
[Sponsors] 
multiphase flow ，mass and volume fraction imbalance 

LinkBack  Thread Tools  Search this Thread  Display Modes 
July 12, 2012, 06:05 
multiphase flow ，mass and volume fraction imbalance

#1 
New Member
万然
Join Date: Jul 2012
Posts: 15
Rep Power: 11 
Hi,everyone！
I'm puzzled a problem for a long time. Could anyone help me? I try to calculate a multiphase flow model containing oil and air. There are two inlet, air and oil separately, one outlet,and a high speed rotar. The BCs are as follow: 1.oil inlet with a mass flow rate 2.air leak to the cavtiy , so quantity is unknown, i set the boundary as opening with direction and press. 3.outlet is opening with direction and press. 4.the rotar runs at high speed(12000_14000rev/min) the multiphase flow pattern changes with different work conditions. I choose steady model to calculate when the work condition is constant . So,I change multiphase model with different work conditions. when the flow pattern is homogeneous, i choose homogeneous model and set the timescale is antomatic and timescale factor is 2. The outfile shows mass and volume fraction imbalance are about 98%. Then i set timescale factor as 100 for mass and volume fraction equations , mass and volume fraction imbalance are down to 1% Then i set the work conditions differently and choose imhomogeneous and free surface model ,The outfile shows mass and volume fraction imbalance are still about 98%. And i changes the timescale seems useless. ++  PVol  ++ Boundary : AIRIN 4.6508E03 Boundary : OILIN 2.6500E02 Boundary : OUT 5.7588E03  Domain Imbalance : 2.5392E02 Domain Imbalance, in %: 95.8191 % ++  Massoil  ++ Boundary : AIRIN 1.4396E15 Boundary : OILIN 2.6500E02 Boundary : OUT 9.4913E04  Domain Imbalance : 2.5551E02 Domain Imbalance, in %: 96.4184 % The mesh is produced by ICEM, the Jacobian is 0.55 above and angle is 27 above . So i think there is no problems with mesh. Last edited by sope111; July 12, 2012 at 22:55. 

July 12, 2012, 08:15 

#2 
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,042
Rep Power: 134 
Sounds like an FAQ: http://www.cfdonline.com/Wiki/Ansys...gence_criteria


July 12, 2012, 08:33 

#3  
New Member
万然
Join Date: Jul 2012
Posts: 15
Rep Power: 11 
Quote:
Hi ，ghorrocks. I'v confused by this problems for a months,and have tried many times. But the imbalance can achieve the target only for homogeneous. Could you give me some advice ? Thanks a lot. 

July 12, 2012, 16:19 

#4 
Senior Member
OJ
Join Date: Apr 2012
Location: United Kindom
Posts: 473
Rep Power: 18 
I would recommend first, if you are not already doing it, to monitor the imbalances along with the residuals when the run is in progress.
It has been my experience that with multiphase, you have to be a real gentleman. I had similar problems, when I used physical timescale though I used a fraction of residence time (Going for higher values resulted in divergence). Then I switched to Auto timescale with factor of (factor=1) with conservative option. Yet, my imbalances kept oscillating. I tried factor of 0.1 and 0.01 and surprisingly, the balances started reducing to much bearable extent. Also, to get a usable results (not perfect), you can also enforce the steady state by using first order discretization scheme, as it will diffuse the turbulent effects to some extent. 

July 12, 2012, 22:49 

#5  
New Member
万然
Join Date: Jul 2012
Posts: 15
Rep Power: 11 
Quote:
Thanks for your reply . This problem bored me for one month . First ,i've try to moniter the imbalances along with the residuals ,but the mass and volume imbalances are always oscillate around 90%. I even calculate it using transient . At first , the imbalance is up to 1, but it reach to 1% after some timesteps. But transient simulation must employ a steady result as initial valve. However ,I didn't get a convergence value, so i used this unconvergence value. Now ,I wonder whether the transient results are usable( unconvergence value as initial value,but the imbalance and residual seems right)? 

July 13, 2012, 08:44 

#6 
Senior Member
OJ
Join Date: Apr 2012
Location: United Kindom
Posts: 473
Rep Power: 18 
If I am right, in the event where Steady State solution is not at all possible, it may be beneficial to use first order upwind (for stability owing to numerical diffusion) to get some sensible solution with SS and initialize a transient solution with it using High resolution. Though, more resourceful CFD guys here may have better suggestions.
In transient solution, if you make sure that the convergence is obtained for every time step by choosing appropriate timestep (using adaptive timestepping/ timestep sensetivity); the time averaged results can be fairly representative of physics you wish to see. 

July 13, 2012, 23:12 

#7  
New Member
万然
Join Date: Jul 2012
Posts: 15
Rep Power: 11 
Quote:
Hi，oj.bulmer. Thanks for your attention. But i still don't know whether the result is usable with the unconvergence result as initial value.
I'm not sure whther the unconvergence result is credible. And another question , as i mentioned above ,the rotar speed is 12000 rev/min , so the timestep must be set to 10E4(1/w). But the initial value is unconvergence, so i must set much time（i set the value as 16s） to get a usable value . However ,the amount of computation is heavy. Besides, i don't concern about the transient process, so i still want to get a steady value as soon as possible. I reduce the timescale factor to 0.1 and 0.01 with automatic timescale, but the imbalance stay in the same level(90%) 。 So , what can i do for steady simulation?? Thanks. 

July 14, 2012, 05:29 

#8 
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,042
Rep Power: 134 
If all you care about is the final steady state solution (or final pseudosteady if transient and it is flapping about) then a nonconverged initial condition will not matter. As long as it is close enough that the solver converges OK in the transient run, that is the main issue.
There is an extensive discussion on setting time steps int he CFX documentation. For tricky steady state simulations you want to start with a small time step to get it going, but once it is starting to converge OK then you increase the time step size. You can increase it massively if it is converging well). 

July 14, 2012, 06:00 

#9  
New Member
万然
Join Date: Jul 2012
Posts: 15
Rep Power: 11 
Quote:
Dear ghorrocks, Thanks for your help . Another question, multiphase model are homogeneous and imhomogeneous, i want to know what's the relationship between vof in many textbooks and FLUENT? 

July 14, 2012, 06:05 

#10 
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,042
Rep Power: 134 
CFX has a lot more multiphase options than homogeneous and inhomogeneous. That merely refers to whether different phases share a variable field or not.
I do not understand your question to VOF and textbooks and Fluent. 

July 14, 2012, 10:36 

#11  
New Member
万然
Join Date: Jul 2012
Posts: 15
Rep Power: 11 
Quote:
There are two main multiphase phase model:homogeneous and inhomogeneous(free surface,mixture,particle). But Vof appears in many papers and textbooks to track the interface of different phase. I don't know the way to track the interface in cfx, by solve the volume fraction equtions?? Thanks 

July 15, 2012, 08:20 

#12 
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,042
Rep Power: 134 
There are a few methods to track free surfaces and VOF is one of them. CFX does not actually implement VOF as it is usually defined, CFX uses a volume fraction equation with an advection scheme designed to keep the interface sharp.


September 2, 2018, 11:49 

#13 
New Member
saima
Join Date: Jan 2017
Posts: 10
Rep Power: 7 
i am stuck with a problem of multiphase flow cavitation in nozzel injector with diesel liquid and vapors and presure inlet 40 MPa and outlet 10 MPa boundary conditions but mass flow rate at the outlet is not as required, i tried to change mesh but all in vain also i get warning about reverse flow i want to know how to implement turbulent vicosity in k epsilon model


September 2, 2018, 18:55 

#14 
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,042
Rep Power: 134 
The ke turbulence model already implements a turbulent viscosity. Or do you want to modify the ke turbulence model? If so, why?
Before you change the turbulence model, have you done all the other checks required to know your simulation is accurate? FAQ: https://www.cfdonline.com/Wiki/Ansy..._inaccurate.3F
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum. 

September 3, 2018, 00:02 

#15  
New Member
saima
Join Date: Jan 2017
Posts: 10
Rep Power: 7 
Quote:


September 3, 2018, 00:05 

#16 
New Member
saima
Join Date: Jan 2017
Posts: 10
Rep Power: 7 
also help me in determing supersonic initial gauge pressure in pressure inlet boundary condition i dont know how to fix it because i think my simulation is effected by this quantity


September 3, 2018, 00:10 

#17 
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,042
Rep Power: 134 
If you are considering changing turbulence models you really should know what the models which are already there have in them. The ke turbulence model works by estimating the turbulent viscosity and adding that to the molecular viscosity in the momentum equation. You can't have a ke turbulence model without the turbulent viscosity.
Inlet condition  please read the documentation on recommended boundary conditions. That covers how to set boundary conditions up.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum. 

Thread Tools  Search this Thread 
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
how to set periodic boundary conditions  Ganesh  FLUENT  15  November 18, 2020 06:09 
mass flow in is not equal to mass flow out  saii  CFX  12  March 19, 2018 05:21 
On the damBreak4phaseFine cases  paean  OpenFOAM Running, Solving & CFD  0  November 14, 2008 21:14 
fluent add additional zones for the mesh file  SSL  FLUENT  2  January 26, 2008 11:55 
[blockMesh] Axisymmetrical mesh  Rasmus Gjesing (Gjesing)  OpenFOAM Meshing & Mesh Conversion  10  April 2, 2007 14:00 