Overview

The TransAT User Manual is a self-sufficient document that provides step-by-step instructions on how to interact with TransAT software, in particular how to setup the simulation, create a grid, setup boundary and initial conditions. It also provides insights on how to execute a simulation and postprocess its output. Furthermore, user defined functions, run time intervention and run quality analysis tools are briefly described herein.

Contents

Chapter 1
Rapid User Guide

In this chapter the basic steps required to run a simulation using TransAT will be very briefly outlined. The following chapters will then explore these steps in further detail, including descriptions of input parameters, etc.

1.1 Basic Steps

1. Start the TransAT user interface TransATUI from the terminal with the follwing command:
    transatui.py

   Click to create a new project, then click to select the folder where the project files will be stored or create a new project folder by clicking and specifying its name. Set the Project Name field with the name of the project, e.g. myproject then click to save the project.
   
   Please note: It is highly recommended to create a new project folder for each project, as some files will always have the same name. (Starting TransAT GUI)

2. Objects: In the Geo tab, create an object or import a CAD file. (Objects)
3. Grid generation: In the Mesh & BCs Set the mesh properties and boundary conditions. (Grid Generation)
4. Physical and numerical parameters: Use the Input tab and navigate inside it to define physical models, phase properties, simulation parameters, initial conditions and the simulation outputs. (Simulation Parameters)
5. Create the project files: Use the Files menu in the top left corner of the TransATUI window to create the output files containing the mesh properties and the simulation parameters by clicking Prepare Simulation Files. This menu can be used to save the project as well by clicking Save. The preparation of simulation files is also available from the Execute tab. (Preparing the Simulation Files)
6. Initial conditions: For setting basic initial conditions use the sub-tab Initial Conditions in the main-tab Input. In order to use advanced initial conditions create a file called initialconditions.cxx (e.g. two–phase flow, where the interface between the two fluids has to be specified) and create the initial conditions by using the dedicated button in the Initial Conditions tab (Advanced Initial Conditions)
7. Run TransAT in the Execute tab. Residuals and other run-time indicators are directly available in TransAT. Post-processing of two- or three-dimensional data can be done using software packages such as Tecplot or freely available Paraview (www.paraview.org). (Execution and Post processing)

1.2 Starting TransAT

TransAT always uses the same names for input files and creates a folder RESULT for the outputs. It is therefore recommended to create a dedicated folder when starting a new simulation.

• To create a new project and run TransAT, launch the TransAT user interface TransATUI by executing the following command in the terminal

A description of the available TransAT commands can be found in the Command Line Options chapter.

• Click to create a new project
• Click to select the folder where the project will be saved
• To create a new project folder,
  • Use the browser to go to the desired parent folder then click in the top right corner of the window
  • In the window that popped up, enter a project folder name, say myproject, then click
• Click to close the browser
• Set Project Name to define the name for the project file, e.g. myproject, then click

The simulation files (grid, boundary conditions,...) will automatically be assigned the given project name when they will be saved later on. Note that the extension of TransAT project files is .stt.

For more information about the creation of projects or files handling, refer to the Project Management chapter.

1.3 Objects

1.4 Grid Generation

The domain is defined and the mesh is created in the Mesh & BCs tab. In the Mesh & BCs tab at the top of the GUI, several sub-tabs can be selected to set the grid parameters.
Domain & Grid  In the Domain & Grid sub-tab the limits of the computational domain along with the number of cells in the mesh and refinement zones are defined. To define refinement zones, check the Customized Refinement check-box, then set the parameters. Blocks  In the Blocks sub-tab, the domain can be split into several blocks. This allows for parallel computation and speeds up the process, and allows to define more complex domains. BCs  The boundary conditions are specified in BCs sub-tab.

For more information about mesh generation using TransATUI, please read the Chapter Grid Generation.

1.5 Simulation Parameters

The simulation parameters are defined in the Input tab at the top of the GUI.
In the Input tab, the physical properties of the flow to be simulated, as well as the numerical parameters of the simulation are set.

For more information about the Input tab, the reader is referred to the chapter Physics and Numerics Inputs.

1.6 Preparing the Simulation Files

To save a project,

• Click Files in the top left corner of the TransATUI window then select Save.

Saving the project stores the current status of the user interface. This does not require much space and is fast. In order to run a simulation from this state, the solver needs additional data files, which are also generated by the user interface. To do so,

• Click Files then select Prepare Simulation Files.

The Prepare Simulation Files option creates the necessary data files (grid, boundary conditions,...) to run a simulation, which require more disk space, depending on the size of the domain.

For more information about the files needed by the solver, please refer to the Project Management chapter.

1.7 Initial conditions

Initial conditions can be set:

• through the Initial Conditions sub-tab to set:
  • constant initial fields
  • automatic initial fields (divergence-free initial velocity field; only for incompressible flows)
  • initial pressure field based on the source terms (only for incompressible flows)
• through an xml file(initialconditions.xml) edited by the user (this option is particularly useful to define shapes with the Level-Set method)
• through a C++ routine (initialconditions.cxx) for complex problems (e.g. inflow velocity with a profile that is not readily available in TransAT, complex initial quantity distributions, ...)

For the initial velocity field, the default behaviour is to make it divergence-free if the fluids are incompressible. The default initial pressure field is based on the source terms if the fluids are incompressible.

To specify basic interface shapes at the initial state with Level-Set method,

• Edit the Level-Set node of initialconditions.xml generated by TransATUI to initialise the interface between the two fluids. Samples of xml initial conditions files initialising interfaces are available in <TransAT_Installation_folder>/transatMB/input/initialconditions_templates and can be used as templates to set this kind of initial conditions.

To specify problem-specific initial conditions,

• Copy the C++ initial conditions template file initialconditions.cxx from the folder transatMB/input to the new project folder, e.g. myproject
• Edit the C++ template file to set the initial conditions for variables that are being solved for (e.g. u, v, w, p, T, Level Set function ϕ, etc..)
• Click Input at the top of the GUI, then Initial Conditions on the side.
• Activate by checking Advanced Initial Conditions
• Click to check the compilation of the file (optional).
• Continue the setup of the simulation.
• Once in the Exectue window, click to initialise the variables in the domain.

An output file in the format specified in the Input tab will be written in the folder RESULT. This can be viewed using visualisation software and then verified to be valid before proceeding with the simulation. (For more details: see Chapter Running a Simulation)

1.8 Execution and Post processing

• In the Execute tab, click to launch the simulation

Residuals and run-time data can be visualized in real time in the Residuals section on the right-hand side. The full 2D or 3D results can be viewed using software such as Tecplot or Paraview (www.paraview.org); results can be found in the RESULT folder.

For more details see the Running TransAT section and the Post-Processing chapter.

Chapter 2
Project Management

Project management is performed from the opening window of the TransATUI (Fig. 2.1) or by using the options offered by the Files button.

In the opening TransAT window projects can be created and loaded. Files provides the same options with the addition of the possibility to create the files that are needed to run the TransAT solver.

2.1 Creating a Project

After starting TransATUI,

• Click to create a new project. In the next window, select the folder where the project files will be stored and click .
• Set the Project Name field with the name of the project, e.g. myproject then click to save the project.

If the Project Name field is not modified before clicking , the default project name newproject will be used.

After clicking , the Mesh & BCs tab will be opened and several tabs will be accessible. To make the simulation ready to run, the simulation files (also called setup files) need to be created. To do so,

• Click the Files button in the top left corner then select Prepare Simulation Files.

2.2 Saving and Loading a Project

Once modifications have been made to a project, they can be saved for future use by clicking Files then selecting Save.

This will not change the simulation files. They need to be re-generated if changes are done in the Mesh & BCs tab. To do so,

• Click Files then select Prepare Simulation Files.

A project can also be renamed by clicking Files then selecting Save As.

Please note: The input file transat_mb.inp and the material property file properties.dat, as well as some grid-related files, will always have the same names, independently from the project name. It is therefore recommended to have only one project in a folder everytime.

To load an existing project,

• Click Files then select Open Project.

If the simulation files were not generated, it will not be possible to run the simulation directly. The simulation files need to be created in the project folder by clicking Files then selecting Prepare Simulation Files.

2.3 Solver Output Files Management

Before running a simulation, the simulation files must be created for the TransAT solver. The list of simulation files includes:

• the corner grid file (extension: .grda), where the cell properties are stored.
• the boundary conditions file (extension: .bc), where all the boundary conditions are defined.
• the input file (transat_mb.inp), which includes all the numerical parameters as well as the physical models used for the simulation.
• the initial conditions file (initialconditions.xml), which includes the parameters that are set in the Initial Conditions tab.

If a CAD file is used to define a geometry inside the mesh domain, an extra file, which is created automatically, is needed to run the simulation:

• a solid properties file (properties.dat), where different solid related properties are defined for each solid in the domain.

In case of coupling TransAT with another software, the Coupling properties file Coupling_parameters.cfg is also written.

A visualisation file is written at the same time as the other simulation files. Its format depends on the visualization software (i.e. either Paraview or Tecplot) chosen in the Output Management sub-tab in the Input tab. Its name is automatically set.

This visualization file is particulary useful to verify the geometry and the simulation domain before running a simulation.

The simulation files can be saved at any time when preparing a simulation, by clicking Files then selecting Save or Prepare Simulation Files.

Please note: All the files are saved in the Project Folder, where the stt file has been saved.

2.4 Recovering Input Files

When running a simulation (See Chapter Running a Simulation), a reference file named transat_mb.out is created, saving all input options in the RESULT folder.

Chapter 3
Grid Generation

Only cartesian meshes can be created using TransATUI. The Mesh & BCs tab gives access to the grid generation modules. There are four tabs on the left-hand side, where all the grid properties can be set.

Geometries in either STL or GTS format can be read by TransAT to generate a 3D mesh with refinements. In TransAT, the meshes are structured per block. The TransAT mesher can be used to generate multi–block meshes, with or without Block-based Mesh Refinement (BMR).

Figure 3.1 shows the tab for grid generation, which contains a preview of the mesh on the right side.

3.1 3D Viewer

The 3D graphics viewer on the right shows the mesh and the surfaces either in a 3D perspective or in 2D planes, adjustable by the user.

The view icons at the bottom left corner of the visualisation panel offer the options to choose between the 3D view and 2D slices in the x-, y- or z-plane.

To reset the view, click in the bottom left of the window. This will return the mesh to the default view in the current perspective or plane selected. This is useful especially if the mesh is away or outside of the current viewing space. Or, if the mesh is zoomed in or out, the reset view will return the entire mesh within the viewing space.

In 2D view mode, when Cut is activated, the intersection between the grid plane and objects is shown in red.

Note that the Cut option is available only in 2D view mode and is displayed after clicking in the top left corner of the visualisation panel. Once Cut is activated, the grid plane can be changed by using the scroller at the top right corner of the graphical view window.

Other view buttons are also available in the top left corner of the visualization pane by clicking to show or hide them. An image of the mesh can be exported in either JPG or TIFF formats by clicking .

By clicking in the top left corner, the mesh will be reset. This can be used to reset the current domain bounds, reset and remove extra blocks and to reset the mesh around CAD objects. For example, if an object was loaded into the mesh, but the object is not shown, clicking in the top left will rebound the domain around the object.

3.2 Create a geometry

TransAT provides a small geometry module to create simple geometries, that can be used afterwards as solid objects in the setup of the simulation to be run.

3.2.1 Creating a geometry

The geometry creation modules is accessible by clicking Geo at the top of the TransAT window.

The Geo module has three tabs where geometries can be created and modified:

• The Create Shape tab enables the user to create simple geometries.
• Database enables one to load pre-existing geometries in TransATUI.
• Objects is used for modifying the properties of objects and enables one to load a geometry file that has been already created. Objects can also be transformed in this tab.

Several shapes can be used to create geometries with TransAT. The shapes of the objects to be created are selected in the drop-down list below the list of objects (dark grey area). The following shapes can be chosen:

• Cube
• Cylinder or cylinder array
• Cone
• Pipe or pipe array
• Sphere
• Plate
• Bend
• T-Junction

A specific name can be given to the geometry to be created by filling in the text field below the shape-selection drop-down list. The geometry is created after clicking .
Once the shape is created it is sent directly to the mesh. The Objects tab can be used to transform objects and modify the properties.

3.2.2 Load a geometry from the TransAT database

To load objects from the TransAT database of objects

• Click Database
• Open a folder and select an object to be imported in the list GTS Object Library
• Click to import the objects
• the object is sent directly into the mesh

3.2.3 Load a geometry from an external source

GTS and STL files can be loaded in the Geo tab. To load a geometry created with an external software

• Click
• Select the geometry (.gts or .stl file) to be loaded with the file browser that popped up then click
• The object is loaded directly into the mesh.

In the Objects sub-tab some transformations can be applied, and properties can be defined for the Objects.

3.2.4 Object operations

Once a geometry has been loaded to the mesh, simple geometric operations can be applied to it: Rotation, Translation and Rescaling.

To apply geometric operations to a geometry

• Click the Objects tab.
• Select an object from the list
• Find the Object Transformation input and choose the transformation type from the drop-down list.
• Click to define the transformation
• Enter the position, rotation, or scale values and click
• The values are saved and can be modified later by the same procedure

3.2.5 Object Motion

Motion can be specified for a CAD file under the Objects sub-tab. This motion can consist of translation or rotation. The user has two options for defining the motion, either as Specified Motion or Flow Coupled.

Specified Motion forces the Object to move with the given translational or rotational velocity. The fluid will be impacted and react to this motion. It is possible to set translational and rotational simultaneously, as well as multiple directions and axes of motion.

Coupled Motion, as the name suggests, couples the movement of the object to the flow of the fluid. A fluid flow impacting the Object will transfer moment and cause motion in the Object. Again, it is possible to have translational coupling and rotational coupling. Both types of coupling can be activated simultaneously.

To define motion to a geometry

• Click the Objects tab.
• Select an object from the list
• Find the Type of Object Motion
• In the drop-down list, Fixed is the default type that keeps an object stationary
• To specify motion, switch the type to Specified Motion. Click to set constant values for translation or rotation
• To define coupled motion, switch the type to Flow Coupled. Click to activate Translational and/or Rotational Coupling.

3.2.6 Properties of Solid Objects

The physical properties of solid objects are available for modification in the Objects sub-tab. Figure 3.2 shows what this tab looks like. To adjust the properties for an object, select an object in the list of objects loaded in the mesh (dark grey area). For problems not involving heat transfer, default values may be used. Figure 3.3 shows the window where object properties are set.

To modify properties of a specific object,

• Highlight the object to be modified in the list of loaded object (dark grey area) then set the properties in the fields below it.

If the CAD file contains several objects, the properties of the different objects can be set individually. To do so,

• Click the cross to the left of the CAD file in the list of loaded objects (dark grey surface area) to make all the objects it includes appear (See Fig. 3.3).
• Select the object to be modified then set its properties

The changes to the properties are automatically saved.

For each solid, the following properties can be defined :

• Heat Source: Volumetric heat source in the solid (available only with conjugate temperature model)
• Heat Capacity
• Thermal conductivity
• Density
• Roughness: Roughness of the solid walls
• Porosity: Value must be between 0 (only solid is present) and 1 (only fluid is present).
• Pore Size: Size (in meters) of pores if porosity between 0 and 1
• Forchheimer Coef.: Flow coefficient in Forchheimer equation for porous objects
• Contact Angle: Angle between the interface and the wall passing through the heavier phase. It can be defined between 10^o and 170^o. If a film thickness is defined, this value is ignored.
• Surface coverage: Number of adsorption sites, in mole per square meter. A value greater than zero enables surface reaction.

Temperature model and Concentration model define the boundary condition at the fluid-solid interface. They can be of the following types:

• Neumann: a constant flux is assumed at the fluid-solid interface. The flux value needs to be defined with that boundary condition
• Dirichlet: a constant value is assumed at the fluid-solid interface. The temperature or scalar value need to be defined with this model.
• Conjugate: this option is only available for the temperature equation. With this boundary condition, on top of being solved in the fluid domain, the temperature equation is also solved in the solid.

Each object is considered as an immersed surface and mesh refinements are applied around each one of them by default. These options can be deactivated.

• To disable the representation of an object as an immersed surface and hide it, uncheck Enable for IS computation when setting the properties of said object.
• To remove the automatic refinements around an object, uncheck Enable for Grid Refinement when setting the properties of said objects.

The deactivation of the Enable for IS Computation option is very useful when several geometries are present and one object hides another.

Note the objects for which Enable for IS computation is deactivated are not exported to new GTS files (see next paragraph). However, they are still taken into account when creating the simulation files.

With the deactivation of the Enable for Grid Refinement option no automatic refinement will be created when selecting Edges Refinement or Blocks Refinement in the Domain & Grid tab (see sections Grid Properties and Multi-Block).

Solve Temperature in Solid can be activated to solve for temperature within an object. Solving for solid temperature is not possible for Conjugate temperature boundary conditions (Dirichlet or Neumann required) Please note: Ensure to activate Temperature under Equations in the Inputs when defining the physics for the simulation.

Optimize Graphics improves the rendering speed for objects loaded into the mesh. This is activated by default, ensuring fast visualization of the object. Un-checking Optimize Graphics will show all details of the object, in case some features were smoothened.

Set CAD as Solid can be used to set Objects as solids (flow obstruction) or fluids (flow domain). This is only possible with one CAD file loaded to the mesh. For the basic use of TransAT, multiple CAD files must all be set as solids. To work around this issue, merge the solids together using a CAD software.
Please note: For advanced techniques to set multiple CAD files as solids or fluids, please contact support at ams@poyry.com

Representation of the Object

Immersed Surfaces is a technique applied for objects in the flow, and applies to all objects for which Enable for IS computation is activated. Immersed Surfaces must be activated if any objects are Enabled for IS computation and properties can be adjusted by clicking . For more information on Immersed Surfaces, refer to the Immersed Surfaces section.

In TransAT, geometries of CAD files are considered as solids by default. This is displayed by the Set CAD as Solid check box. If the CAD file actually represents the fluid domain and not the solid domain, the Set CAD as Solid check box should be de-activated.

For the basic use of TransAT, multiple CAD files must all be set as solids. The check box will be hidden if more than one CAD file is imported into the mesh. To work around this issue, merge the solids together using a CAD software.
Please note: For advanced techniques to set multiple CAD files as solids or fluids, please contact support at ams@poyry.com

Immersed Surfaces

Immersed Surface will enable the use of the Immersed Surface Technology (IST, see Equations and Algorithms manual, Section Immersed Surface Equations ). It is automatically checked when at least one solid object loaded into the computational domain has the Enable for IS computation option activated.

Clicking opens a window to set advanced parameters (Fig. 3.4):

• Surface file format defines the type of the .ls file. Currently, only ASCII file format can be used.
• EI smoothing formulation defines the type of the smoothing near to embedded interface. Two options are available: Smooth and Sharp. Please note: Sharp formulation is still beta released.
• Thicken factor option is useful when the geometry is too thin compared to the mesh: it thickens the object by a width equal to the thicken factor times the minimum cell size.
• Hembed Support: if the fluid region occupies less than this fraction of the cell volume, it is considered that the cell is fully occupied by the solid.
• Apply Initial Embedded Interface: if it is turned on, then properties of the solids are applied at initialization of the simulation.

3.3 CAD File Management

Geometry files can be added or removed from TransAT using the Geo tab. Objects can be added through any of the subtabs Create Shape, Database or Objects directly into the mesh.

CAD File Requirements

Given the particularity of the IST technique applied for solids (See the Equations and Algorithms Manual, Section Immersed Surface Equations ), TransAT has some specific requirements with regards to the CAD geometries that can be imported.

Two CAD formats are supported by TransAT, namely GTS and STL formats, with the latter being the widely used format in which geometries are exported by CAD software.

Note that the geometry file must be written in ASCII format to be usable by TransAT. Also, when using TransATUI on a Linux platform, make sure that the geometry file format is appropriate for Linux.

The geometry must respect the following properties:

• The geometry must represent volumes, or closed surfaces. Open surfaces cannot be loaded in TransAT.
• Two volumes must not be adjacent if they are in the same stl-format file, i.e. they should not have a common surface. If you are in such a case, either merge your volumes with your CAD tool, or save them into two different files, which will be loaded separately, but do not patch different stl-format files together into a single file if they have common surfaces, otherwise TransAT will identify it as an open surface. However, different volumes can overlap.
• With the same idea in mind, several volumes cannot share a single edge if they are saved in the same file. Once again, save the volumes into different files if you find yourself in this case.
• A cell can take into account only one fluid-solid interface with classical Immersed Surface Technology.
• If there is a small gap between the different objects be aware that a fluid flow may develop between the two objects because of possible rounding errors, and this might cause instabilities in the solver.

If you have troubles importing your CAD files, please contact support (ams@poyry.com).

Adding Objects

The button opens a file chooser starting from the current directory to select a geometry file.

After selecting the geometry file and clicking , a window will pop up where units of the objects can be set. Also, the domain boundaries can be adapted for the Object by checking the box Resize Mesh around Geometry.

