1. General
Sometimes we might see some mesh problems or errors in FEM-Design. To fully understand the problems, users must first fully understand the mesh settings and how meshes work.
2. Know your settings
In FEM-Design we have many settings that affect how the mesh is generated – most notably the mesh size settings and refinement.
Mesh size settings can be divided into two main groups: one for bars, other for shells. Also, there are global settings and local overrides for both. Additionally, there are some analysis settings that affect the speed, but do not contribute to the problems, so we just mention them here.
3. Bar element sizes
For bar elements (beams, columns, trusses) we can set the division amount – into how many finite elements the bar is divided.
A global setting is in the Settings menu. Name of this parameter is Default minimum division number:
Figure 1. Global settings for bars
Note. This setting can be overridden for each bar elemetnt with a manual tool. A common misunderstanding is that this setting can be overridden in both directions (smaller and bigger). This is not true.
This setting here sets the minimum number of elements that each bar element has. So, in the model user can override this number to be bigger but never smaller.Please note that this is for bars only! So only beams, columns, trusses and fictitious bars, but not the supports or connections!
Local settings (overrides) are in the Finite elements tab in a tool calledMinimum division number:
Figure 2. Local settings (overrides) for bar/line elements
This setting allows to change the division of any bar or line-type element (so even line supports or line connections, or plate edges). For example, I can set the division to 13 for the beam and line support here in the picture below. 
Figure 3. Overriding the values
I selected the tool, then selected the bar and the line support (number 1 in the picture). Then I set the division to 13 (number 2 in the picture) and pressed OK. After this I can see that the division number 13 is shown next to the bar and line support (number 3 in the picture).
I can also see that some elements have (-) symbol next to them. This is normal and it means that they use their own default (their own global) division. Please note that for anything other than bars, this is not the bar division setting that we described previously, but a totally separate setting instead. The default values for anything except bars cannot be set by the user. For example, the line support and line connection both only have one finite element by default. But the user can still set the manual division with the Minimum division number tool.
The division number that user sets with the tool described above, can only increase the number of elements above the global Default minimum division number that is set in the menu.
For example, in this model the global setting is 2, so no bar can have only one element. Even if the user manually sets a bar to one element, it will still have at least two in the calculations.
Figure 4. Minimum is minimum from global settings
In this picture above, even if I set the bar manually to one element only, it will still have 2 in the calculations, because the global Default minimum division number is the minimum.
4. There are more elements than I set, why?
It must be also understood that it is geometrical system that is divided into finite elements, not the physical model element. To make it clear, let’s look at the bar here:
Figure 5. Bars may have connected elements
Here we have one long beam B.1 and one short beam B.2 connected to it. Also, we have a line connection that is connected to the longer beam. If the global minimum division for bars is 2 then we might expect to see that the long beam B.1 is divided into two finite elements only. That is not true.
The reason is that at every place where we have connection to another element, we split up the geometrical system, and this geometrical system is divided into finite elements. The geometrical system is not usually shown to the user, but it can be turned on in the Object layers or it is also shown when we start the manual Minimum division number tool – it is the red colored system that we see:
Figure 6. Geometrical system behing the scenes
Here we can see that the longer beam has been split into three geometrical system “beams”. Left side of the longer beam (from the start until the connection with the other beam) is one of them and this has the global minimum division. Also, the part between smaller beam and the line connection is one “beam” that has the minimum division. And finally, the part where the line connection is connected to (the whole length of that part) is the third geometrical “beam” and has its own minimum division.
So, in this example the longer beam has at least three times minimum division = minimum of 6 finite elements.
The smaller beam B.2 has only 2 finite elements, because it has no connected elements on its body (the elements connected at the end points do not split up the geometrical system).
