The simple beam problem introduced earlier illustrates a probabilistic design analysis.

Young's modulus is 20E4.

PREP7 is used to build the model in terms of the RV parameters. For our beam example, the RV parameters are H1 (snow height at left end), H2 (snow height at right end), and the Young's modulus E.

...
!  Initialize ANSYS parameters:
H1=100                       ! Initialize snow height H1 @ left end (in mm)
H2=100                       ! Initialize snow height H2 @ right end(in mm)
YOUNG=200.0e3                ! Initialize the Young's modulus (in N/mm**2)
ROOFWDT=1000.0               ! Initialize roof width left and right of beam (in mm)
BWDT=10.0                    ! Initialize beam width (in mm)
BHGT=40.0                    ! Initialize beam height (in mm)
BLEN=3000.0                  ! Initialize beam length (in mm)
SNOWDENS = 200e-9            ! Density of snow (200 kg/m**3)
GRAVACC  = 9.81              ! Earth gravity (in N/kg)
LOAD1 = H1*GRAVACC*ROOFWDT*SNOWDENS  ! Pressure load due to snow @ left end
LOAD2 = H2*GRAVACC*ROOFWDT*SNOWDENS  ! Pressure load due to snow @ right end
DELLOAD = LOAD2-LOAD1
!
! Material definitions:
MP,EX,1,YOUNG                ! Young's modulus
MP,PRXY,1,0.3                ! Poisson's ratio
!
! Create the geometry (a line)
K,1,0,0,0                    ! keypoint at left end
K,2,BLEN,0,0                 ! keypoint at right end
L,1,2,100                    ! line between keypoints
!
! Mesh definitions
ET,1,BEAM3                   ! 2-D beam element
AREA=BWDT*BHGT               ! Beam cross-sectional area
IZZ=(BWDT*(BHGT**3))/12      ! Moment of inertia about Z
R,1,AREA,IZZ,BHGT            ! Real constants in terms of RV parameters
LATT,1,1,1
LMESH,1                      ! mesh the line
FINISH                       ! Leave PREP7
...

As mentioned earlier, you can vary virtually any aspect of the design: dimensions, shape, material property, support placement, applied loads, etc. The only requirement is that the design be defined in terms of parameters. The RV parameters (H1, H2, and E in this example) may be initialized anywhere, but are typically defined in PREP7.

The SOLUTION processor is used to define the analysis type and analysis options, apply loads, specify load step options, and initiate the finite element solution. All data required for the analysis should be specified: master degrees of freedom in a reduced analysis, appropriate convergence criteria for nonlinear analyses, frequency range for harmonic response analysis, and so on. Loads and boundary conditions may also be RVs as illustrated for the beam example here.

The SOLUTION input for our beam example could look like this:

...
/SOLU
ANTYPE,STATIC                  ! Static analysis (default)
D,1,UX,0,,,,UY                 ! UX=UY=0 at left end of the beam
D,2,UY,0,,,,                   ! UY=0 at right end of the beam
!D,2,UX,0,,,,UY                ! UX=UY=0 at right end of the beam
elem=0
*get,numele,ELEM,,COUNT
*DO,i,1,numele
  elem=elnext(elem)            ! get number of next selected element
  node1=NELEM(elem,1)          ! get the node number at left end
  node2=NELEM(elem,2)          ! get the node number at right end
  x1 = NX(node1)               ! get the x-location of left node
  x2 = NX(node2)               ! get the x-location of rigth node
  ratio1 = x1/BLEN
  ratio2 = x2/BLEN
  p1 = LOAD1 + ratio1*DELLOAD  ! evaluate pressure at left node
  p2 = LOAD1 + ratio2*DELLOAD  ! evaluate pressure at left node
  SFBEAM,elem,1,PRES,p1,p2     ! Transverse pressure varying linearly
                               ! as load per unit length in negative Y
*ENDDO
SOLVE 
FINISH                         ! Leave SOLUTION
...

This step is not limited to just one analysis. You can, for instance, obtain a thermal solution and then obtain a stress solution (for thermal stress calculations).

If your solution uses the multiframe restart feature, all changes to the parameter set that are made after the first load step will be lost in a multiframe restart. To ensure that the correct parameters are used in a multiframe restart, you must explicitly save (PARSAV) and resume (PARESU) the parameters for use in the restart. See the Basic Analysis Guide for more information on multiframe restarts.

