33.2. Fluent GPU Solver Tutorial

This tutorial is divided into the following sections:

 

33.2.1. 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.

 

33.2.2. 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.

 

33.2.3. 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 33.7: Problem Schematic.

Figure 33.7: Problem Schematic

Problem Schematic

 

33.2.4. Setup and Solution

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

 

33.2.4.1. 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.

 

33.2.4.2. 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 (2)
================================================================
Area    Settings          From               To                 
----------------------------------------------------------------
solver  rhie chow         distance-weighted  momentum-weighted  
solver  residual scaling  global             local

    For this tutorial, the converted settings are satisfactory.

 

33.2.4.3. Models

  1. Open the Viscous Model dialog box.

     Physics → Models → Viscous...

    Figure 33.8: 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.

 

33.2.4.4. Solution

  1. Review the Solution Methods.

     Solution → Solution → Methods...

    Figure 33.9: Solution Methods Task Page

    Solution Methods Task Page

    1. Retain 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. Run the calculation for 5 iterations.

     Solution → Calculation → Run Calculation...

    1. In the Run Calculation task page, enter 5 for Number of Iterations.

    2. 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 33.10: Residuals

Residuals