CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   ANSYS (http://www.cfd-online.com/Forums/ansys/)
-   -   Not converging flow around cylinder with Re=1000000. Help please! (http://www.cfd-online.com/Forums/ansys/82721-not-converging-flow-around-cylinder-re-1000000-help-please.html)

Wotild December 3, 2010 10:51

Not converging flow around cylinder with Re=1000000. Help please!
 
Dear all,

I am doing my Diplomathesis with ANSYS. I need to simulate a flow around a cylinder as in the Karman vortex street. It is a 3d simulation at a reynolds number of 10^6, which I know is very high. To validate my mesh, I made a smoth mesh with N_x1=42, N_x2=980, N_y=42, N_z=12 and N_diag=42 nodes. The geometry has a hight of 20mm a depth of 10mm and a length of 1000mm. The diameter of the cylinder is 5mm. Please have a look at this image. The medium-fine mesh is the fine one scaled with a factor of 0.5. So is the rough mesh 0.5 times the medium-fine.
I have huge problmes because the simulation will not converge. Only the rough net with a "Reynolds Stress" turbulence model converged in few timesteps. The residuals of the finer meshes jitter around at about 10^(-2) for hours.
Because I do not know, what is relevant for deeper explanation, I linked the result- and the outputfile here CLICK.
I already tried to modify the "Time Scale" to see, if there is an amortisation by changing it. I made the simulations with the "SST" model (Zylinder_3d_re1000000_stat_g_001), changed it for once in "Reynolds Stress" (Zylinder_3d_re1000000_stat_g_004). The file001 did not converged but had a minimal MAX Residual of 10^(-4). File004 converged imidiatly (the cause, it goes a long way straight before, is because I had an "maximum Timescale" activeted. When I deactivated it, it went right down to 10^(-6).

I would appreciate it very much, if someone would have a look at this. This case must be very simple, so there must be something trivial I do not see!

Thank you very much. If there are more files or explanations needed, please ask!

Greetings
Witold

Darren Leong December 3, 2010 21:43

Hi Witold,

I tried opening your .res files to no avail.
Got a few questions:
1. What version of the ANSYS/fluent are you using?
2. What license do you have; research or teaching? (mesh no. limitation applies here)
3. Simulation in steady-state or transient? <- has to be transient XD

Suggestion:
1. Grid independence study - you might be able to get away with ~500,000elements, let me know how many you're at.
2. I highly suggest you look into defining your first node height by calculating the y+ at <2 for sst model. You should get your vortex street but it may be overpredicted compared to k-e model. Put your growth in range of 1- 1.1. The mesh doesn't look fine enough as it is to capture the flow characteristics
3. Reduce your timescale. Have a read-up on "Courant Number".
4. Solve in double precision (64-bit, more information for better accuracy)
5. Extend/enlarge your fine mesh domain, doesn't look big enough as it is for Re=10^6 (optional)

6. Do a literature review/google. Your problem's been already addressed, there are even tutorials available on it =)

-dazza

Wotild December 4, 2010 18:27

Hi dazza,
I do not understand, why the file can't be opened. I am using Ansys 12.1 with ICEM CFX for meshing. All with a research Licence (the one, with a limitation of nodes).
As you mentioned I think my biggest fault is, that I didn't make the simulation transient. Of course there is no steady state in this flow.

1: I tried to make an independence study, but since my simulations did not converge, there are noch results. I am limited to 512k nodes, wehn I remember right, so this would be my finest mesh. Then go down by a scale of 0.5 each time.
2: with the formula from the Ansys help \Delta y = y^+ \cdot  log(Re)^{-13/14} \cdot \sqrt{74} \cdot  \text{Diameter} I realized a y+ about 1 at the cylinder. Because of the change of the shear around the cylinder y+ changes a bit. I have a growth rate of 1.5 at the wall...I will try a ratio of 1.1 .
3: the Courantnumber was a nice hint. It showed, that my timescale was far to long.
4: double precision is always activated.
5: I had this thought too...but how long? Is there any formula like for the laminar or turbulent flow in straight pipes?
6: I will make some more searches. But most of the paper consider high Re-numbers up to 1000. But I continue looking.

Thank you very much as far. I will make some simulations and post the results here.

Greetings
Witold

Darren Leong December 4, 2010 20:00

Hi Witold,

Glad to know it was of help. Best to shift your direction to transient eventually =)

The present setup was alright as a preliaminary result. See if you can plot the wake, it'll give you an idea how far to extend domain. The mesh no. limitation will be a problem depending on whether you have enough to visuallise the vortices smoothly (too coarse -> pixelated ).

Careful about Re at 10^6. Although it's dimentionless, the reported value differs whether they took the diameter or length as ref. I think for your case, you might barely notice the vortex street as it will be compacted at Re of 1000000.

Best wishes,
dazza

ps. try growth rate of 1.3, 1.1 will likely exceed ur mesh limit,

Wotild December 7, 2010 14:41

Hi!

My Re ist based on the diameter. I know the vortices will be very compacted. I need to have a look on the flow in it's mixed state.
I have a further question. I am not an expert in traniscient flow yet. I have timesteps of 7e-8s to achieve a Courant number of about 0.01 .
When i want to simulate a 8s flow, this would mean to make 114e6 steps, each with 2 till 5 coefficient loops. With 30s per iteration it will need 108 years ;)
There must be a faster way, to achieve the results of a fully developed flow, or am I wrong?
I haven't googled this yet, I will immediately, but when someone has an answer right now, I would appreciate it.

Thank you!
Greets

Edit: I already initialized with full velocity

Darren Leong December 7, 2010 22:07

You'll need to run your simulation in parallel if ur pc has multiple processors or over a cluster. However, i think your timestep's too small (overdefined). Try relaxing the value enough for your solution to just converge.

If you thesis work is on a research basis and not coursework, i would suggest investigating/validating your setup at lower speeds to determine the critical reynolds number first and then proceed to Re 10^6.

Forum member, Altomos has done similiar work to yours. Might be helpful msging him on details of his setup. Refer to http://www.cfd-online.com/Forums/ans...ing-ansys.html
He used Strouhal number instead to determine the timestep based on the frequency calculated.

Edit: Just to be sure, check your user license prefences for ANSYS. If there's a research license in the list move it to the top (change the value to 1 if 0). I think only the teaching license has the 512k limitation.


All times are GMT -4. The time now is 22:16.