[frossi]

Hi all,

I am trying to observe the von Karman effect vortex shedding over a cilynder using CFX. I am using transient simulation because vortex shedding changes over time. So, first I ran three 2D simulations, doing like specified in the documentation (extruding the geometry with the same thickness as the smallest element, etc...) and then I ran a 3D simulation as well.

First 2D simulation
RMS tolerance = 1E-4
Simulation total time = 2 s
Time step = 1E-3 s
With these conditions, i observe no vortex shedding (picture 1). So i decided I wanted to get a more accurate result, and I decreased the time step in the second simulation.


Second 2D simulation
RMS tolerance = 1E-4
Simulation total time = 2 s
Time step = 1E-4 s
When I looked at CFX post, I still see no vortex shedding (same as picture 1). Plus I get a great imbalance (almost = 1, so 100% imbalance!).


Third 2D simulation
RMS tolerance = 1E-4
Simulation total time = 2 s
Time step = started 1E-4 s, then changed to 1E-2 s after 900 iterations

When the time step was set at 1E-4 s, the RMS converged within 5-6 iterations, but the imbalance monitor showed values almost equal to 1! again almost 100% imbalance! (picture 2) How could that be? So I increased the time step size to 1E-2, and now the imbalance went almost to 0 (picture 2). How can this be? I thought that with a smaller time step you can achieve a better result because you capture the small details of the flow. Can someone explain me what happened?
After I look at CFX post, I observe vortex shedding for a small amount of time (see picture 3). Then the flow goes back to normal with no more vortices, like in picture 1. Why? I thought vortex shedding was a continuous phenomenon.


3D simulation
RMS tolerance = 1E-4
Simulation total time = 2 s
Time step = started 1E-4 s, then edited during run and changed to 2E-2 s

When the time step is 1E-4, the monitor shows imbalances oscillating from 1 to -1. Again, when i change the time step to 1E-2, the imbalances go to 0. But I still see no vortex shedding in CFX post.



I am really confused, can someone explain me what's going on please?

[ghorrocks]

Have you checked your mesh sensitivity, convergence tolerance sensitivity?

Also, what differencing scheme are you using? Both advection and time - they will both need to be second order.

[frossi]

ghorrocks, I am using a "High Resolution" advection scheme and a "Second Order Backward Euler" transient scheme. How good are these?
(my license only allows Upwind, High Resolution, and Specified Blend Factor Advection schemes, and it only allows First and Second Order Backward Euler for Transient Scheme.

My mesh is a pretty fine mesh (see picture) so I don't think it's a mesh sensitivity problem. The only thing I can think of is a domain sensitivity issue (but even if the domain is not large, I should at least be able to observe one vortex right next to the body).

My convergence tolerance is 1E-4. I know it's not optimal, but I wanted to see if I could first observe the correct phenomenon before moving to a more accurate sensitivity, like E-5 or E-6.

What confuses me is this: I can observe a little of the vortex shedding phenomenon with a higher time step, and then the phenomenon disappears.
If I reduce the timestep, I can't observe any vortex shedding at all.
Any idea of what else this could be?


Also, is my statement

I thought that with a smaller time step you can achieve a better result because you capture the small details of the flow.

correct?

Thanks

[ghorrocks]

My mesh is a pretty fine mesh (see picture) so I don't think it's a mesh sensitivity problem.

How can you say that? On what basis? Because it looks kind of fine? Unless you have really checked you are guessing - and people who guess get it wrong. I cannot count the number of times inexperienced CFD people have told me "the mesh has lots of elements so it must be fine".

In your case I am suspicious that your mesh is not fine enough in the boundary layer area and in the wake region. Make those regions finer and try again (and post an image of the mesh on the forum, please).

Your choice of High Res and second order Backward Euler should be fine. They will be sufficient.

And yes, smaller time steps should resolve more of the flow details.

