[HectorRedal]

Originally Posted by arjun

Now if you are able to get it to run with higher time step size then understand that your solution now is more smooth or diffusive.

At this moment it is hard to know if it is due to bug or it is supposed to behave this way.

Anyway, now I would suggest that run the same calculation with first order upwind then then reduce the timestep. Since upwind scheme also has diffusive nature or error, it shall be stable again and allow you smaller time step.

Also can I ask, what solver we are talking about. Is it one of the commercial code?

It is a software developed on my own based on the Characteristics Based Split Algorithm, Zienkiewicz et all (Finite element Method)

[arjun]

Originally Posted by HectorRedal

It is a software developed on my own based on the Characteristics Based Split Algorithm, Zienkiewicz et all (Finite element Method)

This was really important information. The part in FE type solvers that does the job of dissipation is related to 'inf - sub' condition.

Since I am not an expert on FE solvers, I can not write about it in detail but I know that this directly affect the stability and the dissipation that we talk about. It is also related to mesh size.

For example

http://onlinelibrary.wiley.com/doi/1...m.508/abstract

[FMDenaro]

Originally Posted by HectorRedal

The point with your reasoning that I do not fully agree with is the one stating that the problem is related to diffusion (artificial viscosity). Maybe the error is not in the calculation of the viscotity term of the algorithm but in any other term. Something that I have to investigate. The point is that I am facing this problem more than one year and it is still unsolved. I am not very confident I will be able to find it either.

Be careful, an artificial viscosity does not mean an error in the discretization of the diffusion! Conversely, it is typical of the discretization of time derivative along with convective term.

[arjun]

Originally Posted by FMDenaro

Be careful, an artificial viscosity does not mean an error in the discretization of the diffusion! Conversely, it is typical of the discretization of time derivative along with convective term.

What he said.

It is not the error in viscosity but a error that has effect similar to viscosity in system.

[juliom]

Originally Posted by HectorRedal

Hi Filippo,

The estimated error slope was approximately 2, which matches the second order error of the Characteristics Based Split Algorithm (according to the authors Zienkiewicz et al).

Hector could you please provide more information about the work you used to determine the order of accuracy from your scheme? I have read about the manufactured solution, but I am not quite sure that is the same that you cited.

PS: Please bear with me with my typos, I was writing from my cell phone and my dictionary betrayed me. !!

[FMDenaro]

Originally Posted by arjun

What he said.

It is not the error in viscosity but a error that has effect similar to viscosity in system.

What I want to say is that given the physical (positive) viscosity in the diffusive term, a blow-up corresponds to an asymptotic increasing of the gradient of the solution, a fact that can be explained by an artificial negative viscosity that is greater than the physical one. Since that happens for small time-step my idea is:

1) a spatial error that produces such negative viscosity and appears when the time step is small
2) an error in the time integration, that means the scheme is not consistent

[FMDenaro]

Originally Posted by HectorRedal

It is a software developed on my own based on the Characteristics Based Split Algorithm, Zienkiewicz et all (Finite element Method)

Did you performed the analytical test case by taking dt/h=constant or by fixing one grid and refining the time-step?

[juliom]

Professor, I have a question in regards the analytical test case that you have suggested. We usually do not have the analytical solution of the problem, how can we perform such as analysis?
My guess is that, it is possible to implement the exact discretization scheme (in time and space) that we implemented in our CFD but for the convection equation in 1D whose analytical solution is known. However, I am not sure if the viscous term is present in the convection equation.
In case we had the analytical solution (convection + diffusion), we will be able to compare the analytical solution with the numerical solution. Is this the right track or I am definitely pointing to a wrong direction?
Could you please provide references or guidance to perform such as analysis? I would appreciate that since that analysis is quite useful for identifying bugs.
Thanks!!

[FMDenaro]

Originally Posted by juliom

Professor, I have a question in regards the analytical test case that you have suggested. We usually do not have the analytical solution of the problem, how can we perform such as analysis?
My guess is that, it is possible to implement the exact discretization scheme (in time and space) that we implemented in our CFD but for the convection equation in 1D whose analytical solution is known. However, I am not sure if the viscous term is present in the convection equation.
In case we had the analytical solution (convection + diffusion), we will be able to compare the analytical solution with the numerical solution. Is this the right track or I am definitely pointing to a wrong direction?
Could you please provide references or guidance to perform such as analysis? I would appreciate that since that analysis is quite useful for identifying bugs.
Thanks!!

This is an exact solution for the 3D NS equations, very useful to test own-made codes

http://onlinelibrary.wiley.com/doi/1...20D31EB.f04t04

[juliom]

Thank you very much professor. !

