
[Sponsors] 
March 16, 2010, 04:20 
Overestimated temperature values

#1 
Senior Member

Hello foamers!
I came up with a following problem: during simulation of pouring hot melt into the casting mold I got a temperature values bigger than pouring temperature! My BCs are only fixedValue at the inlet and at the walls of mold (where temperature is lower than at the inlet), and zeroGradient at nozzel boundaries, flat fixed top "freesurface" and at the outlet. Here are the snapshot, where red color indicates overheated cells. From top comes nozzel, flat top interface is with zeroGradient BC, vertical mold is with constant temperature BC: Mold_external.jpg Oveheat1.jpg So you can see from second picture, that difference in temperature is ~30 K over pouring value, which is not appropriated. The problem arises also from other surfaces with zeroGradient BC. For example from outer wall of submerged part of the nozzle: nozzelwall.jpg Where can this problem come from? I don't have any sources of heat, and energy equation contains only energy dissipation parts: DT/Dt = div(alpha_eff grad(T)) My idea was that error comes from gradient schemes due to nonortogonality of the mesh. I use following fvSchemes: Code:
/** C++ **\  =========    \\ / F ield  OpenFOAM: The Open Source CFD Toolbox   \\ / O peration  Version: 1.6   \\ / A nd  Web: www.OpenFOAM.org   \\/ M anipulation   \**/ FoamFile { version 2.0; format ascii; class dictionary; location "system"; object fvSchemes; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // ddtSchemes { default Euler; } gradSchemes { default Gauss linear; } divSchemes { default none; div(phi,U) Gauss upwind; div(phi,T) Gauss upwind; div(phi,k) Gauss upwind; div(phi,epsilon) Gauss upwind; div(phi,R) Gauss upwind; div(R) Gauss linear; div((nuEff*dev(grad(U).T()))) Gauss linear; } laplacianSchemes { default none; laplacian(nuEff,U) Gauss linear corrected; laplacian((1A(U)),p) Gauss linear corrected; laplacian(kappaEff,T) Gauss linear corrected; laplacian(DkEff,k) Gauss linear corrected; laplacian(DepsilonEff,epsilon) Gauss linear corrected; laplacian(DREff,R) Gauss linear corrected; } interpolationSchemes { default linear; } snGradSchemes { default corrected; } fluxRequired { default no; p ; } // ************************************************************************* //
__________________
Best regards, Dr. Alexander VAKHRUSHEV Christian Doppler Laboratory for "Advanced Process Simulation of Solidification and Melting" Simulation and Modelling of Metallurgical Processes Department of Metallurgy University of Leoben http://smmp.unileoben.ac.at 

March 17, 2010, 03:21 

#2 
Senior Member
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,911
Rep Power: 28 
I'd give a try with limiters on the gradients and laplacian.
The mesh is not orthogonal, but it is not skewed either from the detail you showed. Please let us know what you find. Best,
__________________
Alberto Passalacqua GeekoCFD  A free distribution based on openSUSE 64 bit with CFD tools, including OpenFOAM. Available as in both physical and virtual formats (current status: http://albertopassalacqua.com/?p=1541) OpenQBMM  An opensource implementation of quadraturebased moment methods. To obtain more accurate answers, please specify the version of OpenFOAM you are using. Last edited by alberto; March 17, 2010 at 03:21. Reason: remove quote to save space 

March 18, 2010, 04:55 

#3 
Senior Member

Alberto,
I have followed your advice. First please check if I understood you correctly. So, I modified fvSchemes Code:
gradSchemes { default Gauss linear; grad(T) limited Gauss linear; } laplacianSchemes { ....... // !! laplacian(kappaEff,T) Gauss linear corrected; laplacian(kappaEff,T) Gauss linear limited 0.5; ....... } snGradSchemes { // !! default corrected; default limited 0.5; } Over1.gif It represents same geometry with box slice cutted out to see what is going on You can see still overheated cell indicated, T error ~10 K. Waiting for your comments and following advices!
__________________
Best regards, Dr. Alexander VAKHRUSHEV Christian Doppler Laboratory for "Advanced Process Simulation of Solidification and Melting" Simulation and Modelling of Metallurgical Processes Department of Metallurgy University of Leoben http://smmp.unileoben.ac.at 

