High Mach Number Anomalies and Convergence Issues in Hypersonic Simulations Using JST Scheme

[Bot-Enigma-0]

Describe the bug
Give a clear and concise description of what the bug is and what you expect the behaviour to be instead. Please provide enough instructions and data for a developer to reproduce the problem (config, mesh, commands, etc.). Please provide the smallest working example that reproduces the problem.

Hi all,

I posted this on the CFD forum, and one of the members mentioned it may be a bug and post it here.

I am simulating flow over an inlet at hypersonic speeds (Mach 7) in 2D using the JST scheme. I have done a mesh convergence study with an inviscid simulation and the residuals go to machine accuracy for all the meshes and works fine.

I am using the Navier-Stokes solver for the viscous simulations. I have 5 meshes (very_coarse, coarse, medium, fine, very_fine) to do a mesh convergence study. The very_coarse (VC) and coarse (C) meshes converge to a residual rho of -8.5 and -9 with Cauchy on drag = -10 orders of magnitude. The finer meshes barely converge to -4 to -5, before increasing -2 where they plateau. For all of the meshes (including the converged VC and C), there is an abnormal region with a higher Mach number at the leading edge (11 for VC and 9 for C). Following one of the discussion on the CFD forum (https://www.cfd-online.com/Forums/su2/142261-anomalous-mach-number.html), I extended the domain around the leading edge, but that had no effect on this region.

I played around with the 2nd and 4th coefficients in the scheme; the 4th coefficient has not effect on this region. Increasing 2nd coefficient smooths discontinuities, so it decreases the Mach number in those regions but its still higher than freestream. Increasing the 2nd coefficient also makes the shock resolution in the rest of the flow field very smooth (looks like a smudge on the screen).

Is there a reason why this happens? I did a few first order upwind simulations; they converge almost instantly and the higher Mach region does not exist. Nor does it exist in 2nd order upwind scheme, but these dont converge any further than -4. I want to conduct optimisation, for which the JST scheme shows good stability and convergence for adjoint problems.

I have uploaded the config file, convergence history and images of the high Mach region around the leading edge here: https://drive.google.com/drive/folders/1HtBwS9rVuWn5IJoDpMCCpRyYehOTk9by?usp=drive_link. The history file also contains information of the meshes (number of cells and y+ values). I uploaded one of the converging meshes (v_coarse.su2) and one of the diverging meshes (medium.su2).

I used WEIGHTED_LEAST_SQUARES to help with the sharp edge; this decreases the Mach in the region but not by much (~9 for the very_coarse mesh). I have also run the RANS solver with JST, but there is no significant difference from using NS with WEIGHTED_LEAST_SQUARES; the Mach number in the region 8.74.

Thank you,
RK

Bug report checklist
Please make sure that you have followed the checklist below, many common problems can be solved by:

• Consulting the build instructions (https://su2code.github.io/docs_v7/Build-SU2-Linux-MacOS/).
• Looking for similar problems on GitHub or CFD-Online (https://www.cfd-online.com/Forums/su2/).
• Updating to the newest version of SU2 (either develop, master, or the pre-built executables https://su2code.github.io/download.html).

Desktop (please complete the following information):

• OS: Linux Ubuntu 22.04 LTS (also ran on cluster and laptop)
• C++ compiler and version: gcc 11.4.0 (cluster: gcc 12.3.0)
• MPI implementation and version: OpenMPI 5.0.3
• SU2 Version: 8.0.1

[pcarruscag]

I don't think JST is ideal for hypersonic applications, I'll ask the hypersonic experts if they can take a look at your question.

[Hanquist]

I have not used JST for hypersonic applications and have stuck primarily with Roe, MSW, or AUSM varieties.

[Bot-Enigma-0]

Hi,

In the past few days I've been running some AUSM+UP2 and SLAU2 cases, based on a paper which showed good accuracy compared to experimental data for hypersonic conditions . For the very_coarse and coarse meshes, both converge to -5 rho residual with a cauchy of -8 on drag, but the finer meshes don't converge at all.

SLAU2 (with ROE_LOW_DISSIPATION=NTS_DUCROS) is quick to converge, and allows cauchy to go to -10. But the lift and drag coefficients are larger compared to JST, ROE, HLLC or AUSM+UP2.
AUSM+UP2 is slower to converge and when cauchy is set to anything lower than -8, it start to diverge. Do you have any tips for better convergence? I have uploaded the configs to the link above.

