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

1. AIM:

• Simulate Port Fuel injection for a Four Valve 4 Stroke engine as per specifications below. To understand the atomisation and mixing characteristics of the gasoline fuel.
• Simulate Combustion event and flame front propagation through the cylinder during the power stroke.
• Explain about the spray and combustion modelling.
• Characterize the emissions from the engine.

 

 

 

2. GEOMETRY, BOUNDARY CONDITIONS AND INITIALIZATION:

• Geometry is an actual representation of 'wetted region' of an IC Engine with a PortFuel Injected Engine. Basically, the cylinder-piston-intakeport-exhaust port regions and intake-exhaust valves form an enclosed volume.

 Engine Geometric Parameters

1. Bore =0.086 m
2. Stroke = 0.09 m
3. Connecting rod length = 0.18 m
4. RPM = 3000

 

Run parameters

1. Simulation mode: Full hydro solver with chemistry solver, AMR and energy equation
2. Simulation time parameters
3. Start time : -520 deg
4. end time : 120 deg

Turbulence model

1. RANS based RNG K-Epsilon model was used to keep computation costs in check and take into account the highly rotational swirling and tumbling flow in the cylinder.

Boundary conditions

1. Piston - 450K, Law of wall : Translating boundary - Piston, Turbulent Kinetic Energy: Neumann / Turbulent Dissipation: Wall Model. Heat model: O'Rourke and Amsden
2. Liner - 450K, Law of wall : Fixed boundary, Turbulent Kinetic Energy: Neumann / Turbulent Dissipation: Wall Model. Heat model: O'Rourke and Amsden
3. Head - 450K, Law of wall : Fixed boundary, Turbulent Kinetic Energy: Neumann / Turbulent Dissipation: Wall Model. Heat model: O'Rourke and Amsden
4. Spark Plug - 550K, Law of wall : Fixed boundary, Turbulent Kinetic Energy: Neumann / Turbulent Dissipation: Wall Model. Heat model: O'Rourke and Amsden
5. Spark Plug electrode - 600K, Law of wall : Fixed boundary, Turbulent Kinetic Energy: Neumann / Turbulent Dissipation: Wall Model. Heat model: O'Rourke and Amsden
6. Exhaust ports - 500K, Law of wall : Fixed boundary, Turbulent Kinetic Energy: Neumann / Turbulent Dissipation: Wall Model. Heat model: O'Rourke and Amsden
7. Exhaut outflow - 101325 Pa with 800K temp with Velocity Neumann boundary. Species backflow of N2:CO2:H2O - in ratio 0.71913:0.19235:0.088525 
8. Exhaust valve top - 525K, Law of wall : Moving Boundary, Turbulent Kinetic Energy: Neumann / Turbulent Dissipation: Wall Model. Heat model: O'Rourke and Amsden
9. Exhaust valve angle - 525K, Law of wall : Moving Boundary, Turbulent Kinetic Energy: Neumann / Turbulent Dissipation: Wall Model. Heat model: O'Rourke and Amsden
10. Exhaust valve bottom - 525K, Law of wall : Moving Boundary, Turbulent Kinetic Energy: Neumann / Turbulent Dissipation: Wall Model. Heat model: O'Rourke and Amsden
11. Intake port - 1 temperature 425K, Law of wall : Fixed Boundary Turbulent Kinetic Energy: Neumann / Turbulent Dissipation: Wall Model. Heat model: O'Rourke and Amsden
12. Intake port - 2 temperature 425K, Law of wall : Fixed Boundary Turbulent Kinetic Energy: Neumann / Turbulent Dissipation: Wall Model. Heat model: O'Rourke and Amsden
13. Inflow pressure - 101325 Pa with 363K temp with Velocity Neumann boundary. Species inflow of N2:O2 - in ratio 0.77:0.23
14. Intake valve top - 480K, Law of wall : Moving Boundary, Turbulent Kinetic Energy: Neumann / Turbulent Dissipation: Wall Model. Heat model: O'Rourke and Amsden
15. Intake valve angle - 480K, Law of wall : Moving Boundary, Turbulent Kinetic Energy: Neumann / Turbulent Dissipation: Wall Model. Heat model: O'Rourke and Amsden
16. Intake valve bottom - 480K, Law of wall : Moving Boundary, Turbulent Kinetic Energy: Neumann / Turbulent Dissipation: Wall Model. Heat model: O'Rourke and Amsden

The species at the outflow are assigned by considering a stoichometric combustion of iso-octane with normal air.

