Intake And Exhaust Manifolds Simulation

Intake and Exhaust Manifolds Simulation - Comparison With Experiment BOHUMIL MAREŠ, PAVEL BAUMRUK ČVUT v Praze / Výzkumné centrum spal. motorů a automobilů Josefa Božka, Technická 4, 166 07 Praha 6; Tel. +420224352507, Fax. +420224352500, [email protected]

SHRNUTÍ V článku autoři analyzují možnosti numerické simulace proudění v sacích a výfukových potrubích. Při vlastním řešení jsou aplikovány výpočetní metody, které umožňují posoudit vhodnost použité metody při srovnání s experimentálně zjištěnými parametry. Model pro výpočet byl vytvořen na základě stacionární aerodynamické zkoušky, obvykle používané k určení integrálních parametrů proudového pole, v našem případě průtokových součinitelů. Ty mohou být využity pro porovnání dat získaných při experimentu a výsledků numerického řešení. Matematický model byl realizován v prostředí CFD kódu FLUENT. Vzhledem k závislosti výsledků numerické simulace na struktuře a hrubosti výpočetní sítě a použitém modelu turbulence je třeba jisté obezřetnosti při prezentaci výsledků.

KLÍČOVÁ SLOVA CFD, stacionární aerodynamická zkouška, průtokový součinitel

ABSTRACT The aim of the article is to analyze possibilities of a numerical simulation of a flow in intake and exhaust manifolds. The solution is particularly intended on an assignment of a calculation method to obtain the same results as the experimental ones. The model was created on the basis of the steady flow test, usually employed in order to determine flow discharge coefficient. This integral flow field parameter can be used to compare experimental measurements and calculated data. The numerical solution has been realized using commercial CFD code FLUENT. Due to dependence of the simulation results on the grid coarseness and the turbulence model, the numerical methods have to be used with certain cautiousness.

KEYWORDS CFD, steady flow test, discharge coefficient

1. INTRODUCTION In connection with growing demands on reduction of ICE exhaust gas emissions and fuel consumption simultaneously with increasing of its performance, new designs and optimization of existing ones are introduced. Resistance losses in intake and exhaust manifolds form a significant part of efficiency losses. Not only experiments but also mathematical modeling can be employed to determine and optimize flow field parameters. The article presents comparison of the numerical simulation results and experimentally obtained data. Both simple and branched model configurations of an ICE intake and exhaust manifolds and real intake manifold of 3-cylinder Škoda engine were compared. Four basic cases were resolved: - Smooth-surfaced pipeline with an orifice, - T pipes, - One inlet and four outlets - “4-1 manifold” (inverse flow direction respectively) and selected combinations, - Real intake manifold geometry (3-cylinder Škoda engine)

2. EXPERIMENTS As mentioned before, the steady flow test was employed to determine discharge coefficients, (see scheme in Figure 1).

Figure 1: Steady flow rig Obrázek 1: Aerodynamická trať Particular model configurations were made of plastic pipes with 28mm internal diameter and connecting T-parts. In a steady flow rig, volume flow was measured for constant pressure drops of 2.45, 4.9, 7.35 and 9.8 kPa. Setting accuracy of the pressure drop depends on control elements sensitivity, for higher pressure drops the setting accuracy is approximately 1%.

3. MATHEMATICAL MODELING Geometrical shapes of the model configurations were created under use of graphical pre-processor GAMBIT. In the case of the 3-cylinder Škoda engine intake manifold, real geometry was obtained from CAD system Pro/Engineer and transferred into GAMBIT. First it was necessary to eliminate unneeded planes, edges and vertices and correct some discontinuities and inaccuracies. Then the hybrid volume computational grids were created for every particular case. In plain parts of the pipes hexahedral grid was applied. In complex ones unstructured tetrahedral grid was applied. Finally, the grids were imported to FLUENT. Generally, the 3D flow is described by equation of conservation of mass (the continuity equation), set of Navier-Stokes equations and energy equation. Closure of the governing equations is in this case achieved by an RNG k-ε turbulence model. The flow was assumed to be steady and turbulent. Boundary conditions were held in agreement to the experiment, i.e. the constant pressure drop of 2.45 (4.9, 7.35 and 9.8) kPa was considered. At solid walls, fluid mean velocities were considered to be zero and the traditional wall law was applied. When the flow enters the domain at an inlet or outlet boundary, FLUENT requires specification of transported scalar quantities. To specify them, the turbulence intensity and hydraulic diameter method was used. Inlet: Turbulence intensity 5%

Hydraulic diameter - intake port diameter Outlet: Turbulence intensity 10% Hydraulic diameter - outlet port diameter The governing equations were solved iteratively with the SIMPLE algorithm. To acquire more data, there were combined various types of inlet and outlet shapes, more specifically designs, which affect intake and outlet losses – discharge nozzles. It relates also with boundary condition adjustment in FLUENT. If the pressure inlet and outlet boundary conditions are applied, intake and outlet losses are not considered, while in experiments they form significant fraction of total losses. There were created intake and outlet vessels for case of 4-1 manifold to correct this inaccuracy.

4. COMPUTED AND MEASURED DATA EVALUATION The flow discharge coefficients mi, mis respectively have been defined as a ratio of computed (measured) mass to theoretical one. Flows through the inlet port/valve assembly for a given valve lift were investigated. Definition sounds as follows:

& real m , & theor m

mi exp =

& FL m & teor m

Discharge coefficient

p b - ∆p1 287 *Tb

ρair =

& V real = 179.53

π =

mi FL =

Air density [kg.m-3]

Tb π (1 - 0.344 π )

Volume flow - experiment [m-3.h-1]

∆p c p b - ∆p1

& ρ & real = V m real air

w theor =

 p b - ∆p1   κ  2 R To 1-   κ -1   pb 

& theor = S ρ air w theor m

κ -1 κ

Theoretical air speed [m3.h-1]

Theoretical mass flow [kg.h-1]

5. RESULTS AND DISCUSSION Respecting the extent of this article, only several specific results can be presented. They are discussed in the following. T-pipes Scheme of this model is shown in figure 2. Particular pipe elements lengths were designed to match five-fold of the pipes internal diameter. This length is necessary for velocity profile formation.

Figure 2: Schemes of the compared variants – side inlet and side outlet Obrázek 2: Schéma variant T-potrubí: vlevo boční vstup, vpravo boční výstup

Two configurations were created and compared – side inlet and side outlet. Figure 3 shows discharge coefficients depending on pressure drop in case of side inlet. Flag D is for discharge nozzle on inlet and outlet. It is evident, that discharge coefficients increase if the discharge nozzles are used in experiment. In FLUENT, with respect to boundary condition setting, they represent dissipation. 0,85

mi [1 ]

0,8

0,75

mi 0,7

mifluent

miD

mifluentD 0,65 2

3

4

5

6

7

8

9

10

dp [kPa]

Figure 3: Discharge coefficients for side inlet configuration Obrázek 3: Průtokové součinitele pro verzi bočního vstupu One inlet and four outlets - “4-1 manifold” Highly simplified model of real intake or exhaust manifold is presented in Figure 4. 12 various configurations were created closing particular inlets or outlets respectively.

Figure 4: One inlet and four outlets - “4-1 manifold” Obrázek 4: Model potrubí 4-1 Figure 5 shows both measured and computed values of the discharge coefficients for these 12 versions without using any discharge nozzles. Figure 6 illustrates changes in the discharge coefficients magnitude if intake and outlet vessels are applied. X-axis represents individual variants with their

0,9

90

0,8

80

0,7

70

0,6

60

0,5

50 mi_exp mi_fluent dmi

0,4 0,3

40

dmi [ % ]

mi [ 1 ]

schemes, left-hand side placed pointer indicates flow direction, and air-carrying parts of the manifolds are highlighted. Presented discharge coefficients magnitudes are mean value of the four various values of pressure differences (main y-axis). Relative deviation between measured and computed data is plotted on the right-hand placed y-axis. It is obvious, that these differences are minimized if the vessels are applied (see Figure 6), but it changes with variants. This fact may be caused by geometrical inaccuracies in real model, namely in connection of straight pipe elements and T-parts. It is impossible to determine exact geometry inside the manifold.

30

0,2

20

0,1

10

0,0

0 Variants

Figure 5: Average values of the measured and computed discharge coefficients and their relative deviations for configurations without inlet and outlet modifications Obrázek 5: Průměrné hodnoty naměřených a vypočtených průtokových součinitelů a jejich rozdíly pro varianty modelů bez úprav vstupu a výstupu

0,9

0,7

9 8 7

mi [ 1 ]

0,6

6

0,5

5 0,4

4

0,3

dmi [ % ]

0,8

10 mi_exp mi_fluent dmi

3

0,2

2

0,1

1

0,0

0 Variants

Figure 6: Average values of the measured and computed discharge coefficients and their relative deviations for configurations with intake and outlet vessels Obrázek 6: Průměrné hodnoty naměřených a vypočtených průtokových součinitelů a jejich rozdíly pro varianty modelů s nátokovou a výtokovou nádobou Discharge coefficient magnitudes are significantly affected by flow field structure in the inlet area and furthermore downstream the flow in pipeline. Figure 7 illustrates the influence of the intake vessel utilization on the velocity profile in the entry area. Quite good agreement was achieved between computed and measured data under use of model shown in Figure 8 together with demonstration of flow field velocity magnitude distribution for one of the considered configurations.

Figure 7: Inlet into a pipe in FLUENT – without modifications of inlet area (left pipe) and with the intake vessel (right pipe) Obrázek 7: Vtok do potrubí ve FLUENTU – vlevo bez úprav vstupu (bez ztrát), vpravo s nátokovou nádobou

Figure 8: Model with the intake and outlet vessels together with illustration of flow field velocity magnitude distribution for one of the considered configurations. Obrázek 8: Model s nátokovou a výtokovou nádobou včetně ukázky rozložení velikostí rychlostí pro jednu z uvažovaných konfigurací

Real intake manifold geometry

Figure 9: Scheme of the intake manifold model after import to GAMBIT Obrázek 9: Zobrazení modelu sání po importu do programu GAMBIT As mentioned before, the intake manifold module of 3-cylinder 1.2-litre Škoda engine was applied for the comparison of the numerical simulation with the experiment. Both the real intake manifold and its corresponding computer model (CAD system Pro/Engineer) were available. The latter one had to be modified to create a mesh. Therefore, only boundary surfaces were used. The computer model is drawn in Figure 7. A flow was considered to enter the manifold at a plenum volume and than to flow towards one cylinder only through one branch (flag 1,2 and 3, where branch 1 is closest to inlet) remaining manifold branches were closed. In this case, computed discharge coefficients were lower compared with measured ones (see Table 1). This might be caused by smaller influence of intake pressure loss due to a greater intake orifice and therefore lower inlet velocities. When the inlet discharge nozzle is used, the differences between the simulation and the experiment are almost the same (see Table 2). On the other hand, when the outlet discharge nozzle is used, the correspondence of the computation with the measurement is improved again. This is due to the lower outlet pressure loss for higher outlet velocities (Table 3).

mi

mi_fluent

dmi

[1]

[1]

[%]

Inlet 1

0,809

0,752

-7,08

Inlet 2

0,813

0,773

-4,93

Inlet 3

0,831

0,770

-7,34

Variant

Table 1: Discharge coefficients and percentage departure for configurations without adaptations of inlet and outlet Tabulka 1: Průtokové součinitele a jejich rozdíly pro variantu bez úpravy vstupu a výstupu

mi

mi_fluent

dmi

[1]

[1]

[%]

Inlet 1

0,810

0,752

-7,19

Inlet 2

0,818

0,773

-5,43

Inlet 3

0,831

0,772

-7,17

Variant

Table 2: Discharge coefficients and percentage departure for configurations with inlet nozzle Tabulka 2: Průtokové součinitele a jejich rozdíly pro variantu se vstupní dýzou

mi

mi_fluent

dmi

[1]

[1]

[%]

Inlet 1

0,874

0,866

-0,90

Inlet 2

0,883

0,887

0,55

Inlet 3

0,897

0,883

-1,61

Variant

Table 3: Discharge coefficients and percentage departure for configurations with adaptations of inlet and outlet Tabulka 3: Průtokové součinitele a jejich rozdíly pro variantu s vstupní výstupní dýzou

6. CONCLUSION Boundary conditions formulation and setting approach has a significant influence on calculated data accuracy. In all investigated cases, agreement of experimentally obtained values of discharge coefficient with results of numerical simulations is relatively good. Percentage departure of the discharge coefficient does not exceed 5%, if inlets and outlets are modified. Other considerable impact on precision of the numerical simulations has both grid coarseness and its structure, namely in areas of high pressure or velocity gradients. Choice of turbulence model is very important too. In this case, model RNG k-ε performs relatively well, and the additional computational expense of more complex models was not justified.

ACKNOWLEGEMENTS This work has been supported by the Josef Božek Research Centre, No. LN00B073. This help is gratefully appreciated.

REFERENCES [1] Chaloupka. S.: Matematické modelování proudění v sacích a výfukových potrubích. Diplomová práce D2002-M10, ČVUT, U220.1.2002. [2] Dvořák,R.-Kozel,K. : Matematické modelování v aerodynamice. ČVUT, Praha 1996, ISBN 80-0101541-6. [3] Ferziger,J. H.-Peric, M.: Computational methods for fluid dynamics. Springer, 1999, ISBN 3-54065373-2. [4] Baumruk,P. : Problematika náplně válce spalovacích motorů. Skripta ČVUT, Praha 1996, ISBN 80-01-02010-X.