April 1, 2010, 10:11 

#4 
Senior Member

I have found that not a diffusion, but convectional part produces wrong values.
So I splitted energy equation following way: dT1/dt + div(phi, T1) = 0 (1) dT2/dt = div(alpha_eff * grad(T2)) (2) Below are the results only transport equation (1) at the left picture, and equations (2), which accounts only for diffusion at the right picture respectively. "dT" value means temperature overestimation value (above pouring temperature). Flow is present in both cases, it's direction is shown with arrows in the picture on the right. Convection and diffusion splited.jpg All schemes which I used for such test are without limiting. So what are your suggestions in that case? There is nothing about limiting divergence nonorthogonality corrections in either User or Programming Guides. Here I use for equation (1) following divergence scheme: Code:
div(phi,T1) Gauss linearUpwind Gauss linear;
__________________
Best regards, Dr. Alexander VAKHRUSHEV Christian Doppler Laboratory for "Advanced Process Simulation of Solidification and Melting" Simulation and Modelling of Metallurgical Processes Department of Metallurgy University of Leoben http://smmp.unileoben.ac.at 

April 1, 2010, 10:56 

#5  
Senior Member
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,911
Rep Power: 28 
Quote:
in the first fvSchemes you posted, you were using upwind interpolation, which is limited by definition, since you simply use the upwind cell center value on the face. If you use linearUpwind, you can additionally limit the gradient as shown here ( http://www.cfdonline.com/Forums/ope...earupwind.html ), using Code:
div(phi,T1) Gauss linearUpwind cellLimited Gauss linear 1;
__________________
Alberto Passalacqua GeekoCFD  A free distribution based on openSUSE 64 bit with CFD tools, including OpenFOAM. Available as in both physical and virtual formats (current status: http://albertopassalacqua.com/?p=1541) OpenQBMM  An opensource implementation of quadraturebased moment methods. To obtain more accurate answers, please specify the version of OpenFOAM you are using. 

April 1, 2010, 11:03 

#6 
Senior Member

Alberto!
Thank you very much for such immediate response! I will try your suggestions and report here the results.
__________________
Best regards, Dr. Alexander VAKHRUSHEV Christian Doppler Laboratory for "Advanced Process Simulation of Solidification and Melting" Simulation and Modelling of Metallurgical Processes Department of Metallurgy University of Leoben http://smmp.unileoben.ac.at 

April 1, 2010, 12:25 

#7 
Senior Member
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,911
Rep Power: 28 
Just one additional thought: did you try to remesh the part? What mesher did you use to generate the grid that gives you problems?
Best,
__________________
Alberto Passalacqua GeekoCFD  A free distribution based on openSUSE 64 bit with CFD tools, including OpenFOAM. Available as in both physical and virtual formats (current status: http://albertopassalacqua.com/?p=1541) OpenQBMM  An opensource implementation of quadraturebased moment methods. To obtain more accurate answers, please specify the version of OpenFOAM you are using. 

