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

SIMPLE and SIMPLEC produce different results

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

Like Tree2Likes
  • 1 Post By Svensen
  • 1 Post By chegdan

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   July 12, 2017, 04:24
Default SIMPLE and SIMPLEC produce different results
  #1
Senior Member
 
Join Date: Jan 2015
Posts: 150
Rep Power: 8
Svensen is on a distinguished road
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
File Type: jpg SIMPLE_vs_SIMPLEC.jpg (49.2 KB, 187 views)
File Type: png simplec_continuity.png (15.5 KB, 177 views)
File Type: png simple_continuity.png (14.1 KB, 159 views)
File Type: png simplec_residuals.png (17.3 KB, 167 views)
File Type: png simple_residuals.png (15.9 KB, 141 views)
Svensen is offline   Reply With Quote

Old   July 12, 2017, 17:24
Default
  #2
Senior Member
 
Joachim Herb
Join Date: Sep 2010
Posts: 614
Rep Power: 18
jherb is on a distinguished road
Are you sure, that residual values of 0.1 (for pressure) are low enough? Normally they should be below 1E-4.
jherb is offline   Reply With Quote

Old   July 13, 2017, 12:07
Default
  #3
Member
 
Joshua
Join Date: Dec 2016
Location: St. Louis, Missouri
Posts: 91
Rep Power: 6
Joshua14 is on a distinguished road
You could also try smaller time steps.
Joshua14 is offline   Reply With Quote

Old   July 13, 2017, 12:34
Default
  #4
Senior Member
 
Join Date: Jan 2015
Posts: 150
Rep Power: 8
Svensen is on a distinguished road
I think that time step was small enough (dt = 0.0001 s).
Svensen is offline   Reply With Quote

Old   July 13, 2017, 12:36
Default
  #5
Member
 
Joshua
Join Date: Dec 2016
Location: St. Louis, Missouri
Posts: 91
Rep Power: 6
Joshua14 is on a distinguished road
What is your Courant number?
Joshua14 is offline   Reply With Quote

Old   July 13, 2017, 12:46
Default
  #6
Senior Member
 
Join Date: Jan 2015
Posts: 150
Rep Power: 8
Svensen is on a distinguished road
Plot for Courant number is attached
Attached Images
File Type: png courant.png (12.5 KB, 191 views)
Svensen is offline   Reply With Quote

Old   July 13, 2017, 13:01
Default
  #7
Senior Member
 
chegdan's Avatar
 
Daniel P. Combest
Join Date: Mar 2009
Location: St. Louis, USA
Posts: 621
Rep Power: 26
chegdan will become famous soon enoughchegdan will become famous soon enough
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?
__________________
Dan

Find me on
Twitter @dancombest
LinkedIn
WordPress
chegdan is offline   Reply With Quote

Old   July 13, 2017, 13:02
Default
  #8
Senior Member
 
Join Date: Jan 2015
Posts: 150
Rep Power: 8
Svensen is on a distinguished road
I used pimpleFoam
chegdan likes this.
Svensen is offline   Reply With Quote

Old   July 14, 2017, 01:50
Default
  #9
Senior Member
 
akidess's Avatar
 
Anton Kidess
Join Date: May 2009
Location: Germany
Posts: 1,379
Rep Power: 26
akidess will become famous soon enough
Your Courant number is huge.
__________________
*On twitter @akidTwit
*Spend as much time formulating your questions as you expect people to spend on their answer.
akidess is offline   Reply With Quote

Old   July 14, 2017, 06:30
Default
  #10
Senior Member
 
Join Date: Jan 2015
Posts: 150
Rep Power: 8
Svensen is on a distinguished road
Quote:
Originally Posted by akidess View Post
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
File Type: jpg highCo_cells.jpg (24.6 KB, 141 views)
Svensen is offline   Reply With Quote

Old   July 14, 2017, 06:57
Default
  #11
Senior Member
 
sheaker's Avatar
 
Oskar
Join Date: Nov 2015
Location: Poland
Posts: 185
Rep Power: 7
sheaker is on a distinguished road
Hello.
Your are wrong. Even one bad cell crashes Your solution. Prepare better mesh to get Max Courant Number below 1.
sheaker is offline   Reply With Quote

Old   July 14, 2017, 09:24
Default
  #12
Senior Member
 
chegdan's Avatar
 
Daniel P. Combest
Join Date: Mar 2009
Location: St. Louis, USA
Posts: 621
Rep Power: 26
chegdan will become famous soon enoughchegdan will become famous soon enough
@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?
__________________
Dan

Find me on
Twitter @dancombest
LinkedIn
WordPress
chegdan is offline   Reply With Quote

Old   July 14, 2017, 11:13
Default
  #13
Senior Member
 
Join Date: Jan 2015
Posts: 150
Rep Power: 8
Svensen is on a distinguished road
Log files are attached.

Domain was initially meshed by ANSYS, I've just imported the mesh to OpenFOAM by fluent3DMeshToFoam.
Attached Files
File Type: txt log.checkMesh.txt (3.2 KB, 31 views)
File Type: txt log.checkMesh_allGeometry_allTopology.txt (4.6 KB, 10 views)
Svensen is offline   Reply With Quote

Old   July 16, 2017, 18:13
Default
  #14
Senior Member
 
shereez234's Avatar
 
MS
Join Date: Jan 2014
Location: England
Posts: 316
Blog Entries: 1
Rep Power: 10
shereez234 is on a distinguished road
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
shereez234 is offline   Reply With Quote

Old   July 17, 2017, 11:44
Default
  #15
Senior Member
 
Join Date: Jan 2015
Posts: 150
Rep Power: 8
Svensen is on a distinguished road
Quote:
Originally Posted by shereez234 View Post
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...
Svensen is offline   Reply With Quote

Old   July 18, 2017, 02:17
Default
  #16
Senior Member
 
Join Date: Sep 2013
Posts: 269
Rep Power: 16
Bloerb will become famous soon enough
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.
Bloerb is offline   Reply With Quote

Old   July 18, 2017, 09:21
Default
  #17
Senior Member
 
chegdan's Avatar
 
Daniel P. Combest
Join Date: Mar 2009
Location: St. Louis, USA
Posts: 621
Rep Power: 26
chegdan will become famous soon enoughchegdan will become famous soon enough
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.
__________________
Dan

Find me on
Twitter @dancombest
LinkedIn
WordPress
chegdan is offline   Reply With Quote

Reply

Tags
openfoam-dev, simple, simplec

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
Ask help wiht a SIMPLE Method on compressible flow. universez Main CFD Forum 0 February 8, 2010 10:38
SIMPLEC slewness correction results in divergence jrg FLUENT 2 September 26, 2007 03:25
Making SIMPLE converge faster Fabio Main CFD Forum 4 April 9, 2006 11:35
SIMPLE and SIMPLEC Aditya Main CFD Forum 2 January 12, 2006 19:11
SIMPLEC on Co-located Variables Aditya Main CFD Forum 0 January 6, 2006 04:59


All times are GMT -4. The time now is 14:32.