This is where you retrieve results data and assign them to random output parameters to be used for the probabilistic portion of the analysis. Use the *GET command (Utility Menu> Parameters> Get Scalar Data), which assigns ANSYS calculated values to parameters, to retrieve the data. POST1 is typically used for this step, especially if the data are to be stored, summed, or otherwise manipulated.

In our beam example, the maximum deflection and the maximum stress of the beam are random output parameters (RPs). The parameters for these data may be defined as follows:

...
/POST1
SET,FIRST
NSORT,U,Y               ! Sorts nodes based on UY deflection
*GET,DMAX,SORT,,MIN     ! Parameter DMAX = maximum deflection
!
! Derived data for line elements are accessed through ETABLE:
ETABLE,VOLU,VOLU        ! VOLU = volume of each element
ETABLE,SMAX_I,NMISC,1   ! SMAX_I = max. stress at end I of each 
                        !  element
ETABLE,SMAX_J,NMISC,3   ! SMAX_J = max. stress at end J of each 
                        !  element
!
ESORT,ETAB,SMAX_I,,1    ! Sorts elements based on absolute value 
                        !  of SMAX_I
*GET,SMAXI,SORT,,MAX    ! Parameter SMAXI = max. value of SMAX_I
ESORT,ETAB,SMAX_J,,1    ! Sorts elements based on absolute value 
                        !  of SMAX_J
*GET,SMAXJ,SORT,,MAX    ! Parameter SMAXJ = max. value of SMAX_J
SMAX=SMAXI>SMAXJ        ! Parameter SMAX = greater of SMAXI and    
                        !  SMAXJ, that is, SMAX is the max. stress
FINISH
...

See the *GET and ETABLE commands for more information.

If you choose to create your model interactively in ANSYS, you must now derive the analysis file from the interactive session. Use the command log or the session log file to do so. For more information on using these log files, see "Using the ANSYS Session and Command Logs" in the Operations Guide.

You can use the Probabilistic Method Determination Wizard to find the fastest method for solving your probabilistic analysis. You should have completed one analysis prior to starting the wizard.

Use Main Menu> Prob Design> Prob Method> Methods Wizard to access the wizard. Answer the questions on the screens as they are presented. Before you start the wizard, you should know:

Below is one of the wizard screens, as an example.

Based on the information you provide, the wizard will tell you the fastest method for solving your probabilistic design problem. The wizard will issue the PDMETH command and either the PDLHS or the PDDOEL command. You will still need to run the analysis, then fit the results to a response surface, etc. to evaluate your results.

Regardless of whether you opt for serial or parallel processing, ANSYS controls the analysis looping; you cannot modify this process. It does the following:

For the execution of the simulation loops you must specify a solution label (Slab on the PDEXE command). The solution label is used for several purposes:

When you execute the probabilistic analysis (PDEXE), ANSYS creates a probabilistic design loop file (Jobname.LOOP) from the analysis file. This loop file is used to perform analysis loops. Looping continues until all parameters have been evaluated.

If a loop is interrupted due to an error in the execution run (for example, a meshing failure, a non-converged nonlinear solution, etc.), ANSYS PDS aborts that loop. Further processing depends if you are in serial or parallel processing mode. If you are using:

Note that for all failed loops (loops with errors), the results for that loop are discarded, no data from that loop is used for post processing.

After the PDEXE command is issued, the PDS generates a file containing the input sample values. The file is called jobname.samp. An example of the content of the file is given below:

TEST1
ITER CYCL     LOOP                X1                X2                X3
   1    1        1  1.619379209e+000  2.364528435e-001  1.470789050e+000
   1    1        2  2.237676559e-001  5.788049712e-001  1.821263115e+000
   1    1        3  7.931615474e+000  8.278689033e-001  2.170793522e+000
  ..   ..       ..               ...               ...               ...
  ..   ..       ..               ...               ...               ...

The first line contains the solution label (the parameter Slab is set via the PDEXE command); the second line contains the headers of the data columns - the iteration number, cycle number, loop number, and the random variable names. The iteration number and cycle number tell the PDS to which group (with specific PDS method and settings) the loops belong. Subsequent lines provide specific iteration, cycle, loop, and input sample values for the defined input variables.

