[ANSYS, Inc. Logo] return to home search
next up previous contents index

11.3.6 Setting In-Cylinder Parameters

You can enable the In-Cylinder option in the Dynamic Mesh task page (Figure  11.3.1) and click the Settings... button under Options to display the In-Cylinder Settings dialog box. Specify the Crank Shaft Speed, the Starting Crank Angle, and the Crank Period which are used to convert between flow time and crank angle. You must also specify the time step to use for advancing the solution in terms of crank angle in Crank Angle Step Size. By default, ANSYS FLUENT assumes a Crank Angle Step Size of 0.5 degree.

Figure 11.3.16: The In-Cylinder Settings Dialog Box

ANSYS FLUENT provides a built-in function to calculate the piston location as a function of crank angle. If the piston motion is specified using this function, you need to specify the Piston Stroke and Connecting Rod Length. The piston location is calculated using

 p_s = L + {A\over 2}(1 - \cos{(\theta_c)}) - \sqrt{L^2 - {A^2\over 4}\sin^2{(\theta_c)}} (11.3-11)

where $p_s$ is the piston location (0 at top-dead-center (TDC) and $A$ at bottom-dead-center (BDC)), $L$ is the connecting rod length, $A$ is the piston stroke, and $\theta_c$ is the current crank angle. The current crank angle is calculated from

 \theta_c = \theta_s + t \Omega_{\rm shaft} (11.3-12)

where $\theta_s$ is the Starting Crank Angle and $\Omega_{\rm shaft}$ is the Crank Shaft Speed.

The Piston Stroke Cutoff and Minimum Valve Lift values are used to control the actual values of the valve lift and piston stroke such that

$\displaystyle v_{\rm lift}$ $\textstyle =$ $\displaystyle \mbox{max}(v^c_{\rm lift}, v^{\rm min}_{\rm lift})$ (11.3-13)
$\displaystyle p_s$ $\textstyle =$ $\displaystyle \mbox{min}(p^c_s, p^{\rm min}_s)$ (11.3-14)

where $v^c_{\rm lift}$ is the valve lift computed from the appropriate valve profiles, $v^{\rm min}_{\rm lift}$ is the Minimum Valve Lift, $p^c_s$ is the stroke calculated from Equation  11.3-11, and $p^{\rm min}_s$ is the Piston Stroke Cutoff. (See Section  11.3.6 on how the Piston Stroke Cutoff is used to control the onset of layering in the cylinder chamber.)

At the bottom of the In-Cylinder Settings dialog box is an Output Controls... button. Click this button to display the In-Cylinder Output Controls dialog box. In the In-Cylinder Output Controls dialog box, you can specify various quantities needed for the calculation of swirl and tumble along with the frequency of writing the output to the chosen file. Swirl is used to describe circulation about the cylinder axis. Tumble flow circulates around an axis perpendicular to the cylinder axis, orthogonal to swirl flow.

Figure 11.3.17: The In-Cylinder Output Controls Dialog Box

The following list describes the In-Cylinder Output Controls dialog box.

In-Cylinder Data Write Frequency   is an integer entry specifying the interval in number of time-steps.

Swirl Center Method   is a drop-down list which allows you to select the method to calculate the swirl center. The list contains center of gravity and fixed, with center of gravity being the default value.

center of gravity   option calculates the swirl center inside the code and is used as the center of gravity of the chosen cell zones.

fixed   option enables you to specify a swirl center in the entries below the drop-down list.

In addition to these two options, you can chose to use your own compiled UDF to calculate the swirl center.

For details on using a dynamic mesh UDF, see the separate UDF Manual for information on user-defined functions.

Cell Zones   is a list which displays the names of all existing cell zones in the case files. You can select only the zones relevant for the swirl and tumble calculations.

Swirl Axis   specifies the swirl axis with three entries for the directional components. By default, X, Y, Z= 0, 1, 0.

Tumble X-Axis   specifies the directional components of Tumble X-Axis in X, Y, Z directions. By default, X, Y, Z = 0, 0, 1. This applies only in 3D.

Tumble Y-Axis   specifies the directional components of Tumble Y-Axis in X, Y, Z directions. By default, X, Y, Z = 1, 0, 0. This applies only in 3D.

File Name   specifies the name of the In-Cylinder output file. By default, the file name contains the name of the case file appended with a .txt extension.

The In-Cylinder specific output controls can also be controlled using the TUI as follows:

Go to 
\html{\begin{rawhtml}<p><font color="forestgreen">\end{rawhtml}}\mpath{define}\mpath{models}\mpath{dynamic-mesh-controls}\tui{in-cylinder-output?} \html{\begin{rawhtml}</font>\end{rawhtml}}


Enable in-cylinder output?[no]yes

Output Write Frequency[0]10

Cell zone name/id(1)[()]2

Cell zone name/id(1)[()]
File Name["/nfs/devvault/data9/ic-sp-output.txt'']
Swirl Center Method:  (fixed cg user-defined)
Swirl Axis x[0]
Swirl Axis y[1]
Swirl Axis z[0]
Tumble X-Axis x[0]
Tumble X-Axis y[0]
Tumble X-Axis z[1]
Tumble Y-Axis x[1]
Tumble Y-Axis y[0]
Tumble Y-Axis z[0]

If you select fixed as the choice at Swirl Center Method then you will be prompted to enter the swirl center as follows:

Swirl Center(x) (mm) [0]
Swirl Center(y) (mm) [0]
Swirl Center(z) (mm) [0]
If a swirl center method UDF has been compiled already and loaded into UDF then you can choose user-defined as the swirl center method option, in such a case the following is the sequence of prompts.