Detailed Intake (Left) and Exhaust (Right) valve profiles are shown below:

 

 

Events:

Events are provided exactly as per the IC engine timing. Converge uses the events to controls the flow between two regions. Events are mostly provided to simulate the valve movement and disconnection. This is done by means of disconnect triangles in converge. Note: Regions Intake port 1@ and 2@ are both permanantly connected.

The disconnect triangles are temporarily created to stop the flow or disconnect the regions. These triangles are activated and deactivated using events as shown above. The events here will be goverened by valve profiles as shown further in the report.

 

Initialization:

Here the regions are initializaed with following values. Value in intake port 1 is initialized with air, value in intake port 2 near the intake valve is intialzied with a bit of iC8H18 which is a realistic case as some fuel is formed as a film in previous cycle which evaporates. The in cylinder region is considered as a complete combustion case as we discussed before above from the equation of stoichiometric combustion and finally the exhaust with the same species fractions.

 

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

Here the O'rourke model is one of the 4 heat transfer model available. In simplest words, a heat transfer model is a "wall function" for temperature gradient near the walls against an appropriate Y+. 

Before reading further: checkout my conjugate heat transfer simulation for explaination of Y+ and Momentum wall functions : HERE

A QUICK REFRESHER

Law of the wall boundary conditions for velocity means for the simulations with a k-ε turbulence model CONVERGE uses the Launder and Spalding [Launder and Spalding, 1974] wall model for computing (read:modelling) velocity at the wall. This is given by following equation:

For same law-of-the-wall boundary for temperature, O'Rourke & Amsden wall treatments for heat transfer were selected. This is modelled as:

As per the question, we CAN predict the wall temperature from CFD simulation - in most cases very accurately but the penalty to computing such a simulation is too prohibitive for most computers on the planet. The computational costs comes with a very fine grid resolution near the walls (Y+ < 5 atleast) and running the simulation for large number of cycles so that the walls can reach 'an almost' steady state - since the gas and flame temperature are fluctuating during the entire cycle. Not to mention you will have to model the walls as well with a suitable material and mass - as in a real engine geometry; not just some boundaries. The main difficult then comes down to the difference in heat transfer time scales between fluids (convecting & conducting) and the solids (conducting), there is a huge amount of thermal capacitance as well which leads to solids heating up and cooling down very slowly compared to the fluids that it is in contact with. This is exactly why a simulation has to be run for longer period of cycles to equalize the temperature in the solids enough to a steady state.

Interesting side note: With a suitable computational power and time availibility we can actually simulate a pretty close estimation of walls using converge's supercycling feature. One such simulation has already run by converge below. More on Supercycling in one of my previous simulations : HERE

BUT as we saw this poses great computational burden, to mitigate this we use some smart wall approximation was used in this simulation. Maybe someday we will be able to simulate this in household PC.

 

INITIALIZATION:

Intake port - 1 (closer to combustion chamber)

1. ic8h18 - 0.025508
2. o2 - 0.20157
3. n2 - 0.77292
4. Temperature - 390k
5. pressure - 1 bar

Intake port - 2 (away from combustion chamber)

1. Air
2. Temperature - 370K
3. Pressure - 1 bar

Cylinder

1. Pressure - 1.85731 bar
2. Temperature - 1360K
3. Stoichiometric composition

Injection Parameters

1. Fuel flow rate = 7.5e-4 Kg/second
2. Injection start time = -480.0
3. Injection duration = 191.2
4. Fuel temperature = 330K

 

 

Nozzle positions

1. Nozzle diameter = 250 micro-meter
2. Circular injection radius = Nozzle radius
3. 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
• Spark radius = 0.0005m

 

 What is the significance of the simulation here? 

