Help diagnosing mismatch in results using SST and LM transition models

[EngJamal2023]

I’m working on a 2D airfoil RANS case in SU2 and I’m having trouble reproducing the same aerodynamic results I get from other software (Fluent/CFD) and from wind-tunnel data, but only when I use the SST (k\text{-}\omega) turbulence model or the LM transition model.

With the other code I can match lift/drag more closely, but in SU2 the calculated lift and drag don’t line up, and I’m not sure which parameter is driving the difference. I have already tried changing many settings, so I would really appreciate guidance on what to check first.

Below is what I’m doing now.

1. Case setup

• Solver: RANS

• Turbulence model: KIND_TURB_MODEL = SST

• Sometimes I also try KIND_TRANS_MODEL = LM

• Flow conditions:

  • Mach = 0.3
  • AoA = 7.104°
  • (T_\infty = 288.15\ \text{K})
  • (p_\infty = 101325\ \text{Pa})
  • Reynolds number = (6\times 10^6), reference length = 1.0

I’ll attach the full .cfg file I’m using (copy below).

---

2. Mesh

• I generated both a C-type mesh and an O-type mesh around the airfoil.
• First-layer height was computed to achieve the proper (y^+) for SST.
• Growth rate is ~1.05.
• Farfield is sufficiently far.
• SU2 does not report mesh-quality issues.
• So I don’t think the problem is mesh-related.

I can attach both meshes if that helps.

---

3. Things I have already tried

• Switched between MARKER_FAR and explicit inlet/outlet BCs.

• Varied freestream turbulence intensity and turbulence-to-laminar viscosity ratio:

  • FREESTREAM_TURBULENCEINTENSITY = 0.0005
  • FREESTREAM_TURB2LAMVISCRATIO = 0.1

• Tried different convective schemes: JST, ROE.

• Used multigrid with different settings.

• Changed CFL and enabled CFL_ADAPT.

• Adjusted linear solver options (FGMRES, LU_SGS, tolerance).

• Ran for many iterations (up to 50,000).

Despite all of this, the SU2 lift/drag is still not matching what I get from the other solver or what I expect from the tunnel data.

---

4. What I need help with

Could you help me understand which SU2 settings are most sensitive when using:

1. SST (k\text{-}\omega) and
2. The LM transition model

for an external-aero airfoil case at (Re = 6 \times 10^6)?

In particular, I would appreciate guidance on:

1. Freestream turbulence specification

   • Are my values for FREESTREAM_TURBULENCEINTENSITY and FREESTREAM_TURB2LAMVISCRATIO too low for this Reynolds number when using SST?
   • Is there a recommended pair of values for a case like this to match typical wind-tunnel conditions (say 0.5–1% Tu)?

2. BC choice: farfield vs inlet/outlet

   • For low-Mach external aero in SU2, is it better to keep MARKER_FAR instead of total-pressure/total-temperature inlet + static outlet?
   • Could that be affecting the pressure distribution enough to change lift?

3. Transition model coupling (LM)

   • Are there extra variables or recommended defaults for LM in SU2 that I may be missing?
   • Do you have a reference example for “airfoil, high Re, external, with LM” that I can mirror?

4. Turbulence model options for SST

   • I noticed there is an option like SST_OPTIONS = V2003m (commented in my file). For this type of case, should this be enabled?

5. Numerical scheme influence

   • Is JST with these limiter settings appropriate for this laminar-to-turbulent/transition-sensitive problem, or do you recommend a different convective flux / limiter combination to avoid excessive dissipation in the boundary layer?

If you can point me to the SU2 example or a “canonical” config for an airfoil with SST (and especially SST + transition) at this Reynolds number, I can start from that and incrementally change things until I see where my setup diverges.

---

5. My current config (for reference)

(I will also attach it as a file.)

DU_91_W2_250_comp.dat.txt

---

Thank you very much for your time and for SU2. Please let me know if you need:

• the mesh files (C-type and O-type),
• the surface Cp/forces I’m getting in SU2,
• or the reference results from the other software.
  otype_mesh.txt

Best regards,

[EngJamal2023]

log.txt
the log out file during cfd calculation

[bigfooted]

can you dump some figures here showing lift and drag from SU2, the other codes and experimental data?
We have some results here which look OK, so it might be just some configuration option or maybe scaling in the mesh?
https://www.researchgate.net/publication/388934584_SU2_results_for_the_Fifth_High_Lift_Prediction_Workshop

[EngJamal2023]

can you dump some figures here showing lift and drag from SU2, the other codes and experimental data? We have some results here which look OK, so it might be just some configuration option or maybe scaling in the mesh? https://www.researchgate.net/publication/388934584_SU2_results_for_the_Fifth_High_Lift_Prediction_Workshop

configuration file.txt

output su2.txt

Thank you for your fast and helpful reply.My goal is to validate SU2 against experimental data at AoA = 7° and M ≈ 0.30 using an O-type mesh and then refine the setup for accurate prediction.

