CFD Online Discussion Forums

CFD Online Discussion Forums (
-   ANSYS Meshing & Geometry (
-   -   [ICEM] Rigid sphere falling through air. Dynamic mesh (

alexmeier June 28, 2010 03:49

Rigid sphere falling through air. Dynamic mesh
Hi there

I'm trying to set up a problem in fluent.
I'd like to simulate a rigid sphere falling through air at standard conditions accelerated by gravity onely using a dynamic mesh and UDFs.
right now my problem is, that fluent can't read my mesh. I always get the same Error warning:

WARNING: cell 2 of thread 15 has NULL face pointer 3
ERROR: Build Grid: Aborted due to critical error.

Here is the mesh I wanted to use:

There is a region around the Sphere I have declared as new volume part when I have created the prism Layers. The reason for this is, that I want to move the boundary Layer and the Sphere in my simulation.

I have checked what happens, when I try to read in the same mesh in fluent, whiteout declaring the boundary Layer as new volume part. If i do so, there is no ERROR Warning.

For this reason I know, that there is something wrong whit this volume part declaration. but right now I can't think of any other possibility to realize my simulation.

Does anybody know what's wrong?

the Fluent User Manual says:

"If you create a single grid with multiple cell zones, you must be sure that each cell zone has a distinct face zone on the sliding boundary. The face zones for two adjacent cell zones will have the same position and shape, but one will correspond to one cell zone and one to the other."

I think that' why this ERROR occurs. But I don't understand how to realize this in ICEM?

Is there any other possibility to realize this Problem in Fluent?

thank you so much for your support.

jsm June 28, 2010 05:54


If you want separate fluid domain for prism elements, then specify side part and top part names also with new volume part. You can find these fields just below the new volume part. Then you will not get this error.

alexmeier June 28, 2010 06:00

Thx a lot. I'll give it a try

PSYMN June 29, 2010 09:05

more detail
JSM has the right solution, but I got this question a couple times recently (this week), and this is the longer explanation I typed out for them, so I thought I would post it here for others.

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 shell boundary and each shell should have a normal direction so bocos can be applied, but in your case, there isn't one between the tetras and the prisms.

If you had run your mesh checks, you would have had "uncovered faces" and "surface orientation errors".

There are two ways to avoid this error.

1) if you want the material in two different fluids, you need shells between them. You could get this from the "uncovered faces" check, or by using the "top" option when you put Prism into a different part. Then apply an "internal wall" boco to that internal part.

2) if you really just intended to have one fluid zone (but you had created the prisms first for your movement and therefore had the 2 parts as part of your mesh creation process), then you simply need another step 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.

PSYMN June 29, 2010 09:06

Hexa option...
By the way, this model could be very easily scripted/meshed in ICEM CFD hexa and give you the very best quality mesh possible. Each iteration could be precisely controlled in terms of mesh distribution and would generate much more quickly for a faster solve.

jsm June 30, 2010 00:23

Hi Simon,

Normally I will not get uncovered faces error. If I get this error, I simply use Build mesh topology. This error will be removed automatically.

All times are GMT -4. The time now is 20:36.