## Full Hydro Simulation SI8-PFI Engine

OBJECTIVE:

The objective of this study is to set up and run a full hydrodynamic simulation of a SI8-PFI engine model and calculate the combustion efficiency, power and torque produced by the engine based on the simluation results

The following parameters shall be considered for setting up the case

### Engine Geometric Parameters

• Bore =0.086 m
• Stroke = 0.09 m
• Connecting rod length = 0.18 m
• RPM = 3000

### Run parameters

• Simulation mode: Transient

### Simulation time parameters

• Start time : -520 deg
• end time : 120 deg

### Boundary conditions

• Piston temperature - 450K
• Liner temperature - 450K
• Spark Plug temperature - 550K
• Spark Plug electrode temperature - 600K
• Exhaust ports temperature  - 500K
• Exhaut outflow - 1 bar
• Exhaust outlflow temperature - 800k
• Exhaust species concentration - Stoichiometric Condition

Calculation for the stoichiometric condition

The general reaction Equation would be

C8H18+(O2+3.76N2)->CO2+H2O+N2

Now balancing the reacting species on both side we get-

C8H18+12.5(O2+3.76N2)->8CO2+9H20+12.5*(3.76N2)

Now, the molecular weight of CO2=44.01g/mol, H2O=18.01528, N2=28.0134

As per the equation, the mass of CO2=(molecular weight*moles) i.e.,                                  44.01*8=352.08

Similarly for H2O=162.1375 & N2=1316.63

Now, the Total mass of the products= 1830.847

Mass Fraction of CO2=352.08/1830.847=0.192304

Mass Fraction of H2O=162.1375/1830.847=0.088559

Mass Fraction of N2=1316.63/1830.847=0.719137

• Exhaust valve top temperature - 525K
• Exhaust valve angle temperature - 525K
• Exhaust valve bottom temeprature - 525K
• Intake port - 1 temperature 425K
• Intake port - 2 temperature 425K
• Inflow pressure - 1 bar total pressure
• Inflow temperature - 363K
• Inflow species - Air
• Intake valve top temperature - 480K
• Intake valve angle temperature - 480K
• Intake valve bottom temeprature - 480K

Initial conditions

• Intake port - 1 (closer to combustion chamber)
• ic8h18 - 0.025508
• o2 - 0.20157
• n2 - 0.77292
• Temperature - 390k
• pressure - 1 bar
• Intake port - 2 (away from combustion chamber)
• Air
• Temperature - 370K
• Pressure - 1 bar
• Cylinder
• Pressure - 1.85731 bar
• Temperature - 1360K
• Stoichiometric composition

### Injection Parameters

• Fuel flow rate = 3.0e-4 Kg/second
• Injection start time = -480.0
• Injection duration = 191.2
• Fuel temperature = 330K

### Nozzle positions

Nozzle diameter = 250 micro-meter

Spray cone angle = 10

• Nozzle 0
• center 0.0823357 0.00100001 0.07019
• Align Vector -0.732501 0.210489 -0.647408
• Nozzle 1
• center 0.0823357 -0.00099999 0.07019
• Align Vector -0.732501 -0.210489 -0.647408
• Nozzle 2
• center 0.0823357 -0.0004 0.07019
• Align Vector -0.5 -0.2 -0.647408
• Nozzle 3
• center 0.0823357 0.0003 0.07019
• Align Vector -0.5 0.2 -0.647408

### Spark Ignition Parameters

• Start of spark = -15 deg
• Spark duration = 10 deg
• Spark location = -0.003 0 0.0091

The simulation setup process includes three major steps:

1. Preprocessing

1.1. Geometry Import

1.2. Diagnosis

1.3. Boundary Flagging and Surface Preparation

1.4. Case Setup

2. Solving

3. Post Processing

3.1. Plots

3.2. Animation

Note: The boundary flagging and surface preparation are similar to the no hydro setup, the link to which is given below

https://projects.skill-lync.com/projects/Surface-Preparation-Boundary-Flagging-SI8-PFI-Engine-with-No-Hydro-Setup-21539

PROCEDURE:

1. Preprocessing

1.1. Geometry Import:

The SI8-PFI engine model was directly imported into converge studio for setting up the full hydro case.

