CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   CFX (http://www.cfd-online.com/Forums/cfx/)
-   -   wall shear in immersed solid (http://www.cfd-online.com/Forums/cfx/105405-wall-shear-immersed-solid.html)

hamed.majeed July 30, 2012 08:09

wall shear in immersed solid
 
Hi,

In immersed solid module of cfx, I need to find the wall shear; basically use it to find the skin friction coefficient cf
It seems that the immersed solid does not recognize wall shear.
I calculate cf using the following expression:
Wall Shear/(0.5*massFlowAve(Density)@inlet *Uinf^2)

But Wall Shear seems unrecognized.
If I need to plot friction factor for an immersed solid how should I do it!!

Thank you

Regards
Hamed

ghorrocks July 30, 2012 18:26

Immersed solid do not have wall shear as a variable as they are not modelled as walls, but as momentum source terms. You are going to have to calculate wall shear another way - maybe looking at the general flow stress tensor at the locations near the wall or some other calculation which evaluates to wall shear.

hamed.majeed July 30, 2012 22:23

Thnx for the reply.

I figured out two ways, actually the problem is with wall shear.

Method 1:
As wall shear stress is given by
http://s19.postimage.org/6ypmbgulf/Untitled28.png
Then in cfx we can use the expression

Wall Shear = 0.0000198 [Pa s] *Velocity u.Gradient Y
where 0.0000198 is viscosity of air.

I tested this for a flat plate analysis done earlier

Using Wall Shear this was the plot
http://s19.postimage.org/45werfu8z/Untitled29.png

Then I used the expression 0.0000198 [Pa s] *Velocity u.Gradient Y, this was the plot
http://s19.postimage.org/deyl1k34z/Untitled30.png

The results are fairly different,
What is the issue.

Method 2
I then found this link http://www.cfd-online.com/Wiki/Skin_...on_coefficient and decided to use and empirical value. My Max reynolds number is 10^6. I decided to use the first empirical expression. But the problem was that this error!
WARNING
No data exists for variable 'CF' specified in object 'Series 1'\'Chart Line 1'.



Please help!

Regards
Hamed

ghorrocks July 30, 2012 23:51

For the first one: Immersed solids use a momentum sink to behave like a wall. They do this with a factor which has to be a balance between stopping the flow enough to act like a wall versus numerical stability. You need to do a sensitivity analysis on this parameter to check this parameter is set adequately before making any assessments about the accuracy of the approach.

For two: You have not defined the variable "CF" properly. The error message is pretty clear.

hamed.majeed July 31, 2012 00:51

By the factor do you mean the momentum source scaling factor, well I have found out that momentum source scaling factor performs best for momentum source scaling factor of 100 or above. I did that for a flat plate

http://www.cfd-online.com/Forums/cfx...sed-solid.html

hamed.majeed July 31, 2012 00:56

About the method 1, I suggested earlier, it is for a general case not immersed solid. I compared the value of wall shear with the general accepted definition, but the results differ!!
I mean Wall Shear = 0.0000198 [Pa s] *Velocity u.Gradient Y is the definition of wall shear, so it must be justified, unless it is not the case.

ghorrocks July 31, 2012 03:02

I understand now. Are you reporting hybrid or conservative values?

hamed.majeed July 31, 2012 04:17

I am using hybrid values.

ghorrocks July 31, 2012 06:46

What does it give you if you use conservative values?

hamed.majeed July 31, 2012 13:55

Conservative or hybrid values makes no difference, also the difference between either using wall shear or 0.0000198 [Pa s] *Velocity u.Gradient Y is very large.

ghorrocks July 31, 2012 19:07

I suspect it is using conservative variables and hybrid variables are not available for this calculation.

I think the problem is that your equation is based on the value in the control volume next to the wall (ie an average of the wall to a distance out from the wall) and the wall shear stress is evaluated at the wall. To check this, if you do a mesh refinement you will find your equation getting closer as you refine the mesh.


All times are GMT -4. The time now is 16:00.