CFX / FLUENT Troubleshooting

Error / Warning messages in ANSYS FLUENT and CFX

[Q] What are sample 'SCHEME' files for automation in ANSYS FLUENT?

[A]Ref: https://www.cfd-online.com/Forums/fluent-udf/81520-journal-fluent-scheme-programming.html

(Do ((u 0.0 (+ u 0.1))) ((> u 1.0))
(Ti-menu-load-string (format #f "surface/iso-surface z-coordinate z-plane-~a () () ~a" u u)) ) 

• '~a' random variable in general format (string without double quotes "")
• ~ d: integer number
• ~04d: integer with zeros on the front is always 4 digits fill ( 5 is about 0005), eg this is important for file names
• ~f: floating-point number
• ~4.2f: floating point number, a total of 4 characters long, 2 digits after the decimal: 1.2 will be 1.20

(do ((x 0 (+ x 0.2)) (i 1 (+ i 1))) ((> x 3.1))
 (ti-menu-load-string (format # f "surface / iso-surface x-coordinate ~ x-02d () ~ a () 'ix))
)

surface / iso-surface x-coordinate x-01 () 0.0 ()

surface / iso-surface x-coordinate x-03 () 0.4 ()

surface / iso-surface x-coordinate x-16 () 3.0 ()

[Q] How do I export the name of the zones and type of boundary conditions assigned to them?

(define (export-bc-names)
 (for-each
  (lambda (name)
   (display 
    (format #f " {~a, \"~a\", \"~a\"},\n"
     (zone-name->id name) name (zone-type (get-zone name))
    )
   )
  ) (inquire-zone-names)
 )
)

[Q] There are two types of residual option available in CFX: RMS and MAX. Which one should I use to set convergence criteria and why?

CpAir = 1030.33 [J/kg/K] - 0.196044 [J kg^-1 K^-2] * T + 3.93365E-4 [J kg^-1 K^-3] * T * T

kAir = 6.24978E-6 [W m^-1 K^-1] + 9.73517E-5 [W m^-1 K^-2] * T - 3.31177E-8 [W m^-1 K^-3] * T * T

muAir = 1.458E-6 [Pa s K^-0.5] * T^1.5 / (110.4 [K] + T)
Here, T is in [K], the default unit of Temperature used by Solver.

[Q] I have prepared a mesh and obtained solution for 3 operating conditions and 2 turbulence models. Thus, simulation set will consist of 1 [mesh] x 3 [B.C.] x 2 [Turb. Models] = 6 case files. I want to do sensitivity analysis by repeating the same task for 2 more mesh refinements. Can this process be automated i.e. the script reads new mesh files, imports B.C. setting from old cases, starts solver and prepares result file?

COMMAND FILE:
  CFX Pre Version = 12.1
END
# /usw/cfx12.SP1.0_0/v121/CFX/bin/cfx5pre -batch BatchCFX.pre
# Create an ARRAY which holds names of the Mesh Files
# It is assumed that the mesh format is *.cfx5
! @MeshFiles = (MeshData1, MeshData2, MeshData3, MeshData4);
! @FilesCCL = (FilesCCL1, FilesCCL2, FilesCCL3, FilesCCL4);
! @FilesDef = (FilesDef1, FilesDef2, FilesDef3, FilesDef4);
! @FilesCFX = (FilesCFX1, FilesCFX2, FilesCFX3, FilesCFX4);
! $LEN_msh = @MeshFiles;
! $LEN_CCL = @FilesCCL;
! $LEN_Def = @FilesDef;
! $LEN_CFX = @FilesCFX;

#--------------------------------------------------------------------
! for ($i=0;$i<$LEN_CFX;$i++) {
# Use this section when EXISTING *.cfx files are to be opened
>load filename=/home/userX/Case07.cfx, mode=cfx, overwrite=yes
> update

# -------------------------------------------------------------------
# Use this section only when MESH data needs to be imported
#>load mode=new
#> update
#! $temp = "/home/userX/" . $MeshData[$i] . ".cfx5";
#>gtmImport filename=/home/userX/MeshData.cfx5, \
#type=Generic, genOpt= -n, units=mm, nameStrategy= Assembly
#> update
#--------------------------------------------------------------------

>importccl filename=/home/userX/Test_CCL.ccl, mode = replace, \
autoLoadLibrary = none
> update

! $temp = "/home/userX/" . $FilesCFX[$i] . ".cfx";
>writeCaseFile filename=$temp
> update

! $temp = "/home/userX/" . $FilesDef[$i] . ".def";
>writeCaseFile filename=$temp, operation=write def file
> update

#----------------Save CFX File --------------------------------------
>writeCaseFile
> update
#---------------Close CFX File --------------------------------------
>close, deleteLibrary = On
> update
!}

• Check the ICEM translation log in its message window. Was the translation clean? If not, rectify them and recheck. If yes, read next point.
• Have you selected the correct option "2D" for 2D mesh?
• Run the utility "Check Mesh" under "Edit Mesh" tab and rectify error messages, if any. Warning messages can be ignored most of the time, do check them and rectify as far as possible.

