Week 10: Project 1 - FULL HYDRO case set up (PFI)

Aim: Full Hydro Case Setup for Port Fuel Injection(PFI).

 

Objective: To find out the following with the provided engine input:

1. To calculate the compression ratio of this engine.

2. To specify the need a wall heat transfer model and To describe why can't we predict the wall temperature from the CFD simulation?

3. To calculate the combustion efficiency of this engine

4. To determine the power and torque for this engine by using the engine performance calculator.

5. To describe the significance of ca10, ca50 and ca90.

 

Introduction: 

Port Fuel injection is when fuel (either gasoline or diesel fuels) is injected before the valve and cylinder, where the combustion happens. The intake valve will have a fuel injection system that sprays fuel into the air coming into the engine. From there the spark plugs ignite the pressurized slurry of air and fuel, pushing the cylinder head down and spinning the crankshaft.

                         

Fuel injection is the introduction of fuel in an internal combustion engine, most commonly automotive engines, by the means of an injector. 

All Diesel (compression-ignition) engines use fuel injection, and many Otto (spark-ignition) engines use fuel injection of one kind or another. Mass-produced Diesel engines for passenger cars became available in the late 1930s and early 1940s, being the first fuel-injected engines for passenger car use.

In passenger car petrol engines, fuel injection was introduced in the early 1950s and gradually gained prevalence until it had largely replaced carburettors by the early 1990s. The primary difference between carburetion and fuel injection is that fuel injection atomizes the fuel through a small nozzle under high pressure, while a carburettor relies on suction created by intake air accelerated through a Venturi tube to draw the fuel into the airstream.

The term "fuel injection" is vague and comprises various distinct systems with fundamentally different functional principles. Typically, the only thing in common all fuel injection systems have is the lack of carburetion. There are two main functional principles of mixture formation systems for internal combustion engines: internal mixture formation, and external mixture formation. A fuel injection system that uses external mixture formation is called a manifold injection system; there exist two types of manifold injection systems: multi-point injection (port injection), and single-point injection (throttle-body injection). Internal mixture formation systems can be separated into direct, and indirect injection systems. There exist several different varieties of both direct and indirect injection systems, the most common internal mixture formation fuel injection system is the common-rail injection system, a direct injection system. The term electronic fuel injection refers to any fuel injection system having an engine control unit.

The gasoline port fuel injection is the most popular drive system for gasoline engines worldwide. The powertrain system convinces with low costs, reduced technology and new, innovative further developments. When using engines with specific performance of approx. 60 kW/l and downsizing concepts of up to 25%, the gasoline port fuel injection offers significant cost advantages compared with high-pressure direct injection systems. As a low-pressure system (system pressure approx. 6 bar), the gasoline port fuel injection operates with a comparatively simple operating strategy. The complex high-pressure control requirements (system pressure up to 350 bar) are omitted as are the high-pressure pump, the high-pressure sensor, the volume control valve and the high-pressure injectors for multi-point injections. The result is a less complex injection control employing variances regarding the injection time frame. The robust combustion process of the gasoline port fuel injection also tolerates fuel of lower quality.

 

Geometry:

File> Import> Import STL> Browse to the location of geometry and import the .STL file

The PFI geometry imported as a .stl file in converge studio and it has a lot of surface errors. Therefore by running a diagnosis to identify the types of errors and then fixing them.

 

Diagnosis:

By running the diagnosis to identify the different types of errors including intersections, open edges, overlapping triangles, normal orientation. The pink coloured triangles highlighted on the geometry gives the location of the surface that needs to be fixed.

 

i) Intersections:

Inlet valve is so high that it is passing through the cylinder head.

To fix this we have to push open the valve to make sure that intersections do not occur then we will push it back to the right location.  

 

ii) Nonmanifold Problems:

 

iii) Open Edges:

 

iv) Overlapping Tris: 

 

v) Normal Orientation:

Normals are facing away from the fluid domain.

 

Boundary Flagging:

As we flag the boundaries and with that multiple boundaries it will be easier to hide some parts and simultaneously to do the surface clean up.

Creating multiple Boundaries:

 

1. Piston:

`triangle` as an entity selection-By Angle `20^0`> Using cursor pick option> Selecting triangles at the bottom portion of the geometry as shown in below image> Assigning them to Piston Boundary> Apply

 

2. Cylinder Head:

By creating fence it will be easier to assign the triangles to the desired boundary.

Boundary> Fence> By selected edges> Edge as an entity-By Arc> Using cursor pick> Selecting the 5 arcs i.e 4 arcs on ports and one at the top of the cylinder> Mark Fence.

 

After creating fence-

`triangle` as an entity selection-By Boundary Fence> Using cursor pick option> Selecting triangles between the created fences on top of the cylinder as shown in below image> Assigning them to Cylinder Head Boundary> Apply

 

Cylinder Head

             

 

3. Spark Plug:

Creating a fence to assign triangles to spark plug and spark plug terminal boundary.

Boundary> Fence> By selected edges> Edge as an entity-By Arc> Using cursor pick> Selecting the 2 arcs i.e 1 for spark plug and 1 for spark plug terminal> Mark Fence.

 

After creating fence-

`triangle` as an entity selection-By Boundary Fence> Using cursor pick option> Selecting triangles on the inner side of the cylinder head except for the triangles inside that small fence as shown in below image> Assigning them to Spark Plug Boundary> Apply

 

Spark Plug

 

4. Spark Plug Terminal:

`triangle` as an entity selection-By Boundary Fence> Using cursor pick option> Selecting triangles inside that small fence as shown in below image> Assigning them to Spark Plug Terminal Boundary> Apply 

 

Spark Plug Terminal

 

5. Liner:

Boundary> Fence> By selected edges> Edge as an entity-By Arc> Using cursor pick> Selecting the 2 arcs i.e each at bottom and top of the cylinder> Mark Fence.

 

 Piston and Liner

           

 

`triangle` as an entity selection-By Boundary Fence> Using cursor pick option> Selecting triangles between the created fence as shown in below image> Assigning them to Liner Boundary> Apply

 

6. Exhaust Port:

`triangle` as an entity selection-By Angle `20^0`> Using cursor pick option> Selecting triangles (on the shorter port i.e -x direction) as shown in below image> Assigning them to Exhaust Port Boundary> Apply

 

7. Outflow:

`triangle` as an entity selection-By Angle `20^0`> Using cursor pick option> Selecting triangles on the exit face of the exhaust port as shown in below image> Assigning them to Outflow Boundary> Apply

 

Exhaust Port and Outflow

 

8. Exhaust Valve Top:

Creating a fence to divide the valve into 3 different parts and assigning them to 3 different boundaries.

Boundary> Fence> By selected edges> Edge as an entity-By Arc> Using cursor pick> Selecting the 3 arcs on each valve> Mark Fence.

 

`triangle` as an entity selection-By Boundary Fence> Using cursor pick option> Selecting triangles between the top and middle created fence as shown in below image> Assigning them to Exhaust Valve Top Boundary> Apply

 

9. Exhaust Valve Angle:

`triangle` as an entity selection-By Boundary Fence> Using cursor pick option> Selecting triangles between the middle and bottom created fence as shown in below image> Assigning them to Exhaust Valve Angle Boundary> Apply

 

10. Exhaust Valve Bottom:

`triangle` as an entity selection-By Boundary Fence> Using cursor pick option> Selecting triangles at the bottom of exhaust valve as shown in below image> Assigning them to Exhaust Valve Bottom Boundary> Apply

 

If all the above-assigned boundaries are hidden, it can be seen that still the small parts around the exhaust port are not assigned to any boundary. These parts must be assigned to exhaust port boundary.

Using Box Select> Drawing box from left to right to select these parts> All the parts get selected.

 

Assign these small parts to Exhaust Port Boundary.

