The workspace can calculate the local shear rate () on the part of the domain where the velocity field has been calculated. The shear rate is given by

(4–9)

Properties include:

For generalized Newtonian fluids and simplified viscoelastic fluids, the workspace can calculate the local value of the viscosity, which can depend on the shear rate and/or the temperature. The viscosity will appear as a scalar field while postprocessing.

Properties include:

For generalized Newtonian models and simplified viscoelastic fluids, the workspace can calculate the heat generation per unit time and per unit volume (or per unit area for a 2D planar case) that is generated under the given flow conditions. The heat generation originates from the work of internal forces. In addition to the viscous and wall friction heating, the workspace evaluates the dissipated power, which is the integral of the viscous and wall friction heating over the flow domain. When wall slippage is defined, the calculation of the dissipated power also considers the contribution originating from the slipping force, and results are provided for the volume dissipated power and the heat generated from slipping.

It is not necessary to solve a nonisothermal problem in order to compute the viscous and wall friction heating. The workspace can calculate the viscous dissipation that occurs without actually solving the energy equation. Also, the workspace can calculate the viscous and wall friction heating even if it has been neglected in the main nonisothermal flow problem.

Properties include:

For generalized Newtonian model, the workspace can calculate the extra-stress tensor on the part of the domain where the velocity field has been calculated. Three components of the inelastic stress tensor will be calculated for 2D planar cases, four components for 2D axisymmetric cases, and six components for all other cases.

For differential or simplified flow problems, the workspace can calculate the total extra-stress tensor in the domain. The total extra-stress tensor is the sum of the viscous (or the (generalized) Newtonian) components and the viscoelastic components. If more than one relaxation time has been defined, the viscoelastic component is the sum of the viscoelastic components for all modes.

Properties include:

With this postprocessor, you can evaluate the volume of the flow domain. If the flow domain contains overlapping internal restrictor or moving parts, the calculation of the volume will remove the part of the flow domain overlapped by these parts, in order to provide the actual volume occupied by the fluid.

Properties include:

In time-dependent calculations, it is sometimes necessary to calculate the trajectory of material points, the workspace is not a Lagrangian code (that is, it does not use a description and formulation following the particles), and nodes do not correspond, in general, to material particles. Therefore, a postprocessor is provided to track these material points. Typically this is useful in blow molding simulations, when remeshing is not of the Lagrangian type, although it can be very useful in many other situations also.

This is available if the domain is not a shell and if there is at least one inlet fluid boundary condition​. In addition, you should specify the fluid boundaries where it will be initialized and specify the initial value.

Properties include:

 

4.9.4.6.1. Calculation for Tracking Material Points

A material particle’s initial position is tracked according to

(4–10)

where is the initial position of the material particle (that is, the original position before deformation occurs). When the material points postprocessor is used, the workspace will keep track of the initial position of each material point, as well as the final position of that same material point. This allows you, for example, to determine the source on the parison of a flaw that occurs at a particular location on the final product. This post-processor is valid for transient cases defined on a material volume, i.e. without entry and exit.

(4–11)

The mixing index is defined as

where is the equivalent shear rate defined as

(4–12)

In a purely rotational flow, the mixing index is zero. The mixing index is not defined everywhere in the flow problem; singular values arise in regions where the denominator is zero (for example, along the axis of symmetry of a Poiseuille flow).

and is the magnitude of the vorticity vector. For a shear flow, the mixing index is equal to 0.5, whereas its value is 1 in a purely elongational flow.

The mixing index will appear as a scalar during postprocessing.

Properties include:

The workspace can calculate the vorticity vector for the flow. Vorticity is a measure of the rotation of a fluid element as it moves in the flow field, and is defined as the curl of the velocity vector:

(4–13)

This quantity is a vector representation of twice the antisymmetric part of the velocity gradient tensor given by

(4–14)

For 3D flows, the vorticity vector is given in component form by

(4–15)

For 2D planar and axisymmetric flows, the vorticity has one non-zero component only, and it is displayed as a signed scalar quantity. For 2D 1/2 flows, the magnitude of the vorticity vector is displayed, while it will appear as a vector while postprocessing for 3D flows.

