# i dont understand: grid validation - laminar flow

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

August 19, 2013, 11:47
i dont understand: grid validation - laminar flow
#1
New Member

Diego
Join Date: Jul 2011
Posts: 21
Rep Power: 8
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
 Figure 1.png (31.4 KB, 16 views)

 August 19, 2013, 12:36 #2 Senior Member     Alex Join Date: Jun 2012 Location: Germany Posts: 1,532 Rep Power: 25 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.

August 19, 2013, 14:08
#3
New Member

Diego
Join Date: Jul 2011
Posts: 21
Rep Power: 8
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
 Figure 2.png (15.2 KB, 9 views) Figure 3.jpg (100.4 KB, 8 views) Figure 4.jpg (31.8 KB, 12 views)

August 19, 2013, 15:38
#4
Senior Member

Alex
Join Date: Jun 2012
Location: Germany
Posts: 1,532
Rep Power: 25
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).

 August 19, 2013, 16:04 #5 New Member   Diego Join Date: Jul 2011 Posts: 21 Rep Power: 8 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: 1,532 Rep Power: 25 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. rayan24 likes this.

 August 19, 2013, 17:08 #7 New Member   Diego Join Date: Jul 2011 Posts: 21 Rep Power: 8 You're right! thank you very much again.

 Tags grid validation, laminar flow

 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 Blasius_Pohlhausen_Crocco Main CFD Forum 12 September 30, 2013 17:35 JuPa CFX 7 September 9, 2013 07:45 mozafarie FLUENT 0 March 11, 2013 14:42 shashwat Main CFD Forum 0 April 4, 2008 02:20 diaw Main CFD Forum 104 February 16, 2006 06:44

All times are GMT -4. The time now is 13:11.