Alliance Doc

Ansys

Revision as of 19:34, 23 September 2020 by Roberpj (talk | contribs)
Other languages:

Introduction

ANSYS is a software suite for engineering simulation and 3-D design. It includes packages such as ANSYS Fluent and ANSYS CFX.

Licensing

Compute Canada is a hosting provider for ANSYS . This means that we have ANSYS software installed on our clusters, but we do not provide a generic license accessible to everyone. However, many institutions, faculties, and departments already have licenses that can be used on our cluster. Once the legal aspects are worked out for licensing, there will be remaining technical aspects. The license server on your end will need to be reachable by our compute nodes. This will require our technical team to get in touch with the technical people managing your license software. In some cases, this has already been done. You should then be able to load the ANSYS modules, and it should find its license automatically. If this is not the case, please contact our Technical support, so that we can arrange this for you.

Available modules are: fluent/16.1, ansys/16.2.3, ansys/17.2, ansys/18.1, ansys/18.2, ansys/19.1, ansys/19.2, ansys/2019R2, ansys/2019R3.

Documentation

The full ANSYS documentation (for the latest version) can be accessed by following these steps:

  1. connect to gra-vdi.computecanada.ca with tigervnc as described in VDI Nodes
  2. open a terminal window and start workbench:
    • module load CcEnv StdEnv ansys
    • runwb2
  3. in the upper pulldown menu click the sequence:
    • Help -> ANSYS Workbench Help
  4. once the ANSYS Help page appears click:
    • Home

Configuring your own license file

Our module for ANSYS is designed to look for license information in a few places. One of those places is your home folder. If you have your own license server, you can write the information to access it in the following format:


File : ansys.lic

setenv("ANSYSLMD_LICENSE_FILE", "<port>@<hostname>")
setenv("ANSYSLI_SERVERS", "<port>@<hostname>")


put this file in the folder $HOME/.licenses/. Before an ANSYS license server can be reached from any Compute Canada system firewall configuration changes will likely need to be made. To arrange this send the following information to <support@computecanada.ca> describing your ANSYS license server 1) fully qualified hostname 2) flex port (commonly 1055) 3) licensing interonnect port (commonly 2325) and 4) vendor port (site specific). Researchers wanting to use the non-free CMC license server or the free SHARCNET license server simply need to configure theor ~/.licenses/ansys.lic file with the following cluster specific settings:

License Cluster ANSYSLMD_LICENSE_FILE ANSYSLI_SERVERS
CMC beluga 6624@132.219.136.89 2325@132.219.136.89
CMC cedar 6624@206.12.126.25 2325@206.12.126.25
CMC graham 6624@199.241.162.97 2325@199.241.162.97
SHARCNET beluga/cedar/graham 1055@license3.sharcnet.ca 2325@license3.sharcnet.ca

Researchers who purchase CMC license subscription must contact <cmcsupport@cmc.ca> to provide your Compute Canada username otherwise license checkouts will fail. In some situations you may also need to obtain an XML file from the institution which operates the license server in order to ensure that ANSYS on the Compute Canada clusters gives priority to the right kind of license. For example to choose a research license instead of a teaching license, a file with name like license.preferences.xml would be placed into directory $HOME/.ansys/v195/licensing/ assuming you are using the ansys/2019R3 module.

License Preferences

Some Ansys license servers (such as those with a Multiphysics Campus Solution license) provide both Research and Teaching license types. When an Ansys job starts, by default it will be assigned an unlimited Academic Research license (aa_r, aa_r_cfd or aa_r_cfd) if any are available, otherwise a Teaching license (aa_t_a) with the following limits will be assigned ... 

o Mechanical solver limit:  32,000 nodes or elements
o CFD solver limit: 512,000 nodes, cells, elements
o Geometry model limit: 50 bodies and 300 faces

Since Research licenses are typically in short supply and very expensive, researchers are encouraged to use Teaching licenses whenever possible. For example, in the case of the SHARCNET Ansys license, there are 250 limited Teaching licenses but only 25 unlimited Research licenses. To configure ANSYS to only only Teaching licenses perform the following steps on each cluster where you plan to run jobs:

  • connect to a login node with X forwarding (ssh -Y, PuTTY, MobaXTerm) or TigerVNC
  • load an Ansys version such as: module load ansys/2020R1
  • run: $EBROOTANSYS/shared_files/licensing/lic_admin/anslic_admin
  • click "Set License Preferences for User" button
  • tick the module version you will be using, click OK
  • tick Use Academic Licenses, click the Solver tab
  • first: highlight "ANSYS Academic Research Mechanical and CFD"
  • press: the small down arrow to specify Don't Use = 0
  • second: highlight "ANSYS Academic Teaching Mechanical and CFD"
  • press: the small down arrow to specify Use = 1
  • click OK, File -> exit