• Write or record a [clean] script [FLUENT Journal] for 1st set of simulation. Change only those variables which you want to change. Read it in subsequent case files.
• Once the Case file is set as per your requirements, use TUI "File -> write-BC" to write all the settings to a file. Read it after mesh import in later cases. Change B.C. such as mass flow rate, temperature, etc manually.

[Q] When I import a mesh created in ICEM CFD V12.1, I get following error message:

 Warning: Thread 62 has 8 contiguous regions.
        creating extn_int1-shadow
        creating extn_int2-shadow 

[Q] I have prepared a 2D mesh in ICEM CFD V12.1. The "Mesh Check" under "Edit Mesh" tab reports no error message. When I tried to import this mesh in FLUENT V6.3.27, following error message was reported:

WARNING: Unassigned interface zone detected for interface 56
WARNING: Unassigned interface zone detected for interface 57
Checking storage.

[A] One of the case observed is when there is an internal edge and the the two surface mesh either side are in same "part". Sometimes, particularly in ICEM V12.1, if any part name is named as interface_*****, they are automatically assigned the boundary condition type "INTERFACE" in FLUENT. The remedy is either to remove "interface" from name of the part or create a "grid interface" in FLUENT involving zone ID 56 & 57. The former is recommended action.

[Q] While creating a "grid interface", following error message is reported:

Error: Zone interface_bot already in another interface
Error Object: #f

[A]: You need to adjust the size of the window (top-right corner of the "Save Hardcopy" pop-up window).

[Q] How do I start FLUENT in batch mode?

• For windows, to start FLUENT in 3D mode, use "fluent 3d -g -i batch.jou -hidden". Note that without command line option '-hidden', the GUI will still be started but show as an icon. Replace '3d' by '2d' to start fluent in 2-dimensional mode.
• In Windows, a transcript file cannot be generated through command line. It should be (can be) started and stopped withing FLUENT session.
• For Linux or Unix environment, the method further depends on shell:
  • For C-shell: fluent 3d -g < Input.jou >& Output.trn &, where Input.jou is journal script to make fluent read all the necessary files and commands and Output.trn is the transcript file which it will write.
  • For Bash (Bourne Shell) and ksh (Korn Shell): fluent 3d -g < Input.jou > Output.trn 2>&1 &
  • Note that the ampersand (&) at the end of the command tells the OS not to wait till completion of the execution of that line. This is also called running the command in background.
• Note the following additional requirement of run FLUENT in batch mode:
  • "Confirm file overwrite" should be set to 'Yes' for all batch processing. This is to avoid the user prompt to over-write the case file when save frequency is set.
  • Alternatively, "Hide Questions" and "Exit on Error" can be switched on and let FLUENT handle itself
  • Incidentally, all these 3 settings can only be done through GUI and no equivalent script or TUI command is available. Hence, Scheme command, for example (set! *cx-exit-on-error* #t) to switch on "Exit on Error" option, needs to be used.

• to save and exit, create an empty file named "stop-fluent" in /tmp folder. It will make a "#restart.inp" file in the directory from which batch run was started. The files will be written to the same directory where the original input files were read and will have the same names but with appended current iteration number. By default, the case file will be written
• If the machine has several FLUENT sessions running, named check pointing can be used selectively. To stop this particular job, use the following command inside the /tmp directory: "touch exit-fluent-job-1"
• To check your job (i.e. to save data for latest iteration and continue the run) create a file named "check-fluent" in your /tmp directory. Check-pointing code calls the same file I/O routines used by the GUI or TUI and will produce the same error messages if disk space is insufficient In such case, FLUENT will not return to the iteration loop.
• To write data file only, execute following Scheme command before iterating: (rpsetvar 'checkpoint/write-case? #f)
• If the machine has several FLUENT sessions running, named check pointing can be used to selectively stop a specific FLUENT process. A specific check point name can be added to the first line of the batch journal file, as shown below:
  (set! checkpoint/exit-filename "/tmp/exit-fluent-job-1")
  file/read-case-data sample.cas
  solve/iterate 1000
  file/write-case-data final.cas

• to save and exit, create an empty file C:\temp\exit-fluent.txt

[Q] Can I read a journal file from another file?

[Q] Why the direction of rotation I specify in FLUENT is not matching with what I intended for?

[Q] I make runs on remote machines which take long time. How do I get to know that run is finished without continuous monitoring?

[Q] I am unable to generate ANIMATIONS in FLUENT in batch mode?

[Q] How do I customize FLUENT during start up, for example changing the default setting to k-ε instead of laminar, FPS unit system instead of SI, convergence norm to 0.00001 instead of 0.001 and so on?

• Almost all the programs use a "start-up" file and FLUENT is no exception. It auto executed a .fluent file in "home directory" of Linux/UNIX users and C:\ drive of Windows users.
• This file contains Scheme commands to execute as well as it can contain other files containing Scheme commands to load
• As per the the standard norm of any operating system and programming language, FLUENT will search to locate the Scheme files from the working directory unless full path is specified for each Scheme file in .fluent file.
• Example is:
  (set! *cx-exit-on-error* #f)
  ;turn OFF exit-on-error
  (let ((menu (cx-add-menu "USC" #\U)))
  (load mysettings.scm)
  (load postproc.scm)

[Q] Error: Invalid section id: Error Object: #f