CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   STAR-CCM+ (http://www.cfd-online.com/Forums/star-ccm/)
-   -   Simple simulation not converging :( please help! (http://www.cfd-online.com/Forums/star-ccm/98054-simple-simulation-not-converging-please-help.html)

James88 March 1, 2012 19:19

Simple simulation not converging :( please help!
 
Hi everyone

I have done a simple simulation of a cylinder in laminar flow with Re 120, but the residuals are determined not to converge! Could one of you please take a quick look at my file, and see if there is anything that I have done wrong?

Thank you!!

http://www.mediafire.com/?cx224c1bbb1mwn2

James88 March 1, 2012 19:44

Also, the values obtained for lift co-efficient are incorrect, can anyone see what I have done wrong using the report?

thanks

lava12005 March 1, 2012 21:40

Hi, I'm using Star-CCM+ V5, so I can't open your file.
Maybe your mesh is not fine enough?
Are you simulating half cylinder (forcing it to steady) or full cylinder?
Anyway at Re = 120, vortex shedding has appeared, so you might want to run it unsteady and then compare your result.

James88 March 1, 2012 22:39

Hi Lava, I think my mesh is quite fine... When I have access to my simulation tomorrow morning I will get a screenshot/some mesh values.
What do you mean by simulating half cylinder or full cylinder? I have tried running both as just steady state, unsteady state, and started at steady state then changed the model later to unsteady, they all ended up with values around 0.1 to 0.001 on the residual graph.
I will get screenshots for each simulation tomorrow!

You are correct that I am getting vortex shedding, and at the correct frequency according to strouhals number, but my residuals and force coeffients are incorrect unfortunately :(

ali moghimifar March 2, 2012 15:14

Hi dear friend. i can't open your file. but i can give you my mesh file please give me your E_MAIL to send u the file

James88 March 2, 2012 16:00

Quote:

Originally Posted by ali moghimifar (Post 347356)
Hi dear friend. i can't open your file. but i can give you my mesh file please give me your E_MAIL to send u the file

That would be very appreciated, can you please send it to azmcinally@hotmail.com !

ThomasZiegenhein March 2, 2012 20:19

Dear James,
I checked your sim.-File. Some things are not so correct :-) :
  1. it is (as lava already mentioned) an unsteady problem, so try it unsteady
  2. Calculate it with a turbulence model, with Re=130 you are at a critical point between 'laminar' vortex shedding and turbul. vortex shedding, nevertheless I would calculate it for Re> 25 always with a turb. model
  3. The mesh is poor quality, because of the big surface cells the cylinder looks like a polygon.
  4. Don't define outlets at the top and at the bottom, use symm. Planes
  5. Use local refinement with volume shapes to get a fine mesh at the important points
  6. Make your prism layer mesh smaller, check the y+ value. If you want to calculate it exactly use y+ around 1.


I calculate it unsteady with SST (with your mesh), my cw-value is about 1.2 ( corresponding to the wiki-value ).


Hope I can help you.


Good Luck
Thomas

James88 March 3, 2012 11:40

Quote:

Originally Posted by ThomasZiegenhein (Post 347383)
Dear James,
I checked your sim.-File. Some things are not so correct :-) :
  1. it is (as lava already mentioned) an unsteady problem, so try it unsteady
  2. Calculate it with a turbulence model, with Re=130 you are at a critical point between 'laminar' vortex shedding and turbul. vortex shedding, nevertheless I would calculate it for Re> 25 always with a turb. model
  3. The mesh is poor quality, because of the big surface cells the cylinder looks like a polygon.
  4. Don't define outlets at the top and at the bottom, use symm. Planes
  5. Use local refinement with volume shapes to get a fine mesh at the important points
  6. Make your prism layer mesh smaller, check the y+ value. If you want to calculate it exactly use y+ around 1.


I calculate it unsteady with SST (with your mesh), my cw-value is about 1.2 ( corresponding to the wiki-value ).


Hope I can help you.


Good Luck
Thomas

Hi Thomas!