To further describe the default behaviour using a fluent example, if you do not perform any license configuration your first two jobs (1,2) that start running will each be assigned an unlimited Research license if available. If no Research licenses are available each job (1,2) be given a Teaching license. Any more jobs that start (3,4,5,etc) will be given a Teaching license. If your simulation exceeds the above Teaching license size limits, such jobs will fail immediately upon startup and print an error message into their respective slurm output file. The error message maybe searched for using grep for example: 

[gra-login1:~/projects/path/to/my/ansys/jobs] cat -n slurm-38493219.out | grep -A 20 "Error at host"
  131  Error at host:   This is an educational executable, and can only be used
  132    with cases containing less than 512000 cells.
  133    Please exit this fluent session and start another session to continue.

Cluster Batch Job Submission

The ANSYS software suite comes with multiple implementations of MPI to support parallel computation. Unfortunately, none of them supports our Slurm scheduler. For this reason, we need special instructions for each ANSYS package on how to start a parallel job. In the sections below, we give examples of submission scripts for some of the packages. If one is not covered and you want us to investigate and help you start it, please contact our Technical support.

ANSYS Fluent

Typically you would use the following procedure for running Fluent on one of the Compute Canada clusters:

  • Prepare your Fluent job using Fluent from the "ANSYS Workbench" on your Desktop machine up to the point where you would run the calculation.
  • Export the "case" file "File > Export > Case..." or find the folder where Fluent saves your project's files. The "case" file will often have a name like FFF-1.cas.gz.
  • If you already have data from a previous calculation, which you want to continue, export a "data" file as well (File > Export > Data...) or find it the same project folder (FFF-1.dat.gz).
  • Transfer the "case" file (and if needed the "data" file) to a directory on the project or scratch filesystem on the cluster. When exporting, you save the file(s) under a more instructive name than FFF-1.* or rename them when uploading them.
  • Now you need to create a "journal" file. It's purpose is to load the case- (and optionally the data-) file, run the solver and finally write the results. See examples below and remember to adjust the filenames and desired number of iterations.
  • Adapt the Fluent jobscript below to your needs.
  • After running the job you can download the "data" file and import it back to Fluent with File > import > Data....
File : fluent_job.sh

#!/bin/bash
#SBATCH --account=def-group   # Specify account name
#SBATCH --time=00-06:00       # Specify time limit dd-hh:mm
#SBATCH --nodes=1             # Specify 1 or more compute nodes
#SBATCH --cpus-per-task=??    # Specify 32 or 44 on graham, 32 or 48 on cedar, 40 on baluga
#SBATCH --mem=0               # Do not change (allocates all memory per compute node)
#SBATCH --ntasks-per-node=1   # Do not change

module load ansys/2020

slurm_hl2hl.py --format ANSYS-FLUENT > machinefile
NCORE=$((SLURM_NTASKS * SLURM_CPUS_PER_TASK))

fluent 3d -t $NCORE -cnf=machinefile -mpi=intel -affinity=0 -g -i fluent_3.jou
File : fluent_3.jou

; EXAMPLE FLUENT JOURNAL FILE
; ===========================
; lines beginning with a semicolon are comments

; Read input file (FFF-in.cas):
/file/read-case  FFF-in

; Run the solver for this many iterations:
/solve/iterate 1000

; Overwrite output files by default:
/file/confirm-overwrite n

; Write final output file (FFF-out.dat):
/file/write-data  FFF-out

; Write simulation report to file (optional):
/report/summary y "My_Simulation_Report.txt"

; Exit fluent:
exit
File : fluent_3.jou

; EXAMPLE FLUENT JOURNAL FILE
; ===========================
; lines beginning with a semicolon are comments

; Read compressed input files (FFF-in.cas.gz & FFF-in.dat.gz):
/file/read-case-data  FFF-in.gz

; Write a compressed data file every 100 iterations:
/file/auto-save/data-frequency 100

; Retain data files from 5 most recent iterations:
/file/auto-save/retain-most-recent-files y

; Write data files to output sub-directory (appends iteration)
/file/auto-save/root-name output/FFF-out.gz

; Run the solver for this many iterations:
/solve/iterate 1000

; Write final compressed output files (FFF-out.cas.gz & FFF-out.dat.gz):
/file/write-case-data  FFF-out.gz

; Write simulation report to file (optional):
/report/summary y "My_Simulation_Report.txt"

