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

Meshing topology for heat transfer over ribs

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

Like Tree2Likes
  • 2 Post By sbaffini

Reply
 
LinkBack Thread Tools Display Modes
Old   August 22, 2013, 11:49
Default Meshing topology for heat transfer over ribs
  #1
Far
Super Moderator
 
Far's Avatar
 
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,971
Blog Entries: 6
Rep Power: 39
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
I am solving "Numerical Simulations of Flow and Heat Transfer over Rib-Roughened Surfaces"

For this purpose I have built type 2 meshing shown in Image 1 (type2 and its closeup view shown in image2). Second reference uses similar case and study the flow and heat transfer over rib-roughened surface using Type 1 meshing as shown in image1.

My question is "Which mesh topology is better".

Reference 1
http://www.ercoftac.org/fileadmin/us...2/case72d.html

Reference 2
http://cfd.mace.manchester.ac.uk/twi...al_CDFSC09.pdf

Type 1 and 2


closeup view of type 2 blocking
Far is offline   Reply With Quote

Old   August 22, 2013, 11:55
Default
  #2
Senior Member
 
Filippo Maria Denaro
Join Date: Jul 2010
Posts: 1,662
Rep Power: 23
FMDenaro will become famous soon enough
I think that the answer depends on the formulation, model and accuracy of the scheme you want to use,...
How about the scales you want to solve? At a first look I would use mesh 2
FMDenaro is offline   Reply With Quote

Old   August 22, 2013, 12:04
Default
  #3
Far
Super Moderator
 
Far's Avatar
 
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,971
Blog Entries: 6
Rep Power: 39
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
I will use finite volume, second order accurate solver (Fluent, CFX or Star CD etc). Turbulence models to be used are K-epsilon and V2F. I need to compare flow variables and nusselt number with the Reference 1 data. I need that CFD data should be highly accurate
Far is offline   Reply With Quote

Old   August 22, 2013, 12:24
Default
  #4
Senior Member
 
Filippo Maria Denaro
Join Date: Jul 2010
Posts: 1,662
Rep Power: 23
FMDenaro will become famous soon enough
Quote:
Originally Posted by Far View Post
I will use finite volume, second order accurate solver (Fluent, CFX or Star CD etc). Turbulence models to be used are K-epsilon and V2F. I need to compare flow variables and nusselt number with the Reference 1 data. I need that CFD data should be highly accurate
That implies to refine very well the boundary layer regions, Nusselt number is very sensitive to resolution near the walls. I stay with the idea of type 2.
Furthermore, BC setting can be quite difficult in terms of modelling variables owing to the series of recirculating region.
How about the range of Reynolds and Peclet numbers? Maybe a comparison with LES in Fluent (dynamic model) can be useful if not computational expensive
FMDenaro is offline   Reply With Quote

Old   August 23, 2013, 06:28
Default
  #5
New Member
 
Jarda Chlup
Join Date: Aug 2013
Posts: 14
Rep Power: 4
Jared1986 is on a distinguished road
Type 2 is better because of angles of elements. This angle is close to 90 degree, what is better for convergence and accuracy of calculation.
Jared1986 is offline   Reply With Quote

Old   August 23, 2013, 06:31
Default
  #6
Far
Super Moderator
 
Far's Avatar
 
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,971
Blog Entries: 6
Rep Power: 39
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
At the sharp corner angle is arond 45 deg.
Far is offline   Reply With Quote

Old   August 23, 2013, 06:53
Default
  #7
Senior Member
 
flotus1's Avatar
 
Alex
Join Date: Jun 2012
Location: Germany
Posts: 1,107
Rep Power: 19
flotus1 will become famous soon enoughflotus1 will become famous soon enough
Personally, I would choose option 2.

Option 1 has some mayor drawbacks
  • much higher number of cells for the same resolution in the interesting part of the flow field
  • cells with high aspect ratio in the free-stream region of the flow
The fact that all cells are rectangular does not compensate for this because the 45 angles of option 2 are still very good.
flotus1 is offline   Reply With Quote

Old   August 26, 2013, 04:22
Default
  #8
Senior Member
 
sbaffini's Avatar
 
Paolo Lampitella
Join Date: Mar 2009
Location: Italy
Posts: 534
Blog Entries: 14
Rep Power: 17
sbaffini will become famous soon enough
I see why option 2 is having more acceptance but:

1) If accuracy is the main concern, especially in the near wall zone (i guess), i don't get how 45 skewed cells can outperform square cells in option 1

2) As the problem seems 2D (and because accuracy is the main concern) the number of cells should not be a problem for option 1. For 3D cases this might not be true and, actually, if i had to perform a LES computation with several cubes, option 2 might be mandatory.

3) For option 1, unnecessary high aspect ratio cells are only present far away from the region of interest. Still, they shouldn't be as problematic as the skewed cells near the walls due to option 2

4) In my experience for this case, turbulence modeling is far more important (go for v2f) as long as the grids are "fine enough"

5) Some numerical options in Fluent might be very sensitive to option 2 grid (e.g., gradient computation method). Hence, if you go for it, you might also want to check for other discretization options; this should be less relevant for option 1. If i remember correctly, CFX uses a node based Finite Volume approach, i don't know if it might have the same problems (but i guess so).

