CFD Online Discussion Forums - [ANSYS Meshing] 3D Multiblock Structured Hexahedral Mesh

CFD Online Discussion Forums (https://www.cfd-online.com/Forums/)

- ANSYS Meshing & Geometry (https://www.cfd-online.com/Forums/ansys-meshing/)

- - [ANSYS Meshing] 3D Multiblock Structured Hexahedral Mesh (https://www.cfd-online.com/Forums/ansys-meshing/104281-3d-multiblock-structured-hexahedral-mesh.html)

3D Multiblock Structured Hexahedral Mesh

This is my first post so hello to all. :)

I am fairly new to the world to CFD and Ansys and as the first part of my project I have to carry out numerical validation of flow across a single cylinder for varying Reynolds number.

I have successfully done the validation upto Re=150 using 2D multiblock structured quadrilateral mesh.

Now I want to extend the mesh in 3D for validating higher Re. But I just can't figure out a way to do a 3D multiblock structured hexahedral mesh in Ansys Meshing.

This is the mesh which I am looking for.
Front view:
http://i.imgur.com/EEyfh.png

Cut section top view:
http://i.imgur.com/4d038.png

Any pointers how to achieve it?

P.S.:
These are the steps which I have done so far:
1. Created the 3D geometry in Ansys DesignModeler.
http://i.imgur.com/3Xfew.png

2. Imprinted lines on the faces of the enclosing box in Ansys DM to facilitate edge sizing.
http://i.imgur.com/fBPT8.png

3. Used Mapped Face Method for all the surfaces in Ansys Meshing and specified edge sizing on different lines and edges.
http://i.imgur.com/Wt2jG.png

4. Cut section view of the mesh generated.
http://i.imgur.com/A64P0.png

The easiest way to achieve a "multiblock structured hexahedral" mesh in ansys meshing is to section the geometry in the design modeler.

Just model the "blocks" of your mesh as individual geometries.

It works fine for the cylinder, I already did the same thing.

But since this is quite a workaround, I recommend you learn ICEM if you ever want to mesh more complex geometries.

Quote:

Originally Posted by flotus1 (Post 370042)

The easiest way to achieve a "multiblock structured hexahedral" mesh in ansys meshing is to section the geometry in the design modeler.

As Alexander said you need to block your geometry in DM. You can use the slice option available in DM, I explained this method for a C-grid in a Ubend geometry. In your case is quite easilly done, more time consuming (took me 15min) than doing it in 5 min with ICEM but if you don't have access/time to learn ICEM you can still use AM.

I've uploaded some pictures of a similar geometry of yours (I didn't know the exact dimensions). Then you just need to play around with the sizing functions in order to have the desired mesh.

I can upload the WB.zip but I'm using V14 so if you are working with an older version you won't be able to open it, just let me know.

Thank you all for your suggestions and help.

I did manage to create individual blocks in Ansys DM (as frozen) and mesh it individually in Ansys Meshing with the required edge sizing.
http://i.imgur.com/jEvIZ.png

But now the problem is when I open the mesh in Ansys Fluent it gives a series of warning saying:
"Flow boundary zone xx is adjacent to a solid zone (y). This problem MUST be fixed before solution can proceed!"
(where xx & y are boundary zone numbers and solid zone numbers)

In the Boundary Conditions tab a single Named Selection is being split up into 2 parts in Fluent for e.g. inlet is being split up into inlet-part_1-solid and inlet-part_1-solid.1. (exception are backwall and frontwall)
http://i.imgur.com/L6WCu.png

My hunch is that the contacting faces of the blocks in the geometry is creating the problem. I tried changing the type for wall-part_1-solid to "interior" but it gave an error saying:
"Cannot change wall-part_1-solid to interior because adjacent cell threads are of different types."

How to overcome this problem in Fluent?

@Far: Thanks for the video links. Due to time constraint I am forced to use Ansys Meshing for the current project. Maybe in future I would start learning Ansys ICEM. Do you have any good tutorials for beginners?