The PDS also creates a file where the results are stored. The name of the results file is jobname_Slab.pdrs. Before the job is executed, the file looks like this:

TEST1
  ITER CYCL     LOOP ERR            X1           X2           X3       RESULT

In the first line, the PDS enters the solution label. In the second line are the headers for the data columns: the first four columns are the iteration, cycle number, loop number, and an error flag. The fifth and subsequent columns are for the random input variable and random output parameter values. If you run a subsequent analysis (same type of analysis with the same solution label), the cycle is incremented, the loop count is reset to 1, and the result file is appended.

For example, the content of the result file could look like this:

TEST1
ITER CYCL     LOOP ERR                X1                X2                X3            RESULT
   1    1        1   0  1.619379209e+000  2.364528435e-001  1.470789050e+000  4.162928057e+000
   1    1        2   0  2.237676559e-001  5.788049712e-001  1.821263115e+000  4.744249212e+000
   1    1        3   0  7.931615474e+000  8.278689033e-001  2.170793522e+000  1.149997825e+001
  ..   ..       ..  ..               ...               ...               ...               ... 
  ..   ..       ..  ..               ...               ...               ...               ... 

Serial execution of the probabilistic analysis is useful for smaller models, or if you have access to only one machine.

To save time when analyzing large models with PDS, use the parallel processing option available under the PDEXE command, if you have multiple CPUs available.

To successfully execute a probabilistic analysis in parallel mode you need to follow three steps:

Each of these steps is explained in detail in the following sections.

An understanding of the following terms will be useful in the discussion of the parallel analysis.

3.3.9.3.1. Machine Configurations

The slave machines host one or more child processes. To be able to host a child process the slave machine must have the ANSYS Thin Server running. The ANSYS Thin Server may be started automatically using the remote shell option or manually using the connection port option.

3.3.9.3.1.1. Choosing Slave Machines

You can designate any machine that has a licensed copy of ANSYS installed as a remote host (slave machine) but it is a good practice to follow these guidelines when selecting remote hosts:

• Use idling computer power. During regular work hours, computers usually have designated "owners" using the machines for interactive work. Using these computers for parallel processing can slow down the machine performance and possibly disturb your colleagues in their work. However, computers are usually idle at night and can then be used without disturbing others.

• Use machines that are dedicated as computer servers. There might be some computers in your work environment that are not used for interactive work at all. It is fairly safe to use these computers as remote hosts for parallel-processing at all times.

• Check with your System Administrator for additional guidelines.

3.3.9.3.1.2. Using the Remote Shell Option

With this option the ANSYS Thin Server is started and configured to communicate with the Master machine automatically. To use the remote shell option requires the following on each slave machine:

• A remote shell daemon must be running

• An account that the master machines remote shell command can communicate with

• The master machine and user name must be granted access for the account

• The installation path for the ANSYS executable must be in the lookup path

• A valid ANSYS license available for the child process

Remote Shell Daemon

Your system administrator should install and configure your machine to assure that this daemon or service is running. The PC does not ship with a remote shell daemon facility so you will need to acquire one (you may use the connection port ooption instead).

---

Back To Top

Account

Your system administrator should create an account specifically for you or an account utilized only for PDS parallel.

---

Back To Top

Account Access

Depending on how and which remote shell daemon is installed it will need to know which master machines and users can access this account. This is typically done using the .rhosts file located in the account's HOME directory, refer to the documentation for your particular remote shell daemon. So for example:

On all slave machines edit/create the ".rhosts"-file in your home directory to include:

MasterMachine1 UserId

MasterMachine2 UserId

MasterMachine3 UserId

MasterMachine4 UserId

…

each on a separate line. This will allow the user with the account user identification UserId to access the slave machine from the master machines listed in the file using the remote shell service.

---

Back To Top

ANSYS in PATH

To be able to run the parallel process the ANSYS executable and ANSYS Thin Server script must be in your path. The most effective way to determine this is to do the following.

Determining if the ANSYS executable is in your path:

On the master machine use the command "rsh SlaveMachine which ansys110" (replace rsh by remsh if master machine is an HP machine). This should return the string

…/ansys110/bin

Here "…" is for the directory where ANSYS is installed. If you do not get this then you need to modify your PATH variable to contain the installation path. The way this is done depends on the operating system being used, refer to the documentation for your particular O/S environment. Here are some examples for typical uses:

---

Back To Top

UNIX

To change the PATH requires you to modify a certain system file depending which shell you are running under. To find out which shell you are using, issue the UNIX command

echo $shell or echo $SHELL

If the prompt is "/bin/csh" or similar, then you are running under c-shell. If the prompt is "/bin/ksh" or similar, then you are running under k-shell. If the prompt is "/bin/tcsh" or similar, then you are running under tc-shell, which can be treated the same as c-shell.

