By Xiao Hu and Lisa Mesaros, Fluent Inc.

View the pdf of this article

As emissions regulations tighten and fuel economy requirements heighten, improving engine performance is one of the highest priorities of major automotive manufacturers. The overall vehicle performance is highly driven by the efficiency and combustion by-products of the internal combustion (IC) engine. Better control over the turbulent flow structures, air-fuel mixing rates, and ignition patterns can greatly impact the performance. However, the simulation of IC engines remains one of the most challenging applications for CFD modeling. Moving valves and pistons require a mechanism to handle a changing mesh, and this must be coupled with models of complex sprays and combustion processes, all within a highly turbulent flow environment. FLUENT’s general purpose dynamic mesh tool is capable of simulating a wide range of moving boundary applications, including IC engines. Its numerous spray and combustion models have been validated through years of rigorous testing. The compatibility of these three models – dynamic mesh, spray, and combustion – makes FLUENT uniquely qualified to simulate a variety of situations inside internal combustion engines.

For a dynamic mesh application, the domain is decomposed into different zones. This allows for different mesh motions – and the use of different re-meshing algorithms – in different regions within a single simulation. The unstructured smoothing and re-meshing approaches are popular choices for modeling the upper combustion chamber, since they greatly facilitate the process of tracking changes to the complex mesh in the vicinity of the valves. If only traditional structured approaches were available, it would be difficult to generate topologies that could accommodate the full range of valve motion in this region. Typically, such structured moving mesh approaches require special preprocessing tools and involve significant manual work. These tools and procedures are not required for the dynamic mesh model in FLUENT, where only the initial mesh and description of the boundary movement are required. FLUENT also includes tools for treating arbitrarily complicated piston shapes. Engines such as these pose tremendous challenges for structured re-meshing approaches, but are easily handled with the unstructured tools in FLUENT.

A symmetric four-valve engine; local smoothing and remeshing are used in the upper part of the combustion chamber, and dynamic layering is used in the lower part, adjacent to the piston, and in the region above the valves to allow better resolution of the valve seat gap

Grid of an engine with arbitrarily complex shape⁶

Several new models, specific to in-cylinder applications, have been implemented in the upcoming release of FLUENT 6.2. For premixed engines, two critical models have been incorporated. The first is a spark model, which is used to simulate the electric spark required to initiate the combustion process. The second is an autoignition model, which is used to predict knocking. Other new features include an ignition delay model based on the work of Hardenburg and Hase.¹ This model has been developed specifically to simulate direct injection diesel engines. There is also a new wall film model, which is necessary for capturing the fuel formation along walls in direct-injection and port-fuel-injected gasoline engines, and some small-bore or cold-start diesel engines.

Spray and wall film model applied to a port-fuel-injected engine showing the spray (top) and the wall film height (bottom)

Simulations have been ongoing at Fluent for some time to test the new IC engine capabilities. One study was carried out to validate several of the models using a single cylinder version of the Caterpillar 3400 series heavy-duty diesel engine for which experimental data has been published.² The objective of the study was to validate the newly implemented ignition model in conjunction with the dynamic mesh capability for six different load and speed conditions (modes) from a federal transient test procedure. This procedure, from the United States Environmental Protection Agency, evaluates exhaust pollution from diesel engines at different load points. A vehicle is run on a chassis dynamometer and measurements for fuel economy and emissions are made. Speed and load points are specified as a function of time and chosen to represent the typical output of the engine. Europe and Japan have their own procedures. For the CFD analysis, the diesel spray was described using the Lagrangian discrete phase model (DPM). The nozzle was treated as a solid cone atomizer, and the fuel breakup was governed by the wave breakup model.³ Ignition delay was also accounted for using the Hardenburg and Hase model. After evaporation of the spray, the eddy-dissipation model in FLUENT was used to simulate mixing controlled combustion. Results for the mass-averaged cylinder pressure as a function of time were found to be in very good agreement with the experimentally obtained data for each of the six modes. Ignition delay was well represented and the peak pressure was predicted accurately for both magnitude and phasing.

Combustion flame development after the spark ignition of the DaimlerChrysler engine
Courtesy of DaimlerChrysler

The models in FLUENT can also be applied to spark ignition (SI) engines. A study was carried out on a port-fuel-injected, SI gasoline engine from DaimlerChrysler using FLUENT’s Zimont premixed turbulence combustion model.⁴ The Zimont model solves a progress variable equation to predict the turbulent flame speed and rate of energy release on a spatially resolved basis. To use this model, the fuel and air are assumed to be perfectly premixed, an acceptable assumption for many SI engines. Although no species information is available for pollutant calculations, the model runs quickly on a per cell basis so that the flow field can be well resolved without requiring excessive computational time. In the simulation, the electric spark model was used to initiate the combustion. The mesh count varied from 280,000 elements at top dead center to 724,000 elements at bottom dead center. The results were used to illustrate the combustion flame development after ignition. Good agreement between the CFD predictions and experimentally derived values for global burned gas mass fraction as a function of crank angle were obtained. With this tool, the impact of different spark timing on the engine power output can be studied to determine conditions that improve fuel economy.

