Transient FEM analysis/fr

Créer le modèle
A partir d'un projet FreeCAD vierge, nous construisons notre bande bimétallique dans l'atelier Part : Tout d'abord, nous dessinons un solide Cube et le renommons en « aluminium ». Nous lui donnons les dimensions 100 x 10 x 2 mm (longueur x largeur x hauteur). Nous créons un deuxième solide Cube « acier » avec les mêmes dimensions et le décalons de 2 mm le long de l'axe z (via Placement → Position → z). Nous sélectionnons les deux solides (à l'aide de la touche Maj et de votre souris) et créons un ensemble booléen à partir de ceux-ci, que nous renommons « bande bimétal ». Dans l'onglet données, nous passons du mode 'Standard' à 'CompSolid' (Cela devrait aussi fonctionner en utilisant la commande Union au lieu de ensemble booléen, cependant, avec des intersections de formes plus complexes, il pourrait y avoir plus tard des problèmes avec l'analyse FEM. Mieux vaut donc s’habituer à utiliser des ensembles booléens en premier lieu). Le résultat devrait ressembler à ceci :



Affecter les matériaux
Dans l’atelier FEM, nous créons une nouvelle analyse et ajoutons un nouveau  matériau à l'analyse. Dans la fenêtre de tâches à venir, nous sélectionnons l'un des alliages d'aluminium prédéfinis. Sous « sélecteur de référence de géométrie », nous affectons le matériau à la bande inférieure de notre modèle en définissant le mode de sélection sur « Solide », en cliquant sur « Ajouter » et en sélectionnant une face ou un bord de la bande inférieure. Dans la vue liste, 'BooleanFragments:Solid1' devrait apparaître.



We close the task window and repeat the steps to create a second material 'Steel' (material card 'CalculiX-Steel') and assign it to the top strip ('BooleanFragments:Solid2').

Creating the mesh
Since a Finite Element Analysis obviously needs elements to work with, we have to dissect our model into a so-called mesh. The FEM workbench offers two meshing tools: Netgen and GMSH. We will go with Netgen here: With the Boolean Fragments objects 'bimetal strip' selected, we click on the Netgen icon in the FEM workbench. In the upcoming task window, we have to make different selections, starting from the top:


 * Max. size is the maximum size (in millimetres) of an element. The smaller the maximum element size, the more elements we get – usually the result will get more precise, but with a dramatic increase in computing time. We set it to 10.
 * Second order means, that in each element, additional nodes will be created. This increases computing time, but is usually a good choice if it comes to bending as in our analysis. We leave it checked.
 * Fineness: Select, how finely the model should be cut into elements. For more complex models with curvatures and intersections, we can increase the element number in those regions to get better results (at the cost of more computing time, of course). Expert users can also set it to User-defined and set the following parameters. For our simple rectangular model, the fineness selection has not much of an impact, we keep it at moderate level.
 * Optimize: Some kind of post-processing after meshing. We keep it checked.

A click on 'Apply' runs the mesher, and – the time depending on your computer – a wireframe appears on our model. The mesher should have created about 4,000 nodes.



Assigning boundary conditions
An FEM analysis now would result in nothing, because nothing is happening to our model yet. So let’s add some temperature: Use the initial temperature from the FEM workbench and set the temperature to 300 K. Here, no parts of the model can be selected, since this setting applies to the complete model.

Next, we use temperature acting on a face. We select the two faces at one end of the strip (Ctrl + Left mouse key) and click 'add' in the task window. Two faces of the Boolean Fragments object should appear in the list and little temperature icons on the model. We set the temperature to 400 K and close the task window. At the beginning of the analysis, the selected faces will get an instantaneous temperature rise from 300 to 400 K. The heat will be conducted along the metal strips and cause the bending of the strip.



Before we can run the analysis, an additional boundary condition has to be set: The analysis can only run, if our model is fixed somewhere in space. With we select the same two faces as for the 400 K above, and add them to the list. Red bars will appear on the model, visualising that those faces are fixed in space and not able to move around during the analysis.



Running the analysis
The analysis should already contain a solver object 'CalculiXccx Tools'. If not, we add one by using the solver icon from the toolbar. (There are two identical icons, the experimental solver should also work.) The solver object has a list of properties below in the left section of the window. Here we select the following options (leave the ones unmentioned unchanged):


 * Analysis Type: We want to run a thermomechanical analysis. Other options would be only static (no temperature effects), frequency (oscillations), or only to check the model validity.
 * Thermo Mech Steady State: Steady state means, the solver will return one single result with the physics reaching equilibrium. We do NOT want to do that, we would like to get multiple, time-resolved results (transient analysis). So set it to false.
 * Time end: We would like our analysis to stop after 60 seconds (i.e., simulation time, not real time).



After double-clicking the solver object, we check that 'thermomechanical' is selected and run 'write .inp file'. This usually takes some seconds (or a lot more for bigger models) and returns a message 'write completed' in the box below. Now we start the calculation with 'run CalculiX'. After some time, the last messages 'CalculiX done without error!' and 'Loading result sets...' should appear. When the timer at the bottom has stopped, we close the task window. (With larger models and/or slower computers, FreeCAD may freeze and we won’t see the timer running. But be patient, in most of the cases, CalculiX is still running in the background and will eventually produce results.) We should now have multiple FEM result objects listed. By double-clicking, we can open each one of it and visualise the calculated temperatures, displacements, and stresses. We can visualise the bending by selecting 'Show' in the 'Displacement' section. Since the absolute displacements are small, we use the 'Factor' to exaggerate the values.



Within FreeCAD, we can use pipelines to do some post-processing of the results. Alternatively, we can export the results in the VTK format and import them into dedicated post-processors like ParaView. For the export of multiple results (as for this analysis), there is a macro available.

Downloads

 * Example file without results (200 kB)


 * Example file with results (10 MB)