[KleinMoretti]

Originally Posted by KleinMoretti

I used "cout" on the 5*5 grid of thermal bath example, h is 1 in 8.0.0, which is agreed with my expectation, because the initial field is given by the free stream condition, the pressure at all points on the grid is the same, so h is 1, but why is it close to 0 in rollback?

From the mathematical perspective, I can't find the difference of the pressure sensor calculations between 8.0.0 and rollback.

[CatarinaGarbacz]

where are you printing h in 8.0.0?

could you send me the file where you're printing and indicate the line, please?

[CatarinaGarbacz]

nevermind I just saw you posted the images of the code

[KleinMoretti]

Originally Posted by CatarinaGarbacz

where are you printing h in 8.0.0?

could you send me the file where you're printing and indicate the line, please?

Sure. The "cout" is at line 614 in 8.0.0 and line 191 in rollback.

[KleinMoretti]

Originally Posted by CatarinaGarbacz

where are you printing h in 8.0.0?

could you send me the file where you're printing and indicate the line, please?

I noticed in your article that it took 80 hours to calculate with 40 cores, was this calculation done under the rollback branch? Can you give me an approximate number of steps when it converges?

It took me 7 hours to calculate 200,000 steps in modified 8.0.0, but it looks particularly far away from converging.

[CatarinaGarbacz]

the AUSM implementation in the rollback and 8.0.0 branches are supposed to give different results, as discussed at the start of this thread.

if h_k / sensor variable is the only variable in the whole AUSM implementation that you found to be different between rollback and 8.0.0 branches, then this is the correction that has been made.

at the moment we are not sure which implementation is correct. some experimental cases agree better with one approach, and vice-versa. more detailed work would have to be done to get to the bottom of this issue.

-----

about code performance, I have no access to that information as those simulations have been performed too long ago. you mentioned the 7h and 200,000 steps, but what is the number of cores? if using the same number of cores as the paper (40 cores), many more hours are needed to reach convergence since in the paper it took around 80h

[KleinMoretti]

Originally Posted by CatarinaGarbacz

the AUSM implementation in the rollback and 8.0.0 branches are supposed to give different results, as discussed at the start of this thread.

if h_k / sensor variable is the only variable in the whole AUSM implementation that you found to be different between rollback and 8.0.0 branches, then this is the correction that has been made.

at the moment we are not sure which implementation is correct. some experimental cases agree better with one approach, and vice-versa. more detailed work would have to be done to get to the bottom of this issue.

-----

about code performance, I have no access to that information as those simulations have been performed too long ago. you mentioned the 7h and 200,000 steps, but what is the number of cores? if using the same number of cores as the paper (40 cores), many more hours are needed to reach convergence since in the paper it took around 80h

Hello, thank you for your help recently！ The result I got after modifying the 8.0.0 code is very close to the result in your article, but there are still slight differences. Near the degree=80-90 on the wall, the heat flux and pressure converge very slowly, and I have not completely converged in about 10 days under 32 cores.

I guess there may be something wrong with my grid. I want to refer to the structural grid in your article, but I don't understand it.

[KleinMoretti]

Originally Posted by CatarinaGarbacz

the AUSM implementation in the rollback and 8.0.0 branches are supposed to give different results, as discussed at the start of this thread.

if h_k / sensor variable is the only variable in the whole AUSM implementation that you found to be different between rollback and 8.0.0 branches, then this is the correction that has been made.

at the moment we are not sure which implementation is correct. some experimental cases agree better with one approach, and vice-versa. more detailed work would have to be done to get to the bottom of this issue.

-----

about code performance, I have no access to that information as those simulations have been performed too long ago. you mentioned the 7h and 200,000 steps, but what is the number of cores? if using the same number of cores as the paper (40 cores), many more hours are needed to reach convergence since in the paper it took around 80h

What does that mean, please? My understanding is that if there are x points circumferential and y points radial, then the total number of grid points is x*y, and the total number of cells is (x-1) * (y-1).

[KleinMoretti]

Originally Posted by CatarinaGarbacz

the AUSM implementation in the rollback and 8.0.0 branches are supposed to give different results, as discussed at the start of this thread.

if h_k / sensor variable is the only variable in the whole AUSM implementation that you found to be different between rollback and 8.0.0 branches, then this is the correction that has been made.

at the moment we are not sure which implementation is correct. some experimental cases agree better with one approach, and vice-versa. more detailed work would have to be done to get to the bottom of this issue.

-----

about code performance, I have no access to that information as those simulations have been performed too long ago. you mentioned the 7h and 200,000 steps, but what is the number of cores? if using the same number of cores as the paper (40 cores), many more hours are needed to reach convergence since in the paper it took around 80h

One more question, I saw in your paper that you also calculated inviscid flow, how do you give the boundary conditions for inviscid flow? It seems that the wall in NEMO_EULER can only be MARKER_EULER, not Isothermal noncatalytic wall.

