[ziggo]

I'm running a 3D simulation in Fluid and have found that when I change the inflow velocity direction my results are terrible.
I have a three dimensional wedge in a spherical domain. From the side it looks as in image 1. Image 1 also shows the how the domain is meshed.
This situation gives me acceptable lift and drag results w.r.t. the wind tunnel data I have.

Image 1:


When I change the inflow velocity direction the error from the CFD simulation grows w.r.t. the windtunnel data.

If I change the inflow direction for example to the direction shown in image 2 the difference between the CFD and the data is around 20%.

Image 2:



If I change the direction even more, the error becomes larger.

I define the velocity on the velocity-inlet using xyz-components. For the first image this is

x = 0, y = 0, z = -26

and for the second image this is

x = 0, y = =8.9, z = -24.4

I also make sure that Fluent calculates the CL and CD values with the correct direction vectors. So for the first image the CL components are:
[CODE]
x = 0, y = 1, z = 0
[\CODE]
And for the second image the CL components are:
[CODE]
x = 0, y = 0.94, z = -0.34
[\CODE]

How can I make sure that for every velocity direction I get reasonable results as in the situation shown in image 1? Do I need to rotate the geometry instead, re-mesh and keep the velocity parallel to the z-axis?

[flotus1]

Do you really have measurement data for arbitrary angles of attack for the wedge?
What happens if you turn the wedge instead of changing the inflow direction?
How did you validate the results for the zero AoA case? Grid dependency study performed?
Is the flow turbulent? If yes, which kind of turbulence model and wall function do you use?
How about the pressure outlet? Imagine you change the angle of attack to 90°, then only half of the geometry gets an inflow velocity which clearly doesnt correspond to an undisturbed flow. Consider a free stream boundary or a velocity BC for the whole outer boundary instead.

[ziggo]

- Yes, I have wind tunnel data for the wedge from 10 to 55 degrees of attack for every 5 degrees. Image 1 shows the 55 degree angle of attack situation.
It's actually one element of a tetrahedral kite (the image shows 4 elements). From the side it looks like a wedge.

This image show show I defined the angle of attack alfa:


- I haven't tried this yet as this means I have to re-mesh everything again. This costs more time than changing the inflow direction.

- The zero AoA case is actually the 55 degree AoA case shown in image 1. I did a grid convergence study with four different mesh sizes and found that increasing the number of cells after a certain threshold only changed my force coefficients by ~1%. So I used the threshold mesh.

- Yes the flow is turbulent. I use the standard k-epsilon model.

- The 90 degree case would indeed cause a problem, but as I will not be using that case I thought I would be OK with a pressure outlet.
I'm not familiar with other boundary conditions so I'll investigate those.

- The flow simulations for all the cases where the flow was not coming straight from the left did not converge because the residual for the continuity did not go down. Also I kept receiving messages that there was a reversed flow in ### faces. Is this maybe a pointer that I should change something?

[flotus1]

I mentioned the problem with the "90°" AoA only to make it more evident. This problem still exists with all AoA higher than 0° (55° in your case).
In fact that is why you get the messages about reversed flow at the outlet. Because for these cases, there would actually be a reversed flow at some portions of the outlet.

The solution is still the same:
Use a free stream or velocity boundary condition for the whole outer boundary.