How to implement a sensitivity analysis for certain items
1 Attachment(s)
Hi,
I have read lots of the Sensitivity Analysis of some items, e.g. mesh size, inflation layer parameters,,, in this forum. But I'm not very sure how to implement this analysis. In my view maybe like below. Please give your comments.:confused: For the first layer thickness(correlated with Yplus) of inflation layer, if we want to do a sensitivity analysis we need to keep the other mesh parameters same and just change first layer thickness(maybe 1e2mm, 5e3mm, 1e3mm,,,) to finish several simulation and see if results(especially the variable you concern, maybe Drag Force) varies obviously.
Attachment 34377 Is my understanding about sensitivity analysis right or proper? Thank you so much. 
I should write an FAQ to explain this idea more thoroughly.
The main problem with your description is that the whole concept assumes that the output parameter converges as the input parameter is refined. So coarse inputs (such as a coarse mesh) should give large changes as the input parameter is refined, fine inputs (such as a fine mesh) should give small changes as the input parameter is refined, and eventually the changes in input parameter result in changes in output parameter which is too small to see. Further refinement in the input parameter does not affect the output. That is the ideal situation, some things which can cause headaches include: * The sensitivities are coupled, so mesh refinement requires time step refinement and might also change you convergence criteria. * You cannot refine the mesh too much as the simulation run time or memory requirements becomes too large * Effects such as numerical roundoff means you cannot refine the mesh or time step too far either This is a very simple outline of it. This reference goes into more detail: http://journaltool.asme.org/Template...umAccuracy.pdf and the text book "Computational Fluid Dynamics" by Roache is the seminal textbook on CFD accuracy, so is definitely worth a read if you want a thorough understanding of it. 
Quote:
Quote:
Quote:

1 Attachment(s)
Quote:
Is it acceptable that last cell thickness in inflation layer is very small than nearby tetra element size? Like below picture, I know that mesh in (B) is obviously good, but sometimes it's really hard to realize this expansion ratio. And my question is that 'mesh in (A) is acceptable???' Thanks a lot. Attachment 34385 
Case B is preferable. But whether A is acceptable will depend on what you are modelling. Different models have different sensitivities to mesh quality. The best thing to do here is to do a sensitivity study on this parameter (the ratio of the element size from the tets to the first prism layer) and see if it makes a difference in your case.

Is my mesh good enough?
Thanks ghorrocks for helping everyone.
I was applying those criteria but I did not know that this procedure had a name. I found this article for FEA simulation that complements your idea: https://caeai.com/blog/howdoiknow...shgoodenough Quote:
At the beginning, I though that CFX meshing software had some hidden command to evaluate the mesh. :) 
In the .out file you can see the mesh statistics, which are measured by:
OK ok ! OK  this is good ok  this is "okay" but can be improved if needed !  this needs attention 
Thanks Mr CFD, it is good to mention those quality measures.
Note that these mesh quality measures (and in fact any mesh quality measures) need to be considered against the simulation you are doing. For instance if you are doing a simple simulation  maybe a single phase flow at low Reynolds number  then lots of "!" mesh quality elements is still going to be fine. But if you are doing surface tension simulations then any elements which are out of the "OK" zone will cause problems. So a mesh which is good for one type of simulation might not be good for another. So mesh metrics are just a guide. 
Mesh statistics measure
Quote:
Is it the same notation for CFX 5? Did you mean the red words in the following extract of the output file? If your answer is yes. what is the meaning of "**" and "F"? I have no "!" in this file, so I guess "**" and "F" means this needs attention ================================================== ==================== OUTER LOOP ITERATION = 1 CPU SECONDS = 2.298E+01   Equation  Rate  RMS Res  Max Res  Linear Solution  ++++++  UMomAir at 25 C  0.00  3.9E06  9.3E05  4.6E+00 F   VMomAir at 25 C  0.00  3.8E06  8.8E05  6.1E+00 F   WMomAir at 25 C  0.00  1.6E02  1.7E+00  1.8E+00 F   UMomWater  0.00  2.4E05  1.2E03  4.4E+00 F   VMomWater  0.00  2.2E05  1.3E03  5.2E+00 F   WMomWater  0.00  2.4E01  6.3E+01  1.2E+00 F   PVol  0.00  7.5E10  1.1E07  17.2 2.6E01 ok ++++++  MassAir at 25 C  0.00  1.1E01  3.9E01  10.7 1.7E03 OK  MassWater  0.00  9.9E02  3.1E01  10.6 2.5E03 OK ++++++ ================================================== ==================== OUTER LOOP ITERATION = 2 CPU SECONDS = 1.134E+02   Equation  Rate  RMS Res  Max Res  Linear Solution  ++++++  UMomAir at 25 C 99.99  3.0E03  3.5E02  4.5E02 OK  VMomAir at 25 C 99.99  2.7E03  3.3E02  4.7E02 OK  WMomAir at 25 C 72.43  1.2E+00  7.5E+00  5.9E04 OK  UMomWater 99.99  8.5E03  2.5E01  6.4E02 OK  VMomWater 99.99  7.6E03  2.4E01  6.5E02 OK  WMomWater 12.06  3.0E+00  1.9E+01  6.6E04 OK  PVol 99.99  6.4E03  7.7E01  9.1 8.0E02 OK ++++++  MassAir at 25 C  0.39  4.2E02  3.8E01  10.6 1.1E03 OK  MassWater  0.70  6.9E02  4.3E01  10.6 1.3E03 OK ++++++  WMomWater  0.00  2.4E01  6.3E+01  1.2E+00 F   PVol  0.00  7.5E10  1.1E07  17.2 2.6E01 ok  UMomAir at 25 C 99.99  1.2E05  2.6E03  NaN ok   UMomAir at 25 C  0.14  1.8E06  3.0E04  NaN **   MassAir at 25 C  2.49  2.0E02  1.0E+00  10.4 1.8E02 OK 
Same notation as CFX5  Yes. But that is very old, I hope you are not using CFX5, it is very superseded now.
What you have shown here is different. You are showing the convergence of the linear solver. OK means the linear solver converged OK, "ok" means it converged but only just, F means it failed to converge but did not diverge massively, and the other symbols mean you may have a problem. This is discussed in more detail in the CFX documentation. 
CFX documentation
Thanks ghorrocks!
Quote:
Quote:
Quote:

All times are GMT 4. The time now is 09:15. 