If you are running under c-shell (or tc-shell) you need include the following line at the end of your ".cshrc"-file in your home directory:

set path=( .../ansys110/bin $path)

If you are running under k-shell you need include the following line at the end of your ".kshrc"-file in your home directory:

export PATH={ .../ansys110/bin $PATH }

If you don't have a ".cshrc"-file or ".kshrc"-file in your home directory, then you need to create one and include the respective commands mentioned above.

---

Back To Top

PC

To change the PATH variable go to Control Panel and choose System on the Advanced tab choose Environment Variables and add the ANSYS executable to the PATH under System variables.

Determining if the ANSYS Thin Server script is in your path:

On the master machine issue the command "rsh SlaveMachine which ansysts110". This should return the string

…/ansys110/bin

Here "…" is for the directory where ANSYS is installed. If you do not get this then you need to modify your PATH variable as outlined above.

---

Back To Top

Licensing

If the licensing is not managed from a license server, but installed locally then the access to the license must be made available. Include the following line at the end of your ".cshrc"-file or ".kshrc-file in your home directory depending which shell you are running under (see above):

setenv ANSYSLMD_LICENSE_FILE. ../shared_files/licensing/FileName.lic

Here "…" is for the directory where ANSYS is installed. The name "FileName.lic" is for the file containing the license key.

3.3.9.3.1.3. Using the Connection Port Option

With this option the communication between the ANSYS Nanny and the ANSYS Thin Server is manually configured and started. The ANSYS Nanny running on a master machine can only make a connection to an ANSYS Thin Server using a specific connection port. The ANSYS Nanny reads the connection port from the "hosts110.ans"-file. When the ANSYS Thin Server is started, with the same specific connection port, it reads the file "AnsysClients" from the same directory it is started within to determine the communication ports and master machines with which it will communicate.

The purpose of these two different port numbers is a two-level authentication mechanism. You can only use an ANSYS Thin Server on a certain slave machine, if you know which connection port it is using and those communication ports from which it will accept communications. If the connection port is not correct, then you will not be able to even make a connection to the ANSYS Thin Server. If the communication port number is incorrect, then the ANSYS Thin Server will refuse the connection.

To use the connection port option requires the following on each slave machine:

• An account that you have access to

• The installation path for the ANSYS executable must be in the lookup path

• Configuring the AnsysClients file

• A valid ANSYS license available for the child process

• Start the ANSYS Thin Server

• Stop the ANSYS Thin Server

Account

Your system administrator should create an account specifically for you.

---

Back To Top

ANSYS in PATH

See Using the Remote Shell Option for information on how to place the ANSYS executable in your path.

---

Back To Top

AnsysClients

The AnsysClients file is read by the ANSYS Thin Server on startup and must be in the directory in which you are going to run the ANSYS Thin Server. This file must contain a list of each master machine IP address and the communication port that the ANSYS Thin Server will accept communications from. The master machine's IP address must be used, but may be specified with a wildcard to allow connection from a network domain. The communication port is to be a value between 49512 and 65535. The communication port can also be specified as a range, which allows for that many connections. It is best to always specify a range for the communication port numbers. For example:

10.3.* 59100-59130

10.3.20.1 59200-59230

10.2.5.55 59300-59330

10.1.1.104 59400-59430

192.1.10.34 59500-59530

…

…

Make sure that the port number ranges are not overlapping and are unique for each master machine or network domain. You should make the range at least as wide as the number of possible users connecting from a master machine.

---

Back To Top

Start the ANSYS Thin Server

Starting on a PC

On a PC open a command prompt window and go to the directory containing the AnsysClients file mentioned above.

Issue the command: ansysts110 connection port

This will start the ANSYS Thin Server using the specific connection port. The value of connection port is the port on which the master machines will connect to the ANSYS Thin Server. The value of "connection_port" should be between 49512 and 65535. For example:

ansysts110 62000

The ANSYS Thin Server will start without any message and will continue running until the command prompt window is closed or using Ctrl-C to stop the process. The command prompt window may be minimized.

Starting on a UNIX Machine

On a UNIX machine go to the directory containing the AnsysClients file mentioned above.

