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

i dont understand: grid validation - laminar flow

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

Like Tree3Likes
  • 1 Post By flotus1
  • 1 Post By flotus1
  • 1 Post By flotus1

Reply
 
LinkBack Thread Tools Display Modes
Old   August 19, 2013, 11:47
Default i dont understand: grid validation - laminar flow
  #1
New Member
 
Diego
Join Date: Jul 2011
Posts: 20
Rep Power: 5
Diegoesteban is on a distinguished road
in order to validate a grid to simulate the laminar flow in a pipe (2D, diameter=5 cm, lenght=50 cm, inlet velocity=0.1 m/s), I have used five different grids:

Case 1: 40 elements
Case 2: 168 elements
Case 3: 1000 elements
Case 4: 25021 elements
Case 5: 156250 elements


I expected that for the denser grid (case 5), I would get the most accurate solution. However, by plotting the velocity profile (at a distance x = 50 cm, having verified that the flow is already developed) I saw the result in Figure 1. According to these results, case 3 would be the most appropriate since the parabolic profile. Why the best result corresponds to an intermediate grid? Did not I should get the best result for denser grid?
Attached Images
File Type: png Figure 1.png (31.4 KB, 16 views)
Diegoesteban is offline   Reply With Quote

Old   August 19, 2013, 12:36
Default
  #2
Senior Member
 
flotus1's Avatar
 
Alex
Join Date: Jun 2012
Location: Germany
Posts: 1,097
Rep Power: 19
flotus1 will become famous soon enoughflotus1 will become famous soon enough
What is the Reynolds number in your simulation?
Are you sure that your solutions are converged?
What does your mesh look like? I mean in which direction did you refine the mesh?
Diegoesteban likes this.
flotus1 is offline   Reply With Quote

Old   August 19, 2013, 14:08
Default
  #3
New Member
 
Diego
Join Date: Jul 2011
Posts: 20
Rep Power: 5
Diegoesteban is on a distinguished road
First of all, thank you very much for answering.
The reynolds number is around 340.
Respect to convergence, I first used residual values ​​= 0.001, and then 0.0001. Convergence is always achieved.
Figures 2 and 3 show respectively mesh parameters and a printing of the mesh.
Figure 4 shows the average velocity at x = 50 cm, variable chosen to validate the mesh. According to Figure 4, the mesh is not yet validated (although I think it is sufficiently dense), but according to Figure 1, the Case 3 is the one that coincides with the expected solution.
Attached Images
File Type: png Figure 2.png (15.2 KB, 9 views)
File Type: jpg Figure 3.jpg (100.4 KB, 8 views)
File Type: jpg Figure 4.jpg (31.8 KB, 12 views)
Diegoesteban is offline   Reply With Quote

Old   August 19, 2013, 15:38
Default
  #4
Senior Member
 
flotus1's Avatar
 
Alex
Join Date: Jun 2012
Location: Germany
Posts: 1,097
Rep Power: 19
flotus1 will become famous soon enoughflotus1 will become famous soon enough
Quote:
The reynolds number is around 340.
Thats the problem.
With a Reynolds number this high, the flow is not fully developed after a length/height ratio of 10.
The velocity profile is still influenced by the profile at the inlet, which is a uniform profile I guess.

The reason why the solution at intermediate mesh resolutions appears to be the best one is the numerical diffusion caused by the coarse mesh.

You can either decrease the Reynolds number, apply a velocity profile at the inlet or use periodic boundaries between inlet and outlet to obtain a solution which meets your expectations.

Another issue: if you want to compare double to single precision results, you should run both simulations until the round-off accuracy of the machine is reached, indicated by the residuals leveling out. The way you did it you compare the influence of the residual criterion (10e-3 against 10e-4).
Diegoesteban likes this.
flotus1 is offline   Reply With Quote

Old   August 19, 2013, 16:04
Default
  #5
New Member
 
Diego
Join Date: Jul 2011
Posts: 20
Rep Power: 5
Diegoesteban is on a distinguished road
Thank you for your help! I thought that the Reynolds number was low enough to consider that the flow is not fully developed. So I have no reason to expect a parabolic velocity profile.
Diegoesteban is offline   Reply With Quote

Old   August 19, 2013, 16:58
Default
  #6
Senior Member
 
flotus1's Avatar
 
Alex
Join Date: Jun 2012
Location: Germany
Posts: 1,097
Rep Power: 19
flotus1 will become famous soon enoughflotus1 will become famous soon enough
Dont get confused here: with a low Reynolds number (high viscous forces) the flow profile develops faster.
There is even an analytical relation between the Reynolds number and the entrance length L_E for a laminar pipe flow.

L_E \approx 0.06 \text{Re}

Note that this only holds for the flow in a circular pipe.
For the flow between parallel plates (which I think is what you are modeling) the entrance length is even higher because the ratio of surface to volume is lower than in a circular pipe.
rayan24 likes this.
flotus1 is offline   Reply With Quote

Old   August 19, 2013, 17:08
Default
  #7
New Member
 
Diego
Join Date: Jul 2011
Posts: 20
Rep Power: 5
Diegoesteban is on a distinguished road
You're right! thank you very much again.
Diegoesteban is offline   Reply With Quote

Reply

Tags
grid validation, laminar flow

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
Boundary Layer of Laminar Flow over a Flat Plate Blasius_Pohlhausen_Crocco Main CFD Forum 12 September 30, 2013 17:35
Ratio of eddy viscosity to molecular viscosity : Laminar or turbulent flow? RicochetJ CFX 7 September 9, 2013 07:45
laminar and turbulent flow in two regions mozafarie FLUENT 0 March 11, 2013 14:42
Can 'shock waves' occur in viscous fluid flows? diaw Main CFD Forum 105 November 20, 2009 05:19
Validation for laminar Disperse phase flow shashwat Main CFD Forum 0 April 4, 2008 02:20


All times are GMT -4. The time now is 08:16.