# Does domain size matter?

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

 April 21, 2013, 10:17 Does domain size matter? #1 Senior Member   Join Date: Jan 2013 Posts: 121 Rep Power: 7 hi everyone! my question may be stupid, but it's hunting me for a long time. I'm doing something simulations about flow around a cylinder. There are two cases. Case 1: D=0.01m; U=0.15m/s; Re =100; Case 2: D=1m; U=0.0015m/s; Re=100; The two cases are similar in domain size and as can be seen Case 2 is 100 bigger than Case 1, and they have the same mesh fineness. In Case 1, the situation is bigger velocity with smaller cylinder and in Case 2 smaller velocity with bigger cylinder. Nevertheless, it is anticipated that if the Re is the same, Cd and Cl, which are the drag and lift coefficients respectively, should be the same in the two cases. But in my simulations, the result of Case 1 worked very well; however, Case 2 gave very bad results. Why is this happening? should i refine the mesh in Case 2 so that the smallest grid size is as fine as the Case 1？

 April 21, 2013, 11:40 #2 Super Moderator   Sijal Join Date: Mar 2009 Location: Islamabad Posts: 4,358 Blog Entries: 6 Rep Power: 45 Are you assuming it steady or unsteady? It is definitely unsteady and in both situations you have to select different time step size due to difference in vortex shedding frequency. What are the values of density and viscosity?

April 21, 2013, 11:57
#3
Senior Member

Join Date: Jan 2013
Posts: 121
Rep Power: 7
Quote:
 Originally Posted by Far Are you assuming it steady or unsteady? It is definitely unsteady and in both situations you have to select different time step size due to difference in vortex shedding frequency. What are the values of density and viscosity?
Hi Far!
I chose laminar as the RASmodel in OpenFOAM, so I think for both cases it should be unsteady.
The timestep of both cases is small enough to keep the Courant number<1, and my nu is 1.5e-5 and rho 1.2, which is associated with air.
About the vortex shedding frequency, in my two cases they are not the same, how could I adjust my time step in order to get the same Cd and Cl?
I'm now very confused about the similarities in Re and St. For the two cases, if I keep Re the same, St will be different and vise verse. How could I choose the D and U if I want to simulate a bridge cable with certain diameter and flow velocity around it in the real world?

 April 21, 2013, 12:21 #4 Super Moderator   Sijal Join Date: Mar 2009 Location: Islamabad Posts: 4,358 Blog Entries: 6 Rep Power: 45 Strouhal_number is ratio frequency * dia / velocity . In first case ratio of D/U is 0.0666 and in second case ratio is 666.6 and if we assume St no 0.2 you will notice that frequency is 3.003 in one case and 0.0003 in second case. total time is 0.33 sec and 333 seconds and if we want to resolve them in 50 times steps then each time step would be 0.0066s and 6.66 s respectively. PS: Assuming that Reynolds number is same then you should get same Cd (time averaged) kkpal likes this.

April 22, 2013, 02:14
#5
Senior Member

Join Date: Jan 2013
Posts: 121
Rep Power: 7
Quote:
 Originally Posted by Far Strouhal_number is ratio frequency * dia / velocity . In first case ratio of D/U is 0.0666 and in second case ratio is 666.6 and if we assume St no 0.2 you will notice that frequency is 3.003 in one case and 0.0003 in second case. total time is 0.33 sec and 333 seconds and if we want to resolve them in 50 times steps then each time step would be 0.0066s and 6.66 s respectively. PS: Assuming that Reynolds number is same then you should get same Cd (time averaged)
Dear Sijal
Thank you very much for your detailed reply, now I get a better understanding of the St number, may be i need to run the second case for enough long time to get the vortex shedding. In fact I think the proportion of U and D in case 2 is not appropriate because one period takes 3333s.

On a related subject, if i insisted in doing case 2, and I ran the simulation for enough time, do you think it is necessary to refine the mesh in case 2. I'm thinking that with 100 times bigger in the domain size, the smallest grid size also is 100 times bigger, will it affect the simulation result?

April 22, 2013, 02:59
#6
Super Moderator

Sijal
Join Date: Mar 2009
Posts: 4,358
Blog Entries: 6
Rep Power: 45
Quote:
 On a related subject, if i insisted in doing case 2, and I ran the simulation for enough time, do you think it is necessary to refine the mesh in case 2. I'm thinking that with 100 times bigger in the domain size, the smallest grid size also is 100 times bigger, will it affect the simulation result?
I dont think so. Lets try and find out what happens in both cases and let us know as well.

April 22, 2013, 03:11
#7
Senior Member

Join Date: Jan 2013
Posts: 121
Rep Power: 7
Quote:
 Originally Posted by Far I dont think so. Lets try and find out what happens in both cases and let us know as well.
ok, I will do a similar case with D=0.03m and U=0.05m/s for which the frequency is about 3.3s. The original second case takes too much time.
I will post the result to here once I finish the simulation.
Thank you again, Sijal. You have been very helpful!

 April 22, 2013, 06:07 #8 New Member   Mitesh Vegad Join Date: Apr 2013 Posts: 18 Rep Power: 6 In fact i too had the same question troubling me since long... i mean in case of larger domain the size of control volume next to solid region would be RELATIVELY large.... so truncation error wont be the same as in case of smaller domain (to the best of my understanding)... If one checks the grid in FLUENT.. then for the larger size domain the mim and max area and volume reported are significantly higher than the smaller domain.. So would a mesh for smaller domain give mesh independent sol for a larger domain too!!! ( Reynolds no is the same in both cases)

April 22, 2013, 20:41
result of domain size test
#9
Senior Member

Join Date: Jan 2013
Posts: 121
Rep Power: 7
dear all,
here I put up the result of my test.

COMMON CHARACTERISTICS:
Domain size: (15R+40R)*30R
Mesh information: 32010 vertices, 50732 elements
Turbulence model: laminar

CASE 1:
R=0.005m, U=0.15m/s, Re=100, f=St*U/D=3, T=0.33s
Timestep=0.0001s

the drag coefficient Cd is about 1.5 and the lift coefficient Cl 0.35

CASE 2:
R=0.015m, U=0.05m/s, Re=100, f=0.33, T=3s
Timestep 0.001s
Obviously CASE 2 is 3 times larger than CASE 1 in domain size.

Cd is also 1.5 and Cl 0.35.

It is clear that these two cases gave the same result in terms of Cd and Cl. But the confusion is still there. The size of the smallest grid, as m.vegad put it, why is it not affecting the final result?
Attached Images
 domain size.jpg (98.7 KB, 15 views) 0.005.jpg (60.2 KB, 12 views) 0.015.jpg (43.9 KB, 11 views)

 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 andyjo22 Main CFD Forum 2 April 3, 2012 21:43 bengy OpenFOAM 3 May 23, 2011 09:43 Fabio88 OpenFOAM Installation 21 June 2, 2010 03:01 SSL FLUENT 2 January 26, 2008 12:55 zwdi Main CFD Forum 0 March 13, 2004 23:32

All times are GMT -4. The time now is 02:24.