Considering that now almost everyone knows about the four stroke cycles in the engine. This simulation deals with the spray and parcel simulation first and foremost. This is a realistic case study of port fuel injection, where fuel at room temperature is sprayed in the port directly at the back of the valve. Since the spray is highly atomized and contacts the hot intake valves, it evaporates instantly (atleast most of it), when the valve opens it undergoes complex turbulent and discrete phase interaction due to swirl and tumble as well as temperature gradients which causes fuel to further atomize. As not all the fuel atomizes, there is significant amount of wall wetting that occurs which has to be taken care of during engine calibration to make sure that the engine responds well (X-tau tuning). 

After the fuel is vapourised and mixed into the cylinder it is all down to combustion modelling and flame front propagation. The flame is modelled as a parcel of energy given at the spark plug location and then propagating outwards in a self accelerating exothermic reaction. 

THe third and final important result out of this is amount of expected emissions formed during the combustions. This also accounts for volumetric efficiency and expected power out of the engine.

 

 

 

3. UNDERSTANDING THE FUEL INJECTION MODELLING:

Before running the simulation there was considerable amount of time spent on boundary flagging, surface cleanup which HAS to be the first stage of the simulation.

SPRAY MODELLING:

As discussed above, the important portion of this simulation is getting the fuel injection part of it spot on to derive accurate results from the final combustion simulation. Converge fundamentally uses a lagrangian discrete phase injection in an eulerian domain framework.

Converge uses a parcel approach to model the spray. CONVERGE introduces drop parcels into the domain at the injector location. Parcels represent a group of identical drops (i.e., same radius, velocity, temperature, etc.) and are used to statistically represent the entire spray field. This reduces the computational burdeon considerably.

Each parcel has a certain distribution of diameter of drops in the parcels. Converge offers four options: Blob model (currently used), Rossin rammler (most popular), Chi-squared and Uniform. The latter three are computed on the basis of Saunter Mean Diameter.

Here we used Blob model, CONVERGE sets injected drop sizes equal to the nozzle diameter directly. This reduces computations costs and complexity of simulation but is not accurate in most cases. 

The most common model used in Rossin Rammler distribution: 

The cumulative probability distribution function for the Rosin-Rammler distribution is calculated as 

Saunter Mean Radius is specified as half of nozzle dia usually. 

 

When a fuel is sprayed in the combustion chamber or port, it undergoes complex turbulence chemistry interaction. It shows as below: there are multiple outcomes after a spray has been injected. The droplet can experience drag forces and temperature gradients which results into evaporation, breakup, collision and coalescene and dispersion along with secondary breakup if the drag is severe and meets certain criteria.

 

(i) FOR EVAPORATION OF SPRAY PARCELS:

We have 2 models available, The Frossling correlation and The Chiang correlation. CONVERGE also contains 2 different methods for computing thermal transfer and temperature distribution of a drop:Uniform Temperature Model and the Discretized Temperature Model.

Here we used Frossling's correlation which is modelled as:

Also here CONVERGE determines the temperature and its gradient in the droplet, which is used as an input for the above mentioned ODE. This is done in 2 ways, if we specify an explicit ODE solver then converge uses the Discretized Temperature Model for droplet radius value more than the specified value and uses Uniform Temperature Model below that radius. 

Here we used the 2nd way to compute temperature with Uniform Temperature Model. This assumes that the temperature is uniform in the entire droplet diameter and hence it following energy transfer ODE for the solution of temperature. 

This solution is eventually fed into the Frossling's correlation to compute radius which in next step again used in the Uniform Temperature Model to yield next temperature of droplet. This is hence a coupled system and a couple ODE solver is used by CONVERGE.

 

 

(ii) SPRAY BREAKUP & DRAG MODELLING:

The Dispersed phase momentum interaction with the Eulerian continuous phase, CONVERGE solves following equation:

so it is pretty clear that the drag has  to be modelled correctly if the disperson and momentum of the spray parcels are to be simulated accurately:

Con CONVERGE we get 3 options to model drag : No drop drag, Spherical drop drag and dynamic drop drag. Here we used dynamic drop drag since it accounts for the distortion in the droplet as it moves in the domain. This distortion is computed from TAB model.

