Error messages in ANSYS Fluent, their interpretation and troubleshooting
[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:
| [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:
| [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-shadowWhat is the error about and how do I rectify it?
[A]: Note that this is a "Warning" message and not an "Error" message. This message appears usually when there is common edge sharing two different zones of same type (say type "Fluid" on both sides). In this case, you need to go to Define > Boundary Condition and set the extn_int1 & extn_int2 as "Interior".
| [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[A]: This message is generated when a particular "interface zone" is being used in more than 1 "grid interface". This is an error message just to remind you that you are attempting to make an unrealistic interface and Fluent would not have allowed you to do so anyway.
| [Q] When I created a JPEG file of contour plot, some portion of legend is missing|
[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 window in batch mode?|
[A]: The method varies depending upon operating system (OS).
|[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------------------
... 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] Warning: Fluent continuously reports the warning message for exceeding the limit
of turbulent viscosity ratio. |
[A]: This message is an indication of TVR exceeding the default limit of 1.0E+5. The primary cause for such an unphysical value may be: Poor mesh quality (i.e., skewness > 0.85 for Quad/Hex, skewness > 0.90 for Tri/Tetrahedral elements). Use of improper turbulent boundary conditions Not supplying good initial values for turbulent quantities.
|[Q]I try to define operating pressure at a point in Fluent. The co-ordinates have
been taken from mesh model in ICEM where size of the domain was in mm say (X0, Y0, Z0).
Fluent gives warning message: "The point is outside the domain"! |
[A]: Note that all the solvers converted the input "length" dimensions into meter by scaling up/down the input mesh model appropriately. Since, the scaling is usually done about origin of centre of the volume (in 3D) / area (in 2D), the location of point being considered may not be (X0/1000, Y0/1000, Z0/1000). It is always better to find the co-ordinate by mouse-probe function.
|[Q]How to stop a fluent solution run before assigned number of iterations while saving the latest results!
[A]: For Linux:
| [Q] Can I read a journal file from another file? |
[A]: The answer is 'No'. Note that scripting is not a full-fledged programming language and nesting is not allowed.
| [Q] Why the direction of rotation I specify in Fluent is not matching with what I intended for? |
[A]: "Right hand rule" needs to be followed to specify the value of Rotation Angle. E.g. if axis of rotation is along positive X-axis and direction of rotation is from Y-axis towards Z-axis, the angle of rotation would be positive.
| [Q] I make runs on remote machines which take long time. How do I get to know that run is finished without continuous monitoring? |
[A]: The runs are normally made on remote machine in batch mode using an input file described earlier. Fluent can notify the user by e-mail after the completion of a batch job if following line at the end of the batch journal (used to start the run) is added: !mail [e-mail address] < [body.txt] where [e-mail address] (without square brackets) is the user's e-mail address and [body.txt] (without square brackets) is the file, located in the directory where case and data files are stored, that contains the message to be sent.
| [Q] I am unable to generate ANIMATIONS in Fluent in batch mode? |
[A]: Following option need to be added during start up command of the batch job: -driver null
| [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 intead of 0.001 and so on? |