karman vortex street help please
hi @ all,
first of all please excuse my bad english,
im an student and want to simulate the karman vortex street in 2D
the washed body is a cirle of a 4mm diameter
it flows air with and speed of 8.333 m/s or 16 m/s or 25 m/s temperture is 293 K pressure is 1 bar
for the mesh i used polyhedral and surface remesher with a base size of 5mm all other settings are standard
i tried to simulate with the k-epsilon-turbulent model everthing ist set on standard
first i simulate steady then unsteady whit the timestep and maximum physical tim depending on the velocity inner iterations are 5
there is just on problem it does not place itself a karman vortex street no vortex @ all it always looks like the picture i attached to this post
so please if any one knows my error please tell it to me
Are you sure that you set all right?
Maybe this helps you:
yep everthing all right
i use a far field
with and a inlet and a outlet and the cylinder itself
can anybody help me
im out of ideas what to change
Post your setting or a small testfile without mesh (3d testfile).
we had a small success, we were able to get an stabile karman vortex street @ 25 m/s, we are still not able to reproduce this with 16,667 m/s or 8,333 m/s and I have a another problem here
i have only access to star ccm+ @ the university
and they are close till 4-6 january so i cant post you a
testfile or a setting but i can send you our simulation @ 25 m/s in 2D its small only 5 Mb we use the same settings for 16,667 and 8,33 m/s
if you could give a look an tell me whats wrong my gratitude will be boundless
is that okay?
i cant attach it to this post becaue its a little bit to big so i have uploaded it @ rapdishare
i ziped it and now its only 1,92 Mb small
the link is
thanks for your help
of course for 16.66m/s we use the time step 0.000012 s and for 8.33 m/s we use the timestep 0.000024 s
I just had a look on your sim-file and found some points you could improve. I've tried them on my machine and it works even with 8.333m/s.
1. In my opinion, the resolution of the mesh around the antenna is too coarse. I've set a custom surface size of 1,5% (minimum and target) on the boundary antenna.
2. Use prism layers at the walls, but check the thickness after meshing. In your case, 3 prism layers with 1.25% of the base size is a good value for the prism layer thickness while the prism layer stretching was set to 1.3 (but the last is not crucial)
3. The mesh resolution in the wake of the antenna is too coarse. I've added a block shaped volumetric control to volumetric control 3 (height a little bit more than the cylinder diameter, length about 10x diameter).
4. I've decreased the diameter of the volume shape "cylinder 1", because it's not necessary to refine the mesh that far in front, above and below your body.
5. It takes some time until the vortices begin to seperate. With the settings mentioned above, it took about 0,01s simulation time until the first oscillations of the wake could be observed. You have to be patient and wait for about 400 time steps. (by the way, I set the temporal discretization to 2nd order).
6. To speed up, use less inner iterations. Usually more than 5 - 10 shouldn't be necessary, and you will improve the accuracy if you halve the time step as well as the inner iterations - while the computational effort stays the same. (In your case, you can just quarter the inner iterations and keep the time step, it will speed up the simulation).
Some of my settings will increase the cell count, but with 25 000 cells, one time step takes only 1.25 seconds on a single core of my 3,4Ghz Phenom II. So I assume, it's not critical to keep the cell count at 20 000.
There may be some better settings than mine, but it works.
Let me know if you need further help.
If you want the sim-file or the mesh, just send me a PN with your email-adress.
thanks, that will help
|All times are GMT -4. The time now is 20:20.|