Learning Forum

[polmartorell]

Hi,

I am doing a project in which I need to analyze some airfoils at high speed (M 0.88) at a high altitude (51000 ft). I wanted to compare the results between the Spalart-Allmaras model and the SST k-w, which, if I understood correctly, are the right models for high-speed external flows. I am using ANSYS 2019 R1.

I have had no problem setting up the Spalart-Allmaras solver and the results I get are coherent. But when it comes to the SST k-w I am not able to prevent the solution from entering in ressonance, it looks like the averaged value would be correct but the solution does not converge. What are the setup options I should use for these transonic simulations?

Thanks in advance,

Pol

EDIT: I am analyzing a NACA 0012 at 0º. I am expecting a CD of around 0.08 to 0.1 (due to the shock waves) and a CL value of 0, as it is a symmetrical airfoil at 0º.

[Amine Ben Hadj Ali]

Using coupled solver with pseudo-transient might help if not already deployed. You can work on tweaking URF's. How are the residuals and monitor plots looking?

[polmartorell]

Thanks Amine for your answer. The residuals and monitor plots look like this (I only plotted 300 iterations but it goes on an on forever):

 

How should I set up the pseudo-transient method? I have found some information and done a couple of tweaks to the setup but it is still not converging. I've played a little bit with the URF's, but same, still not converging.

Thanks again,

 

Pol

[Karthik Remella]

Hello,

Change the pressure-velocity coupling to 'Coupled' and then you should be able to select 'Pseudo-Transient' option at the bottom. Try to reduce the Fluid Time Scale factor under 'Run Calculation' to see if your residuals go down.

Thanks.

Best,

Karthik

 

[polmartorell]

Thank you Karthik.

I shoud specify, which I forgot before, that I am analyzing a NACA 0012 at M0.88, so I am expecting a 0 lift coefficient and a fairly large drag coefficient (0.08-0.1 or so due to the shock waves).

The coupled solver was already selected, as well as the pseudo-transient option. I tried a timescale factor of up to 0.0001 and it does not converge either, the residuals do the same as in the pictures before, with less error (the residuals go down) but still in ressonance.

This is my setup:

Solver type: pressure-based

Time: steady

Models:    Enegy: ON

                 Viscous: SST k-omega (with production limiter (default) and compressibility effects options)

Material: Air: Density: ideal-gas

                     Cp: constant

                     Thermal conductivity: constant

                     Viscosity: sutherland

Boundary conditions: Operating pressure: 11053 Pa (pressure at 51000 ft) (operating conditions)

                                   Gauge pressure: 0 Pa

                                   Mach number: 0.88

                                   Temperature: 216.65 K (temperature at 51000 ft)

Methods:  Coupled (everything on second order)

                 Pseudo-transient option is checked

Controls: as default

Initialization: Standard: from pressure_far_field

Calcuation:    Time step method: automatic

                     Timescale factor: 0.01

All the optons not mentioned are left as default

The results are these:

The residuals do go down, but it is still not coonverging. What am I doing wrong?

 

 

[Amine Ben Hadj Ali]

Run longer at first.

[polmartorell]

Which setup? I ran the first one for 5000 iterations and it just goes on like this. The second one I did it only for 1000 but it doesn't seem to be going on the right direction.

[Amine Ben Hadj Ali]

The one with better residual till 1000 iterations. I do not like to start tuning turbulence parameters here. Just run longer and if it is still not showing the right trend we can then try with the density based solver.

[polmartorell]

I run the last case for 10.000 iterations and it stopped calculating at the iteration 8696. I guess it converged after all. These are the residuals and monitor plots:

Whilst the CD and CM plots seem to have converged, the CL still makes me uncomfortable. Furthermore, the CM value makes no sense at all, if the lt is so small (-0.00033), how can the CM value be so big (-0.246626)?

The values in which de CL (-0.00033) is oscilating are very close to the real solution which I was expecting (0) and so are the values of the CD (0.07515), both almost identical to the ones obtained with the Spalart-Allmaras model (0.00105 and 0.07496 respectively)

Thanks,

Pol

PS: I also attached the CP vs chord plot, it shows what t should show, as it is a symmetrical airfoil at a null angle of attack, both the upper and lower CP are identical throughout the length of the airfoil.

[Karthik Remella]

Hello,

Please reduce your convergence criteria (redisual values) and run your simulation longer. A deeper convergence might help stabilize your C_l.

Thanks.

Best,

Karthik

[varunT]

[varunT]

Hi

I am currently working on a thermal manikin which is enclosed in a Climate chamber for constant temperature. And the manikin is heated up to see the air flow from the head. So to visulaize it, I am working on Ansys CFD, and I am stuck with choosing the required Parameters in fluent. Can any please help me.

Thanks in advance