@Gweher: I am using Ansys v13.

This is just a guess because I cant try it right now:

Are all cell threads defined as fluid zones in fluent? (check this under "cell zone conditions") Maybe there is a solid zone left which cannot form an interior boundary with the fluid zones.

Did you group the parts in the design modeler? Maybe this could help.

Just out of curiosity: Why do you use different grid spacings in z-direction?

Your guess was correct flotus1. Some of the extruded blocks were of type solid while others were of type fluid in Ansys DM. After I changed all of them to type fluid, neither Fluent didn't give any warning and nor were the Named Selection faces split up.

Quote:

Just out of curiosity: Why do you use different grid spacings in z-direction?

To decrease the number of cells since I would be monitoring the flow parameters only on the XY plane passing midway through the block.

I thought of having finer mesh near the cylinder so I used a bias in the edge sizing on the radial egdes.
http://i.imgur.com/OoNJD.png

But the mesh created in that region is no more a structured hexahedral mesh.
http://i.imgur.com/hcRYV.png

I have successfully done the same thing for the 2D case. Any idea why is it not happening for 3D case?

Did you apply a "structured mesh" to the surfaces?
Did you set the "behavior" of the edge sizings to "strict"?

For the 3D-geometry: Unless the walls in z-direction are no-slip-boundaries, there is no need to use a 3D-mesh.
The results will be identical on a 2D-mesh with any RANS-based approach.

Quote:

Originally Posted by flotus1 (Post 370231)

Did you apply a "structured mesh" to the surfaces

Yes I had right-clicked on the geometry and selected "Select all faces" while selecting the faces for applying the "Mapped Face Method".

Quote:

Originally Posted by flotus1 (Post 370231)

Did you set the "behavior" of the edge sizings to "strict"?

Yes the "Behavior" of all the Edge Sizing Functions are set to "Hard"

Quote:

Originally Posted by flotus1 (Post 370231)

For the 3D-geometry: Unless the walls in z-direction are no-slip-boundaries, there is no need to use a 3D-mesh.
The results will be identical on a 2D-mesh with any RANS-based approach.

Well I have read in literature that for a flow across cylinder after Re~180 the nature of vortex shedding becomes oblique instead of being parallel and hence it is 3 dimensional in structure. That's why I want to use a 3D mesh instead of 2D.
[Ref]C.H.K.Williamson - Oblique and parallel modes of vortex shedding in the wake of a circular cylinder at low Reynolds numbers

Although I don't know how significantly does the change in the nature of vortex shedding affects the frequency of vortex shedding and heat transfer but if you say that the results will be identical then I would better go with 2D mesh because I am not keen on studying the end condition of the cylinder.

You need 3d mesh for Re > 180 due to 3d nature of flow. It is good idea that you can check your mesh for 2d and 3d cases for Re< 180.

How many diameters you are taking in 3rd dimension? Try to search some references that what should be 3rd dimension in terms of dia of cylinder.

You can make the mesh independence study for x-y coordinates for the Re< 180 and therefore for Re>180 you just check the mesh requirements in the Z-direction.

I haven't finalized the dimensions in the spanwise direction (Z-axis) yet but the domain which I have chosen right now has a depth of 40D (D=Diameter of cylinder).

In this report on St-Re relationship they have conducted experiments with cylinders having L/D>50:
A new Strouhal–Reynolds-number relationship for the circular cylinder in the range 47<Re<2×105

By the way do you have any idea of how big or small the time step should be?

Reference 1 (When to perform domain size, mesh density and time step study)
http://www.tfd.chalmers.se/~lada/pro.../proright.html

Quote:

DNS is used to investigate the fluctuating forces acting on a circular cylinder at Re=50~1000, using CALC. For Reynolds number lower than 200, 2D simulations are carried out for evaluating the numerical method regarding to domain size, mesh density, time step, and so on.

