# Build your data file from scratch In this section, we will recreate step by step the data file used in [](../quick_start.md). ## Step 1 : Create an empty data file Create an empty data file named Obstacle.data in an empty `Obstacle` directory. ## Step 2 : Create your mesh Prepare a meshed domain that will be used in the simulation. You can use the [Salome](https://www.salome-platform.org/) software to do so. In order to be compliant with this tutorial, you need to name your mesh `Mesh` defined on a domain named `dom` and written in a MED file named `Mesh.med` is used. The MED file should include five boundaries: - Square: representing the obstacle - Upper: representing the upper-top boundary - Lower: representing the lower-bottom boundary - Inlet: representing the inlet-left boundary - Outlet: representing the outlet-right boundary It is important to note the names of all the boundaries because they will need to be specified when imposing boundary conditions. Here is a visualization of the mesh used in the simulation. Mesh

Now, you can start constructing your data file. You can download the mesh in med format: ```{button-link} ../_static/Mesh.med :download: :color: primary :shadow: :expand: 📥 Download mesh ``` ## Step 3 : Define the domain and read the mesh You should start by defining the dimension of the domain. In this case it is 2D. You should create an instance of the `Domaine` class, named dom as that you used in the MED file. Read the MED file and the mesh using the class `Read_MED`. Since the generated mesh may be somewhat coarse, TRUST allows you to refine it if desired. This can be done via the `Raffiner_isotrope` class applied to your domain `dom`. Insert the following into `Obstacle.data`: # Dimension can be 2D or 3D # dimension 2 # Domain definition # Domaine dom # Read the mesh from MED file # Read_MED { domain dom file Mesh.med } # Refine the mesh to have better results (optional) # Raffiner_isotrope dom ## Step 4 : Define the discretization and the problem The mesh used here allows us to use the VDF discretization. So use the class `VDF` to create an instance with the variable `my_discretization`. We will solve just the Navier-Stokes (NS) equations, making this a hydraulic problem. Create an instance of `Pb_hydraulique` and name it `pb`. Insert the following into `Obstacle.data`: # Discretization on rectangles (hexa), so use VDF # VDF my_discretization # Problem definition # Pb_hydraulique pb ## Step 5 : Define the time integration scheme You need to define which time scheme to use. Here, we will use the Euler explicit scheme. For that, we create an instance of `Scheme_euler_explicit`, named `my_scheme`, and we read its parameters. This block contains many parameters; read the comments carefully and insert the block into `Obstacle.data`. # Define your time scheme; here use explicit # Scheme_euler_explicit my_scheme Read my_scheme { # Initial time [s] # tinit 0 # Min time step # dt_min 5.e-6 # Max time step # dt_max 5.e-3 # facsec such as dt = facsec * min(dt(CFL),dt_max) ; for explicit scheme facsec <= 1. By default facsec equals to 1 # facsec 0.5 # Output criteria # # .out files printing period # dt_impr 5.e-3 # Note: small value to print at each time step # # End time [s] of the simulation # tmax 10.0 } ## Step 6: Associate the instantiated objects Now, you need to link the domain, the discretization and the time scheme to the problem. This is done by the C++ class `Associate` and `Discretize`. Insert the following into `Obstacle.data`: # Association between the different objects # Associate pb dom /* Associate domain */ Associate pb my_scheme /* Associate time scheme */ Discretize pb my_discretization /* Discretize the domain */ ## Step 7: Read the problem (medium, equation, BCs, post-processing) This is the core step: defining the problem. Start by defining the incompressible medium `Fluide_incompressible`. Then, read the Navier-Stokes equation `Navier_Stokes_standard`. Provide the pressure solver `Solveur_pression` and the spatial scheme to be used for the convection operator (here we use the third-order `Quick` scheme). Specify the initial and boundary conditions. This is done by the `Initial_conditions` and `Boundary_conditions` keywords. Here, we consider that the fluid is at rest at the initial state; so the velocity field is zero. At the boundaries, we consider a no-slip BC at the obstacle borders and symmetry at the top/bottom walls. At the inlet, we fix the horizontal velocity to 1 m/s, while the pressure is fixed at the outlet (open boundary). Finally, instruct TRUST to write the velocity and vorticity fields for visualization by creating and reading a `Post_processing` object. Read the syntax and comments carefully, then insert the block into `Obstacle.data`. # Problem description # Read pb { # Physical characteristics of medium # Fluide_incompressible { # Dynamic viscosity [kg/m/s] # mu Champ_Uniforme 1 3.7e-05 # Volumic mass [kg/m3] # rho Champ_Uniforme 1 2 } # NS equation # Navier_Stokes_standard { # Pressure matrix solved with # Solveur_pression PETSc Cholesky { } # Solve the convection operator with a 3rd order QUICK scheme # Convection { quick } # Solve the diffusion too; remember diffusion is always 2nd order centered # Diffusion { } # Uniform initial condition for velocity # Initial_conditions { vitesse Champ_Uniforme 2 0. 0. } # Boundary conditions # Boundary_conditions { Square paroi_fixe Upper symetrie Lower symetrie Outlet frontiere_ouverte_pression_imposee Champ_front_Uniforme 1 0. Inlet frontiere_ouverte_vitesse_imposee Champ_front_Uniforme 2 1. 0. } } # Post_processing description # Post_processing { # Fields # format lata fields dt_post 1.e-2 { vitesse som vorticite som } } } ## Step 8 : Solve the problem End your data file by inserting this block. This will tell TRUST to run and solve the problem. # The problem is solved with # Solve pb Save your `Obstacle.data` file and run the simulation with: trust Obstacle.data ## Results Now, you can visualize your results! You should see an animation similar to the one shown below! the well-known Von Kármán vortex street!