 

Ring Triangles:

Ring triangles must be assigned to an exhaust port instead of exhaust valve top.

Boundary> Fence> By selected edges> Edge as an entity-By Arc> Using cursor pick> Selecting the arc exactly below the ring triangles on both the exhaust valve> Mark Fence.

 

`triangle` as an entity selection-By Boundary Fence> Using cursor pick option> Selecting the ring triangles as shown in below image> Assigning them to Exhaust Port Boundary> Apply

This is done to prevent the shape of the cylinder on top of the valve where it is connected to distort as the valve moves up and down. Flagging these ring triangles to exhaust port to it retains the shape & hence simulation correctness.

 

11. Intake Port-1:

Boundary> Fence> Reconstruct Fences From Existing Boundaries

This option will automatically create fences around the existing boundaries.  

 

`triangle` as an entity selection-By Boundary Fence> Using cursor pick option> Selecting the ring triangles as shown in below image> Assigning them to Intake Port-1 Boundary> Apply

 

12. Inflow:

`triangle` as an entity selection-By Angle `20^0`> Using cursor pick option> Selecting triangles on the exit face of the intake port-1 as shown in below image> Assigning them to Inflow Boundary> Apply

 

14. Intake Valve Angle:

Boundary> Fence> Reconstruct Fences From Existing Boundaries

 

Boundary> Fence> By selected edges> Edge as an entity-By Arc> Using cursor pick> Selecting 2 arcs to assign the intake valve angle> Mark Fence.

 

`triangle` as an entity selection-By Boundary Fence> Using cursor pick option> Selecting triangles between the created fence as shown in below image> Assigning them to Intake Valve Angle Boundary> Apply

 

15. Intake Valve Bottom:

`triangle` as an entity selection-By Boundary Fence> Using cursor pick option> Selecting triangles at the bottom of an intake valve as shown in below image> Assigning them to Intake Valve Bottom Boundary> Apply

 

13. Intake Valve Top:

Boundary> Fence> By selected edges> Edge as an entity-By Arc> Using cursor pick> Selecting 2 arcs as shown below> Mark Fence.

 The above-created fences will separate the ring triangles from valves.

 

Hide Intake Valve Bottom boundary.

`triangle` as an entity selection-By Boundary Fence> Using cursor pick option> Selecting triangles from the bottom of the intake valves after hiding the intake valve bottom boundary OR below the ring triangle fence as shown in below image> Assigning them to Intake Valve Angle Boundary> Apply

 

It is visible from the below image that the Intake valve Top boundary triangles are being selected correctly.

 

 

After hiding the Intake & Exhaust port, Liner and cylinder head there are valves inside the ports which translates into the chamber. The valve geometry is flagged in 3 categories to create events between the cylinder and ports when disconnecting triangles are created to regulate the fuel flow.

 

Intake and Exhaust Valve

By splitting the valve into valve top, valve angle, and valve bottom it is easier to provide the embedding near the valve angle alone.

So that it is going to resolve the flow perfectly. When the valve is about to open the majority pressure drop and the maximum velocity occurs at the valve opening. 

 

16. Intake Port-2: 

Boundary> Fence> By selected edges> Edge as an entity-By Arc> Using cursor pick> Selecting arcs one by one to divide the Intake Port int two parts> Mark Fence.

 

`triangle` as an entity selection-By Boundary Fence> Using cursor pick option> Selecting triangles between the created fence and Inflow boundary Fence as shown in below image> Assigning them to Intake Port-2 Boundary> Apply

 

Intake Port-1,2 and Inflow

The intake port is split into two boundaries & also into two separate regions to provide different boundary conditions. The intake port-1 is where the Fuel spray is injected.

When the intake valve is closed spray parcels are present in one half of the intake port whereas, in another half, there are no spray parcels.

To initialize some amount of fuel in the intake port that is closer to the combustion chamber we need to split the intake port into 2 boundaries.

 

Surface Preparation:

Intersections:

There are 1574 intersection errors at the inlet valve side where the valve angle protrudes out of the cylinder head wall surface. The red selection shows how the triangles are intersecting each other which causes this error.

Inlet valve is so high that it is passing through the cylinder head.

To fix this we have to push open the valve to make sure that intersections do not occur then we will push it back to the right location.

The red colour near the cylinder head and intake port-1 show intersections location.

 

To move the valve to avoid intersection errors triangles can be translated along the normal direction.

Measure> Direction-Arc normal> Vertex as an entity-Any> Using cursor pick option> Selecting 3 vertices on inlet valve top curve as shown below> Apply 

Measured arc normal will appear in the message log. Copy the arc normal values(x,y,z).

 

We can clearly see the yellow colour near the cylinder that show intersections. 

Transform> Translate-Selected Boundary> Direction Vector- Pasting the arc normal values> Translation amount-0.001m> Select Boundary-Intake Valve Top, Intake Valve Angle, Intake Valve Bottom> Apply

 

After translating the inlet valves the intersections are reduced to 3 from 1574.

 

Open Edges:

 

To fix the open edges we need to patch them.

Repair> Patch-Free edge loop(pick exactly one edge)> Check Auto-assign boundary for new triangles> Edge as an entity-Open edge> using cursor pick option select the open edge one by one> Apply

 

Repair> Patch-Free edge loop(pick exactly one edge)> Check Auto-assign boundary for new triangles> Edge as an entity-Open edge> using cursor pick option select the open edge one by one> Apply

 

Nonmanifold Problems:

The yellow coloured edge show open edge and a couple of triangles are intersecting. Need to delete intersecting triangles.

Repair> Delete-Triangle> `triangle` as an entity selection-Any> Using cursor pick option> Slect intersecting triangles> Apply

 

 

Now we can clearly see the open edges.

Repair> Stitch-Stitch vertices> vertex as an entity-Any> Using cursor pick option> Selecting two vertices to be stitched> Apply

 

Repair> Patch-Free edge loop(pick exactly one edge)> Check Auto-assign boundary for new triangles> Edge as an entity-Open edge> using cursor pick option select the open edge> Apply

 

 

Normal Orientation:

Normals are facing away from the fluid domain.

Geometry> Transform> Normal> Propagate change from single triangle> `triangle` as an entity> Any> Selecting one triangle> Apply

Overlapping tris are triangles that overlap each other, usually, they need to be fixed by deleting some overlapping triangles & patching them, however, in this case, they were present due to Normal orientation problem & fixing its normals also fixed the overlapping tris. 

 

After Surface preparation and running diagnosis it can be observed that the geometry doesn't have errors anymore. So with this clean geometry can be used for case setup.

 

No Hydro Case Setup:

1. Application Type: Crank angle-based IC engine.

 

Physical Parameters:

Bore - 0.086 m

Stroke - 0.09 m

Connecting rod length - 0.18 m

Keeping other parameters default.

 

Crank Speed - 3000 RPM

 

References - Boundary

Piston Surface Id -Piston

Liner Id - Liner 

Head Id - Cylinder Head

 

2. Materials:

Enable Parcel Simulation option and confirm the permission to load recommended defaults for solver & simulation time parameters.

 

a) Gas Simulation -

Under Gas thermodynamic data - upload [therm.dat] file. This provides thermodynamic properties to each gas species.

 

b) Parcel Simulation:

 IC8H18-Isooctane is used as a fuel in this simulation because it has physical properties that are very close to gasoline fuel. It is used in relatively large proportions to increase the knock resistance of the fuel. 

Parcel Simulation specifies the fuel being used.

Parcel Simulation> Predefined liquids> Liquid database> Select IC8H18_Isooctane.

 

After selecting IC8H18 as fuel converge include all its properties for chemical reactions and combustion simulation.

 

c) Global Transport parameters:

Keeping all the default values for global transport properties > OK

 

d) Reaction Mechanism:

Using bottom left corner option i.e Import.

