Create a Fluid Flow (Polyflow Classic) analysis system by drag and drop in Workbench.

Save the Ansys Workbench project using File → Save, entering 3D-extrusion as the name of the project.

Import the mesh file (ext3d.msh).

Double-click the Setup cell to start Polydata.

When Polydata starts, the Create a new task menu item is highlighted, and the geometry for the problem is displayed in the Graphics Display window.

Create a task for the model.

  Create a new task

1. Retain the following (default) options:

   • F.E.M. task

   • Steady-state problem(s)

   This problem is a 3D simulation of the extrusion process, that is, a three-dimensional geometry is assumed for the die. A Cartesian (x,y,z) reference frame is used for the 3D calculations. A steady-state condition is assumed for the problem.

2. Click Accept the current setup.

   The Create a sub-task menu item is highlighted.

Create a sub-task for the isothermal flow.

  Create a sub-task

1. Select Generalized Newtonian isothermal flow problem.

   A dialog box appears asking for the title of the problem.

   

2. Enter 3D die swell as the New value and click OK.

   The Domain of the sub-task menu item is highlighted.

Define the domain where the sub-task applies.

Since this problem involves a free surface, the domain is divided into two subdomains; one for the region near the free surface (subdomain 2) and the other for the rest of the domain (subdomain 1). In this problem, the sub-task applies to both subdomains, which is the default condition.

  Domain of the sub-task

Accept the default selection of both subdomains (SUBDOMAIN_1 and SUBDOMAIN_2) by clicking Upper level menu.

The Material data menu item is highlighted.

Click Shear-rate dependence of viscosity.

Click Cross law.

The Cross law exhibits shear-thinning (the decrease in viscosity as the shear rate increases) that is a characteristic of many polymers. The viscosity in this tutorial is given by the Cross law:

(4–1)

where:

= zero shear-rate viscosity = 85000 poise

= natural time = 0.2 s

= Cross law index = 0.3

= shear rate

Specify the value , referred to as “fac” in the graphical user interface (compare the equation at the top of the Cross law menu to Equation 4–1).

  Modify fac

Enter 85000 [units: poise] as the New value and click OK.

Specify the value for , referred to as “tnat” in the graphical user interface.

  Modify tnat

Enter 0.2 [units: s] as the New value and click OK.

Specify the value for , referred to as “expom” in the graphical user interface.

  Modify expom

Enter 0.3 as the New value and click OK.

Select Upper level menu three times to return to the 3D die swell menu.

The Flow boundary conditions menu item is highlighted.

Set the conditions at the flow inlet (BOUNDARY_1).

1. Select Zero wall velocity (vn=vs=0) along BOUNDARY_1 and click Modify.

2. Click Inflow.

3. Retain the default settings, Automatic and Volumetric flow rate.

4. Click Modify volumetric flow rate.

   

   Enter 10 [units: cm³/s] as the New Value and click OK.

   When the Automatic option is selected, Polydata automatically chooses the most appropriate method to compute the inflow condition.

5. Click Upper level menu.

Retain the default condition Zero wall velocity (vn=vs=0) along BOUNDARY_2 at the wall of SUBDOMAIN_1 (BOUNDARY_2).

At a solid-liquid interface, the velocity of the liquid is that of the solid surface. Hence the fluid is assumed to stick to the wall. This is known as the no-slip condition because the liquid is assumed to adhere to the wall, and hence, has no velocity relative to the wall.

By default, Polydata imposes = = 0 along all boundaries. No action is required to accept the default condition.

Set the conditions at the first symmetry plane (BOUNDARY_3).

In 2D axisymmetric problems, Polydata automatically identifies the axis of symmetry, but for 3D flows, you must manually identify a plane of symmetry.

The normal velocity () and the tangential force () are set to zero on a symmetry plane. A particle cannot cross the plane ( = 0) due to the symmetry, so the particles flow at the same velocity on both sides of the symmetry plane, leading to a zero tangential force.

1. Select Zero wall velocity (vn=vs=0) along BOUNDARY_3 and click Modify.

2. Click Plane of symmetry (fs=0, vn=0).

Set the conditions at the second symmetry plane (BOUNDARY_4).

1. Select Zero wall velocity (vn=vs=0) along BOUNDARY_4 and click Modify.

2. Click Plane of symmetry (fs=0, vn=0).

Set the conditions at the free surface (BOUNDARY_5).

