[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

[FMDenaro]

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

[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

[FMDenaro]

Originally Posted by 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

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

[Jared1986]

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.

[Far]

At the sharp corner angle is arond 45 deg.

[flotus1]

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.

[sbaffini]

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]

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

http://www.cfd-online.com/Forums/flu...-transfer.html

[siw]

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

[Far]

Originally Posted by siw

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

[siw]

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?

[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]

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.

[nilesh purohit]

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