# SIMPLE and SIMPLEC produce different results

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

July 12, 2017, 04:24
SIMPLE and SIMPLEC produce different results
#1
Senior Member

Join Date: Jan 2015
Posts: 150
Rep Power: 11
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.
Attached Images
 SIMPLE_vs_SIMPLEC.jpg (49.2 KB, 306 views) simplec_continuity.png (15.5 KB, 279 views) simple_continuity.png (14.1 KB, 249 views) simplec_residuals.png (17.3 KB, 260 views) simple_residuals.png (15.9 KB, 210 views)

 July 12, 2017, 17:24 #2 Senior Member   Joachim Herb Join Date: Sep 2010 Posts: 650 Rep Power: 21 Are you sure, that residual values of 0.1 (for pressure) are low enough? Normally they should be below 1E-4.

 July 13, 2017, 12:07 #3 Member   Joshua Join Date: Dec 2016 Location: St. Louis, Missouri Posts: 91 Rep Power: 9 You could also try smaller time steps.

 July 13, 2017, 12:34 #4 Senior Member   Join Date: Jan 2015 Posts: 150 Rep Power: 11 I think that time step was small enough (dt = 0.0001 s).

 July 13, 2017, 12:36 #5 Member   Joshua Join Date: Dec 2016 Location: St. Louis, Missouri Posts: 91 Rep Power: 9 What is your Courant number?

July 13, 2017, 12:46
#6
Senior Member

Join Date: Jan 2015
Posts: 150
Rep Power: 11
Plot for Courant number is attached
Attached Images
 courant.png (12.5 KB, 334 views)

 July 13, 2017, 13:01 #7 Senior Member   Daniel P. Combest Join Date: Mar 2009 Location: St. Louis, USA Posts: 621 Rep Power: 0 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?

 July 13, 2017, 13:02 #8 Senior Member   Join Date: Jan 2015 Posts: 150 Rep Power: 11 I used pimpleFoam chegdan likes this.

 July 14, 2017, 01:50 #9 Senior Member     Anton Kidess Join Date: May 2009 Location: Germany Posts: 1,377 Rep Power: 29 Your Courant number is huge. __________________ *On twitter @akidTwit *Spend as much time formulating your questions as you expect people to spend on their answer.

July 14, 2017, 06:30
#10
Senior Member

Join Date: Jan 2015
Posts: 150
Rep Power: 11
Quote:
 Originally Posted by akidess 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.
Attached Images
 highCo_cells.jpg (24.6 KB, 248 views)

 July 14, 2017, 06:57 #11 Senior Member     Oskar Join Date: Nov 2015 Location: Poland Posts: 184 Rep Power: 10 Hello. Your are wrong. Even one bad cell crashes Your solution. Prepare better mesh to get Max Courant Number below 1.

 July 14, 2017, 09:24 #12 Senior Member   Daniel P. Combest Join Date: Mar 2009 Location: St. Louis, USA Posts: 621 Rep Power: 0 @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?

July 14, 2017, 11:13
#13
Senior Member

Join Date: Jan 2015
Posts: 150
Rep Power: 11
Log files are attached.

Domain was initially meshed by ANSYS, I've just imported the mesh to OpenFOAM by fluent3DMeshToFoam.
Attached Files
 log.checkMesh.txt (3.2 KB, 44 views) log.checkMesh_allGeometry_allTopology.txt (4.6 KB, 13 views)

 July 16, 2017, 18:13 #14 Senior Member     M Sereez Join Date: Jan 2014 Location: England Posts: 352 Blog Entries: 1 Rep Power: 13 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

July 17, 2017, 11:44
#15
Senior Member

Join Date: Jan 2015
Posts: 150
Rep Power: 11
Quote:
 Originally Posted by shereez234 move on from pimpleFoam to transientSimpleFoam
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...

 July 18, 2017, 02:17 #16 Senior Member   Join Date: Sep 2013 Posts: 353 Rep Power: 20 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.

 July 18, 2017, 09:21 #17 Senior Member   Daniel P. Combest Join Date: Mar 2009 Location: St. Louis, USA Posts: 621 Rep Power: 0 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. lourencosm likes this.

 Tags openfoam-dev, simple, simplec