Case summary

• Flow condition: AoA = 7°, M ≈ 0.30
• Model: SOLVER = RANS, KIND_TURB_MODEL = SST (no transition model in this run)
• Freestream turbulence: FREESTREAM_TURBULENCEINTENSITY = 0.0015
• Turbulent-to-laminar viscosity ratio: FREESTREAM_TURB2LAMVISCRATIO = 0.1
• Mesh: O-type, second-order (“O2”); I will attach the mesh and key metrics (domain size, first-cell height/y⁺, growth rate).
• Boundary conditions: airfoil wall (adiabatic heat flux = 0) and farfield.
• Numerics/time stepping: CFL_NUMBER ≈ 5, CFL_ADAPT = YES with parameters (0.5, 1.5, 1.0, 50.0).
• Iterations: ITER = 50000.
• Linear solver: LINEAR_SOLVER = FGMRES, LINEAR_SOLVER_PREC = LU_SGS, LINEAR_SOLVER_ERROR = 1E-6.
• Multigrid: not used (MGLEVEL = 0).

What I will attach

1. Lift/drag history (traces) from SU2 for this case.
2. Experimental data at AoA = 7°, M ≈ 0.3 (figure/table); I can also attach the paper if helpful.
3. Comparison result from another CFD code for the same condition.
4. O-type mesh and a short note on mesh details.
5. SU2 configuration file used for the run.

Where I’d appreciate guidance

1. Freestream turbulence settings: Are FREESTREAM_TURBULENCEINTENSITY = 0.0015 and FREESTREAM_TURB2LAMVISCRATIO = 0.1 appropriate at M ≈ 0.3 for SST on an airfoil, or do you recommend different values to better match experiments?
2. CFL adaptation: Are the bounds (0.5, 1.5, 1.0, 50.0) sensible for steady RANS SST at these conditions, or should I adjust them for improved stability/convergence?
3. Mesh best practices (O-type): Recommended y⁺ target / first-cell height, outer boundary distance, and growth rate to align with wind-tunnel data?
4. Numerical choices: Preferences for convective flux (e.g., ROE vs JST), gradient reconstruction (WLSQ vs Green–Gauss), and limiters for accurate but robust SST results in this regime?
5. Transition (future step): After the baseline (no-transition) is validated, any recommended LM/γ–Re_θ settings and freestream parameters for adding laminar–turbulent transition at M ≈ 0.3?

My aim is to reproduce the experimental point at AoA = 7°, M ≈ 0.3 with SU2 using the O-type mesh, and then proceed to a transition-enabled validation. Any corrections or recommended settings would be greatly appreciated.

Thank you again for your time and support.

[bigfooted]

Freestream turbulence settings: Are FREESTREAM_TURBULENCEINTENSITY = 0.0015 and FREESTREAM_TURB2LAMVISCRATIO = 0.1 appropriate at M ≈ 0.3 for SST on an airfoil, or do you recommend different values to better match experiments?

How fast are your simulations? Increase the values by a factor of 10 and see. It might be sensitive to the freestream.

CFL adaptation: Are the bounds (0.5, 1.5, 1.0, 50.0) sensible for steady RANS SST at these conditions, or should I adjust them for improved stability/convergence?

You can print AVG_CFL to screen to inspect if it reached CFL=50, and if CFL jumps around a lot or not.

Mesh best practices (O-type): Recommended y⁺ target / first-cell height, outer boundary distance, and growth rate to align with wind-tunnel data?

Recommendation is y+ < 1. y+=1 is really the upper limit, not a safe value. If the growth rate is not too high it should be sufficient to capture the boundary layer correctly

Numerical choices: Preferences for convective flux (e.g., ROE vs JST), gradient reconstruction (WLSQ vs Green–Gauss), and limiters for accurate but robust SST results in this regime?

For quad cells, WLSQ is reported to be a better choice. If ROE or JST is really better in general or even for this testcase, I dare not say.