After the object is loaded, TransAT checks if the object geometry is a Closed surfaces. The Immersed Surfaces Technique in TransAT requiring objects with non-zero thickness, a warning will be displayed if the objects geometry happens to be opened.

Please note: objects representing open surfaces will not be loaded by TransAT.

Removing Objects

The button removes a selected object from the mesh. To do so, select an Object from the list to be removed. Once selected, the is shown above the object list. Clicking this button will remove the selected Object from the mesh.

3.4 Definition of the Domain

The boundaries of the domain are set in the Domain & Grid tab. The domain can then be adjusted thanks to the Multiblock options (See Section Multi-Block). Figure 3.6 shows this Tab. There are several options to modify the boundaries of the domain:

• The first option is to simply enter the domain boundaries in the fields of the domain section
• The second option consists in clicking then moving the sliders to the desired position or filling in the fields in the Define Domain window that popped up after clicking . Click to confirm the changes and close the define domain window

In the Define Domain window, the button resets the domain boundaries back to the default calculated values and the , or can be clicked to change the view.

Also note that the fields are changed accordingly to the position of the sliders and vice versa.

Figure 3.5: Define Domain window

Please note: Be aware that the boundaries of the domain bounding box must be set before the setting the Blocks parameters. After modifications in the Domain & Grid tab, changes done in the Blocks tab are lost.

3.5 Grid

In Figure 3.6, the Domain & Grid tab, in which cell sizes are set, is shown.

In this tab the grid density is set by either giving the minimal cell size or the number of cell (Nx, Ny, Nz) corners for each direction. Furthermore, the Cell Ratio between two neighbouring cells (when refining) and the Maximal Ratio between the smallest and largest cell can also be set.

When setting the number of corners, bear in mind that it is advised to to have Nx- 1, Ny - 1, Nz - 1 divisible by 2 many times over. Such numbers of cells give the possibility for Multigrid preconditioning at several levels.

The three check-boxes at the bottom are used to set the type of refinement applied to the grid. The grid can be refined over the whole bounding box of each surface with the Blocks Refinement option as shown in Fig. 3.7, or it can be refined only around the edges of the bounding boxes with the Edges Refinement option as in Fig. 3.8.

After activating the Customized Refinement check-box, the user can choose to refine in the x, y, or z directions from the options shown, as in Fig. 3.9.

To create a refinement zone

• Select a direction (X-axis, Y-axis or Z-axis) in the tree located below the Customized Refinement check-box.
• Click to create a new refinement zone. A drop-down list and several fields will be displayed below the tree.

Refinements can be done around a point by choosing the Point option or over a Range. in the drop-down menu.

• Coordinates for a point or range can be directly entered.
• Using the button, the ”click-on” grid value can be taken. These are the coordinates shown in the lower right view of the mesh.
• If the ”click-on” grid value is taken, then the corresponding x, y or z value is copied into the input box.
• Once the parameters of the refinement zone have been set, click to the right of the tree to save them.

Figure 3.7: Refinement over whole Objects.

Figure 3.9: Customized refinement parameters

3.6 Blocks

Defining and setting up multi–block meshes is done in the Blocks tab. There, one can split the grid into several blocks of different sizes, which can then be distributed to several CPUs.

3.6.1 Mesh Information

To obtain general information on the mesh, such as the number of cells or the size of the domain, the user can refer to the information in the Mesh Info panel. To display the mesh information,

• Click the icon at the bottom right of the TransATUI.

In the Mesh Info panel that appears after clicking (see Fig. 3.10), the user can find:

• The BMR level of the selected block,
• the number of cells of the selected block in x, y and z direction (denoted by Nx, Ny and Nz, respectively) and its total number of cells,
• the dimensions of the selected block,
• the total number of cells of the mesh.

3.6.2 Block decomposition

The block decomposition is done thanks to the Select Block field, the , , and icons.

• Select Block This box allows the user to select a block among the ones that were already created, either by clicking on the arrows or by directly entering the block number.

  Please note: Selecting a block with the mouse is possible: Ctrl + left click will select the block, Ctrl + right click will display options to do block operations (Modify, Split, Split and Shrink, Add Son Block and Delete)

• The Modify Block icon, , opens a new window that enables modifying the dimensions of the block that is currently selected. The block size can be modified either by dragging the boundary sliders in the desired direction (switching between different 2D views is done by toggling either of the x/y, x/z or y/z view options at the bottom of the window), or by directly specifying the coordinates of the block’s corners on the right-hand side of the window. The coordinates will be automatically rounded off to the nearest grid corner.

  ---

  
  

  Figure 3.11: Modifying the dimensions of a selected block. In this example, the modifications are applied to block number 5 of Fig. 3.13.

  ---

• The Split Block icon, , allows the user to split the selected block in each direction. The split location can be defined either by dragging the boundary sliders in the desired direction (switching between different 2D views is done by toggling either of the x/y, x/z or y/z view options at the bottom of the window), or by directly specifying the coordinates of the split planes on the right-hand side of the window. The coordinates will be automatically rounded off to the nearest grid corner.
• The Split and Shrink Blocks icon, , opens a window with option boxes to specify:
  • Number of new blocks Indicates in how many parts the current block should be split for each direction. An example is shown in Fig. 3.12 where the whole grid is split into 12 blocks in the XY plane.
    

    ---

    
    

    Figure 3.12: Creating a 4x3 block decomposition

    ---

  • Shrink outside Objects Specifies to remove blocks during the split operation. Outside indicates that blocks entirely outside of the Object will be deleted. This is helpful in automatically reducing the number of cells and blocks around an object. It is possible to remove blocks closer or further away from the object by adjusting the Distance.
    
  • Shrink inside Objects Specifies to remove blocks during the split operation. Inside indicates that blocks entirely within the Object will be deleted. This is helpful in automatically reducing the number of cells and blocks around an object. It is possible to remove blocks closer or further away from the object by adjusting the Distance.
    
  • Fast Shrink This option signifies to use a fast algorithm in removing blocks while splitting. This is only available if either Shrink outside Objects or Shrink inside Objects is checked. The algorithm implemented will only remove relevant blocks, while maintaining the default size. In contrast, Detailed Shrink would also shrink the size of blocks near the Object.
    
  • Detailed Shrink This option activates an advanced algorithm for deleting and shrinking blocks. Detailed Shrink is independent from a Fast Shrink, and accordingly, will deactivate Fast Shrink once selected. Along with deleting blocks outside of the shrink region, the Detailed Shrink will also reduce the size of blocks near the Object. This can also be controlled with the Distance input, by giving a smaller distance to reduce the blocks sizes closer to the Object.
    Hint: For large domains, use Fast shrink to quickly test different block decompositions (Nx, Ny, Nz and distance parameters). Optionally, once ideal parameters are found, undo and repeat with detailed shrink to more closely wrap the blocks around the object.
  • Distance The Distance input controls (if Shrink inside and/or outside activated) how close to delete and/or shrink blocks near the Object. A small shrink distance will remove blocks and cells close to the Object. While entering a larger shrink distance will keep more blocks and cells.
    Hint: Typically, a distance value 4 times the minimum cell size provides a reasonable buffer zone of cells around the object.

    By default, the positions and sizes of newly created blocks do not depend on the immersed objects present in the domain. There are cases, however, where the computational domain of interest is mainly inside or outside immersed objects of irregular shapes. To avoid manually deleting and resizing blocks, one can use the shrinking options to directly ignore the inside and/or outside of the objects and shrink the new blocks by a factor or distance. The Distance value is the distance away from the Object to keep cells. All cells located past this distance (inside or outside of Objects according to check-boxes) will be deleted. Deleting unnecessary cells far away from the object will minimize the number of computational cells and hence computational cost. Also, a fast or detailed shrink method can be selected. A Fast Shrink simply deletes blocks, without further shrinking. Using Detailed Shrink, will also shrink blocks so that fewer cells fall outside the shrink distance. An example is provided in Fig. 3.13.

    ---

    
    

    Figure 3.13: Shrinking options. Use the Shrink inside/outside Object option to create blocks fitted around an object’s boundaries. The Distance specifies how close to the Object interface newly created blocks are shrunk.

    ---

• The Delete Block icon, , deletes the currently selected block. This leaves a hole in the computational domain with symmetry boundary conditions on its boundaries. This can be used to create a (cuboid) obstacle, or to reduce the size of the computational domain (e.g. by removing cells inside solids where no equations are to be solved).

3.7 Block Mesh Refinement

For a BMR grid there are some starting parameters for the initialisation and then some tools to modify the resulting grid as needed.

The starting parameters are:

• Number of initial levels: the number of refinement levels.
• Ratio level 2. In the BMR the refinement is done starting from the existing grid and splitting its cells into n parts in each direction (i.e. n³ new cells for each old one). Here one can specify the ratio n between the initial grid and the second level grid. This ratio can also be modified after the initialisation.
• Initialize BMR: this button initialises the BMR framework and builds the BMR grids. If there is at least one object loaded, TransAT will create new refined grid around it. To exclude an object from the BMR refinement or to reduce the refinement levels for a single object, disable it in the properties window (in Objects→Properties).

The initial dimensions of the grids are calculated automatically after clicking . They can be further modified. In fact, once the BMR is initialised, all the other tools can be used. In particular:

• Select block: go through all the grids (all are identified by an index), the selected one is showed in a different colour. The selected grid can be modified in different ways as explained below
• Show BMR Level: makes the selected grid visible/invisible
•  : opens a new window in which the selected block can be modified. In particular
  • ratio of refinement can be modified separately for each direction,
  • size of the block can be modified using the slider and the preview window or modifying manually the coordinates of the sub-domain.
•  : add a new refined block inside the selected one specifying ratio and boundaries.
•  : using this button one can split a block into any number of parts. Splitting a block in either x, y , or z will divide that block uniformly into the given value i.e. giving x direction a value of 3 will result in the one initial block being split into 3 separate blocks of uniform dimensions aligned along the x plane. Shrink enables a user to remove unnecessary split blocks around an embedded object by defining a distance or shrink factor and applying. This feature can be very useful in reducing the number of excess highly resolved blocks around an embedded so as to cheapen the simulation considerably without the user having to manually remove said blocks.
•  : delete the selected block if it does not contain son blocks.

3.8 Boundary Conditions (BCs)

The BCs tab is used to set boundary conditions on surfaces. To define boundary conditions on objects go to the Object sub-tab in the Geo tab. The BCs tab is shown in Figure 3.14.

A boundary surface is defined as boundary cell faces oriented in the same direction AND being located on the same plane. As an example, Figure 3.15 shows three different boundary surfaces highlighted, where independent boundary conditions can be applied.

The top part of the BCs tab contains the list of boundary surfaces in the form of a tree. It is used to list and select boundary surfaces. Modify the value in the drop-down list above the boundary surfaces tree to display the boundary surfaces only in a given direction. The boundary surfaces in all directions can be displayed in the list by selecting All surfaces in the Boundary drop-down list.

3.8.1 Assigning a boundary condition to a surface

With a click on the icon, the user can create a new boundary condition. It can then be given a name, and defined as one of the basic types consisting of:

• Inflow
• Outflow
• Wall
• Symmetry
• OlgaCoupling
• Cyclic

Properties of these boundary conditions can then be defined by clicking on . A description of boundary condition property panels is available in the Section Boundary conditions properties.

Once the boundary condition is defined, it can be assigned to a boundary surfaces. To do this,

• Select the boundary condition by clicking the light grey square next to it in the list of boundary conditions.

The little square will become orange when the selection is effective.

• In the list of boundary surfaces, select the boundary surfaces to which the bounadry condition is to be applied then click

Note that a boundary condition can also be assigned to several surfaces at once. To do so

• Select the surfaces of interest at once by pressing the Ctrl key while selecting them
• Check the boundary condition to be assigned in the boundary conditions table
• Click assign to complete the assignment of the boundary condition

After the assignment is complete, the surfaces are colored with the color associated to the boundary condition in the boundary condition table.

To see which surfaces have a given boundary condition assigned, select the boundary condition and click .

Please note: boundaries can be directly selected in the view window on the right using Ctrl + left click.

Also note that one boundary condition can be assigned to several surfaces, but a boundary surface can have only one condition assigned. To define different boundary conditions on the same boundary surface, sub-boundary conditions need to be created. Their use is described in the next section.

3.8.2 SubBCs

To create a boundary condition that does not span the full boundary surface,

• In the surface tree, select the boundary surface where the sub-boundary surface will be added (e.g. XMIN 0).
• Click to create a subBC. The button is visible next to the other buttons once a surface is selected.

A new window will be opened where boundary patches can be defined (Fig 3.16). With this tool, boundary patches can be specified on each of the boundary surfaces.

Please note: The SubBC takes precedence over the larger boundary condition and SubBCs cannot intersect each other.

SubBCs can however be created inside another patch (See Figure 3.17). In this case, the smallest SubBC will have precedence over the bigger ones.

Figure 3.16: Sub-BCs window

3.8.3 Boundary conditions properties

3.8.4 Inflow boundary conditions

Basic properties for inflow boundary conditions are the temperature of the fluid at the inflow, the bulk velocity and the velocity profile. Other, more specific inflow conditions can be applied. They are described in the following section.

Inflow Properties

Several options exist to specify inflow conditions. Depending on the nature of the inflow, the choices can be narrowed down. They can be accessed by clicking at the corresponding line in the boundary conditions table.

Basic

In the Basic tab the essential inflow variables can be set.

• Inflow Data Source, From BC will let the user define all inflow properties in the current window, From Initial Conditions will apply the inflow properties as defined in initial conditions.
• Inflow Type defines the type of inflow boundary: velocity based (the velocity magnitude) or total pressure based (the total pressure is fixed). In the case of compressible single-phase flows, fixing the total temperature or the Mach number is also possible. For both compressible and incompressible flows an inflow From BC of type Total P and T based (total pressure and total temperature based) is also available.
• Inflow Profile sets the velocity profile for velocity based inflow type (only for velocity-based inflow; inflow can be set by velocity components or volume/mass flow rates). For incompressible flow the choices are: constant, laminar and turbulent. In case of compressible flow two velocity profiles at the inflow are available: constant and laminar.
• Flow direction normal to boundary by default normal flow direction is used, however user may set the flow diection by specifying velocity vector components here (this option is available for pressure based inflow). The magnitude of Flow direction vector is unimportant because TransAT will normalize it.
• Inflow Total Pressure is the total pressure at inflow.
• Inflow Total Temperature is the total temperature at inflow.
• Inflow Static Pressure is the static pressure at inflow, to be used only for supersonic flows, where the pressure must be defined at the inflow. Defining the inflow and outflow static pressure for a subsonic flow may lead to an ill-posed problem.
• Flowrate specification Default is Velocity. This choice drop-down defines the specification type for the inflow. Available options are Velocity, Volume flowrate or Mass flowrate. Details for these specifications are described below in the next three items.
• Inflow Velocity Components provide the vector components for the velocity based inflow.
• Inflow Volume Flow Rate can be given in case the volume flow rate is known. This option is limited to single phase flow and multiphase homogeneous flow (no slip between phases).
• Inflow Mass Flow Rate can be given in case the mass flow rate is known. This option is limited to single phase flow and multiphase homogeneous flow (no slip between phases).
• Inflow Concentration is the value of the scalar at the inflow.
• Inflow Temperature is the static temperature of the flow at the inflow.
• Boundary Layer Thickness is the thickness of the boundary layer in SI units (only for velocity-based inflow).

Turbulence (RANS)

Turbulence(RANS) has two variables.

• Turbulence Intensity is the ratio of the root mean square of the velocity fluctuations to the Reynolds averaged mean velocity.
• Mu_t/Mu is the ratio of the turbulent (eddy) viscosity to the fluid (dynamic) viscosity.

The values described above are used for velocity or pressure based inflow with data source from BC or initial conditions.

Oscillatory Inflow

Oscillatory Inflow has three variables.

• Oscillation Period specifies the time required for one oscillation to complete
• Oscillation Phase Angle is the starting point (angular) at time zero
• Oscillation Relative Velocity provide the factors of the oscillation velocity. The factors are given in terms of relative values to the current inflow velocity components.

Please note: Default values of -10¹⁰ mean that the feature is deactivated. If values are specified, than the formula for the inflow velocity is:

(3.1)

where is the oscillatory inflow velocity, _in is the inflow velocity specified in the basic tab, is Oscillation Relative Velocity, Ω is the Oscillation Period and Θ is the Oscillation Phase Angle.

Unsteady Inflow Generator

• Autocorrelation Length is the spatial autocorrelation length of turbulence.
• Reynolds Stress Tensor gives the components of the Reynolds Stress Tensor.

Please note: Default values of -10¹⁰ mean that the feature is deactivated.

Lagrangian Particle Tracking

• Particle Volume Fraction gives the fraction of the volume at the inflow occupied by the particles.
• Particle Temperature can be used to specify the temperature of all the particles at that inflow.
• Particle Velocity provides the directional components of the particle velocity at the inflow.

N-Phase Algebraic Slip Model

In this tab, Volume fractions and Velocities can be defined for each phase, separately.

Velocities will only be used if the drift velocity model has been enabled (See Section Phase Average Model), otherwise they are ignored and the basic inflow velocity vector will be used.

Inflow Conditions from Data File

• Number of Points gives the number of probe locations at which data is measured.
• Coordinates File locates the file which has the co-ordinates of all the probes.
• Number of Time Instants gives the number of time instances at which the variable values are given (default value is 2).
• Time Index File has the information of the time instants for the variables.
• Read <Variable> From File checks whether to enable or disable the reading of a particular variable from the data file. If disabled, TransAT will use the value defined by the basic BC definitions.
• <Variable> File is the name of the data file for the variable.

When using inputs from data file, the probe coordinates file is compulsory. It stores the coordinates of each probe. These coordinates are given in two dimensions, the third dimension is given by the face location. Thus the y- and z-coordinates must be given for ”west/xmin” and ”east/xmax” faces, x- and z-coordinates for ”north/ymax” and ”south/ymin” faces and x- and y-coordinates for ”top/zmax” and ”bottom/zmin” faces. An example of probe coordinates file is given below:

where each line corresponds to the coordinates of one probe.

The time index file is also compulsory. It stores the time instances at which the values are given for each variables. An example of such a file is given:

Finally, the data files include values of the different variables for each probe at each time instance. It must be written by giving first the values for each probe at the first time point, then the values for the second time point.

Below is an example of a data file.

where each line corresponds to a time instance and each column corresponds to a probe.

If a data file is not found, initial values will be used as boundary conditions.

The boundary conditions will be interpolated in space and time from the data files. If the simulation time is smaller than the first time point, values of this first time point are used. In the same way, if the simulation time exceeds the last time point, values of the last time point are used. Space interpolation is performed using the four probes bordering the cell centre. If no space interpolation can be performed, the value defined by the basic BC definitions will be used.

Chemical Species

Full chemical species inputs are only available if Species and Reaction is enabled.

Depending on the components involved in the reactions, which have been defined in the Reactive Flow Modelling window (see Section 4.1.4), the user can enter the compositions based on one of the following options:

• Mass Fractions
• Mole Fractions

A typical example is shown in Fig. 3.19.

Figure 3.19: Inflow Chemical Species tab

Multiphase Flow Topology

For multiphase flow simulations with the Phase Average model activated, one of the following inflow Topology Types can be selected (By default None is selected):

• Horizontal Slug
• Vertical Slug
• Annular Flow
• Stratified Flow

For the Horizontal\Vertical Slug the following input parameters need to be specified:

• Start Time specifies the time, at which the first slug enters the domain.
• Number of Slugs specifies the total number of slugs entering the domain.
• Film Height specifies the film thickness of liquid between slugs.
• Slug Height specifies the peak height of the slug, with respect to the pipe/channel wall.
• Slug Normal Direction (Horizontal Slug only) specifies which coordinate axis is parallel to gravity.
• Slug Rise Time specifies the amount of time taken by the slug to reach its peak height (assuming a linear increase in height over time).
• Slug Peak Time specifies the amount of time spent by the slug at peak height.
• Slug Drop Time specifies the amount of time taken by the slug to drop back to the film height (assuming a linear decrease in height over time).
• Time Between Slugs specifies the time passing between two consecutive slugs.
• Bulk Film Velocity specifies the bulk velocity of the liquid film between slugs.
• Bulk Slug Velocity specifies bulk velocity of the slug while it is at peak height.
• Bulk Gas Velocity specifies the bulk velocity of the gas between slugs.
• Gas velocity at Slug specifies the bulk velocity of gas while the slug is at peak height.

Please note: Horizontal Slug flow or Vertical Slug flow is only available for unsteady simulations.

For the Annular Flow the following input parameters need to be specified:

• Film Height specifies the film thickness of the annular flow.
• Bulk Film Velocity specifies the bulk velocity of the liquid film.
• Bulk Gas Velocity specifies the bulk velocity of the gas.

For the Stratified Flow the following input parameters need to be specified:

• Height of Liquid Layer specifies the height of liquid, with respect to the pipe/channel wall.
• Bulk Film Velocity specifies the bulk velocity of the liquid layer.
• Bulk Gas Velocity specifies the bulk velocity of the gas.