[CatarinaGarbacz]

Hello,


slight differences are probably due to the slight differences in the mesh and, potentially, also lack of further convergence.

Indeed, near the degree=80-90 on the wall, the convergence was also extremely slow for us.

Your grid is not necessarily wrong, but just different, which could yield slight differences. What's the magnitude of the differences?

You're correct about the grid data, there's something wrong with it. Therefore I am not sure exactly how the grid was set up. But I can tell you that, we needed a first boundary layer thickness of 1e-7m to be able to match the wall heat flux with experimental data. So that is my recommendation. Other than that, even if you don't have exactly the same grid, having a similar or finer grid than the paper should yield similar results (even if not exactly the same, as there is always some influence of the grid, especially a structured grid where it is difficult to capture the shock in a perfect manner).

About the boundary condition, isothermal wall is a viscous boundary condition, so it only is applied for viscous flow. in the inviscid case, MARKER_EULER is the appropriate boundary condition. but this is general CFD knowledge, not specific to this code or paper

[KleinMoretti]

Originally Posted by CatarinaGarbacz

Hello,


slight differences are probably due to the slight differences in the mesh and, potentially, also lack of further convergence.

Indeed, near the degree=80-90 on the wall, the convergence was also extremely slow for us.

Your grid is not necessarily wrong, but just different, which could yield slight differences. What's the magnitude of the differences?

You're correct about the grid data, there's something wrong with it. Therefore I am not sure exactly how the grid was set up. But I can tell you that, we needed a first boundary layer thickness of 1e-7m to be able to match the wall heat flux with experimental data. So that is my recommendation. Other than that, even if you don't have exactly the same grid, having a similar or finer grid than the paper should yield similar results (even if not exactly the same, as there is always some influence of the grid, especially a structured grid where it is difficult to capture the shock in a perfect manner).

About the boundary condition, isothermal wall is a viscous boundary condition, so it only is applied for viscous flow. in the inviscid case, MARKER_EULER is the appropriate boundary condition. but this is general CFD knowledge, not specific to this code or paper

The curves of wall heat flux and pressure look close, but they are not completely converging, and their peaks are about 5%-6% different. The Ttr cloud picture is close, but the Tve cloud picture looks a lot worse. And Tve's cloud picture hasn't changed much in a while.

[KleinMoretti]

Originally Posted by CatarinaGarbacz

Hello,


slight differences are probably due to the slight differences in the mesh and, potentially, also lack of further convergence.

Indeed, near the degree=80-90 on the wall, the convergence was also extremely slow for us.

Your grid is not necessarily wrong, but just different, which could yield slight differences. What's the magnitude of the differences?

You're correct about the grid data, there's something wrong with it. Therefore I am not sure exactly how the grid was set up. But I can tell you that, we needed a first boundary layer thickness of 1e-7m to be able to match the wall heat flux with experimental data. So that is my recommendation. Other than that, even if you don't have exactly the same grid, having a similar or finer grid than the paper should yield similar results (even if not exactly the same, as there is always some influence of the grid, especially a structured grid where it is difficult to capture the shock in a perfect manner).

About the boundary condition, isothermal wall is a viscous boundary condition, so it only is applied for viscous flow. in the inviscid case, MARKER_EULER is the appropriate boundary condition. but this is general CFD knowledge, not specific to this code or paper

The thickness I set for the first layer of the wall normal element is exactly 1e-7

[CatarinaGarbacz]

My first comment is: here you are plotting your results, but there is no visual comparison with the reference results, that makes it difficult to say how they compare. If you're discussing a comparison between different sets of results, always plot them together.

As stated in the previous message, the convergence was seen to be extremely slow. So if you're results are still converging, there is no point in trying to make any final conclusions about small differences in magnitude that might be resolved by letting the simulation converge. Just let it run until it fully converges.

Also, even though you have successfully incorporated the AUSM correction from the older branch into the 8.0.0, there will be other differences between those 2 branches that can possibly be causing the small differences in the results. On top of that, as we discussed, the small differences in the mesh will also lead to slightly different results.

There is another important point I just realised now as you're showing me some results. The symmetry boundary condition of SU2 has a bug that comes up when simulating the stagnation line in supersonic flow. In this type of flow, the heat flux should increase monotonically along the wall and reach a maximum at the stagnation point. The fact that this is not happening in your case is a consequence of this bug. Contrary to the other factors (small differences in mesh and code), this is actually an issue, that you seemed to not have noticed. If you look at Fig. 5 of the paper (Impact of Anisotropic Mesh Adaptation on the Aerothermodynamics of Atmospheric Reentry), the author simulates both halves of the domain, to avoid the use of the symmetric BC, which yields a significantly different shape of the heat flux and pressure around the stagnation point. This is the problematic difference in your results that you should have noticed, because it actually corresponds to a different physical behavior (as opposed to having a similar shape with slight differences in magnitude). It is possible that this explains the differences of the contours of Tve and Ttr.

