
[Sponsors] 
Unable to reach monotonic convergence with mesh refinement 

LinkBack  Thread Tools  Search this Thread  Display Modes 
May 13, 2021, 19:43 
Unable to reach monotonic convergence with mesh refinement

#1 
New Member
Parth
Join Date: May 2019
Posts: 11
Rep Power: 7 
Hi,
I'm simulating a CHT sinusoidal oscillatory flow on CFX using adaptive time stepping (with a moderate initial timestep guess, wide values of min and max timesteps, 25 target loops range and 110 minmax coeff loops) for 5 different structured mesh sizes between 1700k cells and 91k cells. Results are run over sufficient simulation times enough to achieve the transient periodicity nature. Courant number is max upto 3. Normalized imbalances are at 0% for flow var and ~0.1% for energy. For both the fluid and HT variables I observe an overlapping trend of results with a very minor difference of ~0.05% only between 5 grid sizes. Since this shouldn't be the expectation and the monotonic decrease or increase between the values is clearly not noticed. Appears like an oscillatory convergence nature? Request you assist me with any recommendations to further achieve reliability of results for mesh independence. I can provide any necessary snapshots from simulation. Max momentum and energy residual plot is attached. Many thanks. 

May 14, 2021, 05:53 

#2 
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,830
Rep Power: 144 
I do not quite understand what you are asking. Are you saying that the 5 mesh sizes you tested are all within 0.05%? If so, then that suggests your meshes are adequately fine and the coarsest mesh is OK to use.
Don't forget that doing a sensitivity analysis on convergence criteria is often a good idea as well. Rerun the coarse mesh case with the convergence criteria tightened by a factor of 10 and see if that changes results. If no change in results then your results are good, if you get a change you will need to tighten the convergence criteria.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum. 

May 14, 2021, 08:16 

#3 
New Member
Parth
Join Date: May 2019
Posts: 11
Rep Power: 7 
Thanks Glenn for your prompt and precise answer, a few queries still.
As per your comment yes from results it appears my mesh is adequately fine even with a coarse grid of 91k cells. But I suspect if that's a valid case to correctly represent the physics of a simple laminar CHT, given I have a rectangular duct of (10 x 14 x 350)mm long dimensions. What do you think? Sure, I have considered the convergence sensitivity analysis to carry on further. Currently convergence criteria is set to 1e5 target RMS. But in regard to the mesh refinement study can you provide me the right approach to execute one, given this underlying issue between distinct grid sizes or is this nature acceptable to be reported in such a case? (zoomed image of overlapping Pressure variable values attached below for 6 grid sizes) Thanks again. 

May 14, 2021, 08:36 

#4 
Senior Member
Join Date: Jun 2009
Posts: 1,862
Rep Power: 33 
Since you are doing a timeperiodic simulation, your monitor points should show some specific/expected frequencies.
You can create a polar plot in the ANSYS CFX Solver Manager of the monitor point of interest using the expected period of the signal. If the plot goes over itself without any distortion between periods your solution has reached a periodic state.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum. 

May 14, 2021, 09:24 

#5  
New Member
Parth
Join Date: May 2019
Posts: 11
Rep Power: 7 
Quote:
However, my query still remains on performing a mesh independence test for my model. Can you recommend on it kindly (Issues described in posts above)? Thanks. 

May 14, 2021, 09:55 

#6 
Senior Member
Join Date: Jun 2009
Posts: 1,862
Rep Power: 33 
Have you done the time step independence study as well?
If you want to model an accurate oscillatory signal you need an appropriate timestep. The Courant number is (in my opinion) irrelevant for acuraccy purposes unless you write the truncation error as a function of Courant no. Accuracy is a function of truncation errors (spatial and transient), and it can only be controlled by the proper sizing of the timestep and spatial mesh until the solution is no longer dependent on the chosen values. Looking at your convergence plots, it seems you are either running out of coefficient loops or have a high residual target for energy. It seems you are aiming at 10^4, and not 10^5. Hope the above helps
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum. 

May 14, 2021, 10:38 

#7  
New Member
Parth
Join Date: May 2019
Posts: 11
Rep Power: 7 
Quote:
Further, yes I'm encountering some strange jumps and unusual skewness in the thermal parameters, perhaps I'll try with a tighter convergence criteria overall 1e4 perhaps? Coefficient loops between 110 should be still fine? Also would you suggest to rerun those 5 mesh sizes with different timestep setup for each? The zoomed plot I've added is with same adaptive timestep settings for all of them. Thanks for helping out. 

May 14, 2021, 10:51 

#8 
Senior Member
Join Date: Jun 2009
Posts: 1,862
Rep Power: 33 
Apologies I missed the adaptive timestepping initial comment.
I have not used adaptive timestepping myself often to know if it converges to repeatable steps periodically, i.e. every period of the solution uses EXACTLY the same steps as the previous period. If it does not, the nonperiodic integration may introduce a numerical behavior that does not go away easily. For example, for a sinusoidal boundary condition, it could see a different maximum/minimum amplitude between periods which translates into a different wave propagation, i.e. delta BC that is not physical
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum. 

Tags 
cfd  post, cfx, mesh and grid, mesh refinement study, result comparision 
Thread Tools  Search this Thread 
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
decomposePar problem: Cell 0contains face labels out of range  vaina74  OpenFOAM PreProcessing  37  July 20, 2020 05:38 
[snappyHexMesh] Number of cells in mesh don't match with size of cellLevel  colinB  OpenFOAM Meshing & Mesh Conversion  14  December 12, 2018 08:07 
[snappyHexMesh] Disturbance in the mesh after the addition of layers  Dorian1504  OpenFOAM Meshing & Mesh Conversion  0  June 13, 2017 02:27 
Force can not converge  colopolo  CFX  13  October 4, 2011 22:03 
Convergence moving mesh  lr103476  OpenFOAM Running, Solving & CFD  30  November 19, 2007 14:09 