Properties include:

The workspace can calculate the rate-of-deformation tensor on the part of the domain where the velocity field has been computed. Three components of the rate-of-deformation tensor will be calculated for 2D planar cases, four components for 2D axisymmetric cases, and six components for all other cases.

Furthermore, the components are based on the selected reference frame (Cartesian for 2D planar and 3D cases, cylindrical for axisymmetric cases). In many cases, the calculation of the local shear rate (see Shear Rate) is preferred if only a (generalized) scalar kinematics quantity is needed.

Properties include:

The workspace can calculate the resulting forces applied from the fluid to the several boundaries. The result is evaluated independently for each boundary and is printed in the transcript. Enabling this option allows you to know the corresponding force needed for satisfying the imposed flow boundary condition.

Properties include:

The workflow automatically integrates the total volumetric flow rate along all boundary sets. Results are displayed as numerical values in the transcript (search for the word Flow rates to find them).

Properties include:

For thermal cases, the workspace can calculate the resulting heat fluxes which leaves the domain through the several boundaries. The result is evaluated independently for each boundary and is printed in the transcript. Enabling this option allows you to know the corresponding heat flux needed for satisfying the imposed temperature boundary condition.

Properties include:

Die balancing is a major challenge for the die designer. To help address this challenge, the workspace can compute a measure of the die balancing based on the deviation of the normal velocity with respect to the average velocity along the die exit:

(4–16)

where is the velocity, is the flow rate across the boundary set, is the surface of the boundary set, and is the outward normal along the boundary set.

A perfectly balanced die with a uniform velocity at the exit leads to a measure of the die balancing equal to zero. This measure is not absolute; you have to compare the die balancing measure for different die geometries to determine which is the best one (that is, the one with the smallest value for the die balancing measure). Results are displayed as numerical values in the workspace transcript (search for the words Flow balance to find them).

Properties include:

This postprocessor is available for boundaries of fluid zones in thermal simulations. Only boundaries with non-zero normal velocity should be considered. Indeed, along walls or plane of symmetries, the convected heat should be zero.

The convected heat postprocessor computes the integral along selected boundaries of , where is the temperature.

The workspace can calculate the residence time distribution in the part of the domain where a velocity field has been calculated. The residence time distribution can be calculated in 2D and 3D calculations in steady-state and time-dependent modes. This postprocessor differs from individual time integration along a trajectory, where the result is obtained for a single material point only. With this postprocessor, a residence time distribution value is obtained over the whole domain.

 

4.9.4.15.2. Calculation of Residence Time

Consider a simple steady-state free surface flow, where the flow enters from the upper left part of the domain. Assuming that the residence time distribution is zero in the entry section, the workspace will calculate the residence time distribution in the domain. An example of contour lines of the residence time distribution is shown in Figure 4.106: Contour: Residence Time Distribution for a Steady-State Free Surface Problem.

Figure 4.106: Contour: Residence Time Distribution for a Steady-State Free Surface Problem

The workspace computes the residence time distribution using the equation

(4–17)

where at time , and the boundary conditions along the entry sections are taken into account. is the residence time, and is the material derivative of the residence time.

Equation 4–17 states that the residence time increases as the absolute time for particles along their path increases. It is a hyperbolic equation, and it requires boundary conditions (as well as initial conditions for time-dependent problems). The value of the residence time must be set along all entry sections.

Usually you will set a value of zero. On all sections on which an inflow boundary condition has been applied for the momentum equation, the residence time is set to zero by default. You can add boundary conditions on entry sections where a different type of condition has been selected.

For time-dependent calculations, the workspace  imposes as an initial condition. In this case, the time-dependent problem is well-posed provided that has been imposed on all entry sections. For steady-state problems, Equation 4–17 does not define a well-posed problem in recirculating zones (vortices) and along walls where .

This is not usually important, since the residence time distribution is meaningless in these regions, and you can easily exclude these corresponding contour lines from the display in your graphical postprocessing program.

Another possibility for calculating the residence time distribution in the presence of steady-state vortices is to define a time-dependent problem that uses a steady-state velocity field that has already been calculated.

