Setting Up Viscous Fluid Flow

The workflows for setting up viscous flow simulations of different constitutive models are similar. To model a non-Newtonian fluid with a high viscosity or a variable viscosity depending on shear-rate without any elastic effects, choose the Generalized Newtonian Model. If the fluid exhibits time-dependent, shear thinning behavior, choose the Thixotropic Model. If the fluid exhibits normal stress or memory effects, work with the Viscoelastic Model. High shear rates in the flow can lead to a temperature increase—viscous heating. To account for this effect, Simcenter STAR-CCM+ provides the Viscous Energy Model.

The Finite Element discretization imposes certain requirements on the meshes that are suitable for using with the viscous flow model. Generate either tetrahedral meshes, extruded meshes, or directed meshes in combination with prism layers. You can also use imported hexahedral meshes. The viscous flow model is not compatible with polyhedral or trimmed meshes.

If you are replacing an existing mesh with a new mesh, Simcenter STAR-CCM+ automatically interpolates any vertex data, available on the existing mesh, to the new mesh vertices. For more information on the Replace Mesh operation, see Replacing a Mesh Region.

To set up generalized Newtonian or viscoelastic fluid flow:
  1. Create a volume mesh that is suitable for the Finite Element discretization. See Mesh Requirements and Guidelines.
    If you are modeling co-extrusion, and hence have one fluid region in contact with another, use a conformal mesh at the interface between the fluid regions.
  2. Create a physics continuum for each non-Newtonian fluid material in the simulation.
  3. For the physics continuum of each non-Newtonian fluid, under Continua > [Physics Continuum] > Models, select the following models in order:
    Group Box Model
    Time Steady or Unsteady

    To model cases with Weissenberg number > 1 and using the eXtended Pom-Pom model, select Unsteady.

    Material Liquid
    Flow Viscous Flow

    Laminar (selected automatically)

    Constant Density (selected automatically)

    Rheology Select one of the following:
    Optional Models Select one of the following:
    • To model temperature effects such as viscous heating, select Viscous Energy.
    • To model extrusion or any free surface flow of a non-Newtonian fluid, select Free Surface.
    • To model partial filling of a domain, such as for injection molding, select Partial Fill. Partial filling is only available for unsteady simulations.
    • To model the surface tension on the fluid for free surface flow or for partial filling, use the Surface Tension model.
    • To model the slippage of the fluid at boundaries, use the Partial Slip models.
    • To model the flow properties of short fibers suspended in a viscous fluid, use the Short Fiber Orientation model.
    • To simulate a two-way coupled rheology of a suspension of short fibers in a viscous fluid, use the Fiber-Flow Interaction model. This model is incompatible with the Viscoelastic model.
    • To model passive scalar components, use the Passive Scalar model.
    • To curve-fit experimental rheological data for specifying numerical rheological model parameters, select Material Calibration.
    • To set the time-step automatically based on CFL number, in unsteady simulations, select Adaptive Time-Step. See Adaptive Time-Step Models.
    • To model the effects of curing on the rheological properties of the fluid that you simulate, select Chemorheology. (Compatible only with the Generalized Newtonian rheology model.)
  4. These liquids are incompressible. Depending on the type of fluid you model to specify rheological model parameters, do one of the following:
    Fluid Model Type Steps
    Generalized Newtonian Edit the Models > Liquid > [material] > Material Properties node and set the Dynamic Viscosity Properties.
    Viscoelastic
    1. Select the Models > Viscoelastic node and set the Number of Modes. You can specify 1–8 modes. The behavior of the viscoelastic model is the sum of the behaviors of the modes. You can select a different viscoelastic material model for each mode. For more information, see Viscoelastic Properties.
    2. For fast flows of highly entangled polymer melt, activate the Square-root conformal property of the Viscoelastic model. This setting switches the viscous flow solver to the square-root conformal formulation, adapted to the high Weissenberg numbers found in such simulations. See the Square-root conformal property.
    3. Edit the Models > Liquid > [material] > Material Properties node and set
    Thixotropic
    1. Define the structure variable λ:
      1. Select Models > Liquid > [material] > Material Properties > Structure Variableand set Method to either:
        • Generic Kinetic if the fluid returns to the original state when flow ceases.
        • Irreversible Structural Breakdown if the fluid structure remains partially or completely in the new state after flow ceases.
      2. Select the corresponding sub-node and specify the model parameters.
      See Structure Variable.
    2. To account for time-dependent effects on viscosity, define the thixotropic factor:
      1. Select Models > Liquid > [material] > Material Properties > Thixotropic Factor and set Method to Power Law.
      2. Select the Thixotropic Factor > Power Law node and specify the power law model exponent.
      See Thixotropic Factor.

    Alternatively, to obtain the rheological model parameters from experimental rheological data through curve fitting, use the Material Calibration model and follow the additional steps in Calibrating Non-Newtonian Model Parameters. If you are simulating curing, you can also use the Material Calibration model to fit the chemorheological material properties.

  5. To simulate temperature-dependence of the dynamic viscosity, select Liquid > [material] > Material Properties > Horizontal Temperature Shift Factor and Vertical Temperature Shift Factor, then set the temperature shift factors for them or accept the defaults. For the particular case of aT=bT=1, the viscosity of the fluid is independent of the temperature. See Using the Temperature Shift Factors
  6. To simulate free surface flow, perform the additional steps that are described in Setting Up Extrusion and Free Surface Flow.
  7. Set up boundary conditions.
    If there is more than one fluid, separate them with an immiscible wall within the die.
    Because viscous flow simulations use finite-element discretization, mesh vertices sometimes lie on two boundaries at once. If the boundaries specify different boundary condition values, Simcenter STAR-CCM+ uses the average of the two. This averaging is the default procedure. If you want to promote one boundary condition over another, apply a slip condition to the boundary with a less dominant contribution and set its slip coefficient to a value on the order of 10^6 to 10^8, depending on the polymer viscosity.
    If you have a slip wall boundary condition, any pressure outlet boundary must be perpendicular to the slip wall. If the two cannot be perpendicular, use a different boundary condition, such as free-stream outlet.
  8. Set solver parameters.
    For time-dependent cases where the viscous fluid flows in to fill a region, you are advised to have a Courant number between 0.1 and 1.

    For strongly non-linear cases with a Weissenberg number > 1, raise the Relaxation over # iterations property of the Viscous Flow Solver above the default value of 10.

    For fast solutions with the Implicit Unsteady model, select the Solvers > Implicit Unsteady node and set Temporal Discretization to 2nd-order. Second-order discretization gives faster unsteady solutions by using larger time-steps and is more accurate. However, it is harder to stabilize and requires more attention to mesh quality. Start with lower-order schemes and switch to high-accuracy schemes, if necessary, when all strong initial transients have been eliminated. Second-order discretization is not available when the Multiphase or Partial Fill models are selected.

  9. To mimic the effects of constant motions in a region such as a rotor without actually moving mesh vertices, apply moving reference frames to the regions.
    See User-Defined Rotating and Translating Reference Frames and Reference Frames. Viscous Flow does not support reference frames for DFBI motion or mesh motion.
  10. Run the simulation and analyze results.
    When using field functions in a scene or report, make sure that you use Smooth Values , so that you visualize the nodal values.
  11. If you want to analyze the hydrodynamic forces that the fluid exerts on wall boundaries, you can: