HS-1550: Shape Optimization Study Using HyperMesh and Abaqus

This tutorial demonstrates how to perform a shape optimization using HyperMesh and HyperStudy. You will be using the finite element solver Abaqus, and HyperMorph to do the shape parameterization. This tutorial also demonstrates how to solve a problem when HyperMesh and HyperStudy are running in Windows and the solver is on a UNIX platform.

The files used in this tutorial can be found in <hst.zip>/HS-1550/. Copy the tutorial files from this directory to your working directory. The tutorial directory includes the following files:

link.hm	Original HyperMesh file.
HS-1550_solverScript.py	Basic Solver Script Setup (ONLY for LOCAL Machine) – Run everything on local machine (Windows or Unix)
run_abaqus.sh	(ONLY for REMOTE Machine) - Shell script which is designed to run the abaqus solver in the UNIX machine.
ssh_remote.bat	Advanced Solver Script Setup (ONLY for REMOTE Machine) – Run HyperStudy on Windows with Study Directory in Unix and the Solver is Running on Unix. Sample execution script to run Abaqus on UNIX.

In this tutorial, you will:

•	Use HyperMorph to generate a shape variable.

•	Run a study from inside HyperMesh.

•	Perform a shape parameterization using HyperStudy.

•	Set up a study.

•	Write a script to run Abaqus on UNIX and register the script in the preference file.

•	Run an optimization study.

The objective of this tutorial is to minimize the mass of a link that is connected to a shaft, given a stress constraint of 200MPa. The input variables are defined by the outer shape.

hs_1550_outershape

1.	Start HyperMesh Desktop.

2.	In the User Profiles dialog, set the user profile to Abaqus, Standard2D.

hs_1550_userprofile

3.	From the menu bar, click File > Open > Model.

4.	In the Open Model dialog, open the link.hm file. A finite element model appears in the graphics area.

hs-1550-finite-element-model

1.	From the Tool page, click HyperMorph.

hs_2010_hypermorph_panel

2.	Click domains. The Domains subpanel opens, from which you can create domains for the shape parameterization.

3.	Click the first arrow and select 2D domains.

4.	Click the toggle and select all elements.

hs_1550_domains

5.	Click create. Domains and handles are generated and will be used to manipulate the shape of the mesh and to generate shape perturbations required for the shape optimization.

hs-1550-domains-and-handles

6.	Click return.

7.	From the HyperMorph panel, click morph. The Morph subpanel opens, from which you can morph the shape of the mesh. The goal of the following steps is to create one input variable for the outer edge of the link.

8.	Click the second switch and select translate.

9.	In the y val= field, enter -5.0.

hs-1550-move-handles

10.	In the graphics area, click the yellow handle located at the top-right corner of the link as indicated in the image below.

hs_1550_rightcorner

11.	Click morph. The first shape is generated.

hs-1500-morphed-shape

12.	Click save shape.

13.	In the name= field enter, sh1.

14.	Click save.

To run the solver on a local machine, use the supplied python script HS-1550_solverScript.py, which calls the Abaqus solver using arguments specified that you specify.

Change the path in the file to the Abaqus executable on your machine.

Any additional arguments, such as memory requests, can be modified in the script as well.

# import statements

import os

import platform

import subprocess

import sys

# user edits-------------------------------------------------------------------

# set abaqus path

abaqus_exe = '/my/path/to/executable/abaqus.exe'

# set abaqus arguments

abaqus_arguments = 'job=' + sys.argv[1] + ' ' + 'memory=200Mb interactive'

# set log file name

logFile = 'logFile.txt'

# -----------------------------------------------------------------------------

# open log file

f = open('logFile.txt', 'w')

f.write('Hello world')

# get environment information

plat = platform.system()

hst_altair_home = ''

strEnvVal = os.getenv('HST_ALTAIR_HOME')

if strEnvVal:

hst_altair_home = strEnvVal

else:

f.write('%EXA_xx-e-env, Environment variable not defined ( HST_ALTAIR_HOME )')

abaqus_exe = os.path.normpath(abaqus_exe)

lstCommands = [abaqus_exe, abaqus_arguments]

# echo log information

f.write('platform: ' + plat + '\n')

f.write('hst_altair_home: ' + hst_altair_home + '\n')

f.write('abaqus command: ' + abaqus_exe + '\n')

#execute the command

f.write('Running the command:\n' + ' '.join(lstCommands) + '\n')

p1 = subprocess.Popen(lstCommands, stdout=subprocess.PIPE , stderr=subprocess.PIPE)

# log the standard out and error

f.write('\nStandard out' + '\n' + p1.communicate()[0] + '\n')

f.write('\nStandard error' + '\n' + p1.communicate()[1] + '\n')

# close log file

f.close()

(OPTIONAL - ONLY for REMOTE Machine): Advanced Solver Script Setup – Run HyperStudy on Windows with Study Directory in Unix and the Solver is Running on Unix.