For each type of multiphase flow topology a general liquid (slug) part and a general gas part is distinguished, however it is possible to freely choose the composition of each part in terms of phase volume fractions using the inputs under Film\Liquid Composition and Gas Composition. E.g. an annular inflow with liquid droplets entrapped in the bulk gas stream can be defined by specifying some volume fraction of a liquid phase under Gas Composition.

Please note: When using the TransATUI to set up a simulation, for each type of multiphase flow topology a descriptive schematic is displayed describing all parameters that need to be set.

Pump type

A pump type boundary is also available in TransAT. This is particularly useful if the user wants to define an outflow type with known fixed velocity. In order to activate it an inflow should have negative velocity defined (or negative volume/mass flow rate). For the homogeneous model mixture velocity is used to define pump discharge rate, whereas for Algebraic Slip Model both mixture or Phase Velocities can be used to do so. In both cases the void fractions for the pump boundary condition should be set to zero, since they are extrapolated from the domain side. Turbulence parameters are therefore also set based on the values from domain side, and there is no need to define them for the pump.

Please note: For a pump boundary condition the Multiphase Flow Topology option is not available.

3.8.5 Outflow boundary conditions

For outflow boundary conditions, two types of outflows are used:

• Velocity outflows behave as a non-reflective outflow. All variables will be extrapolated, using the Neumann condition

  (3.2)

  where ϕ is the solved variables and n is the direction normal to the boundary.

• In the case of Pressure outflow boundary conditions, pressure will be set to the value given by the user. The boundary behaves as a non-reflective outflow for the other variables.

General

For the Velocity outflow, no further options need to be set.

For the Pressure outflow, two options are available for the Outflow Data Source input:

• From Initial Conditions takes the pressure values initialised at the outflow boundary as boundary conditions for the rest of the simulation. This is especially useful if spatially varying pressure boundary conditions are desired, which can be set using Advanced Initial Conditions.
• From Boundary Conditions lets the user define a constant pressure value for the outflow boundary. Optionally a pressure loss coefficient ζ can be defined.

If a non-zero Pressure loss coefficient is defined TransAT will adjust the boundary pressure value p_BC during the simulation according to the following relation

(3.3)

where p_∞ is the pressure value set for Outflow Pressure, ζ is the value set for Pressure loss coefficient, ρ is the fluid density and u is the bulk outflow velocity, i.e. the average outflow velocity accounting for all the cells that are part of the same outflow.

Please note: The Pressure loss coefficient should be set only for outflows without backflow.

Backflow properties

Backflow properties should be defined for pressure outflow boundary. These are particularly:

• Backflow volume fractions used for N-phase model. If the fields are not defined (zero), then only the first phase is allowed to enter due to backflow.

• Backflow total temperature
• Backflow turbulence intensity
• Backflow eddy viscosity ratio

3.8.6 Wall boundary conditions

Wall boundary conditions usually set no-slip boundary conditions.

When the temperature equation is solved, the user can define the Temperature or Heat Flux at the wall choice.

Basic

Basic lists the essential wall values.

• Wall Velocity fixes the directional components of the wall velocity.
• Temperature/ Heat Flux choice allows the choice of two methods to set the boundary temperature.
  
  The Temperature option gives the possibility to fix a constant temperature at the wall. The temperature value should be set in Kelvin in the Temperature / Heat Flux Value field.
  
  With the Heat Flux option, the heat flux through the wall is fixed. Its value should be in W∕m² in the Temperature / Heat Flux Value
• Temperature/ Heat Flux value gives the value temperature or heat flux.
• Similarly to temperature, there are two choices of methods for concentration. Concentration/ Flux Choice allows the user to set either the concentration value at the wall or the flux of the scalar through the wall.
• Concentration/ Flux Value stores the value of the concentration or the flux.

Interface Tracking

Interface Tracking inputs are only for Level-Set model.

• Contact Angle is the angle made between the interface and the wall passing through the phase 2 (in degrees).
• A liquid Film Thickness can be specified for low Capillary Number flows where a sub-grid film always exists between the wall and the gas phase. Positive value defines a film for phase 2, negative value for phase 1. The film boundary condition does not impose a film, e.g. if a gas film BC has been defined but initially there is no gas near the wall, the film BC will not create a gas film. However, if during the simulation, gas is touching once a wall cell with gas film BC defined, a gas film will remain in this cell for the rest of the simulation.

Please note: The film thickness should be less than the grid size near the wall.

Wall Conditions from Data File

• Number of Points gives the number of probe locations at which the wall data is measured.
• Coordinates File locates the file which has the coordinates of all the wall probes.
• Number of Time Instants gives the number of time points at which the wall values are given.
• Time Index File has the information of the time instants for the wall variables.
• Read <Variable> From File checks whether to enable or disable the reading of a particular variable from the data file. If disabled values from basic wall BC definitions are used.
• <Variable> File is the name of the data file for the variable.

When using inputs from data file, the probe coordinates file is compulsory, and includes the coordinates of each probe. These coordinates are given in two dimensions, the third dimension is given by the face location. Thus the y- and z-coordinates must be given for “east/xmax” and “west/xmin” faces, x- and z-coordinates for “north/ymax” and “south/ymin” faces and x- and y-coordinates for “top/zmax” and “bottom/zmin” faces.

An example of probe coordinates file is given below:

where each line corresponds to the coordinates of one probe.

The time index file is also compulsory, and includes the time points at which the values are given for each variables. An example of such a file is given:

Finally, the data files include the value of the different variables for each probe and each time point. It must be written by giving first the values for each probe at the first time point, then the values for the second time point. Below is an example of such a data file.

where each line corresponds to a time point and each column corresponds to a probe.

If a data file is not found, initial values will be used as boundary conditions.

The boundary conditions will be interpolated in space and time from the data files. If the simulation time is smaller than the first time point, values of this first time point are used. In the same way, if the simulation time exceeds the last time point, values of the last time point are used. Space interpolation is performed using the four probes bordering the cell centre. If no space interpolation can be performed, initial values are used.

Surface Reactions

Surface Coverage provides the concentration of the catalyst (in per m²) on the surface. The higher the surface coverage, the higher the intensity of reaction.

3.8.7 Symmetry boundary conditions

The symmetry boundary condition is a slip boundary condition. Velocity normal to the boundary is set to zero, and homogeneous Dirichlet boundary conditions are applied to all the other variables ϕ:

(3.4)

where n is the direction normal to the boundary.

3.8.8 OLGA Coupling boundary conditions

An OLGA coupling boundary condition must be defined giving three different set of parameters:

• OLGA properties:
  • 1D-code filename which is the name of the file where OLGA writes the physical data corresponding to the coupling interface.
  • TransAT filename which is the name of the file where TransAT writes the physical data corresponding to the coupling interface.
  • 1D-code Boundary tag which is the tag to be defined in OLGA for reading the coupling boundary value. Typically, in OLGA, this is the tag of the position closest possible to the coupling interface.
  • 1D-code Oil Source tag which is the tag to be defined in OLGA for communicating the value of the Oil mass flux crossing the coupling interface.
  • 1D-code Gas Source tag which is the tag to be defined in OLGA for communicating the value of the Gas mass flux crossing the coupling interface.
  • 1D-code Water Source tag which is the tag to be defined in OLGA for communicating the value of the Water mass flux crossing the coupling interface.
• Geometry properties:
  • Pipe diameter defines the diameter of the pipe at the coupling interface. This has to be consistent with the OLGA definition of the pipe diameter.
  • Pipe length defines the length of the pipe as it is in OLGA.
  • Pipe roughness defines the roughness of the pipe as it is in OLGA.
  • Pipe inclination defines the inclination of the pipe as it is in OLGA.
• Coupling scheme properties(irrelevant when Learning method is selected):
  • Pressure equation tolerance The coupling algorithm needs to solve an equation involving the pressure at the boundary and the mass fluxes crossing that boundary. This is the tolerance used for the pressure–fluxes equation. The default value of 1.0e-5 is usually a good setup.
  • Outflow velocity tolerance The coupling algorithm needs to know the convergence status of the outflow velocity at the boundary, before checking the convergence of the pressure–fluxes equation. This tolerance is used for that. The value can be 0.01 (as default), or even higher in some cases.
  • Mass flux tolerance The coupling algorithm needs to know the convergence status of the fluxes at the boundary, before checking the convergence of the pressure–fluxes equation. This tolerance is used for that. The value can be 0.01 (as default), or even higher in some cases.

3.8.9 Cyclic boundary conditions

Cyclic (periodic) boundary conditions will copy the values of all variables at one boundary to the cells of the other boundary (see Fig. 3.20). Pressure forcing can be set in the Physical Models tab by activating the Periodic Conditions check-box and opening its properties window. Details about pressure forcing settings for periodic BCs are available in the section Periodic Conditions.

The settings take effect for surfaces where cyclic BCs have been set. Cyclic BCs must be assigned on all surfaces in the directions where the pressure forcing term is enabled. Cyclic BCs require careful setup and in general are applied to domains with simple geometries.

Chapter 4
Physics and Numerics Inputs

In the Input Tab, all the inputs concerning Physical Models, Phase Properties, Phase Interactions, Simulation Parameters and Output Management are defined, using the different available pages.

4.1 Physical Models

Clicking the Physical Models button enables the user to choose the equations to be solved, and the physical models to be used. A view of the Physical models page is presented in Figure 4.1.

Figure 4.1: Physical Models Page

The tab is split into five sections.

• Basic Equations enables the user to select which basic variables are solved in the simulation: pressure, temperature, concentration, velocities.
• Models and Properties enables the user to select which base models are to be used to run the simulation: Turbulence, Compressibility, Gravity and Reference Properties. Gravity is used for defining the gravity vector and Reference Properties is used for the definition of values used for non-dimensional numbers.
• Multiphase allows the user to choose advanced physical models that involve multiple phases during the simulation. These models are shown by clicking Multiphase.
• Multiphysics allows the user to choose advanced physical models that involve more physics, such as radiation or viscoelasticity. These models are shown by clicking Multiphysics.
• Additional Features provides more models and features available in TransAT. These features are shown by clicking Additional Features.

4.1.1 Basic Equations

The first thing to do is to select the equations to be solved for during the simulation. This is done in the Basic Equations section. The following equations can be selected by checking the small squares next to them (they are colored in light grey when deactivated and in orange otherwise):

• Pressure
• U velocity
• V velocity
• W velocity
• Temperature: Solving the temperature equation is equivalent to solving the energy conservation equation.
• Concentration: This solves the transport equation for a passive scalar.

4.1.2 Models and Properties

The base models are found in the Models and Properties section. These include Turbulence Modelling, Compressibility, Gravity and Reference Properties.

Turbulence Modelling

Clicking the Turbulence Modelling check-box activates a model for turbulent flows. Three families of methods are available: RANS (Reynolds-Averaged Navier Stokes), LES (Large Eddy Simulation) and V-LES (Very Large Eddy Simulation). For more information on the theories underlying these methods, the user can read the Turbulence Theory Manual, Chapters Two-Equation Turbulence Models and Scale Resolving Strategies: LES and V-LES RANS  To use a RANS model, the user should choose RANS in the Turbulence Modelling list.

Clicking opens a new window (Fig. 4.2) where the different parameters of the model can be defined.

Figure 4.2: RANS Parameters window

• the Formulation:
  - High-Reynolds number,
  - Low-Reynolds number or
  - Two-layer model
  - High-Reynolds RNG model
  (See Turbulence Theory Manual, Chapter Near-Wall Modelling for more information).
• the Wall treatment Method:
  - Standard Wall Function is available for High-Reynolds number formulation.
  - None (no treatment) is available for Low-Reynolds number formulation.
  (See the Turbulence Theory Manual, Section Near–Wall Treatment in High–Re Flows for more information).

Extensions to the basic two-equation model can be chosen if necessary. Details of the extensions are available in the Turbulence Theory Manual, Section Extensions to k - ε Turbulence Model .

• The Yap correction is active in non-equilibrium flows and tends to reduce the departure of the turbulence length scale from its local equilibrium level. The correction improved results with the k - ε model in separated flows.
• The swirl correction adjusts the turbulent eddy viscosity for strongly swirling flows because the standard k - ε models tend to overestimate turbulent diffusion for such flows.
• The compressible dilatation dissipation correction accounts for the reduction in turbulence levels at moderate to high Mach numbers.

The different k-epsilon model constants can then be set. Defaults values for σ_k, σ_ε, C_μ, C_ε,1 and C_ε,2 are the values proposed by Launder & Spalding (1974). Value for c_ε,3 is determined by the stability of flow stratification, and is between 0.8 and 1.0 for stable stratification and close to 0 for unstable ones (See the Turbulence Theory Manual, Chapter Buoyancy-Driven Turbulent Flows ).
Default Inflow Conditions values must be defined for the following properties:

• Eddy Viscosity Ratio
• Turbulence Intensity

If the value has already been defined for an inflow BC, this value will have precedence over the value defined here.
Default Wall properties may also be defined in this window. The user can define the default inflow wall roughness (default roughness at the inflow) and the wall roughness. LES  To perform a LES simulation, the user should choose LES in the Turbulence Modelling list. Clicking opens a new window (Fig. 4.3) with the available options for LES. For theory on LES, the reader is referred to the Turbulence theory manual, Section Large Eddy Simulation
The first step is to choose the Subgrid Scale Model (SGS) that must be used. The following models are available in TransAT:

• None
• Smagorinsky model. When using the Smagorinsky model, the user must give values for the constant Cs (Smagorinsky model constant).
  For more information about the Smagorinsky model and all its components, the reader is referred to the Turbulence Theory Manual, Section The Smagorinsky Model
  
• WALE model. The user may also choose to use the WALE model, described in the Turbulence Theory Manual Section, The WALE Model . The Cw value (WALE constant) is calculated automatically from the Cs (Smagorinsky model constant), please refer to Turbulence theory manual.
• Dynamic LES Dynamic model is also available in TransAT. For the theory, please refer to the Turbulence Theory Manual, Section The Dynamic Approach .

  With this model, one must choose the type of Filter Averaging to be applied (volume, plane or line), and the type of averaging for the and tensors (volume, plane or no averaging). Constraints can be then applied to the subgrid scale viscosity, namely positive local SGS viscosity or positive total SGS viscosity. Finally, a relaxation factor must be set when no averaging is applied for the and tensors. The value is very low, because the dynamic model can be very noisy when no averaging is performed.

For more information about these models, the reader is referred to the Turbulence Theory Manual, Chapter Large Eddy Simulation and Very-Large Eddy Simulation   Turbulent Prandtl number  Turbulent Prandtl number can be computed using either the Dynamic model or Kays model. It can also be set as a constant. In this case, the constant value must be given as an input. The dynamic model for the Prandtl number is only available if the dynamic subgrid model is used. For more information, the reader is referred to the Turbulence Theory Manual, Section Turbulent Prandtl Number .   Near-Wall Treatment  A Wall Force Calculation can be applied for the LES simulations. One can choose if mean velocities or instantaneous velocities should be used for the near-wall treatment. The available wall boundary type functions are:

• No slip
• Werner-Wengle wall function

For more information about these functions, the reader is referred to the Turbulence Theory Manual, Section Wall-functions in LES .

With the Smagorinsky model, one can choose a near-wall damping, using Deardorff-Werner model or the Schmidt and Schumann model. In the latter case, the constants C2inh and kappa must be given.   Other Parameters  In some cases, the flow tends to become laminar at the beginning of LES simulations. To avoid this behaviour, the user may uncheck the Recalculate Wall shear box. In this case, initial wall shear is used during all the simulation. Another possibility is to give a Recalculation interval: a value of n means that the wall shear is recalculated every n^th step.

Initial Perturbation: Checking this box will enable the initial velocity field to be perturbed using a random signal, which may enable the flow to reach the statistical steady-state faster. The amplitude of the perturbation is specified with the input variable Perturbation Amplitude, which is in m/s. V-LES  To use the V-LES model, the user should choose V-LES in the Turbulence Modelling list.

Clicking opens a new window, pretty similar to the Fig. 4.2, specific to RANS model. The only difference is that a V-LES filter width can be given, which is used to filter the k -ε equations. A lower value will make it closer to Large Eddy Simulation (although with a different subgrid model) while a large value will make the solver use standard k - ε equations.

For more information, see the Turbulence Theory Manual, Section Very-Large Eddy Simulation Concept . Turbulent Heat Flux Modelling  When solving for temperature along with the RANS turbulence model, a Turbulent Heat Flux (THF) model must be chosen. The different models and available parameters can be chosen and tuned by clicking . In the Turbulent Heat Flux properties window several models can be chosen from:

• Simple Gradient Diffusion Hypothesis (SGDH - default model)
• Generalized Gradient Diffusion Hypothesis (GGDH)
• WET Model (WET)
• Algebraic Turbulent Heat Flux Model with θ′² equation (ATHFM-kT)
• Algebraic Turbulent Heat Flux Model with θ′² and ε_θ′ equations (ATHFM-kTeT)
• Turbulent Heat Flux Model (THFM)

The models can be sorted by increasing complexity (based on the number of additional equations to be solved) as shown in Figure 4.4.

SGDH, GGDH and WET models do not require any additional equation to be solved even if the θ′² equation can be solved based on user-choice. The THFM model requires the solution of 5 equations to solve for the turbulent heat flux explicitely. A more comprehensive description of the different models and required inputs or parameters can be found in the Turbulence Theory Manual, Chapter Turbulent Heat Flux Modelling.

When any of the aforementioned models is activated, some additional simulation outputs can be chosen, namely the turbulent heat flux, the intensity of the temperature fluctuations and the dissipation rate of the temperature fluctuations.

Compressible flows

The Compressibility check-box in the Physical Models page activates the compressible solver of TransAT.

The window where compressibility parameters are set is displayed after clicking (Fig. 4.5).

The drop-down list at the top sets the Density interpolation method. First-order upwind method is more adapted to high-speed flows, while second order central method is better for low-speed flows.

The next input is the Contrast factor for Schlieren image. TransAT can output numerical Schlieren variable for compressible flow, and this factor sets the contrast resolution. Numerical Schlieren images are evaluated by

(4.1)

where κ is the contrast factor and |δρ| is the magnitude of the numerical density gradient. To enable the output of Schlieren images: go to the Output Management tab (Fig. 4.36), then click Output Variables > . This opens the Output Variables window (Fig. 4.35). Finally, check Numerical Schlieren Image.

In the window to set the compressibility model parameters The user can also set the System Pressure. Indeed, unlike incompressible solver, compressible solver must use the absolute pressure. The pressure defined at the boundaries has to be set as gauge pressure. System pressure p_s can then be used as a differential pressure: we have the equation

(4.2)

where p_absolute is the absolute pressure and p_numerical is the pressure that is used and output by TransAT.
If the user wants to output the pressure values around average numerical pressure, he can check the box Automatically adjust system pressure. With this option, the system pressure evolves with time. This is useful when one wants to track small pressure variations, for example when solving acoustic waves. Recommendations 

• For compressible simulations, it is better to use a Auto-relaxation coefficient between 0.5 and 0.77 for relaxation. Out of this interval the simulation may not converge.
• Use a pressure convergence threshold of 10^-2 or less to reduce the total number of pressure iterations.
• When the pattern of the flow is not known, using the inlet velocity as initial velocity and defining an initial pressure gradient as initial conditions may improve the stability of the first iterations.

Gravity

Activating the Gravity check-box allows for adjusting the Gravity vector. Clicking at the right of Gravity opens the gravity sub-window. This allows the user to define the components of the gravity vector. Its components must be given in S.I. units. When gravity is non-zero, the Hydrostatic pressure source term will be automatically enabled for multiphase flows.

Reference Properties

Reference Properties can be activated with the check-box. Clicking at the right opens the reference properties sub-window. Reference values for different variables can be defined:

• Reference Pressure
• Reference Temperature
• Reference Velocity
• Reference Length

With the exception of the reference temperature, which is used when the Boussinesq approximation is applied (section 4.2.7), these values are not used for numerical simulations, only for evaluating the non-dimensional numbers of the simulations and for post-processing. All the values are given in S.I. units.

When the user does not provide a reference value for a property, a default value is automatically set. In the case of the reference length, the automatic default value is -1. Then a length scale is automatically computed from the simulation files at the beginning of any simulation. This automatic value will be used only if no user value has been specified. A message is displayed when launching a simulation which summarizes the different length scales and specifies which one will be used. The automatic length scale is computed as the minimum of:

• the size of the domain
• the maximum distance observed from a cell to a wall (if applicable)
• the maximum distance from a solid cell to the immersed interface (if applicable, gives an estimate of the solid length scale)
• the maximum distance from a fluid cell to the immersed interface (if applicable, gives an estimate of the fluid length scale)

Reference Concentration is also available. It is used to determine the buoyancy effects when solving the concentration of a scalar.

