Mesh Independence Study

Nurzhan · March 28, 2016, 20:52

Dear experts,

I am currently doing a mesh independence study of my CFD model, using ANSY CFX. It is a 3D model of the distribution of electrical current within an isotropic material. The obtained results were verified using the analytical solution of four-electrode resistivity technique (see link below).

https://drive.google.com/file/d/0B8R...ew?usp=sharing

It seems that the error reduces up to certain mesh spacing, and then goes up. Is it normal, if not, then what can be a problem? The result of the mesh independence study is in the link below.

https://drive.google.com/file/d/0B8R...ew?usp=sharing

Thank you in advance!
Regards,
Nurzhan

monkey1 · March 29, 2016, 02:40

Hi Nurzhan!
Your Mesh "independency" looks a little weird to me.
Usually a mesh independent solution would mean the error reaches an asymptotic value independetly of further refinement of the mesh. And refinement would require in the mathematical sense of the word, that you divide each time the cell size by half, meaning doubling the cell number in each direction, resulting in multiplying the number of cells in a 3D simulation by 8 for each refinement step.
Maybe you are still too coarse with your mesh. Don't know what mesh sizes are usually required in simulations of electrical current but looking at your Error Graph I had the feeling that the number of elements is quite low...but I usually do Fluid flow simulations.

Nurzhan · March 29, 2016, 03:20

Hi!

And first of all, thank you for your reply!

I do agree that mesh independence does not look right (the result is highly dependent on the mesh spacing), but this is what I've got based on my model. I checked the residuals and they are fine, and honestly do not know what can be a cause.

Regarding my graph, the number of mesh elements per a single direction means that when I have 100 mesh elements in a single direction, it is 1,000,000 elements in the whole 3D cubic geometry.

Thanks again!
N

monkey1 · March 29, 2016, 03:35

Sorry, seems as if I didn't express myself clearly.
The remark "I had the feeling that the number of elements is quite low" referred to all the points drawn in your diagram for element numbers below 40-50 per direction. Resulting in the fact, that considering the rule to double the number of elements per direction for each new mesh, you only investigated 2 refinements, max. 3 if we want to consider 20 elemnts per direction as suffieciently resolving the case:
One mesh with only 8.000 Elements, then 64.000, then 512.000 and finally 4 Mio Elements.
And I wanted to ask if maybe an even finer mesh than the 4 Mio must be investigated to get a satisfying answer. I observed comparable phenomena to the one shown in your diagram in the fluid flow refinement when looking at meshes that were still too coarse. Of course sometimes it can happen that due to hardware limitations you will not be able to drive your mesh independency study any further in the direction required.

How many cells are there between your electrodes in each case?

You stated that your residuals are fine...unfortunately I had to make the experience, that they can be fine very often although the calculated result is crap

The only reliable indicators, are the values of the relevant variables calculated.

Nurzhan · March 29, 2016, 19:34

Dear monkey1,

I re-did the mesh independence study with slightly different material properties. I also enlarged distance between electrodes. My mesh independence study was done with the following numbers of elements (for a simplicity reason, I used the total number of mesh elements this time): 1,000, 8,000, 64,000, 512,000, 2,744,000, 4,096,000 and 8,000,000. Unfortunately, I cannot refine my mesh any further.

https://drive.google.com/file/d/0B8R...ew?usp=sharing

Although, the mesh independence looks much better now, the fact that the lowest error is at 1,000 mesh elements, makes me quite suspicious.

I also looked at number of elements between electrodes, which at 8,000,000 mesh elements, looks quite dense.

https://drive.google.com/file/d/0B8R...ew?usp=sharing

ghorrocks · March 29, 2016, 20:01

Mesh independance studies often have a converging region where the result converges towards the zero mesh size result, but at very coarse meshes the results go all over the place as the mesh is too coarse to resolve anything important and you are getting almost random numbers.

So in your case I think we can say your coarsest mesh result is in the region where the mesh is too coarse to resolve anything so the results are rubbish and the "accurate" result is just luck. The nicely converging accuracy with finer mesh for the other meshes is strong evidence that you are converging well in that region.

Nurzhan · March 29, 2016, 22:50

Hi Glenn,

Thanks for the explanation, it is highly appreciated!

Regards,
Nurzhan

monkey1 · March 30, 2016, 03:04

Hi Nurzhan,

Glenn was faster answering. But I would have said the same.
Especially now looking at the trend of your curve you definitely see, that you are converging monotonously towards the mesh independence.