Import [mech.dat] file. This takes care of gas-phase chemical reaction.

By clicking on check properties it is necessary to ensure there are no errors.

 

e) Species: We need to add the participating species parcel i.e IC8H18.

 

3. Simulation Parameters:

a) Run Parameters:

Solver - Transient

Temporal type -Crank angle-based engine simulation

Simulation mode - No hydrodynamic Solver

Gas flow solver - Compressible

 

b) Simulation Time Parameters:

Set the start time - (-480 degree)

End time - 240 degree

Initial time step - 1e-7

Minimum time step as 1e-8

Maximum time step - 0.0001 seconds.

Keep all the other CFL values default > OK.

 

c) Solver parameters:

Keeping all settings as default > OK.

 

4. Boundary:

 

1. Piston: A piston is a component of reciprocating engines, reciprocating pumps, gas compressors, hydraulic cylinders and pneumatic cylinders, among other similar mechanisms. It is the moving component that is contained by a cylinder and is made gas-tight by piston rings.

Boundary Type- WALL

Velocity Boundary Condition:

Wall motion Type - Translating

Law of wall - Piston motion

Surface Movement: Moving

Temperature Boundary Condition:

Law of wall - Temp. - 450K

Region: Cylinder Region

 

2. Cylinder Head: In an internal combustion engine, the cylinder head sits above the cylinders on top of the cylinder block. It closes in the top of the cylinder, forming the combustion chamber. This joint is sealed by a head gasket.

Boundary Type- WALL

Velocity Boundary Condition:

Wall motion Type - Stationary

Law of wall

Surface Movement: Fixed

Temperature Boundary Condition:

Law of wall - Temp. - 450K

Region: Cylinder Region

 

3. Spark Plug: A spark plug is a device for delivering electric current from an ignition system to the combustion chamber of a spark-ignition engine to ignite the compressed fuel/air mixture by an electric spark while containing combustion pressure within the engine.

Boundary Type- WALL

Velocity Boundary Condition:

Wall motion Type - Stationary

Surface Movement: Fixed

Law of wall

Temperature Boundary Condition:

Law of wall - Temp. - 550K

Region: Cylinder Region

 

4. Spark Plug Terminal: Spark plug insulated centre electrode is connected by a heavily insulated wire to an ignition coil or magneto circuit mounted external to the engine. The spark plug body forms a grounded terminal on the base of the plug on the cylinder head, with a spark gap inside the cylinder.

Boundary Type- WALL

Velocity Boundary Condition:

Wall motion Type - Stationary

Surface Movement: Fixed

Law of wall

Temperature Boundary Condition:

Law of wall - Temp. - 600K

Region: Cylinder Region

 

5. Liner: In a reciprocating engine, the cylinder is the space in which a piston travels.

Boundary Type- WALL

Velocity Boundary Condition:

Wall motion Type - Stationary

Surface Movement: Fixed

Law of wall

Temperature Boundary Condition:

Law of wall - Temp. - 450K

Region: Cylinder Region

 

6. Exhaust Port: The passage in the cylinder head which connects the exhaust valve and the exhaust manifold. The exhaust gases pass through the port to the exhaust manifold.

Boundary Type- WALL

Velocity Boundary Condition:

Wall motion Type - Stationary

Surface Movement: Fixed

Law of wall

Temperature Boundary Condition:

Law of wall - Temp. - 500K

Region: Exhaust Region

 

7. Outflow:

Boundary Type- OUTFLOW

Pressure Boundary Condition: 101325 Pa

Velocity Boundary Condition:

Specified Value - Backflow

Temperature Backflow: 

Temp. - 800K In backflow exhaust products are typically at a higher temperature.

Species Backflow:

Calculating the stoichiometric condition. combustion of isooctane for it to be stoichiometric.

Stiochiometric Claculation:

`C_8H_18 + 12.5(O_2+3.76N_2) -> 8CO_2 + 9H_2O + (3.76 times 12.5)N_2`

 https://docs.google.com/spreadsheets/d/15DXnPvXJpjX2k-xw_rKq47dqeRJBsE_gIeVYaX29mes/edit?usp=sharing

Region: Exhaust Region

 

8. Exhaust Valve Top:

Boundary Type- WALL

Velocity Boundary Condition:

Wall motion Type - Translating

Surface Movement: Moving

Law of wall - User Specified

Profile: Use file [exhaust_lift.in]

Temperature Boundary Condition:

Law of wall - Temp. - 525K

Region: Exhaust Region

 

Profile Configuration:

Two main things to be ensured are:  Type - Cyclic and Minimum lift of 2e-4m

 

9. Exhaust Valve Angle:

Boundary Type- WALL

Velocity Boundary Condition:

Wall motion Type - Translating

Surface Movement: Moving

Law of wall - User Specified

Profile: Use file [exhaust_lift.in]

Temperature Boundary Condition:

Law of wall - Temp. - 525K

Region: Exhaust Region

 

10. Exhaust Valve Bottom: 

Boundary Type- WALL

Velocity Boundary Condition:

Wall motion Type - Translating

Surface Movement: Moving

Law of wall - User Specified

Profile: Use file [exhaust_lift.in]

Temperature Boundary Condition:

Law of wall - Temp. - 525K

Region: Cylinder Region

 

11. Intake Port-1:

Boundary Type- WALL

Velocity Boundary Condition:

Wall motion Type - Stationary

Surface Movement: Fixed

Law of wall

Temperature Boundary Condition:

Law of wall - Temp. - 425K

Region: Intake Port-1

 

12. Inflow:

Boundary Type- INFLOW

Pressure Boundary Condition: 101325 Pa

Temperature Boundary Condition: 

Temp. - 363K 

Species Boundary Condition:

Species - Air

Region: Intake Port-2

 

13. Intake Valve Top:

Boundary Type- WALL

Velocity Boundary Condition:

Wall motion Type - Translating

Surface Movement: Moving

Law of wall - User Specified

Profile: Use file [intake_lift.in]

Temperature Boundary Condition:

Law of wall - Temp. - 480K

Region: Intake Port-1

 

Profile Configuration:

Two main things to be ensured are:  Type - Cyclic and Minimum lift of 2e-4m

 

14. Intake Valve Angle:

Boundary Type- WALL

Velocity Boundary Condition:

Wall motion Type - Translating

Surface Movement: Moving

Law of wall - User Specified

Profile: Use file [intake_lift.in]

Temperature Boundary Condition:

Law of wall - Temp. - 480K

Region: Intake Port-1

 

15. Intake Valve Bottom:

Boundary Type- WALL

Velocity Boundary Condition:

Wall motion Type - Translating

Surface Movement: Moving

Law of wall - User Specified

Profile: Use file [intake_lift.in]

Temperature Boundary Condition:

Law of wall - Temp. - 480K

Region: Cylinder Region

 

The Intake and exhaust valves are controlled using a file which contains the data of their motion. The motion profiles are:

 

16. Intake Port-1: Intake ports are the final part of an engine's air induction system. They connect the intake manifold with the combustion chamber.

Boundary Type- WALL

Velocity Boundary Condition:

Wall motion Type - Stationary

Surface Movement: Fixed

Law of wall

Temperature Boundary Condition:

Law of wall - Temp. - 425K

Region: Intake Port-2

 

5. Regions and Initialization:

Check Events option

i) Regions:

a) Cylinder Region:

Temperature - 300K

Pressure - 101325 Pa

Species - Pull from the Outflow boundary

 

b) Intake Port-1:

Temperature - 390K

Pressure - 101325 Pa

Species - Add

Name     Mass Fraction

IC8H18 - 0.025508

`O_2` - 0.20157

`N_2` - 0.77292

 

b) Intake Port-2:

Temperature - 370K

Pressure - 101325 Pa

Species - Air

 

d) Exhaust Region:

Temperature - 1360K

Pressure - 185731 Pa

Species - Pull from the Outflow boundary

 

Regions representation:

 

Regions Representation for Valves: 

 

 ii) Events:

Whenever we have multiple regions we have to provide events.

a) Cyclic Event:

Cyclic event is created between Cylinder region and Intake Port-1 Region and also between Cylinder Region and Exhaust Region. The event follows the valve lift profile and according to that Converge enables and disable the disconnect the triangle to regulate the fuel flow.