Issue the command: ansysts110 connection_port &

This will start the ANSYS Thin Server using the specific connection port. The value of connection port is the port on which the master machines will connect to the ANSYS Thin Server. The value of "connection_port" should be between 49512 and 65535. For example:

ansysts110 62000&

The ANSYS Thin Server will start without any message and will continue running in the background until the machine is restarted or you kill the process. You may close or minimize the window in which the ANSYS Thin Server was started.

---

Back To Top

Stop the ANSYS Thin Server

The ANSYS Thin Server should be stopped once the parallel process is complete.

Stopping on a PC

You may stop the process by closing the command prompt window or using Ctrl-C.

Stopping on a UNIX Machine

On a UNIX machine use a "ps -u UserId | grep tclsh" in the command line to find out under which process-id the ANSYS Thin Server is running. Here, UserId is your user account name on the machine. With this "ps" command should get two processes running. Typically, there will be two processes listed, one process for "anstclsh" and another for "tclsh". Use "kill -9 process-id" to kill both processes. Under certain circumstances killing the "anstclsh"-process will also take away the "tclsh"-process (just issue the "ps" command again to verify). If this does not happen, then just kill the "tclsh"-process separately.

3.3.9.3.1.4. Configuring the Master Machine

After you have configured the slave machines you need to configure the master machine for the type of ANSYS Thin Server startup you chose to use on the slave machines. The communication from the master machine to the slave machines is done by the ANSYS Nanny which is a program running in the parent process. It takes care of running the necessary simulations on different slave machines. It will establish the connection to the slave machines, copy the necessary files over to the slave machines, start and monitor the running simulations and clean up the working directories after the entire sequence of simulations is finished. The ANSYS Nanny will be started automatically as you start executing PDS simulations in parallel, distributed mode.

For parallel processing you need to specify the remote hosts you want to use. This information is placed in a file called hosts 110.ans. You can create this file using a text editor or you can use the ANS_ADMIN utility (see the online help available with the ANS_ADMIN utility for more information). This file contains host information for all remote machines on which you may want to run. This file is global and does not contain job-specific information. Typically, your IT administrator would provide this file, including all the information about the slave machines a typical user can use in your network. If you have multiple users running parallel or distributed jobs at your site, you should have one hosts 110.ans file for all users. But you can copy this file to your local working directory and make adjustments. ANSYS searches for this file first in the local directory, followed by the home directory, and finally the apdl directory.

You have two options when setting up the Master Machine to use the ANSYS Thin Server on the slave machines.

Configuration when the Thin Server uses the Remote Shell Option

Let's assume that the slave machine called "MySlaveMachine" has been prepared to work under the remote shell option as outlined above. The slave machine "MySlaveMachine" is an SGI UNIX machine and it has 4 CPUs. On the slave machine we also want to use the directory "/tmp/sdr/pds_runs" as the local directory for the remote simulations to run in. In this case your hosts 110.ans file must include the line:

#
# HOST	OS	PORT	CPU	TIME	LocPORT	I/O Directory
MySlaveMachine	SGI64	0	4	15	0	/tmp/sdr/pds_runs

---

Back To Top

Configuration when the Thin Server uses the Port Option

Let's assume you now want to use the same slave machine "MySlaveMachine" using the ANSYS Thin Server. The ANSYS Thin Server has been started on a slave machine called "MySlaveMachine" using the command "ansysts110 62000as illustrated above. Let us also assume that the file "AnsysClients" looks exactly like shown in the section above, i.e. your master machine "MyMasterMachine" can communicate to the ANSYS Thin Server using the communication port numbers 59400-59430. In this case your hosts 110.ans file must include the line:

#
# HOST	OS	PORT	CPU	TIME	LocPORT	I/O Directory
MySlaveMachine	SGI64	62000	4	15	59400-59430	/tmp/sdr/pds_runs

This will make sure that the ANSYS Thin Server on the slave machine will be contacted using the same connection port it has been started with, i.e. 62000 in this case. Also the communication will use the same communication port numbers the ANSYS Thin Server accepts from the machine "MyMasterMachine" where you try to connect from.

