Chapter 35: Using the Fluent Native GPU Solver

This tutorial is divided into the following sections:

 

35.1. Introduction

This tutorial demonstrates how to use the Fluent GPU Solver to simulate a turbulent flow around a sedan.

This tutorial describes how to perform the following:

  • Start the Fluent GPU Solver from the Fluent Launcher.

  • Read a Fluent case file into the GPU Solver.

  • Define models and settings for the simulation.

  • Initialize and calculate the solution.

 

35.2. Prerequisites

This tutorial is written with the assumption that you have completed the introductory tutorials found in this manual and that you are familiar with the Ansys Fluent outline view and ribbon structure. Some steps in the setup and solution procedure will not be shown explicitly.

 

35.3. Problem Description

The problem considers the turbulent flow of air around a sedan at a free stream velocity of 30 m/s. The sedan modeled here is shown in Figure 35.1: Problem Schematic.

Figure 35.1: Problem Schematic

Problem Schematic

 

35.4. Setup and Solution

The following sections describe the setup and solution steps for this tutorial:

 

35.4.1. Preparation

To prepare for running this tutorial:

  1. Download the sedan_2m.zip file here .

  2. Unzip sedan_2m.zip to your working directory.

  3. The file, sedan_2m.cas.h5, can be found in the folder.

  4. Use the Fluent Launcher to start the Fluent GPU Solver.

  5. Select Solution in the top-left selection list.

  6. On the Fluent Launcher, set the Capability Level to Enterprise, then enable Native GPU Solver under Options.

    After enabling Native GPU Solver, the GPUs available on your machine will be listed under CPU Processes

  7. (optional) To use the GPU solver with multiple GPUs, enable the GPUs you would like to use under CPU Processes.

  8. Click Start.

The graphical user interface (GUI) of the Fluent GPU Solver is nearly identical to Fluent Solution Mode, with the only difference being that some unsupported features are hidden within the GPU Solver GUI.

 

35.4.2. Reading the Fluent Case File Into the GPU Solver

  1. Read the Fluent case file sedan_2m.cas.h5.

     File → Read → Case...

    As the GPU Solver reads the case file, information about the mesh will be reported in the console and converted settings will be reported as follows:

    GPU solver defaults are activated for the following unsupported settings (4)
=========================================================================================
Area                   Settings                         From                   To        
-----------------------------------------------------------------------------------------
solver                 warped face gradient correction  on                     off       
solver                 residual scaling                 global                 local     
hybrid initialization  averaged turbulent parameters    enabled                disabled  
initialization         reference frame                  relative to cell zone  absolute

    For this tutorial, the converted settings are satisfactory.

 

35.4.3. Models

  1. Open the Viscous Model dialog box.

     Physics → Models → Viscous...

    Figure 35.2: Viscous Model Dialog Box

    Viscous Model Dialog Box

  2. In the Model group box, enable k-omega (2 eqn).

  3. In the k-omega Model group box, enable GEKO.

  4. Click OK to close the Viscous Model dialog box.

Note that after enabling the GEKO k-omega model, the discretization scheme for turbulent kinetic energy will automatically be changed from first order upwind to second order upwind, as shown in the console.

 

35.4.4. Solution

  1. Review the Solution Methods.

     Solution → Solution → Methods...

    Figure 35.3: Solution Methods Task Page

    Solution Methods Task Page

    1. Select Coupled for the scheme.

    2. For the Pseudo Time Method, select Global Time Step.

    3. Retain the rest of the default settings.

  2. Initialize the solution using standard initialization.

     Solution → Initialization → Options...

    1. In the Solution Initialization task page, ensure that Standard Initialization is enabled.

    2. From the Compute From drop-down list, select velocity-inlet-10.

    3. Click the Initialize button to initialize the solution.

  3. Specify the Run Calculation settings.

     Solution → Calculation → Run Calculation...

    1. In the Run Calculation task page, enter 10 for the Time Scale Factor.

    2. Enter 5 for Number of Iterations.

    3. Click Calculate to start the calculation.

  4. Reset the GPU performance meter.

     Parallel → Timer → Reset

  5. Rerun the calculation for 100 iterations.

     Solution → Calculation → Run Calculation...

    1. Enter 100 for Number of Iterations, then click the Calculate button to start the calculation.

Figure 35.4: Residuals

Residuals