 

b) Permanent Event:

The intake port is split into two boundaries and two regions but there is a permanent open event between intake port-1 & Intake Port-2. 

 

6. Physical Models:

Enable Spray modelling, Combustion modelling, Turbulence Modeling and Source/sink modelling.

 

a) Spray Modeling: Converge includes models for spray processes including liquid atomization, drop breakup, collision and coalescence, turbulent dispersion and drop evaporation. The model means there is some type of mathematical approximation has been done to capture those physics.

In IC engines, the fuel is sprayed in the combustion chamber or near intake valves. This fuel spray can be completely simulated using CFD multiphase simulations, but doing so in a IC engine simulation would result in the simulation running for very long. This can be prevented if we statistically model the same effect of the spray instead of actually simulating it. This approximating process of fuel sprays is called Spray modelling. Any fuel spray undergoes a mechanism which has the following processes:

1) Primary Breakup: Splitting of a drop from the mainstream

2) Secondary Breakup: Splitting of a primary drop into multiple drops

3) Drop Drag: Drag caused by air on the moving drop.

4) Collision and coalescence: Collision of two or more drops and formation of the new drop.

5) Turbulent dispersion: Transport of mass, heat, or momentum within a system due to random and chaotic time-dependent motions

6) Evaporation: Evaporation of small liquid drops into vapour

 

The sequence of processes is easy to understand. The mainstream breaks into multiple drops by primary and secondary breakups. New drops are formed due to coalescence. The evaporation reduces the drops and dispersion spreads the drops into the region. While modelling the spray, each process is represented mathematically by using some pre-established models. These create the effect of spray without actually simulating the spray.

To calculate the spray in a simulation, CONVERGE introduces drop parcels into the domain at the injector location at a user-specified rate. Parcels represent a group of identical drops (i.e., same radius, velocity, temperature, etc.) and are used to statistically represent the entire spray field.

Evaporation: The evaporation is simulated using Frossling or Chiang model. They are responsible for flagging a parcel drop as evaporated or not. They consider the size of the drop and its evaporation properties to make decisions for drops.

Penetration: The fuel spray penetration is also recorded in the software. It calculates this based on how long did the fuel travel as a liquid. The cell up to which the 0.95*(mass of liquid fuel sprayed) is seen is called the liquid penetration length.

Collision: The software contains two models: O'Rourke model and NTC model. These models simulate the collision using a collision grid. Using a collision grid creates accurate particle movement data.

Drop Drag: This is simulated using Spherical drop drag model or Dynamic drop drag model. The Spherical model calculates the drag coefficient based on assuming the shape of drop as the sphere, while the dynamic model accounts for variations in drop shape. It uses TAB model to determine the drop distortion.

Drop wall interaction: When a drop parcel would collide with the wall, it could rebound back, escape or remain on the wall, creating a film. These effects are modelled using: O'Rourke model or Kuhnke model.

CONVERGE offers two categories of liquid injection mechanisms: injectors and nozzles. An injector is a group of nozzles that have some of the same characteristics. Each injector can have any number of nozzles, each with its own hole size, cone angle, position, and orientation.

Injector models: The models used are 'Kelvin-Helmholtz model' and 'Rayleigh-Taylor model'. These models look after the primary and secondary breakup of parcel drops. The calculations are based on 'Kelvin-Helmholtz instability theory' and 'Rayleigh-Taylor instability theory'. These theories are used for surface tension instabilities of the drop, which lead to a fluid breakup.

 

i) General: For solid cone sprays, converge assumes the injection is conical.

• Parcel distribution: Distribute parcels evenly throughout cone.

                 

• Turbulent Dispersion: O'Rourke model

 

• Drop evaporation: Enable Use evaporation model

                    General: Frossling Model

                   Evaporation source: Source all base parcel species

Enable Temperature discretization: 

•  Radius above which 1D heat diffusion will be solved: 1000m

Specifying the maximum radius of ODE droplet heating will control if the drop temperature is uniform or radially varying.

1. If the drop radius exceeds the maximum value, Converge will assume a radially varying temperature distribution.
2. If the drop radius does not exceed the maximum value, Converge will assume a uniform temperature distribution.

 

• Penetration: Converge writes the liquid and vapor penetration lengths at each output interval, it calculates vapor penetration length for each nozzle.

        Liquid fuel mass fraction for calculating spray penetration: 0.95 

          Liquid penetration length is the distance that encompasses the calculated penetration spray mass. Converge calculates the penetrated spray mass by multiplying the mass fraction by total liquid mass in the domain.

Liquid penetration length is not calculated along the spray axis of the nozzle but it is calculated along the injector axis. 

       

Bin size for calculating vapor penetration: 0.001 m

Providing bin size for calculating the vapor penetration, cell size is at least 2 times smaller than bin size, especially in the location of spray.

Fuel vapor mass fraction for calculating vapor penetration: 0.001     

Cell, where the vapor is present, have some minimum amount of vapour and that is characterized by "fuel vapour mass fraction for calculating vapour penetration". Its value 0.001 means that particular cell content 1e-3 vapour in terms of mass fraction coma anything less than that can be considered as a cell that not containing vapour.

Converge calculate the vapour penetration length (VPL) for each nozzle:
1. Converge calculates the fuel vapour mass fraction in each cell inside the spray cone.
2. For each cell that meets a and b, converge calculates the distance from the centre of the nozzle to the centre of the cell.
       a) The fuel vapour mass fraction exceeds the user-specified Fuel Vapour Mass Fraction.
       b) the cell size does not exceed the user-specified Bin size.

 

 ii) Collision/Breakup/Drag:

Collision model: NTC collision

Collision outcomes: Post-collision outcomes

Enable collision mesh

• Collision calculation based upon if the one parcel is going to hit the other parcel or not.
• Parcels are Lagrangian parcels have their own space and gas-phase have their own space.
• To perform collision calculation we need another mesh which is different from the original mesh provided. This is called the collision mesh

Collision calculations can be highly grid-sensitive when an underresolved the fluid-phase mesh is used. To help alleviate this issue, the collision mesh option has been implemented in CONVERGE, based on the concept of a collision mesh proposed by Hou. In a simulation without collision mesh, parcels collide only with parcels in the same grid cell. This can lead to artefacts in the spray since parcels do not collide across cell walls. This can also slow down computational time because there can be many parcels in larger cells. Using a collision mesh can eliminate both these problems. Simulations with collision mesh can much more accurately represent the spray dispersion by eliminating grid effects.

Using a collision mesh can eliminate both these problems. Simulations with collision mesh can much more accurately represent the spray dispersion by eliminating grid effects.

An alternative to the O’Rourke numerical collision scheme is the No Time Counter (NTC) method of Schmidt and Rutland. The NTC method is based on techniques used in gas dynamics for Direct Simulation Monte Carlo (DSMC) calculations. This model is faster and more accurate than O’Rourke’s model under certain conditions.
The NTC method involves stochastic (randomly determined) sub-sampling of the parcels within each cell. This potentially results in much faster collision calculations. Unlike O'Rourke's method, which incurs an additional computational cost that increases with the square of the number of parcels, the NTC method has a linear cost. O'Rourke's method assumes that multiple collisions can occur between parcels and that this process is governed by a Poisson distribution. However, the Poisson distribution is not correct unless collision has no consequences for the parcels. Since collisions change parcels’ velocities, size, and number, the method of repeated sampling used by the NTC method generates more accurate answers (Schmidt and Rutland, 2000). The NTC method is derived, without assumptions, from the basic probability model for the stochastic collision. The basic probability model requires that the cell size is sufficiently small such that spatial variations in spray quantities can be neglected. These assumptions are a subset of those required for deriving the O’Rourke collision mode.