Fig: SI8-PFI Engine Geometry

1.2. Diagnosis: The diagnosis tool helps in identifying the different problems in the                    geometry. For performing the diagnostics on the model goto Diagnostics Dock>Find>

The Diagnosis tool looks for the following geometric issues

To reduce the time for setting up the case, the input files generated by the No hydro case setup was loaded into this case setup for ease. Since the boundary flagging and surface preparation process were similar loading the similar input files eleminates the repetitive task

Fig: Regions Flagged

Fig: Surface with Edges

Note:

1. The boundaries shown above are coloured by region

2. The purpose of creating two inlet ports was that near to the cylinder region the temperature of the inlet port is higher due to conduction as compared to the port region which is located farther from the cylinder

1.3. Case Setup:

Since all the input files from no hydro case was imported, case settings of no hydro simulation got uploaded onto the converge studio case setup wizard for full hydro. For setting up the full hydro the various changes were made in the case setup and below are the final comprehensive setup values/options opted

Settings Values to be Entered/Selected
Application IC-Engine (Crank angle-based)
Material

Tick on Reaction Mechanism, Parcel Simuation and Species
Gas simulation>No Change
Parcel Simulation>click on predefined liquids and select IC8H18
Global Transport Paramters>No  Change
Reaction Mechanism>Import the Mech.dat file provided
Species>
Gas>Add CO2, H2O, IC8H18 and CO
Passive>Add Intake, Cylinder, Exhaust, HIROY_SOOT, NOX

Simulation Parameters

Run Paramters>Simulation Mode>Select Full Hydrodynamic
Simulation Time Parameter>
Start Time: -520deg.
End time: 120 deg.
Initial time step:1e-07 s
Minimum time step:1e-08 s
Maximum time step: 0.0001 s
Solver Parameters> No Change

Boundary Conditions

Piston:
Boundary Type>Wall
Velocity Boundary Conditions: Wall Motion Type>Translating, Surface Movement>moving, select 'Law of Wall' from the list and tick on piston motion button
Temperature Boundary Conditions: select 'Law of Wall' from the list, Temperature value>450k

Inflow:
Boundary Type:Inflow
Pressure Bounary Condition>Specified Value>tick on Total Pressure> Enter a value of 101325.0 Pa
Temperature Boundary Conditions>Specified Value>363 k
Species Boundary Conditions>Add ic8h18:0.025508, o2 - 0.20157, n2 - 0.77292

Outflow:
Boundary Type: Outflow
Pressure Boundary Condition>Specified Value>Enter 101325.0 Pa
Backflow>Specified Value
Temperature Backflow: 800k
Species Backflow: CO2:H2O:N2::0.192304:0.088559:0.719137

Liner:
Boundary Wall>Wall
Wall Motion Type>Stationary, select 'law of wall' from the list
Temperature Boundary Condition> Law of Wall, temp value>450k

Boundary Type>Wall, Wall motion>stationary, select 'Law of Wall' in both velocity and temperature boundary condition, temp value>450k

Exhaust Port:
Boundary Type>Wall

Velocity Boundary Conditions>Wall Motion type>stationary. select 'Law of Wall' in both velocity and temperature boundary condition, temp value>800k

Exhaust Valve Top:
Boundary Type>Wall
Velocity Boundary Conditions
Wall Motion type>Translating, Surface Movement>Moving. select 'Law of Wall' and check on the user profile button
Profile:tick on user profile and click on profile configuration
In the Profile Config Window>Type>Cyclic, Period>720, Tick on Valve Paramters, select direction from the option.
Direction(X,Y, Z): Enter the valve normal values, Minimum Lift: 2.0e-04
Import the exhaust_lift.in file and click on accept

Temperature Boundary Conditions:
select 'Law of Wall', enter a value of 525k

Do the same for  Exhaust Valve Angle & Exhaust Valve Bottom boundaries as well

Inlet Port:
Boundary Type>Wall, Wall Motion type>stationary. select 'Law of Wall' in both velocity and temperature boundary condition, temp value>425k

Inlet Port 2:
Boundary Type>Wall, Wall Motion type>stationary. select 'Law of Wall' in both velocity and temperature boundary condition, temp value>425k

