[fanta]

Good Morning,
i am stuck with blockMesh/snappyHexMesh: I manage to mesh my cases with blockMesh, usually a big cube. All faces are "defaultFaces" with no patchtype.
When i run sHM with my inlet/out/wall stl file, all goes fine but my solver does not run because of this:

Selecting turbulence model type laminar
Selecting laminar stress model Stokes
No MRF models present

No finite volume options present

Starting time loop

Selecting finite volume options type scalarSemiImplicitSource
Source: IncrementTime
- selecting all cells
- selected 3652902 cell(s) with volume 0.303072
Time = 1

smoothSolver: Solving for T, Initial residual = 1, Final residual = 0.00840505, No Iterations 13
--------------------------------------------------------------------------
MPI_ABORT was invoked on rank 95 in communicator MPI_COMM_WORLD
with errorcode 1.

NOTE: invoking MPI_ABORT causes Open MPI to kill all MPI processes.
You may or may not see output from other processes, depending on
exactly when Open MPI kills them.
--------------------------------------------------------------------------
[76]
[76]
[76] --> FOAM FATAL ERROR: (openfoam-2406)
[76] Continuity error cannot be removed by adjusting the outflow.
Please check the velocity boundary conditions and/or run potentialFoam to initialise the outflow.
Total flux : 1e-300
Specified mass inflow : 2.69687e-05
Specified mass outflow : 0
Adjustable mass outflow : 0
[76]


Here is the main part of my U file:
boundaryField
{
inlet
{
type flowRateInletVelocity;
massFlowRate $massenStrominkgs;
rhoInlet $dichte_;
}
outlet
{
type zeroGradient;
}
wall
{
type noSlip;
}
defaultFaces
{
type empty;
}
}

Can someone help me how to get rid of the defaultFaces (coming obviously from blockMesh)?

[Yann]

Hello Fanta,

What kind of geometry are you meshing? Is it an internal flow?
Before running your case, have you checked your mesh?

When you don't define any boundary in blockMeshDict, patches are automatically named defaultFaces and get an empty type by default.

However, as far as I remember, snappyHexMesh does not like empty types. So it is very likely to find warnings about this in your snappy log (for instance complaining about 2D/3D dimensions), and possibly a failed mesh.

To avoid undefined faces to get an empty type with blockMesh, you can define your boundary section in blockMeshDict as:

boundary
(
    defaultFaces
    {
        type patch;
        faces ();
    }
);

This will define all faces as patch.

If you are meshing an internal flow entirely defined by your STL file, you should not have any remaining defaultFaces in your mesh if snappy ran successfully.

[fanta]

Hey Yann; first of all: thank you for your help!
Yes, i am running an internal flow, using a inlet.stl, outlet.stl and a wall.stl.
I edited the blockMeshDict as you recommended and checkMesh did not complain anymore. Now my simulation is running and Ansys is no longer needed.

FYI:
We have been using Ansys CFD PrepPost for meshing since 2017 on and now i am switching to blockMesh/sHM. Running in parallel it is really a lot more faster than Ansys + we are saving money if we stop using Ansys.