 

Drop Drag:

When parcels entering through the gas phase it encounters air resistance.

Drop drag model: Dynamic drop drag

The drag coefficient calculation accounts for variation in drop shape. This model invokes the TAB model to determine the drop distortion.

 

iii) Wall Interaction:

Spray-wall interaction model: Wall film (Drop actions are calculated with a hybrid approach based on particle-based quantities.)

Film splash model: O'Rourke 

Splash criteria based on the Weber number, film thickness, and viscosity or simply based on Weber number.

 

Each of the models described above are standard models. The values of the variable used for simulation are directly taken depending on what the software recommends. So many values or expressions stated in this report might not have a logical reason mentioned along.

 

iv) Injectors:

One injector can have multiple nozzles and for this project, there are 4 nozzles in one injector.

Add Injector and then edit to add species and rate-shape.

 

a) Injected Species/Rate-shape: 

Injected Species: Add parcel species IC8H18 with mass fraction 1.

Injection rate-shape: Select profile 

 

• Profile configuration:

Add profile as shown below providing file name with an extension .in and click on accept.

 

• Rate-shape:

Profile injt_rate_shape.in where its rate vs crank is determined is is shown below.

 

b)  Models: 

Enable the Kelvin-Helmholtz model(KH) and Rayleigh-Taylor model(RT) with the default values. Both the models are used for solid cone sprays, irrespective of fuel diesel or gasoline.

Discharge coefficient model is enabled.

Discharge coefficient value: 0.8.

Set recommendations for - Gasoline PFI

 

c) Time/Temp/Tke/Eps/Mass/Size: 

Fuel Mass Calculation Link

RPM - 3000

RPS - `("RPM")/60 = 3000/60` = 50

DPS - `RPS times 360 = 50 times 360 = 18000`

Time Per Degree - `1/"DPS" = 1/18000 = 0.000055555 = 5.55e-5`

Time Per 720 degree - `"Time per degree" times 720 = 5.55e-5 times 720 = 0.04`

Total Flow Rate - `7.5e-04 (kg)/s`

Fuel Mass Per Cycle - `" Total Flow Rate" times "Time Per 720 degree" = 7.5e-04 times 0.04 = 3e-05`

Injection temporal type - Cyclic

Cycle period - 720 degree

Start of injection - (-480) degree

Injection duration – 191.2 degree

Total inject mass – 3e-05 kg [Calculated Value]

Total no of injected parcels – 500000

Injected liquid temp – 330K

 

d) Nozzles:

• Nozzle location and orientation: Cartesian
• Injection spray type: Solid cone type

 Select Nozzle_0@injector_0 and click to edit.

 

[Nozzle_0@injector_0] Configuration:

• General 

Nozzle diameter - `250 mum`

Circular injection radius(Equal to nozzle radius) - `125mum`

Spray cone angle - 10 degree

 

• Location and orientation:

[Nozzle_0@injector_0] orientation:

 

Adding Nozzles: 

Using the +Add nozzle added 3 more nozzles.

The nozzle configuration under general edit option will remain the same for all the 4 nozzles as mentioned for [Nozzle_0@injector_0] configuration.

 

• Location and orientation:

 

[Nozzle_1@injector_0] orientation:

 

• Location and orientation:

[Nozzle_2@injector_0] orientation:

 

• Location and orientation:

[Nozzle_3@injector_0] orientation:

 

Nozzle Representation:

 

• Spray Rate Preview:

•  Spray Rate Calculator

 

• Spray rate graph

Using the calculate rate option spray rate graph will open.

 

• Injector Pressure(bar)

 

The associated values can be observed in the log in the spray rate calculator tab.

 

• Validate nozzle locations

All nozzles must be inside the computational domain.

 

b) Combustion modelling: Combustion Facilitates the energy transfer in an engine. 

The combustion is modelled by using its reaction mechanism. There are multiple species and intermediate reactions which govern the combustion process. The reaction mechanism of real-life combustion is very large and simulating it directly would take a long time. So, the combustion is solved only for those reactions and species whose presence affects the combustion results. This is called a reduced mechanism file. These all processes of reducing mechanism and solving them is done by various solvers present in the software: SAGE, CTC/ Shell, G-Equation, CEQ, FGM, etc. In this report, SAGE solver is used, so details of SAGE are only given.

SAGE: It's a detailed chemistry solver which uses local conditions to calculate the reaction rates based on principles of Chemical kinetics. It calculates the heat release, which is used as a source term in fluid flow energy equations. The species are modelled using chemical kinetics ODEs and the values are used in species transport equations. The Solver used to solve the ODEs is CVODES.

Acceleration technique: The SAGE solver is a detailed chemistry solver, meaning that it would calculate values based on full mechanism instead of reducing it. This takes a lot of time if the calculations are done for every cell in the mesh. So, to increase the speed of solving, the solver is run using a multizone model. All the cells where combustion is going to be solved for, are grouped into bins. The bins are created based on the temperature and equivalence ratio of fuel and air. All the cells having the same temperature and equivalence ratio will have the same combustion results. So, the SAGE solver is solved once for each bin and accordingly the flow and species data is remapped to the cells. This increases the speed tremendously. The bins can also be created based on multiple variables like pressure, reaction ratio, etc.

 

i) General:

 Fuel species name: IC8H18

• Timing/Activation:

Temporal type: Cyclic

Cyclic period: 720 degree

Start time: (-170) degree

End time: 130 degree

Combustion temperature cutoff: 600 K

Minimum HC species mole fraction: 1e-08

 

 

ii) Models:

• SAGE detailed chemistry solver: 

                The most predictive and accurate way to model combustion.

               Accurately model ignition and laminar flame propagation.

SAGE detailed chemistry solver uses local conditions to calculate reaction rates based on the principles of chemical kinetics. This solver is fully coupled to the flow solver, but the chemistry and flow solvers parallelize independently of one another, which speeds up the simulation. With the appropriate mechanism, the SAGE solver can predict a wide range of cases (e.g., a variety of fuels [premixed, non-premixed, partially premixed, multiple fuels], emissions modelling, and unique phenomena such as end-gas auto-ignition). With its accuracy and robustness, CONVERGE can perform predictive modelling instead of merely confirming experimental results.

 

• Adaptive zoning:

CONVERGE incorporates numerous acceleration strategies such as adaptive zoning, dynamic mechanism reduction, and stiffness-based load balancing. These techniques, coupled with strategies to speed up species transport, allow using more detailed reaction mechanisms to accurately simulate kinetically limited phenomena and emissions.

 

c) Turbulence Modeling:

Keep the Turbulence model as RNG k-epsilon

Keep all the settings default > OK

 

d) Source/sink modelling:

Introducing two energy sources that are like a spark plug. This energy going to be sourced through energy equation and that is going to increase the temperature of species.

In the species transport equation, this temperature is going to be introduced and in the species transport equation, there is a source term which is responsible for combustion to occur that is going to see this temperature change and that affect the chemical kinetics. This will cause new products and subsequently heat release which will come back to species equation to produce more species release more heat and increases the temperature again.

• Source 1:

General:

 

Shape:

Source 1:

 

• Source 1:

General:

 

Shape:

Same as that of Source 1.

 

Source 2:

 

Energy Release:

On X-axis - Time/Crank Angle.

On Y-axis - Total energy input in spark.

The spark can be broken into 3 phases breakdown, arc and glow. During the breakdown phase, we put in more energy to conduct through the spark gap. Once the breakdown phase is achieved, just need a little more energy to keep the conduction going on.