; Exit fluent:
exit
File : fluent_transient.jou

; EXAMPLE FLUENT JOURNAL FILE FOR TRANSIENT SIMULATION
; ====================================================
; lines beginning with a semicolon are comments

; Read only the input case file:
/file/read-case         "FFF-transient-inp.gz"

; For continuation (restart) read in both case and data input files:
;/file/read-case-data  "FFF-transient-inp.gz"

; Write a data (and maybe case) file every 100 time steps:
/file/auto-save/data-frequency 100
/file/auto-save/case-frequency if-case-is-modified

; Retain only the most recent 5 data (and maybe case) files:
; [saves disk space if only a recent continuation file is needed]
/file/auto-save/retain-most-recent-files y

; Write to output sub-directory (appends flowtime and timestep)
/file/auto-save/root-name output/FFF-transient-out-%10.6f.gz

; ##### settings for Transient simulation :  ######
; Set the magnitude of the (physical) time step (delta-t)
/solve/set/time-step   0.0001

; Set the number of time steps for a transient simulation:
/solve/set/max-iterations-per-time-step   20

; Set the number of iterations for which convergence monitors are reported:
/solve/set/reporting-interval   1

; ##### End of settings for Transient simulation. ######

; Initialize using the hybrid initialization method:
/solve/initialize/hyb-initialization

; Perform unsteady iterations for a specified number of time steps:
/solve/dual-time-iterate   1000

; Write final case and data output files:
/file/write-case-data  "FFF-transient-out.gz"

; Write simulation report to file (optional):
/report/summary y "Report_Transient_Simulation.txt"

; Exit fluent:
exit

Fluent Journal files can include basically any command from Fluent's Text-User-Interface (TUI); commands can be used to change simulation parameters like temperature, pressure and flow speed. With this you can run a series of simulations under different conditions with a single case file, by only changing the parameters in the Journal file. Refer to the Fluent User's Guide for more information and a list of all commands that can be used.

ANSYS CFX

File : mysub.sh

#!/bin/bash
#SBATCH --account=def-group   # Specify account name
#SBATCH --time=00-06:00       # Specify time limit dd-hh:mm
#SBATCH --nodes=1             # Specify 1 or more compute nodes
#SBATCH --cpus-per-task=??    # Specify 32 or 44 on graham, 32 or 48 on cedar, 40 on baluga
#SBATCH --mem=0               # Do not change (allocates all memory per compute node)
#SBATCH --ntasks-per-node=1   # Do not change

module load ansys/2020R1

nodes=$(slurm_hl2hl.py --format ANSYS-CFX)
cfx5solve -def YOURFILE.def -start-method "Intel MPI Distributed Parallel" -par-dist $nodes  <other options>


Note that you may get the following errors in your output file : /etc/tmi.conf: No such file or directory. They do not seem to affect the computation.

Site Specific Usage

Sharcnet License

On 31may2020 the Sharcnet license was upgraded from a CFD (Research CFD) only license to a MCS (Multiphysics Campus Solution) license including the following ANSYS Academic Research products: HF, EM, Electronics HPC, Mechanical and CFD. The Sharcnet ANSYS license supports a total of 275 running jobs consisting of 25 aa_r unlimited simulation size Research tasks and 250 aa_t_a limited simulation size Teaching tasks. There is no limit to the number of jobs a researcher can run using the Teaching tasks. There is however a 2 job limit when using the Research tasks. A total of 384 aa_r_hpc cores are available to all running ANSYS jobs with a limit of 64 cores per user. Researchers are asked to only use Teaching tasks when possible as described in the License Preferences section above. This license has been renewed for over 10 years and there is no reason to expect it will not be renewed again in coming years.

The SHARCNET license can be used by any Compute Canada user on any Compute Canada system for the purpose of Publishable Academic Research. The license is made available on a first come first serve basis. Should a large number of ANSYS jobs attempt to start on a given day, it is possible some jobs may fail to start due to insufficient tokens being available, such jobs will need to be resubmitted. If guaranteed (dedicated) token access is required for your research to progress, open a ticket and request a quote for the quantity of tokens needed. The quote will be obtained from Simutech to ensure compatibility with the existing license (customer #446422). Prices would be at cost plus applicable taxes and the actual purchase would be done directly by the PI with Simutech after that point. Neither LS-DYNA or Lumerical are included with the Sharcnet ANSYS license. Tokens for these products may be added to the SHARCNET server for dedicated use by similarely opening a ticket and requesting a quote.