Also, check out our **[YouTube](https://www.youtube.com/@ceatrustplatform8802)** channel. Don't forget to like the page! 😜 --- ## The complete data file # Dimension can be 2D or 3D # dimension 2 # Domain definition # Domaine dom # BEGIN MESH # Read_MED { domain dom file Mesh.med } raffiner_isotrope dom # END MESH # # BEGIN PARTITION Partition dom { /* Choose Nb_parts so to have ~ 25000 cells per processor */ Partition_tool metis { nb_parts 2 } Larg_joint 2 zones_name DOM } End END PARTITION # # BEGIN SCATTER Scatter DOM.Zones dom END SCATTER # # Discretization on hexa or tetra mesh # VDF my_discretization # Problem definition # Pb_hydraulique pb # Time scheme explicit or implicit # Scheme_euler_explicit my_scheme Read my_scheme { # Initial time [s] # tinit 0 # Min time step # dt_min 5.e-6 # Max time step # dt_max 5.e-3 # dt_min = dt_max so dt imposed # # facsec such as dt = facsec * min(dt(CFL),dt_max) ; for explicit scheme facsec <= 1. By default facsec equals to 1 # facsec 0.5 # make the diffusion term in NS equation implicit : disable(0) or enable(1) # diffusion_implicite 0 # Output criteria # # .out files printing period # dt_impr 5.e-3 # Note: small value to print at each time step # # .sauv files printing period # dt_sauv 100 periode_sauvegarde_securite_en_heures 23 # Stop if one of the following criteria is met: # # End time [s] # tmax 10.0 # Max number of time steps # # nb_pas_dt_max 3 # # Convergence threshold (see .dt_ev file) # seuil_statio 1.e-8 } # Association between the different objects # Associate pb dom Associate pb my_scheme Discretize pb my_discretization # Problem description # Read pb { # Physical characteristics of medium # fluide_incompressible { # Dynamic viscosity [kg/m/s] # mu Champ_Uniforme 1 3.7e-05 # Volumic mass [kg/m3] # rho Champ_Uniforme 1 2 } # NS equation # Navier_Stokes_standard { # Pressure matrix solved with # /* solveur_pression GCP { precond ssor { omega 1.500000 } seuil 1.000000e-06 impr } */ solveur_pression Cholesky { } # Two operators are defined # convection { quick } diffusion { } # Uniform initial condition for velocity # initial_conditions { vitesse Champ_Uniforme 2 0. 0. } # Boundary conditions # boundary_conditions { Square paroi_fixe Upper symetrie Lower symetrie Outlet frontiere_ouverte_pression_imposee Champ_front_Uniforme 1 0. Inlet frontiere_ouverte_vitesse_imposee Champ_front_Uniforme 2 1. 0. } } # Post_processing description # Post_processing { # Probes # Probes { # Note: period with small value to print at each time step (necessary for spectral analysis) # sonde_pression pression periode 0.005 points 2 0.13 0.105 0.13 0.115 sonde_vitesse vitesse periode 0.005 points 2 0.14 0.105 0.14 0.115 sonde_vit vitesse periode 0.005 segment 22 0.14 0.0 0.14 0.22 sonde_P pression periode 0.01 plan 23 11 0.01 0.005 0.91 0.005 0.01 0.21 /* sonde_Pmoy Moyenne_pression periode 0.005 points 2 0.13 0.105 0.13 0.115 sonde_Pect Ecart_type_pression periode 0.005 points 2 0.13 0.105 0.13 0.115 */ } # Fields # format lata fields dt_post 1.e-2 # Note: be mindful of memory usage if dt_post is too small # { /* pression elem pression som vitesse elem vitesse som */ vorticite som } # Statistical fields # /* Statistiques dt_post 1. { t_deb 1. t_fin 5. moyenne vitesse ecart_type vitesse moyenne pression ecart_type pression } */ } # Saving and restarting process # /* resume_last_time binaire datafile.sauv */ } # The problem is solved with # Solve pb # Not necessary keyword to finish # End