Swirl Center UDF[] swirl_udf::libudf

If the name of the UDF library is libudf then you can omit this and enter in the swirl center UDF[]swirl_udf, otherwise the name of the UDF followed by the UDF library name with symbol:: in between, should be entered.

By filling up the various entries that are needed in the In-Cylinder Output Controls dialog box and pressing the OK button, the swirl and tumble calculations will be written at the chosen frequency to the chosen file while doing the solution run. Details of the quantities written to the file are as follows:

CA   = Crank Angle

m   = Mass of the entire fluid contained in the selected cell zones.

L   = Angular momentum vector of fluid mass contained in selected cell zones with respect to the swirl center.

$\vert\vec{L}\vert$   = Magnitude of angular momentum of fluid.

$\vec{sa}$   = Swirl Axis

$\vec{tx}$   = Tumble X-Axis

$\vec{ty}$   = Tumble Y-Axis

I $_{sa}$   = Moment of inertia of the fluid mass about Swirl axis

I $_{tx}$   = Moment of inertia of the fluid mass about Tumble X-Axis.

I $_{ty}$   = Moment of inertia of the fluid mass about Tumble Y-Axis.

$\cdot$   = Dot product between two vectors.

Altogether, eight quantities are written to the output file in the following order, column wise from left to right. A sample file is shown below:

Figure 11.3.18: Sample Output File Showing Various Quantities

Using the In-Cylinder Option

This section describes the problem setup procedure for an in-cylinder dynamic mesh simulation.


Consider the 2D in-cylinder example shown in Figure  11.3.19 for a typical pent-roof engine.

Figure 11.3.19: A 2D In-Cylinder Geometry

In setting up the dynamic mesh model for an in-cylinder problem, you need to consider the following issues:

Defining the Mesh Topology

ANSYS FLUENT requires that you provide an initial volume mesh with the appropriate mesh topology such that the various mesh update methods described in Section  11.3.2 can be used to automatically update the dynamic mesh. However, ANSYS FLUENT does not require you to set up all in-cylinder problems using the same mesh topology. When you generate the mesh for your in-cylinder problem (using GAMBIT or other mesh generation tools), you need to consider the various mesh regions that you can identify as moving, deforming, or stationary, and generate these mesh regions with the appropriate cell shape.

The mesh topology for the example problem in Figure  11.3.19 is shown in Figure  11.3.20, and the corresponding volume mesh is shown in Figure  11.3.21.

Figure 11.3.20: Mesh Topology Showing the Various Mesh Regions

Figure 11.3.21: Mesh Associated With the Chosen Topology

Because of the rectilinear motion of the moving surfaces, you can use dynamic layering zones to represent the mesh regions swept out by the moving surfaces. These regions are the regions above the top surfaces of the intake and exhaust valves and above the piston head surface, and must be meshed with quadrilateral or hexahedral cells (as required by the dynamic layering method).

For the chamber region, you need to define a remeshing zone (triangular cells) to accommodate the various positions of the valves in the course of the simulation. In this region, the motion of the boundaries (valves and piston surfaces) is propagated to the interior nodes using the spring-based smoothing method. If the cell quality violates any of the remeshing criteria that you have specified, ANSYS FLUENT will automatically agglomerate these cells and remesh them. Furthermore, ANSYS FLUENT will also remesh the deforming faces (based on the minimum and maximum length scale that you have specified) on the cylinder walls as well as those on the sliding interfaces used to connect the chamber cell zone to the layering zones above the valve surfaces.

For the intake and exhaust port regions, you can use either triangular or quadrilateral cell zones because these zones are not moving or deforming. ANSYS FLUENT will automatically mark these regions as stationary zones and will not apply any mesh motion method on these cell zones.

The dynamic layering regions above the piston and valves are conformal with the adjacent cell zone in the chamber and ports, respectively, so you do not have to use sliding interfaces to connect these cell zones together. However, you need to use sliding interfaces to connect the dynamic layering regions above the valves and the remeshing region in the chamber. This is shown in Figure  11.3.22 with the exhaust valve almost at full extension. Notice that cells on the chamber side of the interface zone are remeshed (i.e., split or merged) as the interface zone opens and closes because of the motion of the exhaust valve.

