[massive_turbulence]

I linked all the project files, just use pimpleFoam to run it to see what I noticed. Basically I have no idea why the deltaT is increasing rapidly when it is supposed to only change by .0005. I'm not sure about the Courant number and timesteps so that might be it.

This project is a hack made from looking over the TJunction tutorial (in order to make sense out of it). I used Salome to make a mesh (could the mesh not be fine enough?). I included the hdf and step file from that along with the final unv file before creating the boundary files with the ideasUnvtoFoam command.

I then looked over the U,p,nut,k,nuTilda files in the TJunction to properly setup the new boundary files.

The thing I also noticed in paraFoam was that the glyph setting for lines never had a pressure more than 10 (always red). But the simulation also does not generate a 1000 data sets.

[massive_turbulence]

I think this controlDict file might solve the system, anyone with suggestions let me know if you think of something. I changed the maxCo and timeStep properties,

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  2.1.x                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    location    "system";
    object      controlDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

application     pimpleFoam;

startFrom       startTime;

startTime       0;

stopAt          endTime;

endTime         .05;

deltaT          .000001;

writeControl adjustableRunTime;

writeInterval   .001;

purgeWrite      0;

writeFormat     ascii;

writePrecision  6;

writeCompression uncompressed;

timeFormat      general;

timePrecision   6;

runTimeModifiable true;

adjustTimeStep  yes;

maxCo           .5;

functions
{
    probes
    {
        // Where to load it from
        functionObjectLibs ( "libsampling.so" );

        type            probes;

        // Name of the directory for probe data
        name            probes;

        // Write at same frequency as fields
        outputControl   outputTime;
        outputInterval  1;

        // Fields to be probed
        fields
        (
            p U
        );

        probeLocations
        (
            ( 1e-06 0 0.01 )        // at inlet
            ( 0.21 -0.20999 0.01 )  // at outlet1
            ( 0.21 0.20999 0.01 )   // at outlet2
            ( 0.21 0 0.01 )         // at central block
        );
    }
}

// ************************************************************************* //

[msuaeronautics]

Might you explain what you mean when you say deltaT is only supposed to change by 0.0005 or so?

Using pimpleFoam means you assume unsteady flow, so there will be fluctuations in your flow velocity at certain points which, as I'm sure you know, will vary your convective CFL number. Can you show an output file?

[massive_turbulence]

Originally Posted by msuaeronautics

Might you explain what you mean when you say deltaT is only supposed to change by 0.0005 or so?

Using pimpleFoam means you assume unsteady flow, so there will be fluctuations in your flow velocity at certain points which, as I'm sure you know, will vary your convective CFL number. Can you show an output file?

My deltaT for the following output was supposed to run with .0005 but you'll see it goes a lot higher like .2.

Yes, unsteady meaning variables change with time (AFAIK pressure, temp) and no I had no idea it would vary the convective CFL, here's the output for the 0.0005 case (not using the controlDict in my second post, that one actually completes).

The output was super long, here's the pastebin link for it.

[msuaeronautics]

Well, I see its trying hard to reach the max CFL you set. Since it's using large values of deltaT, that means that your cell sizes are probably very large. I would re-mesh with a grid with more reasonable cell sizes, but then again I am not sure what your current mesh looks like.

[massive_turbulence]

Originally Posted by msuaeronautics

Well, I see its trying hard to reach the max CFL you set. Since it's using large values of deltaT, that means that your cell sizes are probably very large. I would re-mesh with a grid with more reasonable cell sizes, but then again I am not sure what your current mesh looks like.

You can download the entire project and run it with pimpleFoam from the link mentioned in the post starting this thread. It's the second word `linked`.

I included the hdf files from Salome and the Unv for openFoam. I already ran ideasUnvtoFoam so the constant directory has the mesh setup.

[msuaeronautics]

Originally Posted by massive_turbulence

You can download the entire project and run it with pimpleFoam from the link mentioned in the post starting this thread. It's the second word `linked`.

I included the hdf files from Salome and the Unv for openFoam. I already ran ideasUnvtoFoam so the constant directory has the mesh setup.

I ran checkMesh and now believe my original hypothesis is true.

Mesh stats
points: 1261
faces: 11802
internal faces: 10754
cells: 5639
boundary patches: 3
point zones: 0
face zones: 0
cell zones: 0

Overall number of cells of each type:
hexahedra: 0
prisms: 0
wedges: 0
pyramids: 0
tet wedges: 0
tetrahedra: 5639
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
wall 1022 520 ok (non-closed singly connected)
inlet 13 12 ok (non-closed singly connected)
outlet 13 12 ok (non-closed singly connected)

Checking geometry...
Overall domain bounding box (0 0 -100) (200 200 300)
Mesh (non-empty, non-wedge) directions (1 1 1)
Mesh (non-empty) directions (1 1 1)
Boundary openness (6.22725e-17 -3.43572e-18 -6.15209e-17) OK.
Max cell openness = 1.97424e-16 OK.
Max aspect ratio = 6.38633 OK.
Minumum face area = 40.9666. Maximum face area = 933.805. Face area magnitudes OK.
Min volume = 123.711. Max volume = 9538.31. Total volume = 8.23502e+06. Cell volumes OK.
Mesh non-orthogonality Max: 47.7293 average: 15.357
Non-orthogonality check OK.
Face pyramids OK.
Max skewness = 0.490081 OK.

Mesh OK.

Your domain bounding box is (0 0 -100) (200 200 300), but your mesh resolution is only 5639 cells. In other words, your cell sizes are quite large and you have an extremely coarse mesh. CFL condition is, most simply, u*dt/dx. So, the solver is trying to apply a large deltaT to achieve the CFL you set (and, in other words, overcome the large dx in the denominator).

[massive_turbulence]

Originally Posted by msuaeronautics

I ran checkMesh and now believe my original hypothesis is true.



Your domain bounding box is (0 0 -100) (200 200 300), but your mesh resolution is only 5639 cells. In other words, your cell sizes are quite large and you have an extremely coarse mesh. CFL condition is, most simply, u*dt/dx. So, the solver is trying to apply a large deltaT to achieve the CFL you set (and, in other words, overcome the large dx in the denominator).

By Looking at the bounding box coordinates I'm guessing the dimensions are (200,200,400) so that would be 200x200x400 = 16 million which is mega compared to 5639.

Around what range should I be though, around 16 million exactly or can I be around 1 million and still get a good simulation?

[msuaeronautics]

Originally Posted by massive_turbulence

By Looking at the bounding box coordinates I'm guessing the dimensions are (200,200,400) so that would be 200x200x400 = 16 million which is mega compared to 5639.

Around what range should I be though, around 16 million exactly or can I be around 1 million and still get a good simulation?

I would just scale your domain down and increase the cell resolution. I didn't look at your mesh as I didn't have the time, but tomorrow I will examine and give suggestions.