CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Software User Forums > ANSYS > CFX

Unable to reach monotonic convergence with mesh refinement

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

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   May 13, 2021, 19:43
Default Unable to reach monotonic convergence with mesh refinement
  #1
New Member
 
Parth
Join Date: May 2019
Posts: 11
Rep Power: 6
parth_k is on a distinguished road
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, 2-5 target loops range and 1-10 min-max 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.
Attached Images
File Type: png MAX RESIDUALS.png (46.3 KB, 15 views)
parth_k is offline   Reply With Quote

Old   May 14, 2021, 05:53
Default
  #2
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,690
Rep Power: 143
ghorrocks is just really niceghorrocks is just really niceghorrocks is just really niceghorrocks is just really nice
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.
ghorrocks is offline   Reply With Quote

Old   May 14, 2021, 08:16
Default
  #3
New Member
 
Parth
Join Date: May 2019
Posts: 11
Rep Power: 6
parth_k is on a distinguished road
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 1e-5 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.
Attached Images
File Type: png closeup_5grids.png (81.7 KB, 15 views)
parth_k is offline   Reply With Quote

Old   May 14, 2021, 08:36
Default
  #4
Senior Member
 
Join Date: Jun 2009
Posts: 1,799
Rep Power: 31
Opaque will become famous soon enough
Since you are doing a time-periodic 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.
Opaque is offline   Reply With Quote

Old   May 14, 2021, 09:24
Default
  #5
New Member
 
Parth
Join Date: May 2019
Posts: 11
Rep Power: 6
parth_k is on a distinguished road
Quote:
Originally Posted by Opaque View Post
Since you are doing a time-periodic 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.
Hi Opaque, many thanks for your tip. Yes have just checked as said and the plot shows a symmetric cyclic behavior which is as per the expectation since I'm simulating the models over a sufficiently long period to achieve transient stability.

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.
parth_k is offline   Reply With Quote

Old   May 14, 2021, 09:55
Default
  #6
Senior Member
 
Join Date: Jun 2009
Posts: 1,799
Rep Power: 31
Opaque will become famous soon enough
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.
Opaque is offline   Reply With Quote

Old   May 14, 2021, 10:38
Default
  #7
New Member
 
Parth
Join Date: May 2019
Posts: 11
Rep Power: 6
parth_k is on a distinguished road
Quote:
Originally Posted by Opaque View Post
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
Hi Opaque, regarding your first comment - I'm running an adaptive timestepping with a fairly wide limits for the min and max timestep range. I input a guess of about 1/(f*100) for the initial timestep and then let the sim to workaround between the adaptive limits. As I have even tried going to a lower timestep size value but it gives me an cfx-overflow error after a few its. Further I have no problem with the oscillatory signals and the velocity/pressure etc. plots are all in line with the expectations.

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 1e-4 perhaps? Coefficient loops between 1-10 should be still fine?

Also would you suggest to re-run 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.
parth_k is offline   Reply With Quote

Old   May 14, 2021, 10:51
Default
  #8
Senior Member
 
Join Date: Jun 2009
Posts: 1,799
Rep Power: 31
Opaque will become famous soon enough
Apologies I missed the adaptive time-stepping initial comment.

I have not used adaptive time-stepping 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 non-periodic 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.
Opaque is offline   Reply With Quote

Reply

Tags
cfd - post, cfx, mesh and grid, mesh refinement study, result comparision

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
decomposePar problem: Cell 0contains face labels out of range vaina74 OpenFOAM Pre-Processing 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


All times are GMT -4. The time now is 00:20.