During the breakdown phase providing 40 mJ of energy that lasts for 0.5 degree and then providing 20 mJ which lasts for 10 degree.

For 0.5 degree both the sources are in the same location giving 40mJ.

Adding this much amount of energy we need to make sure that there is a less numerical diffusion in those areas. So that if we put the energy in and the energy stays there long enough so that it can combust the reactance and for this need to add refinement to that area.

 

7. Grid Control:

Enable Adaptive Mesh Refinement and Fixed embedding.

 

i) Base grid:

Base grid size - 4mm

 

ii) Fixed Embedding:

Depending on the flow taking place, we may require that the flow at some region is more accurate and at some region is more approximate. This can be done by varying the mesh element sizes in the region. The embedding option in Converge CFD does this work of creating finer mesh at the mentioned location. The refinement is based on the scale and number of embed layers. If the base mesh created has cubic elements of size 'E' mm then the scale of 'n' means the elements in the refinement region will be of size `E/2^n` mm. This means that if the base mesh has elements of size 4 mm then elements of scale 1, 2, 3, 4, 5 will have elements of size 2, 1, 0.5, 0.25, 0.125 mm respectively. With each element scale, there is 8 times increase in total cell count. This happens because the elements are divided in size by 2 in all directions (X, Y, Z).

Fixed embedding is provided near valve angles as the space between valve angle and valve seat is very small and base grid with 0.004 m grid size will give inaccurate results.

Fixed embedding is provided to refine the specific areas and capture the combustion details and calculate them properly.

Cylindrical shape type embedding is provided on the cylinder to make them finer as compared to the base grid. 

a) Intake Valve Angle and Exhaust Valve Angle:

 

b) Big Cylinder:

 

c) Small Cylinder:

 

 

 

d) Small Sphere:

 

 

e) Large Sphere:

 

 

iii) Adaptive Mesh Refinement:

The fixed embedding setting is preferred when the refinement is needed in the complete region or complete boundary area. When the refinement is to be done based on the solution of flow equations, the refinement technique is called AMR. The AMR monitors the solution and based on the curvature (second degree of rate of change) of a variable, the mesh is refined. There are two methods to use AMR: Sub-grid scale method and Value-based method. In the value-based method, the value of a solution is specified. If the value is more/less than specified, the mesh is refined. The Sub-grid method works in the following way:

For a scalar, the sub-grid field is defined as the difference between the actual field and the resolved field or

`phi' = phi - bar phi`

This sub-grid can also be represented as an infinite series, but since it's not possible to evaluate the entire series, only the first term in the series is used to approximate the scale of the subgrid.

`phi' = -alpha_([k])(del^2 barphi)/(delx_(k)delx_(k))+1/(2!)alpha_([k])alpha _([l]) (del^4phi)/(delx_(k)delx_(k)delx_(l)delx_(l))-1/(3!)alpha_([k])alpha _([l])alpha _([m]) (del^6 barphi)/(delx_(k)delx_(k)delx_(l)delx_(l)delx_(m)delx_(m)) + ...`

`phi' = -alpha_([k])(del^2 barphi)/(delx_(k)delx_(k))`

A cell is embedded if the absolute value of the sub-grid field is above a user-specified value. Conversely, a cell is released (i.e., the embedding is removed) if the absolute value of the subgrid is below 1/5th of the user-specified value. That means if the user specifies a value of 2.5, the mesh program would calculate sub-grid of the cell, based on the term shown above and if it is larger than 2.5, the cell will be refined.

The velocity Sgs is permanent whereas Temperature is cyclic with the time period of the combustion period from the spark ignition to exhaust valve opening period. Controlling the AMR is also very important because restricting it will reduce simulation time & capture only relevant parts & regions of combustion. Otherwise, it will unnecessarily extend the simulation time a lot. 

The Base grid size is 0.004 m

Velocity & Temperature sgs refinement - `0.004 / 2^3 = 5e-4m`

 

Injector Embedding:

 

8. Output/Post-Processing

Output Files:

 

9. Export all the input files

Export all the input files into a separate folder

Files>Export>Export Input Files>setting up the desired location>OK

 

10. Copy and paste the mpiexec.exe file to the input files folder 

 

Run Simulation

Cygwin - Cygwin is a collection of GNU and open-source tools that provide functionality similar to Linux distribution on windows.

To run the simulation, open Cygwin and navigate to the folder in which the input files are exported.

 

To run the simulation command with executable to be entered

$ mpiexec.exe -n 4 converge-intelmpi.exe restricted </dev/null> logfile.txt &

 

Results:

Meshing:

 

Animation:

 

Injector Refinement Mesh:

 

Source Refinement:

Animation:

 

Timing Map:

The map shows the time and sequence of various embedding and valve motions. The exhaust lift looks like it went out of simulation but since the simulation is cyclic (720 Deg period), anything that goes beyond the end time is treated as placed at starting of simulation with a period as 720 Deg.

 

In-Cylinder Pressure:

The cylinder pressure contains different values at different strokes of the cylinder, the highest of which is achieved during the end of the compression stroke and it decreases as the
combustion and expansion take place. At the end of the compression stroke, the spark plug ignites the air-fuel mixture, creating very high cylinder pressure which rises very quickly. In expansion stroke engine generates power, as it forces the piston down. As the piston goes down, cylinder volume increases which reduce the cylinder pressure right after it. The peak pressure obtained in this cylinder is 3.85MPa.

In the above plot sudden change in slope indicates that the combustion process has started and pressure reaches the peak and then expansion stroke starts. We need to make sure that this plot provides us with the targeted power. The maximum and minimum pressure from the above diagram is used to derive the power output and efficiency of the engine.

 

In-Cylinder Volume:

The volume vs crank angle graph plotted in the cylinder region of the engine. It appears close to sine but its not purely a sine wave. It gives the distance of volume depending on the crank angle. 

The volume curve shows when exactly does each stroke begins. The volume is less when the piston is at TDC and it is more when the piston is at BDC.

The Compression ratio of an engine is the ratio of Total volume of a cylinder to clearance volume of a cylinder. The maximum volume is 0.00057422 `m^3` and minimum volume is 5.7029e-05 `m^3`. 

Compression ratio = `("Maximum Volume") / ("Minimum Volume")` = `0.00057422/(5.7029times10^-5) = 10.0688`

This gives us the compression ratio of 10.0688.

 

Pressure vs Volume Plot:

 

The above PV plot represents the Otto Cycle, and hence it shows that the gasoline engine works based on this cycle. There are discontinuities at the beginning and the end, it is because
of the absence of exchange of working fluid and the system remains at the original position. The area under the PV diagram gives the work done by the engine. From the obtained value, power can be calculated by multiplying work done (J) and the speed of the engine in rps (revolutions per second) and it gives the power in terms of J/s = Watt.

The Pv diagrams were invented to improve the efficiency of engines originally. They're utilized to calculate the work done as well which is usually given by 

`W = intP*dV` for a complete cycle. `

 

Pressure Animation:

 

Heat Release Rate & Integrated Heat Release Rate:

Heat release & Integrated heat release is plotted against crank angle. It gives the Amount of heat i.e the total amount of energy released from the combustion process.  

The highest heat release takes place at around 20 degrees where the combustion takes place and the highest amount of fuel is burnt at that point.

Mean Temperature:

As the pressure varies inside the combustion chamber, the temperature also varies since they both are directly proportional. Due to combustion, the temperature increases. From the above
plot, it can be seen that the engine remains at a minimum temperature of 500 K till the start of combustion in the cylinder region. Once the power stroke occurs, the temperature increases
because of the reaction of a fuel, air which is being ignited. Mean temperature inside the cylinder region reached is 2483.5 K. This data can be used to check the highest cylinder temperature to utilize in liner, engine design parameters & thermal analysis.