In order to run commands on a remote Unix machine, a local program must be installed to communicate the commands remotely. In this example, the program ssh is being used, but other equivalent or better programs exist. In most cases, the program’s protocols require authentication from a password. For this setup to work the environment needs to be configured to work without an active password entry. This setup may require help from your network administrators.

The ssh_remote.bat file is a sample (Windows) batch file to run a script on Unix (run_abaqus.sh) from a HyperStudy session running on Windows.

ssh user_name@unix_machine “./run_abaqus.sh %1 %HST_APPROACH_VARNAM % %HST_STEP_INDEX% %HST_APPROACH_MODELS%”

The batch file uses the ssh command to log onto the Unix machine and execute the solver on the files created by HyperStudy. This script will be registered in HyperStudy as the solver script.

To use the sample script, change the following to match your setup:

1.	Change the generic parameter “unix_machine” to match the name of the remote Unix machine on your network.

2.	Change the generic parameter “user_name” to match your logon on the remote machine.

Note:

As mentioned above, this logon should have been configured to work without a password between these two machines.

The file run_abaqus.sh is a shell script which is designed to run the Abaqus solver on a UNIX machine. This file should be placed in your HOME directory on the Unix machine.

#!/bin/sh

#constuct the model directory

approachName=$1

runNum=`printf %04i $2`

modelString=$3

array=(${modelString//:/ })

modelName=${array[0]}

myDir=~/${approachName}/run_${runNum}/${modelName}

#change the directory to model directory

cd $myDir

#change the format from windows to unix

dos2unix $1 $1

#edit this line to match your solver path and the appropriate arguments

/my/path/to/solver/example/abaq631 job=$1 memory=200Mb interactive

Once there, perform the following:

1.	Change the text formatting to be Unix compatible using the command dos2unix on the file: dos2unix run_abaqus.sh.

2.	Make sure the file has executable permission. Type chmod 755 run_abaqus.sh.

3.	Edit the run_abaqus.sh file and modify the path to the executable and any other options to this command as needed.

1.	Start Hyperstudy.

2.	From the menu bar, click Edit > Register Solver Script.

3.	In the Register Solver Script dialog, click Add Solver Script.

4.	In the HyperStudy - Add dialog, enter Abaqus in the Label and Varname fields.

5.	For solver script type, select Generic.

Click OK.

hs_1550_registersolverscript

7.	In the Path column of the script Abaqus, click .

8.	In the Open dialog, open the python.exe file.

Note:

You can also copy and paste the same path and file from the Python Path field.

hs-1550-register-solver-script

9.	In the Argument column of the Abaqus script, click .

10.	In the Open dialog, navigate to your working directory and open the HS-1550_solverScript.py file.

11.	Click Save.

12.	In the Save Preferences dialog, navigate to your working directory.

13.	In the File name field, enter a label for the new user preference file (example: userprefs.mvw).

14.	Click Save.

Note:

Do not overwrite the system preferences file, which is located in <install_directory>/hw by default.

15.	Click Close.

16.	Optional - ONLY for REMOTE Machines: Register Abaqus as a solver.

hs-1550-register-solver-script2

1.	To start a new study, click File > New from the menu bar, or click on the toolbar.

2.	In the HyperStudy – Add dialog, enter a study name, select a location for the study, and click OK.

Note:

The study directory MUST be your home on the mapped UNIX machine.

3.	Go to the Define models step.

4.	Add a HyperMesh model.

a.	From the Directory, drag-and-drop the HyperMesh (.hm) file link.hm into the work area.

hs_1550_drag_drop_model

b.	In the Solver input file column, enter link.inp. This is the name of the solver input file HyperStudy writes during any evaluation.

c.	In the Solver execution script column, select Abaqus.

d.	In the Solver input arguments column enter, $filebasename.

hs_1550_definedesignvariables

Optional. In addition, you may need to edit the Abaqus environment file (ex: <ABAQUS INSTALL>\v6.11\6.11-1\site\abaqus v6.env) to include:

ask_delete=OFF

comment the line ask delete=on if any.

