CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   Main CFD Forum (http://www.cfd-online.com/Forums/main/)
-   -   No recirculation zone, why?? (http://www.cfd-online.com/Forums/main/113389-no-recirculation-zone-why.html)

o_mars_2010 February 19, 2013 03:30

No recirculation zone, why??
 
I have developed a code to simulate a flow past a circular cylinder using Immersed Boundary Method.
I set Re=40, and the free stream inlet velocity to 1 and the diameter of the cylinder 0.1.
The resultant streamlines results have no recirculation zone behind the cylinder .
Could any one help me to know what is the reason?

FMDenaro February 19, 2013 04:42

Quote:

Originally Posted by o_mars_2010 (Post 408615)
I have developed a code to simulate a flow past a circular cylinder using Immersed Boundary Method.
I set Re=40, and the free stream inlet velocity to 1 and the diameter of the cylinder 0.1.
The resultant streamlines results have no recirculation zone behind the cylinder .
Could any one help me to know what is the reason?

At Re=40 you should have a steady, symmetric separation. Have you reached a full steady state? Are you using upwind discretization? what about your grid?

o_mars_2010 February 19, 2013 05:12

i am using AB-CN discretisation on a staggered grid, the mesh size 0.1D, and a time step of 0.01.
I think i reached the steady state because there is no change in the velocity contours or the vorticity contours is taking place.

o_mars_2010 February 19, 2013 05:16

an intersting thing happened when i changed the Re to 500 i could watch a steady state recirculation zone ????

is my inlet velocity has to be adjusted according to the Re ??
I mean
if Re =40 then the inlet velocity should be

U=viscosity*Re/(D)
because i specified the inlet velocity to be 1, with no relation to Re

FMDenaro February 19, 2013 07:53

Fix your Re number, then you have to fix two among the parameters U, D, viscosity.

Furthermore, AB-CN is a time integration scheme, but says nothing about the spatial discretization

o_mars_2010 February 19, 2013 08:19

sorry, i used second order centeral difference for the spatial discretization.
I will repeat what you say from my understanding to it:
So, for example if i want to make a simulation at Re= 40 around a cylinder with a diameter 0f 0.1 using the kinematic viscosity of water, then the free stream velocity (inlet velocity) will be equal to: (fixing the diameter and viscosity)
U=40*1.04e-6/0.1=4.16e-4 m/s
and in the case of Re=150, the free stream velocity will be:
U=150*1.04e-6/0.1=1.56e-3 m/s

FMDenaro February 19, 2013 08:25

Quote:

Originally Posted by o_mars_2010 (Post 408697)
sorry, i used second order centeral difference for the spatial discretization.
I will repeat what you say from my understanding to it:
So, for example if i want to make a simulation at Re= 40 around a cylinder with a diameter 0f 0.1 using the kinematic viscosity of water, then the free stream velocity (inlet velocity) will be equal to: (fixing the diameter and viscosity)
U=40*1.04e-6/0.1=4.16e-4 m/s
and in the case of Re=150, the free stream velocity will be:
U=150*1.04e-6/0.1=1.56e-3 m/s


correct ;)

be sure you respect the stability constraint for the AB-CN scheme with central second order discretization

o_mars_2010 February 19, 2013 08:31

Thanks a lot for your help.
About the stability condition, i think because i am using an implicit way for the treatment of the viscous term then, the restrict constrain of time will be relaxed, so:
dt<=dx/U
However, i am not sure about the IBM, may be it add additional constrain on the time step!!!

o_mars_2010 February 20, 2013 03:19

I have a very strange results:
When i set the kinematic viscosity as 1.04e-6 i have no recirculation zone.
however, when i set it to 1e-2 i clearly see the recirculation zone.
i calculate the free stream velocity according to the relation i mentioned above in both cases of viscosity.
could you please explain to me why this happened???

FMDenaro February 20, 2013 06:46

by retaining the same reynolds number? :confused:

o_mars_2010 February 20, 2013 07:25

I am using the non-dimensional form of N-S equation, So i have to set the Reynolds no. and the inlet velocity explicitly, the viscosity does not appear explicitely in the momentum equations.
So, lets say i want to make a simulation of flowing water past a circular cylinder with a diameter D=0.1 at Re=40 and the kinematic viscosity of water is 1.04e-6, then the calculated inlet velocity will be U=40*1.04e-6/0.1=4.16e-4 m/s.
I set the parameters like that in my problem, however i didn't have any circulation.
However, when i changed the kinematic viscosity to 1e-2 (i do not know what fluid have such a value) i got circulation zone!!!!!!!!!!!!
So, my question why i do not have a circulation zone for water???

o_mars_2010 February 20, 2013 07:29

Diameter=0.1; % cylinder diameter
%kinematicviscosity=1.04e-6; %water at 20 'C
kinematicviscosity=0.01;
ineltvelocity=Re*kinematicviscosity/Diameter;

FMDenaro February 20, 2013 09:25

I do not understand what you are done... if you have non-dimensional equations (and a non dimensional domain), the only parameter to set is the Reynolds number!

o_mars_2010 February 20, 2013 09:31

So, how can i specify the inlet velocity (Dirchilit B.C) on a recatangular domain ?

FMDenaro February 20, 2013 09:36

Quote:

Originally Posted by o_mars_2010 (Post 409007)
So, how can i specify the inlet velocity (Dirchilit B.C) on a recatangular domain ?

The non-dimensional inlet is the same as well as the non-dimensional diameter!

o_mars_2010 February 20, 2013 09:46

So, if i have a rectangular domain of 40D * 30D, and a grid size 0.05D
then, the non dimensional diameter will be equal to 1
and the non dimensional inlet velocity will be equal to 1
and the rectangular domain will be equal to 40*30
and the grid size will be equal to 0.05

o_mars_2010 February 20, 2013 09:55

x*=x/D, u*=u/U, t*=t.(U/D)

FMDenaro February 20, 2013 11:21

.... yes ! :)

o_mars_2010 February 20, 2013 11:23

Thank's a lot. :)

o_mars_2010 March 18, 2013 23:42

Dear Dr. Filippo
i have some strange results:
when i set the mesh size to 0.1D, i have a good results for the length of the recirculation zone and the drag coefficient.
l/D=2.33 & Cd=1.55
On the other hand, when i decrease the size of the mesh to 0.05D, which is supposed to give better results, it gives worth results:
l/D=2.03 & Cd=1.39

Could you tell me please what could be the reason ???


All times are GMT -4. The time now is 17:07.