I only have one question: The "error" you are plotting is what?
It might be that you would see an even "better" result when looking at the interesting variables.
E.g. for my flow simulations I try to compare the changes in the velocity profiles and not numerical errors made. And when my Profiles change with less than a threshold percentage value, I deduce mesh independency.

So as you are doing electrical current simulations...wouldn't it be more practicable to compare the values of the electric current?

I suspect that your "error" is the deviation from any experimental values. This is certainly a good thing to do for validation purposes to compare the simulated results to experimental ones, but for proving mesh independency it is more practicable to compare the simualtion results to each other. Why I'm saying that, is that you never know how close you will possibly get to experimental values in a simualtion. In most part of the cases because you never measured all required boundary condition values for the simulation in the experiment, so that you will never achieve 0% Error. In the other part it is also due to the still lacking computer power for most of us to carry out "real case" simulations, like e.g. DNS for atmopsheric flow.

Nurzhan · March 30, 2016, 05:41

Hi monkey1,

And again, I am very thankful for your reply!

Actually, the error was calculated using the available analytical solution for this problem. Usually, without an analytical solution, I derive an error from my numerical results, waiting when the result hardly changes. However, the analytical solution is available, I used the exact solution for my verification procedure.

Regards,
Nurzhan

P.S. Being a young CFD engineer, I really appreciate the help provided by senior guys such as you and Glenn! Thanks!

ghorrocks · March 30, 2016, 06:57

In that case your results are still a reasonable distance from the analytical result even with your finest mesh. Don't forget that you should also do sensitivity analyses on convergence tolerance, time step size (if transient) and any other tunable parameter.

March 28, 2016, 20:52	Mesh Independence Study	#1
Nurzhan Member Nurzhan Join Date: Jan 2014 Posts: 56 Rep Power: 12	Dear experts, I am currently doing a mesh independence study of my CFD model, using ANSY CFX. It is a 3D model of the distribution of electrical current within an isotropic material. The obtained results were verified using the analytical solution of four-electrode resistivity technique (see link below). https://drive.google.com/file/d/0B8R...ew?usp=sharing It seems that the error reduces up to certain mesh spacing, and then goes up. Is it normal, if not, then what can be a problem? The result of the mesh independence study is in the link below. https://drive.google.com/file/d/0B8R...ew?usp=sharing Thank you in advance! Regards, Nurzhan

Similar Threads
Thread	Thread Starter	Forum	Replies	Last Post
[snappyHexMesh] SnappyHexMesh for internal Flow	vishwa	OpenFOAM Meshing & Mesh Conversion	24	June 27, 2016 08:54
(New to CFD) How to do a mesh refinement study w/ Fluent?	JAviles	FLUENT	3	June 27, 2014 13:55
Convergence moving mesh	lr103476	OpenFOAM Running, Solving & CFD	30	November 19, 2007 14:09
Icemcfd 11: Loss of mesh from surface mesh option?	Joe	CFX	2	March 26, 2007 18:10
How to control Minximum mesh space?	hung	FLUENT	7	April 18, 2005 09:38

March 29, 2016, 02:40		#2
monkey1 Senior Member Join Date: Jul 2011 Location: Berlin, Germany Posts: 173 Rep Power: 14	Hi Nurzhan! Your Mesh "independency" looks a little weird to me. Usually a mesh independent solution would mean the error reaches an asymptotic value independetly of further refinement of the mesh. And refinement would require in the mathematical sense of the word, that you divide each time the cell size by half, meaning doubling the cell number in each direction, resulting in multiplying the number of cells in a 3D simulation by 8 for each refinement step. Maybe you are still too coarse with your mesh. Don't know what mesh sizes are usually required in simulations of electrical current but looking at your Error Graph I had the feeling that the number of elements is quite low...but I usually do Fluid flow simulations.

March 29, 2016, 03:20		#3
Nurzhan Member Nurzhan Join Date: Jan 2014 Posts: 56 Rep Power: 12	Hi! And first of all, thank you for your reply! I do agree that mesh independence does not look right (the result is highly dependent on the mesh spacing), but this is what I've got based on my model. I checked the residuals and they are fine, and honestly do not know what can be a cause. Regarding my graph, the number of mesh elements per a single direction means that when I have 100 mesh elements in a single direction, it is 1,000,000 elements in the whole 3D cubic geometry. Thanks again! N

