[GAB_STO]

Hi,

I am new to SU2, and I’m really interested to learn more about it. For one of my projects, I want to experiment with hypersonic flow. I also want to simulate every physical aspect of that flow.

I’ve done a few research and it seems that earlier SU2 version had some specialized solver for that task. TNE2_NAVIER_STOKES and TNE_EULER seem to be a great start for that objective. Unfortunately, they don’t seem available in SU2 V7.0.5 Blackbird which is the current version of SU2 and the one that I am working with.

I’ve also noticed that the TNE2 solver will be recast into NEMO (NonEquilibrium MOdels) solver. Does anyone as any indication if this solver is still in development or if it’s available?

I am also wondering if there is any way to get access to those solver (TNE2 or NEMO) and some test cases or tutorials to work with SU2 V7.0.5?

Thanks for your inputs!

[CatarinaGarbacz]

Hello Gabriel,

I am actually one of the people who is currently developing this code. You're right that the old TNE2 solver is nnow called NEMO, and that it is not yet available in the latest master version or the develop branch.

There's a feature_NEMO branch in SU2. I cannot guarantee you this version is working a 100%, but you can try and run some test-cases with it to start getting familiar.

The work I'm doing at the moment is updating feature_NEMO to the develop branch to release it there. We expect to have this ready wihin the next 1 (max 2) months.

Hope this helps to clarify your question. Let me know if there any way I can help.

Best,
Catarina

[atelcikti1]

Hi Catarina,


I appreciate your work, in the original (first) version of NEMO solver named SU2-feature_AdjTNE2, there were some missing points such as boundary conditions, which are only applied for far-field and walls. The pressure outlet, mass flow inlet and pressure inlets were missing. I checked your work in dev-branch and see you are coding the missing parts of it. This is so valuable work.



In this point, I have some questions to you. In the original version also turbulence equations were missing. I know for hypersonic flow laminar approach solves the most of the problems, but I mostly interested in species transport and finite rate chemistry (also Eddy-Dissipation models) for internal flows and consequently one-temperature model. I am trying to add these features to old (first version) but I just wonder is there a plan to expand work out of two-temperature and nemo models ie. to more generic reaction mechanisms and internal flows?


There are too much people lately asking for usability of SU2 into generic combustion problems? If someone enlighten me/public, i will be glad.

Originally Posted by CatarinaGarbacz

Hello Gabriel,

I am actually one of the people who is currently developing this code. You're right that the old TNE2 solver is nnow called NEMO, and that it is not yet available in the latest master version or the develop branch.

There's a feature_NEMO branch in SU2. I cannot guarantee you this version is working a 100%, but you can try and run some test-cases with it to start getting familiar.

The work I'm doing at the moment is updating feature_NEMO to the develop branch to release it there. We expect to have this ready wihin the next 1 (max 2) months.

Hope this helps to clarify your question. Let me know if there any way I can help.

Best,
Catarina

[GAB_STO]

Hello Catarina,

I’ve tried the feature_NEMO branch that you refer to in your post. It worked great!

I was able to successfully launch the two wedge test cases in inviscid and viscous flow.

I’m wondering if both of those cases were linked to any available study or article?

I’m also wondering if there is going to be any publication in the literature about the development of the NEMO solver?

Thank for answering my questions!

Gabriel

[CatarinaGarbacz]

Hi Catarina,


I appreciate your work, in the original (first) version of NEMO solver named SU2-feature_AdjTNE2, there were some missing points such as boundary conditions, which are only applied for far-field and walls. The pressure outlet, mass flow inlet and pressure inlets were missing. I checked your work in dev-branch and see you are coding the missing parts of it. This is so valuable work.



In this point, I have some questions to you. In the original version also turbulence equations were missing. I know for hypersonic flow laminar approach solves the most of the problems, but I mostly interested in species transport and finite rate chemistry (also Eddy-Dissipation models) for internal flows and consequently one-temperature model. I am trying to add these features to old (first version) but I just wonder is there a plan to expand work out of two-temperature and nemo models ie. to more generic reaction mechanisms and internal flows?


