This chapter introduces the Parameter Study Analysis Workflow using OpenFOAM as a calculation example using WHEEL.

Perform a parameter study of inlet flow velocity on a distribution pipe model created in 3D CAD.

1. Overview

The analysis target model used in this example is the distributed-pipe model.

Analytical Model D50-d10

img

Perform an analysis where the fluid coming in from the inlet leaves the outlet.

This tutorial assumes that you are running on Fugaku. If you are running in a different environment, change the script settings accordingly.

Also, be sure to download and extract the file in advance. The archive contains three files:

pipe.unv
Mesh (“SALOME-MECA” is used to create a CAD model and export mesh data in Ideas universal format.)
U
velocity initial condition file
D50-d10.tgz
Case Files

In the final step of this tutorial, you use ParaView, which is installed on the WHEEL server, to visualize the calculation results.

Therefore, if you are running the tutorial with WHEEL installed on a remote server, or if you are running in an environment where ParaView is not installed, you cannot run the Checking Analysis Results chapter.

Workflow Overview

In this tutorial, we will use the parameter study component as shown below to analyze the inlet velocity in 1m/s increments from 5 to 7m/s.

img

convert component
Prepare a mesh file for OpenFOAM.
PS0 component
The analysis is performed while changing the inlet flow velocity. It has the solve component described below as an internal component.
solve component
Perform an OpenFOAM analysis using a mesh created with the convert component.
extract
Expands the analysis results and opens them in ParaView.

2. Workflow Creation

Create a new project and add two task components and one PS component. The first task component should be named convert and the second task component should be named extract.

Also, add one task component inside the PS component and name it solve.

Configure the convert component

First, place the distribution pipe model created in CAD in the convert component. Open the Files area of the convert component and upload the previously downloaded pipe.unv.

You can upload a file by dropping it in the Files area or by selecting the file to upload in the dialog that appears when you click the upload file button. For detailed instructions, see the Reference Manual.

You then create a script that runs on the convert component. Create a new file named run.sh with the following contents:

. /vol0004/apps/oss/spack-v0.17.0/share/spack/setup-env.sh

spack load 'openfoam@2012%fj@4.8.0'

ideasUnvToFoam pipe.unv

This script converts a mesh file in Ideas universal format to OpenFOAM format.

On successful completion, the following file is generated in the constant/polyMesh directory:

  • boundary
  • owner
  • faces
  • neighbor
  • points

Finally, open the component properties window and set the following four items.

  • script: run.sh
  • host: fugaku
  • use job scheduler: Enabled
  • output files: constant

Setting up the solve component

First, place the case file and velocity initial condition file used for the analysis in the solve component. Open the Files area of the solve component and upload the following pre-downloaded files:

  • Case Files (D50-d10. tgz)
  • Initial velocity condition file (U)

Next, create a script file. Create a new file named run.sh with the following contents:

. /vol0004/apps/oss/spack-v0.17.0/share/spack/setup-env.sh

spack load 'openfoam@2012%fj@4.8.0'

tar xvzf D50-d10.tgz
mv ./U ./D50-d10/0
cd ./D50-d10

decomposePar || exit $?
mpiexec -n 12 simpleFoam -parallel || exit $?
reconstructPar || exit $?
touch result.foam

cd ..
tar cvzf D50-d10.tar.gz D50-d10

Finally, open the component properties window and set the following three items.

  • script: run.sh
  • host: fugaku
  • use job scheduler: Enabled

Configuring PS Components

The PS component provides settings for changing inlet flow velocity.

Preparing a folder for storing calculation results

Prepare a folder for storing calculation results. Click the PS component and add results to output files.

Parameter Study Condition Settings

The conditions for the parameter study are in parameterSetting.json. With the parameterSetting.json file selected in the Files area, open a text editor and enter PS settings mode.

Edit the velocity initial condition file U in the solve component to change the velocity. First, click the add new target file button. Select solve, type U in the text box, and click the OK button.

img

The U file opens in the left pane. In the line boundaryField -> inlet -> value, change 5 of uniform (5 0 0); to vel_U.

img

Drag the vel_U part of uniform (vel_U 0 0); to select it. The parameters text box in the right pane displays vel_U.

img

Now click the add new parameter button and enter the value you want to set for the inlet velocity. Set min=5, max=7, and step=1 to perform the parameter study in steps of 1m/s from 5m/s to 7m/s.

img

With these settings, the software automatically generates 5, 6, and 7 m/s velocity condition files and runs the analysis for each condition.

Collection of calculation results

Add a setting to aggregate the results calculated for each condition into a results folder set to output files. Click the add new gather setting button to display the gather settings dialog. Select solve, set srcName to D50-d10.tar.gz, and dstName to results/{{ vel_U }}/D50-d10.tar.gz.

img

This completes the editing of the PS configuration file. Click the save all files button at the top right of the screen to save your edits.

Configuring the extract Component

Create a script file for the extract component. To the extract component Create a new file named run.sh with the following contents:

for i in results/*
  do
    pushd $i
    tar xfz D50-d10.tar.gz
    popd
  enddo

This script sequentially expands the output of the solve component and prepares to launch ParaView.

Finally, open the component properties and set script to run.sh.

Setting File Dependencies

Sets input/output settings between components. Drop ▶ of constant set in the output files of convert into the PS component and connect it.

Also, drop ▶ of results set in outputFile of PS component into extract component and connect it.

This completes the workflow creation process. Click the save project button to save the project you created.

img

3. Running the Project

Click the run project button to run the project. First, you will be asked for the password for the private key you need to log in to Fugaku, but after that, no further action is required until the end of the workflow.

4. Checking Analysis Results

Review the analysis results.

To obtain the path of the calculation result file, open the extract component property screen, display the Files area, and navigate to the results directory -> Inflow Speed directory. The result.foam file appears below it, click to select it and click the share file button.

img

Displays the path to the result.foam file. When you click the Copy button, the file path is copied to the clipboard, so start ParaView with this file name as an argument.

img

Analysis Results

For reference, here are the visualization results for the inflow velocities of 5[m/s], 6[m/s], and 7[m/s].

In the analysis result of Inflow velocity 5[m/s], velocity U is displayed in the cross-sectional view of the distribution pipe and pressure p is displayed as a vector, and the result is as follows.

Inflow velocity 5[m/s]

img

Similarly, the results for Inflow velocity 6[m/s] and Inflow velocity 7[m/s] are shown.

Inflow velocity 6[m/s]

img

Inflow velocity 7[m/s]

img

That’s all for an example of a parameter study analysis workflow using OpenFOAM.

Return to Practical Tutorial

Updated: