1. Introduction
In this tutorial we will present the simulation of wind flow around the buildings. Aerodynamic of the building is a growing challenge in today’s construction industry. Here we will present one of the possible way of analysing the wind flow through the urbanized areas.
An important aspect of this problem is the proper modeling of the boundary conditions. We will use specially dedicated boundary condition for the inlet - Atmospheric Inlet. It defines the flow profiles of mean wind speed and turbulence quantities that are applied in the inlet plane. These profiles model fully developed and representative of the terrain characteristics of the upstream part that is not include in the computational domain.
Finally, we will read the wind velocity which may affect pedestrians between the building. We will display the pressures on buildings that may affect their construction.
2. Download SimFlow
SimFlow is a general purpose CFD Software
To follow this tutorial, you will need SimFlow free version, you may download it via the following link:
Download SimFlow
3. Create Case
Open SimFlow and create a new case named buildings
Go to New panel
Provide name buildings
Click Create Case

4. Import Geometry
Firstly, we need to Download GeometryBuildings
The geometry will be imported in the same units as it was exported to the STEP format.
Click Import Geometry
Select geometry file buildings.step
Click Open

5. Import Geometry II
In some cases, the imported external geometry may contain multiple parts. SimFlow will ask you whether you want to join all geometries into a single component. If not, each part will be put into separate items.
For the purposes of this tutorial, we will combine all parts into a single geometry.
Press Yes button

6. Geometry - Buildings
After importing geometry, it will appear in the 3D window.
Click Fit View to zoom in on the geometry

7. Create Geometry - Refinement
To be able to better resolve flow around the buildings, we will create an area with a higher mesh resolution. To do this, we will add box geometry.
Select Create Box
Change geometry name from box_1 to refinement
Set the origin and box dimensions
Origin \({\sf [m]}\)-20-800
Dimensions \({\sf [m]}\)25016085

8. Meshing Properties - Buildings
After geometry is ready, we can proceed to define meshing properties. To better resolve the flow around the buildings, we want to refine mesh near the buildings geometries by specifying minimum and maximum refinement levels.
Go to Hex Meshing panel
Select buildings geometry
Enable Meshing Geometry
Set the minimum and maximum refinement level
Refinement Min 2 Max 4

9. Meshing Parameters - Refinement
The refinement geometry should be used only for marking refinement zones. Set the proper parameters for the refinement regions.
Click on the refinement geometry
Enable Refine Geometry
Set the refinement Level to 1

10. Base Mesh
Base Mesh is a domain mesh of our simulation from which the final mesh will be created by carving out the geometry of the buildings.
Go to Base tab
Define base mesh parameters accordingly
Min \({\sf [m]}\)-300-3000
Max \({\sf [m]}\)500300400Set the division of the base mesh and its grading
Division322418
Grading113

11. Base Mesh Boundaries
We need to assign individual names to each side of the base mesh in order to be later able to define different conditions on each side. To achieve simplified slip condition on side and top boundaries we will use symmetry as a boundary type.
Define boundary names accordingly
X- inlet
X+ outlet
Y- right
Y+ left
Z- bottom
Z+ topDefine boundary types accordingly
Y- Symmetry
Y+ Symmetry
Z- Wall
Z+ Symmetry

12. Material Point
Material Point tells the meshing algorithm on which side of the geometry the mesh is to be retained. We are simulating flow around the buildings so our material point needs to be located inside the base mesh but outside the buildings.
Go to Point tab
Specify location inside base mesh but outside buildings geometries
Material Point00160

13. Start Meshing
Everything is now set up for meshing.
Go to Mesh tab
Press the Mesh button to start meshing process

14. Mesh
The new mesh will be displayed in the graphics window. To show the mesh of the buildings we can use the Graphics Object List to hide some boundaries.
Click Graphics Object List icon
Select Mesh to show meshes list

15. Mesh - Toggle Visibility
You can hide domain boundaries to inspect the mesh on the buildings.
Hide the following objects
inlet
left
outlet
right
top

16. Select Solver - SIMPLE
We want to analyze incompressible turbulent flow around the buildings. For this purpose, we will use the SIMPLE (simpleFoam) solver.
Go to Setup panel
Enable Steady State filter
Enable Incompressible filter
Select SIMPLE (simpleFoam) solver
Select solver