Engineers at DaimlerChrysler made further use of their CFD results for this case. Convective heat transfer coefficients from the gas side were computed in FLUENT and used as thermal boundary conditions for a steadystate stress analysis calculation in the engine block and head. A steady stress analysis requires less computational time than a transient one, yet still accounts for non-uniform thermal loading. Thus spatially-resolved but time-averaged heat transfer coefficients were exported from FLUENT for import into a structural finite element analysis (FEA) code. Since only thermal information was needed for this purpose, the relatively inexpensive Zimont combustion model, capable of predicting heat release, was sufficient. As expected, the time-averaged heat transfer coefficient on the surface of the cylinder head was found to be highly non-uniform, especially at the exhaust valve seat region where the gas speed is high. The exhaust valve seat area has a heat transfer coefficient more than a factor of ten higher than other parts of the head, which correlates with a significant increase in thermal stress in that region. The piston, on the other hand, has a relatively uniform heat transfer coefficient distribution because of the uniformity of the velocity in that region. The study showed the importance of using CFD to obtain more accurate heat transfer coefficients for thermal stress analysis. It also showed that solutions of this type can be obtained with reasonable computational expense.

Contours of heat transfer coefficient on the cylinder head (top) and piston (bottom) for the DaimlerChrysler engine; this data was imported into a steady-state stress analysis code for analysis of heat transfer in the engine block and head
Courtesy of DaimlerChrysler

Other complex cases have been studied to test other IC application areas. For example, the wall film model has been used in the simulation of a port-fuel-injected gasoline engine. For this analysis, the spray was described using the discrete phase model. The nozzle was treated as a solid cone atomizer, and the O’Rourke and Amsden⁵ model was used for the film on the intake valve. The study was done to investigate whether or not the fuel vapor is uniform when the spark goes off. In another case, the volume of fluid (VOF) model was combined with the dynamic mesh model to predict engine cooling. In this simulation, a moving piston was modeled as a conducting solid with an upper temperature of 1300 K, and an oil jet at a temperature of 400 K was injected onto the piston from below. The high speed engine had a piston speed that was greater than the speed of the jet. The jet was found to cool the piston, as evidenced by surface temperature contours as a function of time.

Mass averaged cylinder pressure for the six mode CAT engine simulation that includes internal combustion

The VOF model is used with the dynamic mesh model to simulate piston cooling; surface temperatures are shown on the piston and oil surface at two times during the simulation

Validation and testing continues on these and other models in FLUENT 6.2 that are targeted at IC engines. Other advanced combustion capabilities are also being planned for future development, including unsteady flamelet approaches and multi-component vaporization. When combined with the flexibility of the dynamic mesh model, these options will allow for the most comprehensive suite of internal combustion modeling tools available in commercial software today.

Mass fraction of burned gas vs. crank angle for the DaimlerChrysler case shows very good agreement between FLUENT predictions and measurements
Courtesy of DaimlerChrysler

References:

1. H.O. Hardenburg and F.W. Hase, An Empirical Formula for Computing the Pressure Rise Delay of a Fuel from its Cetane Number and from the Relevant Parameters of Direct-Injection Diesel Engines, SAE 790493, 1979.
2. D. Montgomery and R.D. Reitz, Six Mode Cycle Evaluation of the Effect of EGR and Multiple Injections on Particulate and NO Emission from a DI Diesel Engine, SAE 960316, 1996.
3. R.D. Reitz, Modeling Atomization Processes in High-Pressure Vaporizing Sprays, Atomization and Spray Technology 3, pp.309-337, 1987.
4. V.L. Zimont, To Computations of Turbulent Combustion of Partially Premixed Gases, Chemical Physics of Combustion and Explosion Processes; Combustion of Multi-phase and Gas Systems, Chernogolovka, OIKhF, pp.77-80 (Russian), 1977.
5. P.J. O’Rourke and A.A. Amsden, A Particle Numerical Model for Wall Film Dynamics in Portinjected Engines, SAE paper 961961, pp.143-156, 1996.
6. E.S. Suh and C.J. Rutland, Numerical Study of Fuel/Air Mixture Preparation in a GDI Engine, SAE 1999-01-3657, 1999.

FluentNEWS