6) Node distribution in case 2 is clearly not optimal, with several jumps in cell size in the most important part of the flow. This is not a judgement on the grid, but an observation on the fact that is far more difficult to create an optimal grid for case 2 than case 1

At the end of the day, if there are no pathological behaviors in the solver (to be checked) i think that, for sufficiently refined grids, both option will eventually give you a sufficiently accurate answer (sufficiently meaning within the accuracy of the turbulence model)
Far and FMDenaro like this.
sbaffini is offline   Reply With Quote

Old   August 30, 2013, 13:20
Default
  #9
Far
Super Moderator
 
Far's Avatar
 
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,971
Blog Entries: 6
Rep Power: 39
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
Solved another example with same mesh topology. some observations are:

1. Mesh topology is good enough

2. decreasing Y+ below 0.5 and doubling the mesh size has no effect on heat transfer calculations

3. SST is bettar than V2F model

4. All other models are not good in predicting heat transfer

Fluent Tutorial on Heat transfer
Far is offline   Reply With Quote

Old   August 30, 2013, 13:59
Default
  #10
siw
Senior Member
 
Join Date: Jul 2009
Posts: 446
Rep Power: 14
siw will become famous soon enough
Far,

Regarding the O-grid in mesh option 2, how did you determine/justify the size of the O-grid in relation to the size of the cube? You say about getting the y+ of 0.5 but can you comment on what the node expansion rate inside the O-grid was and why you chose such a value? Also can you comment on why you chose such large cell area transitions from the last O-grid cells to the first right-angled cells (I've highlighted your image)? Experience and literature for me says that area (or volume in 3D) cell expansion should not be more than 20% (30% at a push).

I'm interested in this topology because I'm looking at something very similar, but not from a heat transfer point of view, for my PhD (3D and completely difference objectives) and I like to justify all my mesh features (node quantities, expansion rates etc). I'm currently running some Fluent cases for my PhD also on the simplest topology, like your option 1.

Thanks
Attached Images
File Type: jpg 1xvt.jpg (60.8 KB, 17 views)
siw is offline   Reply With Quote

Old   August 30, 2013, 14:12
Default
  #11
Far
Super Moderator
 
Far's Avatar
 
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,971
Blog Entries: 6
Rep Power: 39
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
Quote:
Originally Posted by siw View Post
Far,

Regarding the O-grid in mesh option 2, how did you determine/justify the size of the O-grid in relation to the size of the cube? You say about getting the y+ of 0.5 but can you comment on what the node expansion rate inside the O-grid was and why you chose such a value? Also can you comment on why you chose such large cell area transitions from the last O-grid cells to the first right-angled cells (I've highlighted your image)? Experience and literature for me says that area (or volume in 3D) cell expansion should not be more than 20% (30% at a push).

Thanks

yes you are correct expansion should not be more than 20-30%. Maximum mesh expansion inside the o-grid is not more than 1.1-1.2

The mesh shown in pic is not the representative of the mesh i am using in my computations. It was just give to an idea about the mesh topology. The actual mesh i am using is here and you will notice that there is no jump in mesh at any point.







Edit
closeup view of mesh inside the ogrid


Last edited by Far; August 30, 2013 at 14:20. Reason: adding image # 4
Far is offline   Reply With Quote

Old   August 30, 2013, 14:41
Default
  #12
siw
Senior Member
 
Join Date: Jul 2009
Posts: 446
Rep Power: 14
siw will become famous soon enough
Thanks for that Far.

How did you decide on the size for the O-grid or did you leave to the default size when made in ICEM?
siw is offline   Reply With Quote

Old   August 30, 2013, 14:55
Default
  #13
Far
Super Moderator
 
Far's Avatar
 
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,971
Blog Entries: 6
Rep Power: 39
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
Based on just visuall appreance, no calcualtion for boundary thickness is made. But I am sure it will be sufficient

50 layers are used in boundary layer based on my expereince with transition simulations.
Far is offline   Reply With Quote

Old   August 31, 2013, 07:36
Default
  #14
Far
Super Moderator
 
Far's Avatar
 
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,971
Blog Entries: 6
Rep Power: 39
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
Can any body help me in getting article:

Baughn, J.W., Yan, X., 1992. Local heat transfer measurements in square ducts with transverse ribs. ASME National Heat Transfer Conference.
Far is offline   Reply With Quote

Old   November 8, 2013, 01:08
Default meshing of duct flow with ribbed surface 2D
  #15
New Member
 
nilesh
Join Date: Nov 2013
Posts: 1
Rep Power: 0
nilesh purohit is on a distinguished road
hello sir
I am new to ICEM so please help me to mesh the surface properly
please reply me in some what detail as i am fresher to this software
nilesh purohit is offline   Reply With Quote

Reply

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
[ANSYS Meshing] Can I use ANSYS Meshing for manual meshing? Kirjain ANSYS Meshing & Geometry 3 June 12, 2012 08:35
Volume 1 has invalid topology for mapped brick meshing georgewar ANSYS 0 July 24, 2011 16:02
[ANSYS Meshing] Migrating from GAMBIT to ANSYS Meshing David-CFD ANSYS Meshing & Geometry 1 April 1, 2011 05:22
Convective Heat Transfer - Heat Exchanger Mark CFX 6 November 15, 2004 16:55
additional variable mass transfer in CFX5.6 john CFX 1 February 14, 2004 01:30


All times are GMT -4. The time now is 04:56.