In CONVERGE the values of the drop distortion parameter are determined from the TAB model. The Taylor Analogy Breakup (TAB) model is a very popular method for calculating drop distortion and breakup. This method is based on Taylor’s analogy between an oscillating and distorting droplet and a spring-mass system. 

 

Image above shows how the TAB model works, it computes the modes of distortion on the droplet as it deforms due to aerodynamic drag. Once it exceeds a threshold value of distortion breakup is said to occur and the momentum of the new droplets formed is computed by the law of momentum conservation.

 

Primary and secondary Droplet Breakup:

The fuel in most cases emerges as a liquid jet in a quiescent chamber from the injector. In such cases, the droplets and ligaments first form from a primary droplet breakup. There are numerous models in CONVERGE available for simulating such a flow.

 

Here we have used Kelvin-Helmholtz instability for primary breakup and Kelvin-Helmholtz+Rayleigh Taylor instability model for secondary - they are most realistic models when there is an injection of certain diameter jet in a quiescent chamber such a port. Here TAB models can also be used if there is suitable evidence from validation study that TAB is better at predicting atomization characteristics.

KH Instability:

This is developed due to velocity shear at the interface between two fluids due to large relative velocity across the interface. A common example is wind blowing across the surface or such cloud formations as shown below. Eventually this instability translates into waves and then due to turbulence and vortex formation, the breakup occurs into ligaments or droplets.

So it is clear that when a jet emerges out of the injector, instability develops and eventually this results into formation of large ligaments and droplets.

Since it is already highly technical, the discussion of modelling approach is beyond the scope of this article.

 

RT Instability:

Unlike KH instability, this occurs due to the density differences among the two fluids. It can be easily explained by two different density fluids being placed into a column with denser fluid on the top and less dense fluid on the bottom separated by planar surface. This surface is highly unstable and if subjected to perturbation, would lead heavier fluid is displaced downward with an equal volume of lighter fluid displaced upwards. This continues to form and results in extreme mixing of two fluids eventually. This can be represented with a diagram below:

 

 (iii) Turbulent Dispersion and spray penetration:

CONVERGE models the effects of the turbulent flow on spray drops by adding a fluctuating
velocity ui' to the gas velocity u. 

The RANS (Reynolds-Averaged Navier-Stokes) turbulence models in CONVERGE include
source terms to account for the depletion of turbulent kinetic energy due to work done by
turbulent eddies to disperse the liquid spray droplets. The source terms Ss include the
fluctuating component of the fluid-phase velocity ui' a

 

One more important aspect is the liquid and vapor penetration lengths (LPL and VPL). These are two of the properties that characterize a spray. CONVERGE calculates both quantities for each nozzle at each time- step

Below shows a small diagram depicting different terminologies and spray code geometry.

To measure the LPL, CONVERGE first calculates the total mass of the liquid parcels from the nozzle and then multiplies this mass by the liquid penetration fraction to yield the penetrated spray mass. Starting from the center of the nozzle hole, CONVERGE sums the mass of the liquid parcels until it reaches the penetrated spray mass. This distance is the LPL.

To measure the VPL, CONVERGE identifies cells within the spray cone where the mass fraction of fuel vapor exceeds  the vapor penetration fraction and then calculates the distance from the nozzle hole center
for each of these cells. The largest of these distances is the VPL.

 

(iv) Collision and coalescence:

As one can assume, there are number of particles in the parcel - computing collision of each and every particle will be very computationally intensive. Consider N drops, each having N-1 possible collision partners, the number of possible collision pairs is approximately (0.5)*N^2. This N^2 -dependence would render the collision calculation computationally prohibitive for the millions of drops that may exist in a simulation.

Although parcel approach can alleviate the problem a bit, further using collision models can make it computationally very economical. There are 2 collision models : NoTimeCounter model and O'Rourke model.

Here we utilized NTC method: 

The NTC method involves stochastic (randomly determined) sub-sampling of the parcels within each cell. This sampling potentially results in much faster collision calculations. The NTC method is based on techniques used in gas dynamics for direct simulation Monte Carlo calculations.

