[KleinMoretti]

Hello,everyone.
I want to reproduce the HEG cylinder testcase in《SU2-NEMO: An Open-Source Framework for High-Mach Nonequilibrium Multi-Species Flows》.

I made many attempts, but the results did not match the article at all. I looked at some of the questions in the forum and I guess there may be something wrong with my boundary conditions.

In this two-dimensional example, there are four boundaries, and I set them as MARKER_FAR,MARKER_SYM,MARKER_SUPERSONIC_OUTLET, and MARKER_ISOTHERMAL, respectively.

However, my wall heat flux and wall pressure are much different from the picture in the article.

I want to know if there are any errors in my boundary conditions.

Thank you in advance for your time and consideration. I truly appreciate any insights or advice you may have to offer.

[KleinMoretti]

This is my grid, which I cut from the article using incscape and AutoCAD.

[KleinMoretti]

In addition, I have another guess, is there a problem with my grid? If so, how can I improve it?

[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?

[CFDWhite]

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?

Could you provide your configuration file？

[KleinMoretti]

Originally Posted by CFDWhite

Could you provide your configuration file？

Thank you for your kind reply！ I really want to know where the problem is.

[KleinMoretti]

Originally Posted by CFDWhite

Could you provide your configuration file？

This is my cfg file.

[CatarinaGarbacz]

Hi, I'm one of the people that participated in this paper.

For this cylinder case, there was a code-fix that allowed to match the heat flux results. This fix is not in the develop/master branch, but it is in the branch NEMO_AUSMPLUSM_Rollback. If you restart your solution with this branch, you should get better results.

Furthermore, we have observed that heat flux convergence is more difficult to achieve than surface pressure, so make sure you have a fine enough first boundary layer ~ 1e-7m.

Of course, for accurate results, using a grid that captures the shock well is also important.

Catarina

[KleinMoretti]

Originally Posted by CatarinaGarbacz

Hi, I'm one of the people that participated in this paper.

For this cylinder case, there was a code-fix that allowed to match the heat flux results. This fix is not in the develop/master branch, but it is in the branch NEMO_AUSMPLUSM_Rollback. If you restart your solution with this branch, you should get better results.

Furthermore, we have observed that heat flux convergence is more difficult to achieve than surface pressure, so make sure you have a fine enough first boundary layer ~ 1e-7m.

Of course, for accurate results, using a grid that captures the shock well is also important.

Catarina

Hi,Catarina！Thank you very much!!!

You mean, I need to set CONV_NUM_METHOD_FLOW = AUSMPLUSM and modify the grid near the wall, right?

I'll try it right away！

[KleinMoretti]

Originally Posted by CatarinaGarbacz

Hi, I'm one of the people that participated in this paper.

For this cylinder case, there was a code-fix that allowed to match the heat flux results. This fix is not in the develop/master branch, but it is in the branch NEMO_AUSMPLUSM_Rollback. If you restart your solution with this branch, you should get better results.

Furthermore, we have observed that heat flux convergence is more difficult to achieve than surface pressure, so make sure you have a fine enough first boundary layer ~ 1e-7m.

Of course, for accurate results, using a grid that captures the shock well is also important.

Catarina

Hi,Catarina.

I have another question, what has been changed in this branch compared to master? From the point of the branch name, it seems that just modified the space discrete part about AUSMPLUSM scheme? Sorry, although I've seen some of SU2 source code, I'm not very familiar with it.

Thank you again for your kind reply!

[CatarinaGarbacz]

Hello,


yes that is correct, the main difference is a fix in the AUSMPLUSM scheme that will allow you to get the correct heat flux.

However, this was implemented a couple years ago in NEMO_AUSMPLUSM_Rollback which derived from the develop branch at the time, which has evolved significantly since then. Therefore, besides this specific fix, you will find a lot of structural differences between the NEMO_AUSMPLUSM_Rollback and the current develop/master, but most of those differences, if not all, should not impact the results.

