I think, you have to do external loop. Linux script (loop for check convergence and start new computation) is a possible solution.

Which CFD solver do you use for your calculation? Which convergence criteria do you use? Could you also provide some more information about your setup (i.e. used models) - this might help to give a more helpful answer.

Also, I don't understand why you want to adapt the boundary conditions based on a non-converged flow calculation. Everytime you assign new values to your boundary conditions, you alter the mass balance of your system...

Best regards,

Stephan

Hi Stephan

  Thanks for your answer. I am using Volume of Fluid method (VOF) in Ansys Fluent to simulate two phase slug flow. The problem is that to reach the pseudo-steady solution the Taylor bubble should ceases moving up or down in the axial

direction of the bubble and hence the inlet velocity is the terminal velocity and convergence is established. So if that is not reached we need to calculate new velocity (based on bubble movement in solution) and reassign new velocity in boundary condition.

Hi Enass,

Got it - never worked on Taylor bubbles before.

As you might know, the inlet boundary can be adjusted with the DEFINE_PROFILE() macro. Assuming that you can define a uniform inlet velocity, this part of the UDF would look something like:

DEFINE_PROFILE(veloprofile,t,i)

{begin_f_loop(f,t)

{ F_PROFILE(f,t,i)=vin;}   /*vin has to be calculated based on the Tayler bubble velocity*/

end_f_loop(f,t)

}

The local gas volume fractions and velocities, which should be required to calculate the velocity of the rising bubble, are accessible with a loop over all cells inside your domain considering the subthreads of your two phases, something like:

Domain *domain = Get_Domain(1);  /*domain index, typically 1*/

Thread *thread;

cell_t c;

thread_loop_c(thread,domain)

{

Thread *subthreadg = THREAD_SUB_THREAD(thread,1); /*gas phase*/

Thread *subthreadl = THREAD_SUB_THREAD(thread,0); /*liquid phase*/

begin_c_loop(c,thread)

{

alpha = C_VOF(c,subthreadg);

u = C_U(c,thread); /*x-velocity*/

v = C_V(c,thread); /*y-velocity*/

w = C_W(c,thread); /*z-velocity*/

} }

end_c_loop(c,thread) /*end of cell loop*/

}

I'm still not sure how to calculate the inlet velocity based on the Taylor bubble velocity. However, the bigger issue might be the termination/restart of your calculation - I don't know any macro in Fluent that would provide this functionality and I also could not find anything in the UDF manual (version 15 available for download here: http://148.204.81.206/Ansys/150/ANSYS%20Fluent%20UDF%20Manual.pdf). As far as I know, you can only simulate a pre-defined number of time-steps or iterations and I don't know any way to start a new calculation automatically (other than using a journal file, but this doesn't help in your case...). For such detailed questions, I recommend to contact the ANSYS support, or to ask for help in the CFDonline forum (http://www.cfd-online.com/Forums/main/)

Hope this helps!

Best regards,

Stephan

Hi Stephan

   Thanks alot for reply. Yes i agree with the define profile part to update the velocity at the boundary condition. Bu the problem i am facing is that.; i estimate the in let velocity from correlation and place it as a parameter in fluent as it has to be assigned at 2 boundary conditions, then i run the case file for a round 2 seconds, then i check the bubble velocity by the following;

   checking x distance for the isosurface of vof 0.5 at t=0s and at t=2s by report from fliuent, then the distance traveled by the bubble= x at t=2s- x at t=0s/ 2 seconds. 

Then  i calculate new inlet velocity = initial velocity - velocity moved by the bubble. Then i repeat the process until there is small changes between the velocities an hence the bubble ceases moving in the =axial direction and convergence is established. 

So do you have any suggestions on how to calculate the distance and check convergence??

  Your help is most appreciated.

  Thanks

    Enass

Hi Enass,

You have a quite difficult task ;-)

Never did such calculations, hence just an educated guess: You should be able to calculate a representative length scale of your bubble using the F_CENTROID macro. This estimates the coordinate position of the centroid of the face f and stores the coordinates in the x array. I would try to pass the ID of the isosurface at vof=0.5 to your UDF, loop over the faces of this isosurface, get the centroids and calculate for example the mean y-coordinates (if the bubble rises in y-direction the mean value should increase over time with a rate corresponding to the rising velocity).

The surface ID can be hard coded or can be set/get with the RP_GET and RP_SET macros. The thread pointer can be looked up with:

Thread *thread_name = Lookup_Thread(domain, zone_ID) /*zone_ID is the ID of the isosurface */

The loop would look something like:

face_t f;

begin_f_loop(f,t)

{F_CENTROID(x,f,t);

xcoord = x[0]; ycoord=x[1]; zcoord=x[2]; 

ysum=ysum+ycoord;

ycount++;

}

end_f_loop(f,t)

yave=ysum/ycount;

}

If you include this code in an EXECUTE_AT_END function, you can return the result to the TUI at the end of the 2s simulation. Again, this is just a first idea and I never tested this (unfortunately i also have no time to try it).

Hope this helps.

Regards,

Stephan

Hi 

   Thanks alot for your reply. I know its so hard.  i will give it a try. Thanks alot.