This is needed because Abaqus prompts you to overwrite the old files when re-running the analysis. In order to eliminate the need for user interaction, you need to command Abaqus not to ask this question and overwrite.

5.	Click Import Variables.

6.	In the Model Parameters dialog, select parameters to import into HyperStudy.

a.	Expand Shape, and click sh1.S.

b.	Verify that the Lower bound is 0.0 and the Upper bound is 1.0.

c.	Click Add.

Click OK.

hs_1550_modelparameters

7.	Go to the Define Input Variables step.

8.	Review the design variable's lower bound, initial and upper bound range.

9.	Go to the Specifications step.

1.	In the work area, set the Mode to Nominal Run.

2.	Click Apply.

3.	Go to the Evaluate step.

4.	Click Evaluate Tasks.

5.	Go to the Define Output Responses step.

In this step you will create two output responses: Mass and Max_Stress.

1.	Create the Mass output response.

a.	From the Directory, drag-and-drop the link.inp file, located in the approaches/nom_1/run__00001/m_1 directory, into the work area.

b.	In the File Assistant dialog, set the Reading technology to Altair® HyperWorks® and click Next.

c.	Select Single item in a time series, then click Next.

d.	Define the following options, and then click Next.

•	Set Type to ABAQUS.dat.

•	Set Request to TOTAL MASS.

•	Set Component to MASS.

e.	Label the output response Mass.

f.	Set Expression to First Element.

g.	Click Finish. The Mass output response is added to the work area.

2.	Create the Max_Stress output response.

a.	From the Directory, drag-and-drop the link.obd file, located in the approaches/nom_1/run__00001/m_1 directory, into the work area.

b.	In the File Assistant dialog, set the Reading technology to Altair® HyperWorks® and click Next.

c.	Select Multiple items at multiple time steps (readsim), then click Next.

d.	Define the following options, and then click Next.

•	Set Subcase to Step-2.

•	Set Type to S-Global-Stress components (PART-1-1).

•	Set Request to E1 - E378.

•	Set Component to vonMises.

e.	Label the output response Max_Stress.

f.	Set Expression to Maximum.

g.	Click Finish. The Max_Stress output response is added to the work area.

3.	Click Evaluate Expressions to extract output response values.

1.	In the Explorer, right-click and select Add Approach from the context menu.

2.	In the HyperStudy - Add dialog, select Optimization and click OK.

3.	Go to the Select Input Variables step.

4.	Review the input variable's lower and upper bound ranges.

5.	Go to the Select Output Responses step.

6.	Click Add Objective.

7.	In the HyperStudy - Add dialog, add one objective.

8.	Define the objective.

a.	Set Type to Minimize.

b.	Set Apply On to Mass (r_1).

hs_1550_obj1

9.	Click the Constraints tab.

10.	Click Add Constraint.

11.	In the HyperStudy - Add dialog, add one constraint.

12.	Define the constraint.

a.	Set Apply On to Max_Stress ( r_2).

b.	Set Bound Type to <= (less than or equal to).

c.	For Bound Value, enter 200.0.

hs_1550_constraint

13.	Click Apply.

14.	Go to the Specifications step.

15.	In the work area, set the Mode to Adaptive Response Surface Method (ARSM).

Note:

Only the methods that are valid for the problem formulation are enabled.

16.	Click Apply.

17.	Go to the Evaluate step.

18.	Click Evaluate Tasks to start the Optimization.

1.	Click the Iteration History tab to review the Optimization results. The optimal design in highlighted green.

2.	Click the Iteration Plot tab to plot the Optimization results. Use the Channel selector to select Constraint 1 and Objective 1.

hs_1550_iterationplot

HS-1550: Shape Optimization Study Using HyperMesh and Abaqus

HS-1550: Shape Optimization Study Using HyperMesh and Abaqus

HS-1550: Shape Optimization Study Using HyperMesh and Abaqus

(OPTIONAL - ONLY for REMOTE Machine): Advanced Solver Script Setup – Run HyperStudy on Windows with Study Directory in Unix and the Solver is Running on Unix.

See Also: