
[Sponsors] 
March 9, 2022, 10:40 
Negative flow inlet

#1 
New Member
Kristian
Join Date: Jan 2022
Posts: 6
Rep Power: 4 
There are several posts about natural convection in this forum, but none of those solves my problem.
I have created a 2D 0.5m high small "scale" and model for a case, with partly heated wall. There is one inlet and outlet. This is a kepsilon model using perfectGas and buoyantSimpleFoam as solver, for air. Boundary conditions, system folder and velocity profiles are attached in this post. if you want to run the case, I have to create a blockMesh, My mesh exeeds the storage limit. The problem I am struggling with is negative flow at inlet (left picture). The U_magnitude is positive, but both U_X and U_Y are negative and U_Z is zero. The outlet flow (right picture) is positive, resulting in a constant loop of the model and after 100k+ iterations, the model crashes. How do i manage to add a positive inlet flow to the model? I have tried different approaches with outletInlet for U, p_rgh and T + many other approaches, without any success . What fixed mye positive outlet flow was setting T_outlet to inletOutlet. pressure is calculated using: p = p_rgh + rho*gh + pRef. p_rgh is pressure without hydrostatic pressure. p_rgh diverges, which is a common problem in this forum. QUICK scheme have been used to discretize the momentum and energy equations, without luck. (Litterature study suggest using QUICK scheme for the mentioned eq's) Any help solving this back flow problem? 

March 9, 2022, 15:26 

#2  
Senior Member
Join Date: Sep 2013
Posts: 353
Rep Power: 20 
your p_rgh boundary
Code:
inlet { type fixedValue; value uniform 0; } outlet { type zeroGradient; } Code:
inlet { type zeroGradient; } outlet { type pressureInletOutletVelocity; inletValue uniform (0 0 0); value uniform (0 0 0); } Quote:
The problem with natural convection is that your flow does not result from a boundary condition, but is generated inside the domain. The problem with that is, that your boundaries are essentially inlet or outlet and you need conditions which can switch based on what is present. For example totalPressure/prghTotalPressure and pressureInletOutletVelocity. This might however not be all that stable especially with high order schemes like quick. The best thing one can do is move the atmosphere far away from the problem and use stable but not all that realistic boundary conditions. For your geometry however this should be solvable. Also are you sure you want to calculate natural convection with steadyState conditions? natural convection is a pretty transient phenomenon. 

March 10, 2022, 14:03 

#3  
Senior Member
Agustín Villa
Join Date: Apr 2013
Location: Alcorcón
Posts: 313
Rep Power: 14 
Quote:
I am working as well in a natural convection flow, where 3 of 4 boundaries are open. I impose known values in one of these patches but there are still 2 "degress of freedom" and it is not so easy to find a wellposed BC in the available ones. If you know how the fluid should act close to the boundaries it could be possible to prepare a custom BC. 

March 11, 2022, 13:31 

#4 
New Member
Kristian
Join Date: Jan 2022
Posts: 6
Rep Power: 4 
Thank you for the reply.
Okey, I will fix the inlets. Any suggestions to solve this inlet? a baginner, and in the other tutorials uses fixed fluxpresssure with fix velocities. I want the solver to determine the inflow by it self. As you say, the model is determined with what is happening inside the domain, and setting fixed values may confuse the model? When I am later validating the large scale model, measured valus will be used, and can be the reserve plan to set fixed inlet and outlet values. I agree with the atmosphere, and it will be in my mind when I put the solver into the large scale/actual case. Yeah, natural convection is transient, but at the moment my computer is not capable to solve PIMPLE case, too slow... For large scale, I have access to a cluster, so pimple will not be a problem then 

March 11, 2022, 14:01 

#5 
Senior Member
Agustín Villa
Join Date: Apr 2013
Location: Alcorcón
Posts: 313
Rep Power: 14 
FixedFluxPressure acts as a zeroGradient BC, therefore any imposed value would be needed.
You could use a PIMPLE simulation (you could coarse the mesh) as a starting point for your steady simulations. If BCs are not posed properly the steady solvers stops and suggests you to use potentialFoam 

March 12, 2022, 00:55 

#6 
Senior Member
Uwe Pilz
Join Date: Feb 2017
Location: Leipzig, Germany
Posts: 744
Rep Power: 15 
You have too much degrees of freedom here.
I recommend using a closed volume with no inlet or outlet. Simply lengthen your wall at the top and the bottom. These added walls have a nonslip boundary, but no heating. You get some kind of circular flow. But if your volume is large enough, the downward flow does not influence your heated side. If you want to study the transient flow / beginning of rising that may be sufficient. If you want to study the stationary case you should add a cooling at the opposite side. So the fluid does not heat to infinity or to the wall temperature (dependung on your b.c.). I think that is a far better model. I used a similar for my calculations of gravity driven convection / dissolving of a component at the boudary.
__________________
Uwe Pilz  Die der Hauptbewegung überlagerte Schwankungsbewegung ist in ihren Einzelheiten so hoffnungslos kompliziert, daß ihre theoretische Berechnung aussichtslos erscheint. (Hermann Schlichting, 1950) 

Tags 
back flow, natural convection, p_rgh devergence 
Thread Tools  Search this Thread 
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
[Other] mesh airfoil NACA0012  anand_30  OpenFOAM Meshing & Mesh Conversion  13  March 7, 2022 17:22 
Issues on the simulation of highspeed compressible flow within turbomachinery  dowlee  OpenFOAM Running, Solving & CFD  11  August 6, 2021 06:40 
Two Mass flow inlet bc convergence problem  nabidinhomessi  Main CFD Forum  5  December 14, 2015 07:11 
Mass flow rate boundary condition with negative values  ashtonJ  CFX  3  November 26, 2014 05:21 
[blockMesh] nonorthogonal faces and incorrect orientation?  nennbs  OpenFOAM Meshing & Mesh Conversion  7  April 17, 2013 05:42 