To enable the dynamic mesh model, turn on Dynamic Mesh in the Dynamic Mesh Parameters panel (Figure 11.7.1) .
Define Dynamic Mesh Parameters...
If you are modeling in-cylinder motion, turn on the In-Cylinder option. If you are modeling 2.5D applications (e.g., pumps) , turn on the 2.5D option (3D flows only). If you are going to use the six degrees of freedom solver , then turn on the Six DOF Solver option.
Next, you will need to select the appropriate mesh update methods, and set the associated parameters, as well as the in-cylinder or Six DOF parameters, if relevant.
Selecting the Mesh Update Methods
Under Mesh Methods, select Smoothing, Layering, and/or Remeshing. Details about these methods and their applicability to different cases are provided in Section 11.3.2. Information about setting parameters for the mesh update methods is provided below.
Setting Mesh Update Parameters
To turn on spring-based (or Laplacian smoothing if the 2.5D model is enabled), enable the Smoothing option under Mesh Methods in the Dynamic Mesh panel (Figure 11.7.1). The relevant parameters are specified in the Smoothing tab.
You can control the spring stiffness by adjusting the value of the Spring Constant Factor between 0 and 1. A value of 0 indicates that there is no damping on the springs, and boundary node displacements have more influence on the motion of the interior nodes. A value of 1 imposes the default level of damping on the interior node displacements as determined by solving Equation 11.3-3.
The effect of the Spring Constant Factor is illustrated in Figures 11.7.2 and 11.7.3, which show the trailing edge of a NACA-0012 airfoil after a counter-clockwise rotation of 2.3 and the mesh is smoothed using the spring-based smoother but limited to 20 iterations. Degenerate cells (Figure 11.7.2) are created with the default value of 1 for the Spring Constant Factor. However, the original mesh distribution (Figure 11.7.3) is recovered if the Spring Constant Factor is set to 0 (i.e., no damping on the displacement of nodes on the airfoil surface).
If your model contains deforming boundary zones, you can use the Boundary Node Relaxation to control how the node positions on the deforming boundaries are updated. On deforming boundaries, the node positions are updated such that
where is the Boundary Node Relaxation. A value of 0 prevents deforming boundary nodes from moving (equivalent to turning off smoothing on deforming boundary zones) and a value of 1 indicates no under-relaxation.
You can control the solution of Equation 11.3-3 using the values of Convergence Tolerance and Number of Iterations. FLUENT solves Equation 11.3-3 iteratively during each time step until one of the following criteria is met:
where is the interior and deforming nodes RMS displacement at the first iteration.
Note that for 2.5D modeling (3D flows only), you can only change the Boundary Node Relaxation and the Number of Iterations. Note that the Number of Iterations is used for both spring-based and Laplacian smoothing . The Boundary Node Relaxation is used differently by FLUENT when the 2.5D model is used. On deforming boundaries, the node positions are updated such that
To turn on dynamic layering, enable the Layering option under Mesh Methods in the Dynamic Mesh Parameters panel (Figure 11.7.4). The layering control is specified in the Layering tab.
You can control how a cell layer is split by specifying either Constant Height or Constant Ratio under Options. The Split Factor and Collapse Factor ( in Equation 11.3-7 and in Equation 11.3-8, respectively) are the factors that determine when a layer of cells (hexahedra or wedges in 3D, or quadrilaterals in 2D) that is next to a moving boundary is split or merged with the adjacent cell layer, respectively.
To turn on local remeshing, enable the Remeshing option under Mesh Methods in the Dynamic Mesh Parameters panel (Figure 11.7.5). The local remeshing controls are specified in the Remeshing tab.
You can view the vital statistics of your mesh by clicking the Mesh Scale Info... button. This displays the Mesh Scale Info panel where you can view the minimum and maximum length scale values as well as the maximum cell and face skewness values.
In local remeshing, FLUENT agglomerates cells based on skewness, size, and height (adjacent moving face zones). The value of Maximum Cell Skewness indicates the desired skewness of the mesh. By default, the Maximum Cell Skewness is set to 0.9 for 3D simulations and 0.6 for 2D simulations. Cells with skewness above the maximum skewness are marked for remeshing. The size criteria are specified with Minimum Length Scale and Maximum Length Scale. Cells with length scales below the minimum length scale and above the maximum length scale are marked for remeshing.
For 3D simulations, the Face Remeshing option is available, allowing you the convenience of remeshing deforming boundary faces if you so desire. Once the option is turned on, you are able to set the Maximum Face Skewness to a specific value. In addition, you should turn on the Remeshing option in the Meshing Options tab of the Dynamics Zones panel for a deforming zone type (see Section 11.7.2). You also have the option of choosing either the local face remeshing method or the face region remeshing methods by selecting the appropriate option under Remeshing Methods for a deforming zone type. Note that depending on the case, either or both methods have to be enabled.
The marking of cells based on skewness is done at every time step when the local remeshing method is enabled. However, marking based on size and height is performed between the specified Size Remesh Interval since the change in cell size distribution is typically small over one time step.
By default, FLUENT replaces the agglomerated cells only if the quality of the remeshed cells has improved. However, you can override this behavior by disabling Must Improve Skewness under Options.
When you use the Size Function remeshing option (see Figure 11.7.6), you can control three parameters that govern the size function. You can specify the Size Function Resolution, the Size Function Variation, and the Size Function Rate or you can return to FLUENT's default values by using the Use Defaults button.
The Size Function Resolution controls the density of the background grid (see Section 11.3.2). By default, it is equivalent to 3 in 2D simulations and 1 in 3D simulations.
The Size Function Variation corresponds to in Equation 11.3-12. It is the measure of the maximum permissible cell size and it ranges from .
The Size Function Rate corresponds to in Equation 11.3-12. It is the measure of the rate of growth of the cell size, and it ranges from . A value of 0 implies linear growth, whereas higher values imply a slower growth near the boundary with faster growth as one moves toward the interior.
Setting In-Cylinder Parameters
If you turn on the In-Cylinder model in the Dynamic Mesh Parameters panel (Figure 11.7.1), you need to 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, FLUENT assumes a Crank Angle Step Size of 0.5 degree.
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
where is the piston location (0 at top-dead-center (TDC) and at bottom-dead-center (BDC)), is the connecting rod length, is the piston stroke, and is the current crank angle. The current crank angle is calculated from
where is the Starting Crank Angle and 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
where is the valve lift computed from the appropriate valve profiles, is the Minimum Valve Lift, is the stroke calculated from Equation 11.7-4, and is the Piston Stroke Cutoff. (See Section 11.7.5 on how the Piston Stroke Cutoff is used to control the onset of layering in the cylinder chamber.)
Setting Six DOF Solver Parameters
To use the six degree of freedom solver for your unsteady dynamic mesh simulation, select Six DOF Solver under Models in the Dynamic Mesh Parameters panel (Figure 11.7.1) and click on the Six DOF Solver tab (Figure 11.7.8).
Define Dynamic Mesh Parameters
You can specify the gravitational acceleration in the x, y, and z directions either in this panel, or in the Operating Conditions panel.