# Fluent + flow past cylinder at Re=40

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

 April 3, 2013, 23:48 Fluent + flow past cylinder at Re=40 #1 New Member   Mitesh Vegad Join Date: Apr 2013 Posts: 18 Rep Power: 5 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, 03:06 #2 Senior Member     Philipp Join Date: Jun 2011 Location: Germany Posts: 1,297 Rep Power: 19 Can you post pictures? __________________ The skeleton ran out of shampoo in the shower.

April 4, 2013, 05:50
#3
New Member

Join Date: Apr 2013
Posts: 18
Rep Power: 5
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.

Thanks
Attached Images
 Course Mesh2.jpg (42.1 KB, 38 views) Fine Mesh.jpg (76.9 KB, 35 views)

 April 4, 2013, 06:44 #4 Senior Member     Philipp Join Date: Jun 2011 Location: Germany Posts: 1,297 Rep Power: 19 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, 01:25
#5
New Member

Join Date: Apr 2013
Posts: 18
Rep Power: 5
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.

Thanks
Attached Images
 c50r50(re40) cylinder mesh With Result.jpg (68.8 KB, 29 views) C125R125 cylinder mesh No result.jpg (67.4 KB, 34 views)

 April 5, 2013, 01:52 #6 Senior Member     Philipp Join Date: Jun 2011 Location: Germany Posts: 1,297 Rep Power: 19 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, 02:27 #7 New Member   Mitesh Vegad Join Date: Apr 2013 Posts: 18 Rep Power: 5 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, 12:29 #8 Super Moderator   Sijal Join Date: Mar 2009 Location: Islamabad Posts: 4,299 Blog Entries: 6 Rep Power: 43 See post # 23 in particular here Meshing in Gambit for analysis of flow past cylinders

 April 5, 2013, 12:35 #9 Senior Member   Filippo Maria Denaro Join Date: Jul 2010 Posts: 2,609 Rep Power: 33 are you sure that the solution on the fine grid reached the same convergence and the residual is small?

 April 5, 2013, 12:47 #10 Super Moderator   Sijal Join Date: Mar 2009 Location: Islamabad Posts: 4,299 Blog Entries: 6 Rep Power: 43 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, 02:17 #11 New Member   Mitesh Vegad Join Date: Apr 2013 Posts: 18 Rep Power: 5 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, 04:22 #12 Super Moderator   Sijal Join Date: Mar 2009 Location: Islamabad Posts: 4,299 Blog Entries: 6 Rep Power: 43 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

 April 6, 2013, 05:45 #13 Super Moderator   Sijal Join Date: Mar 2009 Location: Islamabad Posts: 4,299 Blog Entries: 6 Rep Power: 43 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, 08:37 Re = 40, Coarse mesh #14 Super Moderator   Sijal Join Date: Mar 2009 Location: Islamabad Posts: 4,299 Blog Entries: 6 Rep Power: 43 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

 April 6, 2013, 16:51 Drag at Re = 40 for two meshes #15 Super Moderator   Sijal Join Date: Mar 2009 Location: Islamabad Posts: 4,299 Blog Entries: 6 Rep Power: 43 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.

 April 7, 2013, 10:55 #16 Super Moderator   Sijal Join Date: Mar 2009 Location: Islamabad Posts: 4,299 Blog Entries: 6 Rep Power: 43 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, 00:00 #17 New Member   Mitesh Vegad Join Date: Apr 2013 Posts: 18 Rep Power: 5 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, 02:43
#18
Super Moderator

Sijal
Join Date: Mar 2009
Posts: 4,299
Blog Entries: 6
Rep Power: 43
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.

 April 8, 2013, 04:33 #19 New Member   Mitesh Vegad Join Date: Apr 2013 Posts: 18 Rep Power: 5 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, 11:15
#20
Super Moderator

Sijal
Join Date: Mar 2009
Posts: 4,299
Blog Entries: 6
Rep Power: 43
Quote:
 Originally Posted by m.vegad 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.

 Thread Tools Display Modes Linear Mode

 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 OffTrackbacks are On Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post rshbhb FLUENT 53 November 5, 2014 20:07 [ICEM] Flow past a 2D cylinder arun7328 ANSYS Meshing & Geometry 0 February 15, 2013 13:17 goodegg Main CFD Forum 12 January 22, 2013 12:47 pedroxramos FLUENT 0 January 14, 2013 13:39 joe FLUENT 6 August 11, 2007 09:02

All times are GMT -4. The time now is 07:48.