UFR 4-13 Best Practice Advice

From QNET
Jump to navigation Jump to search

Front Page

Description

Test Case Studies

Evaluation

Best Practice Advice

References




Compression of vortex in cavity

Underlying Flow Regime 4-13               © copyright ERCOFTAC 2004


Best Practice Advice

Best Practice Advice for the UFR

The vortical flow in a cavity results from the interaction of the jets and the valves and chamber walls. A clear large-scale vortex occupies the whole chamber volume and persists after the filling is terminated. At the end of compression, this large-scale vortex motion breaks up into smaller structures generating high turbulent fluctuations. The modelling of such a complex unsteady flow requires a time dependent simulation.

7.1. General strategy

To predict the aerodynamic behaviour of a vortex when compressed in a cavity, CFD modelling could be based on a one or several cycles. The idea of the Multiple Cycle method is to compute as many cycles as possible, so that the first initial conditions (with their errors) are almost forgotten. This is extremely difficult (even with well-known RANS models) because everything should be well computed right away, so this is almost never done. With the Single Cycle method, only part of a cycle is computed, this allows to study each phenomenon separately. The specification of the initial conditions is the main problem.

2D or 3D computation could also be chosen, but 2D computation cannot simulate accurately the compression stroke, especially the vortex breakdown. Nevertheless, this could be applied successfully on the intake stroke.

7.2. Turbulence modelling

As it could be seen through the bibliographical review, the turbulence modelling of the compression of a vortex in cavity could be achieved using several models. The choice of the turbulence model depends on the expected results. This model should be chosen in advance, because it influences the other CFD modelling specifications (meshing, boundary and initial conditions …).

For overall quantities, it is recommended to use RANS equations to access to the mean flow structure. Modelling of practical in-cylinder configurations (currently 10e5 to 10e6 elements with 2nd order spatial scheme) is able to capture about 80% of the flows kinetic energy). The RANS-equations allow the time-dependent Reynolds-averaged flow fields to be computed, with the assumption that the temporal average of the turbulent quantities is not affected by the global unsteadiness. This is physically correct if the spatial scale of the turbulent eddies is much smaller than the geometrical scale of the analyzed geometry. In the case of compression of vortices, this assumption is too simple. So k-ε models results are qualitatively similar to measurements essentially during induction, the vortex breakdown during compression is not well replicated.

There are no great differences between the k-ε models, but the Two-Scale k-ε seems to be better suited in an IC engine, and at different speeds (Mc Landress et al, 1996).

Concerning Reynolds Stress models (RSM) methods, despite the fact that they have not given satisfaction in the prediction of the compression and the break-up of confined vortices in our test case, these turbulence models (and specifically ASM) are often preferred for swirling flows to the k-ε models.

To obtain more detailed results, such as cycle-to-cycle variations, LES is better suited. It can eliminate many of the shortcomings and assumptions made in RANS and RSM simulations. They have shown high potential for accurately predicting vortical flows. But only recently they have been extended for predicting complex turbulent such as the decay of compressed vortices. Realistic applications of LES still need tuning and finalization. Moreover, obtaining an ensemble mean with LES implies great care in fixing initial conditions, and computing multiple cycles is perhaps to be considered. One must also find a suitable model for the simulated scales.

There are different Sub-Grid Scale (SGS) models available for LES: eddy viscosity (Smagorinsky) model, scale similarity model, mixed model. The Smagorinsky model is the most known and used, while the others are relatively rare. The scale similarity model doesn’t model any dissipation of energy, so it cannot be used alone, hence the mixed model (hybrid of Smagorinsky and scale similarity model). In general, it is believed that the Smagorinsky model performs better with spatial discretisation and the mixed model with finite difference or volume method.

Aside from those, one can find mention of the Dynamic model. It is rather a procedure, as it takes one of the models above as a basis. It is a mean to estimate dynamically the parameter of the LES. Dynamic models were compared to constant coefficient model in studies (specific for IC engines), and performed noticeably better.

A spectral SGS model exists, but its accuracy for the smallest resolved scales is in doubt. It seems also not much used in the IC engine domain, so it is perhaps not to be recommended.

