cross-section things are way more realistic.

Let’s now look at the results for the resonance frequencies.

Mode Number | Coarse Model | Refined Model |
---|---|---|

$1$ | $824.50$ $\textrm{Hz}$ | $865.18$ $\textrm{Hz}$ |

$2$ | $824.57$ $\textrm{Hz}$ | $865.18$ $\textrm{Hz}$ |

$3$ | $4941.17$ $\textrm{Hz}$ | $5196.91$ $\textrm{Hz}$ |

$4$ | $4941.69$ $\textrm{Hz}$ | $5196.91$ $\textrm{Hz}$ |

$5$ | $7290.90$ $\textrm{Hz}$ | $7147.42$ $\textrm{Hz}$ |

From the table above we can see that the resonance frequencies of the bar did change. Also, we can see that modes $1$ and $2$ have the same frequency of $865.18$ $\textrm{Hz}$, while $3$ and $4$ have the same frequency of $5196.91$ $\textrm{Hz}$, confirming that those modes are degenerate: for each one of those two degenerate frequencies the bar can oscillate in two different modes. Let’s compare again with the thin clamped bar model:

Mode Number | Thin Clamped Bar Model |
---|---|

$1$ | $824.86$ $\textrm{Hz}$ |

$2$ | $5215.20$ $\textrm{Hz}$ |

$3$ | $14486.67$ $\textrm{Hz}$ |

We can see that the agreement between the fundamentals got a bit worse in the refined model, but now the second thin bar modal frequency agrees better with the second and third degenerate mode of the refined model.

As we noted in the previous episode, the thin clamped model and the full 3D linear elasticity model are not really the same, as the governing equation for a thin bar is written for a 1D object allowed to displace only in one direction. We hence have to expect the two models predictions to differ. This is the reason why the thin bar model does not admit degeneracy while the 3D bar model does, for example. Still, this is not to say that the thin bar model does not offer insight. As a starter, we see that the first two modal frequencies are essentially the same, suggesting that our numerical solution is realistic, being in agreement with an analytical solution, albeit one for a simplified system. Moreover, the way the modal frequencies changed when we refined the model shows us that it is always worth to take a look at the bigger picture: had we focused on the fundamental frequency only instead of looking at the higher order modes we might have felt reassured by the agreement between the coarse model and the analytical one, and wrongfully concluded that our FEM model did not need any improvement.

# Conclusion

In general, when you expect your field to vary significantly along a certain length, your mesh size should be lower than a tenth of that length. But it doesn’t have to be that small everywhere! If you know, from a simplified analytical model or from a simplified FEM run with a coarse mesh, that the field will vary significantly only along a certain direction you can have your mesh to be denser along that direction only and coarser along the others. The FEM method is powerful also due to this flexibility.

Clearly, this is not an exhaustive explanation about how to mesh your domain properly. In fact, you probably noticed how many advanced options the Salome *Mesh Module* has. However, we now know where to look at first every time things smell fishy, and we also have an idea about how to go around pocking our nose to check if the smell is fishy or not. We also know that meshing is, in reality, the most important aspect of solving a FEM problem: bad mesh equals bad solution. So, as always, never blindly trust your solver and put it to the test!

On the next episode we will be moving out from vibration and we will simulate some simple acoustics!

# License Information

This work is licensed under a Creative Commons Attribution 4.0 International License.