There are too much people lately asking for usability of SU2 into generic combustion problems? If someone enlighten me/public, i will be glad.

Hello there.

There might be some confusion about SU2 branches. We used to have feature_TNE2 and the corresponding adjoint solver feature_AdjTNE2. both of them were missing some parts, correct.

The work I have been doing is to bring feature_TNE2 to feature_NEMO, which consists on updating the code to develop branch (which includes some improvements in performance, amongst others), correcting several bugs that existed on previous versions, fill in those gaps (and change of name TNE2-->NEMO)

1 - Now to answer your questions. Turbulence modelling with Eddy dissipation for hypersonic flows is not there yet but it is currently being implemented by one of my colleagues.

2 - If you're intending to do this yourself and also to implement instead a 1T model, you can keep going as you are, with the older version. but given the aforementioned, ideally I would suggest you to give a look to feature_NEMO since this is the most solid version of the code so far. these developments are still currently on going, hence the branch is being constantly updated, but you can pick up commit 931e6a08ea53875c0dd57f2e2d79c64f405b0be5 which should be the most solid up to this day.

3 - extending NEMO to more generic reaction mechanisms is certainly going to happen very soon, as one of the ongoing implementation is a link with the library Mutation++, with flexibility of mixture and reaction mechanism being the main motivation. we are not specifically planning to implement a 1T model, but it is something doable with NEMO.

4 - about combustion, NEMO can do laminar finite-rate chemistry with any mechanism that is sufficiently addressed by mutation++ library. however, to model generic combustion, it would be necessary to embed a library like CANTERA, to give the extra capability of modeling complex mechanism of reactions with lots of radicals but at lower temperatures (TODO list), and also implementing TCI will allow covering turbulent combustion (TODO list)

Hope this helps!

[CatarinaGarbacz]

Hello Catarina,

I’ve tried the feature_NEMO branch that you refer to in your post. It worked great!

I was able to successfully launch the two wedge test cases in inviscid and viscous flow.

I’m wondering if both of those cases were linked to any available study or article?

I’m also wondering if there is going to be any publication in the literature about the development of the NEMO solver?

Thank for answering my questions!

Gabriel

Very happy to know you're running it successfully!

these cases are not linked to any specific article. they were picked simply for regression testing purposes. To have confindence in the results, we picked the inviscid wedge with a small angle since this can be compared to the theory of shock oblique relations (and it matches perfectly, since nonequilibrium ends up being negligible) and then we simply add the viscous effects in the other test-case, including a boundary layer.

However, as we solidify all these developments, we plan to add one or more test cases that we can fully use for validation as well.

There is indeed a publication in the NEMO solver, you can refer to https://doi.org/10.2514/6.2020-1805. the paper is not about the NEMO implementation, actually it focuses on the physics of shock interaction in nonequilibrium air and CO2 flows, but the simulations were done with the su2 TNE2/NEMO solver coupled to mutation++ (the previous version of feature_NEMO ) and you can find the equations there as well as a short description of the solver and library.

Feel free to ask any more questions!

Catarina

[hk.narahari]

Hi,
In the test cases regarding Wedge, the grid file is mentioned as "invwedge.su2", is this a different grid or the same one used in the base tutorial case viz. mesh_wedge_inv.cgns
Regards
Narahari

[hk.narahari]

Missed this point, it shows the following error " Invalid Solver option NEMO_EULER" . Is there a different File instead of the standard 7.06 ?
Regards
Narahari

[GAB_STO]

Originally Posted by hk.narahari

Missed this point, it shows the following error " Invalid Solver option NEMO_EULER" . Is there a different File instead of the standard 7.06 ?
Regards
Narahari

Hi,


As far as I know, NEMO solver as not yet been added to the master branch of SU2 witch mean that it is not on SU2 standard 7.06.



