Fluent

This is the documentation for all Fluent solver wrappers. The focus of this page is on fluid-structure interaction (FSI). Currently no other multiphysics problems are supported, but these are envisioned in future developments. FSI with inviscid flows is not supported, but that would be straightforward to add if required.

Fluid-structure interaction with Fluent

ANSYS Fluent can be used to solve the flow field in partitioned FSI simulations. The FSI interface consists of one or several surface threads in Fluent. During each FSI iteration, the solver wrapper imposes a certain displacement on this FSI interface. Fluent then automatically deforms the rest of the mesh (using dynamic mesh capabilities), solves the flow field and returns the calculated loads on the FSI interface to the solver wrapper. Displacements are applied in Fluent in nodes. As displacements are the input of Fluent, these nodes are collected in one or more ModelParts in the input Interface. Loads (pressure and traction) can be obtained from the Fluent faces. As loads are the output of Fluent, these faces are collected in one or more ModelParts in the output Interface. A fixed naming convention is used for the Fluent ModelParts in CoCoNuT: each ModelPart gets the name of the corresponding Fluent surface thread, plus "_nodes" or "_faces", depending on their content. As a consequence, each ModelPart in the input Interface has a counterpart in the output Interface. More information about ModelParts and Interfaces can be found in the data structure documentation.

Parameters

This section describes the parameters in the JSON file, listed in alphabetical order.

parameter	type	description
case_file	str	Name of the case file. It must be present in the folder specified by working_directory. The corresponding data file must also be present but has no key in the JSON file.
cores	int	Total number of processor cores to use when running Fluent. When its value is negative or bigger than the maximum number of available cores, it will be automatically replaced by the maximum number of available cores.
debug	bool	(optional) Default: false. For every iteration, text files are saved with the input and output data of the solver.
delta_t	float	Fixed time step size in flow solver. This parameter is usually specified in a higher Component.
dimensions	int	Dimension used in flow solver: 2 for 2D and axisymmetric, 3 for 3D.
end_of_timestep_commands	str	(optional) Fluent journal command(s) to be executed after every time step, to store drag and lift forces for example.
flow_iterations	int	Number of non-linear iterations in Fluent per coupling iteration.
fluent_gui	bool	Set to true to run Fluent with the graphical interface.
interface_input	list	List of dictionaries to describe the input Interface (Fluent nodes). Each dictionary defines one ModelPart with two keys: model_part contains the name of the ModelPart and variables contains a list of variable names. Each ModelPart name must be the concatenation of an entry from thread_names and "_nodes". The variable names must be chosen from data_structure/variables.py.
hostfile	str	(optional) Filename of the hostfile in case of a multi-node job, this file has to be in the working_directory and contain the names of the available machines. Not required for single-node jobs.
interface_output	dict	Analogous to interface_input, but for the output Interface (Fluent faces). Each ModelPart name must be the concatenation of an entry from the file thread_names and "_faces".
max_nodes_per_face	int	This value is used to construct unique IDs for faces, based on unique IDs of nodes (provided by Fluent). It should be at least as high as the maximum number of nodes on a face on the interface. Use e.g. 4 for rectangular faces, 3 for triangular faces and 2 in 2D simulations (edges).
multiphase	bool	(optional) Default false. true for multiphase Fluent case, false for singlephase.
print_coupling_convergence	bool	(optional) Default false. If true and if the solver coupling convergence is checked, a statement is printed when the solver converges in the first solver iteration, see solver coupling convergence.
save_results	int	(optional) Default 1. Number of time steps between consecutive saves of the Fluent case and data files.
thread_names	list	List with Fluent names of the surface threads on the FSI interface.
timestep_start	int	Time step number to (re)start a transient FSI calculation. If 0 is given, the simulation starts from the case_file, else the code looks for the relevant case and data files. This parameter is usually specified in a higher Component.
unsteady	bool	true for transient FSI, false for steady FSI.
working_directory	str	Absolute path to the working directory or relative path w.r.t the current directory.

timestep_start and delta_t are necessary parameters, but are usually defined already in the parameters of the coupled solver. However, they can also be given directly as parameter of the solver wrapper (e.g. for standalone testing). If they are defined both in the coupled solver and in the solver wrapper, then the former value is used and a warning is printed.