License Server File

To use the Sharcnet ansys license configure your ansys.lic file as follows: 

[gra-login1:~/.licenses] cat ansys.lic
setenv("ANSYSLMD_LICENSE_FILE", "1055@license3.sharcnet.ca")
setenv("ANSYSLI_SERVERS", "2325@license3.sharcnet.ca")

Query License Server

To check all ANSYS licenses currently in use as running jobs by your username: 

ssh graham.computecanada.ca
module load ansys
lmutil lmstat -c $ANSYSLMD_LICENSE_FILE -a | grep "Users of\|$USER"

where there lines beginning with ...

  • Users of aa_r = Total number of ANSYS Academic Research tasks in use by all users (maximum 25 jobs running)
  • Users of aa_t_a = Total number of ANSYS Academic Teaching tasks in use by all users (maximum 250 jobs running)
  • Users of aa_r_hpc = Total number of ANSYS hpc licenses in use by all users (maximum 384hpc cores = 640total - 256reserved)

If you discover any licenses unexpectedly in use with the above commands (usually due to ansys not exiting cleanly on gra-vdi) then connect to the node where its running, open a terminal window and run the following command to terminate the rogue processes pkill -9 -e -u $USER -f "ansys" after which your licenses should be freed. Note that gra-vdi consists of two nodes (gra-vdi3 and gra-vdi4) which researchers are randomly placed on when connecting to gra-vdi.computecanada.ca with tigervnc. Therefore its necessary to specify the full hostname (gra-vdi3.sharcnet.ca or grav-vdi4.sharcnet.ca) when connecting with tigervnc to ensure you login to the correct node before running pkill.

Remote Visualization

1) Using global Compute Canada cluster modules:

  1. Connect to gra-vdi.computecanada.ca with TigerVNC
  2. module load CcEnv StdEnv
  3. module load ansys/2020R1
  4. export HOOPS_PICTURE=opengl
  5. runwb2|vglrun fluent|cfx5|icemcfd

2) Using local gra-vdi modules (may provide better graphics performance):

  1. Connect to gra-vdi.computecanada.ca with TigerVNC
  2. module load SnEnv
  3. module load ansys/2019R3
  4. runwb2|fluent|cfx5|icemcfd|apdl
  5. Press y then enter to accept the two conditions.
  6. Press enter to use the sharcnet license.

where the cfx5 command allows starting the following components: 

   1) CFX-Launcher  (cfx5launcher)
   2) CFX-Pre       (start cfx5pre directly)
   3) CFD-Post      (start cfx5post directly)
   4) CFX-Solver    (start cfx5solve directly)

Additive Manufacturing

To get started configure your ~/.licenses/ansys.lic file to point to a license server that has a valid ANSYS Mechanical License. This must be done on all systems where you plan to run the software.

Enable Additive

To enable ANSYS Additive Manufacturing in your project do the following 3 steps:

Start Workbench

On Gra-vdi:

  • connect to gra-vdi.computecanada.ca with TigerVNC
  • module load CcEnv StdEnv ansys/2019R3
  • export PATH=/cvmfs/soft.computecanada.ca/nix/var/nix/profiles/16.09/bin:$PATH
  • cd to the directory where your test.wbpj file is located
  • runwb2

On a cluster:

  • connect to a cluster compute node with TigerVNC
  • module load ansys/2019R3
  • export PATH=/cvmfs/soft.computecanada.ca/nix/var/nix/profiles/16.09/bin:$PATH
  • cd to the directory where your test.wbpj file is located
  • runwb2

Install Extension

  • click Extensions -> Install Extension
  • specify the following /path/to/AdditiveWizard.wbex then click Open: /cvmfs/restricted.computecanada.ca/easybuild/software/2017/Core/ansys/2019R3/v195/aisol/WBAddins/MechanicalExtensions/AdditiveWizard.wbex

Load Extension

  • click Extensions -> Manage Extensions and tick Additive Wizard
  • click the ACT Start Page tab X to return to your Project tab

Run Additive

Gra-vdi

ANSYS Additive Manufacturing can be run in Gui Mode on gra-vdi with upto 8cores for 24hours as follows:

  • Start Workbench On Gra-vdi as described above in Enable Additive
  • click File -> Open and select test.wbpj then click Open
  • click View -> reset workspace if you get a grey screen
  • start Mechanical, Clear Generated Data, tick Distributed, specify Cores
  • click File -> Save Project -> Solve

Check utilization:

  • open another terminal and run: top -u $USER
  • kill rogue processes from previous runs if required: pkill -9 -e -u $USER -f "ansys"

Cluster

To submit an Additive job to a cluster queue, you must first prepare your additive simulation to run on Compute Canada clusters. To do this open then save your simulation (on gra-vdi OR the cluster you are working on in a salloc session) to initialize the projects internal path configuration as described above in the Enable Additive section. Next create a slurm script in the directory where your project file is located (similar to one below) and submit it to the queue by doing: sbatch script.txt Be sure that value of --ntasks in the slurm script matches the Cores value last set in Mechanical in particular if moving the project to a different cluster. To change the Cores value on a cluster without opening your simulation follow the "Open Mechanical on login node" section found near the bottom of this page.