But if you want to experiment with the development code, you can clone or download the NEMO_feature branch on git hub. (https://github.com/su2code/SU2/tree/feature_NEMO)


The development code can be compile the same way as the latest version of SU2 Blackbird.


I hope that this information can help you.


Gabriel

[CatarinaGarbacz]

Originally Posted by hk.narahari

Missed this point, it shows the following error " Invalid Solver option NEMO_EULER" . Is there a different File instead of the standard 7.06 ?
Regards
Narahari

Hi Narahari,

sorry for such a late response, somehow I didn't see this.

I am one of the main developers of SU2-NEMO.

this solver is already available in the develop branch of SU2 v7. If you clone this version, SOLVER= NEMO_EULER will definitely work.


About the mesh question. The folder su2code/SU2/TestCases has an extensive list of test-cases, including the nonequilibrium/invwedge you are asking about. The SU2/TestCases does not contain any meshes by default, since these files are too big for the repository. you can find the meshes in the repo su2code/TestCases. you should clone this repo and then do:

cp -R TestCases/* SU2/TestCases/

this will copy all the meshes to your SU2 flder, in the right locations, including the invwedge.su2 mesh.

Bear in mind that the version of NEMO available in develop ony allows for simulations with AIR5 and N2. But I am currently working on making this linked to Mutation++ library, which will allow for any mixture to be simulated.

Hope this helps,
Catarina

[giovanni.medici]

Dear Catarina,

First of all thank you and the SU2 team for delivering such a great piece of software. Recently I gave a try to the NEMO implementation (taking the viscous wedge example, found in su2code/SU2/TestCases) SU2 7.1.0, and I’ve a couple of questions: KIND_TURB_MODEL is set to none, but some BC aren’t for inviscid ( MARKER_ISOTHERMAL). I understand NEMO_NAVIERSTOKES has its own way to deal with turbulence, hence I can't pick a different turbulence model, such as: SST, correct? I read in this thread that initially no viscous implementation was done, but I saw quite a lot of activity in the last SU2 releases on this topic, so maybe now things are changed.

The case runs with AIR-5 GAS_MODEL: what are the five terms of GAS_COMPOSITION referring to? Molar fraction of the components ? Where can I find some reference of the model? Probably you didn't because it is simply too obvious, but did you consider adding a comment describing that line in the cfg file ?

I understand that AIR-5 and N2 model are currently implemented, do you foresee the implementation of new/different GAS_MODEL(s) in the next future? Is the implementation of new GAS_MODEL something you expect the user to do, if so, how (like with an xml)? Maybe taking advantage of Mutationpp?

[CatarinaGarbacz]

Hello Giovanni

1. NEMO is divided in 3 different solvers, following SU2's typical structure: NEMO_EULER, NEMO_NAVIER_STOKES and NEMO_RANS.

NEMO_EULER concerns nonequilibrium inviscid simulations, with BCs like MARKER_SYMMETRY, MARKER_EULER, MARKER_OUTLET, MARKER_FARFIELD.

NEMO_NAVIER_STOKES concerns laminar viscous flow, that's why KIND_TURB_MODEL is set to none. But in laminar viscous flow you still need a wall boundary condition, therefore we aditionally have MARKER_ISOTHERMAL or MARKER_HEATFLUX

NEMO_RANS concerns turbulent viscous flow, but this is still currently in development and not available to the community.

2. the terms in GAS_COMPOSITION are referring to mass fractions. This is clarified in the config_template.cfg file of SU2, but I took your suggestion on board and will add this description also in the .cfg files of those examples (viscwedge, invwedge, thermalbaths).

3. about the models of the mixtures. There are 2 libraries to deal with thermochemistry/transport in NEMO, that you choose by setting the flag FLUID_MODEL to either:

a) SU2_NONEQ - this is the native hardcoded SU2 library that we implemented, where you have AIR-5, N2 but also ARGON.

b) MUTATIONPP - this fluid model uses mutation++ as a thermochemistry/transport library (so yes, this link it is actually already implemented in SU2 ) and since this library is much more flexible, you can provide any mixture/mechanism you want through a .xml file. For this you go to SU2/subprojects/Mutationpp/data/mixtures and SU2/subprojects/Mutationpp/data/mechanisms and you create your own custom files, following the examples already provided.