4.1.3 Multiphase

By default on opening TransAT, the Multiphase models will be displayed. If this is not the case, clicking Multiphase will display these models. The models available in the Multiphase section includes Interface Tracking, Phase Average, Phase Change, and Lagrangian Particle Tracking.

Interface Tracking

The check-box Interface Tracking enables using an Interface Tracking Method (Level Set). The user should first activate the Interface Tracking check-box then click to define the parameters of the model. More information is available in the Multiphase Theory Manual, Section The Level Set Method for Level-Set and The VOF methodology for Volume Of Fluid (VOF). Please note: when using a multiphase flow method, initial conditions must be defined for the interface or for the initial volume fractions. See Section Creating Initial Conditions to define initial conditions. Level Set Method  The more feature-rich interface tracking method in TransAT is the Level Set method. The window where its properties are set is shown in Fig. 4.6

Figure 4.6: Level Set properties window

• Interface Width Factor is the ratio between the minimum cell size and the width of the interface.
• H smooth is the type of function to be used in the smooth interface region for defining the proportion of gas and liquid. Choices are tanh (use of a hyperbolic tangent function), linear or sharp (Sharp interface).
• Delta Type is the method used to calculate the Dirac delta function at the interface. It is expressed as the norm of the gradient of the H smooth function. Analytical uses the analytical expression, while Discrete uses discretised differential operators.
• LS Narrowband: If this option is selected, the Level Set function is updated only in a region around the interface, instead of the whole domain.
• Implicit Treatment of Surface Tension: For surface tension dominated flows, typically small-scale flows, the time step restriction arising due to explicit treatment of the surface tension source is too severe. This is combined with the issue of parasitic velocities, which finally results in a low effective CFL condition and the solution proceeding very slowly. The implicit curvature treatment reduces the parasitic currents by a significant amount resulting in larger effective CFL numbers. The method proposed by Hysing (2006) has been implemented and can be turned on by checking the corresponding box. This method allows the surface tension time step criterion (See Section Control Parameters) to be set as high as:

  Surface Tension	Min = 5.0	Max=10.0

  
  
  For the explicit treatment, the maximum surface tension criterion should be kept lower than 1.0.
  
  Please note: For BMR grids the implicit surface tension treatment will be automatically disabled.
• Dynamic Contact Angle Model

  TransAT has both static and dynamic contact angle modelling capabilities. The equilibrium contact angle can be defined in the current window. If the dynamic contact angle model is deactivated, the value of the equilibrium contact angle will be used as static contact angle. To specify different values for each wall boundary, please refer to the Boundary conditions section. The maximum contact angle that can be specified is 170^∘ and the minimum is 10^∘. This limit is imposed due to the way the contact angle boundary condition is implemented. For situations very close to fully wetting or fully non–wetting, the thin film boundary condition can be used, see Section Wall Boundary Conditions.
  
  To activate the dynamic contact angle, check the Dynamic Contact Angle Model checkbox. Output Dynamic Contact Angle can be selected to output the diagnostic file for contact angle (RESULT/dyn_contact_angle.dat).
  
  For more information about these methods, the reader is referred to the Multiphase Theory Manual, Section The Level Set Method .

• Interfacial eddy viscosity damping: When using the k -ε model, turbulent viscosity can be damped in the interface region. Indeed, turbulent viscosity is usually over-estimated in this region, which results in a damping of the surface movements. Available methods are none, delete, smoothsign and cubic which suppress turbulent viscosity at the interface.
• Surface Tension defines the surface tension between Phase 1 and Phase 2.

• To insert bubbles, click . This will open the bubble generator window.

In the Bubble Table the relevant parameters of the bubbles, such as the position and the time where they should appear, are stored.

• Click below the Bubble Table to create a new bubble, then set the time at which it should appear, its radius and the coordinates of its center.

TransAT will automatically modify the level-set field to add this bubble when the nucleation time is reached.

A second table, Mdot Table is present in this window. It allows for defining regions with different rates of phase change. This is available only when the phase change correlation is set to fixed (see Multiphase Theory Manual, Section Phase Change Modelling ).

• Click below the Mdot Table to define a new region.

The first column stores the mdot value that must be assigned to this region, and the next columns store the parameters to locate the boundary of the regions.   Marangoni Model  The Marangoni model enables a temperature-dependent surface-tension model. One must specify the temperature T weber at which the reference surface tension (as defined in the Level Set Properties window) is given and the temperature at which surface tension is zero (T crit). For more information, see Multiphase Theory Manual, Section Marangoni Effect .   Redistancing 

• Redistancing Method. The methods available for reinitialisation of the Level Set functions are:
  - WENO
  - Fast Marching 1st order
  - Fast Marching 2nd order
  For more information about these methods, the reader is referred to the Equations and Algorithms Manual, Section The Level Set Method .
• Redistancing Steps is the maximum number of cycles to be performed for Level Set function reinitialisation.
• Mass conservation: Two methods are available for mass conservation with Level Set, a Local method and a Global method. For more information, see the Equations and Algorithms Manual, Section The Level Set Method . Option Local + Global will use both methods.
• Cmin and Cmax are the minimum and maximum values for the mass conservation coefficient.

• Level-Set method can be activated only for unsteady simulations.
• Initial value of the Level-Set function must be defined using initialconditions.cxx or initialconditions.xml. If the distance to the interface is not known everywhere, the user may give an arbitrary positive or negative value (to define the phase) and use the Redistance Level Set function of the initial conditions page (See Section Initial Conditions Input).
• When the ratio between density of the phases is high, it is advised to use First-Order Euler scheme. (See Section Numerical Schemes).

Figure 4.7: VOF properties window

• Use the VOF method only for unsteady simulations.

Phase Average

The check-box Phase Average enables using the Homogeneous model or Algebraic Slip model (ASM). The user should first activate the Phase Average check-box then click to define the parameters of the model. The Algebraic Slip model adds Drift Velocities to the Homogeneous model. More information is available in the Multiphase Theory Manual, Section Phase-Average Multiphase Flow Modelling for the Homogeneous model and ASM.

Please note: when using a multiphase flow method, initial conditions must be defined for the initial volume fractions. See Section Creating Initial Conditions to define initial conditions.

Homogeneous Model   
To enable the Homogeneous model,

• Select Homogeneous in the Phase Average drop-down menu.

With this model, up to ten different phases can be modelled.

• Click to open the dedicated window to set the Homogeneous model parameters Fig. 4.8.

A turbulent dispersion term can be added, which adds to the drift velocity a term due to turbulence. This term allows for a better description of mixing for turbulent flows.

Please note: The turbulent dispersion term is only available when turbulence is being modelled. Additionally, it is enabled by default if turbulence modelling is activated.

For more information on the Phase Average Mixture Model, please refer to the Multiphase Theory Manual, Section Phase-Average Mixture Models

Suspension viscosity model can be turned on in order to modify the viscosity of the mixture as an effect of the phase volume fractions. The user has to give the state of each phase of the mixture. Suspension viscosity model has then to be defined for each type of dispersed phases: bubbles, droplets and/or particles. Choices are as follows:

• Averaged (only for bubbles and droplets) means that a default volume fraction based averaging is used for mixture viscosity computation.
• None (only for particles) means that the impact of dispersed phase on viscosity is not taken into account.
• Ishii-Zuber
• Hydrates enables the hydrate rheology if hydrates model is enabled.
• Mooney (only for particles)
• Mills (only for particles)

The Maximum packing volume fraction must also be given, which is the maximum volume fraction that can be occupied by the particles phase, For more information, see the Multiphase Theory Manual Mixture viscosity .

ASM Model   
An extension to the homogeneous model is the algebraic slip model. To enable ASM,

• Select Algebraic Slip Model in the Phase Average drop-down menu.

The window as in Fig. 4.9 is used to set the general parameters for ASM. Some of the parameters are the same as in the homogeneous model (turbulent dispersion and suspension viscosity model). By choosing the algebraic slip model, drift velocities will be activated which will make the velocities of the phases different from each other. Drift velocity will then be computed as a function of the pressure gradient. This can be set in the Pressure gradient approximation drop-down menu. If Hydrostatic is selected instead, the pressure gradient is computed by ρg, allowing for faster computations.

For ASM, drag, lift and wall lubrication models need to be defined. These models are chosen within the Phases Interactions tab, Momentum Transfer section. Refer to 4.3.1 for information about defining the interphase slip models. Examples of the interphase slip models include; drag models of stokes, clift, tomiyama and schiller; lift models of auton and tomiyama; and wall lubrication models of antal, frank, hosokawa and tomiyama. The slip models are described in the Multiphase Theory Manual, Section Algebraic Slip Model .

Phase Change Modelling

This section describes the Phase change modelling capabilities of TransAT. Phase change modelling is turned on by clicking the corresponding check-box. Currently, phase change is available with Level-Set and Phase-Average multiphase models.

Clicking opens the Phase Change Parameters window.

Please note: The options displayed in the Phase Change Parameters window depend on the type of Multiphase Flow Method selected (i.e. Level-Set or Phase Average).

For the Level-Set method (Fig. 4.10) the following phase change correlations are available:

• None: the mass transfer rate ṁ is directly calculated from the energy/temperature equation. Values for Latent Heat and Saturation temperature must be given by the user.
• Fixed: the value of ṁ should be specified in the input file via the variable Rate in SI units . Moreover, it must be set whether evaporation or condensation occurs using the Phase Change list.
• Hiemenz, Lim wavy and Lim smooth are global correlations for phase Change. They are explained in the Multiphase Theory Manual, section Phase change modelling . Values for Latent Heat and Saturation temperature must be given by the user, as well as velocity and length scales for gas and liquid phases.
• Interface Mass Transfer models are local correlations for phase change, explained in the Multiphase Theory Manual, section Phase change modelling . Values for Latent Heat and Saturation temperature must be given by the user. The type of interface mass transfer model must also be selected, as well as the way of computing the turbulent Reynolds number and the reference phase to compute it.

Curvature correction of saturation temperature will adjust the saturation temperature as a function of liquid-gas curvature and surface tension (available only for Level-Set).

Meniscus model accounts for heat transfer near the triple point (solid-liquid-gas point). It can only be used when the Correlation is set to none.


When using the Phase Average multiphase model, the following options are available (Fig. 4.11):

Please note: With the Phase Average model, phase change occurs between phase 1 and 2 only. This means that if the phase change model is activated, the state of the first two phases must be Liquid and Gas.

Please note: With the Phase Average model, wall phase change will not be applied for immersed surfaces of conjugate objects.

The Latent Heat Method input offers two options for the value of the latent heat:

• constant: a value needs to be specified
• variable: in this case a scrolling list appear at the botton of the window and the user must choose between the available materials (water and ammonia).

The Thermally Limited Phase Change option is available only if solving for Temperature. It contains the following entries:

• Dispersed phase Nusselt correlation: possible options are Ranz-Marshall or None. Refer to the Multiphase Theory Manual, section Dispersed-phase phase change for more details.
• Interfacial Shear HTC (heat transfer coefficient) model: possible options are Banerjee model or None.
• Interfacial diffusion HTC model: Schrage, Relaxation and None are the possible options.
• Tsat method: two options are possible: either Constant or Variable. In the first case a value must be entered, in the latter a saturation curve must be defined. See 4.1.3 below for details about saturation curve.
• Activate wall boiling model with or without Condensation Inside.
  • Deactivate Condensation Inside turns condensation ON or OFF in the bulk of the flow in the scenario of Subcooled Boiling Flows.

The Inertial Phase Change / Cavitation model section is available for both compressible and incompressible flows. Two cavitation models are available:

• Sauer correlation: the two model parameters nucleate density and minimum radius must be given. Refer to the Multiphase Theory Manual, section Sauer cavitation model for more details.
• Singhal correlation: can only be used if Turbulence Modelling is activated. Refer to the Multiphase Theory Manual, section Singhal cavitation model for more details

The Psat method can either be

• Constant: a value needs to be entered
• Variable: a saturation curve must be defined. See 4.1.3 below for details about saturation curve.

For more information on Phase change models, please refer to the Multiphase Theory Manual, sections Phase change modelling (for Level-Set method) and Phase change in the bulk (for Phase Average method).

Saturation Curve  The saturation curve is defined within the Phase Properties. Phase 1 and 2 will have a Saturation Curve method available to choose from. This allows pre-defined curves from Ammonia or Water. Also, the Antoine equation is available, with the corresponding A, B and C model parameters. If using the Antoine equation, model parameters for various materials can be found in literature or reference material. The saturation curve for phase 1 and 2 must be the same (i.e. same Antoine model parameters, or defined from the same phase). More information about defining the Saturation Curve is available in the Phase Properties section 4.2.14.

Lagrangian Particle Tracking

It can be used by selecting the Lagrangian Particle Tracking Model in the Physical Model tab. The particle positions and velocities are updated at each time step in conjunction with the carrier flow field which evolves in time. Particle Tracking theory is available in the Multiphase Theory Manual, Chapter Particle Tracking Models . Properties  Here is a list of available parameters that can be set by the user in the Properties tab of the Lagrangian Particle Tracking window.

• Particle density: density of particle material.
• Heat Capacity: heat capacity of particle material.
• Thermal Conductivity: thermal conductivity capacity of particle material.
• Computational ratio: decides how many particles are computationally tracked as compared to the real number of particles dictated by the volume fraction. This factor is important only for two-way coupled cases. It is an integer ≥ 1.
• Volume fraction: Total initial volume fraction occupied by particles.
• Number of particle size bins: number of particle diameter groups
• Diameter Discretization : the distribution of diameters between minimum and maximum diameters (Linear or Logarithmic law).
• Diameters: Minimum and maximum particle diameters
• The parameter Size PDF Function decides how the number of particles in each size group is computed. The option Constant Mass divides the total volume fraction equally for each group resulting in less particles in the large size groups. Constant NP results in equal number of particles in each group, and the Log normal distribution option uses the standard log-normal distribution Apte et al. (2003).

  (4.3)

  where d_p⁺ = d_p∕(d_p^max - d_p), and D_nm⁺ = D_nm∕(d_p^max - D_nm) are the normalised particle diameters , d_p^max is the upper limit of particle diameter(Log Normal Dmax), D_nm the mean (Log Normal Dmean), σ₀ the standard deviation (Log Normal Sigma), and a₀ a factor used to normalise the distribution.

• Momentum Coupling: Particle-fluid coupling (One-way or Two-way).
• Two-way Coupling: provides two ways in which the fluid-particle interaction force is distributed back to the fluid grid. When it is set to Particles in Cell the force on each particle is distributed to the cell in which the particle is located. When set to Sundaram Sundaram & Collins (1999) the force is put back on to all the nodes which formed the interpolation stencil to obtain the fluid velocity at the particle position.
• Hold Particles Fixed: do not move particles
• Strong F-P Coupling: recalculate fluid-particle force inside implicit iterations
• Solve Temperature: solve for particle temperature
• Solve Angular Velocity: solve for the angular velocity of particles
• Dense Particles Method: account for non-dilute particle suspension
• Volume Fraction Method: method to calculate volume fraction of particles
• Particle Sources: introduce particle sources

• Drag force, with Shiller-Naumann or Clift Gauvin Model.
• Max. Particle Re denotes the maximum particle Reynolds number that is allowed by the user. If at any time a particle acquires a higher value the program is stopped. This is based on the limitations imposed by the equations governing the particle motion.
• Buoyancy force
• Lift force with Auton or Saffman Model. For Auton model, the Lift Coefficient must be given.
• Added-mass force
• Fluid force
• Basset force Please note: This module is currently deactivated.
• Thermophoresis Please note: This module is currently deactivated.
• Axisymmetric Swirl Please note: This module is currently deactivated.
• Convective heat transfer
• Magnus lift force for the angular velocity model.
• Shear Torque for the angular velocity model.
• Collision pressure model can be used using Snider (2001) or Johnson & Jackson (1987) model. For both of these models, the close packing volume fraction and particle restitution must be given.
• Langevin particle dispersion model can be applied. The user must give the Intensity factor and fluid time scale factor for this model
• Approximate deconvolution for LES of particle-laden flows.

Please note: The forces that are to be included are to be explicitly chosen by the user based on the relevant physics of the problem at hand. None of the forces are hard-wired. For example, in the case of bubbles it is left to the user to turn on the added-mass force. Numerical  The Interpolation method is the order of interpolation to evaluate the fluids properties, such as velocity, temperature, …at the location of the particle.

The Time integration provides methods to solve the particle variables such as velocity, position, temperature, angular velocity. Time stepping control is the method of controlling the time step: fluid CFL number or response time can be used.

The parameter Response time factor is used to return the maximum allowable time-step from the particle side. The smallest particle response time (τ_p,min) is multiplied by this value to arrive at the maximal time-step. Response time factor can be as high as 0.9 for 4^th order Runge-Kutta time integration and should be maintained below 0.4 for the Adams-Bashforth and 2^nd order Runge-Kutta methods. Initialise  In Initial Particle Location, the user can define the initial position of particles as the intersection of Primary and Secondary Volumes.

The parameter Random Series with the option fixed allows repeatability when using random numbers (to initialise the particle positions). The geometrical properties of these volumes has then to be defined.

In this intersection, the Particle Distribution can then be defined. If it is random, defining the Random series as fixed, allows repeatability when using random numbers to initialise the particle positions. Changing Random seed changes the random distribution for fixed random series.

In the panel Initial Variable Values, checking Velocity equilibrium will initialise particle velocity equal to the fluid velocity. Otherwise, Mean velocity and RMS velocity must be given.

Temperature equilibrium uses fluid temperature as initial particle temperature. If it is not checked, Initial temperature can be defined for particles.

Angular velocity equilibrium uses fluid angular velocity as initial particle angular velocity. If it is not checked, Initial angular velocity can be defined for particles.

Read particle data from file initialises particles with parameters defined in read_particle.ini. Each line represents the set of parameters used to initialise a particle. The set of parameters that must be defined are:

• the time of particle initialisation t_init,p
• the particle diameter d
• the particle initial position (x_p,y_p,z_p)
• the particle initial velocity (u_p,v_p,w_p)
• the particle initial temperature T_p (when solving for particle temperature only)

read_particle.ini should be formatted as such:

Example

In the following example, two particles with the following parameters are initialised through read_particle.ini:

Particle 1

• t_init,p = 0.0s
• d = 0.5mm
• (x_p,y_p,z_p) = (2.0,0.0,0.0)m
• (u_p,y_p,z_p) = (0.0,0.0,1.0)m.s^-1
• T_p = 300K

Particle 2

• t_init,p = 5.2s
• d = 1mm
• (x_p,y_p,z_p) = (0.0,3.0,1.0)m
• (u_p,y_p,z_p) = (0.5,0.5,0.0)m.s^-1
• T_p = 350K

The corresponding read_particle.ini file consists of the following lines:

Particle 1 will be initialised at the beginning of the simulation (t = 0s). Particle 2 will be added at the specified location with the specified properties after the simulation has reached a time of t = 5.2s. Particles with negative time values will be initialised at the beginning of the simulation. Boundary Conditions  The Wall interaction defines the behaviour of particles when they hit a wall. They can be Reflected or Absorbed. Wall friction coefficient and coefficient of restitution can also be given.

Symmetry interaction defines the behaviour of particles when they hit a symmetry boundary, in the same way as for a wall. Particles can be Reflected or Absorbed.

Particle Inflow Type is used for inflow condition. If Per cell is selected, particle volume fraction for the inflow will be verified for each cell. With Per boundary, only the average for the boundary will be verified, and volume fraction can vary from cell to cell.

The parameter Random Series with the option fixed allows repeatability when using random distribution of particles for boundary conditions. Changing Random seed changes the random distribution for fixed random series. Output  In Variables for Output, Particle Step defines the ratio between simulated particles and output particles. If the value is more than 1, Random Output enables one to select particles randomly.
The particles variables to be output have then to be defined.

The following options can be selected:

• Write Old Velocity: writes the particle velocity at the previous time step.
• Write Particle cell: writes the cell that contains the particle.
• Write Fluid Velocity at Particle Position: writes the velocity of the surrounding fluid interpolated onto the particle position.
• Write Particle Temperature: writes the particle temperature.
• Write Particle Rotation: writes the particle rotational velocity.
• Write Particle Torque: writes the particle torque.

Finally, Post Processing provides several outputs to be written as functions of time during simulations.

• Store collision data: logs all collision events of particles with a wall boundary or an embedded interface and writes corresponding information to the file collision_data.dat in the RESULT folder of the simulation.
• Store particles leaving: stores information for each particle that is leaving the domain through any permeable boundary (time, diameter, position and velocity) and writes it to the particles_leaving.dat in the RESULT folder of the simulation.

Please note: The format of the particles_leaving.dat file written by selecting the Store particles leaving postprocessing option is compatible with the feature Read particle data from file in the Initialise tab. These files can be used for example to simulate the transition of particles into an adjacent domain

4.1.4 Multiphysics

The Multiphysics section of the Physical Models contains more physics models. Clicking Multiphysics will show these available models. The Multiphysics models include the Species and Reaction, the Hydrate Model, the Radiation Model and the Viscoelasticity Model.

