Hey everyone,

I am trying to hex-core mesh in ICEM v11.0.1. While the hexcore works beautifully, even on complicated geometries, I cannot import any form of hex core into Fluent, no matter how high the mesh quality is. I have even tried a simple cube and that fails with the following errors:

12494 nodes.

40882 mixed cells, zone 5. Error: read: face 85032, zone 6. Reading Faces: failed while reading section 13.

Clearing partially read grid.

Error: Read aborted due to critical error. Error Object: ()

Here is a pic of the cross section of the mesh where that error originated. I am using Fluent 6.3. I have tried windows and Linux.

http://www.calpoly.edu/~rperry/Icem%20Hex%20Core.PNG

In that pic there is only one set of surfaces, which I set as pressure-far-field for import into Fluent. I selected FluentV6 as my solver and output as a .msh. I have also tried generating a tet mesh and turning it into a hex mesh afterwards, but got the same errors.

I have no idea what could be going wrong, but any help would be very greatly appreciated!!

Cheers,

-Robert

http://www.calpoly.edu/~rperry/Icem%20Hex%20Core.PNG

I believe this was discussed recently ... its apparently a bug in fluent(windows). Search the forum ...

I have also tried doing it in 32 and 64 bit Linux, so I think it's more than a bug?!~

What do Fluent support say?

I have duplicated your problem on linux64 (Icemcfd + fluent 6.3).

"Read aborted due to critical error"

> Reading "/home/fluent.msh"...

19342 nodes.

50796 mixed cells, zone 7. Error: read: face 112020, zone 8. Reading Faces: failed while reading section 13.

Clearing partially read grid.

Error: Read aborted due to critical error. Error Object: #f

Error: Error reading "/home/work/dynamic/Fluent/trialrun/2D/geom/krishnan/2dofsimple/delmenow/fluent.msh". Error Object: #f

However, there are workarounds. I exported the mesh for CFX11, created a basic CFX11 def file (mesh + BC specifications), imported this into fluent. This worked and solved fine.

Icemcfd has a myriad of export options, fluent has a myriad of import options. Somewhere the twain should meet.

Let us know how you get on.

Well, I had a friend try the CFX thing, and it didn't work either!

Error: bad syntax. Usage: utility fe2ram dimension read_format zoning write_format [inputfile [outputfile]] utility fe2ram dimension read_format zoning write_format [inputfile [outputfile]]

dimension: [-d2 | -d3 | -surface]

Building...

grid, Error: Null Domain Pointer

I'll contact Fluent and ICEM tech support and see what they say. I'll be sure to post the results here.

Thanks Joe!

convert hexcore mesh into polyhedra using utility tpoly so it becomes conformal grid then read into Fluent. This is the rec procedure for TGrid exported hexcore meshes for running in Fluent parallel.

What do I do if I don't have Tgrid? This is also a serial job, not parallel.

There has to be something wrong with Fluent/ICEM, because I can import hex-core from Gambit without using tpoly, and even run it in parallel (though it scales poorly).

Have you defined "Body" for your mesh in ICEM...It can be one of the resons for "Null Domain Pointer - Error.." just check it out...!

Well, here's what Fluent tech support said:

FLUENT ADMINISTRATOR: ----------------------------------------------------- There is a bug with ICEM - Fluent translator in ICEM 11, and when you see the section f error, it is because of this bug. So I will suggest you to use other version of ICEM with latest version of Fluent (6.3.26 version). If this does not work then please try following workarounds

1) You may write your ICEM mesh in ASCII format rather than Binary format (default?). We have seen that files written in ASCII format reads fine in Fluent with out any errors. 2) (a) Read (import) your ICEM mesh in GAMBIT using (File -> Import -> Mesh, Fluent5/6, 3d). (b) Export the mesh from Gambit (File -> Export -> Mesh) (c) Read this mesh in Fluent

One advantage here is that GAMBIT will retain all Boundary definitions you have made in ICEM intact. 3) You can try to export a CGNS file from ICEM, and read it in Fluent. However, this way we will loose the naming convention we have used in ICEM mesh. Also please note that files written in binary format are not transferable between Unix and Windows systems.

ME: ----------------------------------------------------- Thanks for the reply! I tried all your suggestions. Here are the results:

1.) By writing in ASCII I received the same errors.

2.) Gambit was not able to read in the mesh. I created a simple mesh of a cube in Gambit, exported it as cube.msh, and then imported it back in without problems. But for any ICEM grid import I got the following errors:

Originally Posted by Gambit

import uns "/home/aero/Desktop/test.msh" angle 135 d3 scale 1 \ Reading |utility fe2ram -m1e-06 -d3 -tRAMPANT -oFIDAP7 /home/aero/Desktop/test.msh (feature angle = 135) ERROR: Error encountered while reading the header information. Makre sure that correct mesh dimension and type has been supplied. Gambit is unable to import. Process completed with exit code 256.

Could this be because I am using 64 bit Linux, and Gambit is a 32 bit program? If that's the case, I will try to get a 32 bit windows install and see if it works then, and post the results. I did check 3-D for the grid import, etc.

3.) Exporting to CGNS in ICEM did work, and Fluent read the mesh in fine. However, it did lose the naming conventions. I'd really like the get the gambit method to work, as I will be doing automated studies, so I need the names to match!

[atheism]

Originally Posted by Robert Perry
;145981

Well, I had a friend try the CFX thing, and it didn't work either!

Error: bad syntax. Usage: utility fe2ram dimension read_format zoning write_format [inputfile [outputfile]] utility fe2ram dimension read_format zoning write_format [inputfile [outputfile]]

dimension: [-d2 | -d3 | -surface]

Building...

grid, Error: Null Domain Pointer

I'll contact Fluent and ICEM tech support and see what they say. I'll be sure to post the results here.

Thanks Joe!

I faced the same situation, but I figure out. There was a wrong path where you saved the file. Change it !