One school note that LES calculation can be conducted without any SGS model: the ‘diffusion’ of the numerical scheme (central differencing for example) can produce the SGS effect.

7.3. Computational domain

As the intake and the exhaust pipes have a direct impact on the in-cylinder flow behaviour, the calculation domain includes:

  • Upstream volume
  • Whole port between this volume and valve
  • Valve geometry and lift
  • Combustion chamber with piston movement
  • Exhaust system
  • Moving boundaries (piston and valves)
  • Fixed boundaries

7.4. Grid and grid resolution

Use a mesh which fits closely the topography of the chamber and the inlet port, including the moving parts. The objective is indeed to analyze the impact of changes in the geometry on the engine performance.

Use a mesh in a manner to allow, to the greatest possible extent, the control local resolution, and so to optimize the number of nodes. To have the maximum accuracy only where it is mostly needed use a high concentration of points in some regions of high gradients i.e. boundary layers and embedded shear layers and a coarse mesh elsewhere.

  • Assure that each grid point is being connected to the same number of neighbouring points. It is recommended to not use tetrahedral elements in boundary layers
  • Typical cell size dimensions of 1 or 2 mm are recommended, avoiding highly skewed cells; the angles between the grid lines and the boundary of the computational domain (the wall or the inlet- and outlet-boundaries) should be close to 90 degrees.

More generally, studies seem to indicate that meshes of at least 125000 points are necessary to reduce numerical errors to acceptable, if low, level in 3D calculations.

For IC engines, LES mesh requirements seem to be comparable to those needed to obtain RANS grid independent (to a 10%-20% level) computation, so this is not a discriminating criteria.

In an IC engine one cannot forget the effect of the walls on the flow. There are two alternatives: refine drastically the mesh near the walls and modify the turbulence model, or use ‘wall functions’ (such as functions derived from 1D steady Couette flow analysis). The wall functions are often preferred; they give acceptable results without surcharging the calculations with numerous mesh nodes.

Different methods can be used. The body force method is well suited to dynamic SGS LES model, and could perform well on normal workstations, but its physical approach (strict incompressibility) is not recommended for IC engine, for obvious reasons. Furthermore, implementing advanced boundaries (with wall laws for example) is very difficult. The Arbitrary Lagrangian Eulerian (ALE) method allows fully unstructured meshes. Arbitrary mesh motion is possible to accommodate piston and valves, and can be calculated independently. This method was used in several cases with success.

7.5. Discretisation method and solution algorithms

  • Use at least a second order accuracy in space and time. It may be necessary to use a 1st order scheme at the start of a calculation. Through the bibliographical review, simulations are based on second order for spatial discretisation, but only first order implicit time differencing for temporal discretisation. In this case the time step is chosen far below the Kolmogorov time scale, which is in the order of 10e-4 -– 10e-5 for a size of a typical IC engine.
  • Uniform time steps could be used for most of the simulation, although it is recommended to reduce the time steps around events such as the intake valve opening and closing (for example a time step 0.5 CAD (crank angle degree) to be reduced to 0.1 CAD for approximately 5 CAD).
  • It is recommended to check the influence of the time-step on the results.
  • In absence of other information, it is advised to assume quiescent mean flow and 10% turbulence intensity for initial conditions.

There are several schemes available and documented, but they are rarely compared in the case of an IC engine. The most known and used are perhaps (this is not exhaustive) PISO, SIMPLE, QUICK, HYBRID and SUDS. QUICK is free of any numerical diffusion, and SUDS reduces greatly this source of errors. However, they are both unbounded; this could be problematic in regions having large gradients of turbulence quantities. In this case, it is recommended to use a bounded scheme when an unbounded solution arises, and the more accurate QUICK/SUDS everywhere else. In a comparison between HYBRID and QUICK, the latter showed markedly better results. There are also the iterative SIMPLE and non-iterative PISO. PISO is recommended for an IC engine, comparison showed that PISO is four time faster than SIMPLE.

© copyright ERCOFTAC 2004



Contributors: Afif Ahmed - RENAULT


Front Page

Description

Test Case Studies

Evaluation

Best Practice Advice

References