The inputs directly related to the free surface or moving interface are provided in this section. You will need to set up the rest of the problem (material properties, other boundary conditions, etc.) as usual. See also Defining the Direction of Motion – Constraint on Global Displacement for guidelines about free-surface and moving-interface problems.
Note that you have access to Polyflow project templates, which are Workbench project files that you can modify in order to quickly and easily set up your own problem. These templates include extrusion problems. See Polyflow Project Templates in the Polyflow in Workbench User's Guide for further details.
Specify the boundary that represents the free surface or moving interface.
For a free surface, follow the steps below:
In the Flow boundary conditions menu, select the boundary set that represents the free surface and click Modify.
Flow boundary conditions
Select Free surface as the boundary type.
Free surface
For a moving interface, follow the steps below:
In the Flow boundary conditions menu, select the boundary set that represents the moving interface and click Modify.
Flow boundary conditions
Select Interface as the boundary type.
Interface
Enable the motion of the interface.
Switch to moving interface
If you want to include the slip effect between the two fluids along the interface (as described in Slipping Between Two Layers in Coextrusion), turn on the fluid-fluid slip effect.
Specify fluid/fluid slip effect
(You will need to click Yes to confirm that you want to proceed.)
Select the Navier form of the slip law (Equation 15–12).
F(v)= Generalized Navier’s
law
Specify the friction coefficient for the Navier slip law (
in Equation 15–12).
Modify k
Click Upper level menu twice to return to the Interface menu.
Important: Note that there is also an Advanced options menu, where you can modify the value of
, a parameter that influences the
penalty formulation for the slip effect. Changing the
value of 
from the default value is not
recommended, except on the advice of your support
engineer.Move to the menu where you can specify additional parameters for the moving interface (described in the next few steps).
Specify moving interface parameters
If you want to model surface tension on the free surface or moving interface, specify a nonzero value for the surface tension coefficient (
in Equation 15–17).
Surface tension
Specify the conditions to be imposed at the boundary of the free surface or moving interface.
Boundary conditions on the moving surface
The inputs will be slightly different, depending on whether surface tension is being modeled.
If you are not modeling surface tension (that is, if you did not specify a nonzero surface tension coefficient in step 2, above), the inputs will be as follows:
Select the adjacent boundary or subdomain on which the position of the free surface is to be imposed.
Click Modify.
Select Position imposed.
If you are modeling surface tension (that is, if you specified a nonzero surface tension coefficient in step 2, above), the inputs will be as follows:
Select the adjacent boundary or subdomain (or the first one if there are multiple choices).
Click Modify.
Indicate whether you want to impose the position or the angle at this boundary:
To impose an angle at the boundary (for modeling the traction force), select Angle imposed, and enter the value of
in Equation 15–20, when prompted. To impose the position of the free surface at the boundary, select Position imposed.
If there are multiple adjacent boundaries or subdomains, repeat the steps above until conditions for all of them have been set.
Important: Specifying a zero-force boundary condition (for example, an outflow) for a 2D axisymmetric problem will violate the requirement that the normal force cannot be equal to zero in an axisymmetric geometry when the surface tension coefficient
is nonzero (see Surface Tension). For both generalized Newtonian and
viscoelastic flows, you can alleviate this problem by imposing a
constant exit velocity instead of using an outflow
boundary.
(free surfaces only) Specify the normal force on the free surface (
in Equation 15–1).
Normal force
By default, directors for the free surface (
) are normal to the initial mesh, and are calculated before
each step of a time-dependent or evolution problem. If you prefer, you can
prescribe the components of the director yourself and/or have the directors
calculated just once for a time-dependent or evolution problem. See Defining the Direction of Motion for
guidelines and further explanation.
Direction of motion
Select which condition you want to impose (along the whole surface, or on the intersection with an adjacent boundary).
Click Modify.
Modify the constraint on the appropriate component(s) of the direction vector by selecting the corresponding menu item and entering the desired value when prompted.
When you are satisfied, click Accept the current condition. If you change your mind and want to return to the default (no condition imposed), select Deletion of the current condition.
(evolution and time-dependent problems only) By default, Ansys Polyflow will compute the director
before each evolution or time step of the task
calculation (D calculated before each step). If
you want the director 
to be computed just once at the beginning of the
task calculation, click the button next to D calculated
before each step. The condition will now be
D calculated once for the whole task.
