CFD Online Discussion Forums (https://www.cfd-online.com/Forums/)
-   FLUENT (https://www.cfd-online.com/Forums/fluent/)
-   -   why in fluent report the skin friction coefficient is positive (https://www.cfd-online.com/Forums/fluent/108511-why-fluent-report-skin-friction-coefficient-positive.html)

 gomnam15010 October 25, 2012 06:32

why in fluent report the skin friction coefficient is positive

hi.
why in fluent report the skin friction coefficient is positive in everywhere of separation zone?! while in separation zone the skin friction coefficient must be negative.

 cfd seeker October 25, 2012 06:44

Quote:
 Originally Posted by gomnam15010 (Post 388451) hi. why in fluent report the skin friction coefficient is positive in everywhere of separation zone?! while in separation zone the skin friction coefficient must be negative. please help me thanks for your attention
Skin friction coefficient is always positive and what do you mean by separation zone?

 gfoam October 25, 2012 07:32

Quote:
 Originally Posted by gomnam15010 (Post 388451) hi. why in fluent report the skin friction coefficient is positive in everywhere of separation zone?! while in separation zone the skin friction coefficient must be negative. please help me thanks for your attention
Be careful, because the criterion of skin friction (Cf) equals cero (not negative) to find flow separation only aplies when you have a 2D case like a 2D airfoil or a cylinder, but not in 3D cases like a wing.

 gomnam15010 October 25, 2012 08:27

Quote:
 Originally Posted by cfd seeker (Post 388452) Skin friction coefficient is always positive and what do you mean by separation zone?

in the separation zone the velocity gradiant is negative and so the skin friction coefficient must be negative

 gfoam October 25, 2012 09:01

Quote:
 Originally Posted by gomnam15010 (Post 388471) in the separation zone the velocity gradiant is negative and so the skin friction coefficient must be negative
But in which reference frame the velocity gradient is negative? May be FLUENT calculates the Cf with the absolute value of the wall shear, may be you must look at the components of wall shear and see if there is separation or not. regards
Gonzalo

 sbaffini October 25, 2012 09:37

The total wall shear stress used by fluent in defining the skin friction coefficient is, of course, a positive definite quantity (it is the magnitude of the total stress). Do what Gonzalo said and you will find what you're looking for.

 manukamin March 14, 2013 02:27

I'm having the same problem here. The velocity vectors over the airfoil surface is clearly reversed(flow reversal). But then the skin friction coefficient plot is positive everywhere.

I understand the possibility that Fluent might be using only the magnitude of wall shear stress to calculate the skin friction, hence it being positive everywhere. But of course, it is physically incorrect.

So is there any option in Fluent by which I can get the actual physical skin friction coefficient plot?

 flotus1 March 14, 2013 03:22

It is not physically incorrect.

The skin friction coefficient based on the wall sheat stress magnitude has to be positive.
If you want negative values in recirculation zones, you will have to evaluate the components of the wall shear stress.

 manukamin March 15, 2013 05:48

Hi Alex,

Thanks for the response. However, Fluent seems to ignore the sign of even the wall shear stress. So there is no way for me to even evaluate cf from the wall shear stress by myself too. So how can I obtain negative cf in recirculation zones?

 flotus1 March 15, 2013 06:33

Quote:
 Originally Posted by manukamin (Post 414144) However, Fluent seems to ignore the sign of even the wall shear stress
I know for a fact that the streamwise component of the wall shear stress changes sign in a recirculation zone in reality and in fluent aswell.
What exactly are you simulating? Please post a picture of your setup with the orientation of the coordinate axes.

The wall shear stress is a a vector, it should have two components, say x-wall-shear & y-wall-shear in 2D simulation and three components in 3D simulation. Maybe there is something called "wall stress" which actually is the magnitude of wall stress vector, then you should look into the stress vector instead.

Fluent does do funny things. It reports the magnitude instead of the z-component of vorticity in 2D simulation.

Quote:
 Originally Posted by manukamin (Post 414144) Hi Alex, Thanks for the response. However, Fluent seems to ignore the sign of even the wall shear stress. So there is no way for me to even evaluate cf from the wall shear stress by myself too. So how can I obtain negative cf in recirculation zones?

 manukamin March 18, 2013 09:04

1 Attachment(s)

I'm simulating a flow problem in a 2-D compressor cascade. Hence my upper and lower walls are periodic.

I have attached an image of my meshed domain. Now the thing is that the wall shear stress is shown to be positive everywhere as per fluent (complete and not x and y). But I see that there are some recirculation zones when i plot the velocity vectors. Does that make sense? Or should I individually plot x and y wall shear stress?

I'm not sure how to display the co ordinate system. In Fluent are X and Y directions are as per a fixed global co -ordinate system or is it a local co-ordinate system that varies from point to point in which x is in the streamwise direction and y in the normal direction?

X- and Y- directions are global coordinate system. The wall shear in Fluent is the magnitude of wall shear stress vector so that it is always positive. But the shear should approach to zero near the separation point. Then you can do a xy-plot to verify whether that the x-wall-shear change its sign around that point.

 manukamin March 19, 2013 02:27

Well then my problem still persists! There is no way I can know if there is a recirculation zone if the shear stress plotted is always positive. Of course x and y shear stresses do have magnitude as well as a sign. But what's the point? They are as per a global co ordinate system. Since each element of my airfoil is oriented at a unique angle, there is no way that the x and y shear stress can tell me anything about streamwise and stream-normal shear stress.

Unless, I create a custom function that resolves the x and y shear stress into streamwise and stream normal vectors at each element along the airfoil surface (wall).. But I'm not sure how to do that on Fluent.