April 1, 2010, 12:44 

#8  
Senior Member

It was a Gambit, so actually mesh is the third part product, I should not change it...
Btw, I have already tried Quote:
Alberto, what is your opinion regarding reasons, which can cause such problems with a simple scalar transport equation? Just for additional information, here is output of checkMesh: Code:
Mesh stats points: 378191 faces: 1625937 internal faces: 1540645 cells: 642651 boundary patches: 10 point zones: 0 face zones: 0 cell zones: 0 Overall number of cells of each type: hexahedra: 227870 prisms: 138900 wedges: 0 pyramids: 1338 tet wedges: 0 tetrahedra: 274543 polyhedra: 0 Checking topology... Boundary definition 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 SEN_Outer 5072 2916 ok (nonclosed singly connected) Port_Wall 10588 5414 ok (nonclosed singly connected) SEN_Wall 16692 12887 ok (nonclosed singly connected) WW_c 22256 22896 ok (nonclosed singly connected) WW_b 13272 11878 ok (nonclosed singly connected) WW_a 7734 6059 ok (nonclosed singly connected) NarrowWall 2782 3024 ok (nonclosed singly connected) TopWall 2974 2570 ok (nonclosed singly connected) Outlet 3442 2762 ok (nonclosed singly connected) Inlet 480 519 ok (nonclosed singly connected) Checking geometry... Overall domain bounding box (0.686 1.05 0.0816556) (0.686 0.803 0.0820117) Mesh (nonempty, nonwedge) directions (1 1 1) Mesh (nonempty) directions (1 1 1) Boundary openness (1.55627e17 2.36049e16 1.53059e17) OK. Max cell openness = 3.32553e16 OK. Max aspect ratio = 15.485 OK. Minumum face area = 1e06. Maximum face area = 0.000136551. Face area magnitudes OK. Min volume = 8.95047e10. Max volume = 8.44667e07. Total volume = 0.0974925. Cell volumes OK. Mesh nonorthogonality Max: 65.4515 average: 13.9421 Nonorthogonality check OK. Face pyramids OK. Max skewness = 0.959158 OK. Mesh OK. End Code:
Mesh stats points: 378191 faces: 1625937 internal faces: 1540645 cells: 642651 boundary patches: 10 point zones: 0 face zones: 0 cell zones: 0 Overall number of cells of each type: hexahedra: 227870 prisms: 138900 wedges: 0 pyramids: 1338 tet wedges: 0 tetrahedra: 274543 polyhedra: 0 Checking topology... Boundary definition OK. Point usage OK. Upper triangular ordering OK. Topological cell zipup check OK. Face vertices OK. Faceface connectivity OK. <<Writing 3 cells with with single nonboundary face to set twoInternalFacesCells Number of regions: 1 (OK). Checking patch topology for multiply connected surfaces ... Patch Faces Points Surface topology Bounding box SEN_Outer 5072 2916 ok (nonclosed singly connected) (0.157456 0.22 0.0476851) (0.157458 4.17144e15 0.0476866) Port_Wall 10588 5414 ok (nonclosed singly connected) (0.153715 0.22 0.021562) (0.153715 1.06581e17 0.021562) SEN_Wall 16692 12887 ok (nonclosed singly connected) (0.0846087 1.24345e17 0.0599263) (0.0846087 0.803 0.0599263) WW_c 22256 22896 ok (nonclosed singly connected) (0.686 1.05 0.0380647) (0.686 4.09273e15 0.0378848) WW_b 13272 11878 ok (nonclosed singly connected) (0.3 1.05 0.0766829) (0.3 8.1554e15 0.0763984) WW_a 7734 6059 ok (nonclosed singly connected) (0.1 1.05 0.0816556) (0.1 8.8413e15 0.0820117) NarrowWall 2782 3024 ok (nonclosed singly connected) (0.686 1.05 0.027) (0.686 1.36424e15 0.027) TopWall 2974 2570 ok (nonclosed singly connected) (0.686 1.3667e14 0.0816556) (0.686 8.8413e15 0.0820117) Outlet 3442 2762 ok (nonclosed singly connected) (0.686 1.05 0.027) (0.686 1.05 0.027) Inlet 480 519 ok (nonclosed singly connected) (0.0599263 0.803 0.0599263) (0.0599263 0.803 0.0599263) Checking geometry... Overall domain bounding box (0.686 1.05 0.0816556) (0.686 0.803 0.0820117) Mesh (nonempty, nonwedge) directions (1 1 1) Mesh (nonempty) directions (1 1 1) Boundary openness (1.55627e17 2.36049e16 1.53059e17) OK. Max cell openness = 3.32553e16 OK. Max aspect ratio = 15.485 OK. Minumum face area = 1e06. Maximum face area = 0.000136551. Face area magnitudes OK. Min volume = 8.95047e10. Max volume = 8.44667e07. Total volume = 0.0974925. Cell volumes OK. Mesh nonorthogonality Max: 65.4515 average: 13.9421 Nonorthogonality check OK. Face pyramids OK. Max skewness = 0.959158 OK. Min/max edge length = 0.001 0.01938 OK. All angles in faces OK. Face flatness (1 = flat, 0 = butterfly) : average = 0.999998 min = 0.996924 All face flatness OK. Cell determinant (wellposedness) : minimum: 0 average: 2.69124 ***Cells with small determinant found, number of cells: 3 <<Writing 3 underdetermined cells to set underdeterminedCells Failed 1 mesh checks. End
__________________
Best regards, Dr. Alexander VAKHRUSHEV Christian Doppler Laboratory for "Advanced Process Simulation of Solidification and Melting" Simulation and Modelling of Metallurgical Processes Department of Metallurgy University of Leoben http://smmp.unileoben.ac.at 