Transition (future step): After the baseline (no-transition) is validated, any recommended LM/γ–Re_θ settings and freestream parameters for adding laminar–turbulent transition at M ≈ 0.3?

I'll leave this for the experts to answer:-)

[bigfooted]

got it — here’s a clean, academic message you can post on GitHub or email to the SU2 developer for this separate CFD-only case (no adjoint, O-type mesh only).

LOL

[sun5k]

Hi @EngJamal2023

I don't see anything unusual in your configuration file settings.
However, the significant difference in the lift coefficient is interesting.

The image below shows the comparison results between Fluent, OpenFOAM, and SU2.

NLF-0416
*The NLF-0416 mesh wasn't generated by me; it was downloaded from AVT-313.

S809

As you can see, although the transition onset location differs slightly, the differences in the aerodynamic coefficients aren't as large as in the your results.

Here is the configuration file and mesh that I used.
LM_Model.zip

[EngJamal2023]

Hi @EngJamal2023

I don't see anything unusual in your configuration file settings. However, the significant difference in the lift coefficient is interesting.

The image below shows the comparison results between Fluent, OpenFOAM, and SU2.

NLF-0416 *The NLF-0416 mesh wasn't generated by me; it was downloaded from AVT-313.

S809 As you can see, although the transition onset location differs slightly, the differences in the aerodynamic coefficients aren't as large as in the your results.

Here is the configuration file and mesh that I used. LM_Model.zip

As per your earlier suggestions, I have implemented the model and made some modifications to the code. I have attached the files showing the mesh and some of the cases that you have used in the past with the transition turbulent model.

Here is a summary of what I have done:

I used the same mesh as yours, with a few small changes.

I modified the convergence criteria (setting the residual to -10) and increased the inner iteration count to 50,000. However, after running 50,000 iterations, the minimum residual value only reached -5 (half of the target), and it did not converge to -10 as expected.

I set the Mach number to 0.3 and the angle of attack to 7.104.

I changed the fluid model to Standard Air but kept the rest of the settings the same as you suggested.

For the boundary conditions, I adjusted the heat flux marker to airfoil and used inlet and outlet markers. I also reduced the CFL number because, with the original value, the solution failed to converge and generated errors. I will attach the error log as well.

Despite these adjustments, the simulation is still not converging as expected. I have attached the code I am using and the simulation results for your review. I would greatly appreciate it if you could help me figure out what might be causing this issue and suggest any further adjustments that could resolve the problem.

Additionally, I have a few specific questions and would appreciate your guidance:

Convective Numerical Method: Should I change the convective numerical method from L2ROE to GST (Jameson-Schmidt-Turkel)? I’m considering this change to see if it improves convergence and avoids instability in the left and right coefficients, as they are currently oscillating. Do you recommend this adjustment, or is there a better approach?

Monotonic Upwind Scheme: For the Monotonic Upwind Scheme for Conservation Laws (MUSCL), I currently have MUSCL_FLOW = YES and MUSCL_TURB = YES. Do you think changing these values to NO could improve the results, especially in terms of stability and convergence? Or is it better to keep them enabled?

Other Suggestions: Based on your experience, are there any other adjustments I should consider to get more accurate results? For example, should I consider any changes in the mesh, boundary conditions, or other numerical methods that might help with the convergence and stability of the solution?

I have changed the mesh now and will follow any suggestions you have. I greatly appreciate your help, and I look forward to your feedback.

Thank you so much for your time and your fast replies. I truly appreciate all the guidance and support you’ve given me so far.

LMmodelMycase.zip

Thank you for your time and support. I look forward to hearing from you.

[fomistul-cfd]

What is the results that you want to match? If you want to match the stall, the Transition model is not intended for that, for matching stall of an airfoil the best shot is LES or DES simulation that require a lot of computational power. The Transitional Model main goal was to correct the overprediction of drag for low Re cases where laminar flow zone is significant. As shown in this article https://www.mdpi.com/1996-1073/14/24/8224 ( page 10) the Drag and Stall point does not match Experimental data for SST-LM, with drag being overpredicted. If you want to match Fluent data to SU2 data then it will be better to include the desired value of CL and CD given by Fluent. And as a side note, don't ever use ChatGPT for technical advice, the more niche is your question the dumber it is and will hallucinate a lot.

[rois1995]

I think this should be moved to a discussion rather than an issue. Moreover, there is too much to follow and too many images to look at. We haven't seen any Fluent results until now. Are the Fluent results yours, or are they taken from a paper? And please, keep the answers concise and clear.