March 29, 2016, 03:35		#4
monkey1 Senior Member Join Date: Jul 2011 Location: Berlin, Germany Posts: 173 Rep Power: 14	Sorry, seems as if I didn't express myself clearly. The remark "I had the feeling that the number of elements is quite low" referred to all the points drawn in your diagram for element numbers below 40-50 per direction. Resulting in the fact, that considering the rule to double the number of elements per direction for each new mesh, you only investigated 2 refinements, max. 3 if we want to consider 20 elemnts per direction as suffieciently resolving the case: One mesh with only 8.000 Elements, then 64.000, then 512.000 and finally 4 Mio Elements. And I wanted to ask if maybe an even finer mesh than the 4 Mio must be investigated to get a satisfying answer. I observed comparable phenomena to the one shown in your diagram in the fluid flow refinement when looking at meshes that were still too coarse. Of course sometimes it can happen that due to hardware limitations you will not be able to drive your mesh independency study any further in the direction required. How many cells are there between your electrodes in each case? You stated that your residuals are fine...unfortunately I had to make the experience, that they can be fine very often although the calculated result is crap The only reliable indicators, are the values of the relevant variables calculated.

March 29, 2016, 19:34		#5
Nurzhan Member Nurzhan Join Date: Jan 2014 Posts: 56 Rep Power: 12	Dear monkey1, I re-did the mesh independence study with slightly different material properties. I also enlarged distance between electrodes. My mesh independence study was done with the following numbers of elements (for a simplicity reason, I used the total number of mesh elements this time): 1,000, 8,000, 64,000, 512,000, 2,744,000, 4,096,000 and 8,000,000. Unfortunately, I cannot refine my mesh any further. https://drive.google.com/file/d/0B8R...ew?usp=sharing Although, the mesh independence looks much better now, the fact that the lowest error is at 1,000 mesh elements, makes me quite suspicious. I also looked at number of elements between electrodes, which at 8,000,000 mesh elements, looks quite dense. https://drive.google.com/file/d/0B8R...ew?usp=sharing

March 29, 2016, 20:01		#6
ghorrocks Super Moderator Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,700 Rep Power: 143	Mesh independance studies often have a converging region where the result converges towards the zero mesh size result, but at very coarse meshes the results go all over the place as the mesh is too coarse to resolve anything important and you are getting almost random numbers. So in your case I think we can say your coarsest mesh result is in the region where the mesh is too coarse to resolve anything so the results are rubbish and the "accurate" result is just luck. The nicely converging accuracy with finer mesh for the other meshes is strong evidence that you are converging well in that region.

March 29, 2016, 22:50		#7
Nurzhan Member Nurzhan Join Date: Jan 2014 Posts: 56 Rep Power: 12	Hi Glenn, Thanks for the explanation, it is highly appreciated! Regards, Nurzhan

March 30, 2016, 03:04		#8
monkey1 Senior Member Join Date: Jul 2011 Location: Berlin, Germany Posts: 173 Rep Power: 14	Hi Nurzhan, Glenn was faster answering. But I would have said the same. Especially now looking at the trend of your curve you definitely see, that you are converging monotonously towards the mesh independence. I only have one question: The "error" you are plotting is what? It might be that you would see an even "better" result when looking at the interesting variables. E.g. for my flow simulations I try to compare the changes in the velocity profiles and not numerical errors made. And when my Profiles change with less than a threshold percentage value, I deduce mesh independency. So as you are doing electrical current simulations...wouldn't it be more practicable to compare the values of the electric current? I suspect that your "error" is the deviation from any experimental values. This is certainly a good thing to do for validation purposes to compare the simulated results to experimental ones, but for proving mesh independency it is more practicable to compare the simualtion results to each other. Why I'm saying that, is that you never know how close you will possibly get to experimental values in a simualtion. In most part of the cases because you never measured all required boundary condition values for the simulation in the experiment, so that you will never achieve 0% Error. In the other part it is also due to the still lacking computer power for most of us to carry out "real case" simulations, like e.g. DNS for atmopsheric flow.

March 30, 2016, 05:41		#9
Nurzhan Member Nurzhan Join Date: Jan 2014 Posts: 56 Rep Power: 12	Hi monkey1, And again, I am very thankful for your reply! Actually, the error was calculated using the available analytical solution for this problem. Usually, without an analytical solution, I derive an error from my numerical results, waiting when the result hardly changes. However, the analytical solution is available, I used the exact solution for my verification procedure. Regards, Nurzhan P.S. Being a young CFD engineer, I really appreciate the help provided by senior guys such as you and Glenn! Thanks!

March 30, 2016, 06:57		#10
ghorrocks Super Moderator Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,700 Rep Power: 143	In that case your results are still a reasonable distance from the analytical result even with your finest mesh. Don't forget that you should also do sensitivity analyses on convergence tolerance, time step size (if transient) and any other tunable parameter.