
[Sponsors] 
March 22, 2006, 19:32 
Hello friends
I have been u

#1 
Senior Member
kumar
Join Date: Mar 2009
Posts: 112
Rep Power: 17 
Hello friends
I have been using rasInterFoam to study wave making of hydrofoils in a channel. the problem i am experiancing is that although i have defined an outlet the fluid seems to be flowing back into the computational domain . let me explain this in detail. figure 1 shows the boundary conditions i have imposed The boundary conditions for the atmosphere are exactly same as that of damBreak case in rasInterFoam tutorial. The boundaries for hydrofoil is simple ( basically a noslip wall) figure 2, 3 , 4 & 5 shows the results after only 1000 time steps . As you can see there seems to be a serious error at the outlet. The velocity seems to have significantly slowed down and the flow seems to change direction and flow back into the domain ( see for example figure 5). i wonder what is happening to the mass conservation equations? Could anyone please comment on these results Thanks in advance kumar 

March 22, 2006, 20:05 
Can't see the images  could y

#2 
Senior Member
Hrvoje Jasak
Join Date: Mar 2009
Location: London, England
Posts: 1,905
Rep Power: 33 
Can't see the images  could you please try and upload them again?
Thanks, Hrv
__________________
Hrvoje Jasak Providing commercial FOAM/OpenFOAM and CFD Consulting: http://wikki.co.uk 

March 22, 2006, 20:12 
Sorry friends
my images are

#3 
Senior Member
kumar
Join Date: Mar 2009
Posts: 112
Rep Power: 17 
Sorry friends
my images are too big . so could not upload. but let me explain with 2 figures. figure 1 shows gamma. you can also notice the inlet . there are 2 patches for the inlet so that gamma is 0 in the top and 1 in the bottom. U is specified and equals 0.8 in top & bottom patches . pd has zero gradient. there are also small values for k & epsilon . The top boundary is atmosphere and the boundary conditions are same as in the tutorial of rasinterFoam. The outlet is specified as two outlet patches with zero gradient for most quantities ( including U ). But gamma is 1 for the bottom patch of outlet and 0 for top patch of outlet. pd is set to zero as shown below ( in file /0/pd) patch atmosphere { type totalPressure; p0 uniform 0; value uniform 0; } the hydrofoil is a noslip boundary and bottom of channel is symmetryPlane. figure 2 shows the velocity field. you can see that the flow is decelerating and turning back into the computational domain . something terribly wrong is happening at the outlet all comments welcome thanks in advance kumar 

March 22, 2006, 20:16 
Dear Hrv
I would love to he

#4 
Senior Member
kumar
Join Date: Mar 2009
Posts: 112
Rep Power: 17 
Dear Hrv
I would love to hear your comments . i have just uploaded the images regards kumar 

March 22, 2006, 20:42 
You need to change the outlet

#5 
Senior Member
Hrvoje Jasak
Join Date: Mar 2009
Location: London, England
Posts: 1,905
Rep Power: 33 
You need to change the outlet boundary condition. Definitely not totalPressure on pd  use either fixedValue zero or zeroGradient (my bet is on zeroGradient, but this kind of thing is worth trying out). On U, use zeroGradient and on gamma do inletOutlet, using some sensible distribution for the refValue.
Your problem is definitely caused by the pressure b.c. Good luck, Hrv
__________________
Hrvoje Jasak Providing commercial FOAM/OpenFOAM and CFD Consulting: http://wikki.co.uk 

March 22, 2006, 21:42 
Dear Hrv
thanks a lot for y

#6 
Senior Member
kumar
Join Date: Mar 2009
Posts: 112
Rep Power: 17 
Dear Hrv
thanks a lot for your comments. now that i know there is a problem with the pressure.b.c i am going to try out your suggestions. i will let you know once i fix the problem. thanks a lot once again regards kumar 

May 23, 2006, 18:07 
Hello Dear Friends
The figu

#7 
Senior Member
kumar
Join Date: Mar 2009
Posts: 112
Rep Power: 17 
Hello Dear Friends
The figures show waves generated by a hydrofoil with rasInterFoam + nuTilda turb.model. The Boundary Conditions are like in the prevoius posts , as recommended by HRV. i got good results with k epsilon model . But k epsilon model has problems in the low Re range ( the Cp distribution has problems which in turn is reflected in the free surface deflections) . so i switched over to spallart allmaras model and my results are blowing up ! The free surface profile , velocity magnitude and nuTilda ( just before the solution blows up) are shown in the 3 figures. What seems to be happening is that the nuTilda gets very large near the atmosphere and the solution blows up. Please also note the patches of zero velocity near the atmosphere. Note the hydrofoil is at the bottom left corner. The top wall is modeled as the atmosphere with U as ( 0 0 0)  similar to the damBreak case . or should this be (0.8 0 0) ? where 0.8 is the inlet velocity /////////////////////////////////////////// The important BC's for nuTilda are InternalField = 5.7*10^6 ; 1. atmosphere type inletOutlet; inletValue uniform 5.7e06; value uniform 5.7e06; 2. Both the inlets ( one for air and one for water have fixedValue nuTildas of 5.7e06 ) ////////////////////////////////////////////// The nuTilda value that i have specified are different from those given in the rasInterFoam tutorial . I found that with those ( the tutorial case )there was severe fluctuations of the free surface profiles  because of concentrations of nuTilda near the free surface. Also the nuTildas i have specified above resemble more closely the 'k' boundary condition. All comments are welcome. Thanks a lot Kumar 