For flow problems, you can track particles by assigning a value of a material property (a conventional scalar field named for "color") in the flow domain and integrating the pure advection of this property in the flow domain:

(4–18)

Equation 4–18 is subject to inlet boundary conditions that can be defined separately on each inlet section. This postprocessor is typically used to calculate the transport of the property in the flow. Each separate entry has a different color represented by a separate value of the property along the inlet. The flow transports the property and you can locate the color at each position in the flow domain.

The continuous interpolation used in the numerical scheme will produce some interpolation error, so intermediate values will also be displayed in the flow domain. However, provided you select distinct values of the property along inlets (such as 1 and 10, for example), you can easily identify regions of the flow during postprocessing.

Properties include:

Evaluation of the extension components is available for blow molding and thermoforming simulations. This is available if the domain is a shell. Two kinds of extensions can be evaluated:

For blow molding and thermoforming processes in shell models, there are times when self-contacts such as folds or knit-lines can occur in the blown part. In such cases, the self-contact postprocessor can simply detect self-contact of the parison.

In 2D as well as in 3D simulations of blow molding and pressing, you can compute the thickness of the final object (as well as during shaping). In industrial processing, the thickness has to be understood as the distance between two arbitrary surfaces; it is therefore subjected to an appropriate definition. Also, from the point of view of modeling, it would require the identification of preferably distinct topological entities; however this cannot always be achieved. A technique has been implemented, which matches a reasonable industrial definition as much as possible: at a given point, it basically consists of evaluating the distance with respect to the closest opposite surface. A topological object has to be constructed for the thickness evaluation, and a few parameters for geometric tolerances have to be given. In 3D, the thickness is evaluated on the selected boundary; planes of symmetry can be discarded from the domain of evaluation. Note that in 2D, a similar scenario applies; however, since the display of a quantity along a line is not easy, the evaluation is expanded onto the domain via a Laplace equation.

Typically, the thickness at the end of the process is of interest. Hence, it is not necessary to perform a thickness evaluation at each time step. Also, since the thickness at a point is evaluated as a distance measured along a line perpendicular to the surface at this point, it is preferable to bound its value.

The Fluent Materials Processing workspace automatically creates mesh quality fields when the mesh deforms during the calculation. These fields allow you to analyze the mesh and identify distorted elements.

The mesh quality fields are:

The best way to evaluate mesh quality in the Fluent Materials Processing workspace is to create isosurfaces of the mesh quality fields to locate distorted elements. The minimum and maximum values displayed in the iso-surface property panel also allow you to gauge mesh distortion.

 

4.9.4.20.1. Element Distortion Check

An interior angle is defined as the angle between two adjacent edges at a vertex. For example, the interior angles of a square are of 90 degrees, while the angles of an equilateral triangle are of 60 degrees. By default, the minimum and maximum angles are set to 5 and 170 degrees, respectively.

The aspect ratio of an element is defined as the ratio of the lengths of the longest edge to that of the shortest edge. By default, a maximum aspect ratio of 10 is set.

The bend is evaluated based on the cross product between unit normal directions and defined at two opposite vertices of a quadrilateral defined in the plane or in the space. More precisely, it is defined as . Obviously for a triangular face, the bend is always zero and consequently a tetrahedron is never bent. A regular quadrilateral face has also a zero bend; however, the bend of a quadrilateral in the space may equal 1 or 2 when an edge is rotated by 90 or 180 degrees out of the plane of the quadrilateral, respectively. The element displayed in Figure 4.107: Bent Quadrilateral and Unit Normal Directions at Vertices is obtained by lifting one vertex of a square element in the upward direction over a distance that corresponds to 70% of the side length; it exhibits a bend of 0.33. If that same vertex was placed above the diagonally opposite one, at a distance corresponding to the side length, the bend would have been of 1.58. By default, a maximum bend of 0.8 is set.

Figure 4.107: Bent Quadrilateral and Unit Normal Directions at Vertices

For evaluating the skewness of an element, the transformation that relates the element considered in the -space and a parent element in the -space is invoked. Let J denote the Jacobian of the transformation. The skewness can be evaluated as follows:

(4–19)

If the transformation is regular, or if J does not vanish, the previous equation is equivalent to

(4–20)

where and are the volume of the element in the -space and of the corresponding parent element in the -space, respectively. The skewness of a triangle and of a tetrahedron always vanishes.

