CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   Main CFD Forum (http://www.cfd-online.com/Forums/main/)
-   -   viscosity ratio in wake of ellipse - physical meaning? (http://www.cfd-online.com/Forums/main/120858-viscosity-ratio-wake-ellipse-physical-meaning.html)

MachZero July 16, 2013 08:59

viscosity ratio in wake of ellipse - physical meaning?
 
Hello all,

I am trying to model and capture the separation length behind an elliptical cylinder. I have done so reasonably well with k-omega SST but would like to move to an RSM model to get a more certain answer. My grid is high quality in the wake and I am using double precision.

As I activate 1st order RSM, I get a warning that viscosity ratio is greater than 1e5 and then it diverges. I checked my solution and this occurs in the wake. Reading one of ANSYS's response, they state:

Also note that for certain types of flows, for instance atmospheric boundary layer flows, the turbulent viscosity ratio can be as high as 1e+08 or 1e+09. In such cases, the limit can be increased.

Does anyone have any physical idea what range of viscosity ratios are possible in a wake? Should I actually increase this value? I dont have much physical understanding of turbulent viscosity ratio.

triple_r July 16, 2013 09:30

No idea why you are getting turbulence viscosity warnings with RSM, as the whole point of RSM is not having to use the Boussinesq approximation, it might be a post-processing thing. Anyhow, turbulence viscosity value depends on the grid resolution as well as flow conditions, so if the grid is coarse you might get very high values. Have you tried using the SST solution as the initial condition for the RSM run?

flotus1 July 16, 2013 09:53

AFAIK, the turbulent viscosity also depends on the Reynolds number. That is why it can be higher in atmosperic boundary layers.
If the Reynolds number of your flow setup is not exeedingly high, the warning about limited TVR should vanish after some iterations.
If it doesnt, review the boundary conditions and, as triple_r already mentioned, the mesh size and quality in the boundary layer and in the wake region.

MachZero July 16, 2013 10:04

Thank you for your quick responses!

I tried initially using SST values for initialization, but found that when I switched to RSM, it diverged. Looking over ANSYS notes, they recommend initializing using k-e, then switching to RSM. So that is what I have been doing since. I have been using low UR factors in momentum and rsm, and starting with 1st order before switching to 2nd.

I just checked the solution history. The warning is:

turbulent viscosity limited to viscosity ratio of 1.000000e+05 in 19 cells. I will attach an image of my mesh quality. Maybe it really isnt high enough.

My Re is about 1,000,000.

Thank you both for responses.

MachZero July 16, 2013 10:14

2 Attachment(s)
Under closer inspection, I see on the midplane of my "wind tunnel", the TVR is maxing out around 6000, BUT near the symmetry plane (3d simulation of elliptical cylinder using symmetry plane) is where I am getting very high values. I have attached two images that show this (range for picture with mesh is 0-6000, range for image with red blip is 0-85000).

High TVR values are not reducing with iterations, but rather generating in more cells with iterations. I have seen several posts on this forum seeing similar issues , so thank you for your responses! I would love to get this figured out.

Attachment 23536

Attachment 23537

flotus1 July 16, 2013 11:33

How about the Y+ values? And the aspect ratio of the cells where the maximum value of TVR occurs? Does this point coincide with the separation point?

triple_r July 16, 2013 11:59

With regard to initialization, you are absolutely right, depending on the seventh equation for RSM you might be better off with k-e instead of k-o.

As flotus1 mentioned, you might want to check your grid around that blip for aspect ratio. If y+ is low, you can get rectangular elements stretched in the direction parallel to the wall, and usually that is a good way to save on elements as gradients are much higher normal to the wall than parallel to the wall. But, if that point is near the separation point, then you probably need more square-like elements.

From your pictures it looks like you are using a "mapped" mesh, if that is so then try slicing the domain radially right where the blip is, and add gradients to the line meshes on the two sides of the slice so that they become finer near the blip. Let me see if I can show this in a schematic picture :-) I made it in paint, so sorry for the bad quality :-p

http://www.cfd-online.com/Forums/dat...AASUVORK5CYII=

triple_r July 16, 2013 12:02

1 Attachment(s)
Sorry, the picture didn't get attached, so hopefully here it is.

MachZero July 22, 2013 16:32

First off thank you all for your suggestions. I have taken a step back and taken some time to look at this file with reapect to all your comments.

First thing to note is that yes I have a y plus of 1. Next is that I have found that if I use an fmg initialization and run 1st order rsm immediately it does not diverge. I ran it for 10k iterations so I am pretty sure of that. I switched to second order and it diverged eventually. Note that the regions with ultra high tvr were at the symmetry planes.

An ansys engineer told me that I should use kw sst since it will give a better solution then switch to rsm. He said that when I do that I should freeze the flow and solve turbulence only for a while. I tried this approach with several variations and it still diverged.

Last thought is to build a coarser mesh and use non equilibrium wall functions. Should I be worried about this killing bl calculations and separatipn location calculation since it is not being resolved?


All times are GMT -4. The time now is 09:28.