17. Turbulence
We are going to use the \(RNG \; k{-}\epsilon\) model to handle turbulence.
Go to Turbulence panel
Select turbulence model
Turbulence Modelling RANSChange default turbulence model
Model \(RNG \; k{-}\epsilon\)

18. Boundary Conditions - Inlet
On the inlet boundary, we are going to apply Atmospheric Inlet boundary condition. It is dedicated condition for atmospheric airflow. The Atmospheric Inlet provides log-law type ground-normal inlet boundary conditions for wind velocity and turbulence quantities. It is applied for homogeneous, two-dimensional, dry-air equilibrium and neutral atmospheric boundary layer modelling. More about Atmospheric Inlet boundary condition you can find here.
Go to Boundary Conditions panel
Select inlet boundary
Change boundary character to Atmospheric Inlet
Set the velocity
\(U_{ref}\) \({\sf [m/s]}\)5

19. Monitors - Sampling (I)
During the calculation, we can observe intermediate results on a section plane. To add sampling data on a plane we need to define plane properties and also select fields that will be sampled. We will monitor the pressure and velocity at a height of 2 metres from the ground. Note that runtime post-processing can only be defined before starting calculations and can not be changed later on.
Go to Monitors panel
Switch to Sampling tab
Select Create Slice
Set slice plane location
Point \({\sf [m]}\)002

20. Monitors - Sampling (II)
Now, create a vertical slice.
Select Create Slice
Set slice normal vector
Normal \({\sf [-]}\)010

21. Monitors - Sampling (II)
Now, specify which results should be sampled on the section planes.
Expand Fields list
Select pressure p and velocity U

22. Run - Time Control
Finally, we can start our computation.
Go to RUN panel
Set the maximum Number of Iteration to 500

23. Run - CPU
To speed up the calculation process increase the number of CPUs basing on your PC capability. The free version allows you to use only 2 processors in parallel mode. To get the full version, you can use the contact form to Request 30-day Trial
Estimated computation time for 2 processors: 4 minutes
Switch to CPU tab
Use parallel mode
Increase the Number of processors
Click Run Simulation button

24. Residuals
When the calculation is finished we should see a similar residual plot.

25. Slice - Velocity Field
Slices tab appears next to the Residuals tab. Under this tab, we can preview results on the defined section plane.
Change tab to Slices
Select the velocity U
Click Adjust range to data
Click Graphics Object List icon
Select GEOMETRIES and show the buildings

26. Postprocessing - ParaView
After computations are finished, we can do complex visualization of our results with ParaView.
Go to Postprocessing panel
Start ParaView

27. ParaView - Load Results
Load the results into the program.
Make sure you have your case selected buildings.foam
Click Apply to load results
Select contour coloring variable to U
Click Last Frame to load the final result set
After loading results they will be shown in the 3D graphic window

28. ParaView - Clip
To limit the investigation area we will Clip the domain by the box.
Select Clip option
Change the Clip Type to Box
Enter box parameters accordingly
Position8000
Rotation000
Scale0.50.30.1Click Apply

29. ParaView - Velocity Field
Now we will create velocity magnitude parameter. It will be helpful in scaling and coloring the velocity vector field.
Make sure you have Clip1 field selected
Select Calculator
Type the magU as Result Array Name
Type the formula mag(U)
Click Apply

30. ParaView - Velocity Field Settings
To visualize the flow around the building we will create vector field.
Make sure you have Calculator1 field selected
Select Glyph option
Set the scale factor to 2
Change the Maximum Number Of Sample Points to 2000
Click Apply
Hide the Calculator1 field
Click Rescale to Data Range

31. ParaView - Import Geometry (I)
To display results with the original geometry, we can import the case once again and select only suitable boundaries. Now, we will import the buildings and the ground boundaries.
Click Open
Select the buildings.foam file from the case directory …/buildings/buildings/buildings.foam
Click OK button

32. ParaView - Import Geometry (II)
Check bottom and buildings instead internalMesh boundary
Click Apply button to show the geometry
Set the coloring as Solid Color

33. ParaView - Display Velocity Field
Now we can see the velocity vector field around the buildings.

34. ParaView - Pressure on Buildings (I)
To display pressure on the buildings we need to hide vector field and change the coloring to the pressure.
Hide the Glyph1
Select buildings.foam field (with the buildings and ground boundaries)
Change the coloring set to pressure p

35. ParaView - Pressure on Buildings (II)
Pressure field is displayed on the selected boundaries.
