# Mesh refinement

 User Name Remember Me Password
 Register Blogs Members List Search Today's Posts Mark Forums Read

 LinkBack Thread Tools Display Modes
May 16, 2010, 05:19
Mesh refinement
#1
New Member

Join Date: Apr 2010
Posts: 6
Rep Power: 7
To understand mesh refinement concepts I modelled a pipe (10 mm dia, 500 mm long) having three flow velocities (4, 6 and 8 m/s, water as fluid). Mesh refinement was carried out in the 2 mm thick layer by changing no of elements in the layer. Four runs were taken with no of elements 5, 7, 9 and 11. The mesh was generated in such a way that element thickness is smallest near the wall and gradually increases towards the centre. Figure shows the typical grid profile showing 11 elements in 2 mm thick layer.

Fig-1

The analysis was carried out using k-e model with scalable wall function. (As a rule, none of the defaults were changed). Inlet temperature for water was 300 K. Wall temperature was 373 K.
Values for y+ and wall heat transfer coefficient (hf) were noted at a distance of 400 mm from entry. Line averaging was carried out.
Inlet pressure was also noted (using ‘area averaged’ tool). Outlet pressure was set 0 Pa.

Figure shows variation in y+ as a function of number of elements (at a plane 400 mm from inlet).

Fig-2

Figures show variation in heat transfer coefficient (at a plane 400 mm from inlet) and inlet pressure as a function of number of elements.

Fig-3 and Fig-4

Doubts:-
- Can I consider that I have obtained mesh convergence with 5 elements? The two important parameters ‘heat transfer coefficient’ and ‘pressure drop’ remain practically unchanged.
- Should I be greedier and try to use even less than 5 elements say 3 or 4 in the 2 mm thick layer near wall?
Attached Images
 Fig-1.jpg (96.0 KB, 41 views) Fig-2.jpg (30.5 KB, 32 views) Fig-3.jpg (27.8 KB, 29 views) Fig-4.jpg (30.6 KB, 28 views)

 May 16, 2010, 05:32 #2 New Member   Wei Zhao Join Date: Mar 2010 Posts: 28 Rep Power: 7 i think it is based on your requirement for the problem.

 May 16, 2010, 18:40 #3 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 10,826 Rep Power: 85 Wei is right. It depends on what you want to do. If you are trying to do the world's most accurate CFD simulation of pipe flow then you are not even close. If you are doing an approximate engineering analysis and errors of 10% are OK then you are fine. So the mesh you require is also a function of how accurate your results need to be.

May 16, 2010, 21:15
#4
New Member

Join Date: Apr 2010
Posts: 6
Rep Power: 7
Thank you both Mr. Wie and Mr. Horrocks,

I am sorry I should have indicated the desired accuracy. But for an average engineer like me, I consider 10% to be quite good. I have additional doubts:-

1. I tried to plot relations between hf=f(v), shown in Fig-5 and Del-P=f(v), shown in Fig-6.
2. I am used to hf to be having a power law of 0.8 (The good old Dittus-Boelter) and Del-P following a square law. Fig-5 shows a power law with n=0.863 (in place of 0.8) while Fig-6 shows a power law with n=1.792 (in place of 2).

What is the explanation for the mismatch? Is it lack of mesh refinement or the fact that the experimental correlations are valid over far too large a data and may not be strictly valid over the small calculation set done by me).

With best regards,
Dev325
Attached Images
 Fig-5.jpg (26.6 KB, 23 views) Fig-6.jpg (25.7 KB, 16 views)

 May 16, 2010, 21:27 #5 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 10,826 Rep Power: 85 Could be lots of reasons. Firstly look at your simulation - check mesh and convergence sensitivity. Secondly look at what the empirical correlations actually mean - is it for fully developed flow? Was the flow fully developed in your simulation? You have to make sure you are modelling exactly what the correlation assumes. And finally many of these empirical correlations are approximateions anyway. They are only good to within 10% or so anyway, and the heat transfer ones it is more like 50%. Refer to the original papers to find out exactly how accurate they are. Don't expect them to be precise.

May 17, 2010, 14:59
#6
New Member

Join Date: Apr 2010
Posts: 6
Rep Power: 7
Dear Mr. Horrocks,

Thank you for pointing out the slip of not checking the fact if the flow has fully developed or not. I carried out the check by doing analysis for 10 mm dia pipes with lengths 500 mm and 1000 mm. The mesh height is identical for both cases. The hex mesh layout is also identical.

I plotted variation of flow velocity at the centre line of the pipe. (Fig-7). I also noted wall heat transfer coefficient at a uniform step height of 100 mm from inlet till outlet. (Fig-8).

Can the flow velocity plot be considered correct? Why should the flow velocity overshoot the so called "stable" value and then drop back?

In my opinion flow has fully developed. But ideally if values at 400 mm and 900 mm are compared, the values at 400 mm are slightly incorrect. In future I should consider a pipe length of at least 700 mm for such an analysis.

I shall also analyse other aspects pointed out by you.

Thanking you and with best regards,
Dev325.
Attached Images
 Fig-7.jpg (41.6 KB, 17 views) Fig-8.jpg (40.7 KB, 12 views)

May 17, 2010, 18:37
#7
Super Moderator

Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,826
Rep Power: 85
Quote:
 Why should the flow velocity overshoot the so called "stable" value and then drop back?
Have a look at how the inlet boundary condition (which is probably plug flow, ie constant velocity over the whole patch) transitions to fully developed flow and the boundary layers develop. That is where the overshoot comes from.

 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 adona058 OpenFOAM Running, Solving & CFD 6 October 23, 2009 09:17 lr103476 OpenFOAM Running, Solving & CFD 30 November 19, 2007 15:09 Joe CFX 2 March 26, 2007 18:10 Korsh Mik CFX 0 January 11, 2006 08:07 Mark CFX 3 October 14, 2004 21:18

All times are GMT -4. The time now is 17:41.

 Contact Us - CFD Online - Top