Fluent + flow past cylinder at Re=40
 

Hi,
I am trying to simulate steady flow around a circular cylinder for Re=40 (two dimensional)

For a coarse mesh, things are fine and there is flow separation.

However.... to check mesh independence when in keep refining the mesh the flow separation dose not happen ans the solution is absurd...

Can some one help.

Thanks

Can you post pictures?

Hi,

Am attaching image of vector plot next to cylinder surface... one with coarse mesh shows flow separation.

However, on refining the mesh the flow separation is not captured and the solution shows that the fluid flows sticking to the surface without reverse flow in region next to the cylinder!!!!

Have used structured mesh generated using GAMBIT.

Have not taken expansion/contraction factor more than 5% and have ensured that the control volume size dose not change abruptly.

Please reply.

Thanks

Can you upload both meshes?

Just one simple idea: Did you forget to scale the fine mesh?

Hi,

Am attaching pic of mesh next to cylinder.

Coarse mesh simulation shows separation, where as fine mesh dose not.

Have taken due care to scale the mesh properly before setting up the case for the Fluent solver.

Please reply

Thanks

No, I meant, can you upload the .msh files, so I can try them in Fluent?

The file size if in MB and cant be attached.

Can i have your email ID. Will send them as an email attachment

Thanks

See post # 23 in particular here http://www.cfd-online.com/Forums/ans...linders-2.html

http://www.cfd-online.com/Forums/att...eward-mesh.jpg

are you sure that the solution on the fine grid reached the same convergence and the residual is small?

Recently we did a class excerise at Reynolds numbers from 100 to 1000 in fluent.

We have following setup:

1. Fine mesh of size 40000 nodes

2. pressure - coupled solver

3. second order upwind for momentum

4. second order implicit time

5. For Re= 100 : Density = 100 Kg/m3, V = 1 m/sec, Dia = 1 m, viscosity = 1

6. For Re= 1000 : Density = 100 Kg/m3, V = 1 m/sec, Dia = 1 m, viscosity = 0.1

7. Strouhal no is 0.2 and therefore Frequency is also 0.2. For this if you take 25 times step per cycle time step would be 0.2.

8. Initialize with patching to get highly non-uniform initial guess and have convergence in less time steps (order of 5-10)

For your case, Re= 40 , I guess you need steady state solution if convergence is OK.

Hi,

The convergence criteria i have specified for simulation is 0.0001 for mass and momentum conservation.

For coarse as well as the fine mesh the residual is below the convergence criteria as specified above.

Am following all steps as suggested in the previous post... still things are not working out.

Actually more than the solution... i want to find where the mistake is in my approach and why fine mesh dose not give flow separation !!!! .. so am not using any other mesh form online source.

Please reply

lower your convergence criteria to 1e-18 and see what happens ...

What is the overall mesh size. Can you show more pics of yor mesh.

Edit : I saw your mesh and I would like to recommend that at least use 15 dia upstream.

Here I got from your fine mesh and results are according to available literature.

Non uniform solution intialization to speed up convergence specially for transient flows with vertex shedding etc.
http://imageshack.us/a/img593/1643/initialize.png

http://imageshack.us/a/img843/2384/mesh2.png

http://imageshack.us/a/img705/9949/mesh3.png

http://imageshack.us/a/img40/6452/vorticity.png

Re = 40, Coarse mesh
 

Flow setup:

Re = 40

Velocity = 1, density = 40, dia = 1 m , viscosity = 1 (All units in SI)

Pressure -coupled solver

Second order upwind flow scheme

convergence criteria = 1e-19 and residuals dropped to 1e-14


http://imageshack.us/a/img856/4845/vorticitycoarse.png

http://imageshack.us/a/img203/3127/vorticitycoarse2.png

Drag at Re = 40 for two meshes
 

Cd = 1.618 from your fine mesh 125*125
Cd = 1.5321 from my mesh as shown in post # 8

From reference ftp://ftp.demec.ufpr.br/CFD/bibliogr...artigo-jcp.pdf

Cd = 1.54

From http://www.me.iitb.ac.in/~fmfp/FMFP%20PROC/cf_04.pdf

Cd = 1.5

Something very interesting and strange is happening.

Results from my mesh:

Case 1 :With extended domain 25 upstream and 50 downstream (meshing done by me)

Cd= 1.5277

Case 2 : With nominal domain: 15 upstream and 35 downstream

Cd = 1.5321

Case 3 : With shorter domain: 7.5 dia upstream and 35 dia downstream.

Cd = 1.6234

Case 4 : From your fine mesh: 7.5 upstream and 38 downstream

Cd = 1.618

I referred several good papers including one (published in journal) which used the same mesh size, domain extent and topology as your have used and results are same as shorter domain from your mesh and mine mesh. So are they wrong?

May be the trouble with the solution that i had got was...

with the lower convergence criteria.... the solution still had error and so the vortices downstream of the cylinder were not captured...

About change in the UPSTREAM distance in the previous post... well i guess the solution is not wrong... but the thing is that probably i need to provide larger upstream length as the post shows...

But again how large is large???

as you can see 15 is large enough and after that it does make any significant difference as confirmed from 25 dia upstream . Even if you plot velocity contours you will notice the big difference in plot for larger upstream and shorter upstream domain.

In Fluent it is hard to visualize these vortices, use tecplot instead and draw streamlines.

No.... by how large is large what I actually meant is that would the upstream distance be related to the Reynolds number?

If so then how dose one determine the upstream distance other than taking the largest Re of interest and testing as above!

Is there any other way?

higher the reynolds number and less effect of domain extent.

I usually take:

For reynolds number less 200:

Upstream 15 dia and downstream 25 dia

Greater than 200:

10 dia upstream and 20 dia downstream.