The NTC method first sorts the parcels into groups that reside in the same cell. Next, the NTC method picks a stochastic subsample from all of the possible pairs in a cell. The probabilities for the sub-sample pairs are multiplied by the reciprocal of this fraction, increasing the probability of collision. The resulting method incurs a cost that is linearly proportional to the number of parcels, as opposed to the N-squared cost of many existing methods.

After the collision is completed, it is imperative to produce the outcome of the collision. In CONVERGE, there are 2 collision outcome models. Here we used Post Collision outcome model.

 

(v) Wall film formation and wall interaction:

The wall film is formed in a PFI intake system as the injected spray deposits on the wall. It is imperative to check for mixing and emissions as well as to pass on information to the calibration team down the line.

The film momentum equation is used to model liquid film transport wherein momentum transfer from
impinging spray parcels and inter-particle momentum transfer is accounted for via a drag force term

Based on the film formation and film spray interaction, there can be following iteractions mostly:

 

 

 

4. UNDERSTANDING THE COMBUSTION:

Combustion in general is a very complex phenomena and so is the simulation of the same. There are chemical kinetics involved along with complex turbulent in the fluid varying in multiple time scales. There are varying regimes of combustion: premixed, non premixed and partially premixed. There are also regimes of turbulent combustions which are out of the scope of this article. 

Here we are simulating a PFI gasoline engine which is more of a 'pre-mixed' approach. Premixed combustion requires that the fuel and oxidizer species be completely mixed before combustion is allowed to take place. But under low-temperature conditions, combustion reactions are considered frozen. The frozen state is metastable because a sufficiently strong heat source, a spark for example, can raise the temperature above the threshold and initiate self accelerating reaction. Once the fuel and oxidizer species have been homogeneously mixed and a heat source is supplied, a flame front can propagate through the mixture. 

Typically, the gas behind the flame front rapidly approaches the burned gas state close to chemical equilibrium. The mixture in front of the flame typically remains in the unburned state.

Here we used CONVERGE's SAGE Detail chemistry solver:

SAGE uses detailed chemistry mechanism file in a CHEMKIN format (this is what mech.dat is). A chemical reaction mechanism is a set of elementary reactions that describe an overall chemical reaction. The combustion of different fuels can be modeled by changing the mechanism. In the simulation we used Primary Reference Fuel mechanism developed by Yao-Dong Liu, Ming Jia, Mao-Zhao Xie, and Bin Pang. 

SAGE calculates the reaction rates for each elementary reaction while the CFD solver solves the transport equations. The reaction rates are then integrated with a timestep to form a source term for the species equation. The reaction rates are normally Arrhenius terms. 

 

This source term gathered from the arrhenius term is added into species transport and energy equation for result into development of species, modelling of emissions and the rise in temperature which we would be able to see in the end as a flame-front iso surface.

 

 

 

5. UNDERSTANDING THE SPARK AND COMBUSTION TRIGGER:

In an actual engine, the spark plug provides the necessary energy at a point in the cylinder. This energy allows the reactants to cross the activation energy barrier, which leads to reactions proceeding forward. This releases the heat energy due to exothermic reaction which initiates the combustion in surrounding molecules and the reaction zone propagates as a flame front in the domain with complex turbulent-chemistry interaction. 

Actual spark occurs in 3 phases: 

Breakdown phase: A very high voltage is supplied to the terminals - of order of more than 20000 Volts. This exceeds the dielectric strength of the air gap and hence that ionizes air in the gap making it conduct electricity.

Arc Discharge : After the breakdown phase, the arc strikes in the air gap and the current is atleast upto 0.1A with voltage dropping to several 100s from 20000+ volts. This discharge generates lot of heat which triggers the chain reaction and develops something called as flame kernel.

Glow Discharge: This is after the arc discharge phase as the energy is used up to heat kernel as well as the electrodes during this phase. This is why most focus goes into maximizing arc discharge rather than glow discharge as flame kernel is energized most during arc discharge phase.

