
[Sponsors] 
August 16, 2015, 00:15 
sonicfoam nozzle case

#1 
New Member
mohammad javad
Join Date: Jul 2015
Posts: 9
Rep Power: 2 
hi
i am try to simulate aerospike nozzle and examine different bc. when i decrease initial p solving diverge. my bc for p dimensions [1 1 2 0 0 0 0]; internalField uniform 500000; boundaryField { gasInlet { // type fixedValue; // value uniform 800000; type totalPressure; p0 uniform 700000; U U; phi phi; rho none; psi none; gamma 1.3; value uniform 364000; // type zeroGradient; } airInlet { // type fixedValue; // value uniform 100000; type zeroGradient; } outlet { type waveTransmissive; field p; phi phi; rho rho; psi thermosi; gamma 1.3; fieldInf 14000; lInf 1; value uniform 14000; // type zeroGradient; } symPlane { type symmetry; } freestreem { type zeroGradient; } spikeWall { type zeroGradient; } frontAndBack { type empty; } } for u dimensions [0 1 1 0 0 0 0]; internalField uniform (100 0 0); boundaryField { gasInlet { // type fixedValue; //value uniform (650 0 0); type pressureInletOutletVelocity; phi phi; rho rho; value uniform (0 0 0); } airInlet { // type fixedValue; // value uniform (10 0 0); type pressureInletVelocity; phi phi; rho rho; value uniform (0 0 0); /* type supersonicFreestream; pInf 380000; TInf 300; UInf (650 0 0); gamma 1.3; value uniform (0 0 0); */ } outlet { type pressureInletOutletVelocity; inletValue uniform (0 0 0); value uniform (0 0 0); } symPlane { type symmetry; } freestreem { type supersonicFreestream; pInf 500000; TInf 300; UInf (400 0 0); gamma 1.3; value uniform (0 0 0); // type slip; } spikeWall { type fixedValue; value uniform (0 0 0); } frontAndBack { type empty; } } for T dimensions [0 0 0 1 0 0 0]; internalField uniform 300; boundaryField { gasInlet { type fixedValue; value uniform 320; } airInlet { type fixedValue; value uniform 300; } outlet { type inletOutlet; inletValue uniform 300; value uniform 300; } symPlane { type symmetry; } freestreem { type inletOutlet; inletValue uniform 300; value uniform 300; } spikeWall { type zeroGradient; } frontAndBack { type empty; } } I want the flow to be induced by the pressure difference between inlet (exit of the nozzle) and the ambient.Screenshot from 20150816 08:41:44.png Screenshot from 20150816 08:42:32.png With thanks for your attention 

August 16, 2015, 08:57 

#2 
New Member
mohammad javad
Join Date: Jul 2015
Posts: 9
Rep Power: 2 
no one comment???????


August 17, 2015, 03:52 

#3 
Senior Member
Matvey Kraposhin
Join Date: Mar 2009
Location: Moscow, Russian Federation
Posts: 326
Rep Power: 10 
Hi, can you show picture with schematic view of your computational domain  where inlet is located, where outlet and so on.


August 17, 2015, 03:59 

#4 
Senior Member
Matvey Kraposhin
Join Date: Mar 2009
Location: Moscow, Russian Federation
Posts: 326
Rep Power: 10 
Can you als share your case directory with 0, constant and system?


August 17, 2015, 05:37 

#6  
Senior Member
Matvey Kraposhin
Join Date: Mar 2009
Location: Moscow, Russian Federation
Posts: 326
Rep Power: 10 
Quote:
information on the link, that you provided do not gives more about your numerical model. Problem can be:  in numeric schemes (fvSchemes, fvSolution)  in physical properties (constant/thermopysicalProperties)  in boundary conditions (0/) The first step, i would recommend is to switch outlet pressure condition to totalPressure. Can you also upload your case here? 

August 17, 2015, 06:26 

#7 
New Member
mohammad javad
Join Date: Jul 2015
Posts: 9
Rep Power: 2 


August 17, 2015, 16:23 

#8 
Senior Member
Matvey Kraposhin
Join Date: Mar 2009
Location: Moscow, Russian Federation
Posts: 326
Rep Power: 10 
Hi,
I would suggest next steps to improve stability  change pressure "outlet" condition to totalPressure Code:
outlet { type totalPressure; p0 uniform 350000; U U; phi phi; rho none; psi none; gamma 1.3; value uniform 350000; } Code:
freestreem { type slip; } Code:
divSchemes { default none; div(phi,U) Gauss upwind; div(phi,e) Gauss upwind; div(phid,p) Gauss upwind; div(phi,K) Gauss upwind; div(phiv,p) Gauss upwind; div(phi,k) Gauss upwind; div(phi,epsilon) Gauss upwind; div((muEff*dev2(T(grad(U))))) Gauss linear; } Code:
"p.*" { solver PBiCG; preconditioner DILU; tolerance 1e08; relTol 0; } "(UeR).*" { $p; } "(kepsilon).*" { $p; } Code:
relaxationFactors { } Code:
PIMPLE { nOuterCorrectors 1; nCorrectors 2; nNonOrthogonalCorrectors 1; } Also, you must check that max Courant number (Co) do reach values 0.5 or higher. Also you can try rhoCentralFoam for your case. Unfortunately, i can't check this case updated with my changes, because polyMesh folder is missing in tgz 

August 17, 2015, 18:17 

#9 
New Member
mohammad javad
Join Date: Jul 2015
Posts: 9
Rep Power: 2 
thank you very much for the your exact answer and Attention.
after apply your suggest,i am decrease the ambient pressure and case Converged. i am try rhoCentralFoam but Unfamiliarity with that setup, case diverged. if i increase the nozzle pressure to supersonic flow, must i change freestreem and outlet BC? polymesh file i have attached here. Thanks for all. 