4. AIR-5 is the most standard mixture model used in hypersonic flow, and it comes from Chul Park, Review of chemical-kinetic problems of future NASA missions. I - Earth entries / Assessment of two-temperature kinetic model for ionizing air.

everything written above concerns already the version 7.1.0 of SU2. you can also check out the config_template.cfg file to clarify some of the input options.

Let me know if this was helpful and if you have any further questions

[giovanni.medici]

Dear Catarina,
thanks for the fast and comprehensive reply, I really appreciated it. I definitely missed the SU2/subprojects/Mutationpp/ folder, I'll have a look there! Thanks also for the clear and detailed summary of the NEMO options (and references) currently implemented in SU2 7.1.0, I'm sure they will help/guide the SU2 user community

[hk.narahari]

I have been wanting to try the new NEMO solver in the newest 7.1.1 SU2 version. I have used the same mesh as in repo (invwedge.su2) and made changes to the cfg file to match with the template. The codes processes the mesh starts the processes and just stops . I am not able to figure out what mistakes I have done in the cfg file . I am attaching cfg file (renamed) along with the screen dump, any suggestions would be very helpful.
Thanks in advance
Narahari

[CatarinaGarbacz]

Originally Posted by hk.narahari

I have been wanting to try the new NEMO solver in the newest 7.1.1 SU2 version. I have used the same mesh as in repo (invwedge.su2) and made changes to the cfg file to match with the template. The codes processes the mesh starts the processes and just stops . I am not able to figure out what mistakes I have done in the cfg file . I am attaching cfg file (renamed) along with the screen dump, any suggestions would be very helpful.
Thanks in advance
Narahari

Hello,

this is because you are using the option FLUID_MODEL = STANDARD_AIR which is a fluid model that corresponds to standard air as a perfect ideas gas PIG (gamma = 1.4, R = 287), which is a specific case of FLUID_MODEL = IDEAL_GAS, where you can define another game and R. both these fluid models only work with the PIG solvers, such as EULER, NAVIER_STOKES, RANS, INC_EULER, INC_NAVIER_STOKES.

for the nonequilibrium solvers NEMO_EULER, NEMO_NAVIER_STOKES, you need a nonequilibrium fluid model. 2 are available in SU2:

-USER_DEFINED_NONEQ (or SU2_NONEQ in newer versions) which is a hardcoded library in SU2 for air-5, N2, air-7 depending on the versions.
-MUTATIONPP - coupling with the Mutation++ therchemistry library. you can define your own mixture and reaction mechanism or use some already defined ones in their database

in any case, I will raise an error for this kind of situation, thanks for reaching out

Catarina

[hk.narahari]

Thanks a lot Catarina Garbacz. Have changed the CFG and it is now running ok, will update the results later ( on convergence or any other issues). Just curious, about how many iterations should it run before we see reasonable low residues ? Are the expected results (screen shot) in the directory containing the NEMO branch .
Again thanks a lot
Narahari

[CatarinaGarbacz]

Originally Posted by hk.narahari

Thanks a lot Catarina Garbacz. Have changed the CFG and it is now running ok, will update the results later ( on convergence or any other issues). Just curious, about how many iterations should it run before we see reasonable low residues ? Are the expected results (screen shot) in the directory containing the NEMO branch .
Again thanks a lot
Narahari

Hello, I don't know by heart, I would have to run the full simulation to answer the question. So I would suggest you do that, run the simulation for many iterations and keep checking the residuals and the solution from time to time, and you'll be able to see. You should expect to see an oblique shock, and you have convergence when the flowfield does not change anymore.

Not sure what you meant by the last sentence but I don't see any screenshot attached.