Reactive Flow Modelling

Activating the reactive flow solver of TransAT is done by checking the box Species and Reaction. The window for the model properties (Fig. 4.12) opens after clicking .

Please note: As of TransAT version 5.7 the surface and porous interface reaction modules are deprecated and not available anymore in TransATUI.

The Cantera library can be used with TransAT to evaluate material properties and import complex reaction mechanisms. If the Cantera database is used an input file (cantera_input.cti) has to be in the working directory. The syntax of the Cantera input file is described in the section Cantera Input File document Cantera_Input_Manual. Theory for reactive flow modelling is available in the Equations & Algorithms Handbook, Chapter Reactive Flow Modelling

The definition of a reaction in a mixture consists in three main steps:

• setting the general parameters for reactive flows
• defining the components with their properties
• defining the reactions

The mixture contains the species O2, H2, H2O which contain the elements H and O. The elements always have to be the element name in uppercase letters because some data (e.g. molar weights) are directly linked to these elements. The term gri30 in front of the species names indicates that the thermodynamic data and the transport properties are imported from the gri30 (gri30.xml) mechanism.

Note that species can be imported from any mechanism that is present in the folder
transatMB/properties_database/cantera_data in the xml format.

The transport keyword defines the transport manager used for the transport properties. The mixture transport model is the appropriate model to be used with TransAT. To define the reaction add:

The terms in square brackets specify the Arrhenius reaction constant ([“pre-exponential factor”,“temperature exponent”, “Activation Energy”]).

Several sample input files are present in the aforementioned folder cantera_data.

  Diffusion Model  The simplest model is to use the same coefficient for all species: set the Diffusion Model to Constant, and set the constant value of the Diffusion Coefficient.

A more accurate model available is the mixture model. The mixture model can only be used in conjunction with Cantera. The diffusion coefficient of species k is evaluated under the assumption that all other species have equal diffusion velocity. This leads to a mixture diffusion coefficient D_km for every species. As unequal diffusion coefficients do not guarantee conservation of mass (the mass weighted diffusion velocities do not sum to zero), a correction has to be applied to ensure mass conservation. This can be done by constraining one species, which is particularly convenient when one species is always in excess (see Solve constrained component).   Define the components and their properties  The components can be added by clicking the button below the Components table. A new line will appear in the component table where one can enter the component name in the first column and specify the molar weight in the second column. By default the properties of the mixture are constant and set in the Phase Properties window.   Define the Reactions  Having defined all the components the next step is to define the reactions. Note that only simple homogeneous reactions can be defined with TransATUI. Homogeneous reactions with a more complex reaction rate expression such as pressure-dependent reactions can only be specified in the Cantera input file. To learn how to define reactions in the Cantera input file refer to the document Cantera_Input_Manual.

If the Cantera database is used (i.e activation of Cantera Database), all the reactions have to be defined in the Cantera input file.

To define a new reaction,

• Click the button below the reaction table which opens the Reaction Creator window (Fig. 4.13).
• In Reaction Creator window, click to add reactants and products in the bottom left corner of the corresponding frame.
• Use the drop-down menu in the Name column to choose the reactant/product from the list of components.
• Fill in the Stoichiometric Coefficient and the Reaction Order in the corresponding columns.
  Note that the default value for Reaction Order is -1, meaning that the Reaction Order is equal to the Stoichiometric Coefficient.
• For volumetric reactions with the reaction model Mass Action Kinetics, the reaction rate coefficients have to be provided (Temperature Exponent, Pre-exponential Factor, Activation Energy).
• If Cantera Database is switched off and Activate Chemical Heat Source is activated the Reaction Enthalpy has to be specified. If Cantera Database is activated, the reaction enthalpy will be calculated automatically from the enthalpies of the components.
• Once all the parameters are set, click to save the settings and close the Reaction Creator window.

The reaction definition should now appear in the Reaction column.

Figure 4.13: Reaction Creator Window

To delete a component or a reaction, check the delete check-box at the lines corresponding to the items to be removed then click below the table.

Reactions can also be edited by clicking edit at the corresponding lines in the list of reactions.

Hydrate Model

The Hydrate Model can be used to define interactions between phases. Activating Hydrate Model will allow the user to edit the Phase Interactions. In order to activate the Hydrate Model, Phase Average needs to be activated with at least three phases. More information can be found in the Phase Interactions section.

Radiation

This section describes the Radiation modelling in TransAT. Radiation is activated by clicking on the checkbox adjacent to it.

There is one option only: Rosseland model.

In the Phase Properties, the user can enter the coefficients for all phases and specify the different radiation bands to be taken into account. For a particular band, a separate set of coefficients can be entered, making the formulation flexible to accurately calculate the Rosseland Extinction Coefficient.

Note that solving for the temperature equation is required to activate the radiation model, and that for multiphase problems, the homogeneous or Algebraic Slip models have to be used, whereas it is not possible to use the level-set model.

Viscoelasticity

This section describes the viscoelasticity modelling capabilities in TransAT. Viscoelasticity is activated by clicking on the checkbox adjacent to it.

There are several model options to choose from: Oldroyd-B., linear PTT and exponential PTT. The model choice will determine the complexity of the modelling and the number of model parameters required. In addition, the user must specify the number of viscoelastic modes considered in the problem, and specify if the LCT formulation (Logarithm of Conformation Method) is to be used.

In the Phase Properties, the user can enter the model parameters for each phase and each viscoelastic mode, by selecting Non-Newtonian in the viscosity method, and Viscoelasticity in the drop-down lists. Depending on the choice of the model, the following model parameters may be required:

• the elastic relaxation time λ (all models)
• the polymeric viscosity μ_p (all models)
• ϵ (PTT models)
• ξ (PTT models)

In addition, it is possible to include a temperature dependence of the polymeric viscosity to the temperature by activating the Arrhenius Tmperature Dependence model.

4.1.5 Additional Features

contains supplementary geometric and physical models. The Additional Features include Axisymmetry, Vibrating Body Force, Point Sources, 1-D Coupling, and Rotating Reference Frame.

Axisymmetry

Axisymmetric flows can be solved for with TransAT by checking the Axisymmetry check-box.

In axisymmetric setups, cylindrical coordinates are used instead of Cartesian ones. Note that axisymmetric simulations are limited to the x-y plane, with y representing the radial component and x the axial component. The axis of symmetry is defined at the line y = 0 (and therefore along the x-axis).

For more information, please report to the Equations and Algorithms Manual, Section Axisymmetry .

Vibrating Body Force

An oscillating force can be applied with TransAT by using the Vibrating Body Force capability. To apply an oscillating force,

• Check Vibrating Body Force then click to open the window where the body force parameters are set (Fig. 4.14).
• The following parameters can be set in that window
  • The Frequency of the oscillation (in Hz)
  • The Phase of the oscillation (in deg)
  • The Amplitude of the displacement (in m)
  • The coordinates of the point where the oscillating force is to be applied
  • The Start Time and End Time for the application of the body force.
• Click to save the settings and close the Body Force Properties window

Periodic Conditions

When cyclic boundary conditions are used, a pressure source term can be added. This is done in the Periodic conditions panel (Fig. 4.15). To apply pressure forcing to cyclic BCs,

• Check Periodic Conditions
• Then click to open the window
• From the first choice, choose whether to define the superficial velocity or pressure gradient
• Choose which phase(s) to define pressure forcing for (if multiple phases)
• Define parameters in the X, Y or Z directions

A choice drop-down can choose between defining a superficial velocity or pressure gradient. Next, a spinner shows for which phase to set a velocity or pressure gradient. It is therefore possible to have a different magnitude and direction of pressure forcing for each phase.

Superficial velocity specifies a bulk velocity in the fluid domain, i.e. the space-average velocity over the whole fluid domain. It is not possible to define a velocity profile. However, a fully developed flow will naturally occur from periodicity during a transient phase early in the simulation. This profile is dependent on the geometry for the flow.

If defining pressure gradient instead of the superficial velocity the pressure source term is directly set. The user must define the components of the source term in the desired directions.

The settings take effect for surfaces where cyclic BCs have been set. Cyclic BCs must be assigned on all surfaces in the directions where the pressure forcing term is enabled. Cyclic BCs require careful setup and in general are applied to domains with simple geometries. To assign cyclic boundary conditions to surfaces the reader is referred to Assigning a boundary condition to a surface.

Point sources

Point sources can be positioned in the domain by activating the Point sources. After activating Point sources, the icon will appear.

To create point sources and set their parameters

• Click opens a window where you can define point source for mass, momentum, heat or concentration.
• In the window that popped up, click to create a point source.

To define a point source, the following parameters need to be set:

• Coordinates of the point (X coor, Y coor, Z coor)
• Start Time and End Time are the times at which the point source is activated and deactivated.
• Other values, depending on the type of the source, must be defined. When a mass source is created, the velocity and temperature at which the phase is injected must be defined.

Also note that a point source can be deleted by clicking Delete at the end of the corresponding line in the point source table.

Coupling modelling

The Coupling modelling of TransAT can be enabled by clicking the corresponding check-box. The coupled code has to be chosen among the list:

• OLGA (supported version is 7.2)

When coupling modelling is enabled, next the coupling parameters need to be set.

• Click to open the Coupling Model properties window.

The coupling algorithm parameters are listed as follows:

• Shared location folder defines the location of the folder where the coupling data is written.
• Learning method determines which method to be applied for computing a new pressure guess. If it is checked, history points are taken into account to predict the pressure value, otherwise the pressure constraint method is employed.
• Number of history points is shown only when Learning method is checked. It defines how many history points are involved in the learning method.
• Max global number of iteration factor is shown only when Learning method is unchecked. It defines the factor for internal coupling boundary pressure iterations. A value of 5 is usually a good trade-off between simulation-speed and stability of the coupling model.
• Time stepping coupling tolerance defines the tolerance when the two solvers read the data of the other solver. The default value of 1.0e-5 was found to give good results.
• TransAT oil phase index defines the numbering of the oil phase defined in Phase Properties.
• TransAT gas phase index defines the numbering of the gas phase defined in Phase Properties.
• TransAT water phase index defines the numbering of the water phase defined in Phase Properties.

The exclusive parameters for OLGA(Fig. 4.16) are listed as follows:

• Module name is the name of the module specified in OLGA.
• Model name is the name of the model specified in OLGA.
• Time step can be forced to be in a specific range compared to TransAT time step. If the 1D-code is freely allowed to choose its own time-step, regardless what it chosen by TransAT, the coupling model can become unstable. A good suggestion is to take the 1D-code time step being in the range [0.5 - 2] * TransAT time step.

Rotating Reference Frame

A rotating reference frame can be defined with TransAT by checking the Rotating reference frame check-box.

Opening the properties window for defining a rotating reference frame, inputs are available to define the center of rotation as well as the angular velocities for the rotation. The angular velocity is defined in radians per second. After clicking to save and close the settings, the rotating reference frame will be applied once the simulation is executed.

4.2 Phase Properties

When clicking the Phase Properties button, the Phase Properties page is opened, as shown in Fig. 4.17.

Figure 4.17: Phase Properties

The properties of the phases are defined in that page. It is separated in two sub-windows:

• A catalog of phase properties, represented within a tree structure, as shown in Fig. 4.19
• The sheet related to the item chosen on the catalog, as shown in Fig. 4.18

The sheet provides input boxes to enter in values of the various properties. The catolog gives an overview of all the phases and properties per phase. By default, the tree is collapsed, but can be expanded by clicking on the plus box per item in the tree.

Figure 4.18: Sheet

4.2.1 Material Library

The user can enter pre-defined properties using the catalog displayed for each phase on the sheet, as shown in Fig. 4.20

4.2.2 Density

For incompressible simulations, a fixed density can be defined for each fluid. For a compressible setup, an equation of state can be chosen for defining the density. For more details on the equation of state and possible settings refer to section 4.2.11.

4.2.3 Viscosity

Assuming that the simulation solves for velocity, viscosity can be defined through several methods. A fixed viscosity can be defined by choosing a constant viscosity for a fluid. For a temperature dependent viscosity, the curve fit option can be selected. For more details on defining viscosity in this manner, refer to section 4.2.8. Another possibility is to define viscosity by Sutherland’s Law, which is described in section 4.2.9. Or, fluids can be set as Non Newtonian, through various methods such as Bingham, a Power Law, Carreau or others. Viscosity through Non-Newtonian models are described in section 4.2.10.

4.2.4 Temperature related fluid properties

For simulations that solve for temperature, corresponding properties need to be defined for the fluid. These include thermal conductivity, thermal expansion, and heat capacity. Each of these can be set with a fixed value. Thermal conductivity can instead be defined by curve fit method or Sutherland’s Law. For heat capacity, curve-fit method is the only additional method available.

4.2.5 Concentration Diffusivity

Solving for a passive scalar (activated by concentration, under equations), it is necessary to define a diffusivity. For multiple phases, the diffusivity can be defined uniquely for each phase.

4.2.6 Species Diffusivity

Additional to Concentration, TransAT can also add species to a simulation for reactions. These species also need a value for the diffusivity. Unlike concentration, multiphase simulations are not possible with species. For species defined in a simulation, the diffusivity is defined by the transporting fluid, i.e. the only phase in the Phase Properties tab.

4.2.7 Boussinesq Approximation

The Boussinesq approximation can be used to solve natural convection problems without having to solve the full compressible Navier-Stokes equations. The Boussinesq approximation is applied in TransAT by setting the value of the thermal expansion coefficient for each phase and the reference temperature in the reference properties under Physical Models (see also section 4.1.2).
Please note: The Boussinesq approximation only affects the gravity term in the Navier Stokes equation and will have no effect on any other terms.

4.2.8 Curve-Fit

Viscosity, heat capacity or thermal conductivity can be defined by the user as a function of the temperature. To do this, the curve fit method must first be selected in the drop-down list next to the corresponding property. The file defining the property as a function of the temperature must then be selected. To select the file with the temperature-dependent values of the physical properties, click >.

The data file should be in the project folder. Its format is as follows:

where the first column gives the temperatures and the second column gives the corresponding value of the property. At least two rows must be present. Hermite interpolation method (cited in Sarfraz (2003)) will then be used. If the data available in the file shows a monotonic behaviour, the method proposed by Sarfraz (2003) is used to keep monotonicity.

If temperature lies outside the temperature range given in the file, the property will have the same value as the one given for the lowest or highest temperature.

4.2.9 Sutherland Law

The user may also choose to apply Sutherland’s law for viscosity or thermal conductivity, instead of setting a constant value for this quantity, by checking the corresponding check-box. Parameters for this model become accessible by this action. The following properties can be modified:

• The reference viscosity or thermal conductivity
• The reference temperature
• The Sutherland temperature

Sutherland’s law is described in the Equations and Algorithms Manual, Section Sutherland’s Law .

4.2.10 Non Newtonian Fluid

In Non-Newtonian fluids, the viscosity, defined by the ratio of stress-to-strain, is not a constant anymore. A Non-Newtonian model can be used in TransAT to take this behaviour into account. To do so, Non-Newtonian needs to be selected in the viscosity model drop-down list next to the viscosity label. Non-Newtonian models can be selected in the new drop-down list will be displayed to the right of the viscosity model drop-down list.

The following models are currently available:

• Bingham: adapted to plastic materials.
• Casson: adapted to plastic materials.
• Power Law: for pseudoplastic or dilatant fluids.
• Carreau: for polymeric liquids.
• Cross: for generalized fluids that behave as Newtonian fluids at low shear rates and follow a power law at higher shear rates.
• Carreau-Yesuda: for polymers.
• Thixotropic Flows: for fluids with time-dependent rheology like clays, drilling muds, etc...
• Hershel Bulkley: generic three-parameter model.

When choosing a model, the corresponding constants that must be set appear in the panel. All these models are presented in the Algorithms Handbook, Chapter Non-Newtonian Models .
Note that non-Newtonian models are implemented per phase.

4.2.11 Compressible Flows

For compressible flow models, the Equation of state (EOS) of the fluids has to be specified. Several choices are possible:

1. The Perfect Gas EOS is adapted for gas. Ratio of specific heats γ must be given, as well as the Molecular Weight and the Heat capacity C_p in the Phase Properties page (See Fig. 4.17).
2. The Stiffened Gas EOS is adapted for a liquid. Ratio of specific heats γ, cohesion pressure p_∞ and heat capacity C_p in the Fluid Properties page (See Fig. 4.17) become parameters to define the fluid density. The fluid will behave as a perfect gas at a pressure of p_∞.
3. The Tait Water equation has been specifically designed for liquid water.
4. The Tait Ammonia equation has been specifically designed for liquid ammonia.
5. The Incompressible option enables a user to have an incompressible phase (constant density). This is useful for mixtures where a phase is compressible but not the other.
6. Peng-Robinson enables the use of the generic Peng-Robinson equation of state, where by the user can specify Acentric Factor, Volume Translation, Critical Pressure and Critical Temperature. Typical inputs for various materials can be found in reference literature.
7. For pre-defined Peng-Robinson parameters, the Peng-Robinson-Water equation of state for liquid or vapour -water can be enabled.

TransAT also offers the possibility to calculate the Heat Capacity of a phase using the selected equation of state (this option is not accessible if the selected equation of state is Incompressible). To use this option the entry Eq. of State must be chosen in the drop-down list of the Heat Capacity property.

Note that the Ideal Gas, Stiffened Gas and Incompressible equations of state are general in the sense that a user-input is required. The Tait equation of state for ammonia or water is specific as all the numerical parameters are pre-entered in TransAT.
The user can also select the option Resolution of pressure waves. When this option is turned on, pressure wave velocities are taken into account when calculating the CFL criterion. This enables TransAT to capture acoustic waves. Note that the timestep Δt will be much lower when this option is activated. This option is not accessible if the selected equation of state is Incompressible.

For more information on the equations, models and algorithms for compressible flow, the reader is referred to the Equations and Algorithms Manual, section Equations of State .

4.2.12 Radiation Rosseland model

If Radiation is activated, then the inputs for the Rosseland model have to be specified for each phase. This is done in the Rosseland properties window as shown in Fig. 4.21

The inputs required from the user are the Refraction Index of the phase and the Rosseland Coefficients. TransAT’s radiation model uses the extinction coefficient to calculate the radiative component of the heat transfer, and the Rosseland model allows the user to give either a constant value of the extinction coefficient (this is when the a0 coefficient is non-zero, and a1 ... a5 are zero) or a polynomial fit (up to fourth order) to take the temperature dependence of the extinction coefficient into account. In addition, it is also possible to take into account the dependence of the extinction coefficient on the wavelength. This is done using the definition of Radiation Bands. Each band corresponds to an interval between two wavelengths where the Rosseland coefficients a0 ... a5 can be defined. At least 1 and up to 10 bands are allowed in TransAT.

For each new band, the maximum wavelength of the band must be provided (in meters). The first band always starts at 0, and the last one will go up to infinity by default (when the maximum wavelength is defined as -1). Bands must be defined in increasing order of the maximum wavelength.

4.2.13 Viscoelastic model

If Viscoelasticity is activated, then the inputs for the different models have to be specified for each phase. This is done in the viscoelasticity properties window as shown in Fig. 4.22

The inputs required from the user are the values of the model parameters and the temperature dependence for each phase.

4.2.14 Phase Change

For simulations including Phase Change between two phases, it is possible to define the saturation curve between the phases, based on pre-defined phases (available is either Ammonia or Water), or based on the Antoine equation.

To define the saturation curves from the Phase Properties, set the Tsat method or Psat method to variable while defining Phase Change settings under the Physical Models, before changing Phase Properties.

4.3 Phase Interactions

Interactions between phases are defined in the Phases Interactions tab. Momentum Transfer is used to define phase interactions (drag, lift and wall lubrication) for the algebraic slip model (ASM). In Hydrate Reactions a hydrate formation and dissociation model is available.

4.3.1 Momentum Transfer

When ASM is activated for the Phase Average, Momentum Transfer between phases becomes available. This is necessary for the proper definition of miscibility, drag, lift and wall lubrication. Before these relations are defined, it is first necessary to ensure that the state of each phase is correctly set to the desired solid, liquid or gas, in the Phase Properties tab, because the momentum transfer mechanisms depend on this. After setting the state of each phase, the phase interaction will be automatically initialized to the recommended models for each pair of phases.

Please note: Modifying the State of Phase input in the Phase Properties tab, resets all Interphase Slip Relations. Please make sure that state of phases are set correctly, before modifying the phase interaction tables.

The Momentum Transfer section of TransAT is shown in Fig. 4.23. the drop-down choice below the title ”Interphase Slip Relations” can be used to switch between each of the six parameters (miscibility, drag, lift, wall lubrication, lift coefficient and surface tension). The default table displayed on opening the Phases Interactions is the Miscibility table.

Each of the tables is setup in a similar fashion, with each row representing a dispersed phase and each column representing a continuous phase. For example in Fig. 4.23, five phases have been defined: two liquids, two gases and a solid. The row and column labels are each displayed with the name set for each phase from the Phase Properties tab. Notice also, that the row labels are given with the proper dispersed phase characteristic (bubble/drop/particle), versus the continuous phases which are labeled as either gas, liquid or solid.