The mean temperature is maximum at the point when the integrated heat release is close to its max value, i.e. the entire heat energy is released. It is also the point where there is maximum pressure in the cylinder.

Temperature Animatron:

The spark occurring and temperature shooting up as the combustion begins is captured using a cut plane. 

 

Temperature distribution & combustion. The left side shows the spray discrete parcels with their temperature & right side shows the cut plane view. The spray parcels force their way into the valve opening it in a turbulent way & inside the combustion chamber they vaporize & hence can be seen disappearing. Combustion can be observed along with valve movements, spark ignition zone.

 

Mass:

Density:

When we study IC engines we always assume density, specific heat is constant, usually, it is not. They change as a function of crank angle because they all depend on pressure and temperature.

 

 

Spray Parcels:

Liquid spray drop plot gives the number of lagrangian parcels active in the domain. There is a significantly large number of parcels that were injected almost double the size that reached maximum inside the cylinder region. Sometimes fuel vapourization occurs and some fuel gets trapped. 

Spray Parcels Injector Region:

This plot tells us the number of fuel drops that are created during the spray of fuel into the combustion chamber. The drops are formed because of the vaporization (Lagrangian parcels are active in the domain). After the combustion takes place, towards the end the graph shows that amount of drops which are leftover i.e, the unburnt hydrocarbons. From this data, we can know the amount of fuel involved in combustion.

Isooctane(IC8H18) Cylinder Region:

The plot of isooctane gives the amount of fuel sprayed for the number of parcels injected.

 The parcel counts are extremely important because this is the fuel basically that's injected and to properly atomize it, combust it & overall simulation is highly dependent on it. 

This plot shows the amount of fuel injected into the combustion chamber. The intake port region near the combustion chamber has some species mass which is trapped. Designers often
focus on this trapped mass not taking place in combustion. This is because of wall collisions and scattering of liquid vapor particles while they are injected. It is quite negligible but care should be taken for it so that it is always kept minimum.

Animation:

 

 

Spray Parcels Cylinder Region:

In the above plot, the peak value shows around 44000 parcels and further parcels actually start to drop this is because of vaporization and combustion takes place. Towards the end, we can see zero parcels that means there is not much fuel left which indicates there won't be a lot of unburnt HC.

 

Spray Injection Plots:

The parcels increased as injection started. The parcels started collecting in films on the cylinder wall when the intake valves were open. This is because when the intake valves were fully open, the fuel spray was directly hitting the cylinder wall.

 

Mass Injected:

The total mass injected was 3e-5 kg. It was as specified in the spray modelling conditions. The mass flow rate can also be seen as varying due to the changing injection velocities.

 

Emissions:

Undesirable emissions in Internal Combustion engines are of major concern because of their negative impact on air quality, human health, and global warming. Undesirable emissions include unburned hydrocarbons (HC), carbon monoxide (CO), nitrogen oxides (NOx), and particulate matter (PM). 

Hiroy Soot:

Soot is a mass of impure carbon particles resulting from the incomplete combustion of hydrocarbons. It is more properly restricted to the product of the gas-phase combustion process but is commonly extended to include the residual pyrolysed fuel particles such as coal, cenospheres, charred wood, and petroleum coke that may become airborne during pyrolysis and that are more properly identified as cokes or char.

Soot causes various types of cancer and lung disease.

Soot is a black substance which is the by-product of combustion. It comes out with exhaust gas but sometimes gets trapped inside the port, walls of the cylinder, head and piston. Its accumulation will affect the engine’s performance. The above plot is a result of one cycle only and it is insufficient to study about the soot. Normally the engine should be run for many cycles to get the valid data of Hiroy – soot.

 

NOx:

NOx – Nitrogen Monoxide, is a harmful gas. They are generated because of the high-temperature processes taking place inside the combustion chamber and the reactions occurring at
that time. From the above plot, the max Nox emission is about `1.37 times 10^-6`kg (for one cycle). NOx should be kept as low as possible.

 

HC:

CO:

CO2:

CO – Carbon Monoxide, is a poisonous gas which is resulted due to incomplete combustion of the fuel. Normally CO2 is released after combustion. If there is insufficient oxygen to burn the
fuel i.e, there is no enough oxygen to complete the oxidation, CO is released. High levels of CO indicated the mixture has rich fuel content than air. From the above plot, we can see that the CO level is completely below the CO2 level. So the mixture has enough oxygen to burn the fuel yet it slightly leaves some amount of CO due to incomplete combustion (for one cycle).

 

Animation:

 

 

Comparison of Emissions:

In a rich fuel mixture, there is not enough oxygen to react with all the carbon and resulting in high levels of HC & CO in emissions exhaust products. This is particularly true at the start when the air-fuel mixture is purposely made very rich. If the air-fuel mixture is too lean poorer combustion again leads to HC emissions. Similar reasons lead to the formation of CO & NOx. NOx is created mostly from nitrogen in the air. NOx leads to photochemical smogs and there are stringent norms to reduce it.

It can be observed from graphs that all the emissions are highest at the combustion stroke and slightly dips down the curve once the peak is reached. The simulation was run for only 1 cycle so the data is not perfectly acceptable, it needs to be run for more cycles. This data is extremely important as it can be utilized to make necessary design changes & improve emissions. 

 

Cell Count:

Total Cells:

 

1. What is the compression ratio of this engine?

The ratio of the maximum to minimum volume in the cylinder of an internal combustion engine is known as Compression Ratio.

Volume vs Crank Angle Plot:

The above plot shows us how the piston creates the volume inside the cylinder. The crests and troughs describe the four strokes of the PFI engine.

The formula to find out the compression ratio of the engine is 

The volume curve shows when exactly does each stroke begins. The volume is less when the piston is at TDC and it is more when the piston is at BDC.

The Compression ratio of an engine is the ratio of Total volume of a cylinder to clearance volume of a cylinder. The maximum volume is 0.00057422 `m^3` and minimum volume is 5.7029e-05 `m^3`. 

compression ratio (CR)  is calculated by the formula

`CR = ("Total Volume")/("Clearence Volume")`

`CR = (V_d + V_c)/V_c`

Where:

`V_d` = displacement volume. This is the volume inside the cylinder displaced by the piston from the beginning of the compression stroke to the end of the stroke.

`V_c` = clearance volume. This is the volume of the space in the cylinder left at the end of the compression stroke.

`V_d` can be estimated by the cylinder volume formula

  `V_d = pi/4b^2s`

Where:

`b` = cylinder bore (diameter)

`s` = piston stroke length

Because of the complex shape of `V_c` it is usually measured directly. This is often done by filling the cylinder with liquid and then measuring the volume of the used liquid.

Compression ratio = `("Maximum Volume") / ("Minimum Volume")` = `0.00057422/(5.7029times10^-5) = 10.0688`

`therefore` compression ratio = 10.0688

 

2. Why do we need a wall heat transfer model? Why can't we predict the wall temperature from the CFD simulation?

• Why do we need a wall heat transfer model?

Internal combustion engines are now extremely optimized, in such ways improving their performance is a costly task. Traditional engine improvement by experimental means is aided by engine thermodynamic models, reducing experimental and total project costs. For those models, accuracy is mandatory to offer a good prediction of engine performance. Modelling of the heat transfer and wall temperature is an important task concerning the accuracy and the predictions of any engine thermodynamic model, although it is many times an overcome task.

To perform good prediction of engine heat transfer and wall temperature, models are required for accomplishing heat transfer from hot gases to engine parts, heat transfer inside each engine part, and also heat transfer to coolant and lubricating oil. This paper presents an overview of engine heat transfer and wall temperature modelling, with the main purpose to aid engine thermodynamic modelling and offer more accurate predictions of engine performance, consumption and emission parameters. The most important are three engine heat transfer approaches: gas to the wall, wall to wall and wall to liquid heat transfer models. To obtain a good prediction of wall temperature, those three approaches must be coupled, which may imply convection-conduction-convection problems, although, for some applications in diesel engines, radiation problems must be considered.