Reference 2 (For span wise depth)
http://www.iawe.org/Proceedings/5EACWE/103.pdf

Quote:

To adequately resolve the flow, an O-type body-fitted grid system is used. The computational
domain is basically 30D on the circular plane by 4D in the spanwise direction for all Reynolds
numbers, but the spanwise domain is 8D for Re=200. The vortex instability experiences mode change
in the Reynolds number range of 50<Re<1000, and one feature of mode A instability at Re=200 is the
4D wavelength structure in the wake in the spanwise direction. Therefore, the computational domain
in the spanwise direction is set to 8D for Re=200 in order to illustrate mode

Reference 3 (Time step and other details)
http://www.cfd-online.com/Forums/ans...cylinders.html

Quote:

Originally Posted by Far (Post 340398)

First domain extend: Either take these values from good paper or try: 10 dia upstream and 20 dia downstream, 15 dia up and 30 down and 20 dia up and 40 down. or may be 25 up and 35 down as taken in this post http://www.cfd-online.com/Forums/flu...ou-reward.html. You should understand the basic idea, which is to avoid the reflections from the boundaries.

Mesh Sensitivity This can done by refining the mesh size by factor of 1.44 in each direction (that is equivalent to doubling the overall mesh size). Create at least three meshes and then compare the important parameters and if you see that values between two meshes are not changing then you have achieved the mesh Independence and you can use the mesh with less no of nodes from these two grids.

Time step This depends upon the frequency of vortex shedding. The frequency of vortex shedding can be determined from the Strouhal no for that particular Reynolds no. See this Fig. http://img341.imageshack.us/img341/7...exshedding.pngand this one http://en.wikipedia.org/wiki/File:Srrrpd.png

Strouhal no. is defined as $St = \frac{fL}{L}$
where St is the dimensionless Strouhal number, f is the frequency of vortex shedding, L is the characteristic length (for example hydraulic diameter) and V is the velocity of the fluid [Ref :http://en.wikipedia.org/wiki/Strouhal_number

From this formula you can get the idea of the shedding frequency (be careful: You need to calculate the Strouhal no. from the shedding frequency found from the FFT (see below) and compare to experimental St no. For all three meshes to see what is happoing while refining the meshes with this important parameter) For example if St no. is 0.18 and velocity is 1 m/s and L = 1 m. Therefor shedding frequency is 0.18 and time to pass one frequency is
$\frac{1}{f} = \frac{1}{0.18}= 5.5 sec$
Now you decide in how many time steps you want the reach this time. For example if you take 25 steps then your time step would be 0.22. This imply you are resolving one cycle in 25 steps ( 25*.22 = 5.5 seconds).
You may start with 25 steps and double for each time step sensitivity analysis. This look like time step = .22 (25 time steps) , 0.11 (50 time steps) and 0.055 (100 time steps)

Yes.

Create points along the periphery of circle with the interval of 5 deg (or less depending upon the resolution requirements) and then get the values on these points. For this use surface integral and apply vertex averaging.

Use the lift coefficient graph and then take the FFT available in Fluent. From that graph the dominate frequency is the shedding frequency and strouhal no. can be found from the above formula. OR create the point at some downstream point (may be at x= 1.5 and Y = 0.5) and create surface monitor (Choose velocity as variable and apply vertex averaging) and apply FFT on these values. Caution: Do not change any parameter when recording these files other wise data may not valid for FFT analysis.

This may be due to the fact that your mesh is not capturing the vortex shedding and therefore you are getting the converged steady state solution, while other mesh is capturing the vortex shedding and hence giving you the oscillating steady solution, which clearly shows that you need to run this case as transient.

Use double precision solver.

Quote:

Originally Posted by flotus1 (Post 370231)

For the 3D-geometry: Unless the walls in z-direction are no-slip-boundaries, there is no need to use a 3D-mesh.
The results will be identical on a 2D-mesh with any RANS-based approach.

Well, flotus1 is not saying that you must use 2d mesh rather he is saying that if you use the slip wall in z-direction than results will be identical to 2d case due to zero velocity gradient and shear stress in lateral direction.