August 18, 2015, 15:06 

#10 
New Member
mohammad javad
Join Date: Jul 2015
Posts: 9
Rep Power: 2 
hi dear Matvej.
can you check the k,epsilon,alphat,mut files?? thanks a lot. 

August 18, 2015, 16:55 

#11 
New Member
mohammad javad
Join Date: Jul 2015
Posts: 9
Rep Power: 2 
hi matvej
i am decrease the ambient pressure to 14000 and case diverged. so i refinement mesh to 109000 cell but diverged. 

August 19, 2015, 13:27 

#12 
Senior Member
Matvey Kraposhin
Join Date: Mar 2009
Location: Moscow, Russian Federation
Posts: 326
Rep Power: 10 
Hi, mohammad
After inspecting your case i found next issues about computational domain and B.C.: 1) Mesh is too thick in zdirection. Despite the absence of third coordinate (Z) in solution, it is a good practice, to have thickness of cells in Zdirection for 2D simulation in OpenFOAM of order 1/100 of some characteristic length. In your case i would propose to make thickness of mesh 100 or more times smaller then you have now 2) Also, checkMesh tells, that you have some edges, that are not aligned or not perpindicular to empy (Z) direction. This usually means, that mesh is corrupted somewhere. See checkMesh log at the end of my message. 3) For supersonic flows you have to change your boundary conditions at inlet as follow:  if you know velocity and it is supersonic, then you must supply pressure (p), velocity (U) and temperature (T) at inlet  if you know only pressure at inlet, then you must extend your inlet in upwind direction to build convergingdiverging nozzle to resolve subsonicsupersonic flow correctly I hope, this will help you Code:
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // Create time Create polyMesh for time = 0 Time = 0 Mesh stats points: 9208 internal points: 0 faces: 31351 internal faces: 13229 cells: 8916 faces per cell: 5 boundary patches: 7 point zones: 0 face zones: 0 cell zones: 0 Overall number of cells of each type: hexahedra: 0 prisms: 8916 wedges: 0 pyramids: 0 tet wedges: 0 tetrahedra: 0 polyhedra: 0 Checking topology... Boundary definition OK. Cell to face addressing OK. Point usage OK. Upper triangular ordering OK. Face vertices OK. Number of regions: 1 (OK). Checking patch topology for multiply connected surfaces... Patch Faces Points Surface topology frontAndBack 17832 9208 ok (nonclosed singly connected) outlet 17 36 ok (nonclosed singly connected) freestreem 47 96 ok (nonclosed singly connected) spikeWall 86 176 ok (nonclosed singly connected) gasInlet 2 6 ok (nonclosed singly connected) symPlane 87 176 ok (nonclosed singly connected) airInlet 51 104 ok (nonclosed singly connected) Checking geometry... Overall domain bounding box (0.0441409 0 0) (2.07111 0.82878 1) Mesh (nonempty, nonwedge) directions (1 1 0) Mesh (nonempty) directions (1 1 0) ***Number of edges not aligned with or perpendicular to nonempty directions: 7 <<Writing 14 points on nonaligned edges to set nonAlignedEdges Boundary openness (2.96576e17 7.11784e17 1.0531e19) OK. Max cell openness = 2.18691e16 OK. Max aspect ratio = 2.09584 OK. Minimum face area = 1.5752e06. Maximum face area = 0.0662324. Face area magnitudes OK. Min volume = 1.57525e06. Max volume = 0.00138491. Total volume = 1.74312. Cell volumes OK. Mesh nonorthogonality Max: 18.7975 average: 4.39822 Nonorthogonality check OK. Face pyramids OK. Max skewness = 0.402559 OK. Coupled point location match (average 0) OK. Failed 1 mesh checks. End 

August 19, 2015, 22:49 

#13 
New Member
mohammad javad
Join Date: Jul 2015
Posts: 9
Rep Power: 2 
Hi Matvej.
You know what is the reason of diverge case in very low ambient pressure(14000)? فرستاده شده از GLX G5ِ من با Tapatalk 

August 20, 2015, 02:58 

#14 
New Member
MB
Join Date: Sep 2012
Posts: 29
Rep Power: 5 

August 20, 2015, 04:43 

#15 
Senior Member
Matvey Kraposhin
Join Date: Mar 2009
Location: Moscow, Russian Federation
Posts: 326
Rep Power: 10 

August 20, 2015, 12:42 

#16 
Senior Member
Matvey Kraposhin
Join Date: Mar 2009
Location: Moscow, Russian Federation
Posts: 326
Rep Power: 10 
Hi, mohammad
Did you fixed your mesh and B.C.? 

Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
extracting outlet velocity profile from one case to another case's inlet  tonggysun  OpenFOAM  2  September 13, 2013 04:19 
Laval Nozzle sonicFoam inlet and outlet bc  BernhardGrieser  OpenFOAM Running, Solving & CFD  9  August 14, 2010 21:35 
Problem with axisymmetric case using sonicFoam  Madhura  OpenFOAM  0  April 16, 2010 16:59 
Free surface boudary conditions with SOLAVOF  Fan  Main CFD Forum  10  September 9, 2006 12:24 
compressible flow in a counterflow nozzle  d.vamsidhar  FLUENT  0  November 24, 2005 02:45 