[CatarinaGarbacz]

and yes, you should set CONV_NUM_METHOD_FLOW = AUSMPLUSM and modify the grid near the wall.

As i said in my first reply, if refining the wall grid + using this shceme in the NEMO_AUSMPLUSM_Rollback branch doesn't do the job, this could mean the shock also needs further refining

[KleinMoretti]

Originally Posted by CatarinaGarbacz

and yes, you should set CONV_NUM_METHOD_FLOW = AUSMPLUSM and modify the grid near the wall.

As i said in my first reply, if refining the wall grid + using this shceme in the NEMO_AUSMPLUSM_Rollback branch doesn't do the job, this could mean the shock also needs further refining

Thank you very much！

I'll try it right away！

[CFDWhite]

Originally Posted by CatarinaGarbacz

and yes, you should set CONV_NUM_METHOD_FLOW = AUSMPLUSM and modify the grid near the wall.

As i said in my first reply, if refining the wall grid + using this shceme in the NEMO_AUSMPLUSM_Rollback branch doesn't do the job, this could mean the shock also needs further refining

Hello, I have also read this article and calculated some examples, do you have any suggestions about the example of RAMC?

[KleinMoretti]

Originally Posted by CatarinaGarbacz

and yes, you should set CONV_NUM_METHOD_FLOW = AUSMPLUSM and modify the grid near the wall.

As i said in my first reply, if refining the wall grid + using this shceme in the NEMO_AUSMPLUSM_Rollback branch doesn't do the job, this could mean the shock also needs further refining

Hiya, I tried to compile the NEMO_AUSMPLUSM_rollback branch in linux and I have clearly set Dwith-mip=enabled, but the compiled file still can not use parallel computation.

I used the ldd command to look at the libraries that the SU2_CFD relies on, it does include mpi.

Why is that?

[KleinMoretti]

Originally Posted by CatarinaGarbacz

and yes, you should set CONV_NUM_METHOD_FLOW = AUSMPLUSM and modify the grid near the wall.

As i said in my first reply, if refining the wall grid + using this shceme in the NEMO_AUSMPLUSM_Rollback branch doesn't do the job, this could mean the shock also needs further refining

I also noticed that the NEMO solver in this branch can't use the implicit scheme, so did you use the explicit format to compute this example? If so , can you give me some advice about the CFL number?

Thank you for your kind help!

[CFDWhite]

Originally Posted by KleinMoretti

Hiya, I tried to compile the NEMO_AUSMPLUSM_rollback branch in linux and I have clearly set Dwith-mip=enabled, but the compiled file still can not use parallel computation.

I used the ldd command to look at the libraries that the SU2_CFD relies on, it does include mpi.

Why is that?

I'm a little confused about branch compilation： When compiling a new branch, does the previously compiled content need to be deleted？Thank you for all your suggestions

[KleinMoretti]

Originally Posted by CFDWhite

I'm a little confused about branch compilation： When compiling a new branch, does the previously compiled content need to be deleted？Thank you for all your suggestions

I don't think you need to delete it, because your previously compiled file and the new branch are usually not in the same folder.

[CatarinaGarbacz]

Hi,


yes, implicit scheme will not work in the NEMO_AUSMPLUSM_rollback branch.


Compiling without deleting anything should be enough. But if you're having issues, just clear everything and install/compile from scratch in the desired branch

[CatarinaGarbacz]

For the explicit scheme the CFL will vary depending on the mesh and the state of the simulation, and if you're using 1st or 2nd order, so there's no specific wrong or right answer.

It's the user's role to test different values and see what works, and gain their own sensitivity to this parameter. When explicit 1st order simulations converge easily CFL = 0.5-0.75 usually works. If using 2nd order or a mesh leading to more difficult convergence, CFL = 0.1 could be used. In some rare occasions, where the bow shock is very strong and may lead to carbuncle problem, I have had to use CFL = 0.01 to get an initial developed flow, and then raised it again. It's a bit of trial and error exercise that's very case dependent.