CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   CFX (http://www.cfd-online.com/Forums/cfx/)
-   -   Opening boundary condition (http://www.cfd-online.com/Forums/cfx/119243-opening-boundary-condition.html)

hmasenger June 12, 2013 15:30

Opening boundary condition
 
Hi all
Opening boundary condition. I am modeling super cavitation in a pipe.as model runs and the vapor cavity reaches the outlet boundary the solver expresses an error that a wall has been placed at 100% of the outlet and suggests to turn the outlet to opening boundary condition!
Do you think this kind of BC doesn’t affect the results? Should I really change the pressure outlet BC to an opening one?

ghorrocks June 12, 2013 18:46

A better solution would be to extend the outlet boundary downstream so the cavitation region is not present at the outlet.

hmasenger June 13, 2013 00:29

Tnx for the answer glenn
one more thing
i have read somewhere that in cavitation modeling in fluent we should first start simulation at a pressure which we are sure that cavitation does not occur and without activating the cavitation function and then we should use the results as initial condition and after that we can reduce outlet pressure or increase the inlet pressure in some steps while cavitation function activated and monitor this phenomena.(one run without cavitation activated for first step and activated cavitation function for next steps)
Now do i need to follow this procedure in CFX too?
what if we just run the model without cavitation function activated and then use results as initial cond for every single step(one run without cavitation activated and one with cavitation activated for every steps).
(i dont know if you got my point or not )
Best regards

ghorrocks June 13, 2013 06:37

I think I get your point.

For all the steady state cavitation modelling I have done I did an initial simulation with the cavitation model not activated but at full system flow. Then you use this as an initial condition for a simulation with the cavitation model activated. I have never tried ramping the pressure up from below the cavitation point - I suspect many simulations do not need this additional complexity as the simple initial condition with cavitation not activated is good enough.

hmasenger June 13, 2013 07:37

tnx glenn i will keep it in my mined

hmasenger June 13, 2013 11:46

3 Attachment(s)
:(:(:(I have found that the error ‘’100% wall has been place at the outlet ...’’ in not related to reaching the cavity length to outlet boundary!!
I should say I don’t know what is going on?!! i have used a fully converged initial condition for the cavitation activated run and I have used this method for several runs and I get several good results for other valve openings but I don’t know why I get this massage for this situation!
The grid has acceptable quality (maximum skewness =0.88)
Initial condition without cavitation activation is fully converged (RMS =10e-6)
The momentum and mass RMS values are experiencing severe fluctuation and The volume fraction RMS mass is fluctuating
!!The error (the 100% wall has been placed…) is emerging and disappearing after some iterations and this starts over and over!!
Don’t you think I have reached to some special kind of cavitation (like attached cavitation, sheet cavitation or cloud cavitation or…)that CFX default cavitation model cant simulate ?
Pleas guide me .I am really confused
here are some pic of water volum fraction befor solver failor

ghorrocks June 13, 2013 18:43

This is common in cavitation studies.

The 100% wall is not an error, it is a warning. It means it is having a hard time converging. It might pull through it, but it probably needs some help.

Based on your images I doubt there is a steady state solution to this flow. It is almost certainly transient. So try a transient run with adaptive time steps (homing in on 3-5 coeff loops per iteration, but this case might need 5-10 as it is a tricky multiphase simulation).

But before you try a transient run (which will take a long time), try local timescale factor=5.0. Run that for a while and it might be able to get the convergence started.

hmasenger June 15, 2013 17:51

tnx glenn for the clue
i think i have found the problem.i just decreased the pressure steps(steps which i am increasing on inlet BC up to cavitation happening- first it was 0.3e5 pa and now it is 0.05e5 pa) and the problem disappeares!it takes hell of a time !it is going to take so much time and amount of disk space to save all the design points for later investigation of cavtation accurance amongh them after solution completion.i am totally exusted


All times are GMT -4. The time now is 17:04.