In a steady-state problem, the velocity field must be tangential to a free surface, since no fluid particles go out of the domain through the free surface. This constraint is called the kinematic condition, . This equation requires an initial condition, that is, the starting line of the free surface. In the current problem, the starting line of the free surface is the intersection of boundary 2 and boundary 5 (see Figure 4.2: Boundary Sets for the Problem).

1. Select Zero wall velocity (vn=vs=0) along BOUNDARY_5 and click Modify.

2. Click Free surface.

3. Click Boundary conditions on the moving surface.

4. Select No condition along BOUNDARY_2 and click Modify.

5. Select Position imposed.

6. Click Upper level menu.

7. Click Upper level menu to return to the Kinematic condition menu.

8. Click Upper level menu to return to the Flow boundary conditions panel.

Set the conditions at the flow outlet (BOUNDARY_6).

It is assumed that a uniform velocity profile is reached at the exit. The melt is not subjected to any externally applied stress at the exit, so the condition of zero normal and tangential forces is selected.

1. Select Zero wall velocity (vn=vs=0) along BOUNDARY_6 and click Modify.

2. Click Normal and tangential forces imposed (fn, fs).

3. Accept the default value of 0 for the normal force, , by clicking Upper level menu.

4. Accept the default value of 0 for the tangential force, , by clicking Upper level menu.

5. Click Upper level menu at the top of the Flow boundary conditions panel.

Specify the region where the remeshing is to be performed (SUBDOMAIN_2).

In general, only one local remeshing is required for direct extrusion simulations. It becomes necessary to define multiple local remeshings for inverse extrusion simulations. A single local remeshing is sufficient for this case.

  1–st local remeshing

1. Select SUBDOMAIN_1 and click Remove.

   SUBDOMAIN_1 is moved from the top list to the bottom list, indicating that only SUBDOMAIN_2 will be remeshed.

   

2. Click Upper level menu.

Define the parameters for the remeshing method.

The purpose of the remeshing technique is to relocate internal nodes according to the displacement of boundary nodes due to the motion of the free surface, since a part of the mesh is deformed. For 3D extrusion problems where large deformations of the extrudate are expected, the optimesh remeshing technique is recommended

The optimesh remeshing technique requires the direction of extrusion to be parallel to the , , or axis, and all slices into which the remeshing domain is cut must be perpendicular to the extrusion axis.

The domain to be remeshed is cut into a series of 2D slices (planes) in a direction perpendicular to the direction of extrusion, and each plane is remeshed independently. For this process, Polyflow Classic requires the selection of the initial plane and the final plane. In this problem, the initial plane is the intersection of subdomain 2 with subdomain 1, and the final plane is the intersection of subdomain 2 with the flow exit (boundary 6).

  Optimesh-3D (extrusion only)

1. Specify the initial plane for the optimesh remeshing technique, by selecting SUBDOMAIN_1 and clicking Modify.

   

   1. Select Part of inlet section.

   2. Select Upper level menu.

2. Specify the final plane for the optimesh remeshing technique, by selecting BOUNDARY_6 and clicking Modify.

   

   1. Select Part of outlet section.

   2. Select Upper level menu.

3. Click Upper level menu.

   Polydata asks if you want to change from the surface kinematic condition to the line kinematic condition.

   

4. Click Yes to use the line kinematic condition.

   The line kinematic condition is recommended for extrusion problems, and should be used in combination with the optimesh remeshing technique.

5. Click Upper level menu three times.

   The top-level Polydata menu is displayed.

Specify the system of units for the simulation.

1. Click Modify system of units.

2. Select Set to metric_cm/g/s/A+Celsius

3. Click Upper level menu twice.

   

Click Accept current setup in the Convergence strategies menu.

Click Accept in the Field Management menu.

This confirms that the default Current field(s) are correct.

Click Continue.

This accepts the default names for graphical output files (cfx.res) that are to be saved for postprocessing, and for the Polyflow Classic format results file (res).

Run Polyflow Classic by right-clicking the Solution cell of the simulation and selecting Update.

This executes Polyflow Classic using the data file as standard input, and writes information about the problem description, calculations, and convergence to a listing file (polyflow.lst).

Check for convergence in the listing file.

1. Right-click the Solution cell and select Listing Viewer....

   Workbench opens the View listing file dialog box, which displays the listing file.