Figure 11.3.22: The Use of Sliding Interfaces to Connect the Exhaust Valve Layering Zone to the Remeshing Zone

Defining Motion/Geometry Attributes of Mesh Zones

As the piston moves down from the TDC to the BDC position, you need to expand the remeshing region such that it can accommodate the valves when they are fully extended. To accomplish this, you need to specify the dynamic layering zone adjacent to the piston surface to move with the piston until some specified distance from the TDC position. Beyond this cutoff distance, the motion of the layering zone is stopped and the piston wall is allowed to continue to the BDC position. Because there is relative motion between the piston head surface and the now non-moving dynamic layering zone, cell layers will be added when the ideal layer height criteria is violated. Figures  11.3.23 to 11.3.28 show the sequence of meshes before and after the onset of cell layering when the motion in the layering zone above the piston surface is stopped (shown with $\Delta\theta$ = 5 $^\circ$).

Figure 11.3.23: Mesh Sequence 1

Figure 11.3.24: Mesh Sequence 2

Figure 11.3.25: Mesh Sequence 3

Figure 11.3.26: Mesh Sequence 4

Figure 11.3.27: Mesh Sequence 5

Figure 11.3.28: Mesh Sequence 6

ANSYS FLUENT provides built-in functions to handle the full piston motion and the limited piston motion for the dynamic layering zone above the piston surface. When you define the motion attribute of the dynamic layering zone above the piston surface, you need to use the limited piston motion function ( **piston-limit** in the C.G. Motion UDF/Profile field in the Dynamic Mesh Zones dialog box). Note that you must define the parameters used by these functions before you can use them. In the current example, the piston stroke is 80 mm and the connecting rod length is 140 mm. The piston stroke cutoff is assumed to happen at 25 mm from TDC position. The lift as a function of crank angle between $344^\circ$ and $1064^\circ$ is shown in Figure  11.3.29 for both limited and full piston motion.

Figure 11.3.29: Piston Position (m) as a Function of Crank Angle (deg)

To define the motion of the valves, you need to use profiles that describe the variation of valve lift with crank angle. ANSYS FLUENT expects certain profile fields to be used to define the lift and the crank angle. For example, consider the following simplified profile definition:

((ex-valve 5 point)
 (angle 0   180  270  360   720)
 (lift 0.05 0.05 1.8  0.05 0.05))

((in-valve 5 point)
 (angle 0   355   440  540  720)
 (lift 0.05 0.05 2.0 0.05 0.05))

ANSYS FLUENT expects the angle and lift fields to define the crank angle and lift variations, respectively. The angle must be specified in degrees and the lift values must be in meters. The actual valve lift profiles that you will use for the current example are shown in Figure  11.3.30. Notice that there is an overlapped period where both the intake and exhaust valves are open.

Figure 11.3.30: Intake and Exhaust Valve Lift (m) as a Function of Crank Angle (deg)

The valve lift profiles and the built-in functions will describe how each surface moves as a function of crank angle with respect to some reference point. For example, the valve lift is zero when the valve is fully closed and the valve lift is maximum when it is fully open. In order to move the surfaces, ANSYS FLUENT requires that you specify the direction of motion for each surface. ANSYS FLUENT will then update the "center of gravity'' of each surface such that

 \vec{x} = \vec{x}_{\rm ref} - l\vec{e}_{\rm axis} (11.3-15)

where $\vec{x}_{\rm ref}$ is some reference position, $\vec{e}_{\rm axis}$ is the unit vector in the direction of motion, and $l$ is either the valve or the piston distance with respect to the reference position $\vec{x}_{\rm ref}$. Note that the unit vector of the direction of motion is specified to point in the negative direction. For example, the correct intake valve axis for this example is $(-0.3421,~ 0.9397)$, as shown in Figure  11.3.31.

Figure 11.3.31: Definition of Valve Zone Attributes (Intake Valve)

Defining Valve Opening and Closure

ANSYS FLUENT assumes that once you have set up the mesh topology, the mesh topology is unchanged throughout the entire simulation. Therefore, ANSYS FLUENT does not allow you to completely close the valves such that the cells between the valve and the valve seat become degenerate (flat cells) when these surfaces come in contact (removing these flat cells would require the creation of new boundary face zones). To prevent the collapse, you need to define a minimum valve lift and ANSYS FLUENT will automatically stop the motion of the valve when the valve lift is smaller than the minimum valve lift value. The minimum valve lift value can be specified in the In-Cylinder Settings dialog box. For the current example, a minimum valve lift value of 0.1 mm is assumed.

When the valve position is smaller than the minimum valve lift value, it is normal practice to assume that the valve is closed. The actual closing of the valves is accomplished by deleting the sliding interfaces that connect the chamber cell zone to the dynamic layering zones on the valves. The interface zones are then converted to walls to close off the "gaps'' between the valves and the valve seats.

The valve opening is achieved by the reverse process. When the valve lift has reached beyond the minimum valve lift value, the valve is assumed to be open and you can redefine the sliding interfaces such that the chamber zone is now connected to the dynamic layering zones above the valves.

next up previous contents index Previous: 11.3.5 Steady-State Dynamic Mesh
Up: 11.3 Using Dynamic Meshes
Next: 11.3.7 Six DOF Solver
Release 12.0 © ANSYS, Inc. 2009-01-29