If different parameters are used with different Fluent versions, this should be specified both in this section and in the version specific documentation section.

Overview of operation

The solver wrapper consists of 3 files (with X the Fluent version, e.g. "v2023R1"):

• X.py: defines the SolverWrapperFluentX class,
• X.jou: Fluent journal file to interactively run the FSI simulation, written in Scheme,
• X.c: Fluent UDF file that implements additional functionality used in Fluent, written in C.

The initialize method

During initialization, the journal and UDF files are adapted (parameter values are filled in) and copied to the working_directory. Fluent is then started in that directory using the parameters cores, dimensions and fluent_gui. Fluent then writes a case summary, so that the solver wrapper can link the interface thread names (specified in thread_names) to Fluent thread IDs, for use in the UDFs. Then the Model and ModelParts are created, based on data written by Fluent in time step 0. After a restart, this same data must be found, i.e. if those data files are removed from the working_directory folder, the simulation cannot be restarted. Finally, the Interfaces are created.

Files created during simulation

In these file conventions, A is the time step number and B the Fluent thread ID.

• Fluent case and data files are saved as files of the form case_timestepA.cas and case_timestepA.dat.
• Current node and face coordinates are passed from Fluent to CoCoNuT with files of the form nodes_timestepA_threadB.dat and faces_timestepA_threadB.dat.
• The new node coordinates are passed from CoCoNuT to Fluent with files of the form nodes_update_timestepA_threadB.dat.
• Pressure and tractions are passed from Fluent to CoCoNuT with files of the form pressure_traction_timestepA_threadB.dat.
• Files with extension .coco are used to exchange messages between CoCoNuT and Fluent.

Setting up a new case

Following items should be set up and saved in the Fluent case file (this list may be non-exhaustive):

• additional UDFs must be configured,
• steady/unsteady (should match with the unsteady parameter),
• 2D, 3D or axisymmetric (should match with the dimensions parameter),
• dynamic mesh zones for all deforming surfaces, except for the FSI interfaces,
• dynamic mesh smoothing parameters,
• boundary conditions, material properties, numerical models, discretization schemes, operating conditions, turbulence modeling, convergence criteria.

A data file should also be present with the fields either initialized or containing the results of a previous calculation.

Following items are taken care of by CoCoNuT, and must therefore not be included in the Fluent case file:

• dynamic mesh zones for the FSI interfaces (these are defined in thread_names),
• the time step (delta_t).

Solver coupling convergence

The convergence criterion solver coupling convergence is implemented for the Fluent solver wrapper. Instead of comparing the different residuals (continuity, x-velocity, ...) with their respective tolerances before the first iteration, they are checked after the first iteration due to implementation restrictions.

Version specific documentation

v2019R3 (19.5.0)

Base version. With respect to older Fluent versions, the solutions in this version are (slightly) different because the Rhie-Chow face flux interpolation in the pressure-based solver has changed. This setting can be reverted with the TUI command solve set previous undo-2019r3 y n, which is included in v2019R3.jou.

The results can be slightly different when restarts are used for multi-core simulations for the following reason: For parallel cases with smoothing that do not use dynamic load balancing, a zonal partitioning with Laplace smoothing will automatically be applied when the file is read, which should result in better load balancing for the mesh smoothing calculations. After a restart, the partitioning can be different and hence the mesh deformation can be slightly different.

v2021R1 (21.1.0)

This version fails for the tested multiphase problems. The saving of "cell residuals" for postprocessing with the following command solve set expert y y n y results in the following error: Error at Node 0: alloc_thread_sv: storage already exists for SV_RECON_MIN on thread 2, domain 3. This issue is solved in v2023R1.

v2023R1 (23.1.0)

No major changes.