2. It is a common practice to confirm that the solution proceeded as expected by looking for the following printed at the bottom of the listing file:

   The computation succeeded.

Double-click the Results cell in the Workbench analysis and read the results files saved by Polyflow Classic.

CFD-Post reads the solution fields that were saved to the results file.

Display the velocity distribution on the boundaries.

1. Click the Insert menu and select Contour or click the   button.

2. Click OK to accept the default name (Contour 1) and display the details view below the Outline tab.

3. In the Outline tree tab, under User Locations and Plots, deselect Wireframe.

4. Perform the following steps in the details view of Contour 1:

   1. In the Geometry tab, click the   button next to Locations.

      

   2. Select all topological entities under SUBDOMAIN_1 and SUBDOMAIN_2 in the Location Selector dialog box (use Shift) and click OK.

   3. Select VELOCITIES from the Variable drop-down list (or by clicking  ).

   4. In the Render tab, deselect Show Contour Lines.

   5. Click Apply.

In Figure 4.3: Contours of Velocity Magnitude, the velocity is zero along the die wall (as expected) and there is a fully developed profile at the inlet of the die. At the die outlet, the velocity profile changes to become constant throughout the extrudate cross-section. The transition between these two states can be seen in the beginning section of the extrudate.

Figure 4.3: Contours of Velocity Magnitude

Display contours of velocity in cross-sections.

1. Deselect Contour 1 in the Outline tree tab under User Locations and Plots.

   

2. Create the cross-section planes, at Z = 0, 0.08, 0.15, 0.45 m.

   1. Select Plane from the Location drop-down menu ( ).

   2. Click OK to accept the default name (Plane 1) and display the details view below the Outline tab.

      

   3. In the Geometry tab of the details view of Plane 1, ensure XY Plane is selected from the Method drop-down list.

   4. Enter 0 for Z.

   5. Click Apply.

   6. Repeat steps 3.b.i.–v. for the other planes, at Z = 0.08, 0.15, and 0.45 m.

   7. In the Outline tree tab, under User Locations and Plots, deselect Plane 1, Plane 2, Plane 3, and Plane 4.

      

3. Click the Insert menu and select Contour or click the   button.

4. Click OK to accept the default name (Contour 2) and display the details view below the Outline tab.

5. In the Outline tree tab under User Locations and Plots, select Wireframe.

6. Perform the following steps in the details view of Contour 2:

   1. In the Geometry tab, click the   button next to Locations.

      

   2. Select all planes under User Locations and Plots (use Shift for multiple selection).

   3. Click OK.

   4. Select VELOCITIES from the Variable drop-down list (or click  ).

   5. In the Render tab, deselect Show Contour Lines.

   6. Click Apply.

Velocity profiles at the flow inlet, the flow outlet, and planes just before and just after the die exit are displayed (Figure 4.4: Velocity Profiles at Cross-Sections). Compare the velocity profile within the die to the velocity profile just after the die exit at the end of the computational domain. In the die the flow is fully developed. The velocity profile is flat in the extrudate, far away from the die exit; all the particles in the cross-section plane are at the same velocity. Just beyond the die exit, in the transitional zone, the velocity profile is reorganized. The velocity profile on the plane = 15 is no longer fully developed, but it is not yet flat either. The velocity rearrangement is the source of the deformation of the extrudate.

Figure 4.4: Velocity Profiles at Cross-Sections

Compare the cross-section shape of the extrudate with die.

1. Simplify the display.

   In the Outline tree tab, under User Locations and Plots, deselect Contour 2 and Wireframe.

2. Display the die shape using a polyline.

   1. Select Polyline from the Location drop-down menu ( ).

   2. Click OK to accept the default name (Polyline 1) and display the details view below the Outline tab.

      

   3. In the Geometry tab of the details view, select Boundary Intersection from the Method drop-down list.

   4. Click   next to Boundary List and select SUBDOMAIN_1_BOUNDARY_2, SUBDOMAIN_1_BOUNDARY_3, SUBDOMAIN_1_BOUNDARY_4 (use Shift for multiple selection). Click OK to close the Location Selector dialog box.

