CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Software User Forums > OpenFOAM > OpenFOAM Verification & Validation

chtMultiRegionFoam transient case issue

Register Blogs Members List Search Today's Posts Mark Forums Read

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   July 3, 2020, 20:48
Default chtMultiRegionFoam transient case issue
  #1
New Member
 
Join Date: Jun 2020
Posts: 2
Rep Power: 0
Rustralia is on a distinguished road
update--- the time step was too big in the setting. Still not sure how fluent was able to get the right value with the same time step, but Openfoam needs a much smaller (6 magnitudes smaller) time step so that the diffusion number is reasonably small to get accurate results.


All,

I am new to OpenFOAM and currently solving a heat transfer problem with two different materials.

Here is the model setup: I have a quarter of a sphere with a core and a shell. the initial Temperature is uniform everywhere, and the surface of the sphere is losing heat through convection with constant h.

To verify the basic model setup, I set both core and shell to be the same material property, and the Biot number is small enough that the Temperature variation with time should be the same as the results from Lumped Capacitance Method. However, the results from Openfoam case is different from the LCM and Fluent model. I attached a plot to show the difference.



Since I converted the mesh from Fluent, and the Fluent case ran just file, I am guessing this is not a meshing issue. I have checked the material properties many times and they are the same as what I used for LCM and fluent. Any advice would be appreciated!

Here is the boundary condition on the surface of the shell:
Code:
boundaryField
{
    shell_to_core
    {
        type            compressible::turbulentTemperatureCoupledBaffleMixed;
        value           $internalField;
        kappaMethod     solidThermo;
        kappa           kappa;
        Tnbr            T;
    }
    sym1-shell
    {
	type 		symmetry;
    }	
    sym2-shell
    {
        type            symmetry;
    }
    outershell
    {
	type 		externalWallHeatFluxTemperature;
	mode		coefficient;
	kappaMethod	solidThermo;
	kappa		kappa;
	Ta		uniform 293.15;
	h		uniform 100.0;
	value		uniform 773.15;
	kappaName	none;
	QrName		none;
    }	
}
Boundary condition is also pretty straightforward:

Code:
(
    outershell
    {
        type            wall;
        inGroups        1(wall);
        nFaces          788;
        startFace       18592;
    }
    sym1-shell
    {
        type            symmetry;
        inGroups        1(symmetry);
        nFaces          320;
        startFace       19380;
    }
    sym2-shell
    {
        type            symmetry;
        inGroups        1(symmetry);
        nFaces          320;
        startFace       19700;
    }
    shell_to_core
    {
        type            mappedWall;
        inGroups        1(wall);
        nFaces          788;
        startFace       20020;
        sampleMode      nearestPatchFace;
        sampleRegion    core;
        samplePatch     core_to_shell;
    }
)
Maybe the problem is the in the fvSchemes and fvSolution, I tried to change a couple of things but didn't seem to make too much of a difference:

Code:
ddtSchemes
{
    default         Euler;
}

gradSchemes
{
    default         Gauss linear;
}

divSchemes
{
    default         none;
}

laplacianSchemes
{
    default         Gauss linear uncorrected;
}

interpolationSchemes
{
    default         linear;
}

snGradSchemes
{
    default         uncorrected;
}
Code:
solvers
{
    "(h|e)"
    {
        solver           PCG;
        preconditioner   DIC;
        tolerance        0;
        relTol           0.001;
	maxIter		 200;
    }

    "(h|e)Final"
    {
        $h;
	tolerance	0;
        relTol           0.001;
	maxIter		200;
    }
}

PIMPLE
{
    nNonOrthogonalCorrectors 0;
}

relaxationFactors
{
    equations
    {
        ".*" 1;
    }
}

One more piece of info: If I run the model for longer time, all three curves will converge to the same final Temperature.
Attached Images
File Type: png TValidation.png (18.0 KB, 9 views)

Last edited by Rustralia; July 14, 2020 at 16:33.
Rustralia is offline   Reply With Quote

Old   July 4, 2020, 14:22
Default
  #2
New Member
 
Join Date: Jun 2020
Posts: 2
Rep Power: 0
Rustralia is on a distinguished road
Oh and this is check mesh info before it was split into two regions:
Code:
Create time

