[Thomashoffmann]

Hi All.
I want to make a simulation of non newtonian fluid running in a tube. I have created a 2D mesh in ICEM, but when I'm trying to export the mesh I get the following error:
https://dl.dropbox.com/u/19953951/Capture1.PNG

Is this because ICEM don't understand that its only an area-mesh.
How do I construct a 2 dimensional mesh for my task?

Thansk

[Thomashoffmann]

I really don't understand why ICEM wants me to define a volume mesh on a 2 dimensional grid. Can anyone explain?

Thanks

[diamondx]

can you show us some picture of your geometry. did you make sure to sketch on the XY plane ? it has to be XY plan.

[Thomashoffmann]

Hi Ali.
I made 4 points by explicit coordinates; (0 0 0),(2 0 0)(2 0.1 0)(0 0.1 0) ie. a square in the XY-plan..
I created curves between the points and then I created a surface from the 4 curves.
Then I went to the mesh tap and then 'surface mesh setup' and computed the 'surface mesh only', see picture below
https://dl.dropbox.com/u/19953951/Capture2.PNG
But when I try to write the input I still get the same error (as shown in the picture)...
Am I missing something as I'm setting up the mesh?

[diamondx]

have you created a body ?? once i had a problem similar and i created a body, named it fluid , then generated the mesh again. you trying to export for cfx ?

[Thomashoffmann]

Yes, I just started over again. And I made a Body named fluid and generated a mesh as before.. I still get the exact same error

And yes I'm exporting for CFX

[diamondx]

weird, it should be a very small forgotten detail. i have never tried to export a mesh for cfx, may be the problem comes from the boundary condition you declared. if you don't mind sharing your project i can take a look at it...

[Thomashoffmann]

I tried to double check my boundary conditions, but couldn't see any problems.. I think it should be kind of simple, but I can't find it - but if you can help me with it I will be gratefull

https://dl.dropbox.com/u/19953951/cap.zip

[diamondx]

i couldn't locate the problem, i never had the chance to mesh a simple 2d geometry like this without using the block... that being said i blocked it and generated the mesh, when i exported it to fluent it work. you just need to change it to CFX. Also i noticed that you mentioned ANSYS-CFX, maybe you should try CFX-4 instead ?
here is the link : https://dl.dropbox.com/u/35161486/cap.zip

[Far]

In hexa meshing, ICEM automatically extrude the mesh by one element, when you output the mesh for CFX solver. But for direct meshing algorithms (denauly, octree or auto-block) you need to extrude the mesh by one element. For details see the attached pic

[Thomashoffmann]

Thanks Ali. It seems that I have to do blocking. I'm new in ICEM and I haven't heard about blocking before. Can you explain what it is? or do you know where I can read about it?

[Thomashoffmann]

@Far, If I extrude my mesh by one element in the Z direction wouldn't my geometry turn out as a 3 dimensional problem?

[Far]

No. If you define the symmetry condition on two side walls (two x-y planes at two z locations) in CFX (or any code), you will get the 2d results. This is done (mandatory) because CFX is 3d solver and wont accept 2d meshes and therefore ICEM is not exporting 2d mesh for CFX and asking for volumes.

Try to export your original mesh and set the solver as Fluent and see the difference. You can also read this mesh in Fluent without any error.

Moreover you can export the mesh in Fluent format (.msh) and when you read this mesh in CFX, it will automatically extrude it by one element.

As Ali suggested blocking method is good thing to learn, although may be it is tough in starting and will give you full control.

[Thomashoffmann]

----------------

[Thomashoffmann]

ok thanks. But when I open my mesh in cfx and apply an inlet velocity it gives me a strange result, see below

https://dl.dropbox.com/u/19953951/Capture3.PNG

is this because my boundary conditions are made wrong?
I'm not sure whether I have to attach symmetry on my top curve or top plan. And the same for my wall condition - do I have to attach it on the bottom curve or the bottom plan?
Do I need to worry about the third dimension face - shouldn't it be defined as a fluid domain? and the same for the back face, or can I just ignore that face?

[Far]

What boundary you would use for top and bottom if that was the 2d case?

Few thoughts:
If that is not the pressure outlet or inlet or wall or you are simulating wind tunnel then I will define them symmetry condition for top and bottom.


It is for sure that symmetry condition will be defined for two side walls.

[Thomashoffmann]

Never mind, I figured it out - Thanks for your help