SIMPLE and SIMPLEC produce different results
 

I've tested a SIMPLEC vs SIMPLE algorithms for my simulation and found that SIMPLEC produced a significantly higher velocities compared to SIMPLE.

The case was the same. The only things that were changed were:
1) consistent yes;
2) no relaxation for pressure; relaxation for velocity 0.9

A screenshot with comparative cross-sections is attached.

From my own experience I could say that result with SIMPLE seems to be correct.
But why SIMPLEC gives a different result ?

The residual plots are attached.
It is a pulsatile flow with pulse period of 0.77 s. I've simulated 5 full periods.

I can upload the case if it is necessary.

Are you sure, that residual values of 0.1 (for pressure) are low enough? Normally they should be below 1E-4.

You could also try smaller time steps.

I think that time step was small enough (dt = 0.0001 s).

What is your Courant number?

Plot for Courant number is attached

Just a question here...are you using a steady solver (simpleFoam) for a transient flow? If so then your time step size has no influence on the solution since there is no time derivative in the simpleFoam solver. Furthermore, your differences in solution are just comparisons of two un-converged flow fields. With that, what solver are you using?

I used pimpleFoam

Your Courant number is huge.

As you can see in the attached file, Courant number is high only for a few cells and doesn't affect the overall solution.

Hello.
Your are wrong. Even one bad cell crashes Your solution. Prepare better mesh to get Max Courant Number below 1.

@Svensen Again, just curious,

• What does checkMesh output look like?
• What is the composition of the mesh in terms of hex, poly, prisms, and tet cells?
• What was used to mesh this domain?

Log files are attached.

Domain was initially meshed by ANSYS, I've just imported the mesh to OpenFOAM by fluent3DMeshToFoam.

if you want to use large courant number such as 100-200 and compare SIMPLE and SIMPLEC time accurate simulations move on from pimpleFoam to transientSimpleFoam - this solver is discussed and attached somewhere in this forum cant remember which thread actually

I think that the actual problem is this set of few high Courant cells. I don't know why they were created by mesher. Maybe it is an OpenFOAM problem, because meshing was done by ANSYS, which is commercial and highly tested software.

If it would be possible to omit these cells then the problem would be solved. However it is not an easy task. According to my experience, If I just manually remove them, then some other cells will have a high Courant...

This is not because fluent is highly tested, but rather because it limits accuracy when faced with bad mesh cells without user intervention. OpenFOAM on the other hand needs the user to step in. Nearly all tutorial settings are for accuracy. Not for bad mesh quality. Your mesh is not bad on average, but as pointed out a single bad cell is enough to lower your convergence rate immensely. The main problem here is the non orthogonality. Now you can either work with limiters and change your schemes, or simply create a better mesh. For this geometry snappyHexMesh should work absolutely fine.

The issue here is the tetrahedra cells. OpenFOAM can use them but you will get poor results from them without additional steps. Since I run away from tetrahedra cells and stick with hex-dominant meshes, from memory you can:

• Convert your mesh to an arbitrary polyhedral mesh with ANSYS (my suggestion) or use polyDualMesh. For the latter, you need to take additional steps to ensure that this will be a good conversion by removing any delaunay violations and also prescribing the correct feature angle to the polyDualMesh utility.
• Use appropriate Laplacian schemes settings and divergence schemes that are for non-orthogonal cells (mentioned by Bloerb). For divergence, you may want to try a scheme called reconCentral

I actually suggest remeshing with a hex dominant mesher and save yourself some time. I used the two above steps during my PhD on really complicated geometries and adopted the ABT (anything by tet) approach was the best option in OpenFOAM. good luck.