 In real life, some part of the heat due to combustion is released from the cylinder walls. This heat transfer takes place due to all modes of heat transfer. When more than one heat transfer modes are considered in the simulation with solid bodies, the simulation is called a conjugate heat transfer simulation. Simulating the IC engine flow along with CHT simulation would increase computation time. So, instead of simulating the heat transfer through walls, it is modelled (approximated) using different models like O'Rourke model. In this simulation, the O'Rourke model is used as the wall heat transfer model. We can't predict wall temperature from CFD simulation without using these models, because the wall heat transfer is only captured by a model or CHT simulation and not CFD simulation.

• Why can't we predict the wall temperature from the CFD simulation?

Generally, the operation of an IC engine is based on chemical reactions taking place during the combustion. During the power stroke, the fuel-air mixture gets ignited (in case of spark ignition engine) by the spark plug and chemical reactions take place inside the combustion chamber. These reactions raise the temperature inside the chamber and force the piston to expand. During this process, there will be an energy interaction between the fluid and the walls i.e, surfaces of the IC engine in the form of heat. The heat transfer between the fluid and solid surface takes place generally in two modes – convection and radiation. In general case CFD simulation, the Navier – Stokes equation is solved to get the results of the fluid flow. To get accurate results, mesh size should be less and it increases computational time.

For this PFI engine simulation, it takes a lot of time to compute the case as it involves a complex geometry and processes. If we want to capture the heat transfer – especially convection of heat from the fluid to the solid surface, energy equations should also be solved. This increases the time of the simulation. For radiation of heat from the solid surface to atmosphere, an external mesh is to be made to depict the external atmosphere and to solve the energy equation which increases the cell count. It makes the simulation to run forever. Hence, we use conjugate heat transfer model where the solid part is solved in a steady-state using super-cycling option and the fluid part is solved in transient case.

For simulating complex geometries like IC engines, it takes a lot of time for computing the fluid part itself in a transient case along with the combustion and reaction processes. So it becomes difficult to predict the wall temperature from the CFD simulation as solving of heat transfer along with the Navier – Stokes equation consumes a lot of computational power and time. Wall heat transfer models are used to approximate this case. Basically, all the physical models used in a CFD simulation uses some approximation to minimize computational time. Wall heat transfer models are used if we are focused only on heat transfer giving less importance to fluid motions and reactions. For efficient operation of the engine, the walls should be maintained at a certain temperature. This is achieved by pumping coolant to take away the excess heat from the cylinder wall.

 

3. Calculate the combustion efficiency of this engine

In real engine applications, the combustion process is incomplete. This means that not all the energy content of the fuel supplied to the engine is released through the combustion process. There are several factors which can influence the combustion process, the most important being the fuel-air intake and fuel atomization (size of droplets).

The fuel inside the cylinder needs air (oxygen) to burn. If there is not enough oxygen available, not all the fuel is burnt, therefore only partial energy is released from combustion.

If we analyze the exhaust gas of an internal combustion engine, we can see that it contains both incomplete combustion products (carbon monoxide CO, nitrogen oxides NO_x, unburnt hydrocarbons HC, soot PM) and complete combustion products (carbon dioxide CO₂ and water H₂O).

 

Combustion Efficiency(`eta_c`): 

The combustion efficiency `eta_c` is defined as the ratio between the energy released by the burnt fuel and the theoretical energy content of the fuel mass during one complete engine cycle.

`eta_c = ("Total Heat Released")/("Total Energy Content")`

 

Heat Release and Integrated Heat Release Plots for the given engine:

The heat released by the given engine can be obtained from the below plots.

Integrated heat release plot gives us the amount of energy released due to the combustion process alone. This data is used to find the combustion efficiency of the engine by normalising
the energy content of the fuel. Difference between the energy released from the combustion process and the total energy content of the fuel tells the efficiency of the combustion.

 

Integrated Heat Release Value:

The total amount of energy from the combustion process alone is found out from the graph given below as 1241.1646 J.

 

Combustion Efficiency (`eta_c`) Calculation:

Combustion efficiency is a measure of how effectively the heat content of a fuel is transferred into usable heat.

`eta_c = ("Total Heat Released")/("Total Energy Content")`

 

Total Heat Released = 1241.1646 J

Total Energy Content = `CV times m_f`

Calorific value (CV) for gasoline = 44 MJ/kg

Fuel mass (`m_f`) per cycle = 3 * 10^(-5) kg

Total energy content of the fuel = `[44 times 10^6] times [3 times 10^-5]` = 1320 J

`eta_c = 1241.1646/1320 times 100 = 94.02%`

Combustion Efficiency of this engine = 94.02%

 

4. Using the engine performance calculator, to determine the power and torque for this engine.

Engine Performance Calculator:

The engine performance calculator is used to analyse physical data and get useful results from the data. It is a useful tool to calculate the quantities that need to define an engine.

Add Files> Add 'thermo_region0.out' file

To provide stroke and bore values - Load from engine.in> selecting 'engine.in' file> Calculate.

 

Calculated Results:

CA: Crank Angle

Duration: Total duration of combustion

Work: Work done by the engine

IMEP: Indicated Mean Effective Pressure

Duration of combustion = 240.199 degree

Work done = 468.646 N-m

Indicated Mean Effective Pressure (IMEP) = 896428 Pa

CA 10(deg) = 6.83717 degree

CA 50(deg) = 18.4623 degree

CA 90(deg) = 31.701 degree

Power is the rate of work done i.e, the amount of work done per unit time.

Power (P) = `"Work Done" / "Time"`

 

RPM - 3000

RPS - `("RPM")/60 = 3000/60` = 50`

DPS - `RPS times 360 = 50 times 360 = 18000`

Time Per Degree - `1/"DPS" = 1/18000 = 0.000055555 = 5.55e-5`

Calculated Time per Degree = 5.55e-5 s

`therefore` For one cycle of operation time taken (t) = `240.199 times 5.55e-5 = 0.013331 s`

Power (P) = `"Work Done" / "Time" = 468.646 / 0.013331= 35154.60 J/s`

Power = 35154.60 W = 35.15 kW

Since Work and Torque has the same unit (N-m) , it doesn't mean value for Torque and Work will be the same. Both are different quantities and has totally different meaning. So the value
for work got from the engine performance calculator is not the value for the torque.

Work: The energy transferred to or from an object via the application of force along a displacement.

Torque: The rotational equivalent of linear force. It is also referred to as the moment, moment of force, rotational force or turning effect, depending on the field of study

The Torque is calculated from the formula:

Power = `(2 times pi times N times T) / 60`

Torque (T) = `(P times 60) / (2 times pi times N)`

Crank speed (N) = 3000 rpm

T = `(35154.60 times 60) / (2 times pi times 3000)`

Torque = 111.9 N-m

 

5. What is the significance of ca10, ca50 and ca90?

The CA refers to Crank Angle followed by its position in a degree at 10%, 50% & 90%. These angles are captured to store the data such as heat release, combustion data. The significance of it is that CA10 is used to determine the start of ignition, CA50 determines the end of premixed combustion and CA10-90 determines combustion duration and at CA90 the burning of unburnt fuel is done by the propagating flame. If CA90 value is large, the crank angles are taken increases and the exhaust stroke tends to push the premature combustion products. This data is used to compare the simulation data from experimental results or simulation data from previous results at specified percentages. Parameters like the accuracy of pegging, encoder phasing, trapped mass estimate, Volume estimate, heat generation etc. Combustion phasing angles of heat release are determined by integrating the AHRR.