CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   ANSYS Meshing & Geometry (http://www.cfd-online.com/Forums/ansys-meshing/)
-   -   [ICEM] prism and convergence (http://www.cfd-online.com/Forums/ansys-meshing/109762-prism-convergence.html)

Markus November 26, 2012 06:26

prism and convergence
 
1 Attachment(s)
Hi Everyone,


I am trying to mesh an underwater model of a satellite. I made
a prism layer around it and then a tetra mesh. The convergence is really bad in Fluent.
How do i increase the quality of the boundary layer? make especially the elements in the inner corner better?

I would appreciate any help, thank you :-)


Markus

flotus1 November 26, 2012 06:35

What makes you so sure thar the "bad" convergence is caused by the mesh quality?
Did you evaluate some of the quality indicators?

Markus November 26, 2012 07:21

1 Attachment(s)
Yes it seems that the quality especially in the transition between prism and tetra. and also if i have the very small prisms next to the bigger ones thats not very good right? In gambit there was this option to wedge the edges, is there something similar in icem?

Thanks, Markus


In the picture, the elements have a quality worse than 0.2

Far November 26, 2012 07:31

Hey I gave you the fully hexa mesh!!! did you try it? http://www.cfd-online.com/Forums/ans...direction.html

Far November 26, 2012 07:34

for prisms quality of 0.01 is good enough for fluent.

Markus November 26, 2012 07:35

hey

Yes but i didnt manage to make the mesh. It never created the volumes, only surface mesh.

Far November 26, 2012 07:36

Right click on premesh and then select convert to unstructured mesh. Afterwards follow the same procedure you followed for the prsim+tetra mesh i.e. boundary conditions, selection of solver and then output.

Markus November 26, 2012 10:03

1 Attachment(s)
Ok thanks..
I ran it with fluent but the result can not be right.

I put the laminar solver

Far November 26, 2012 10:06

Why laminar? Whats the Reynolds Number? May be your problem is transient!!!

can you attach your case file?

Markus November 26, 2012 11:35

Reynolds number is around 60000

0.2 m/s flow

I thought as long as it doesnt work with the laminar model it wont with the turbulent either..

ill send you the case file per mail

Far November 26, 2012 12:26

2 Attachment(s)
Few things

1. Boundary conditions

I would prefer to define the upper, lower, right side and left side faces as wall with slip condition instead of pressure outlet.

2. Domain

Increase the domain size : Inlet at 15*L and outlet at 25*L

3. Mesh
Most important factor
The hexa mesh is still not finalized model, you need to set the edge mesh parameters, sizing, expansion rate, edge mesh matching, y+ consideration if turbulence is importnat (ever in case of laminar model you need to resolve the shear layers so make sure that the mesh is refined in important areas) etc to make it pleasant to solver.

4. Solver
Try pressure based coupled solver.


5. Flow scheme
First start with 1st order convection scheme then switch to 2nd order.

6. Turbulence or laminar
Also try turbulence model along with transition model.

PS: I believe there would be high level vortex shedding behind your object due to many protruded bodies.

flotus1 November 27, 2012 11:52

Please use some kind of turbulence modeling for turbulent flows. If it still does not converge, you can still spend some time on improving the mesh.
Simulating a turbulent flow as an underresolved DNS cannot create correct results.

Engr.RZA November 28, 2012 10:48

I think the you should try the last steps as mentioned by FAR.

Your Reynolds number suggest that you can assume laminar flow.

Regards,

RZA


All times are GMT -4. The time now is 21:27.