|
[Sponsors] |
March 12, 2024, 22:33 |
HEG cylinder boundary conditions in NEMO
|
#1 |
Member
AN
Join Date: Jan 2024
Posts: 43
Rep Power: 2 |
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. |
|
March 12, 2024, 22:46 |
|
#2 |
Member
AN
Join Date: Jan 2024
Posts: 43
Rep Power: 2 |
This is my grid, which I cut from the article using incscape and AutoCAD.
|
|
March 14, 2024, 04:03 |
|
#3 |
Member
AN
Join Date: Jan 2024
Posts: 43
Rep Power: 2 |
In addition, I have another guess, is there a problem with my grid? If so, how can I improve it?
|
|
March 14, 2024, 20:52 |
|
#4 |
Member
AN
Join Date: Jan 2024
Posts: 43
Rep Power: 2 |
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? |
|
March 17, 2024, 22:12 |
|
#5 | |
New Member
Liming Yang
Join Date: Sep 2023
Posts: 28
Rep Power: 2 |
Quote:
|
||
March 17, 2024, 22:31 |
|
#6 |
Member
AN
Join Date: Jan 2024
Posts: 43
Rep Power: 2 |
||
March 17, 2024, 22:33 |
|
#7 |
Member
AN
Join Date: Jan 2024
Posts: 43
Rep Power: 2 |
This is my cfg file.
|
|
March 18, 2024, 07:04 |
this is the right answer, should fix it
|
#8 |
New Member
Catarina Garbacz
Join Date: Jun 2020
Posts: 25
Rep Power: 5 |
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 |
|
March 18, 2024, 20:24 |
|
#9 | |
Member
AN
Join Date: Jan 2024
Posts: 43
Rep Power: 2 |
Quote:
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! |
||
March 18, 2024, 21:08 |
|
#10 | |
Member
AN
Join Date: Jan 2024
Posts: 43
Rep Power: 2 |
Quote:
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! |
||
March 19, 2024, 08:02 |
|
#11 |
New Member
Catarina Garbacz
Join Date: Jun 2020
Posts: 25
Rep Power: 5 |
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. |
|
March 19, 2024, 08:04 |
|
#12 |
New Member
Catarina Garbacz
Join Date: Jun 2020
Posts: 25
Rep Power: 5 |
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 |
|
March 19, 2024, 22:25 |
|
#13 | |
Member
AN
Join Date: Jan 2024
Posts: 43
Rep Power: 2 |
Quote:
I'll try it right away! |
||
March 20, 2024, 20:58 |
|
#14 | |
New Member
Liming Yang
Join Date: Sep 2023
Posts: 28
Rep Power: 2 |
Quote:
|
||
March 20, 2024, 21:06 |
|
#15 | |
Member
AN
Join Date: Jan 2024
Posts: 43
Rep Power: 2 |
Quote:
I used the ldd command to look at the libraries that the SU2_CFD relies on, it does include mpi. Why is that? |
||
March 20, 2024, 21:15 |
|
#16 | |
Member
AN
Join Date: Jan 2024
Posts: 43
Rep Power: 2 |
Quote:
Thank you for your kind help! |
||
March 21, 2024, 02:48 |
|
#17 | |
New Member
Liming Yang
Join Date: Sep 2023
Posts: 28
Rep Power: 2 |
Quote:
|
||
March 21, 2024, 03:49 |
|
#18 |
Member
AN
Join Date: Jan 2024
Posts: 43
Rep Power: 2 |
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.
|
|
March 21, 2024, 08:33 |
|
#19 |
New Member
Catarina Garbacz
Join Date: Jun 2020
Posts: 25
Rep Power: 5 |
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 |
|
March 21, 2024, 08:39 |
|
#20 |
New Member
Catarina Garbacz
Join Date: Jun 2020
Posts: 25
Rep Power: 5 |
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. |
|
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
CFD analaysis of Pelton turbine | amodpanthee | CFX | 31 | April 19, 2018 18:02 |
Out File does not show Imbalance in % | Mmaragann | CFX | 5 | January 20, 2017 10:20 |
Waterwheel shaped turbine inside a pipe simulation problem | mshahed91 | CFX | 3 | January 10, 2015 11:19 |
An error has occurred in cfx5solve: | volo87 | CFX | 5 | June 14, 2013 17:44 |
Error finding variable "THERMX" | sunilpatil | CFX | 8 | April 26, 2013 07:00 |