|
[Sponsors] |
April 4, 2013, 00:48 |
Fluent + flow past cylinder at Re=40
|
#1 |
New Member
Mitesh Vegad
Join Date: Apr 2013
Posts: 18
Rep Power: 13 |
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 |
|
April 4, 2013, 04:06 |
|
#2 |
Senior Member
Philipp
Join Date: Jun 2011
Location: Germany
Posts: 1,297
Rep Power: 27 |
Can you post pictures?
__________________
The skeleton ran out of shampoo in the shower. |
|
April 4, 2013, 06:50 |
|
#3 |
New Member
Mitesh Vegad
Join Date: Apr 2013
Posts: 18
Rep Power: 13 |
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 |
|
April 4, 2013, 07:44 |
|
#4 |
Senior Member
Philipp
Join Date: Jun 2011
Location: Germany
Posts: 1,297
Rep Power: 27 |
Can you upload both meshes?
Just one simple idea: Did you forget to scale the fine mesh?
__________________
The skeleton ran out of shampoo in the shower. |
|
April 5, 2013, 02:25 |
|
#5 |
New Member
Mitesh Vegad
Join Date: Apr 2013
Posts: 18
Rep Power: 13 |
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 |
|
April 5, 2013, 02:52 |
|
#6 |
Senior Member
Philipp
Join Date: Jun 2011
Location: Germany
Posts: 1,297
Rep Power: 27 |
No, I meant, can you upload the .msh files, so I can try them in Fluent?
__________________
The skeleton ran out of shampoo in the shower. |
|
April 5, 2013, 03:27 |
|
#7 |
New Member
Mitesh Vegad
Join Date: Apr 2013
Posts: 18
Rep Power: 13 |
The file size if in MB and cant be attached.
Can i have your email ID. Will send them as an email attachment Thanks |
|
April 5, 2013, 13:29 |
|
#8 |
Senior Member
|
||
April 5, 2013, 13:35 |
|
#9 |
Senior Member
Filippo Maria Denaro
Join Date: Jul 2010
Posts: 6,892
Rep Power: 73 |
are you sure that the solution on the fine grid reached the same convergence and the residual is small?
|
|
April 5, 2013, 13:47 |
|
#10 |
Senior Member
|
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. |
|
April 6, 2013, 03:17 |
|
#11 |
New Member
Mitesh Vegad
Join Date: Apr 2013
Posts: 18
Rep Power: 13 |
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 |
|
April 6, 2013, 05:22 |
|
#12 |
Senior Member
|
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. Last edited by Far; April 6, 2013 at 05:45. Reason: see post |
|
April 6, 2013, 06:45 |
|
#13 |
Senior Member
|
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. |
|
April 6, 2013, 09:37 |
Re = 40, Coarse mesh
|
#14 |
Senior Member
|
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 Last edited by Far; April 6, 2013 at 10:11. Reason: adding description about solution setup |
|
April 6, 2013, 17:51 |
Drag at Re = 40 for two meshes
|
#15 |
Senior Member
|
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 Last edited by Far; April 6, 2013 at 18:51. |
|
April 7, 2013, 11:55 |
|
#16 |
Senior Member
|
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? |
|
April 8, 2013, 01:00 |
|
#17 |
New Member
Mitesh Vegad
Join Date: Apr 2013
Posts: 18
Rep Power: 13 |
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??? |
|
April 8, 2013, 03:43 |
|
#18 | ||
Senior Member
|
Quote:
Quote:
|
|||
April 8, 2013, 05:33 |
|
#19 |
New Member
Mitesh Vegad
Join Date: Apr 2013
Posts: 18
Rep Power: 13 |
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? |
|
April 8, 2013, 12:15 |
|
#20 | |
Senior Member
|
Quote:
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. |
||
Thread Tools | Search this Thread |
Display Modes | |
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
FLuent simulation of taylor couette flow of concentric cylinder geometry. | rshbhb | FLUENT | 53 | November 5, 2014 20:07 |
[ICEM] Flow past a 2D cylinder | arun7328 | ANSYS Meshing & Geometry | 0 | February 15, 2013 13:17 |
benchmark: flow over a circular cylinder | goodegg | Main CFD Forum | 12 | January 22, 2013 12:47 |
Drag coefficient of flow past cylinder vs time | pedroxramos | FLUENT | 0 | January 14, 2013 13:39 |
flow past cylinder | joe | FLUENT | 6 | August 11, 2007 10:02 |