Convergence problem of CFX when comparing with FLUENT with same mesh
 

Hi, all,

Thank you for reading my post. I am carrying comparison of 2D simulation between CFX and FLUENT. Results from FLUENT agrees well with experiments (residuals reduce to 3E-7). But CFX results only have residuals of 5E-5, with same mesh and setting. The lift and drag coefficients in CFX are near to FLUENT results and experimental data. But the turbulence intensity decay too fast in CFX. The intermittency have a total different distribution compared with FLUENT, with intermittency=1 in free space.
How can I reduce the residual of CFX? Why I have a different turbulence intensity and intermittency distribution in CFX?

Here is the detailed question: Validation of lift and drag for airfoil Aerospatile-A, chord=1m, attack angle=13, exterior flow, Inlet velocity=51, Re=1E7.
Mesh: size=194720, O Grid, Y+<1
Model: SST transition

FLEUNT CASE:

boundary condition
INLET: Ux=51 m/s (Uy=Uz=0), intermittency=0, turbulent intensity=0.3%, turbulent viscosity ratio=35. The left line, the top line and down line are both considered inlet.

SOLUTION METHODS

SIMPLE, Green Gauss Node Based, Second-order upwind for other discretization

The residuals and turbulence intermittency and intensity are shown in attached files. The maximum intermittency is 1, with free space intermittency=0. The intensity decay from inlet to leading edge, from 0.298% to 0.278%.

CFX CASE

In order to carry out the 2d simulation, we extruded the same 2d mesh for one element thickness, only one layer in Z direction.

Boundary condition
INLET: turbulence intermittency in GUI cannot be set. We edit in Command Editor, with specified inlet intermittency, velocity, intensity and viscosity ratio.

================================================== ========
MASS AND MOMENTUM:
Option = Cartesian Velocity Components
U = 51.46714 [m s^-1]
V = 0 [m s^-1]
W = 0 [m s^-1]
END
TRANSITIONAL INTERMITTENCY:
Intermittency = 0
Option = Value
END
TURBULENCE:
Eddy Viscosity Ratio = 35
Fractional Intensity = 0.003
Option = Intensity and Eddy Viscosity Ratio
END

==============================================
Boundary Condition for Top and Bottom surfaces in extruded mesh: Symmetric

Fluid Model
SST gamma-theta
(shown in pics)

CFX RESULTS:
only have a residual of 6e-5.

Turbulence intermittency
The Maximum is 2. For the free space, it is filled by intermittency=1.
However, in Fluent results, the maximum is 1. The free space is filled by intermittency=0. It is very strange.
(shown in attached files)

Turbulent intensity from inlet to the leading edge
Decay too fast. Only 0.13% for leading edge. While in Fluent, it is 0.278% for leading edge.
(shown in attached files)

I would appreciate if anyone can help me.

Thank you!

Not sure what your problem is. You are getting matching answers to experiment from both CFX and Fluent. Well Done!

1) You shouldnt be trying to compare residual magnitudes between codes. That is meaningless.

2) Apparently the parameter you are worried about, turbulence and intermittancy, is not a big player in on the items (Cl and Cd) you are comparing to experiment. At least not at the level of the codes predicting different values and their impact on Cl and Cd.

3) You are failing in pressure in the linear solver in CFX. Be careful.

Thank you for your reply. My question is that how can I reduce the residuals, then I can trust the results. At least 1E-6.

Yes, pressure in the linear solver sometimes failed, and U-mom, V-mom also failed. How can I solve this problem？

Thank you very much!

Do not look to residuals to "trust" your results. Are you matching experimental data or aren't you? If you are, then you're golden.

In industry, you often will not make models that drive the residuals way down. But you can make models with compromise, monitor the values you are really interested in, run the analysis to drive them to a suitable convergence, and call it good. Comparison to experimental data then tests your level of trust, not residuals.

If you insist on driving the residuals down, check your inputs and improve your mesh. One or the other is not suitable to what you are modeling to drive the residuals down to the level you want.

From the FLUENT setup it is not clear if you are using second order discretization for all the equations (including turbulence), or only mass/momentum and energy. In your CFX setup, it is explicit you are using High Resolution for all of them (including turbulence).

Are you running single or double precision ?

There are differences in how FLUENT and CFX normalize their residuals; therefore, do not focus on the exact values between the two codes, but the meaningful quantities for the problem at hand.

How much relative extrusion did you apply on the CFX setup ? That is, how thick is your 2D model respect to the characteristic length of the problem.

Thank you very much! in Fluent, I use all second order , see attached pic.

For FLUENT, it is double precision. But for CFX, it is single precision. I can try double precision later to check the difference. Does it matter so much?

For the 2D mesh, the whole domain is 100mX 120m, the airfoil in the middle is 1m chord. The thickness is 0.01m for extruded mesh. I also try 0.005m, but it doesnot change much for results.

Actually when I reduce the timescale in CFX, 0.01s, the linear solver works fine.
Maybe this is one way to avoid the failure in linear solver.