   5. Select SUBDOMAIN_1_BOUNDARY_1 from the Intersect With drop-down list.

   6. Under the Color tab, click   next to Color and select dark blue.

   7. Click Apply.

3. Display the extrudate shape using a polyline.

   1. Select Polyline from the Location drop-down menu ( ).

   2. Click OK to accept the default name (Polyline 2) and display the details view below the Outline tab.

   3. In the Geometry tab of the details view, select Boundary Intersection from the Method drop-down list.

   4. Click   next to Boundary List and select SUBDOMAIN_2_BOUNDARY_3, SUBDOMAIN_2_BOUNDARY_4, SUBDOMAIN_2_BOUNDARY_5 (use Shift for multiple selection).

   5. Select SUBDOMAIN_2_BOUNDARY_6 from the Intersect With drop-down list.

   6. Click Apply.

4. On the axis triad in the graphics window click +Z to view from Z-direction.

   This allows you to compare the size and shape of the flow inlet with that of the flow outlet without distortion due to perspective.

Figure 4.5: Swelling of the Extrudate

Since the model involves a generalized Newtonian fluid, there are no viscoelastic effects. The swelling (Figure 4.5: Swelling of the Extrudate) is only due to reorganization of the velocity profile at the die exit. Fluid from the high-speed region moves to the low-speed region and pushes the free surface to the exterior.

Create a 2D plot on the diagonal of the die.

1. Define the line of the plot with the points (0.0, 0.1, 0.1) and (0.1, 0.0, 0.1).

   These values are in meters.

   1. Select Line from the Location drop-down menu ( ).

   2. Click OK to accept the default name (Line 1) and display the details view below the Outline tab.

      

   3. Enter 0, 0.1, 0.1 for Point 1 and 0.1, 0, 0.1 for Point 2.

   4. Click Apply.

2. Create a plot.

   1. Click the chart button  .

   2. Click OK to accept the default name (Chart 1) and display the details view below the Outline tab.

      

   3. In the General tab of the details view, ensure XY - Line is selected for Type, and enter 3D Extrusion for Title.

   4. In the Data Series tab, for Series 1, select Line 1 from the Locations drop-down list (or by clicking the   button).

   5. In the X Axis tab, select X from the Variable drop-down list.

   6. In the Y Axis tab, select VELOCITIES from the Variable drop-down list.

   7. Click Apply.

Figure 4.6: Velocity Magnitude Along a Diagonal of Die Exit Section

The shear-thinning introduced by the Cross law is not clearly visible in Figure 4.6: Velocity Magnitude Along a Diagonal of Die Exit Section due to the large finite elements along the die wall. The mesh should be refined in that zone.

Plot X-velocity close to center of the die.

1. Define the line of the plot with the points (0.08, 0.02, 0.00) and (0.08, 0.02, 0.50).

   1. Select Line from the Location drop-down menu ( ).

   2. Click OK to accept the default name (Line 2) and display the details view below the Outline tab.

   3. Enter 0.08, 0.02, 0 for Point 1 and 0.08, 0.02, 0.5 for Point 2.

   4. Click Apply.

2. Create a plot.

   1. Click the chart button  .

   2. Click OK to accept the default name (Chart 2) and display the details view below the Outline tab.

   3. In the General tab of the details view, ensure XY is selected for Type, and disable Display Title.

   4. In the Data Series tab, select Line 2 from the Locations drop-down list for Series 1.

   5. In the X Axis tab, select Z from the Variable drop-down list.

   6. In the Y Axis tab, select VELOCITIES X from the Variable drop-down list.

   7. Click Apply.

Figure 4.7: X-Velocities Along a Line Close to the Center of the Die

Plot Y-velocity close to the center of the die.

1. In the Y Axis tab of the details of Chart 2, select VELOCITIES Y from the Variable drop-down list.

2. Click Apply.

Figure 4.8: Y-Velocities Along a Line Close to the Center of the Die

Plot Z-velocity close to the center of the die.

1. In the Y Axis tab of the details view of Chart 2, select VELOCITIES Z from the Variable drop-down list.

2. Click Apply.

   Figure 4.9: Velocities Along a Line Close to the Center of the Die shows that the flow slows down ( decreases) after the die exit. Meanwhile, particles travel from the center of the extrudate toward the edge, creating the swelling of the extrudate. Figure 4.7: X-Velocities Along a Line Close to the Center of the Die and Figure 4.8: Y-Velocities Along a Line Close to the Center of the Die show that the peak values of and are located at the very beginning of the extrudate, and vanish at the end of the free jet.

Figure 4.9: Velocities Along a Line Close to the Center of the Die