File : script.txt

#!/bin/bash
#SBATCH --account=def-account
#SBATCH --time=00-06:00      # Time (DD-HH:MM)
#SBATCH --ntasks=8           # Number of cores
#SBATCH --mem-per-cpu=2G     # Memory per core
unset SLURM_GTIDS
rm -f test_files/.lock
module load ansys/2019R3
export KMP_AFFINITY=balanced
export I_MPI_HYDRA_BOOTSTRAP=ssh
export PATH=/cvmfs/soft.computecanada.ca/nix/var/nix/profiles/16.09/bin:$PATH
runwb2 -B -F test.wbpj -E "Update();Save(Overwrite=True)"


For parametric studies change Update() to UpdateAllDesignPoints() in the last line of your slurm script. For initial performance testing one can avoid the solution from being written by specifying Overwrite=False in the slurm script so further runs to be conducted without needing to reopen the simulation in workbench (and mechanical) to clear the solution and recreate the design points. Another option is to create a replay script once and for all in workbench to perform these tasks then run it on the cluster between runs as follows. The replay file can be used in different directories by changing its internal FilePath setting accordingly. 

module load ansys/2019R3
rm -f test_files/.lock
runwb2 -R myreplay.wbjn

Resource utilization:

Once your additive job has been running for a few minutes a snapshot of its resource utilization on the compute node(s) can be obtained with the following the srun command. Sample output corresponding to the above 8core submission script as as follows where it can be noticed that two nodes were selected by the schedular: 

[demo@gra-login1:~] srun --jobid=jobnumber top -bn1 -u $USER | grep R | grep -v top
  PID USER   PR  NI    VIRT    RES    SHR S  %CPU %MEM    TIME+  COMMAND
22843 demo   20   0 2272124 256048  72796 R  88.0  0.2  1:06.24  ansys.e
22849 demo   20   0 2272118 256024  72822 R  99.0  0.2  1:06.37  ansys.e
22838 demo   20   0 2272362 255086  76644 R  96.0  0.2  1:06.37  ansys.e
  PID USER   PR  NI    VIRT    RES    SHR S  %CPU %MEM    TIME+  COMMAND
 4310 demo   20   0 2740212 271096 101892 R 101.0  0.2  1:06.26  ansys.e
 4311 demo   20   0 2740416 284552  98084 R  98.0  0.2  1:06.55  ansys.e
 4304 demo   20   0 2729516 268824 100388 R 100.0  0.2  1:06.12  ansys.e
 4305 demo   20   0 2729436 263204 100932 R 100.0  0.2  1:06.88  ansys.e
 4306 demo   20   0 2734720 431532  95180 R 100.0  0.3  1:06.57  ansys.e

Scaling tests:

After a job completes its elapsed time can be found from the "Job Wall-clock time" output from the seff jobid. One can use this value to perform scaling tests. If the Wall-clock time decreases by ~50% when the number of cores are doubled (for example from "#SBATCH --ntasks=8" to "#SBATCH --ntasks=16") further core doubling increasements can be investigated. While jobs may run faster when the number of cores is increased, the wait time will also increase significantly unless the research group has a RAC award.

Open mechanical on login node:

This procedure explains howto initialize your mechanical environment on a cluster by opening the simulation on a cluster login node. If the simulation requires more than 8GB which is the typical login node memory limit than a cluster compute node will need to be used. When a simulation is moved to a different cluster the project will need to be opened and saved again if the path and directory location have changed. 

* Login to a cluster login node with TigerVNC  
* Open a terminal window in vncviewer and run:
   [demo@beluga3:~] module load ansys/2019R3
   [demo@beluga3:~] runwb2
   o start Mechanical by clicking Component Systems -> Mechanical Model -> Model
   o under Solve for My Computer enter Cores: 8
   o under Solve for My Computer tick Distributed 
   o quit Mechanical by clicking File -> Close Mechanical
   o quit Workbench by clicking File -> Exit (do not save the current project)

Message Passing Interface

Retrieved from "https://docs.alliancecan.ca/mediawiki/index.php?title=Ansys&oldid=89972"