Tip. To see it even better, you can turn on the finite element numbers. Just follow these steps:
* turn on mesh crosses and finite element numbers in the settings:
Figure 7. Turn on finite element numbers and end points
* let FEM-Design generate the geometrical system, if it is not yet made (this happens automatically in the beginning of any analysis, so we can just start the analysis and close it after it has renumbered the elements:
Figure 8. Start analysis to generate the geometrical system and number elements
* In the Analysis tab, make sure that the Object layer called Automatically generated elements is turned on
Figure 9. Look at the layer for automatically generated elements
* you can see the finite element numbers on the elements in the Analysis tab:
Figure 10. See how many finite elements there are
* The crosses we turned on earlier show beginning and end of finite elements, so it is easy to see how many elements were generated.Note! If you select the Fine finite elements when starting the analysis (it is the default option), then there will be even more finite elements, since each element is divided up into smaller pieces. The Standard element option produces the result above, but the default Fine setting will produce this:Figure 11. More elements with Fine finite elements The finite element option is under the analysis dialogue:
Figure 12. Fine or Standard finite elements
5. What about shell element size?
Shell settings are quite similar to bars, but there are of course some additional points to look at. Shells do not have their own minimum division, instead they are divided into smaller finite elements. The finite element size is controlled by global and local settings as it were for the bars.
First let’s see the global settings on shell elements:
Figure 13. Global settings for shells
The Calculated element size setting uses a slider to set the difference from average element size that algorithm calculates. So, for example user can decide that they want 2-times denser mesh than the algorithm normally would calculate by just dragging the slider down.
The Correct according to the minimum division numbers option modifies the average element size of the shell, if the minimum division number (automatic or custom) of the boundary lines and edges requires that. So, if user has manually assigned a high division number on the edge of the plate (by using the same tool that is used for beams and was described above), then without this option turned on, the plate has normal element size but very dense edge mesh:
Figure 14. If not corrected to minimum division
With this option turned on, the mesh will be more uniform and a little bit denser everywhere, but there are no concentrated dense parts on the mesh:
Figure 15. If corrected to minimum division
The last option Region by region calculates separate element size for each region (each plate, wall, shell). It is suitable if the model has different size geometry. It makes denser mesh on smaller objects and thus may produce more finite elements than the other option. This increases the accuracy on the smaller shells, but increases the calculation run time as well:
Figure 16.Region by region
Option Consider all regions together tries to find a mesh size that fits all the shell elements in the model. This way even smaller elements get big mesh, and the number of finite elements is smaller, but at the same time the accuracy of the calculation is also smaller, but the calculations run faster. This is suitable for a model with similarly sized elements:
Figure 17. All regions together
Local size settings for shells are under the Finite elements tab in a tool Average surface element size:
Figure 18. Average surface element size tool
This tool behaves similarly to the bar minimum division tool. User can set the size of the average finite element on each shell object (plate, wall, fictitious shell). This size is then used when algorithm calculates the mesh.
Figure 19. Setting a size for plate
Here in this example, the mesh in the middle plate is even denser than on the upper small plate, because the average mesh size is set very small by the user.
Please note! When a shell already has a mesh, then just changing the settings does not mean that the mesh will be regenerated. The best way is to delete old mesh and then prepare new mesh:Figure 20. Delete old and prepare new mesh
Also, it is important to remember that as it was with bars, the shells also have connected elements, and these change the mesh size. For example, a wall and a plate are connected in the example below and there is a beam on the other edge of the plate:
Figure 21. Connected elements affect the mesh
In this example, the wall has denser mesh, since it is smaller than plate and also has windows. The plate inherits some of that because the wall and plate are connected and, in the connection, there must be the same number of finite elements. Little bit away from the edge, the plate’s mesh is getting coarser, since the plate does not require dense mesh – it is a very simple and quite big plate.
On the other side, there is a beam, which is on the edge of the plate. The beam size is half of the edge, other half is totally free. The minimum division number of that beam is set to quite high number, so the beam is divided into many finite elements as we saw before in the bar settings paragraphs. Since this beam is on the edge, the plate must use the same number of finite elements as the beam. On the other part of the plate’s edge, where there is o beam, there is no need for dense mesh. So here the mesh size is dictated by the connected objects. If we would separate the elements, then the mesh looks like this:
Figure 22. Without any connection, the mesh is simple