Thanks Far for the elaborate description. As a coincidence I had stumbled upon this post of yours while browsing the net before I signed up on cfd-online. :)

Quote:

Originally Posted by Far (Post 370330)

So if I am interested only in calculating the Strouhal's number and heat transfer coefficient without considering the effect of the bounding walls I may use 2D mesh to save on computational resources without losing accuracy right?

As always, it depends...

If you want to simulate the flow past the cylinder using a LES or even a DNS approach, you will need a 3-dimensional mesh. In this case, there are a lot of other things to worry about when setting up the case, the structure of the mesh is just one of these issues.

But if you are using a turbulence model based on a RANS-approach (like k-epsilon for example) and there is no gradient of the mean velocity along the z-axis, the results will be the same on a 2D and a 3D mesh.
And yes, a strouhal number can be obtained with an unsteady RANS simulation.
The heat transfer will be in rather poor agreement with experimental data in this case, since the intrinsic assumptions of the RANS-approach are not necessarily fullfilled in a detached flow.

Quote:

Originally Posted by zeo (Post 370036)

good one....

hi to all.. am new to ansys 13.0 ... i finished the vortex shedding problem in fluent 6.3.. now i want to do it in ansys 13.0... am unable to create the geometry in DM... i need step by step tutorial.... thanks in advance...

Hi All,

I've split the main block into smaller blocks by using the extrude>add frozen method in DM. However when I go into Fluent, it shows that there are multiple walls at the boundary conditions.

May I know is this the correct method to split the main block into smaller blocks? If so will the multiple walls shown under the boundary conditions in Fluent affect the results?

Thanks!

Regards,
Hee

I think you should get rid of the "surface body" and the non-frozen solid body in DM before proceeding.

Now the next step depends on the type of interface you want between the blocks.

Method 1: non-nonformal interface
Proceed with the multiple independent frozen bodies.
This allows you to mesh every block independently. However, you will get an interface between each block which affects your results.

Method 2: conformal interface
Select all the bodies, right-click and "form new part".
There will be no additional interfaces created in fluent since the mesh transition between the blocks is conformal.

I've got it, thanks so much for your quick response!

Another question is that which model should i use in FLUENT to simulate an airflow of Re= 10,000? Is there any reference materials which i can refer to to obtain information such as boundary conditions settings (intensity & viscosity ratio), solution methods, time-step sizing and etc?

Thanks!

Regards,
Hee

Sorry for jumping in :

Quote:

you will get an interface between each block which affects your results

i have to deal with a very complex geometry, i like to mesh that in hexa. so i sliced and mesh each block and i'm planning to do use non-conformal mesh to join them together. Do you have any additional source about how bad they can be, limitation ? other than the fluent tutorial. Thanks a lot

hi , would u mind sending me wb.zip too?

cylinder with finite length

Hi everyone,

I would like to make a 3d mesh with a circular cylinder in it, but the cylinder has a finite length, so it doesn't "touch" the boundaries of the domain. I don't know how to create a mesh above and below the cylinder.

Anyone has some idea about his?

Thanks

cylinder with finite length

Hi darazsbence,

I know its late but just wanted to show a couple of meshing methods (for future). Even if it has finite length, you can mesh it the exact same way as mentioned above. But assuming you have another body other than the cylinder (cylinder+body) in the domain, then the basic idea for a mesh is shown in the attached pictures.

Best,
Rahul

hi, can i know the step to do those meshing? when i use multizone, i got an error which is found free block in swept body. I am doing with a sphere instead of cylinder

Hi Karl,

Multizone is not a magic option that will automatically generate a hexa mesh for all geometries. Here the error is quite obvious "found free block in swept body". You need to partition your geometry using slice planes in order to help the mesher and successfully achieve the mesh you want. I would recommend you to look at tutorials on blocking strategies to gain more insights on how to partition your geometries.

Have fun ;)