Miscibility Table

Fig. 4.23 shows the Miscibility table, where miscibility is displayed and defined. If two phases are miscible, the ASM will not calculate a slip between them and their respective phase velocities are equal. The majority of relations within the table are not available to be set by the user; miscibility can only be defined for liquid-liquid interactions, thus miscibility is not available to be set by the user for other state of phase combinations. When phases are of a different state (e.g. gas-liquid, liquid-solid, etc.) the phases are by default immiscible with each other. The implemented slip model does not consider direct gas-gas or solid-solid interactions, thus these relations are displayed as ”N/A”. Shown in the example for the five phases, the liquids have been set to be miscible with each other.

Some conditions on miscibility include reciprocity and consistency between phases. If one phase is miscible in a second, then the second is also miscible in the first. Therefore, the miscibility table will be symmetric. Miscibility must also be consistent between a group of phases. Given three phases, if the first and second phases are miscible, and the second and third phases are miscible, then the first and third phases must also be miscible. Breaking this consistency between groups will display a warning and prevent a simulation from running.

Drag Model Table

The definition of the drag model between phases is available by selecting Drag Model in the Interphase Slip Relations drop-down menu. The table for defining drag models has a similar structure as the miscibility table. Rows define the dispersed phase and columns define the continuous phase. The drag table is shown in Fig. 4.24 for the example setup.

Possible drag models to choose from include Stokes, Clift, Tomiyama Contaminated, Tomiyama Slightly Contaminated, Tomiyama Pure and Schiller relations. The various Tomiyama relations were empirically determined for bubbles in liquids, as such these models are unavailable for other state of phase pairs. Tomiyama models also refer to the conditions of the liquid, for example, pure refers to a liquid that has been distilled several times to remove impurities. A contaminated liquid would not have been distilled, and a slightly contaminated liquid is inbetween a contaminated and pure liquid. Choosing a drag model from the table is shown in Fig.4.24

There are certain phase interactions where drag relations are not permitted. This includes miscible phases, and solids as the continuous phase. Miscible phases do not have a slip and no drag is applied between them. When the solid is the continuous phase, fluids become trapped inside and there is no drag relation possible.

Lift Model Table and Coefficient

The definition of the lift model between phases is available by selecting Lift Model in the Interphase Slip Relations drop-down menu. The usage and restrictions of the lift model table are analogous to the drag model table. Possible models to choose from are either Auton or Tomiyama. Tomiyama is again only valid for gas bubbles dispersed in a liquid. For miscible phases, and solids as the continuous phase, there is no slip and a lift model cannot be applied. The auton lift model requires a coefficient to be defined. This is accomplished by choosing Lift Coefficient in the Interphase Slip Relations drop-down menu. In the lift coefficient table, the lift coefficient can only be set for phase interactions where Auton was defined as the lift model.

Wall Lubrication

The definition of the wall lubrication model between phases is available by selecting Wall Lubrication Model in the Interphase Slip Relations drop-down menu. Wall lubrication is a model only applied to bubbles in a liquid, so the choice of model is only available for corresponding pairs of phases. Models to choose from are Antal, Frank, Hosokawa and Tomiyama.

Surface Tension

The definition of surface tension between phases is available by selecting Surface Tension in the Interphase Slip Relations drop-down menu. Surface tension is required for Frank, Hosokawa, and all Tomiyama models. If one of these models has been selected within any of the model tables, then an input for surface tension becomes available in the surface tension table. Surface tension must be given a value greater than zero.

4.3.2 Hydrate Properties

Please note: The Hydrate Reactions can only be activated when Phase Average is chosen as Multiphase Flow method, with at least three phases defined given that water, hydrocarbon and hydrate phases are needed to simulate hydrate formation.

The parameters that can be set in the Phase Properties tab are the following:

• Hydrate Reactions. The choice is between Bishnoi and infinite. These model are explained in the Multiphase Theory Manual, Section Hydrates modelling .
• Water Phase: defines the phase which corresponds to the water phase, according to your definition in the Phase Properties tab. Please note: This input is compulsory, as previously said. Moreover, the phase selected for this input cannot be used in any other input in the Hydrate Reactions, e.g. in the hydrate phase definition. If the input is not correctly set, an error message will be displayed in red.
• Methanol Phase: defines the phase which corresponds to the methanol phase, according to your definition in the Phase Properties tab. Please note: This input is not compulsory: the selection can remain empty, but it must be defined uniquely.
• Margins to thermodynamic equilibrium: defines the temperature limits for hydrate reactions. In the range between the above equilibrium and below equilibrium, there are no hydrate reactions.

Please note: the model is built such that the user is not allowed to assign the same phase defined in Phase Properties tab to different inputs of the hydrate model. For instance “Phase1” cannot be the hydrate model water phase and the hydrate model methanol phase at the same time. The same is true for the hydrate phases and for the hydrocarbons phases to be defined in the hydrate reactions. Red error messages of “incompatible values” will be displayed if there is a conflict in the hydrate models inputs.

In fact, many hydrate reactions can then be defined in the same simulation. One can add a hydrate reaction by clicking .

To modify a hydrate reaction click edit at the corresponding line.

For deletion of hydrate reactions, click the delete check-boxes of the reactions to be deleted in the hydrate reaction table then click .

Hydrate Reaction

When adding a hydrate reaction, a sub-window Hydrate Reaction Creator will open. The parameters to be set in this window are the following:

• Hydrate: defines the phase that corresponds to the hydrate phase, according to your definition in the Phase Properties tab.
  Please note: The Hydrate input is compulsory. Moreover, the phase chosen cannot be used in any other inputs in the hydrate model.
• Hydrocarbons material: Available materials are:
  • Methane
  • Ethane
  • Propane
  • Isobutane
• Hydrate formation enthalpy: is the heat released for the formation, in Joule.
• Hydration number: is the number of molecules of water for each molecule of hydrocarbon needed for hydrate formation).

The user can then select one or several hydrocarbon phases from which hydrate will form, and one of the forming phases can be selected as dissociation phase.

One can add a hydrocarbon by clicking .

For deletion of hydrocarbons, click the delete check-boxes of the hydrocarbons to be deleted in the hydrocarbons table then click .

For information on hydrate formation and dissociation models, please refer to the Multiphase Theory Manual, Section Hydrates modelling .

4.4 Simulation Parameters

The page Simulation Parameters can be accessed by clicking the button of the same name (Fig. 4.25). This is where the numerics are set. The page is divided in three different sections:

• Simulation Type. In that section, the user can choose between a steady simulation, in which case the equations are solved to steady-state without taking into account the time terms, and unsteady simulation.
• Control Parameters. In that section, the user can specify more detailed parameters depending on the simulation type chosen.
  Please note: Advanced Options in the middle of the window shows all the options for this section.
• Equations Parameters. The user can specify different solver parameters for each of the equation solved by TransAT.
  Please note: Solver Options at the bottom of the page shows all the options for the equations which can be selected in the equation tree to the left. The set of equations is split into Pressure and Other Variables).

Figure 4.25: Simulation Parameters tab

4.4.1 Control parameters

In this section, one defines the control parameters of the simulation. Most of them depend on the Simulation Type specified, as described in the following sections.

Steady Simulation Control Parameters

When running a steady simulation, the Number of Iterations must be defined. It corresponds to the maximum number of iterations to be performed if convergence thresholds are not reached. If the simulation reaches this number of iterations, it is automatically stopped.

For the definition of convergence criteria, see Section Convergence Parameters.

Unsteady Simulation Control Parameters

• Total simulation time defines the maximum time that is simulated. The simulation stops when this time is reached.
  Please note: Start time is 0s.
• Max Number of Time Steps is the maximum number of time-steps performed in an unsteady simulation. It is always useful to fix a maximum number of time-step, so that the simulation stops even if the total simulation time has not yet been reached.
• Initial time step defines the time-step for the first iteration. If adaptive time stepping is enabled, TransAT will automatically calculate a time step which satisfies the stability limits and replace the given time step if too large.
• Max Number of iterations per Time Step defines the maximum number of iterations to be performed within a time-step, if the convergence threshold is not reached for all the variables.
• Time Stepping strategy is available to choose from. If Fixed is selected, the time-step will be the same during the entire simulation, and is defined by the Initial Time Step value. If Adaptive is chosen, lower and upper bounds for the following non dimensional parameters must be given:
  • CFL number is a convection parameter, defined by

    (4.4)

    It should be noted that the CFL bounds are also used as bounds for the Gravity and Phase-Change non-dimensional numbers:

    (4.5)

    (4.6)

  • Diffusion is a non-dimensional number which takes into account diffusion phenomena. It is expressed as

    (4.7)

    where μ_eff includes material viscosity plus turbulent viscosity or other modifications to local viscosity.

  • Surface Tension non-dimensional number is defined by

    (4.8)

    where δ^I is the interfacial Dirac Delta function, and n_i is the normal to the interface. This expression is obtained by deriving a surface tension based velocity . (See also Section Level Set Method)

  • Fourier non-dimensional number is in relation with thermal phenomena. It reads

    (4.9)

  • Fluid Particle Force criterion is related to Lagrangian particles tracking. It reads

    (4.10)

    where f_pf is the particle-fluid force, α_p is the particle volume fraction and Δx is the cell size.

  • Chemical Reaction criterion is applied when mixture reaction is enabled. The criterion is defined as

    (4.11)

    where _i is the source term due to chemical reactions applied on component i, and Y _i is the mass fraction of this component.

Other Control Parameters

Regardless of the Simulation Type, two more options can be specified:

• the Autorelaxation button can be checked to set the relaxation factor for all equations at once. Lower relaxation parameters mean a more stable simulation, but also a larger number of iterations before convergence.
  If Autorelaxation is not used, under-relaxation parameters must be set directly for all the equations that will be solved. This is done in the Equations section.
  The effect of the relaxation number is described in the Equations and Algorithms Manual, Section Final form of discretised equations .
• the Pressure-velocity coupling scheme can also be chosen. TransAT currently proposes the Simple and SimpleC procedures. For more details about these procedures or about the pressure solvers, see the Equations and Algorithms Manuals, Section Pressure-Velocity Coupling .

SArP (Smart Adaptive run Parametrisation)

The SArP module is a controller for simulation convergence. The SArP module may stabilise a simulation and optimise numerical parameters of a simulation to make it converge faster. These objectives are achieved by tuning:

• adaptive time-stepping inputs for unsteady simulations
• Autorelaxation
• numerical parameters of the solvers (except Convergence Tolerance and Relative Solver Tolerance) defined in the Equations section of the Simulation Parameters tab

The whole set of these numerical parameters is referred as Chromosome in the present document and in TransATUI. Likewise, every individual parameter from the numerical parameter set is referred as a Gene.

The SArP module has two modes which are depicted in Figure 6.1 and Figure 6.2:

• Optimisation: call to the SArP module from the start of the simulation to optimise parameters
• Stability: call to the SArP module when convergence issues are detected

When triggered, the SArP module automatically sets the numerical parameters by means of an optimising and learning iterative process (genetic algorithm).

The SArP module can be activated by checking the SArP check-box. The corresponding mode is set accordingly to the entry selected in the drop-down menu. SArP triggers
 
In stability mode, the SArP module can be triggered if either one of the following issues are encountered while running a simulation:

• Residuals are not decreasing over a window of iterations (steady simulations) or at a specific time step (unsteady simulation)
• Solver of an equation does not converge for several consecutive unconverged iterations
• The rate of unconverged iterations over a window of iterations (steady simulations) or other a time step (unsteady simulations) is too high
• Slope of time step duration is decreasing (only for unsteady simulations)
• Time step becomes too small (only for unsteady simulations)
• A jump in the residuals is detected

Note that in optimisation mode, SArP is triggered right from the beginning of the simulation. After the first execution the SArP module remains activated in stability mode to monitor the convergence of the simulation. SArP Advanced Parameters
 
By clicking , the advanced parameters of the SArP module can be accessed as shown in Figure 4.28. The advanced parameters are classified into two sections corresponding to the two main features of SArP, namely a Monitoring section and a Correction and Optimisation section.

The Monitoring section has one subsection where non-convergence of a simulation is set. The Correction and Optimisation section has 4 different subsections:

• Main Algorithm Properties
• Convergence
• Genetic Operations
• Fitness Approximation

Monitoring  The Monitoring section contains the parameters of the convergence monitoring feature of SArP.

Convergence is monitored over an analysis window whose size can be set in the Analysis Window Size field. This parameter is used in several settings of the monitoring and correction features of SArP which will be expanded on in the next paragraphs.

The Residual Analysis Window Size field is only available for steady simulations. This field specifies the window over which the residuals must be decreasing overall.

Please note: if residuals fluctuate, low values of Residual Analysis Window Size may result in triggering the correction module of SArP too often hence slowing down the simulation. Using higher values of Residual Analysis Window Size avoids this potential issue. However it may delay the triggering of the correction module.   Non-convergence Thresholds  The non-convergence thresholds are the set of thresholds that are used to define the convergence quality of a simulation. They are based on residuals, iteration convergence and time steps. The set of non-convergence thresholds is the following:

• Consecutive Unconverged Iterations: number of equation-wise consecutive unconverged iterations above which the simulation is deemed non-converging
• Unconverged Iteration Rate rate of unconverged iterations over analysis window (steady) or time step (unsteady) above which the simulation is deemed non-converging
• Max. Residual Ratio: ratio of residuals between current iteration and previous iteration above which the simulation is deemed non-converging
• Unconverged Time Steps: (unsteady only) number of consecutive non-converged time steps above which the simulation is deemed non-converging
• Min. Time Step: (unsteady only) time step value below which the simulation is deemed non-converging
• Min. Time Step Drop Factor: (unsteady only) value of the ratio between the time step value at the end of the analysis window and the time step value at the beginning of the analysis window below which the simulation is deemed non-converging

Figure 4.29: Genetic Algorithm Process

• Configuration: pre-defined settings of the correction module
• Evaluations Per Generation: number of fitness evaluations to be performed at every generation
• Max. Generations: maximum number of generations to be evaluated at every call of the correction module
• Max. Parallel Fitness Evaluations: number of fitness evaluations to be performed in parallel
• Max. Genetic Algorithm Runs: maximum number of times the correction module may be run during one simulation
• Enable Roll-Back: perform the correction before the last time step/ iteration where the non-convergence of the simulation was verified

Two pre-defined configurations can be selected in the Configuration drop-down menu: the fast configuration and the normal configuration. Fitness Evaluations Per Generation, Max. Generations and Analysis Window Size are greater with the normal configuration. With this configuration, the space of the parameters is more thoroughly explored. This may lead to better convergence of the genetic algorithm and make the computational cost of the SArP module higher.

An evaluation or fitness evaluation consists of a simulation run from the point where the correction module is triggered. The simulation is run over a number of iterations/time steps corresponding to Analysis Window Size. A steady simulation evaluation is illustrated in Figure 6.9.

The Enable Roll-Back option for an unsteady simulation is depicted in Figure 4.31. The principle is exactly the same for steady simulations. As shown in Figure 4.31, the Enable Roll-Back option runs some preliminary steps before correcting numerical parameters:

1. restart simulation using the latest restart backup file
2. stop simulation before the time step/iteration where convergence issues have been detected
3. launch the SArP module from that point

The offset is determined depending on the detected convergence issue. Depending on the value of the offset, the simulation may be restarted from an earlier point than the backup restart file.

Please note: the frequency of restart backup file can be set in the Output Management sub-tab by the modifying the Frequency of Restart Backup entry.

  Convergence  This subsection contains the convergence criteria of the correction module which are the following:

• Stagnating Generations: number of consecutive generations with a stagnating best solution
• Residual Drop Factor: (steady only) value of the ratio between residuals at the end of the analysis window and the maximum residual at the beginning of the analysis window

• Altered Inputs Proportion: Proportion of numerical parameters to be changed from one generation to another
• Input Variability: rate at which numerical parameter may vary from one generation to another
• Selection Operator: operator for the selection of the best solution

The Selection Operator may be one of the following:

• elitism
• roulette
• tournament
• nsga2
• spea2

More information can be found on the selection operators in the SArP section of the TransAT Algorithms Handbook .   Fitness Approximation  Approximation of the optimal set of parameters can be activated by checking the Fitness Approximation check-box and selecting the corresponding Learning Method in the drop-down list. The approximation method can be one of the following:

• bagging
• decision trees
• extra trees
• random forest

When Fitness Approximation is activated, the number of evaluation is divided by 2 from the second generations onwards. Five other sets of parameters are evaluated using the learning fitness approximation algorithm.

More information can be found on the learning methods in the SArP section of the TransAT Algorithms Handbook .

4.4.2 Equations

In the bottom part of the Simulation Parameters tab, the equations properties are shown. On the left, the available equations can be selected (depending on the setting in the Physical Models tab).

Equations are divided into subgroups. Clicking the Solver Options check-box at the bottom of the page, will expand Other Variables into different subgroups, depending on the models used and on the basic equations solved for.

Multiple selection is allowed using Ctrl + left click. Moreover, when selecting a tree node (symbolised with a folder in the equation tree), all its subnodes are automatically selected. This is done in order to facilitate applying changes to similar equations. If you want to unselect one or more subnodes, just use Ctrl + left click again on these subnodes.

Whenever the user does a selection on a node, the corresponding equation properties are shown on the right. When using multiple selections, a warning symbol is displayed for the inputs for which there is a conflict of values.

Please note: the conflict of values for an input simply means that every input is not the same for all the equations that have been selected.

In order to apply changes on one of the parameters on the right, e.g. the Convergence Tolerance, the user must first select the equations in the tree, then change the desired value on the right.

Please note: If one wants to apply the same parameters to all the equations, the root node All Quantities can just be selected. With All Quantities selected, all the parameters modification will be applied to all the equations.

Please note: The same parameters can be set for all the equations except for the pressure equation. For the pressure equation has the same parameters as the other equation except the Convection Scheme option which is not available for it.

All the Equation Parameters on the right of the Equations panel are described in detail in the following section.

Equation Parameters

Here, a full description of the equation parameters is given.

• Convection Scheme: the convection schemes available in TransAT are
  • Hybrid: 1^st order central/upwind scheme
  • Quick: 3^rd order unbounded scheme
  • Central: 2^nd order accuracy
  • HLPA: 2^nd order bounded scheme

  Note that not all the convection schemes are available for each equation. For more information on the convection scheme, the reader is referred to the Equations and Algorithms Manual, Section Approximation of convection terms

• Convergence Tolerance: it fixes the convergence threshold for each equation.
  • For steady implicit simulations, the convergence parameter for Other Equations is suggested to be set at 10^-6 or below, and the convergence parameter for Pressure should be set at 10^-2 or below.
  • For unsteady simulations, it is recommended to use 10^-2 for all the equation convergence parameters.
• Relaxation: if Autorelaxation is not selected in the Control Parameters section, then a different relaxation value can be chosen for each equation by setting the value of Relaxation.
• Solver: the solver can be selected among the following:
  • GMRES Generalized Minimal RESidual method
  • SIP Stone’s Implicit Procedure
  • BiCG Biconjugate gradient method
  • BiCGSTAB Biconjugate gradient stabilized method
  • AMG R-cycle, adaptive
  • AMG R-cycle, geometric
  • AMG F-cycle, adaptive
  • AMG F-cycle, geometric
  • AMG W-cycle, adaptive
  • AMG W-cycle, geometric
  • AMG V-cycle, adaptive
  • AMG V-cycle, geometric

  The AMG solvers can be run in different modes (geometric/adaptive) and with different cycles (V/W/F/R). Adaptive is more expensive than geometric but it can result in a faster convergence for difficult problems, the same is true for the cycle type (from simple to complex: V/W/F/R-cycle). For instance, for simple grids and single phase flows it is recommended to select V-/W-cycle, geometric, same for compressible flows. F-/R-cycle, adaptive are recommended for incompressible multiphase problems or complex grids.

• Preconditioner: it sets a preconditioner for the solver with the aim of accelerating convergence. Available preconditioners are
  • Jacobi
  • Block Jacobi
  • ILU: Incomplete LU factorization
  • AMG: Algebraic Multigrid
  • AMG cluster: Algebraic Multigrid configured for distributed memory machines like clusters.
  • Additive Schwarz

  Please note: the Preconditioner option is available only when the selected solver is GMRES or BiCG or BiCGSTAB. Moreover, AMG, AMG cluster and Additive Schwarz are available only when GMRES solver is chosen.

• Subpreconditioner: a subpreconditioner can also be selected, depending on the solver and on the preconditioner. Possible options are:
  • None
  • Jacobi
  • ILU

  Please note: Subpreconditioners are available only when Block Jacobi or Additive Schwarz preconditioner is selected.

