Fume extraction simulation tutorial
Fume extraction is an important topic for the environmental health in a city. A Computational Fluid Dynamics simulation can effectively calculate the effectiveness of the solution chosen and predict in a reliable way the fume pattern and whether it will hit other buildings or affect pedestrians. Once this phase is completed it is possible to fine tune the fume extraction system to minimise the impact on surrounding buildings or people.
Fume extraction CFD simulation definition in SimWorks
The fume extraction tutorial will simulate a typical fume extraction system in an urban environment with 2 kitchen extraction tubes and will calculate the fume pattern and how those affects the surrounding buildings. Two different extraction tubes geometries will be assessed, the first one is a curved exit pointing down, the second one is a classic straight chimney solution with the exit placed 1m above the building roof.
The simulation is going to be carried out with a 3m/s wind, which corresponds to the average wind speed in London. The wind angle to the buildings will be 15°.
Define the simulation
- As already seen in the SimWorks advanced introduction tutorial define a new project, geometry and simulation
- Rename them as Fumes investigation, Exit geometries and Curved exit respectively
- Load the Fumes_extraction_curved.igs file
- Enable the Passive scalar option to be able to trace the fumes dispersion
- Define a maximum number of iterations of 500 and number of processes of 4
- Define a outer domain with Dimensions 100,70,25 and Position 0,0,12.5 to simulate an adequate portion of space around the buildings
- Define a Rotation angle around z of 15°, this simulates the wind incidence to the buildings
- The OD left face will be the inlet with a Velocity Normal boundary condition with speed 3 m/s
- Define a Pressure Outlet boundary condition on the face OD right with pressure difference 0 Pa, meaning that on this face the pressure value will be the same of the ambient one
- Select the fume exits part from the dropdown menu and define a new Part Group. Then apply a Velocity Inlet with values 0 0 -6, since the velocity values are in the 3 components along X, Y and Z in this case the Surface normals don’t really matter (see the emergency room tutorial for an example of surface normal calculation). Finally define a passive scalar value of 1 for this inlet to simulate the fume dispersion
- The base cell size is 4m and the Point in mesh is -30 0 5 with a radius of 1, again the Point in mesh can be in any position as long as it is outside of the buildings geometry and inside the Outer domain. It is only used to define the area of space which we want to simulate
- The buildings contained in the PartBody will have a refinement level of 0 4 and an edge level of 4
- Select the fume exits from the drop down menu and define a new Surface mesh group. Those parts will have a refinement level of 5 7 and an edge level of 7. This was done to better capture the exit geometry as it is relatively smaller wrt the surrounding buildings
- Define a Refinement box with dimensions 20 16 10, position 0 -3 5 and Mesh level 4. This is to make sure that we properly capture the fume pattern and the way it affects the surrounding buildings.
Before running the CFD simulation it is necessary to define the output planes required and the isosurfaces necessary to visualise the portion of space where the concentration of pathogen is above certain levels.
- Define 60 planes X between -20, 20, 60 planes in Y between -15, 15 and finally 10 in Z between 0 and 10
- Click on the add isosurface icon in the Simulation editor menu
- Define 5 isosurfaces of passive scalar with values 0.001, 0.0025, 0.005, 0.01 and 0.025
Running the simulation
Run the setup phase, the mesh phase and the running phase, depending on the machine you are using the process can take 10-15 minutes.
Run the alternative geometry
Once the first option has run, it is possible to right click on the Curved exit simulation in the Simulation Manager window and select Duplicate.
in the Geometry entry select the Fumes_extraction_straight.igs file and load it in the new simulation. All the boundary conditions and mesh parameters will be automatically applied to the new simulation. Please just make sure that in the Regions tab in the Fume exits Velocity is no 0 0 6 as the exits are now pointing upwards
Just complete all the phases of this simulation as well as already done for the previous one
Load the results in the Fields viewer right clicking on the simulation and selecting Fields → Load to visualise the results of the simulation. Do the same for both the Sim_1 and the Sim_2.
Select pressure as parameter to be shown and select between -5 Pa and +5 Pa. This is showing the pressure on the surfaces of the two buildings. The portions of the buildings which are facing the flow show clearly an increase in pressure as expected. You can also appreciate the different between the two cases in terms of tubes exit geometries:
If you show the passive scalar isosurface 0.01 you can see that the straight chimney solution is more effective in displacing the fumes away from the surrounding building.
Select the passive scalar parameter with range from 0 to 0.05 and show a section normal to Y. You can then use the Pick value option to see the actual pollutant concentration in front of the rear building. As you can see the straight chimney option is showing a much cleaner flow in front of the rear building sine the whole fume pattern is displaced above the building.
Feel free to repeat the same simulations as above changing the wind incidence angle to get a sensitivity of fume extraction to wind direction. It is also possible to complete the full range of wind directions and compare them to the actual wind directions in the specific location of the study.
Download SimWorks and activate a free 14-day licence or contact us to find out more