CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Main CFD Forum

Fluent + flow past cylinder at Re=40

Register Blogs Members List Search Today's Posts Mark Forums Read

Reply
 
LinkBack Thread Tools Display Modes
Old   April 3, 2013, 23:48
Default Fluent + flow past cylinder at Re=40
  #1
New Member
 
Mitesh Vegad
Join Date: Apr 2013
Posts: 18
Rep Power: 4
m.vegad is on a distinguished road
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
m.vegad is offline   Reply With Quote

Old   April 4, 2013, 03:06
Default
  #2
Senior Member
 
RodriguezFatz's Avatar
 
Philipp
Join Date: Jun 2011
Location: Germany
Posts: 1,099
Rep Power: 16
RodriguezFatz will become famous soon enough
Can you post pictures?
__________________
The skeleton ran out of shampoo in the shower.
RodriguezFatz is offline   Reply With Quote

Old   April 4, 2013, 05:50
Default
  #3
New Member
 
Mitesh Vegad
Join Date: Apr 2013
Posts: 18
Rep Power: 4
m.vegad is on a distinguished road
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
Attached Images
File Type: jpg Course Mesh2.jpg (42.1 KB, 36 views)
File Type: jpg Fine Mesh.jpg (76.9 KB, 32 views)
m.vegad is offline   Reply With Quote

Old   April 4, 2013, 06:44
Default
  #4
Senior Member
 
RodriguezFatz's Avatar
 
Philipp
Join Date: Jun 2011
Location: Germany
Posts: 1,099
Rep Power: 16
RodriguezFatz will become famous soon enough
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.
RodriguezFatz is offline   Reply With Quote

Old   April 5, 2013, 01:25
Default
  #5
New Member
 
Mitesh Vegad
Join Date: Apr 2013
Posts: 18
Rep Power: 4
m.vegad is on a distinguished road
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
Attached Images
File Type: jpg c50r50(re40) cylinder mesh With Result.jpg (68.8 KB, 26 views)
File Type: jpg C125R125 cylinder mesh No result.jpg (67.4 KB, 31 views)
m.vegad is offline   Reply With Quote

Old   April 5, 2013, 01:52
Default
  #6
Senior Member
 
RodriguezFatz's Avatar
 
Philipp
Join Date: Jun 2011
Location: Germany
Posts: 1,099
Rep Power: 16
RodriguezFatz will become famous soon enough
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.
RodriguezFatz is offline   Reply With Quote

Old   April 5, 2013, 02:27
Default
  #7
New Member
 
Mitesh Vegad
Join Date: Apr 2013
Posts: 18
Rep Power: 4
m.vegad is on a distinguished road
The file size if in MB and cant be attached.

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

Thanks
m.vegad is offline   Reply With Quote

Old   April 5, 2013, 12:29
Default
  #8
Far
Super Moderator
 
Far's Avatar
 
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,971
Blog Entries: 6
Rep Power: 39
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
See post # 23 in particular here Meshing in Gambit for analysis of flow past cylinders

Far is offline   Reply With Quote

Old   April 5, 2013, 12:35
Default
  #9
Senior Member
 
Filippo Maria Denaro
Join Date: Jul 2010
Posts: 1,661
Rep Power: 23
FMDenaro will become famous soon enough
are you sure that the solution on the fine grid reached the same convergence and the residual is small?
FMDenaro is offline   Reply With Quote

Old   April 5, 2013, 12:47
Default
  #10
Far
Super Moderator
 
Far's Avatar
 
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,971
Blog Entries: 6
Rep Power: 39
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
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.
Far is offline   Reply With Quote

Old   April 6, 2013, 02:17
Default
  #11
New Member
 
Mitesh Vegad
Join Date: Apr 2013
Posts: 18
Rep Power: 4
m.vegad is on a distinguished road
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
m.vegad is offline   Reply With Quote

Old   April 6, 2013, 04:22
Default
  #12
Far
Super Moderator
 
Far's Avatar
 
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,971
Blog Entries: 6
Rep Power: 39
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
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 04:45. Reason: see post
Far is offline   Reply With Quote

Old   April 6, 2013, 05:45
Default
  #13
Far
Super Moderator
 
Far's Avatar
 
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,971
Blog Entries: 6
Rep Power: 39
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
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.






Far is offline   Reply With Quote

Old   April 6, 2013, 08:37
Default Re = 40, Coarse mesh
  #14
Far
Super Moderator
 
Far's Avatar
 
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,971
Blog Entries: 6
Rep Power: 39
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
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 09:11. Reason: adding description about solution setup
Far is offline   Reply With Quote

Old   April 6, 2013, 16:51
Default Drag at Re = 40 for two meshes
  #15
Far
Super Moderator
 
Far's Avatar
 
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,971
Blog Entries: 6
Rep Power: 39
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
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 17:51.
Far is offline   Reply With Quote

Old   April 7, 2013, 10:55
Default
  #16
Far
Super Moderator
 
Far's Avatar
 
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,971
Blog Entries: 6
Rep Power: 39
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
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?
Far is offline   Reply With Quote

Old   April 8, 2013, 00:00
Default
  #17
New Member
 
Mitesh Vegad
Join Date: Apr 2013
Posts: 18
Rep Power: 4
m.vegad is on a distinguished road
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???
m.vegad is offline   Reply With Quote

Old   April 8, 2013, 02:43
Default
  #18
Far
Super Moderator
 
Far's Avatar
 
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,971
Blog Entries: 6
Rep Power: 39
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
Quote:
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.

Quote:
with the lower convergence criteria.... the solution still had error and so the vortices downstream of the cylinder were not captured...
In Fluent it is hard to visualize these vortices, use tecplot instead and draw streamlines.
Far is offline   Reply With Quote

Old   April 8, 2013, 04:33
Default
  #19
New Member
 
Mitesh Vegad
Join Date: Apr 2013
Posts: 18
Rep Power: 4
m.vegad is on a distinguished road
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?
m.vegad is offline   Reply With Quote

Old   April 8, 2013, 11:15
Default
  #20
Far
Super Moderator
 
Far's Avatar
 
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,971
Blog Entries: 6
Rep Power: 39
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
Quote:
Originally Posted by m.vegad View Post
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.
Far is offline   Reply With Quote

Reply

Thread Tools
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are On
Pingbacks are On
Refbacks are On


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 09:02


All times are GMT -4. The time now is 13:48.