• Max Number of Solver Iterations: for all types of solvers, the maximum number of iterations when solving a linear system can be defined. This value defines the maximum number of inner cycles to be performed by the solver if it does not manage to converge. This will not affect the solver for the other variables.
• BMR Iterations: this defines the number of coupling iterations between BMR grid levels. Please note: It is recommended to use a value of 5 for all the equations except for the pressure equation, for which it is suggested to use 10.
• Relative Solver Tolerance: this parameter defines the relative target tolerance for solving the linear system of the equation per inner iteration. A value range between 10^-2 and 10^-3 is recommended.
• Normalised Residue: the activation of this option normalises the residues of the solutions with respect to the residues at the first iteration.
• Relax Linear System: if activated, the linear system is first relaxed and then solved (Patankar relaxation), otherwise the system is solved unrelaxed.

4.5 Initial Conditions

In the Initial Conditions tab (see Fig. 4.32), initial conditions can be set for variables to be solved for. Simple initial conditions can be set here, along with advanced initial conditions. Variables defined with advanced initial conditions will overwrite any basic initial conditions defined. Basic initial conditions not overwritten will still be used together with advanced initial conditions.

4.5.1 Methods

Basic initial interfaces with the interface-tracking method can be defined in initialconditions.xml. Please refer to the User-defined Initial Conditions section. For more complex initial conditions, please refer to the Advanced Initial Conditions section.

The basic set of initial conditions that can be set in the Initial Conditions tab comprises the following methods:

• Automatic
• Constant
• Userdefined

For velocity components, the Automatic option consists in making the initial velocity field divergence-free if the fluid is incompressible.
For pressure the Automatic option consists in setting the initial pressure field based on the source terms.

Note that the default Method for all variables is Automatic.

When Method is set to Constant for a variable, the variable field is initialised with a constant value throughout the domain. The value that is used is the one given in the Value field.

When Method is set to Userdefined for a variable, the variable field needs to be specified directly in the initialconditions.xml file created by TransATUI.

Please note: an extra input, Sub Method, is available for the phase variables when the Constant method is chosen and the Species and Reactions option is activated in the Physical Model tab. The Sub Method option allows the user to specify either mass or mole fractions for initial values of the species variables.

Please note: the Userdefined method can only be set by editing initialconditions.xml by hand.

Please note: the values set using Advanced Initial Conditions overwrite the basic values set in the Initial Conditions tab.

4.5.2 Variable tree

In the tree on the left, the available variables can be selected (depending on the models enabled in the Physical Models tab). The variables in the tree are divided into subgroups.

Multiple selection is allowed using Ctrl + left click or by dragging the mouse. Moreover, when selecting a tree node (symbolised with a folder in the variable tree), all its subnodes are automatically selected. This is done in order to facilitate applying changes to one set of variables in one go. If you want to unselect one or more subnodes, just use Ctrl + left click again on these subnodes.

4.5.3 Setting parameters

Whenever a user selects a node, the corresponding initial conditions parameters are shown on the right. When using multiple selections, a warning symbol is displayed for the inputs for which there is a conflict of values. The warning symbol is displayed in orange for the Method and Value inputs. It is displayed in red for the Sub Method input.

Please note: the conflict of values for an input simply means that the value for that very input is not the same for all the variables that have been selected.

In order to apply changes on one of the parameters on the right, e.g. the Method, the user must first select the variables in the tree, then change the desired value and sub-method (if available) on the right.

Please note: If one wants to apply the same parameters to all the variables, the root node All Quantities can just be selected. With All Quantities selected, all the parameter modifications will be applied to all the variables.

Figure 4.32: Initial Conditions tab

4.5.4 File structure

All the information relevant to the parameters of the Initial Conditions tab are written in the file initialconditions.xml.

4.5.5 Advanced Initial Conditions

The user can set more advanced initial conditions using the C++ interface to TransAT’s code. The method to do so consists in creating a C++ subroutine, called initialconditions.cxx.

Advanced initial conditions are introduced in more details in the Advanced initial conditions section.

If variables are to be initialised using advanced initial condtions

• Put/copy the file initialconditions.cxx in the project folder if available
• Open the project with TransATUI if that is not already the case
• In the sub-tab Initial Conditions of the Inputs main-tab, select the Advanced Initial Conditions.
• The initialconditions.cxx can be opened with an editor from here. If there is not initialconditions file in the project folder, a template will be copied. After editing the initialconditions, save and close the file.
• Click to test that the file can be compiled (without initializing flow conditions)
• Setup the remaining inputs for the simulation.
• Once in the Execute window, click to initialize the ICs from initialconditions.cxx

4.6 User Defined Functions

In the User Defined Functions tab (see Fig. 4.33), user defined functions (UDFs) can be defined. A brief description of how to define UDFs is given in this section, for greater detail and explanation of UDFs refer to the User-Defined Functions section.

4.6.1 Creating UDFs

Click on the button to define a new UDF. A window will open to define the basic features of the UDF. First a name for the UDF must be defined. This name must be a valid C++ file name (no special characters and cannot begin with a number). The UDF name, file name and class name must all be the same.

After defining the UDF name, a type must be selected. The types of UDFs are organized with templates. By choosing a template, the UDF will be set with the same type (the type is shown by the folder that the template is in). If a template is not desired, the choice ”None” can be selected, which exists within each folder. This is helpful if the file for the UDF already exists in the usercompile folder, to prevent it from being overwritten.

Once finished defining the UDF, click to create the UDF. If a template was selected, the implementation (.cxx) and header (.h) files will be copied from the installation directory into the usercompile folder of the project directory. The UDF can be edited by clicking the button.

A UDF can be removed by clicking . This will not delete any of the files, but prevent it from being compiled or used during a simulation. Only the UDFs activated in the table of the User Defined Functions tab will be compiled and executed. When a UDF is not desired during a certain run, it can be deactivated using the checkbox, there is no need to delete it from the table.

4.6.2 Compiling and Executing UDFs

To test that a UDF was written properly, click the button. This will compile UDFs activated by the orange check-box. The text output at the bottom of the tab will display the results of compilation. An error will display if UDFs failed to compile.

Activated UDFs are compiled automatically at the start of a simulation. This will ensure that changes to a UDF file will be included.

Please note: UDFs regarding drag models, lift models, and wall lubrication models require additional steps in order to be executed. Refer to Extended UDF Types for more information.

Figure 4.33: User Defined Functions tab

4.7 Output Management

The last page of the Input Tab revolves around Output Management and Post-Processing (Fig. 4.36). It is divided into three sections:

• Visualization Files sets the parameters for visualization files
• Post-Processing defines some post-processing outputs.
• Restart Parameters sets the parameters for reading/writing restart files.

4.7.1 Visualization Files

The output of the visualization files and of the restart/backup files are controlled in the Output Management tab.

Output File Format input sets the output format for visualization. Two visualization formats are supported by TransAT: Tecplot files, and vtk file format, which is the standard format for Paraview. The default option for Paraview is point-data. For further information, please refer to the Paraview User Manual.

Frequency of output files sets the interval at which visualization files are saved: a value of n means that visualization files are written every n^th iteration/timestep. For unsteady simulation the output frequency can also be set based on time interval. These files are stored in the RESULT subfolder of the project folder.

In the file names, xxxx represents the iteration/time-step index, and ext is the file extension, namely dat for Tecplot files and vtm for Paraview files.

The second part of the tab deals with extra parameters for the visualization files.

These extra parameters are the following:

• Averaging If this option is selected, some variables are averaged over time and written into files. These variables are listed in the Statistics group of Output Variables (note that this group is greyed out unless the Averaging box is checked)

  Clicking opens a dialog window (Fig. 4.34) to set up the following parameters:

  • Time Step to Start Averaging Before this time step, it is considered that the system has not reached statistical steady-state, and values are not taken into account.
  • Sampling Interval determines the number of time steps between samples: a value of 1 means that each time step is taken into account, whereas a value of 10 means that 9 time steps out of 10 are skipped.

  ---

  
  

  Figure 4.34: Averaging

  ---

• Geometric Series Output: The output is written every 2ⁿ timestep / iteration until it reaches the iteration number reaches the frequency output.

Managing which variables are written in the output files is done in the Output Variables dialog window, which opens by clicking Output Variables.

Choice of Output Variables

Clicking Output Variables opens the Output Variables window (Fig. 4.35). The variables are grouped for better readability. Primary Variables Group
  The Primary Variables group is always activated.

• Pressure: P in the visualization file.
• U-Velocity: U in the visualization file.
• V-Velocity: V in the visualization file.
• W-Velocity: W in the visualization file.
• Temperature: T in the visualization file.
• Concentration: C in the visualization file. This gives the concentration of a passive scalar, or the particle volume fraction for settling models.

• Density: DEN in the visualization file.
• Viscosity: VISC in the visualization file. This is the Dynamic viscosity
• Heat Capacity: Cp in the visualization file.
• Thermal Conductivity: Lambda in the visualization file.

In this group of variables, only Density and Viscosity are always activated. Heat Capacity and Thermal Conductivity are activated only if temperature is solved for. Geometry Group
 

• Wall Distance: WallDistance in the visualization file.
• Solid Step Function: HEmbI in the visualization file.

In this group, only Wall Distance is always activated. Solid Step Function is activated only if Immersed Surfaces in Objects is enabled. Miscellaneous Group
  The variables of the Miscellaneous group are available only if Compressibility is activated in the Models and Properties section of the Input tab.

• Mach Number: MACH in the visualization file. Only for compressible flows.
• Speed of Sound: SOUNDSPEED in the visualization file. Only for compressible flows. The speed of sound depends on the equation of state that is used to model the fluids. See the Equations & Algorithms theory manual, Section Equations of state for more details.
• Numerical Schlieren Image: SCHLIEREN in the visualization file. Only for compressible flows. Please refer to Section Compressible Flows for a description of its evaluation.

• Particle Volume Fraction: Pvf in the visualization file.
• Particle Eulerian U-Velocity: Pu in the visualization file.
• Particle Eulerian V-Velocity: Pv in the visualization file.
• Particle Eulerian W-Velocity: Pw in the visualization file.
• Fluid-Particle X-Force: Fluid-Particle X-force in the visualization file.
• Fluid-Particle Y-Force: Fluid-Particle Y-force in the visualization file.
• Fluid-Particle Z-Force: Fluid-Particle Z-force in the visualization file.

• Level Set: PHI in the visualization file. This writes the distance to the interface, with positive value in phase 2 and negative values in phase 1. Only for Level Set method.
• Liquid Indicator: HLIQ in the visualization file.
• Interface Marker: markerGL in the visualization file.
• Interfacial area: IFaceArea in the visualization file.
• Interface Curvature: curv in the visualization file.

• Phase Volume Fractions: PhaseAlpha in the visualization file.
• Phase Densities: RhoPhase in the visualization file
• Phase Velocity: UPhase, VPhase and Wphase in the visualization file
• Drift Velocity: Udrift, Vdrift and Wdrift in the visualization file

• Phase Change Rate: Mdot in the visualization file.

• Mass Fraction: Massfrac:(component name) in the visualization file.
• Reaction Rates: rr in the visualization file.
• Molar Fraction: Molefrac:(component name) in the visualization file.

• Mean flow: this enables averages for basic properties: PM, UM, VM, WM, TM, CONM, and also for drift velocities (if any) PhaseUDM, PhaseVDM and PhaseWDM, and mean phase volume fraction PhaseAlphaM
• Normal Stress: U’U’, V’V’, W’W’, P’P’, T’T’ in the visualization file.
• Cross Stress: U’V’, U’W’ and V’W’ in the visualization file, and also U’T’, V’T’ and W’T’.

If the Turbulence model selected is RANS or V-LES, three other output variables are available:

• Mean Turb. Kinetic Energy: TKEM in the visualization file.
• Mean Turb. Dissipation Rate: EpsM in the visualization file.
• Mean Eddy Viscosity Ratio: MutM in the visualization file.

• Turbulent Kinetic Energy: TKE in the visualization file.
• Turbulent Dissipation Rate: EPS in the visualization file.
• Eddy Viscosity Ratio: MUT in the visualization file. Turbulent viscosity ratio ;
• Turbulence Production: TProd in the visualization file.

If LES is chosen in the Turbulence Modelling drop-down list:

• SGS Viscosity Ratio: SgVis in the visualization file. (SGS= Subgrid Scale)
• Turbulent Prandtl Number: TPrandtl in the visualization file.

Turbulent Prandtl Number is available only if Turbulent Prandtl Number Model is not constant in LES model properties. Hydrates Group
  The Hydrates group of variables is activated only if Hydrate Model is selected in the Multiphysics section of Physical Models tab.

Please note: Hydrate Model is only available when Phase Average is selected as Multiphase Flow method and when the number of phases is bigger than 2.

The list of variables for this group is the following:

• Formation Rate: Hydrate Formation Rate in the visualization file.
• Equilibrium Temperature: Teq in the visualization file.

4.7.2 Post-processing panel

This section enables the user to set post-processing parameters and outputs. Their use is described later in the Section Data Processing.

4.7.3 Restart Parameters

In the third section, Restart Parameters of the restart files which allow restarting simulations are set.

• Frequency of restart files and Frequency of Backup files gives the interval at which restart files should be saved: a value of n means that restart files are written every n^th iteration.
  • Restart files are stored in the project folder. They are named <project_name>.runa for ASCII format or <project_name>.runb for binary format. The restart file is overwritten as soon as another restart file is produced.
  • A restart file called properties.dat.runb is also created for restart properties of objects. This is always saved with the extension runb; the format cannot be changed.
  • Backup files are stored in the same folder. They are named <project_name>.xxxx.runa and <project_name>.xxxx.runb for ASCII and binary format respectively. “xxxx” represents the time-step index. Note that these files are stored and not overwritten.
  • A backup file is also stored for the object properties, named properties.dat.xxxx.runb.
• Restart Read Format and Restart Write Format lists enable choosing the format of the restart file that can be read and that of the restart and backup files written during the simulation. ASCII format is larger but can be used on any machine, while binary format produces more compact files which might not be readable on an other machine.

Figure 4.36: Output Management tab

Chapter 5
Running a Simulation

The last tab of the GUI is the Execute tab. Fig. 5.1 gives an example of how this tab looks like when a simulation is running. There are mainly 4 elements displayed which will be further discussed in this chapter:

• Simulation control
• Runtime information
• Simulation residual graph output
• Simulation screen output

5.1 Simulation control

This part of the execute window controls the solver. Simulations can be started, stopped and restarted.

5.1.1 Running TransAT

To run simulations, it is important the project is saved and all solver input files generated. The manual way to do this:

• to save project and models parameters, click Files then select Save. Every change in the TransATUI - Input tab requires this step before a simulation can be started.
• to write the necessary files to run the simulation such as the mesh and the boundary conditions file, click Files then select Prepare Simulation Files. Every change in the TransATUI - Geo/Mesh tab requires this step before a simulation can be started.

The automatic way to do exactly the same is to keep the checkbox ”Save and Prepare Simulation Files” ticked. This will automatically write all necessary files whenever a simulation is started. This is the default behavior and recommended to keep. Expert users might disable this option and manually save model parameters or remaining files.

Clicking the button will start the simulation. Runtime messages output by TransAT solver are shown in the output field.

Please note: Before starting a simulation, make sure that:

• All the project files have been saved and setup files written or the checkbox to automatically generate them is ticked.
• All desired outputs are configured. The possible outputs with TransAT are available in Section Output Management for the visualisation, and Section Data Processing.
• Initial conditions have been defined/created, particularly for multiphase flows

Warning and error messages might appear at the beginning of the simulation. It is strongly recommended to read these messages and to correct the input parameters to comply with the given advise. Otherwise, the solver may not run properly.

Fig. 5.2 and 5.3 show typical outputs of the solver for different types of simulation.

5.1.2 Stopping a Simulation

Clicking stops the current simulation. The stop occurs only at the end of the time-step (or iteration for a steady simulation), so there may be a lag between the moment is clicked and the actual stop of TransAT.

A restart file is then written, called <project_name>.runa or <project_name>.runb (depending on the restart file format, see Section Output Management). It can be used for a future restart of the simulation. Another restart file is also written called properties.dat.runb. This contains properties for any objects in the mesh (such as center of mass, velocity, rotation, and others).

Please note: This restart file overwrites any restart file that could have been saved previously.

5.1.3 Restarting a Simulation

Restarting a previous simulation is done by clicking and selecting restart file(s) (Fig. 5.4). Restart files have the extension .runa or .rsta for ASCII format, and .runb or .rstb for binary format.

The solution file is mandatory, and loads all the simulation values for the various variables in the cells. The Object properties file is optional, and is important if the object properties have changed during the simulation. For example, if the object was specified with motion, then the simulation must be restarted with the current position. The restart file for objects is always called properties.dat, with the extension .runb set.

Figure 5.4: Restart Dialog box

TransAT can also be restarted (initialised) using a restart file from a coarser or finer grid. It is assumed that the geometry is exactly the same (or almost the same). The results from this solution and grid will be interpolated on the current grid. An exact restart is not guaranteed in this case since the grid itself is different.

To do this,

• Select Nonmatching in the Restart method drop-down list
• Specify both the restart solution file name, restart properties file for embedded objects and grid file name by clicking and selecting the corresponding file using the file browser.

Please note: Old and new grids must have the same format, i.e. both files must be in ASCII format or binary format. Also, the new grid cannot be outside of the old grid boundaries (but it can be smaller).

5.2 Runtime information

In the left window of the execute tab below the buttons to run a simulation, there are several elements accessible to display important information while running a simulation. The dropdown menu gives access to all runtime information which will be displayed in the box below the menu.

Detailed information from the running simulation are displayed in the text window on the left side of the Execute tab of the TransATUI (”Runtime information” in Fig. 5.1).
Five information views are possible:

• Simulation Info: detailed information on the current iteration/timestep

    - contains information about residuals and other info, for example simulation time remaining

    - Fig. 5.5 gives an example. See Info: Timing and convergence

  ---

  
  

  Figure 5.5: Simulation information (timing and convergence)

  ---

• License Info: license data

    - displays license information

  ---

  
  

  Figure 5.6: License information

  ---

• Warnings Info: all the warning messages collected from the current simulation

  ---

  
  

  Figure 5.7: Warning messages

  ---

• Errors Info: all the error messages collected from the current simulation

  ---

  
  

  Figure 5.8: Error messages

  ---

• Other Info: additional information from the current simulation

  ---

  
  

  Figure 5.9: Other messages

  ---

Every time the simulation is started all the info content is cleared. However when TransATUI loads a project of a simulation that has already run and finished, the runtime information will display the information from the previous run. To the right of the runtime information selection menu there is another output displaying the current run-state of the simulation:

• Ready
  Displayed when the simulation is not running (before/after simulation).
• Preparing
  Displayed while the simulation input files are prepared (grid/boundary/... files)
• Running
  Displayed while the simulation is running.
• Stopping
  Displayed after clicking on the stop butten while the simulation is running. The simulation will not stop immediately. Only after reaching a point where a restart file can be written. For unsteady simulations this is at the end of a time step. For steady simulation the simulation can be stop after every outer iteration.

Info: Timing and convergence

As shown in Fig. 5.10 the runtime information window can be split in 3 sections:

• Timing information (section 1):
  In the first section timinig information is displayed. For iterations/time steps current and average walltime is displayed.
  
• Inner iterations (section 2):
  For each equation solved, the convergence of solving the linear system in the current outer iteration is displayed. The number of solver iterations used compared to the maximum allowed is displayed. The equations are marked as:
  • (green) → ok when the linear system converges to the target Relative Solver Tolerance within the Maximum number of Solver Iterations as defined in TransatUI → Input → Equations → Advanced Solver Options
  • (green) → converged if the equation is already satisfied (nothing to solve, residual below numerical minimum limit)
  • (yellow) → problematic if the linear system could not be converged to the target.

  Please note: It is good practice to always converge the linear system. However, if the linear system does not reach the target convergence in every outer iteration it is still possible to converge the equation in the outer iteration to the target. This behavior is not ideal but acceptable.

• Outer iterations (section 3):
  For each equation solved, the convergence within the segregated solver is displayed. Current and target residual are displayed. The equations are marked as:
  • (green) → converged when the equation has reached the target Convergence Tolerance as defined in TransatUI → Input → Equations
  • (yellow) → stagnating when residual is not decreasing with respect to the previous outer iteration
  • (red) → NOT converged if the equation did not reach the target Convergence Tolerance within the maximum number of outer iterations defined in
    • ”steady simulation”:
      Number of iterations in TransatUI → Input → Simulation Parameters → Advanced Options
    • ”unsteady simulation”:
      Max number of iterations per Time Step in TransatUI → Input → Simulation Parameters → Control Parameters → Advanced Options

Figure 5.11: Runtime Information for BMR

Fig. 5.11 shows timing and convergence info for a BMR simulation.