Create polyMesh for time = 0

Time = 0

Mesh stats
    points:           6435
    faces:            41775
    internal faces:   39569
    cells:            18366
    faces per cell:   4.4290537
    boundary patches: 5
    point zones:      0
    face zones:       3
    cell zones:       2

Overall number of cells of each type:
    hexahedra:     0
    prisms:        7880
    wedges:        0
    pyramids:      0
    tet wedges:    0
    tetrahedra:    10486
    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
    outershell          788      427      ok (non-closed singly connected)
    sym1-shell          320      363      ok (non-closed singly connected)
    sym1-core           392      223      ok (non-closed singly connected)
    sym2-shell          320      363      ok (non-closed singly connected)
    sym2-core           386      220      ok (non-closed singly connected)

Checking geometry...
    Overall domain bounding box (-0.0001 0 0) (0.0001 0.0001 0.0001)
    Mesh has 3 geometric (non-empty/wedge) directions (1 1 1)
    Mesh has 3 solution (non-empty) directions (1 1 1)
    Boundary openness (-1.0818631e-18 -2.9004236e-17 -4.2481159e-16) OK.
    Max cell openness = 2.1197891e-16 OK.
    Max aspect ratio = 4.2659031 OK.
    Minimum face area = 3.420192e-12. Maximum face area = 5.9869127e-11.  Face area magnitudes OK.
    Min volume = 3.3910793e-18. Max volume = 2.8077274e-16.  Total volume = 1.0435124e-12.  Cell volumes OK.
    Mesh non-orthogonality Max: 49.726612 average: 13.776316
    Non-orthogonality check OK.
    Face pyramids OK.
    Max skewness = 0.51786021 OK.
    Coupled point location match (average 0) OK.

Mesh OK.

Let me know if if you need more info to help out! Thanks!
Rustralia is offline   Reply With Quote

Old   July 20, 2020, 03:49
Default
  #3
Super Moderator
 
Tobi's Avatar
 
Tobias Holzmann
Join Date: Oct 2010
Location: Augsburg
Posts: 2,404
Blog Entries: 6
Rep Power: 43
Tobi has a spectacular aura aboutTobi has a spectacular aura aboutTobi has a spectacular aura about
Send a message via ICQ to Tobi Send a message via Skype™ to Tobi
Hi, the first thing that is obvious is the following:



Code:
Mesh non-orthogonality Max: 49.726612 average: 13.776316
You do have non-orthogonality which should be corrected (explicit term). However, you define your numerical schemes to be uncorreced. https://cfd.direct/openfoam/user-gui...20-1490004.5.4

Quote:
Generally the uncorrected and orthogonal schemes are only recommended for meshes with very low non-orthogonality (e.g. maximum 5). The corrected scheme is generally recommended, but for maximum non-orthogonality above 70, limited may be required. At non-orthogonality above 80, convergence is generally hard to achieve.

Furthermore, many people are not aware how the numeric works and how the equations are solved explicit and implicit terms. Are you sure that your energy equation is converged (even the explicit terms) within on time-step?

The statement that FOAM needs a time-step which is much smaller compared to ANSYS is a hint that you do wrong things in the numerical stuff if the meshes are identical.
__________________
Keep foaming,
Tobias Holzmann
Tobi is offline   Reply With Quote

Reply

Tags
chtmultiregionfoam, heat transfer, solid

Thread Tools Search this Thread
Search this Thread:

Advanced Search
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are Off
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Transient Simulation - Fluent remove my case and data lape95 FLUENT 4 April 22, 2020 09:20
Which terms to seach for: transient thermal multi case RichardL ANSYS 1 July 31, 2018 12:04
[OpenFOAM] post-processing chtMultiRegionFoam case in paraview? phsieh2005 ParaView 2 July 15, 2016 15:05
Is Playstation 3 cluster suitable for CFD work hsieh OpenFOAM 9 August 16, 2015 14:53
Fluidisation transient case Vikas Kumar Main CFD Forum 0 April 24, 2003 03:29


All times are GMT -4. The time now is 14:04.