CFD Online Discussion Forums

CFD Online Discussion Forums (
-   FLUENT (
-   -   .msh file cann't be by Fluent (

nchuche June 17, 2010 23:03

.msh file cann't be by Fluent
Fig. 1 is my model. The origin part is a vessel (import by .stl file), and the green part is an extension. Two regions are fluid. The extension is built by means of “extrude mesh” method from INLET part. Then, I delete the mesh of the INLET part. Then, I make a .msh file and a .cfx file for for Fluent and CFX, respectively. Unfortunately, .msh file can not be read by Fluent, but .cfx file can by CFX. I can’t use CFX. Fig. 2 is the message of the Fluent. Who can tell me where the problem is and give me some suggestions to fix this ICEM file.
p.s. 1 If I didn’t delete the mesh of the INLET part, the .msh file can be read by Fluent. But the INLET part becomes a wall. This boundary is not my want.

(So strange, I can't attach my doc file....)
The message in the Fluent is
> Reading "E:\post doc\research\2010-biomechanics plan\plan\2010-Amira-chest-CT\chest CT model practice\20100609-tracheal\mesh\fluent3-1.msh"...
6432 nodes.
26534 tetrahedral cells, zone 14.
1500 wedge cells, zone 15.
51202 triangular interior faces, zone 16.
3445 mixed interior faces, zone 17.
100 triangular pressure-outlet faces, zone 18.
3557 triangular wall faces, zone 19.
460 quadrilateral wall faces, zone 20.
75 triangular wall faces, zone 21.
Cell Centroid is xc -4.454064 yc -7.567721 zc 440.377377
WARNING: cell 5 of thread 14 has NULL face pointer 3.Error: Build_Grid: grid error.
Clearing partially read grid.
Error: Null Domain Pointer
Error Object: ()

"Error: Null Domain Pointer"...I have seen many times in this forum, but I don't know how to fix my model.

PSYMN June 29, 2010 10:38

Uncovered faces
In Fluent, you can not have two different fluid volumes next to each other without a boundary between them. If you do that, you will get a "null pointer" error. This really means that each fluid volume should have a boundary with a normal direction so bocos can be applied, but in your case, there isn't one.

This problem happened because you extruded the end with a new volume part and then removed the shells between the original fluid volume and the extruded fluid volume. If you had run your mesh checks, you would have had "uncovered faces" and "surface orientation errors".

There are two options for the fix. 1) if you want the material in two different fluids (perhaps one is a porous media or you have some other reason), don't delete the shells between them. Instead, apply an "internal wall" boco to that internal part (make sure it is different from the INLET part). 2) if you really just intended to increase the length of the fluid (so that your boundary flow could more fully develop or something like that), then you simply need to add all the volume elements to the same part. In the model tree, right click on the volume part you want to keep (perhaps (FLUID)) and choose "Add to Part". The message int he display window should say "select elements". (if it says select entities, then you should click the last icon in the selection toolbar so it changes to "select elements".) Then click the second last icon in the selection tool bar to select all the volume elements in your model. Now that all the volume mesh is in the same part, you can run the mesh checks and won't get the uncovered faces error, even after deleting the internal inlet face. You also won't get the null pointer error in Fluent.

By the way, this model (a blood vessel with and extruded end) could be very easily meshed in ICEM CFD hexa and give you the very best quality mesh possible.

All times are GMT -4. The time now is 06:32.