To simulate this, the energy is given at the exact location of the spark plug air gap in two phases. The general graph is as shown below:

Note the mesh needs to be resolved to a very fine resolution in order to capture the spark plug and complex turbulent chemistry interaction accurately. It is noted that the spark phenomena and the flame front propagation is very grid sensitive in general for most CFD codes.

NOTE: These equations are basically NS equations for Species transport and transport of energy.

 

 

 

6. MESH CONTROL AND ADAPTIVE MESH REFINMENT:

As we know the solution for CFD simulation can be highly grid dependent especially events like spark, turbulent-chemistry interaction flamefronts and discrete phase injections which are all present in this simulation. This means that the grid has to be suitably refined at appropriate places:

FIXED EMBEDDING:

This is a permanent or time based embedding added to the grid as shown below, we have made number of refinement to areas.

dx_embed = dx_base/2^embed scale.

 The mesh sizes we used is as follows:

Base grid - 4mm
Embedding	Location	Scale	Size (mm)
Cylinder	(0,0,0.08) to (0,0,-0.15) : radius 0.05mm	1	2.00
Small Cylinder	(0,0,0.016) to (0,0,-0.15) : radius 0.05mm	2	1.00
Spherical Spark	(-0.003, 0, 0.0091) - Radius 0.001	5	0.13
Spherical Spark Large	(-0.003, 0, 0.0091) - Radius 0.003	3	0.50
Exhaust Valve angle	Boundary: Intake Valve Angle	3	0.50
Intake Valve angle	Boundary: Exhaust Valve Angle	3	0.50

 

ADAPTIVE MESH REFINEMENT:

As we have already seen, Converge requires minimal input from the user's end for its own mesh generation. It automatically generates the best possible cartesian mesh for its domain. Ideally we would want as coarse mesh as possible with refinements at the places only and only where it is absolutely needed. The AMR algortihm of converge does just that, it adds embedding determined by algorithm to the portion of domain where the flow field variables are least resolved or so to speak where sub-grid field is largest. In simple words, it will check for the curvature gradients of the variable in the spatial domain and compares it to user defined tolerance. 

In converge, this subgrid field is defined as a difference of actual field and resolved field,

The sub-grid for any scalar can be expressed as an infinite series (Bedford and Yeo
(1993) and Pomraning (2000), as is given by

Since it is not possible to evaluate the entire series, only the first term (the second-order
term) in the series is used to approximate the scale of the sub-grid :

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
sub-grid is below 1/5th of the user-specified value.

Base grid - 4mm
Name	Regions	SGS Criteria	SGS Parameter	Embed level
AMR Group 1	Cylinder Intake Port 1@ Intake port 2@	1 m/s	Velocity	3
AMR Group 1	Cylinder	3 K	Temperature	2.5

 

After running the simulation the mesh was generated as shown in the video below, the mesh is refined by fixed embeddings and the adaptive mesh refinements at different time intervals as we can see.

Note: this is during the simulation run, so one can easily see the refinement due to temperature and velocity gradients which occur during the simulation near the valve heads and the cylinder walls where the flame is quenched.

 

TIMING MAP:

Before discussing the results of the simulation it is imperative to look at the timing map to get an overview on that is happening when. 

 

 

 

6. FINAL RESULTS & ANIMATIONS:

When discussing results, we would go over in an exact order of the simulation. As shown in above, the simulation starts during exhaust stroke, the first activity that is simulated is the fuel injection itself. Fuel is injected in the quiescent intake manifold and starts accumulating at the back of intake valve where it start evaporating due to heat transfer and accumulation starts reducing, then the valve opens and the vaccum of piston and overlap sucks in the new charge which results in further mixing as the charge tumbles and swirls in the relatively hot combustion chamber. Some animations showing this are as below:

And with temperature gradient we can see

A very common quantity to validate the injector CFD simulation is the injector spray penetration, below we can see the penetraton occur upto 0.2m in the domain, even after the injection is completed. The variation amongst the 4 nozzles is because they inject in different directions and the parcels face different sets of possibilities during their phase in the domain:

 

To validate our experiments we can also plot the total injection mass as a function of crank angle as shown below:

One more important quantity which we are interested in as we discussed above is the wall film formation and the amount of mass trapped in into the wall film at the end of the cycle. To see that we can plot the below line graph. As one can see the film is thickened as there is a lot of deposition during the injection phase until the intake valve opens and then the film mixes and vapourises due to interaction with heat thereby decreasing to certain value.

