Database Full Index

7. Output to Solver

7.1. What are the file formats that the output interface supports?

To get the documentation for the file formats in which the output interface exports and imports please click here

7.2. Why can't I write Fluent output for a hexa mesh having refinements?

Fluent output requires the refinement to be defined in Hexa uniformly in all directions and in 1:2 form. Fluent's own solver prefers the grid adaptation in that way only i.e. one hexa cell can only be divided into 8 pieces; twice in each direction.

[ top ]

7.3. I see HDF format to write my mesh output but the executable is not there. Why?

HDF executable is only available on HP platform. This format is not a general HDF format but has been written for a particular company's specific needs. Hence, the changes in the code may not be reflecting for a general user. We suggest to use the CGNS format rather.

[ top ]

7.4. Why don't I see GASP or GUST interface on windows?

They are not available either on windows NT/2000. As of now, we do not have the libraries from Aerosoft on these platforms. Please use some other platform for the time being.

[ top ]

7.5. I don't see CFL3D executable on Windows. Why?

CFL3D solver is not supported on windows and the files written by our filter are and not portable to Unix (Fortran unformatted). Hence, it is removed from the distribution. Please use the UNIX machine to write the CFL3D output,

[ top ]

7.6. I have a 2D domain file but I can't read it in Fluent. Why?

There could be multiple reasons for that to happen:

You must have surrounding bar elements all over the 2d meshes. These bar elements will have bcs for Fluent. If you do not have a complete enclosed domain of bar elements you will have problem reading this mesh in Fluent. Unfortunately, we do not have boundary check for 2D meshes (like check for uncovered faces in 3D) thus you are mostly dependent on visual check,
You must not mix-up volume elements with any other kind of elements. The family which has cells like 2d quad/tri elements must not have any bar elements in it otherwise it confuses the solver/translator.

[ top ]

7.7. I cannot read a mesh into Fluent. It's a hexa mesh and I have done collapsing there. Why?

See this answer .

[ top ]

7.8. I have multiple materials in my HEXA blocking and I have defined shared wall between them. Why can't I write the Fluent output for the same?

Fluent requires that multiple materials should be separated by walls (and wall shadows). Defining shared wall in HEXA means that we assume that the two materials are essentially same.
To get rid of the trouble, the user should try to do the diagnostics for "internal faces" inside MED for the mesh generated by HEXA. The fix, at times, put the duplicate faces there. So, as a precautionary step, check for duplicate faces and delete them if there are any. Then you should be able to write a proper Fluent mesh.

[ top ]

7.9. I want to define pressure boundary for Ansys Interface. When I write the output, the bcs don't come in the input file. Why?

You, probably, are not choosing to write "quad/tri" elements for writing the mesh for Ansys. You will have to choose them so that you get the pressure boundary information correct in the input file for Ansys. Unfortunately, tri/quad elements itself create trouble for the mesh. At this stage, you will have to read in the mesh file in a text editor and update following lines:

Lines defined by "ET" command. You only need it for the "ET,1,45,......" line if you have tetra elements. Rest all the lines with 63 element type should be deleted i.e. "ET,2,63,.....", "ET,3,63......" etc.
These lines are also referenced by "EBLOCK" statements. The first EBLOCK statement should be left as it is and the second through last should be deleted.
You might want to remove the "SOLVE" line towards the end for faster reading of mesh inside Ansys.

This should be taken care of in the next Ansys interface.

[ top ]

7.10. For Nastran Output, is it possible to get thickness parameter information attached on shells created with 'surface> Midsurface' function,

In ICEM CFD midsurface capability, many customers want to be able to pass the compressed midsurfaces thickness to the shell elements (mesh). We can do this, for uniform thicknesses, in the following way:

When a midsurface is compressed, the thickness is stored to the surface's height entity parameter. If you were to look at the height, you could then use this to define the thickness for the shell elements.
For example, Let us say we want to set up a shell model for Nastran. In structural solvers, shells typically/always need thickness information.
If you go into Nastran->BCs, for a family you would define this family to be shell elements (BC.10 Shell Elements). In this form there is a membrane thickness. This should be the height (thickness) of the specified family.

If you want to put an average thickness on a family of midsurfaces, you could use the following script that will list the average thickness per family.

foreach fam [ic_geo_list_families] {
	set total 0
	set num 0
	set avg 0
    	foreach surf [ic_geo_get_objects surface $fam] {
		set param [ic_get_meshing_params surface $surf]
		set thickness [expr [lindex $param 3] / [ic_geo_get_ref_size]]
		#mess "param is $param; thickness is $thickness\n"
		set total [expr $total + $thickness ]
		incr num
	}
	if $num {set avg [expr $total / $num]}
	mess "fam $fam has average shell thickness of $avg\n" blue
}

[ top ]

7.11. Why do I get "Incorrect node count (13404 != 13392)" type of message when I do "Grid Check" on a Fluent mesh inside Fluent?

You most probably have internal walls in the model which are making T or A kind of connections. We do not know the exact reason but looks like Fluent gets confused for these kind of junctions where there are all kind of single as well as multiple elements. There are two workaround for this:

Read the mesh inside Fluent and save it back. Next time you load your saved case file inside Fluent, this error would disappear,
In ICEM CFD, pull out the surfaces coming from other junction into a different family, for example put the horizontal stuff in A junction into a different family. This should resolve your trouble also and you would not see any error in Fluent

[ top ]

7.12. How do I output the element material numbers in the nastran input file?

You can set the material number in the Nastran Boundary Conditon menu under

Volume elements -> Material id number

The material property data are defined under

AD.02 Elastic materials (material property data)

When starting the translator you should also set the following option:

Write volume elements - defined by B.C.

[ top ]

7.13. I want to use replay file to write Fluent output for my multiple models. Looks like it is broken. How do you do it?

Please put a command like as follows in your replay file:

ic_run_application_exec . {} $env(ICEM_ACN)/icemcfd/output-interfaces/georampant {-dom output_test/tetra_mesh.uns -b output_test/boco output_test/fluent}

where

Mesh file:    output_test/tetra_mesh.uns
Boco file:    output_test/boco
Fluent file:  output_test/fluent   (you will get .msh extension automatically)

[ top ]

7.14. The mesh looks fine in Med, but Output to NASTRAN results in mesh with all nodes squished into one plane,why does this happen?

If the user outputs as Long format and then reads it into Nastran in short format, then there is a zero in the long format file where the z would be in the short format. The result is that all the nodes have a z value of 0 and they are squished into the plane.To avoid this the user should export in Short format.

[ top ]

7.15. I wrote output for CFDesign from ICEM CFD 4.3.1 but looks like my CFDesign version cannot read this file. Why?

CFDesign no longer supports GBI files, the file format written by Ansys ICEM CFD CFDesign output interface. Blue Ridge Numerics (the company behind CFDesign) has decided to drop support of this file format, opting instead to support import of generic files, including Nastran bulk data and I-DEAS Universal files. Please write your Ansys ICEM CFD output in one of these formats and try reading it in CFDesign.

However, this means that the user cannot possibly use the applied boundary conditions in Ansys ICEM CFD. Fortunately, CFDesign has new tools to just grab the mesh and apply boundary conditions. they virtually need only the volume mesh now.

[ top ]

7.16. What are the supported element types and material properties/keywords in AI*Environment for Ansys, Nastran, LS-Dyna, and ABAQUS?

Please click here to see the supported element types, Material Properties, and various keywords for ANSYS, LS-Dyna, Nastran, and ABAQUS in AI*Environment 10.0.

[ top ]

[ top ] [ previous ] [ next ]

created by faq-system 0.3.6 Thomas Linden