LTH
Department of Energy Sciences
2017-09-7
kursen i
Advanced Methods for Numerical Fluid Dynamics and Heat Transfer (MVKN70)
Instruction for computer Exercise2
Introduction
This exercise is on performing numerical simulations for (1) premixed combustion and (2) non-premixed combustion,usingANSYS fluent.
The computational geometryisa 2D T-junction channel. There is a small bump in the horizontal channel wall. It has a left-inlet (2 mm wide) and a bottom inlet (1.5 mm wide) and a pressure-outlet, the bump shape is a half-circle with radius 0.7 mm intend for adding certain flow complexity.The length of the horizontal channel is 35 mm. All walls will be set to adiabatic.
For the premixed combustion simulations, perfectly-mixed fuel/air mixture will be fed into the left inlet, the bottom inlet is used to supply (a little) hot product to prevent the premixed flame front being blown away. Fig. 1 shows apremixed combustion example with a plotof the reaction-progress-variable field.
In ANSYS fluent, the premixed flame is modeled by solving only a single transport equation of reaction-progress-variable (c), c=0 denotes the fresh unburned mixture, c=1 is the burned state. The equation is in a general convection+diffusion+reaction (CDR) form :
Note c is Favre-averaged for handling turbulent combustion, the reaction rate is modeled in a way to supply a “correct” local flame speed to account for the self-propagation motion of the local premixed flame front. Temperature and species mass is a function of c.
Fig 1: The progress-variable field from a premixed combustion case solved using ANSYS fluent
For the non-premixed combustion case, the left-inlet is fed with pure fuel and the bottom-inlet is for air supply. In ANSYS fluent, the diffusion combustion is model a mixture-fraction (Z) equation, z=0 denotes the pure fuel, z=1 means pure oxidizer.
Note, there is no source (reaction rate) term in this equation. Temperature and species mass now are a function of Z.
Beginning of Instructions
Download from the course website the fluent-case file, unzip it and only use the “.cas” file. Open it with fluent.
General setting
In setup->General:
Make sure you select
Type = Pressure-based solver
Time = Steady
The first task we do is to simulate the premixed combustion:
Premixed flames: (Part 1)
Make sure the following list are selected:
Setup->models->Energy (off)
Setup->models->Viscous ( standard k-epsilon 2 eqn)
Setup->models->Species (Premixed Combustion)
[Adiabatic, C-equation, zimont-model, default constants … ]
Setup->Materials->Fluid->Air
Inside this item make sure to use the default “Properties””
Laminar Flame Speed =0.2 m/s
Adiabatic unburned Temperature: 300K
…..
Setup->Boundary Conditions->inlet-bottom->Momentum: Velocity Magnitude =0.01 m/s
Setup->Boundary Conditions->inlet-bottom->Species: Progress variable=1
Setup->Boundary Conditions->inlet-left->Momentum: Velocity Magnitude =10 m/s
Setup->Boundary Conditions->inlet-bottom->Species: Progress variable=0
(1) Start the firstsimulations (usingthe default solution-setting). You can view the results
Results->Graphics->Contours :
Inside it, you should view various contours:
Premixed combustion …
progress variable , static temperature , turbulent flame speed, and others ….
Velocity…
Velo magnitude , ….
Pay attention to the overall inclination of mean premixed flame front.
(2) Perform multiple simulations after each of the following sequential adjustment to the setting; compare the change in overall flame front shape
Setup->Boundary Conditions->inlet-left->Momentum: Velocity Magnitude =5 m/s
Setup->Boundary Conditions->inlet-left->Momentum: Velocity Magnitude =2 m/s
Setup->Boundary Conditions->inlet-left->Momentum: Velocity Magnitude =1 m/s
Setup->Boundary Conditions->inlet-left->Momentum: Velocity Magnitude =0.5 m/s
Setup->Boundary Conditions->inlet-left->Momentum: Velocity Magnitude =0.3 m/s
Try to explain what you observed.
(3) Change setting back to
Setup->Boundary Conditions->inlet-left->Momentum: Velocity Magnitude =10 m/s
But also set
Setup->Boundary Conditions->bottom-left->Momentum: Velocity Magnitude =0 m/s
Run the simulation and check the results,
What happen now? Why?
(4) Decrease the “bottom-inlet” velocity to 0.3 m/s and keep the “bottom-inlet” velocity at zero, and run the simulation for a bit more iteration, i.e. make sure it converge to steady state solution.
Check the results. What is the difference with previous run at m/s and =0.01 m/s? What happen?
Non-premixed diffusion flames: (Part 2)
Make sure the following list are selected:
Setup->models->Viscous ( standard k-epsilon 2 eqn)
Setup->models->Species (Non-Premixed Combustion) ;
Inside the “Chemistry” TAB:
Read the default settings, try to change the “Energy treatment” between “adiabatic” and “Non-adiabatic”, do you notice the “Models->Energy” also change to “on” or “off”? For our next simulation, we use “adiabatic”, while use other default settings.
Inside the “Boundary” TAB:
Change the 2nd column(Fuel) in the first row to 1, this means setting the fuel stream as pure methane.
The default 3rd column(Oxidizer) is kept as Air (n2:o2=0.767: 0.233).
Be aware, the default Temperature for Fuel and Oxid are all set to 300 K .
Inside the “Table” TAB:
Click to ”Calculate PDF table” , using the default PDF-Table parameters.
Setup->Materials->Mixture:
Explore the items inside, find parameters such as “thermal conductivity”, “Cp” , etc.. , can you find item such as “Laminar flame speed” as in previous case, why?
Setup->Boundary condition:
Inlet_bottom->Species-> Mean Mixture Fraction=1
Inlet_left->Species-> Mean Mixture Fraction=0
inlet-bottom->Momentum: Velocity Magnitude =1 m/s
inlet-left->Momentum: Velocity Magnitude =5 m/s
(5) Start the simulations (use default solution setting). You can view your results
Results->Graphics->Contours :
Inside it, you should view various contours of :
pdf …
Mean Mixture Fraction ….
Species…
Mas fraction of CH4 , O2, and others …
Temperature…
Static Temperature, (Various) Enthalpy and (Various) Energy …
Vecloity…
Velo magnitude , ….
Pay attention to the overall shape of the region of largest temperature.
(6) keep m/s, change 2 m/s , 1m/s , 0.3 m/s , 0.01m/s and perform various run, notice the difference.
(6) Change both and run the simulation and check the result, did it differ much with previous case of 1m/s and
(7) In setup-general->Mesh->Scale ….
Select “Specify scaling factors”, set the two scaling factors in X, Y both as 100, then click only once “Scale” button, make sure the domain extension is x_min =-970mm, Y_min is -730mm
Now run the simulation again, what have changed, why?