[LBellmann]

Hello there

I am simulation a Fan-Stage with Nacelle in a farfield using Ansys CFX. My goal is to simulate it under an angle of attack. What I did is I first did a run with no angle of attack and then wanted to initialize the next runs (with AOA) with the results of the first run. Unfortunately the next run took the boundary conditions of the one I tried to initialize with and not the ones set in CFX-Pre so there was no angle of attack seen in the Post-results.
I am running my simulations on a cluster and I start them via batch files. I also tried to change boundary conditions using CCL-files but nothing helps. Even the solver manager says that the boundary conditions are set as I want to but as I said there is nothing seen in the results.
By the way, the AOA is big enough so it should definitely make a difference.

Thanks for your time. I hope someone got an idea

[Gert-Jan]

Please share the output file. To upload it, use 'Go Advanced' below in your screen.

[LBellmann]

I've deleted the convergence history in the out-file to match the maximum data size.
In the Out-file you can see that velocity components in x and z direction were defined to create an angle of attack.

[Gert-Jan]

From an output file it is difficult to completely understand what you are doing.

But I see an angle on OUTLET_FF
And on INLET_FF I read

FLOW DIRECTION:
Option = Normal to Boundary Condition
END

Shouldn't that have an angle of attack?
Bottomline: How does your file CCL_15deg.ccl look like?

[LBellmann]

I've set an Total Pressure boundary condition at the inlet to make the convergence more stable. In previous simulations I've seen that the incoming flow in the farfield quickly turns over to an angle so that shouldn't be the problem.

The CCL files looks like:

FLOW: Flow Analysis 1
DOMAIN: FERNFELD
&replace BOUNDARY: OUTLET_FF
Boundary Type = OUTLET
Location = OUTLET_FF,OUTLET_FF 2
BOUNDARY CONDITIONS:
FLOW REGIME:
Option = Subsonic
END
MASS AND MOMENTUM:
Option = Cartesian Velocity Components
U = 14.489 [m s^-1]
V = 0 [m s^-1]
W = 3.882 [m s^-1]
END
END
END
END
END

FLOW: Flow Analysis 1
DOMAIN: TONNE
&replace BOUNDARY: OUTLET_TONNE
Boundary Type = OUTLET
Location = TONNE_OUTLET,TONNE_OUTLET 2
BOUNDARY CONDITIONS:
FLOW REGIME:
Option = Subsonic
END
MASS AND MOMENTUM:
Option = Cartesian Velocity Components
U = 14.489 [m s^-1]
V = 0 [m s^-1]
W = 3.882 [m s^-1]
END
END
END
END
END

FLOW: Flow Analysis 1
&replace SOLVER CONTROL:
Turbulence Numerics = High Resolution
ADVECTION SCHEME:
Option = High Resolution
END
CONVERGENCE CONTROL:
Local Timescale Factor = Timescale
Maximum Number of Iterations = 4000
Minimum Number of Iterations = 1
Timescale Control = Local Timescale Factor
END
CONVERGENCE CRITERIA:
Residual Target = 1e-06
Residual Type = RMS
END
DYNAMIC MODEL CONTROL:
Global Dynamic Model Control = On
END
END
END

[Gert-Jan]

I don't know how your geometry looks like. Therefore I can't tell if things work the same on different simulations. So I think the normal direction on your inlet is the problem.

[Opaque]

I will second the Gert-Jan, from the settings w/o seeing the geometry of your model, the red flag seems to be the "Normal to Boundary Condition" setting.

From your output file, something else called my attention and it is the use of Local Timescale Factor. I have used Ansys CFX for 20+ years, and it is rare to use Local Timescale Factor except for some extreme cases. Wonder what kind of flow condition/mesh issues you are dealing with

[LBellmann]

The Total Pressure condition is defined not the problem. I‘m dealing with the problem that a simulation which was initiated by anothers result file (same geometry/ mesh) does not run with specified boundary conditions (specified via def-file or CCL-file). It runs with exactly the same conditions as the previous run which generated the result-file I‘m initializing with. Even if I change the Inlet form one surface to another one it does not overwrite the boundary conditions of the old run.

[LBellmann]

I‘m simulating a fan-stage with all passages. In order to do that I chose local timescale because Autotimescale and physical timescale did not lead to a stable convergence. The variable „Timescale“ which is called in the CCL-file is just a user-function I created in CFC-Pre
To be honest I can’t really tell why it’s running on local timescale the best

[Opaque]

I have reused previous calculations as the initial guess for new calculations and I have never seen this problem. Wonder if you have frozen something.

Auto Timescale is an auto-computed physical timescale; however, the Local Timescale Factor is NOT a physical timescale (note it is dimensionless), and it can lead to frozen convergence and unphysical solutions.

I would restart the solution with standard Auto Timescale and verify it is working, i.e. using the new conditions. Then, you can try your approach to make converge at your will.