In any case, at this point, it seems that everything is going in the right direction.

If you're just trying to match your results with the paper, in my view, the conclusions is:
1- simulate the full domain to avoid the symmetry BC and focus on obtaining the correct shape of heat flux and pressure distributions

2- once the shape seems to be the correct one, let your results FULLY converge until they do not change anymore, and then compare the magnitude in more detail
3- this will probably already make your results much closer to the paper
4-if, at the end, the shape of the curves is the same but there are still small differences in magnitude, this is fine, as it is expected due to differences in the mesh and small corrections that have been done in the code
5- if those differences are small enough, given point 4, you can consider your results verified

[KleinMoretti]

Originally Posted by CatarinaGarbacz

My first comment is: here you are plotting your results, but there is no visual comparison with the reference results, that makes it difficult to say how they compare. If you're discussing a comparison between different sets of results, always plot them together.

As stated in the previous message, the convergence was seen to be extremely slow. So if you're results are still converging, there is no point in trying to make any final conclusions about small differences in magnitude that might be resolved by letting the simulation converge. Just let it run until it fully converges.

Also, even though you have successfully incorporated the AUSM correction from the older branch into the 8.0.0, there will be other differences between those 2 branches that can possibly be causing the small differences in the results. On top of that, as we discussed, the small differences in the mesh will also lead to slightly different results.

There is another important point I just realised now as you're showing me some results. The symmetry boundary condition of SU2 has a bug that comes up when simulating the stagnation line in supersonic flow. In this type of flow, the heat flux should increase monotonically along the wall and reach a maximum at the stagnation point. The fact that this is not happening in your case is a consequence of this bug. Contrary to the other factors (small differences in mesh and code), this is actually an issue, that you seemed to not have noticed. If you look at Fig. 5 of the paper (Impact of Anisotropic Mesh Adaptation on the Aerothermodynamics of Atmospheric Reentry), the author simulates both halves of the domain, to avoid the use of the symmetric BC, which yields a significantly different shape of the heat flux and pressure around the stagnation point. This is the problematic difference in your results that you should have noticed, because it actually corresponds to a different physical behavior (as opposed to having a similar shape with slight differences in magnitude). It is possible that this explains the differences of the contours of Tve and Ttr.

In any case, at this point, it seems that everything is going in the right direction.

If you're just trying to match your results with the paper, in my view, the conclusions is:
1- simulate the full domain to avoid the symmetry BC and focus on obtaining the correct shape of heat flux and pressure distributions

2- once the shape seems to be the correct one, let your results FULLY converge until they do not change anymore, and then compare the magnitude in more detail
3- this will probably already make your results much closer to the paper
4-if, at the end, the shape of the curves is the same but there are still small differences in magnitude, this is fine, as it is expected due to differences in the mesh and small corrections that have been done in the code
5- if those differences are small enough, given point 4, you can consider your results verified

Thank you very much! I will have a try.
.

[lqliang1222]

Originally Posted by KleinMoretti

After slightly expanding the calculation area, the result is better, but it can be seen that it is still far from the results in the article.

But I don't understand why the thickness of the shock layer is so thin.

It is said in the article that the radius of the cylinder of HEG is 45mm. From the picture in the article, the thickness of the shock layer is about 8-10mm, and my shock layer is only about half of it.

My heat flux on the wall is also about half of the results in the article, but the pressure on the wall is correct, why is this?

Hello, I would also like to reproduce this case and compare it with the experimental solution. Do you have any relevant data on wall pressure and heat flux? If possible, I would greatly appreciate it。

[CatarinaGarbacz]

Hello,


the experimental data you are asking for are plotted in Fig. 7 of the paper, so I am not sure what would you like me to provide

[lqliang1222]

Originally Posted by CatarinaGarbacz

Hello,


the experimental data you are asking for are plotted in Fig. 7 of the paper, so I am not sure what would you like me to provide

Hello,
What I understand is that I can roughly determine the values of the experimental results based on the coordinates in Figure 7, right?

[CatarinaGarbacz]

Yes but that's also how you would usually get reference data from other papers, using some plot digitizer software to extract the point from an image plot

[lqliang1222]

Originally Posted by CatarinaGarbacz

Yes but that's also how you would usually get reference data from other papers, using some plot digitizer software to extract the point from an image plot

Thank you very much. I just learned from my senior brother how to use software to extract points, and the issue has been resolved. Thank you