[HectorRedal]

Originally Posted by arjun

This was really important information. The part in FE type solvers that does the job of dissipation is related to 'inf - sub' condition.

Since I am not an expert on FE solvers, I can not write about it in detail but I know that this directly affect the stability and the dissipation that we talk about. It is also related to mesh size.

For example

http://onlinelibrary.wiley.com/doi/1...m.508/abstract

According to the authors, the algorithm satisfy the Babuska Brezzi (BB) restrictions:
https://www.researchgate.net/publica..._CBS_algorithm

So, I understand the inf-sup condition is also satisfied.

[HectorRedal]

Originally Posted by FMDenaro

Did you performed the analytical test case by taking dt/h=constant or by fixing one grid and refining the time-step?

I built three diferent meshes for the typical problem of the Lid Driven Cavity Flow, for Re1000:
- One coarse mesh
- A medium mesh
- A fine mesh

I measured the L_0 and L_inf error of the solution obtained in each mesh, then take the logarithm of that error and draw the straight line fit that passes throught the three points. The slope of the line gives me the order of the algorithm, which was aproximately 2.

I have to admit that I didn't take the dt/dh constant.

[FMDenaro]

Originally Posted by HectorRedal

I built three diferent meshes for the typical problem of the Lid Driven Cavity Flow, for Re1000:
- One coarse mesh
- A medium mesh
- A fine mesh

I measured the L_0 and L_inf error of the solution obtained in each mesh, then take the logarithm of that error and draw the straight line fit that passes throught the three points. The slope of the line gives me the order of the algorithm, which was aproximately 2.

I have to admit that I didn't take the dt/dh constant.

well, the lid-driven cavity is not suitable to perform a convergence analysis ... use instead the analytical solution and use the L_inf norm on both velocity component.

[arjun]

Originally Posted by HectorRedal

According to the authors, the algorithm satisfy the Babuska Brezzi (BB) restrictions:
https://www.researchgate.net/publica..._CBS_algorithm

So, I understand the inf-sup condition is also satisfied.

This is why I said I draw your attention to it and can not make definite statement. If you think this part is not important then ignore it as I don't understand FE implementation much.

On paper though, in FV Rhie and Chow should take care of coupling but in practice the coupling weakens as time step goes down or skew increases.

So i wished you look into it if this is the case in FE too (in my understanding they behave quite similar but i am not sure).

[HectorRedal]

Originally Posted by arjun

This is why I said I draw your attention to it and can not make definite statement. If you think this part is not important then ignore it as I don't understand FE implementation much.

On paper though, in FV Rhie and Chow should take care of coupling but in practice the coupling weakens as time step goes down or skew increases.

So i wished you look into it if this is the case in FE too (in my understanding they behave quite similar but i am not sure).

Hi Arjun,

I really appreciate your help and support on this issue.

I would like to comment that finally I have found an error in the code when retrieving the value of the pressue from the previous step. There was an initialization error in a loop that iterates over the nodes of the TRIA element.
After having fixed the error, I have tested and it (reducing the time step), and it appears that it is working now.

I have tested with delta T = 10e-6 and even with 10e-7, and the solution does not blow up at all. It really provides quite accurate and good results, at first sight.

Thanks a log for your help.

BR

[FMDenaro]

Good, that's what I expected.

However, you still can not be sure of further bugs in your code. The lid driven cavity test-case does not help in this assessment (we can discuss a lot about why) and you should still consider the analytical test-case to compute the solutions on several refined grids both while taking dt/h= constant and using via via refined time step fixing one grid with the smallest h you can use.

[juliom]

I was thinking about that , the why??? Yesterday, you mentioned that the cavity flow was not the most appropriate case, but I was not able to find out the reason.

It would be very interesting to know the reasons. !!

[FMDenaro]

Originally Posted by juliom

I was thinking about that , the why??? Yesterday, you mentioned that the cavity flow was not the most appropriate case, but I was not able to find out the reason.

It would be very interesting to know the reasons. !!

First of all, the solution of the lid-driven cavity is obtained by your code. Therefore, if you have a bug and it does not produce a blow-up, the solution you will use contains an error that you simply scale-off from the convergence analysis.
Second, the slope must be evaluated asymptotically, therefore if you do not have an analytical solution you have to introduce some corrections (we discussed about that). A very refined grid is necessary

[juliom]

Thanks professor; I thought that the reasons were more from another physical limitation of the cavity flow.
Although your last comment summarize very well the discussions in this post.

[FMDenaro]

Originally Posted by juliom

Thanks professor; I thought that the reasons were more from another physical limitation of the cavity flow.
Although your last comment summarize very well the discussions in this post.

well, it is well known that the lid driven has a singularity in the lid corner