[hokhay]

Hi all,

I am try to simulate a wing subject to 63m/s flow at 10 degrees of angle of attack. The wing is placed horizontally inside a rectangular domain and the flow is coming from left and bottom (lowerWall) face with a velocity component of (62 0 11). The right and top face (upperWall) is set to be outlet. The p and U boundary conditions are presented below:

P

inlet
{
type fixedValue;
value $internalField;
}

outlet
{
type fixedValue;
value $internalField;
}

upperWall
{
type fixedValue;
value $internalField;
}

lowerWall
{
type fixedValue;
value $internalField;
}

U

outlet
{
type fixedValue;
inletValue uniform (0 0 0);
value $internalField;
}

upperWall
{
type fixedValue;
inletValue uniform (0 0 0);
value $internalField;
}

inlet
{
type fixedValue;
value $internalField;
}

lowerWall
{
type fixedValue;
value $internalField;
}

However after 100 iteration, the solution has no sign of convergence. The field is not reasonable. The problem should be with the B.C. but I don't know what should be used. After running potentialFoam, the result shows velocity at the corner where inlet and outlet meet is very high. Could anyone can provide solution for correct B.C. to me please?

Thank you very much

[elones]

Hi, look at freestream boundary condition.

[hokhay]

Originally Posted by elones

Hi, look at freestream boundary condition.

Thanks for your advice. It works well now

[Joshua14]

A few questions to consider.
1) What is your Reynolds number?
2) What solver are you using? (steady or transient)
3) How large is your domain compared to your wing.

All these things will effect your results. My first reaction is that you should not be seeing convergence in only 100 iteration, especially at a near stall angle (guessing as I don't know the airfoil).

Another is that if your domain is not large enough that you will experience wall effect that will distort your flow field around the wing, depending on boundary conditions.

Also, at times the flow may be unsteady meaning a transient solver should be used. A steady solver will still work but you will get different answers depending on the case.

These are just things to consider as you move forward with your simulations in modelling your wing.

Joshua

[hokhay]

Thank you very much for your useful reply Joshua.

My case Reynolds is 2 millions and I am using steady state solver (simpleFoam). You are right, the residuals keep osillating at high error level. I see vortex generating from the leading edge of the wing. I should switch to transient solver.

My domain side walls are connected with both ends of the wing and assign with symmetry B.C. I actually not quite confident with these B.C. Please correct me if I am wrong. The top and bottom wall are 5 times the chord length away from the wing centre.

Looking for forward to some advice

Thank you

Sent from my LG-H818 using CFD Online Forum mobile app

[juliom]

Why are you using so little iterations ? Is there any evidence suggesting that your solution will reach a numerical solution at 100?. I always suggest to use transient approach. The steady approach is more stiff from a mathematical perspective. The transient solver helps to solve problem whose mathematical behavior is stiff. I always, aleays use transient approach

[Joshua14]

Originally Posted by hokhay

Thank you very much for your useful reply Joshua.

My case Reynolds is 2 millions and I am using steady state solver (simpleFoam). You are right, the residuals keep osillating at high error level. I see vortex generating from the leading edge of the wing. I should switch to transient solver.

My domain side walls are connected with both ends of the wing and assign with symmetry B.C. I actually not quite confident with these B.C. Please correct me if I am wrong. The top and bottom wall are 5 times the chord length away from the wing centre.

Looking for forward to some advice

Thank you

Sent from my LG-H818 using CFD Online Forum mobile app

If you are seeing vorticies being generated then you should definitely be using a transient solver.

As far as your domain, one symmetry plane is okay, but if you are trying to simulate a full 3D wing then you need to allow for wing tip effects. In this case you need to extend the domain out on one side of you wing (Look at previous research). You can then assign that wall a slip wall boundary condition.

The approach you are using is refereed to as infinite aspect ratio. Which ends up being a high cell count two-dimensional simulation. You are better off just doing a two-dimensional airfoil (front and back face defined as empty) or the full three-dimensional wing with wing tips exposed.

Joshua

[hokhay]

Thanks Juliom and Joshua, I think you are right that I should use transient approach for high aoa.

For the B.C., I am actually intent to do an infinite aspect ratio for this case, since the model is actually the mid section of a wing and I want to calculate the lift and drag changes when flap deploy.

Thanks for your advice on 3D wing analysis. It is very useful on my future simulations

Sent from my LG-H818 using CFD Online Forum mobile app