[gauthamnarayan]

I am facing a very unusual problem with the Ansys CFD post tool. I am unable to produce streamlines starting from a wing surface in the cfd post processing tool. The software attempts to calculate the streamline but simply does not produce a 3D streamline from the surface.

My guess is that there is an error in the selection of surfaces. But i have followed the same Cfd procedures on certain other geometries and it has worked for me previously. I have attached a two pictures of an experiment that has worked for me previously and the uav that I am trying to analyse for the trailing vortices generated.

It would be really great if someone can highlight my mistake in post processing. i have tried googling and asking around at a few other places and could not resolve the problem.

[ghost82]

Hi,
If you set a no slip boundary conditiom for that wall it's ok that there are no stremlines from that surface, as the velocity is zero. So, generate stremlines close to that wall, not on the wall.
In the first picture streamlines are not generated on the wing.

[gauthamnarayan]

Originally Posted by ghost82

Hi,
If you set a no slip boundary conditiom for that wall it's ok that there are no stremlines from that surface, as the velocity is zero. So, generate stremlines close to that wall, not on the wall.
In the first picture streamlines are not generated on the wing.

Hi ghost82,

Thanks for taking the time to respond to my question.

I agree that due to the no slip condition velocity streamlines cannot be released from the surface of the wing. In the case of the front wing of the racecar, I had selected the surface of the front wing, selected a forward and backward condition and ansys automatically generated the streamline for me, of course here also the walls were under the no-slip condition.

Please can you explain, what could be the possible difference in both the cases that causes the software not to release streamlines near and around the surface.

I have also attached a another photo of an Ahmed body and a car where I had got the streamlines by simply selecting the surface, which I am unable to do so in the case of the aircraft. What could be the possible reason for this. How do I generate streamlines close to the airplane wing tips so that i can visualise the developing tip vortex.

thanks,

[ghost82]

I suggest to plot contours of that surfaces to look at the velocities (absolutes): then maybe you can understand why streamlines do not propagate in your domain.
Maybe for ahme body and wing you set moving walls with the no slip condition?
What are the boundary conditions for the airplain case?

In the case of the airplain, create a xy plane in front of the wing, then if you want you can clip that surface to limit its height/width: then, release streamlines from this new surface.

[gauthamnarayan]

Originally Posted by ghost82

I suggest to plot contours of that surfaces to look at the velocities (absolutes): then maybe you can understand why streamlines do not propagate in your domain.
Maybe for ahme body and wing you set moving walls with the no slip condition?
What are the boundary conditions for the airplain case?

In the case of the airplain, create a xy plane in front of the wing, then if you want you can clip that surface to limit its height/width: then, release streamlines from this new surface.

I have tried your method. it worked.

just one more thing, i am able to limit the plane size easily through x and y dimensions, but how can I position the plane at my tips, i want to visualise only the tip vortices, i need to centre the plane on the x-y axes.

[ghost82]

Just create a small square/reactangle in front of each tip.

1- create a xy plane (location-->plane)
2- create isoclip (location-->isoclip)

In isoclip, choose the new plane and add visibility parameters (variable X --> x>=, x<=, variable Y --> y>=, y<=)

[Idiom_1]

Hello,

i got usually problem with streamlines.
Idk why it appears because i saw so plenty tutorials and noone got problem with streamlines like me. I just say what i mean:
i got closed zone object (as a fluid) with one input and one output, so between is space with water. I throw velocity on input and i would like to see flow of water by streamlines and here is the problem. Streamlines are so short, it just leave from inputp and just cut, wont show how fluid flows in output direction. Idk why, because when i see results by vectors in fluent solution, i can see there 'stream' of fluid by the other colour of points.
I relaise my problem is not so clear for sure and is possibility of many solutions, but well... i try maybe someone got any idea how can i make streamlines just from input to output, even if velocity flow between is close to 0.

Greetings