• inner iterations
  • LDC (Local Defect Correction) - sweeps are iterations between the different grid levels. For one LDC sweep all grid levels are solved, correction terms are calculated. After each sweep a composite solution (fine + coarse) is constructed for the residual calculation.
  • Solver sweeps are now the average number of sweeps for the solvers. The number displayed here is the average for all BMR-levels and LDC sweeps.
    Therefore is possible to see here 0 like in the picture. This happens in the current example since one of the 2 BMR levels is solved within 1 solver sweep, the other is already below the target residual.
• outer iterations
  • same output as before, however the residual displayed is the residual of the composite residual (for the combined fine/coarse solution)

Expert information

All the information printed in the runtime info window can be also found in the following files in the project directory where the simulation is running:

• simInfo.txt: file containing Simulation Info data, it is updated per each iteration for steady/unsteady simulation therefore only last status is written
• licenseInfo.txt: contains License Info data
• warningsInfo.txt: contains Warnings Info data
• errorsInfo.txt: contains Errors Info data
• sarpInfo.txt: contains SArP Info data which consist of:
  • information relative to the progress of SArP’s genetic algorithm when it is running
  • the number of SArP launches
  • the history of the SArP launches during the simulation
• Info.txt: contains Other Info data

Running on clusters using a job system these files will be created as well, except simInfo.txt. The files are useful to check for info/warning/error messages of a simulation.

5.3 Screen output

The runtime information as described in the previous sections is a summary of the solver screen output in the ”Simulation screen output” part of the execute window as shown in Fig. 5.1. Information, warnings, errors and convergence information are displayed in the solver output window. The information and the coloring displayed is slightly different however and it will also code all convergence information if colors are disabled using markers. The coloring differs for the following events:

• convergence
• last iteration
• normal iteration

For convergence or last iteration the residual line is separated from the other lines and marked

• with ”-” characters in green (if colors enabled) for reaching convergence
• with ”*” characters in red (if colors enabled) for reaching the last iteration without convergence

Figure 5.12: Simulation convergence screen output

The screen output gives a lot of information about convergence already without the additional simulation info of the GUI. Depending if colors are enabled or not, colors or markers are used to give additional information. See Fig. 5.13 for screen output with and without colors displaying:

• As soon as a variable has reached its convergence criterion, it will be either displayed in green or with the marker ”>”. In this example, e has converged after 5 outer iterations.
• The equation solving t is displayed in yellow or with the ”!” marker which indicates a problem to converge the linear system Ax=b. The relative solver tolerance cannot be reached with chosen solver and number of inner iterations.
• In the second iteration the equations for variable u and v are displayed in capital letters plus ”?” in the output without colors. This indicates the reference residual for normalisation had been reset.

Figure 5.13: Color- and marker-based convergence information

5.4 Visualization of residuals

Residuals of the simulation are displayed in the Graphs section of the Execute tab.

Clicking Custom opens a window where one can output data of interest written in the RESULT folder in real time.

5.4.1 Unsteady simulations

For unsteady simulations, the relative residuals for each time step are written in files L1_resnorm.dat, L2_resnorm.dat and Linf_resnorm.dat, using norms L¹, L² and L^∞, respectively. These files can be selected in the Graphs section of the Execute tab of the TransATUI

5.5 Run-time Intervention

Run-time intervention is available when using TransAT. However, this is not available in TransATUI yet except for the simulation-stopping and SArP-module-stopping buttons.
During a simulation, the user can click to stop it. Inputs can then be changed and saved before re-running the simualtion or restarting it by clicking . See Section 5.1.3 for restart options.

When the SArP module is running, the SArP module can be stopped by clicking . After stopping the simulation, the simuation is restarted with the parameters of the best solution found by the SArP algorithm.

The run-time behaviour of TransAT can be changed by creating run-time intervention file transat_mb.rti in the project folder.

5.5.1 Inputs for run-time intervention

The file transat_mb.rti is made up of the first line which indicates the action to be taken on reading the file and the Namelist Run_Time_Control. The following strings are accepted in the first line: output, reread_input, stop, noaction.

• output: writes out an output file immediately after the file is read.
• reread_input: reads the new input given in the Namelist Run_Time_Control in the file.
• stop: stops the simulation and writes a restart file.
• stop_sarp: stops the SArP algorithm and restarts the simulation with the parameters of the best solution found.
• noaction: does not do anything. This option can be used while editing the Namelist in transat_mb.rti. After the appropriate inputs are specified, noaction can be changed to reread_input.

Below is a sample of the Namelist Run_Time_Control input variables:

Example of transat_mb.rti file:

The number of iterations to be run can be changed without stopping the code using the above transat_mb.rti file.

Another option would be to stop the simulation using , change inputs as needed, save the project and restart the simulation.

5.6 Quitting the GUI

Clicking Files then selecting Exit closes the GUI. If a simulation is running at the same time, a dialog box pops up, as shown in Fig. 5.14. The following choices are possible:

• Stop and restart the simulation in xterm: the GUI closes, stops TransAT cleanly and restarts it in a terminal.
• Stop and restart the simulation “nohup”: the GUI closes, stops TransAT cleanly and restarts in “nohup” mode, without any terminal to control it.
• Stop simulation and exit: the GUI closes, stops TransAT cleanly and saves a restart file.
• Kill simulation and exit: the GUI stops immediately, without creating any restart file.

Click to keep the GUI open and the simulation running.

Chapter 6
Settings Guides

6.1 SArP Guide

6.1.1 When to use SArP

The SArP module has two modes which are depicted in Figure 6.1 and Figure 6.2:

• Optimisation: call to the SArP module from the start of the simulation to optimise parameters
• Stability: call to the SArP module when convergence issues are detected

Before using the optimisation mode, it is advised to first run the simulation without it as the optimisation process can be costly. If the simulation can be completed in an acceptable time, it is advised not to use the optimisation mode. Otherwise the optimisation mode can be used to correct and accelerate the simulation.

The typical use cases for the optimisation mode are:

• simulations that have trouble converging from the very start. Convergence issues can be stagnating or oscillating residuals, time-steps reaching the maximum number of iterations, etc.
• simulations that are crashing from the very start
• simulations that may require a lot of time to reach the target residuals or physical time i.e. cases where the residuals decrease very slowly or where the time steps are low

There is no specific restriction regarding the use of the stability mode.

Please note: the optimisation can be accelerated by tuning some parameters or exiting the optimisation process early. See the Speeding up SArP section to get more information.

Please note: after the initial SArP launch in optimisation mode, the simulation runs in stability mode in the remainder of the simulation.

6.1.2 Detection of convergence issues

To use the SArP module optimally, it is important to understand how it operates to detect convergence issues. The parameters that are used to detect convergence issues can be tuned so that the SArP module is only triggered when necessary. Convergence issues can be detected by the SArP module by monitoring the following quantities:

• residuals
• solver iterations
• time steps

Residuals based issues

Figure 6.3: Oscillating residuals

Figure 6.4: Stagnating residuals

Figure 6.5: Simulation with unconverged time steps

Solver based issues

In a given simulation, each equation is solved iteratively at each iteration. The iterative solvers have a maximum number of iterations parameter. This parameter can be set in the Equations section of the Simulation Parameters tab after activating Advanced Solver Options. The parameter is called Max Number of Solver Iterations. Figure 6.6 is a typical TransAT output shown in the Execute tab of a simulation with unconverged iterations. In this example there are residuals that are coloured in orange indicating that the solver of the corresponding equation did not converge.

Whenever the solver of an equation reaches the maximum number of solver iterations, it indicates convergence issues especially in cases where this happens frequently. In the remainder of this section we will refer to iterations where the maximum number of solver iterations is reached as unconverged iterations. Consecutive unconverged iterations  One way to check convergence issues down to solvers is to monitor the number of consecutive unconverged iterations for each equation. The SArP module is triggered as soon as the number of consecutive unconverged iterations reaches a threshold value. This threshold value is set in the Consecutive Unconverged Iterations field in the Advanced Parameters window of SArP in TransATUI. Unconverged iterations rate  Another way to check convergence issues down to solvers is to monitor the rate of unconverged iterations. For steady simulations, the unconverged iterations rate is measured over the SArP analysis window while it is measured over whole time steps for unsteady simulations. The SArP module is triggered as soon as rate of unconverged iterations reaches a threshold value. This threshold value is set in the Unconverged Iterations Rate field in the Advanced Parameters window of SArP in TransATUI.

Time step based issues

6.1.3 Correction And Optimisation

Evaluations

For a given simulation, the SArP module can be launched only a limited amount of times. The limit of SArP launches is the value in the Max. Genetic Algorithm Runs field in the Advanced Parameters window of SArP in TransATUI.

In the SArP module, solutions – set of random parameters – are evaluated. A solution evaluation is done in two steps. Firstly, a simulation is run for n iterations/time steps, with n the value in the Analysis Window Size field in the Advanced Parameters window of SArP in TransATUI. Secondly, the results are analysed to determine the validity status and the score of the solution.

Unless a stopping criterion is met, each SArP launch evaluates n_eval solutions for g_max generations as shown in the diagram of Figure 6.7. g_max and n_eval are respectively the Max. Generation and the Evaluations Per Generation fields in the Advanced Parameters window of SArP in TransATUI.

Roll-back option

The roll-back option which is activated by the Enable Roll-Back check box in the Advanced Parameters window of SArP in TransATUI. With this option, preliminary steps are run before correcting numerical parameters:

1. restart simulation using the latest restart backup file
2. stop simulation before the time step/iteration where convergence issues have been detected
3. launch the SArP module from that point

Figure 6.8 depicts the roll-back option for an unsteady simulation. The principle is exactly the same for steady simulations. The offset shown in Figure 6.8 is determined depending on the detected convergence issue. Depending on the value of the offset, the simulation may be restarted from an earlier point than the closest backup restart file.

Stopping criteria

The SArP module stops when one of the stopping criteria is met. Setting appropriate stopping criteria of the SArP module is recommended The stopping criteria vary accordingly to the nature of the simulation, steady or unsteady. The stopping criteria are described below. Steady simulations  For steady simulations, the SArP module stops if:

• the best solution found has not been improved upon for n consecutive generations with n the value in the Stagnating Generations field in the Advanced Parameters window of SArP in TransATUI
• the ratio between residuals at the end of the analysis window and the maximum residual at the beginning of the analysis window is less than a user-defined ratio. On top of this condition, the residuals of each equation must be overall decreasing or below the target residuals to exit the SArP module
• the maximum number of generations, n_max, set by the user is reached with none of the SArP module convergence criteria being met (n_max is the value in the Max. Generation field in the Advanced Parameters window of SArP in TransATUI). In that case if at least one valid solution has been found during the process, the valid solution with the highest score is selected. If no valid solution is found, the simulation is stopped

A typical steady simulation evaluation is shown in Figure 6.9. In that example the residuals exit condition is met by the variable represented with red disks and green crosses since their residuals drop below γRes_max where γ is the user-defined residual drop factor. The exit condition is however not met by the variable represented with purple diamonds.

Unsteady simulations  For unsteady cases, the SArP module stops if:

• a solution for which the last time step has reached the target residual has been found
• the best solution found has not been improved upon for n consecutive generations with n the value in the Stagnating Generations field in the Advanced Parameters window of SArP in TransATUI
• the maximum number of generations, n_max, is reached with with none of the SArP module convergence criteria being met (n_max is the value in the Max. Generation field in the Advanced Parameters window of SArP in TransATUI). In that case if at least one valid solution has been found during the process, the valid solution with the highest score is selected. If no valid solution is found, the simulation is stopped

6.1.4 Speeding up SArP

• Option 1: set Configuration to fast
• Option 2: adjust the genetic algorithm parameters by:
  • reducing Analysis Window Size
  • reducing Evaluations Per Generation
  • reducing Max. Generation
• Option 3: adjust the genetic algorithm convergence criteria to exit the SArP module early by
  • reducing Stagnating Generation
  • increasing Residual drop factor (only for steady cases)
• Option 4: activate Enable Fitness Approximation

Please note: with these options the space of the parameters is searched less. It makes finding the optimal set of parameters less likely. This is usually not an issue especially when acceptable or reasonably fast set of parameters can be found with less effort compared to the deeper search required to find the optimal set of parameters. User intervention  Alternatively, the SArP module can be stopped in the middle of the process if a satisfactory solution has been found. This can be done by clicking in the Execute tab of TransATUI or creating the file transat_mb.rti and setting its content to stop_sarp (only one word in the file).

To check whether a solution is satisfactory the SArP Info tab of the simulation information panel along with the simulation output can be checked.

The simulation information panel contains information related to the SArP module progress and selection process. During the SArP module run, a table with the validity status and the score of the evaluated solution is displayed in the SArP Info tab. The validity status of a given solution indicates whether the solution has convergence issues. Valid solutions are coloured in green while invalid ones are coloured in orange.

The score is a metric of the convergence of the simulation based on the residuals. The higher the score the better the convergence. To get a more detailed view of the convergence quality, the simulation output can be looked at. For steady simulations, the residuals of the best solution at the previous generation can be directly checked in the simulation information panel. Figure 6.10 shows a typical SArP Info tab of a steady simulation.

Figure 6.10: SArP info tab of a steady simulation

Figure 6.11: SArP info tab of an unsteady simulation

Chapter 7
Post-Processing

7.1 Output Files

7.1.1 SArP

When the SArP module is activated, the following ouptut files are generated:

• simulation folder
  • sarpInfo.txt: contains history of the SArP launches
  • sarp_log.log: contains log of SArP runs
• sarp_result folder
  • transat_mb.XXXXX.inp: TransAT input file used after the i^th run of SArP
  • diff.XXXXX.txt: contains the input changes in the input file after the i^th run of SArP

7.2 Visualisation with ParaView

To get a rough idea about visualisation of TransAT results with ParaView, please refer to the TransAT Paraview Tutorial .

More detailed information can also be found in the Paraview Tutorial on the ParaView website.

7.3 Visualisation with Tecplot

Start Tecplot in you working directory by:
tecplot
Open your result file:
File → Load Data File(s)...
Tecplot Data Loader
Choose your result file and click ’OK’.
When asked to select your Initial Plot Type, select the (default) 3D Cartesian type and click ’OK’. Now the tecplot window should look like in Fig. (7.1).

Define Variables

Open the window to define variables (see Fig. (7.2)).

Define variable C1 to be Temperature and C2 to be EmbI, which is the function representing the immersed surfaces. Close this window.
Define Isosurface
Enable and define the isosurface representing the immersed objects (see Fig. (7.3)).

Define the Interface using variable C2:EmbI at 1 specific value which is zero. By default, the interface is coloured by variable C1 which should be the temperature.
Define Slice
Enable and define the slice like in Fig. (7.4).

7.4 Data Processing

This section describes the various post-processing utilities available in TransAT. All input files related to the post–processing utilities are created in the project folder, and all results are written in the RESULT folder by default.

Please note: Some post-processing utilities are not available in the GUI yet. To enable them, the user may have to edit and modify directly the input file transat.inp, which is located in the project folder.

7.4.1 Non-dimensional numbers

Non-dimensional numbers can be evaluated by TransAT during the simulation. This feature is turned on by default.

It can be activated or deactivated in the Output Management sub-tab of the Input tab. One simply needs to check or uncheck the Non Dimensional Numbers box in the Postprocessing section (Fig. 4.36).

This utility calculates a variety of non-dimensional numbers and writes them to the file RESULT/ND_numbers.dat.

The reference length scale and reference velocities are taken from the value given in the Physical Models sub-tab of the Input tab (See Section Physical Models).

Depending on the physical models used, the available non-dimensional numbers can be the following

• The gas and liquid Reynolds numbers give the ratio of the inertial and viscous forces.

  (7.1)

  where reference length and velocity are given in the Reference State panel of the Physical Models tab.

  If the maximum velocity magnitude exceeds twice the reference velocity, maximum Reynolds number is also written.

• The Froude number gives the ratio of inertial and gravitational forces.

  (7.2)

  where reference length and velocity are given in the Reference State panel of the Physical Models tab, and g is the gravity magnitude.

• The gas and liquid Prandtl numbers are the ratios of momentum and thermal diffusivities (printed if temperature equation is solved).

  (7.3)

• The gas and liquid Rayleigh are associated with buoyancy driven flows (printed if temperature equation is solved).

  (7.4)

  where β is the thermal expansion coefficient, ΔT = 2, with T_max the maximum temperature in the domain. ref subscripts refer to values given in the Reference State panel of the Physical Models tab.

• The Weber number is the ratio of inertia to surface tension forces (printed for two-phase flow).

  (7.5)

  with σ the surface tension and ref subscripts denoting reference values given in the Reference State panel of the Physical Models tab.

• The Eotvos number is the ratio of gravitational forces to surface forces (printed for two-phase flow).

  (7.6)

  with σ the surface tension and L_ref the reference length given in the Reference State panel of the Physical Models tab.

• The Morton number characterizes the shape of bubbles or drops

  (7.7)

• The gas and liquid Capillary numbers are ratios of viscous forces to surface tension forces (printed for two-phase flow).

  (7.8)

  with u_ref the reference velocity given in the Reference State panel of the Physical Models tab.

• The Rossby number is the ratio of inertial to Coriolis forces (printed for rotating frames).

  (7.9)

  with Ω the angular velocity. Two Rossby numbers are written: one with L = L_ref given in the Reference State panel of the Physical Models tab, and one with L = L_D the domain size.

A typical output of this utility is shown below.

Checking the ND_numbers.dat file at the beginning of every simulation and specifying a reasonable value of the reference length and velocity is part of the best practice guidelines for using TransAT.

7.4.2 Time signals probes

This utility saves time signals at a given set of points in the domain. The points do not have to match with a grid point, values are interpolated.

This feature can be turned on by creating an input file named timesignalxyz.dat in the project folder. The input file contains coordinates of points at which data has to be extracted. Each line should have 4 columns: viz. probe number (integer), x–coordinate, y–coordinate, z–coordinate.

The output file is stored in the RESULT folder and has a name of the type timesignal.yyyy., with y the index of the time signal (Note: If ”blockfile” is set by hand to true in the input file transat_mb.inp then y represents the block number and can contain several time signal points).
The signal is stored at every time step. The following variables are written in timesignal.yyyy, depending on different equations solved:

• Monitor point index
• Time
• Pressure
• System pressure (Compressible flows)
• Velocities
• Temperature
• Subgrid viscosity (LES)

7.4.3 Section Output

This utility saves output on a given section plane. The plane could be aligned to the grid or can be defined at an arbitrary angle. The utility can also be used to extract ouput on a sub-section of a plane. An example of a section plane is shown in Fig. (7.5).

This feature can be turned on by creating an input file named sectionsxyz.dat in the project folder. The input file contains definitions of section planes. Each plane is defined by its normal and a point on the plane.
A sub-section in a given plane can also be defined by defining the extents of the sub-section in the plane. Each line in the input file should have either 6 columns: viz. plane–normal (x–axis), plane–normal (y–axis), plane–normal (z–axis), x–coordinate, y–coordinate, z–coordinate or 12 columns: viz. plane–normal (x–axis), plane–normal (y–axis), plane–normal (z–axis), x–coordinate, y–coordinate, z–coordinate, xmin, xmax, ymin, ymax, zmin, zmax, where xmin, xmax, ymin, ymax, zmin and zmax defines the extents of a sub-section in a given plane.

First line defines a plane with normal in x-direction through point (0.1,0.0,0.0). The second line defines a plane rotated by 45⁰ around the z-axis and through point (0.0,0.3,0.0). The last line finally has the same definition as the first one. The section is further limited by x/y/z-plane integration limits.

The output file is stored in the RESULT folder and has a name of the type section.y., with y the index of the plane.
The section output is stored at every iteration for steady simulation and at every time step for unsteady simulation. The following variables are written in section.y, depending on different equations solved:

• Time step number, time step and simulated time for unsteady simulations and iterations for steady simulations
• Area per phase - activated by default
• Mass flux per phase - activated if either U-velocity, V-velocity or W-velocity equation is solved.
• Mass flux and area weighted static and dynamic pressure if pressure equation is solved.
• Heat capacity flux weighted temperature and cross-sectional wall averaged temperature if temperature equation is solved.
• Cross-sectional immersed surface wall averaged temperature if temperature equation is solved and immersed surfaces is enabled.
• Massflow averaged mass fractions, wall averaged mass fractions, Sherwood number and averaged reaction rates if mixture equation is solved and immersed surfaces are enabled.
• Massflow averaged mass fractions, wall averaged mass fractions, and averaged reaction rates if mixture equation is solved, immersed surfaces and write mole fractions are enabled.

Area weighting of a variable ϕ is defined as:

(7.10)

Mass flux weighting of a variable ϕ is defined as:

(7.11)

Heat capacity flux weighting of a variable ϕ is defined as:

(7.12)

Chapter 8
Command Line Options

Multiple TransAT operations such as the generation of simulation files, setting of initial conditions and simulation execution can be directly launched in command line. The command line options of TransAT are of particular use to run multiple simulations. Indeed, scripts can be created using the TransAT command lines to run large number of simulations without user intervention.

8.1 Environment variables setting

Some of the operations supported by TransATUI can be directly executed in command line. TransAT commands can be directly executed if the PATH environment variable contains the following folders:

• <TransAT_Installation_directory>/transatMB/bin
• <TransAT_Installation_directory>/transatUI/bin

To check if the first folder is in the PATH environment variable, execute the following command in a terminal:

It should point to a file located in <TransAT_Installation_directory>/transatMB/bin. If that is not the case, execute the following command