[whysoserious]

Hello!
I use converge 2.3.10 to simulate DI gas engines. When I reduce the diameter of gas nozzles while mass flow rate remains unchanged, the gas jet speed becomes very high and exceeds sound speed. As we know, when Ma >1, choke will happen near the outlet of nozzles.

In my case, the timestep declines into #e-7 which is too small to let my case finished within a reasonable time. In the time.out, the timestep is limited by dt_cfl mostly and by dt_piso occasionally.

what can I do to let myself out of such a dilemma?

Thank you for your advice~

[Blanco]

Originally Posted by whysoserious

Hello!
I use converge 2.3.10 to simulate DI gas engines. When I reduce the diameter of gas nozzles while mass flow rate remains unchanged, the gas jet speed becomes very high and exceeds sound speed. As we know, when Ma >1, choke will happen near the outlet of nozzles.

In my case, the timestep declines into #e-7 which is too small to let my case finished within a reasonable time. In the time.out, the timestep is limited by dt_cfl mostly and by dt_piso occasionally.

what can I do to let myself out of such a dilemma?

Thank you for your advice~

I think your only choice is to decrease the mesh refinement locally (increase AMR subgrid settings or fixed embedding scale, locally) in order to increase cell size and so move to bigger time-steps. This for sure will reduce your spatial resolution, but you can do a sensitivity study to assess your results, by trying different AMR/embedding settings.

Btw, are you using the total energy solver for this case? It is specifically suited for high speed flows

[whysoserious]

Originally Posted by Blanco

I think your only choice is to decrease the mesh refinement locally (increase AMR subgrid settings or fixed embedding scale, locally) in order to increase cell size and so move to bigger time-steps. This for sure will reduce your spatial resolution, but you can do a sensitivity study to assess your results, by trying different AMR/embedding settings.

Btw, are you using the total energy solver for this case? It is specifically suited for high speed flows

thank you for your advice~

From what you suggest, I need to coarsen my model mesh or use the total energy solver, right? I have two questions.

First, I have done the sensitivity study of mesh size before and found a suitable embedding strategy for my previous case. If I do this again, I need to revalidate the pressure trace and emission statistics which may be time-consuming. Alternatively, can I change Simulation Time Parameters to solve this problem?

Second, which parameter should I change to use the total energy solver? can you tell me more detail about this solver?

[Blanco]

Originally Posted by whysoserious

thank you for your advice~

From what you suggest, I need to coarsen my model mesh or use the total energy solver, right? I have two questions.

I would suggest to use the total energy solver in any case, even if you'll proceed with a fine mesh, because you're simulating flow having Ma>= 1

Originally Posted by whysoserious

thank you for your advice~

First, I have done the sensitivity study of mesh size before and found a suitable embedding strategy for my previous case. If I do this again, I need to revalidate the pressure trace and emission statistics which may be time-consuming. Alternatively, can I change Simulation Time Parameters to solve this problem?

Do you mean change the CFL_U limit? You can try to play with CFL and go above 1 for velocity, but keep in mind that you'll have to underelax to stabilize the solver (personally I've not tried to go above max CFL_U=1 yet if not in particular cases...in which I ended up going back to max CFL_U=1 because of stability).

Originally Posted by whysoserious

thank you for your advice~

Second, which parameter should I change to use the total energy solver? can you tell me more detail about this solver?

You can switch on the total energy solver by putting to 1 the solve_total_energy_flag in inputs.in. You can find more details on the total energy solver in the paragraph 4.3 of the manual (and I remember some slide in the advanced training material too, new features of v2.3).

[whysoserious]

Originally Posted by Blanco

I would suggest to use the total energy solver in any case, even if you'll proceed with a fine mesh, because you're simulating flow having Ma>= 1



Do you mean change the CFL_U limit? You can try to play with CFL and go above 1 for velocity, but keep in mind that you'll have to underelax to stabilize the solver (personally I've not tried to go above max CFL_U=1 yet if not in particular cases...in which I ended up going back to max CFL_U=1 because of stability).



You can switch on the total energy solver by putting to 1 the solve_total_energy_flag in inputs.in. You can find more details on the total energy solver in the paragraph 4.3 of the manual (and I remember some slide in the advanced training material too, new features of v2.3).

It works.
Thanks a lot

[hmzha]

Originally Posted by whysoserious

Hello!
In the time.out, the timestep is limited by dt_cfl mostly and by dt_piso occasionally.

Hi,

How did you generate time.out file? I could not find it in the manual.

Thank you

[whysoserious]

I don't know how to turn on this function. I think it may be related to software version. I am using CVG 2.3.10. What about you?

[Blanco]

If you're using linux you have to redirect converge output to a text file during the run, e.g.

converge-2.3-.... > log.out &

You can also set verbosity level in inputs.in


Sent from my HUAWEI TAG-L01 using CFD Online Forum mobile app

[MFGT]

Originally Posted by hmzha

Hi,

How did you generate time.out file? I could not find it in the manual.

Thank you

time.out was added with a certain release, but i dont know which one it was. Since then its always there, if not, your version is older.
In this case check the screen print in the log file as Blanco suggested.

You can also change the command in windows to write the text output to a file.
Simply add
> log.txt

after he command

[hmzha]

Yes you are right. I am using v2.3.6. I already have the output in a text file, just wondering why I don't have the time.out file.

Thanks

[SamWijey]

CONVERGE writes the time.out file starting from v2.3.10. Its a good idea to read the release notes from time to time to get updated on the bug fixes that has been happening.

[hmzha]

Thanks for the reply Sam. Would you recommend updating the software to the latest version each time there's a new release?

[SamWijey]

This is a good question that a lot of the people in the forum can learn from. Let me try to answer this below:

1. If you are in the middle of a project, then you should try not to upgrade the executable unless you find out that there's a bug in the version you are using, that affects your project results.
If the system you are simulating is sensitive to small perturbations, then changing the executable can result in a different (yet valid) realization of the results. This might affect your project progress if you swap the executables in the middle of the project

2. Read release notes periodically to find out the bug fixes and improvements that has been done to the code. If the bug fixes in the newer versions of the executables do not affect your project, do not change executable in the middle of the project.

3. If you are going to start a new project then this would be a good time to read the release notes to figure out if you want to upgrade the executable or not.

4. CONVERGE typically releases minor versions monthly and a major version yearly.

Hope this helps,