I am currently re-running the simulation making changes from your suggestions:
  • I changed the number of prism layers around the cylinder to 360, so that should make a finer cylinder shape!
  • I am using the physics models of: two dimensional, turbulent, K-epsilon, implicit unsteady, liquid, segregated flow.
  • I have set the top and bottom regions as outlets
  • Used a block shape to refine the mesh around the cylinder

I have a few questions though...
The sources I have looked at define the flow at Reynolds numbers of ~250 and below as laminar flow, however you suggested using turbulence? Is it just accepted that when vortex shedding is involved, it is better to use a turbulence model?
Why is it best to use a symmetry plane for the top and bottom planes? Also, the next step of my simulations is to run a 3D model of a finite cylinder, do you think it would be best again to use symmetry planes for the walls of the model in that case?

My residuals look great so far, however, the simulation is taking a veeery long time to run. I am using 155 iterations per 0.2s time step, at this level the residuals reach around 1E-4 to 1E-7. Obviously I could reduce the mesh size, but this may sabotage my results! On the other hand, I could decrease the iterations per step... but then my residuals wouldn't converge. I am just concerned of how long this will take to simulate when using a 3D model!

Many thanks for all your suggestions, you've been a massive help! And I really appreciate it :)

ThomasZiegenhein March 3, 2012 13:26

Hey James,
Good to hear that your simulation runs now. Now you have to go to detail. Your plan, first to simulate it simplified in 2D and then 3D is good.
To your questions:

-360 prism layers are not necessary I think. Look up how thick is your boundary layer, this should be your orientation for the prism layer thickness.

- k-epsilon is perhaps not the best choice for turbulence like this, the k-omega-SST (from Menter) is good for such cases (important wall effects with vortex shedding). Also the k-epsilon two layer model is suitable

-symmetry planes do this what you want, at the boundaries is the normal derivation zero. If you use outlets this may cause numerical troubles at the edges (Outlet 90 degree at Outlet). This may end up in a not converged simulation, or the residuals are at a high level.

-Use more than one block shape to resolve the separation points from the wall.

-I think your source defined the spec. length for Re with radius, I used the diameter ( 250 ~= 130 *2). If this is laminar or not is an interesting question, depending how you define laminar. I understand laminar as a flow status, were the streamlines are always parallel and the streamlines donít interact through convection. When you have such vortex shedding, I would say it is turbulent. All in all you are at a critical point, therefore I would activate the turb. model. But try it laminar and turbulent, and see what happens :-)

- 155 steps per 0.2s is too much. Take a courant number between 1-5 (if you know what you do, a max. courant number of 100 should work in some applications too) and around 10 inner iterations per time step. The flow around the cylinder needs around 10s to running in (avg. in time is constant), in this time you get high residuals. So donít be afraid when you get high residuals at the beginning, they should decrease.

Greetings
Thomas

James88 March 3, 2012 17:32

Hi Thomas

I honestly cannot thank you enough! My simulation is running perfectly, there is hope for me yet ;)

If I have any other questions, would you be okay helping me in the future?

Again, thank you so much, you have been incredibly helpful, I don't know how to repay you!

ThomasZiegenhein March 4, 2012 05:11

hey james,

you did all the work, I only noticed the main problems, so thank yourself :-).

Sure you can, just post further questions here or under another topic. I think other members can help also, and perhaps other members are also interested in our discussion.

And perhaps a hint for the future: If u are not sure about something (like if it's turb. or laminar, or a new feature), go back to the 2D case, try it out and validate it with exp. results. That's my way and the way I tell students to do, and it work's quite well :-).

Good luck for your further simulation
Thomas

James88 March 6, 2012 11:45

Hi again! I am trying to look at the effect that the free end of the cylinder has on the vortex shedding... Before now, I have used the force lift co-efficient monitor (on the cylinder), looked at the timestep, and taken the time period. But I saw in the user guide that the data set function can be used to get the strouhal number? This would be very useful, but it does not actually give any proper instructions how to use the function...
I have set the function as a fourier transform, and frequency function as Strouhal number, however, I do not know what to do from here? Or where/how the data is inputted/outputted?

Sorry for more questions :p

James


All times are GMT -4. The time now is 03:55.