Inlet Valve Top:
Boundary type: Wall
Velocity Boundary Conditions:
Wall Motion type>Translating, Surface Movement>Moving. select 'Law of Wall' and check on the user profile button
Profile:tick on user profile and click on profile configuration
In the Profile Config Window>Type>Cyclic, Period>720, Tick on Valve Paramters, select direction from the option.
Direction(X,Y, Z): Enter the valve normal values, Minimum Lift: 2.0e-04
Import the intake_lift.in file and click on accept
Temperature Boundary Conditions:
select 'Law of Wall', enter a value of 480k

Follow the same process for Inlet Valve Angle & Inlet Valve Bottom boundaries as well

Note:

1. The direction values entered for the intake and exhaust valve boundaries (top, angle and bottom) can be obtained from the geometry. For this goto measure>direction>arc normal>select three points on the value shaft top's cross sectional area and click on apply. A message will be displayed on the message log window with the normal values, copy this  value and paste it to the valve normal. The valve normal for inlet and outlet valves shall be different as both the set of valves will be moving along different axes

2. Disconnect Triangles: these traingles are created to control the fluid flwo different two different region. The region around the inlet/exhaust valve angle and the cylinder in one such are where these triangles are created, as the flow between these two regions is established during the intake and exhaust cycle only, for the other cycles: compression and power stroke cycle, there is no flow between these region. So the minimum lift be set in such as way that the following conditions are fulfilled

a. It should not be too big so that very large size disconnect traingles are formed

b. While opening the valves should not collide with the cylinder head/piston

Spark Plug:
Boundary Type>Wall, Wall Motion type>stationary. select 'Law of Wall' in both velocity and temperature boundary condition, temp value>550k

Spark Plug Terminal:
Boundary Type>Wall, Wall Motion type>stationary. select 'Law of Wall' in both velocity and temperature boundary condition, temp value>600k

Assign the regions to the boundaries as per the following:

 Boundary Region Piston Cylinder Liner Cylinder CylinderHead Cylinder Exhaust_Valve_Bottom Cylinder Inlet_Valve_Bottom Cylinder Spark_Plug Cylinder Spark_Plug_Terminal Cylinder Inlet_Port Inlet_Port1 Inlet_Valve_Top Inlet_Port1 Inlet_Valve_Angle Inlet_Port1 Inflow Inlet_Port2 Inlet_Port2 Inlet_Port2 Outflow Exhaust_Port1 Exhaust_Port Exhaust_Port1 Exhaust_Valve_Top Exhaust_Port1 Exhaust_Valve_Angle Exhaust_Port1

Initial Conditions & Events

Regions and Initialization
Add region>Cylinder, Inlet_Port1, Inlet_Port2 and Exhaust_Port1

Cylinder:
Stream ID: 0
Temperature: 1360k
Enter Pressure value:185731.0 Pa
Species: Add CO2, H2O and N2 put the mole fractions as 0.192304, 0.088559, 0.719137 respectively

Passive: Add HIROY_SOOT ant NOX, assign 1 to the value of both

Inlet_Port1:
Stream ID: 0
Temperature: 390 k
Enter Pressure value:101325.0 Pa
Species: Add O2, N2 and IC8H18 put the mole fractions as 0.20157, 0.77292, 0.025508 respectively

Passive: Add Intake and put the value 1

Inlet_Port2:
Stream ID: 0
Temperature: 372 k
Enter Pressure value:101325.0 Pa

Exhaust_Port1:
Stream ID: 0
Temperature: 1360k
Enter Pressure value:185731.0 Pa
Species: Add CO2, H2O and N2 put the mole fractions as 0.192304, 0.088559, 0.719137 respectively

Passive: Add Exhaust, HIROY_SOOT, NOX and assign value of 1 to individual ones

Events
Tick on Cyclic & Permanent
Cyclic:
Event1- Region A: Cylinder, Region B: Inlet_Port1, Event: Valve, Profile: intake_lift.in
Event2- Region A: Cylinder, Region B: Exhaust_Port1, Event: Valve, Profile: exhasut_lift.in
Permanent:
Event1- Region A: Inlet_Port1, Region B: Inlet_Port2, Event:Open

Physical Models

Activate Spray Modelling, Combustion Modelling & Source/Sink Modelling from the Menu

Turbulence Modeling-RNG-K Eplison is selected

Spray  Modelling:

Under the general Tab the following settings were opted

Collision/Breakup/Drag tab the following settings were opted

Wall Interation Tab Settings

Injectors Tab Settings

Select Injector 0 and click on edit for further configuration. Below is the image for the same

Click on plot to check the injection rate graph and it should look as given below

Close the above window and goto Model tab for the below given settings

Goto Time/Temp/Mass/Size and provide the setting given below

Goto Nozzle and use the following configurations

Select Nozzle 0 and click on edit to enter the nozzle configuration

Similarly for the other 3 nozzles enter the values given below

Nozzle diameter = 250 micro-meter

Circular injection radius = 125 micro-meter

Spray cone angle = 10

• Nozzle 1
• center 0.0823357 -0.00099999 0.07019
• Align Vector -0.732501 -0.210489 -0.647408
• Nozzle 2
• center 0.0823357 -0.0004 0.07019
• Align Vector -0.5 -0.2 -0.647408
• Nozzle 3
• center 0.0823357 0.0003 0.07019
• Align Vector -0.5 0.2 -0.647408

Combustion Modelling

Goto combustion modelling and provide the following settings

Goto Emissions and provide the following settings

Goto General tab and provide the following settings

Source/Sink Modelling

The source/sink model is used to provide the spark parameters. Here we need to add 2 sources as a real spark takes place in 3 stages: Breakdown, arc and blow. At around 0.5 crank degrees the spark initiation takes place which emits around 40 mJ of heat post which arc formation takes place followed by blow. After the initiation phase less energy is required so in the arc and blow phase around 20 mJ of heat is emitted for spark continuation in these 2 phases

Source 2 Motion- same as source 1

Grid Controls

Base Grid:
Enter the grid values for (dx, dy, dz) as per
dx = 0.004 m; dy = 0.004 m; dz =0.004 m

Add AMR Group1, select inlet_port1, inlet_port2 and cylinder to active regions and goto the temperature tab

Enter the following values

In the velocity tab enter the following values

Note: Adaptive mesh refinement is added to capture the physics at these regions with greater accuracy

Fixed Embedding-
Add embedding Intake_Valve_Angle, Exhaust_Valve_Angle, BigCylinderEmbed, Small CylinderEmbed, Large Sphere, injector embedding

Intake_Valve_Angle:
Entity Type: Boundary
BoundaryID: Inlet_Valve_Angle
Mode: Permanent
Scale: 3
Embed Layer: 1

Exhaust_Valve_Angle:
Entity Type: Boundary
BoundaryID: Exhaust_Valve_Angle
Mode: Permanent
Scale: 3
Embed Layer: 1

BigCylinderEmbed

Entity Type: Cylinder
Mode: Permanent
Scale: 1

In the Center of Cylinders add the following:

Center 1 & 2- (0.0,0.0,0.08): (0.0,0.0,-0.15)

SmallCylinderEmbed

Entity Type: Cylinder
Mode: Permanent
Scale: 2

In the Center of Cylinders add the following:

Center 1 & 2= (0.0,0.0,0.018): (0.0,0.0,-0.15)

Spherical:
Entity Type: Sphere
Mode: Cyclic

Period: 720 degree
Scale: 4

Start Time:-16 degree

End Time: 7 degree

Center of Sphere (-0.003, 0.0, 0.0091)

Large Sphere:
Entity Type: Sphere
Mode: Cyclic

Period: 720 degree
Scale: 3

Start Time:-16 degree

End Time: 7 degree

Center of Sphere (-0.003, 0.0, 0.0091)

Note: 2 AMRs are added at the spark location for better capture of the physics during the spark duration

Injector Embedding:
Entity Type: Injector

Mode: Cyclic

Period: 720 degree
Scale: 4

Start Time:-482 degree

End Time: -288 degree

InjectorID: Inector 0

Length=0.02

Output/Post Processing

Post Variable Selection>

Typical Parameters/Geometry>No Change

Species/Passives: Species>Add Mass Fraction for N2, CO, CO2, NO, NO2, H2O, IC8H18

Passives>NOX, HIROY_SOOT

Soot>Parcel: tick on mass fraction

Output Files

Time Interval for writing 3D output data files: 2 deg
Time Interval for writing text output: 0.1 deg
Time Interval for restarting output: 10.0 s

