[Daaman]

I am simulating flow over a 6-blade propeller and modeling 1/6th of the domain with an assumption that it is axisymmetric. I meshed the computational domain generating an unstructured grid using ANSYS Meshing with a targetted y+<1 and simulated the case using Fluent with Pressure-based S-A turbulence model. It is a steady-state simulation and used a frozen rotor approach. Fluent converged after the reduction of continuity residuals by four orders of magnitude.

For simulating the domain in SU2, I had converted the mesh into CGNS format, used the .cgns file and configuration file with similar settings using SU2's RANS Solver (S-A) with rotating domain and periodic boundary conditions. After 50k iterations, the SU2 simulations have achieved a reduction of RMS residuals of four orders of magnitude as well, but the y+ value tends to be around ~ 450 and is increasing steadily after every 250 iterations. ANSYS Fluent predicts y+<1. Similarly, the pressure distribution over the surface is overpredicted by SU2 on comparing it with ANSYS Fluent's results. I assume that the convergence has been achieved as the residuals haven't reduced any further for past 2k iterations and are oscillating around similar values. I'm wondering what might have caused the overprediction of the results, especially relatively high y+ values by SU2 while the same mesh was used for the two simulations.

I am new to SU2, and your inputs/suggestions are most welcomed.

[pcg]

Attach your config file and the screen output of the code please.
Such a large difference in y+ suggests scaling issues.

[atelcikti1]

Comparing results with fluent density based ausm/roe solver is more consistent.

[Daaman]

Originally Posted by pcg

Attach your config file and the screen output of the code please.
Such a large difference in y+ suggests scaling issues.

Thanks for the reply pcg. These are the files from a different latest simulation I performed using a finer grid, although y+ value reduces but stays in the range of ~ 400. The resulting skin friction coefficient differs as well.

[Daaman]

Originally Posted by atelcikti1

Comparing results with fluent density based ausm/roe solver is more consistent.

The reason I chose pressure-based solver was the low inlet Mach for my case ~ 0.08 and max tip Mach is around 0.3, inclusive of the effect of induced velocities. But, I think I would still like to give density-based solver a try.

[pcg]

I find it odd that you need to specify boundary conditions for GEOM_1_2_SOLID, make sure the flow is not doing anything strange around that region, like encountering a wall.
Is it really an internal boundary? Or something that was not named correctly, etc.

Also I would not use Inlets and outlets together with a farfield boundary, either make everything farfied, or if the domain looks like a cylinder, specify the outer boundary as a slip wall.

From the computed volumes / areas you do not have a scaling problem.

[Daaman]

Originally Posted by pcg

I find it odd that you need to specify boundary conditions for GEOM_1_2_SOLID, make sure the flow is not doing anything strange around that region, like encountering a wall.
Is it really an internal boundary? Or something that was not named correctly, etc.

Also I would not use Inlets and outlets together with a farfield boundary, either make everything farfied, or if the domain looks like a cylinder, specify the outer boundary as a slip wall.

From the computed volumes / areas you do not have a scaling problem.

The whole domain is divided into two- Far-field (GEOM_1_1) and near-field (GEOM_1_2) for the purpose of meshing. The mesh in the nearfield domain comprises propeller geometry and flowfield of interest, thus much finer grid as compared to the farfield domain. The ANSYS Meshing generates the boundary between the two domains and acts as an internal boundary. Therefore, I assigned it as an internal BC in the config, as Fluent does. But, it doesn't affect the flowfield in any way as per the one computed by SU2.

It can be considered as a cylinder as I am modeling 1/6th of the domain (60° sector) and will be using periodic boundary conditions. Any reason why inlet and outlet pressure shouldn't be recommended to be used with farfield? I can try to run with the slip wall.

[Daaman]

Can there be an issue with the preprocessing of the mesh by the solver, because the high values of y+ are predominantly found near the root of the propeller blade and spinner junction wrt to the geometry, which is so to say at a 'sharp angle'? There is also a huge difference in the values of thrust and torque, as compared to the experimental & Fluent results for the similar settings.

[pdp.aero]

Originally Posted by Daaman

I am simulating flow over a 6-blade propeller and modeling 1/6th of the domain with an assumption that it is axisymmetric. I meshed the computational domain generating an unstructured grid using ANSYS Meshing with a targetted y+<1 and simulated the case using Fluent with Pressure-based S-A turbulence model. It is a steady-state simulation and used a frozen rotor approach. Fluent converged after the reduction of continuity residuals by four orders of magnitude.

For simulating the domain in SU2, I had converted the mesh into CGNS format, used the .cgns file and configuration file with similar settings using SU2's RANS Solver (S-A) with rotating domain and periodic boundary conditions. After 50k iterations, the SU2 simulations have achieved a reduction of RMS residuals of four orders of magnitude as well, but the y+ value tends to be around ~ 450 and is increasing steadily after every 250 iterations. ANSYS Fluent predicts y+<1. Similarly, the pressure distribution over the surface is overpredicted by SU2 on comparing it with ANSYS Fluent's results. I assume that the convergence has been achieved as the residuals haven't reduced any further for past 2k iterations and are oscillating around similar values. I'm wondering what might have caused the overprediction of the results, especially relatively high y+ values by SU2 while the same mesh was used for the two simulations.

I am new to SU2, and your inputs/suggestions are most welcomed.

I guess the over prediction is because of order of your solution. Makes your converged solution in SU2 is second order accurate in case in fluent you go for second order for pressure, momentum and turbulence.

In SU2 you should make sure that whatever numerical method you pick despite the slope limiter converges to the second order. To explore this idea you may run your fluent case with first order accuracy and then compare the solution with your over predicted SU2 solution to see if they agree. If they do then make sure when you go for 2nd order, they both converge.