
[Sponsors] 
August 19, 2013, 11:47 
i dont understand: grid validation  laminar flow

#1 
New Member
Diego
Join Date: Jul 2011
Posts: 20
Rep Power: 5 
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? 

August 19, 2013, 12:36 

#2 
Senior Member
Alex
Join Date: Jun 2012
Location: Germany
Posts: 1,097
Rep Power: 19 
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? 

August 19, 2013, 14:08 

#3 
New Member
Diego
Join Date: Jul 2011
Posts: 20
Rep Power: 5 
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. 

August 19, 2013, 15:38 

#4  
Senior Member
Alex
Join Date: Jun 2012
Location: Germany
Posts: 1,097
Rep Power: 19 
Quote:
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 roundoff 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 (10e3 against 10e4). 

August 19, 2013, 16:04 

#5 
New Member
Diego
Join Date: Jul 2011
Posts: 20
Rep Power: 5 
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.


August 19, 2013, 16:58 

#6 
Senior Member
Alex
Join Date: Jun 2012
Location: Germany
Posts: 1,097
Rep Power: 19 
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 for a laminar pipe flow. 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. 

August 19, 2013, 17:08 

#7 
New Member
Diego
Join Date: Jul 2011
Posts: 20
Rep Power: 5 
You're right! thank you very much again.


Tags 
grid validation, laminar flow 
Thread Tools  
Display Modes  


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 