When you are satisfied with all the settings for the direction of motion, click Upper level menu at the top of the Imposing the direction of surface motion panel.
Specify fluid-fluid contact parameters.
Fluid/fluid contact
Specify the source free surface and the target free surface. Polyflow automatically defines the reverse relationship (for example, both boundary 1 → boundary 2 and boundary 2 → boundary 1 are defined) during file generation.
You can modify the numerical parameters used to define the constraints on the velocity (see Fluid-Fluid Contact): the element dilatation and the minimum coupling coefficient. A "reset" item allows you to return to the default settings.
You may want to modify the parameters used to define the mapping problem between the two surfaces in contact. Select Options for mapping to open the Fluid/fluid contact: options for mapping menu. The Fluid/fluid contact: options for mapping menu allows you to modify the numerical parameters used to define the mapping (see Mapping for Fluid-Fluid Contact) including threshold contact value, element dilatation, scaling factor, fraction of displacement, upper and lower bounds of mapping, allow or disallow correction in the x/y/z direction.
Specify contact with guiding device(s).
Contact with guiding device(s)
This item is available only if guiding devices have already been defined (see Guiding Devices)
When a guiding device is available, it can be invoked in the simulation. For this, you must select the required guiding device, and specify a few data for the calculation. Here, the most relevant information is the slipping coefficient that exists between the extrudate and the guiding device. By default, a zero value is assigned, and corresponds to a full slipping. The contact depth is a geometric transition distance along which friction with the guiding device belt develops when contact occurs; it may be changed if appropriate. Eventually a reasonable default value is selected for the penalty coefficient: it is calibrated to obtain a good contact accuracy between the guiding device and an extrudate profile whose typical height is of the order of 0.01 m. Selecting a larger value for the coefficient will increase the accuracy of the contact as well as the stiffness of the model.
Note that more than one guiding device can be used. In particular, this is interesting for defining a conveyor system involving multiple rollers. You should anyway make sure that your combination produces the required effect on the flow.
By default, no upwinding is used for the calculation of the kinematic equation. If you want to include it, select the Upwinding in the kinematic equation option.
Upwinding in the kinematic condition
Invoking upwinding is generally recommended for steady state or evolution calculations, also for 2D flows, as it may have a positive impact on the stability of the solver. This is especially true when wiggles (oscillations) appear in the shape of the free surface, as can be typically observed when a take-up force or velocity is imposed at the exit of the calculation domain. Note that upwinding is automatically applied when you choose the line kinematic condition, described in Discontinuity of the Normal Direction and Guidelines for 3D Extrusion Problems.
Upwinding is not recommended for use with surface tension.
By default, no drag is applied on the free surface. If you want to include it, select the Drag option
Drag
In some fiber spinning cases, it is not unusual that drag force originating from the air surrounding the free boundary of the fiber becomes significant with respect to the take-up force. When this is the case, the option should be selected, and numerical values for the various parameters should be entered. Also it is important to explicitly activate the selected feature by clicking
Enable drag
Failing to do so will simply not activate the calculation of the drag, regardless of the numerical values for the various parameters.
Note that this option is available for 2D axisymmetric calculations only.
When running a so-called inverse extrusion case, it is important to specify the shape of the extrudate. For this, select the option Outlet (Inv. Prediction):
Outlet (Inv. Prediction)
See Inverse Extrusion and Die Design for further details on inverse prediction and die design.
Define the remeshing procedure for the sub-task (after you finish setting all boundary conditions and return to the sub-task menu one level above the Flow boundary conditions menu).
Global remeshing
See Remeshing for details. For inverse extrusion problems, see Inverse Extrusion and Die Design for information about additional inputs in the Global remeshing menu.
Modify the interpolation scheme(s) for the sub-task, if necessary.
Interpolation
See Controlling the Interpolation for details.
If necessary, impose a constraint on the free jet displacement (in the task menu).
Constraint on free jet displacement
See Constraint on Global Displacement for details.
For 3D extrusion problems, specify the use of the line kinematic condition for handling discontinuities in the normal direction (in the task menu).
Numerical parameters
See Guidelines for 3D Extrusion Problems for details. Note that the line kinematic condition can be used only if you are using the Optimesh or streamwise remeshing method for every local remeshing region in the task.
To mitigate possible convergence difficulties in an extrusion problem, you should apply evolution to the moving boundaries. For more information about these techniques, see Convergence Strategies.