Mesh for coupled problems

Mesh for coupled problems#

This exercise demonstrates creating meshes for coupled multi-domain problems where interface connectivity is critical.

Problem Description#

Consider the cooling of a solid block by a fluid flowing through circular cross-section channels. The channel is centered within a square cross-section block. The outer boundaries of the solid are adiabatic.

Coupled problem schematic

Two domains need to be created:

  • Domain 1: Solid block

  • Domain 2: Fluid channel

Key requirement: Mesh elements must be connected at the interface between domains for TRUST to read the mesh correctly.

Setup#

mkdir -p TRUST_tutorials/salome/exo4
cd TRUST_tutorials/salome/exo4
$PathToSALOME/salome &

  • Create a new study: File → New

  • Select the Geometry module

  • Save frequently in HDF format

Creating the Geometry#

  • Create the solid block: New Entity → Primitives → Box

    • Dx = 200, Dy = 200, Dz = 400

    • Click “Apply and Close”

  • Create a vertex for the cylinder base: New Entity → Basic → Point

    • X = 100, Y = 100, Z = 0

    • Click “Apply and Close”

  • Create the fluid channel: New Entity → Primitives → Cylinder

    • Base Point: Vertex_1

    • Vector: OZ

    • Radius R = 40

    • Height H = 400

    • Click “Apply and Close”

  • Cut the cylinder from the block: Operations → Boolean → Cut

    • Main Object: Box_1

    • Tool Objects: Cylinder_1

    • Click “Apply and Close”

  • Create a partition: Operations → Partition

    • Objects: Select both Cylinder_1 and Cut_1

    • Click “Apply and Close”

Note: This partition ensures mesh connectivity at the interface.

Defining Volume Groups#

Create groups for each domain:

  • Solid domain: New Entity → Group → Create Group

    • Shape Type: Volume

    • Name: Solid

    • Main Shape: Partition_1

    • Select the hollow box

    • Click “Add” → “Apply”

  • Fluid domain: Continue in the same dialog

    • Name: Fluid

    • Main Shape: Partition_1

    • Select the cylindrical channel

    • Click “Add” → “Apply and Close”

Defining Boundary Groups#

Create surface groups for all boundaries:

  • Fluid inlet: New Entity → Group → Create Group

    • Shape Type: Surface

    • Name: Fluid_inlet

    • Main Shape: Partition_1

    • Select the bottom of the cylinder → “Add” → “Apply”

  • Fluid outlet:

    • Name: Fluid_outlet

    • Select the top circular boundary → “Add” → “Apply”

  • Solid top:

    • Name: Solid_top

    • Select the top of the box → “Add” → “Apply”

  • Solid bottom:

    • Name: Solid_bottom

    • Select the bottom of the box → “Add” → “Apply”

  • Solid lateral walls:

    • Name: Solid_lateral_walls

    • Select the four lateral boundaries of the box → “Add” → “Apply”

  • Solid-Fluid interface:

    • Name: Solid_Fluid_Interface

    • Select the top of the box → “Hide selected”

    • Select a lateral boundary → “Hide selected”

    • The lateral surface of the cylinder should now be visible

    • Select it → “Add” → “Apply and Close”

Creating the Mesh#

  • Switch to the Mesh module

  • Create the mesh: Mesh → Create Mesh

    • Name: Mesh_1

    • Geometry: Partition_1

    • 3D algorithm: NETGEN 1D-2D-3D

  • Configure parameters:

    • Click the wheel icon next to “Hypothesis” → “NETGEN 3D Parameters”

    • In “Arguments”: Change fineness from “Moderate” to “Fine”

    • Click “OK” → “Apply and Close”

  • Compute the mesh:

    • Right-click on “Mesh_1” → Compute

  • Verify groups:

    • Check that six boundaries appear under “Group of Faces” of Mesh_1

    • Check that two volume groups appear under “Group of Volumes” of Mesh_1

Exporting the Mesh#

  • Export to MED format:

    • Select “Mesh_1”

    • Right Click → Export → MED file

    • Choose MED 3.2 if possible

    • Save as Mesh_1.med

  • Dump the study: File → Dump Study

    • Save as a Python script (needed for the next exercise)

Running the Coupled Problem#

Copy and run the TRUST data file:

cp $TRUST_ROOT/doc/TRUST/exercices/salome/Coupled_pb.data .
trust Coupled_pb.data

Visualize the results with VisIt:

visit -o Coupled_pb.lata

Plot the temperature field on both domains and set the color bar min/max to 300 and 400 respectively. You will observe the solid cooling over time. Given sufficient simulation time, the solid temperature will eventually match the fluid temperature at steady state.

Contents