A sample hosts110.ans file looks like this:

# This file is used to specify those hosts that the ANSYS Nanny may
# run children on.
#
# Each host entry is to be on its own line.  The host entry consists of
# several fields which are space delimited.
#
#  Field 1 - host IP address or name
#  Field 2 - host machine type
#  Field 3 - execution key (used for Probabilistic Design only):
#        0-Use a remote shell to start the child process;
#          this requires a remote shell server to be
#          running on the host machine.
#    >1024-Use a running ANSYS thin server on the host
#          which is listening on this port number.
#  Field 4 - The default maximum number of jobs to run on this host
#  Field 5 - The time in minutes to check again if the host is available.
#            If this is zero then the host will not be checked again.
#  Field 6 - The local port number to start the communication with the
#            ANSYS Thin Server on. This is tied to authentication on the
#            ANSYS Thin Server.
#  Field 7 - The directory to create the children subdirectories in
#  Field 8 - The cluster type.  Only valid entry is MPI.
#  Field 9 - The speed factor (relative speed to other machines listed).
              Only valid entry is 1.
#  Field 10 - Number of OpenMP threads.  Only valid entry is 1.
# Example:
#
#  UNIX box that has five processors
#  zeus  sgi64    0     5  30    2000     /scratch/wjc
#  Microsoft box using the ANSYS Thin Server
#  wjcpc XP       2010  1  0     2000     C:\TEMP
alpha1   alpha    0      1     15    2000     /scratch/epc   MPI 1 1
athena   sgi64    0      1     15    2000     /scratch/epc   MPI 1 1
rs43p    rs6000   0      1     15    2000     /home/pdstest  MPI 1 1
rs260    rs64     0      1     15    2000     /home/pdstest  MPI 1 1
snoopy   hppa8000 0      1     15    2000     /home/pdstest  MPI 1 1
alpha24  alpha    0      1     15    2000     /home/pdstest  MPI 1 1
hp770    hppa8000 0      1     15    2000     /home/pdstest  MPI 1 1
us60     usparc   0      1     15    2000     /home/pdstest  MPI 1 1
ss60     sun64    0      1     15    2000     /home/pdstest  MPI 1 1

3.3.9.3.1.5. Illustration of the host set-up using port option

The picture below illustrates an example of the set-up of a network with 2 master machines and 4 slave machines using the connection port option. Here, the first master machines uses slave machines 1, 2 and 3, while the second master machine is using only slave machines 2, 3 and 4. In this illustration "NN" represents the revision number of ANSYS.

3.3.9.3.1.6. Host and Product selection for a particular analysis

After the host110.ans file is specified you need to provide specific information that may change from analysis to analysis.

If you are working in interactive mode then select:

Main Menu> Prob Design> Run> Exec Parallel> Host Select

In this menu you can:

• Select the slave machines you want to use for a particular analysis. This is necessary, for example, if you know that some machines in your network are in use by another user at the time you want to start the analysis.

• Choose the licenses you want to use for the particular analysis. If there are multiple levels of licenses of ANSYS available in your network, then you should first select the lower license that will be able to run your analysis.

Based on the information provided in this menu a Jobname.hosts file is created or updated as you press OK in the menu.

If you are working in batch mode, you must create this file using a text editor. However, for sake of simplicity it is recommended to let ANSYS create this file using interactive mode and then to proceed with batch mode operation. This file must reside in the directory where you are running ANSYS PDS. This file must include the following information:

• Remote hosts to be used for this particular parallel run.

• Number of processes that can run in parallel on each host. If a remote host has more than one CPU, you can use all of the CPUs on the remote host. For performance reasons, we recommend leaving one CPU for system tasks and using only N-1 CPUs for parallel processing (if N is the number of CPUs on the remote host).

• Directories in which you want the child processes to be executed. It is recommend that you use temporary directories like "/scratch" or "/tmp" on UNIX or "C:\TEMP" on PCs. These remote directories are cleaned up automatically after the parallel processes finish running. Make sure that there is enough disk space in the directory for the files created by the analysis.

A sample jobname.hosts file looks like this:

# This file is used to specify those hosts that the ANSYS Parent may
# run children processes on.
#
# Each host entry is to be on its own line. The host entry consists of
# several fields which are space delimited.
#
# Field 1 - host IP address or name
# Field 2 - username to use for a remote shell to the host
# Field 3 - execution key:
# 0 - Use a remote shell to start the child process
# >1024 - Use a running ANSYS thin server on the host
# which is communicating on this port number
# Field 4 - the product code sequence to attempt to start ANSYS jobs
# on the host with. This is a colon delimited list.
# Field 5 - the number of jobs to run on this host
# Field 6 - The time in minutes to check again if the host is available.
# If this is zero then the host will not be checked again.
# Field 7 - If field 3 is nonzero then this is the local port number
# or range to start the communication with the ANSYS Thin
# Server on. This is tied to the "authentication" on the
# ANSYS Thin Server.
# If field 3 is zero then this should be set to zero.
# Field 8 - directory to create the children subdirectories in
#
# Example:
#
# UNIX box that has five processors and will first attempt to
# run with ANSYS Mechanical Batch Child and then ANSYS Mechanical
# zeus wjc 0 MEBACH:ANSYS 5 30 2000 /scratch/wjc
# XP box running the thin server on port 2010
# wjcpc wjc 2010 ANSYS 1 0 2000 C:\TEMP
alpha1 epc 0 MEBA:MEBACH 1 15 2000 /scratch/epc
athena epc 0 MEBA:MEBACH 1 15 2000 /scratch/epc
rs43p pdstest 0 MEBA:MEBACH 1 15 2000 /home/pdstest
rs260 pdstest 0 MEBA:MEBACH 1 15 2000 /home/pdstest
snoopy pdstest 0 MEBA:MEBACH 1 15 2000 /home/pdstest
hp160 pdstest 0 MEBA:MEBACH 1 15 2000 /home/pdstest
alpha24 pdstest 0 MEBA:MEBACH 2 15 2000 /home/pdstest
hp770 pdstest 0 MEBA:MEBACH 1 15 2000 /home/pdstest
us60 pdstest 0 MEBA:MEBACH 1 15 2000 /home/pdstest
ss60 pdstest 0 MEBA:MEBACH 1 15 2000 /home/pdstest

# Files to copy to the ANSYS server for job Jobname
# created on Fri Oct 13 10:33:44 EDT 2000.
pdsrun1.inp
/home/staff/epc/ddts/pds/tags

The results generated by the response surface fitting procedure as well as the results generated by applying the approximation equation (Monte Carlo Simulation) are combined in a response surface set. Each response surface set includes the following information:

There is a one-to-one relationship between solution sets and response surface sets. For each solution set containing sample points you can have only one response surface set containing the response surfaces fitting these sample points. The reverse is also true, that each response surface set can only contain the response surfaces that are based on the sample points of one solution set.

To fit a response surface you must specify a name for the response surface set where you want the results to be stored, the solution set you want to use, one random output parameter, the regression model, an output transformation technique (if any), and whether to filter terms.

The regression model describes which regression terms are used for the approximation function of the response surface. In the ANSYS PDS, the following regression models are implemented:

While you can use all terms included in the regression model, the ANSYS PDS also offers an option that automatically filters out insignificant terms. This technique is called the forward-stepwise regression analysis. For example, where the Young's modulus E and the thermal expansion coefficient are random input variables, a full quadratic regression model reads:

A full regression model uses the available sampling points to determine values for all regression coefficients c₀ to c₃. Of course the values for c₀ to c₂ will be zero or very close to zero; taking more coefficients into account than really necessary reduces the degrees of freedom of the algebraic equation to be solved to evaluate the coefficients. This in turn reduces the accuracy of the coefficients that are important for the regression fit. The forward-stepwise regression analysis takes this into account and automatically eliminates terms that are not needed.

The ANSYS PDS offers a variety of transformation functions that can be used to make the random response parameter to be more appropriately described by a quadratic function after the transformation has been applied. These transformation functions can be found in Transformation of Random Output Parameter Values for Regression Fitting in the Theory Reference for ANSYS and ANSYS Workbench.

Here, y_i is the value of a random output parameter obtained in the i-th sampling loop and is the corresponding transformed value. The physical nature of the problem should indicate which transformation to use; for example, lifetime parameters (such as the number of cycles until low cycle fatigue occurs) are usually transformed with a logarithmic transformation. If you do not have this kind of information, then you should start with the Box-Cox transformation. The PDS automatically searches for an optimum value for the Box-Cox parameter λ within the interval (-2,2). As guidelines:

To fit a response surface:

Whether a response surface is a good representation of the sampling point that it is supposed to fit can be best illustrated by plotting the response surface. The ANSYS PDS plots the sampling points as symbols and the response surface as a contour plot so you can visually compare them. However, you can only plot one random output parameter as a function of two random input variables at a time.

To plot a response surface:

After using a regression analysis to fit a response surface, ANSYS automatically prints all necessary results in the output window:

The goodness-of-fit measures provide a means to verify the quality of the response surface and whether it is a good representation of the underlying data (in other words, the sample points).

