Turbulent Flow in a curved pipe (3D)

Turbulent Flow in a curved pipe (3D)#

Goals of the tutorial:

  • Using a turbulence model in TrioCFD: RANS or LES

  • Using a periodic box to obtain a developed turbulent flow for inlet boundary conditions

  • Using TrioCFD’s parallel capabilities

Figure 7 shows the geometry of the test case you will run in this tutorial. Figure 8 shows the inlet of the pipe, where the special periodic box computation will be used.

pipe1

Figure 7 Geometry of the curved pipe#

pipe2

Figure 8 Zoom on the pipe inlet, with the periodic box in blue#

Preparation of the tutorial#

For this tutorial, start from an empty directory, e.g. TrioCFD_tutorial_curved_pipe and source the TrioCFD environment.

This tutorial will start from the validation form PeriodicBox. Use the following commands to copy this validation form:

mkdir -p PeriodicBox && cd PeriodicBox
cp ${TrioCFD_project_directory}/share/Validation/Rapports_automatiques/Turbulence/RANS/PeriodicBox/src/* .

You should now have serveral files in your PeriodicBox directory, including:

  • BuildMeshes.data: for generating the curved pipe and box meshes

  • PeriodicBoxRANS.data: for running the RANS simulation in the periodic box

  • DomainFlowRANS.data: for running the RANS simulation in the pipe with inlet steady boundary conditions

  • PeriodicBoxLES.data: for running the LES simulation in the periodic box

  • DomainFlowLES.data: for running the LES simulation in the pipe with inlet unsteady boundary conditions

Generating the meshes#

Now you will generate the meshes. The pipe mesh is stored in an archive, simply decompress it using:

gunzip Tube_coude_463259.msh.gz

For the periodic box, the mesh will be generated by the tools provided by Trust. For this, run the BuildMeshes.data file with TrioCFD/TRUST:

triocfd BuildMeshes.data

This dataset will first partition the pipe mesh for 6 cpu parallel simulation, and then generate the periodic box mesh and partition it, making it usable with 2 to 6 cores.

You can look at the BuildMeshes.data and try to understand what each line do. The syntax is relatively straightforward.

Running the PeriodicBox simulations#

Before running, open the files PeriodicBoxRANS.data and PeriodicBoxLES.data and change the parameter nb_pas_dt_max to 100, to shorten the simulations. Running the full calculations may take up to a few hours.

Then, run the simulations in parallel with two processes:

triocfd PeriodicBoxRANS 2
triocfd PeriodicBoxLES 2

Running the pipe simulations#

Before running the simulations on the full pipe, take a look at the data sets for each simulation: DomainFlowRANS.data (resp. DomainFlowLES.data). To better visualize the differences between the two, you can open/edit them via meld:

meld DomainFlowRANS.data DomainFlowLES.data &

First, change nb_pas_dt_max to 10 in both files, to shorten the calculations.

You can see that the data files contains two problems, one for the box (pb_box) and one for the pipe (pb_dom). They will be coupled together, so that the pipe problem takes the output from the periodic box as its inlet boudary condition.

Notice that:

  • we use the last iteration of the previous calculation PeriodicBoxXXX as an initial condition for the box problem (pb_box).

    • This is done for the velocity field of the Navier_Stokes_Turbulent equation and for the temperature of the Convection_Diffusion_Temperature_Turbulent equation.

    • This initialization is done with the keyword Champ_fonc_reprise in initial_conditions, and using the argument last_time (at the end of the line). last_time can also be replaced by a specific time you want to use.

  • the special coupled boundary condition is done in boundary_conditions of the pipe problem (pb_dom) with the line: inlet frontiere_ouverte_temperature_imposee Champ_front_recyclage { pb_champ_evaluateur pb_box temperature 1 }

  • most of the differences between the 2 datasets are in the definition of the turbulence models: k-espilon for the RANS simulation and WALE for the LES simulation, each having their own parameters.

Now, you can run the Pipe simulations:

triocfd DomainFlowRANS 6
triocfd DomainFlowLES 6

You can take a look at the result with visit. But using visit is out of the scope of this tutorial.

Contents