Fig: Geometry with Embedded and Nozzles

Fig: Timing Map

The timing map highlights all of the events of mesh refinement and fixed embedding timing for the 720 degree cycle

After this all the input files was imported to a seperate folder. Converge creates .txt  files which contains all the values entered while setting up the case for respective settings done above. These input files will be processed by converge using Message Passing Interface (MPI) standard

2. Solving:

For running the simulation, Cygwin tool was used instead of converge studio interface. Cygwin is a POSIX-compatible API which is based on command prompt is used to run the simulation

Steps:

a. Navigated to the folder location containing the input files

b. Entered the command> mpiexec.exe -n 2 converge.exe logfile & : This allows converge to run two processors (selection on number of processor cores present as per the system configuration, can use multiple cores if available) for the parallel processing and load balancing

c. Entered the command> taif -f logfile

d. After the simulation is over. Went back to converge studio>Post-Processing 3D

e. Enter Case Name>"Test", Change the File Type to Paraview VTK in-line binary format

d. Enter the address for the output files>Select all files>Select all Cell Variables>click on Convert

e. After the conversion of the post files to the binary output, open the Test.vtm (group file) file in Paraview

3. POST-PROCESSING:

Plots

Fig: Volume (M^3) vs Crank Angle (Degree)

Fig: Cell Count Vs Crank Degree

Fig: Emission Species- Soot, NOx, CO, CO2, HC(Kg) vs Crank Angle (Degree)

Fig: Integrated Heat Rate (Joule) vs Crank Angle (Degree)

Fig: Maximum Pressure (MPa) Vs Crank Angle (Degree)

Fig: Mean Temperature (K) vs Crank Angle (Degree)

ANIMATION:

No Hydro Simulation: SI8-PFI Engine Isometric View

No Hydro Simulation: SI8-PFI Engine Cutplane View

Full Hydro Animations:

Exhaust: SI8-PFI Engine

Temperature Contour Animation: SI8-PFI Engine

Velocity & Flame Front Temperature Distribution Contour Animation: SI8-PFI Engine

yC8H18 & Pressure Contour Animation: SI8-PFI Engine

KEY CONCLUSIONS:

1. Compression Ratio: It is the ratio of total swept volume of the cylinder covered by the piston travelling fromTDC to BDC to the clearance volume or the total volume compressed with piston at the TDC

Compression Ratio: Maximum Volume/Minimum Volume= 5.74x10^4/5.701x10^5 (Both the values are acquired from the volume vs crank angle graph)=10.07:1

2. Combustion Efficiency: It is defined as the ratio of energy released by the burning the fuel to the theoritical energy content of the fuel mass during one complete cycle

Combustion Efficiency= Heat Released/Heat Content of the Fuel

Heat content= Fuel Mass inducted*CV of fuel=(3.0x10^-5 )x(44x10^6)=1320 J

Heat Released=1241 J (from the Integrated HR graph)

Combustion Efficiency=(1241/1320)x100= 94.015%

Significance of Wall Heat Transfer Model: Wall heat transfer model is used to the

3. Power and Torque:

In converge a engine performance calculator tool was used for this

Work=468.646 Nm

Total Degree=120.11- (-120.09)=240.2 Degree

Engine speed = 3000 RPM or 50 RPS

For 1 rotation (360 degree), time= 1/50= 0.02 sec

For 240.2 degree, time = 240.2x0.02/360=0.013344 sec

Power =Work/Time=468.464/0.013344= 35,106 W or 35.1 KW

Power Output=2piNT/60 or T= Px60/(2piN)=35106x60/(2x3.14x3000)=111.8 Nm

Theory:

Significance of Wall Heat Transfer Model: In any CFD simulation, the Navier stokes equation is solved for getting the results. The complexity of the equation increases significantly as the simulation case gets more complex and therefore more time is required to solve the equations. To reduce the complexity of the equation various models are used which simplifies the equation thereby reducing the time required for the same, without compromising the result effectiveness or rather capture near to experimental results. Wall heat transfer model is one such model which is used to capture the physics near the wall boundaries. In case this wall heat transfer model is not used the solver will simulatenous solve the heat transfer equation as well as the NV equation which can consume significant amount of time. Apart from this the selection of these models also depend on the type of simulation which is being run, in cases where conjugate heat transfer is a mandatory consideration, the concept of supercycling can be used alongside wall heat transfer model, else only the wall heat transfer model can do the predict the desired accuracy in the results. As in the SI8-PFI engine case, the focus or the domain is limited to within the cylinder and the ports, here heat transfer through the cylinder chest (conduction heat transfer) is not of prominent concern so wall heat transfer model is used to capture the heat transfer physics within this domain. If the cylinder/engine chest cooling has to be considered and were of the key interest then the supercycling concept could have been used alongwith the wall transfer model

Significance of CA10, CA50 and CA90:

CA10, CA50, CA90 are combustion phases which refers to the corresponding crank angle traversed for 10%, 50% and 90% of the total heat released during the combustion respectively. The pressure, temperature, premix ratio and other parameters are collected for these angles and compared with the experimental results, which can be further used to predict the combustion lag  for engine output optimization.

For the  current setup the following are the values

CA10: 6.8371 Degrees

CA50:18.4623 Degrees

CA90: 31.701 Degrees

### Data Analysis Gaurav Samanta · 2020-01-08 12:32:09

Objective: The objective of this project is to write a code for data analysis from an input file and perform the following operations 1. Compatibility Check: The program will ask for the file name with valid extension which if provided incorrect will terminate the prog Read more

### Constraint Minimization Gaurav Samanta · 2020-01-08 11:52:01

Objective: The objective of this project is to minimize a simple non-linear funtion using Lagrange Multiplier The target equation is: f(x,y)=5-(x-2)^2-2(y-1)^2 & the constrain equation: x+4y=3 Theory: In real engineering applications there is a Read more

### Curve Fitting Gaurav Samanta · 2019-12-27 19:42:51

Objective: The objective of this project is to perform a curve fitting between the temperature and Cp values given the data file   Theory:  Curve Fitting: it is a process of constructing a curve that best fits the provided data series. Curve fitting in gene Read more

### Ice Breaking Challenge Gaurav Samanta · 2019-12-27 19:01:57

Objective:  The objective of this project is to determine the minimum pressure required to break a given thickness of ice using an air cushion vehicle through Newton Raphson Method Equation: `p^3(1-beta^2)+(0.4hbeta^2-(sigmah^2)/r^2)p^2+((sigma^2h^4)/(3r^4))p-((s Read more

### 3D CAD Modelling in Star CCM+ Gaurav Samanta · 2019-12-17 17:47:36

Objective: The objective of this report is to understand the CAD modeller features in Star CCM+ and use it to generate a 3D model of an Ahmed Body and a Convergent Divergent Nozzle in the same as per the drawing given below   Procedure & Results: Conv Read more

### Air Standard Cycle Gaurav Samanta · 2019-12-10 14:51:18

Objective: The objective of this report is to create a python based Otto Cycle simulator which can create the  PV diagram and give the thermal efficiency of the engine as output  Theory: Otto cycle is the set of processes used by the spark ignition Read more

### 2R Robotic Arm Gaurav Samanta · 2019-12-10 14:33:33

Objective: The objective of this report is to simulate the foward kinematics of a 2R robotic arm using python programming   Theory: Robotic arm manipulators are used in various industry verticals such as automotive, electronics, warehouses and logistic Read more

### Solving 2nd order ODE Gaurav Samanta · 2019-12-10 08:14:29

Objective: The objective of this report is the simulate the transient behaviour of a simple pendulum and the create the animation of its motion for a given time interval Theory: The following equation (Ordinary Differential Equation) for the position of the bob w. Read more

### Flow over Bicycle Gaurav Samanta · 2019-11-22 18:54:05

Objective:   The objective of this  study to understand the change in drag force with respect to velocity different cycling positions and drag coefficeint for constant frontal area and constant velocity.   Theory: Cyclists tend to experien Read more

### Steps involved in any CFD Simulations & Industrial Applications of CFD Gaurav Samanta · 2019-11-09 05:13:29

Objective: The objective of this report is to understand the different steps involved in any CFD simulation and the applications of CFD in Medical, Oil & Gas and Construction Industry 1. Steps involved in a CFD Simulation  Step 1. CAD Modelling/Geometry Impor Read more