|
[Sponsors] |
November 26, 2012, 05:26 |
prism and convergence
|
#1 |
New Member
Join Date: Oct 2012
Posts: 14
Rep Power: 13 |
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 |
|
November 26, 2012, 05:35 |
|
#2 |
Super Moderator
Alex
Join Date: Jun 2012
Location: Germany
Posts: 3,399
Rep Power: 46 |
What makes you so sure thar the "bad" convergence is caused by the mesh quality?
Did you evaluate some of the quality indicators? |
|
November 26, 2012, 06:21 |
|
#3 |
New Member
Join Date: Oct 2012
Posts: 14
Rep Power: 13 |
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 |
|
November 26, 2012, 06:31 |
|
#4 |
Super Moderator
|
Hey I gave you the fully hexa mesh!!! did you try it? http://www.cfd-online.com/Forums/ans...direction.html
|
|
November 26, 2012, 06:35 |
|
#6 |
New Member
Join Date: Oct 2012
Posts: 14
Rep Power: 13 |
hey
Yes but i didnt manage to make the mesh. It never created the volumes, only surface mesh. |
|
November 26, 2012, 06:36 |
|
#7 |
Super Moderator
|
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.
|
|
November 26, 2012, 09:03 |
|
#8 |
New Member
Join Date: Oct 2012
Posts: 14
Rep Power: 13 |
Ok thanks..
I ran it with fluent but the result can not be right. I put the laminar solver |
|
November 26, 2012, 10:35 |
|
#10 |
New Member
Join Date: Oct 2012
Posts: 14
Rep Power: 13 |
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 |
|
November 26, 2012, 11:26 |
|
#11 |
Super Moderator
|
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. Last edited by Far; November 26, 2012 at 11:51. Reason: Images |
|
November 27, 2012, 10:52 |
|
#12 |
Super Moderator
Alex
Join Date: Jun 2012
Location: Germany
Posts: 3,399
Rep Power: 46 |
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. |
|
November 28, 2012, 09:48 |
|
#13 |
New Member
RZA
Join Date: Nov 2012
Posts: 25
Rep Power: 13 |
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 |
|
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
Convergence and discretization | karananand | FLUENT | 3 | August 29, 2010 06:07 |
Discretization and convergence | karananand | Main CFD Forum | 0 | August 4, 2010 16:19 |
early stall, poor convergence, and mesh quality | everest | CFX | 2 | May 12, 2010 16:27 |
Convergence issue in SST for Porous model | Raj | CFX | 0 | May 2, 2008 02:43 |
problem in convergence with the prism layer genera | rakesh | CFX | 3 | September 18, 2006 10:13 |