Thanks,
RK

[pcarruscag]

Are you initializing the fine meshes from the coarse ones?
There is the ACCURATE_JACOBIAN option that may help with the AUSM/SLAU schemes.

[Bot-Enigma-0]

Yes I'm refining the finer meshes from the coarse ones. I'm also using the USE_ACCURATE_FLUX_JACOBIAN = YES.

[jtneedels]

As @pcarruscag notes, JST isn't a great choice for high speed applications - I've never used a centered scheme for a hypersonic problem, but I'm not surprised issues are arising. I would recommend against using JST.

I'm surprised the finer meshes don't converge - when you say the "Cauchy is set to anything less than -8 it starts to diverge", you mean if you run it sufficiently long it diverges? With SLAU, it may be there is insufficient numerical dissipation on the finest mesh?

I tried to open your config but it won't download. Are you using MUSCL reconstruction with limiters? If so, which limiter?

I generally find the most robust performance from the standard AUSM scheme for hypersonic problems in SU2.

[Bot-Enigma-0]

When setting the cauchy to less than -8, the solution has next to no drop in residual, and looks like it plateaus. I will upload the history of these on the drive soon. After that the solution starts to diverge. I have uploaded the config files as .txt files.

I am using MUSCL reconstruction with a Barth-Jespersen limiter. I have used VENKATAKRISHNAN with a range of coefficients up to 0.5. There is no significant difference in the results.

I will run some standard AUSM schemes and see if that works.

Thanks,
RK

[jtneedels]

Sounds good - the issues with the cauchy criterion are surprising to me. Large heat fluxes at boundaries (common in hypersonic problems) are added as residual values, and may explain the small reduction in residual even for a converged solution.

For the limiter, I've had best experience with VENKATAKRISHNAN (with the default coefficient value) and VAN_ALBADA_EDGE for high-speed problems, I would recommend against Barth-Jespersen.

[Bot-Enigma-0]

Hi,

I did a few standard AUSM runs with Barth-Jespersen on the very coarse, coarse and medium meshes. The convergence isn't much better.
I've set some runs with VENKATAKRISHNAN and VAN_ALBADA_EDGE simulations and will post the results for both here in the morning.

Thanks,
RK

[Bot-Enigma-0]

Hi,

I've did some AUSM simultions with the VENKATAKRISHNAN limiter which showed similar properties to the SLAU2 scheme with BARTH_JESPERSEN. The VAN_ALBDA_EDGE limiter diverged on all of the meshes with the AUSM scheme, so I didn't do any more runs with it. I ran the AUSM+UP2 and SLAU2 schemes with the VENKATAKRISHNAN limiter on all of the meshes. These runs showed steady convergence, but plateaued near a residual of -5, like before. The noisiness in the AUSM+UP2 scheme was notably reduced, compared to BARTH_JESPERSEN. SLAU2 and standard AUSM were stable across all of the simulations; but neither achieved residuals below -5. The medium mesh doesn't converge; it looks like the residuals are dropping but they dont. I'm running the medium mesh in the backgorund to see if the residuals drop any further, as of now it doesn't look like it.

I also looked at the shock resolution across each scheme, limiter and mesh. The AUSM+UP2 scheme shows greater smoothing compared to the other schemes, yet is noisier; this might be because of the numerical dissipation. The VENKATAKRISHNAN limiter has a more oscillations in shock resolution and is sharper than BARTH_JESPERSEN, yet shows better convergence. I find this behaviour odd, not too sure if this is meant to happen?

I turned off the CAUCHY on drag and set the convergence criteria to CONV_RESIDUAL_MINVAL= -7; which none of the simulations converge to. Something I noticed in the simulations is that the shock-shock-boundary-layer induced separation bubble at the expansion corner grows quite a bit when the simulations are let to run for a long time. The medium mesh experiences this growth quite early on which may be the reason for no convergence. The very coarse and coarse meshes see this area grow as well, but after many many more iterations. Despite refining this area, it keeps growing and is likely the cause of the no convergence. Is there any special treatment that is usually given to areas like this? Running the very_coarse simulation for a long time sees the same phenomena.

I've attached a pdf with the images for the residual history, shock resolution and separation bubbles for all of the simulations I've done.

Thanks,
RK
simulation_results.pdf