April 1, 2010, 13:17 

#9  
Senior Member
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,911
Rep Power: 28 
Quote:
Was this mesh working OK in FLUENT if you tried it? Best, Alberto
__________________
Alberto Passalacqua GeekoCFD  A free distribution based on openSUSE 64 bit with CFD tools, including OpenFOAM. Available as in both physical and virtual formats (current status: http://albertopassalacqua.com/?p=1541) OpenQBMM  An opensource implementation of quadraturebased moment methods. To obtain more accurate answers, please specify the version of OpenFOAM you are using. 

April 3, 2010, 13:40 

#10 
Senior Member
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,911
Rep Power: 28 
FYI, similar problems on meshes with tets were described her:
http://www.cfdonline.com/Forums/ope...foamtets.html Best,
__________________
Alberto Passalacqua GeekoCFD  A free distribution based on openSUSE 64 bit with CFD tools, including OpenFOAM. Available as in both physical and virtual formats (current status: http://albertopassalacqua.com/?p=1541) OpenQBMM  An opensource implementation of quadraturebased moment methods. To obtain more accurate answers, please specify the version of OpenFOAM you are using. 

April 27, 2010, 11:38 

#11 
Senior Member

Alberto, thank you for reference!
I will comment there to join our effort.
__________________
Best regards, Dr. Alexander VAKHRUSHEV Christian Doppler Laboratory for "Advanced Process Simulation of Solidification and Melting" Simulation and Modelling of Metallurgical Processes Department of Metallurgy University of Leoben http://smmp.unileoben.ac.at 

May 1, 2010, 04:48 

#12 
Senior Member

A have a following question:
Is there any reason why we solve energy equation in buoyantBoussinesqPisoFoam after momentum predictor and not after pressure and mass flux correction? Have a nice weekend! Best, Alexander
__________________
Best regards, Dr. Alexander VAKHRUSHEV Christian Doppler Laboratory for "Advanced Process Simulation of Solidification and Melting" Simulation and Modelling of Metallurgical Processes Department of Metallurgy University of Leoben http://smmp.unileoben.ac.at 

May 1, 2010, 21:31 

#13  
Senior Member
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,911
Rep Power: 28 
Quote:
Best,
__________________
Alberto Passalacqua GeekoCFD  A free distribution based on openSUSE 64 bit with CFD tools, including OpenFOAM. Available as in both physical and virtual formats (current status: http://albertopassalacqua.com/?p=1541) OpenQBMM  An opensource implementation of quadraturebased moment methods. To obtain more accurate answers, please specify the version of OpenFOAM you are using. 

Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
Calculation of the Governing Equations  Mihail  CFX  7  September 7, 2014 06:27 
DieselFoam Droplet Temperature Issues  OF 1.6  viv05  OpenFOAM  0  February 27, 2010 12:20 
max node values exceed max element values in contour plot  jason_t  FLUENT  0  August 19, 2009 11:32 
strange node values @ solid/fluid interface  help  JB  FLUENT  2  November 1, 2008 13:04 
nodal temperature values  Mcgregor  FLUENT  0  May 5, 2003 08:19 