CFD Online Discussion Forums

CFD Online Discussion Forums (https://www.cfd-online.com/Forums/)
-   ANSYS Meshing & Geometry (https://www.cfd-online.com/Forums/ansys-meshing/)
-   -   [ICEM] 2D meshing (https://www.cfd-online.com/Forums/ansys-meshing/109329-2d-meshing.html)

Thomashoffmann November 15, 2012 05:56

2D meshing
 
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 November 15, 2012 10:47

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

Thanks :confused:

diamondx November 15, 2012 12:05

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 November 15, 2012 13:50

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 November 15, 2012 13:58

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 November 15, 2012 14:20

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:confused:

And yes I'm exporting for CFX

diamondx November 15, 2012 15:41

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 November 15, 2012 16:15

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 November 15, 2012 18:01

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 November 16, 2012 01:43

2 Attachment(s)
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

http://img706.imageshack.us/img706/9958/86435442.png

http://img210.imageshack.us/img210/285/35236929.png

Thomashoffmann November 16, 2012 03:30

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 November 16, 2012 03:37

@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 November 16, 2012 03:47

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 November 16, 2012 05:09

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

Thomashoffmann November 16, 2012 08:12

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 November 16, 2012 11:18

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 November 16, 2012 12:00

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


All times are GMT -4. The time now is 01:53.