You can request a print out of this data at any time.

After you have generated a response surface set that includes one or more response surfaces for one or more random output parameters then you also need to perform Monte Carlo Simulations using these response surfaces to generate probabilistic results. This is where the PDS generates sampling values for the random input variables in the same way it did for the simulation looping performed using your analysis file. But instead of using the random input variable values in the analysis file and running through the analysis file, it uses the approximation function derived for the response surfaces to calculate approximated response values. The process of calculating an explicitly known equation is much faster than running through the analysis file and performing a finite element analysis, so you can run a large number of simulation loops in a relatively short time. Usually, several thousand simulation loops are performed if you utilize the response surfaces.

After you have generated the Monte Carlo Simulation loops on the response surfaces, you can begin probabilistic postprocessing and review the probabilistic results the same way as you would for Monte Carlo Simulations. However, there is one difference for postprocessing between Monte Carlo results and Monte Carlo results derived from response surface approximations. For Monte Carlo simulation results, the accuracy of the results is determined by the number of simulation loops that are performed. The PDS can visualize the accuracy of Monte Carlo results by means of confidence limits or confidence bounds. For Monte Carlo results derived from response surface approximations, the confidence bounds are suppressed. This is necessary because the accuracy is not determined by the number of simulation loops (as mentioned above, you typically perform a large number of these) but by the goodness-of-fit or the response surface model itself. With increasing numbers of simulation loops the confidence bounds tend to merge with the result curve you are plotting (the width of the confidence band shrinks to zero). This could lead you to conclude that the results are very, very accurate. However, the underlying response surface approximation could have been completely inadequate (for example, using a linear approximation function for a highly nonlinear problem).

To postprocess one particular design variable, choose this option. The statistics options are described below.

Plot Sample History

Use the PDSHIS command to request a sample history plot.

You must choose the results set you want to use, the design variable you want to review, the plot type to use, and the confidence level.

Use the PDHIST command to request a histogram plot of a design variable.

You must choose the results set you want to use, the design variable you want to review, the number of classes/points to use, and the type of histogram.

Use the PDCDF command to request a histogram plot of a design variable.

You must choose the results set you want to use, the design variable you want to review, and the confidence level.

The confidence level is a probability expressing the confidence that the values for the cumulative distribution function are in fact between the confidence bounds. The larger the confidence level, the wider the confidence bounds. Plotting of the confidence bounds only makes sense for the postprocessing of Monte Carlo simulation results. Here, the confidence bounds represent the accuracy of the results and with increasing sample size the width of the confidence bounds gets smaller for the same confidence level. For response surface methods the number of simulations done on the response surface is usually very large. Therefore, the accuracy of the results is determined by the goodness of the response surface fit and not by the confidence level.

Use the PDPROB command to request the value of a design variable at an specific point on the cumulative distribution curve.

You must choose the results set you want to use, the design variable you want to review, the relation (greater than, less than), the limit value, and the confidence level.

Use the PDPINV command to request the value of a design variable at a specific point on the cumulative distribution curve.

You must choose the results set you want to use, the design variable you want to review, the relation (greater than, less than), the limit value, and the confidence level.

To postprocess one particular design variable as it relates to another, choose this option. The trend options are described below.

Scatter Plot

Use the PDSCAT command to request a scatter plot showing the correlation between two design variables.

You must select the results set that you want to use, the design variables that you want to review, the type of trendline curve to use (and if plotted, the polynomial order), and the maximum number of point to include in the scatter plot.

Use the PDSENS command to request the sensitivities of an output parameter to the input variables.

You must choose the results set and output parameter you want to use, the type of chart to plot, the type of correlation coefficient, and the sensitivity level.

Use the PDCMAT command to calculate the correlation coefficient matrix.

You must choose the results set you want to use, which type of design variables you are looking at, the specific design variable names, the type of correlation, the significance level, and whether you want to see the probabilities with the correlation coefficients.

To visualize and summarize all results of a probabilistic analysis, choose this option. Details on specifying a report are described below.

Report Options

Use the PDROPT command to request an HTML report.

You must choose which statistics and trends to show in the report and in what form you want to see them. See the PDROPT command for details, and see the other probabilistic results options for further details.

Use the PDWRITE command to request the sensitivities of an output parameter to the input variables.

You must enter a name for the report file, your first and last name, and whether links should be generated between your report and the analysis file, each analysis loop, and the response surface output parameter details (if the response surface method was used).