[urosgrivc]

It probably goes back to (no vortex sheding) when you have increesed the timestep, now your flow details are gone (timestep too large).
1e-2 is more than 1e-4 not less, you probably see nice vortex shedding when your timestep is 1e-4 you shoul probably decreese it further to get beter convergence I dont understand why you have increesed it.
-And again what is your courant number at dt=1e-4?
Did you ever try to decrese the dt.
What is your inlet speed and diameter of the obstruction?

mesh is... well it looks so so (you were probably done in 60s), you will definitly make beter meshes when you will do this a couple of times.
-elements does not need to be that small in the farfield
-inflation can be thiner with better transition to surounding mesh
-more refined in the areas of interest less refined vhere it doesent need to be
-for a problem like this bodies of influence are a good choice...

[frossi]

Thank you guys for your answers. I'm glad you are giving me helpful corrections.

So, from what I understand, I am not doing the mesh fine enough at the boundary layer and in the wake zone.
To practice this aspect, I want to show you another simulation: flow past an inclined metal bar on a CFX 2D simulation. I apologize for switching simulation, but this one clearly show what my problem is. I believe that if I can fix this one, I could use the same tactic to tackle the flow around a cylinder.
Total time: 1 s
Time step size: 1E-4 s
inlet velocity: 80 m/s

ghorrocks, when you mentioned

In your case I am suspicious that your mesh is not fine enough in the boundary layer area and in the wake region

I realized I don't completely understand the inflation layers. I refined the elements around the bar like you suggested; then, I added 20 inflation layers, but as you can see, when the Element Quality metric is on, the quality of the inflation layers is really bad (red around the corners).

Question 1. Should I delete the inflation layers and reduce the surrounding mesh size? Or keep the small inflation layers, even though their quality is bad? I am tempted to make super small inflation layers, to capture the small boundary layer. What holds me back is the element quality of those layers (red, bad quality). Is it better to use small but bad quality inflation layers, or I replace them with normal elements of good quality (last picture)?

Question 2. Before I believed that with smaller elements I can obtain better results. Is this always true, even when the quality of the small elements is bad? Because I saw that when I make the inflation layers really small, their quality is extremely bad, because they are deformed hexa.

Question 4. Because it's a 2D simulation, I followed the documentation and extruded the geometry about the thickness of one element. But I noticed that the quality of the mesh elements depends on the thickness of the extrusion! In fact, with a very small thickness I get a bad overall mesh quality; but if I increase the thickness, the overall mesh quality improves. Does the thickness of extrusion matter? Or it's not important because it is a 2D simulation?


Question 5. When I mesh, I assess mesh quality based on: Element quality (try to get 1); Skewness (try to get between 0 and 0.25. Is it good if it's less than 0?); mesh convergence study (check the results with a finer mesh) and Domain convergence (try to expand the domain). What other mesh metric should I consider, in order to check my mesh quality?

Question 6. urosgrivc, how can I get

better transition to surounding mesh

without decreasing the overall mesh element size? If I make the farfield elements small, transition is improved. But like you said, mesh doesn't need to be that fine in the farfield. Other ideas on how to do it?

[frossi]

Question 7. If you look at my imbalance minitor for the bar simulation, you see that the plot shows an imbalance of 1 (100% imbalance). But the solver result next to it ("Normalised Imbalance Summary" highlighted in blue) reports imbalances of less than 0%. Which of the two should I look at? Which one reports the actual imbalance value? I am confused, I can't understand what the actual imbalance value is.

[ghorrocks]

Time step size - I know urosgrivc advocates manually setting the time step to get a courant number but I do not recommend this, especially for people relatively new to CFD. If you use adaptive time steps, homing in on 3-5 coeff loops per iteration then you will automatically find your proper time step with little effort from you. It also takes into account changes in convergence tolerance and when difficult numerical things (such as a vortex hits a boundary).

Inflation: Make sure the transition from the inflation layers to the bulk mesh is smooth. You cannot have a big jump in mesh size. So expand the inflation layers until they are the size of the bulk mesh so there is no size jump.

Q1: This inclined plate model has little influence from the boundary layer. So it will not matter much what you do in the inflation layers.

Q2: A good quality tet/prism mesh is better than a poor hex mesh.

Q4: See the FAQs on 2D meshes in CFX. Unfortunately CFX does not have a proper 2D so silly things like what you discuss are important.