March 9, 2007, 16:22 
Hi, Dear all,
Can anybody tel

#8 
New Member
JZ
Join Date: Mar 2009
Location: PBC, Florida, USA
Posts: 14
Rep Power: 17 
Hi, Dear all,
Can anybody tell me if it is possible to use pressure inlet boundary ( without giving velocities) in interFoam solver. I tested this kind of boundary in simpleFoam, it worked. When I tried to use it in interFoam Solver, if gamma=0, it worked; but when gamma=1, it would brokenup. What I intend to use this kind of boundary is to simulate constant head of water head passing through a hump in a open channel, and study the flow passing capacities. Thus it seems I need gamma=1? Thanks in advance! Jack 

March 24, 2008, 18:38 
I am trying to solve a back st

#9 
New Member
Onur Dundar
Join Date: Mar 2009
Location: Davis, CA, US
Posts: 7
Rep Power: 17 
I am trying to solve a back step in rasinterfoam with k epsilon turbulence model. I added boundary
conditions in FoamX but when I run the rasInterFoam it gives error about boundary conditions. I run after making the given correction. The result is this #0 Foam::error::printStack(Foam:stream&) in "/home/dundar/OpenFOAM/OpenFOAM1.4.1/lib/linuxGccDPOpt/libOpenFOAM.so" I can not find a true boundary conditions. fvSchemes and FvSolution is the same with damBreak Thanks for your concern Onur The boundary conditions are inleta atmosphere inletw inlet outlet atmospehre lowerwall wall ############################################ U boundaryField { inleta { type pressureInletOutletVelocity; phi phi; value uniform (0.4289 0 0); } inletw { type fixedValue; value uniform (0.4289 0 0); } outlet { type pressureInletOutletVelocity; phi phi; value uniform (0 0 0); } lowerWall { type fixedValue; value uniform (0 0 0); } atmosphere { type pressureInletOutletVelocity; phi phi; value nonuniform List<vector> ############################################# pd boundaryField { inleta { type totalPressure; p0 uniform 0; U U; phi phi; rho none; psi none; gamma 1; value uniform 0; } inletw { type zeroGradient; } outlet { type totalPressure; p0 uniform 0; U U; phi phi; rho none; psi none; gamma 1; value uniform 0; } lowerWall { type zeroGradient; } atmosphere { type totalPressure; p0 uniform 0; U U; phi phi; rho none; psi none; gamma 1; value uniform 0; } ############################################## k boundaryField { inleta { type inletOutlet; inletValue uniform 0; value uniform 0; } inletw { type fixedValue; value uniform 0.00184; } outlet { type inletOutlet; inletValue uniform 0; value uniform 0; } lowerWall { type zeroGradient; } atmosphere { type inletOutlet; inletValue uniform 0; value uniform 0; } ############################################## gamma boundaryField { inleta { type inletOutlet; inletValue uniform 0; value uniform 0; } inletw { type fixedValue; value uniform 1; } outlet { type inletOutlet; inletValue uniform 0; value uniform 0; } lowerWall { type zeroGradient; } atmosphere { type inletOutlet; inletValue uniform 0; value uniform 0; } ################################################ R boundaryField { inleta { type inletOutlet; inletValue uniform (0 0 0 0 0 0 0 0 0); value uniform (0 0 0 0 0 0 0 0 0); } inletw { type fixedValue; value uniform (0 0 0 0 0 0 0 0 0); } outlet { type inletOutlet; inletValue uniform (0 0 0 0 0 0 0 0 0); value uniform (0 0 0 0 0 0 0 0 0); } lowerWall { type zeroGradient; } atmosphere { type inletOutlet; inletValue uniform (0 0 0 0 0 0 0 0 0); value uniform (0 0 0 0 0 0 0 0 0); } ################################################# Epsilon boundaryField { inleta { type inletOutlet; inletValue uniform 0; value uniform 0; } inletw { type fixedValue; value uniform 0; } outlet { type inletOutlet; inletValue uniform 0; value uniform 0; } lowerWall { type zeroGradient; } atmosphere { type inletOutlet; inletValue uniform 0; value uniform 0; } ################################################# nutilda boundaryField { inleta { type inletOutlet; inletValue uniform 0; value uniform 0; } inletw { type fixedValue; value uniform 0; } outlet { type inletOutlet; inletValue uniform 0; value uniform 0; } lowerWall { type fixedValue; value uniform 0; } atmosphere { type inletOutlet; inletValue uniform 0; value uniform 0; } fvSchemes and FvSolution is the same with damBreak Thanks for your concern Onur 

Thread Tools  Search this Thread 
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
Newton Raphson  strange results  Bren  Main CFD Forum  5  February 11, 2009 10:47 
[blockMesh] Strange Block Mesh results  ivan_cozza  OpenFOAM Meshing & Mesh Conversion  1  December 4, 2008 08:24 
Slip boundary condition giving strange results  hemph  OpenFOAM Running, Solving & CFD  3  January 18, 2007 05:15 
UDS transport: strange results  Ale  FLUENT  1  November 6, 2003 06:28 
Strange results !  Dimitri  FLUENT  1  August 8, 2002 11:07 