[wizards]

Hi,I am working on wings' fluid-structure interaction in CFX. When I set the v of inlet to 100m/s, the solver tell me there is a wall at the outlet. And then, I change the v of inlet to 1m/s, the error disappear and the solver works normally. So, if I want to change the v to 100m/s, I must use the opening boundary at outlet?
and another question, in the solver, the line of F CRIT goes higher and higher, is this normall?
THANKS TO EVERYBODY!

[urosgrivc]

if you use opening this will alow inflow not just outflow so the problem will go away but this might mean that your outlet is too close (if it is, it can effect your results, solution must be independant) so check if you need to move your outlet further downstream, it is also posble to wait a while this wall at an oppening might go away threw time when the flow developes but if it doesent than further examination is needed.

[wizards]

Originally Posted by urosgrivc

if you use opening this will alow inflow not just outflow so the problem will go away but this might mean that your outlet is too close (if it is, it can effect your results, solution must be independant) so check if you need to move your outlet further downstream, it is also posble to wait a while this wall at an oppening might go away threw time when the flow developes but if it doesent than further examination is needed.

thanks for your reply. Im sure that outlet is enough far. BUT I got a new question. When the v of inlet is 1m/s, solver works good, but i want to know what happens in higher speed. In this way, I changed the v to 100m/s or 200m/s, then the solver broken down, told me that its overflow. what should i do? I dont want to rebuild my model and mash... please. Hope that i can fix it easily by changing some settings.

[urosgrivc]

Hi

I think that this might be a timescale or initialization problem.
In your case I would try to ramp up the timescale.
Example; that you would use a timescale of 0.1 for the first few iterations than 0.5 and than more.
I usualy solve ramping timescale with an expression.
It can also be a mesh related problem.

And think about using some additional models in your simulation, at velocities as high as 200m/s i would include a total energy model and air ideal gas.
I am not 100%, but it should work.

For a start just set the timescale to something smaller than 1, if it works than you can solve this by ramping it up.
Be aware that if you leave it at let say constant 0.1 through the whole simulation; the simulation will converge very slowly as your domain is quite large I gues, ramping it up will lead to faster convergence but if you go too high convergence will become bouncy, I wouldnt go abbove 100 but this max number is a guess as each simulation is diferent.

Vith initialization I ment that you initalize your domain vith the same velocity as at the inlet i suspect you have a windtunel like scenario.

[ghorrocks]

Im sure that outlet is enough far (enough downstream)

How are you sure? Did you do some analysis to show it? Or does it just look a long way so you are guessing it is far enough?

The faster you go, the longer the wake. The longer the wake, the longer the domain needs to be so the wake does not hit the exit boundary. If the wake hits the exit boundary then you will get the "A WALL HAS BEEN PLACED...." warnings.

This says your exit boundary is too close for the high speed case. It should be further downstream.