But there are still some film parcels left at the end of intake which are deposited on the intake manifold behind the intake valves which has to be factored in during the engine calibration and to get a better transient response from the engine.

 

Question: What is the compression ratio of this engine?

The compression ratio is also very important parameter. It is the compression of the air in the engine after the intake stroke, for a standard otto cycle, more the compression ratio more the efficiency of the engine and hence more and more manufacturers are trying to maximize the same. With engine downsizing trend, the engines are coming out with higher and higher boost levels with more and more compression and hence more and more high octane fuels are required to prevent detonation.

Here we can see from the graph that the max volume is 0.0005742 m^3 and minimum volume is 0.000057029 m^3. Computing compression ratio by below formula it gives 10.0688.

 

The second phase we consider here is the combustion phase. We have already discussed on how the energy is released and the reaction is triggered by a spark, since this is a premixed case the combustion takes place in a thin reaction zone where there is complex turbulent chemistry interaction and the flame front propagates into the chamber. 

An animation of flame front proagation approximated as an ISO surface at 1700K is shown below:

 

Question: What is the significance of ca10, ca50 and ca90?

The CA here represents the Crank Angle, although CA10-50-90 doesnt represent actual degrees on the crank. It is a notation of Crank Angle when the combustion is 10%, 50% and 90% complete. This is usually considered as respective increase in the burned mass fraction as shown below. 

This is important as usually CA10 is considered as the commencement of combustion, CA50 which is considered as the mid of the combustion and most important since it corresponds to the max heat release rate due to the combustion and lastly CA90 is the final phase of combustion which concludes the process and from CA10 to CA90, the area of graph under the HRR curve represents total heat energy input in the system.

 

A full cut section view with the injection and combustion phases from different angles is shown below:

 

We can obtain number of line plots here to characterize our combustion. As shown below first plot is the Heat Release Rate, here we can see the CA10 is about 7 degrees, CA50 about 18 degrees and CA90 is at about 32 degrees.

The max pressure graph can be used to understand when the pressure peaks. Ideally during calibration one requires it to be around 5-10 degrees ATDC, here we have max pressure of 3.88MPa at around 25 degrees which is quite conservative. Similiary we can also have plot for in cylinder mean temp.

 

Question: What is the combustion efficiency of the engine?

Combustion efficiency of the engine is defined as the ratio of total energy release by the combustion of the fuel to the energy input from the fuel in the form of calorific value.

Total energy released by the combustion: 1241.13 J

Total energy input from fuel: m X calorific value = 0.00003kg X 44000000J/kg =  1320 J

Efficiency thus comes out to be = 1241.13 / 1320 = 94.025%

 

Last but the most important is the emissions characterization in the engine. The COx, NOx and soot characteristics buildup in the engine and formation of emission in CFD simulation can be a guide to emissions after the actual engine has been developed. Infact this is one of the reasons why CFD modelling is used to design the internals of combustion chamber, fuel injection and timing of injection. CFD modelling also helps in calculation of swirl and tumble ratios which are out of the scope of this article.

 

 

Question: Calculate engine power and torque from the engine performance calculator.

Before moving forward, the engine performance calculator screen shot is here:

Work done from the performance calulator = 468.646 N-m

Combustion duration = 300.6 deg

Crank speed(N) = 3000 RPM = 50 RPS

Number of degrees per second = 18000 

Time for one degree = 5.555556e-05 seconds

Time taken for combustion = 5.555556e-05*300.6 = 0.0167 seconds

Power = work done/time = 468.646/(0.0167 x 10^3) = 28.062 KW = 37.63 bhp @ 3000RPM

Torque = Power*60/2*pi*N = [(28062W)*60]/[2*PI*(3000 RPM)]= 89.369 N-m @ 3000RPM