[Q] I have created a 2D mesh in ICEM CFD using blocking. However, Fluent is unable to read the data and prints error message "Segementation Violation"!
[A] Before I answer to your question, be informed that "Segmentation Violation" message is not unique to a particular error. There may be many causes to your problems. Follow the following steps to trace them:
- 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, to check them.
[Q]If have change the material from "Air" to "Water" using GUI: Define > Material. However, the solver is still using Air.
[A] In most of the cases, the user has to manually set the material for the domain ("fluid" boundary condition) to new material defined.
[Q] I have created a 3D axi-symmetric mesh in ICEM CFD. There was NO error message during "Mesh Check" in ICEM. The mesh on the periodic faces are conformal i.e. 1:1. However, grid check in Fluent is not printing correct value of periodicity.
[A] It requires a small adjustment in Fluent. You have to use TUI: define > boundary-conditions > repair-periodic. Sometimes, creation fails because of slightly non-matching mesh nodes, increasing the matching tolerance up to 0.5 (default is 0.05) may help: grid/modify-zones/match-tolerance.
[Q] I am studying the effect of various operating conditions on a given geometry and similar but different type of mesh. How do I ensure that the Solver Setting, Material, Discretization Scheme remains same for all such cases?
[A] There are two ways you can accoplish this:
- 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 subsquent 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.
Depending upon the complexity of the problem, sometimes one has to use a combination of both the approached mentioned above. [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
What is the error about and how do I rectify it?
[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 automotically 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
[Q] How do I start window 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.
[Q] We have limited Fluent solver license and try to maimize its utilization. For this purpose, we try to start next runs as soon as possible (the solution does not take more that an hour and needs to simulate around 100 cases). Is there a way to keep solver busy all the time?
[A] This can easily be done by starting solver in batch mode. You can prepare many case and data file using Fluent Post and use following input files to keep solver running all the day-and-night:
You need to run Fluent in batch mode and specify following content as Input.jou. Note that the file extension does not need to be .jou. Instead it can be .in as well.
-------------------Input File Starts------------------ file/read-case-data Case01.cas solve/iterate 5000 file/confirm-overwrite no file/write-data Case01.dat file/read-case-data Case02.cas solve/iterate 5000 file/confirm-overwrite no file/write-data Case02.dat file/read-case-data Case03.cas solve/iterate 5000 file/confirm-overwrite no file/write-data Case03.dat ... so on
For Windows: Create a batch file with following content
call cd .\Case1 call fluent 3d -wait -g -i Case1.jou call cd ..\Case2 call fluent 3d -wait -g -i Case2.jou -------------------Input File Ends------------------
[Q]How to stop a fluent solution run before assigned number of iterations while saving the latest results!
- 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:tempexit-fluent.txt
To receive mail notification upon the completion of a batch job, add the following line at the end of the batch journal:
!mail email-address < message.txt
[Q] I make runs on remote machines which take long time. How do I get to know that run is finished without continuous monitoring?