For illustrating the skewness of a deformed hexahedron, consider three deformation scenarios applied to the initially cubic element displayed in Figure 4.108: Three Deformation Scenarios. Note that these three deformation scenarios are applied to an initially cubic element for evaluating the skewness.

Figure 4.108: Three Deformation Scenarios

In the first scenario, the segment AB is moved along the x-direction; in the second scenario, the segment AB is moved along the 0xy-bisector; in the third scenario, vertex B moves along the central line of the 0xyz-trihedron. The first two scenarios also apply to a square. Figure 4.109: Skewness Values vs. Element Shape displays the skewness values as a function of the element shape dictated by the segment AB according to the selected scenario of Figure 4.108: Three Deformation Scenarios.

Figure 4.109: Skewness Values vs. Element Shape

Use the Methods task to determine specific solution techniques that can be applied to your simulation.

Figure 4.110: Properties of Methods

The choice of numerical methods can influence the simulation's rate of convergence as well as the solution's accuracy and stability, however, the default settings applied in the workspace are adequate most of the time.

See Methods Properties for details.

Use the Calculation Activities task to determine what, if any, activities will be performed during the calculation of the solution.

Figure 4.111: Properties of Calculation Activities

In most cases, the default settings are adequate. However, information on the AMF and AMF + secant solver types are outlined in AMF Direct Solver and AMF Direct Solver + Secant.

See Calculation Activities Properties for details.

 

4.9.4.22.3. MUMPS Solver

The Fluent Materials Processing workspace provides the MUMPS (Multifrontal Massively Parallel Solver) for shared memory.

You can specify the MUMPS solver within the Calculation Activities properties panel by selecting MUMPS direct solver from the Solver Type drop-down list.

MUMPS is a package for solving systems of linear equations of the form Ax=b, where A is a square sparse matrix. As the AMF solver, MUMPS implements a direct method based on a multifrontal approach which performs a Gaussian factorization

(4–21)

where is a lower triangular matrix and an upper triangular matrix.

Similarly to the AMF solver, the system is solved in three main steps:

1. Analysis

   During the analysis, Mumps creates the elimination tree (variables elimination order) and estimates the number of operations and the memory necessary for the factorization and the solution.

2. Factorization

   The factorization computes the and matrices and stores them in double precision. They can be stored in core memory or on disk.

3. Solution

   The solution is obtained through a forward elimination step:

   (4–22)

   followed by a backward elimination step

   (4–23)

 

4.9.4.22.3.1. Recommendations for the MUMPS Solver

In terms of continuation/transient steps and iterations, the AMF and MUMPS solvers behave similarly. Extensive testing on approximately one thousand cases has shown that any convergence issues only occurred in about 1% of cases. For most cases, the MUMPS solver is recommended.

If the CPU time is dominated by the system resolution (large 3D extrusion problems or large 3D problems with contact), MUMPS can reduce the CPU time by about 25 - 30% with peak value up to 50%. The additional memory requirement can reach 200 - 300%. If Out-Of-Core storage is invoked, this additional memory requirement is only 10 to 20% with a CPU penalty of a few percent on fast disks.

If the CPU time is not dominated by the solver (2D problems, problems with contact evaluation, problems with mesh refinement) the benefit of MUMPS in term of CPU is around 10% with peak value up to 20%. Usually, for these kind of problems, the memory is not an issue.

To activate the Out-Of-Core (OOC) storage of the factor's matrix, that is, storage on disk, you can enter the following command for Solver Keywords within the Launch Options group of the Calculation Activities panel

MUMPS_AUTO_SWITCH_OOC_MEMORY NNN

where NNN is the in-core (IC) memory value (in MB) to be used before switching to OOC memory for the MUMPS solver. For example, entering MUMPS_AUTO_SWITCH_OOC_MEMORY 500 specifies the MUMPS solver to use 500 MB of in-core memory before switching to out-of-core memory. If the estimated memory evaluated by MUMPS is greater than the value of NNN, then the Out-Of-Core storage will be used by MUMPS.