Prepare a working folder for your simulation.

Download the 2d_axi_blow_molding.zip file here .

Unzip the 2d_axi_blow_molding.zip file you have downloaded to your working folder.

The mesh file 2d-axi-blowmold.msh can be found in the unzipped folder.

Start Workbench from Start > Ansys 2025 R1 > Workbench 2025 R1.

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

Save the Ansys Workbench project using File → Save, entering Final-blow-mold as the name of the project.

Import the mesh file (2d-axi-blowmold.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. Select the following options:

   • F.E.M. task

   • Time-dependent problem(s)

   • 2D axisymmetric geometry

   The Current setup is updated to reflect the selected options. This example is a simulation of blow molding for a 2D axisymmetric bottle and the mold is two-dimensional. The problem is assumed to be time-dependent.

2. Click Accept the current setup.

Define the mold.

  Define molds

1. Create a mold.

     Create a new mold

2. Select an adiabatic mold.

     Adiabatic mold

3. When prompted, click OK to retain the default name for the mold (Mold 1).

4. Specify the solid region that represents the mold.

     Domain of the mold

   1. Select SUBDOMAIN_1 and click Remove.

      SUBDOMAIN_1 is moved from the top list to the bottom list, indicating that the mold is defined as SUBDOMAIN_2 .

   2. Click Upper level menu at the top of the menu.

5. Specify the boundary that represents the part of the mold that comes into contact with the fluid.

   Polyflow Classic uses this information to determine the penetration distance (into the mold) of every point of the free surface (BOUNDARY2).

     Contact conditions

   1. Select No contact along BOUNDARY5 and click Modify.

      The free surface, BOUNDARY2 of the preform comes into contact with the mold wall, BOUNDARY5 (as shown in Figure 2.2: Boundary Set for the Problem).

      

   2. Select Contact.

6. Click Upper level menu four times to return to the F.E.M. Task 1 menu.

Create a sub-task for the isothermal flow.

  Create a sub-task

1. Select Generalized Newtonian isothermal flow problem.

   A dialog box opens, asking for the title of the problem.

   

2. Enter blow molding 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.

The domain is divided into two subdomains, one for the fluid preform (SUBDOMAIN_1) and the other for the mold (SUBDOMAIN_2). In this problem, the sub-task applies only to the preform.

  Domain of the sub-task

1. Select SUBDOMAIN_2 and click Remove.

   

   SUBDOMAIN_2 is moved from the top list to the bottom list, indicating that the sub-task is defined on SUBDOMAIN_1 .

2. Click Upper level menu at the top of the menu.

   The Material data menu item is highlighted.

Define the viscosity of the preform.

1. Click Shear-rate dependence of viscosity.

2. Click Constant viscosity.

3. Click Modify fac to specify the value of , which is referred to as “fac” in the graphical user interface.

   Polydata prompts for the new value of the viscosity.

   

4. Enter 100000 [units: poise] as the New value and click OK.

5. Click Upper level menu two times to continue with the Material Data specification.

Define the density of the preform.

1. Click Density.

2. Click Modification of density to specify the value of the density.

   Polydata prompts for the new value of the density.

   

3. Enter 1 [units: g/cm³] as the New value and click OK.

4. Click Upper level menu to continue with the Material Data specification.

Enable the calculation of the inertia terms in the momentum equation.

In this problem inertia plays an important role. When internal pressure is applied, the preform expands, and the fluid accelerates towards the mold. In order to obtain a realistic blowing time, inertia must be taken into account.

1. Click Inertia terms.

2. Select Inertia will be taken into account.

3. Click Upper level menu to continue with the Material Data specification.

Include the effects of gravity in the flow.

The fluid preform flows in the negative y direction under gravity, so specify the component of gravity along the y direction ().

1. Click Gravity.

2. Click Modify gy to specify the value of gravity in the y direction.

     Modify gy

   Polydata prompts for the new value of the gravity along the y-axis.

3. Enter -981 [units: cm/s²] as the New value and click OK.

4. Click Upper level menu two times to return to the blow molding menu.

   The Flow boundary conditions menu item is highlighted.

Retain the default condition Axis of symmetry along BOUNDARY1.

No action is required to accept the default value. You can simply proceed to the next step. For 2D axisymmetric models, Polydata recognizes the axis of symmetry from the mesh file and automatically imposes the symmetry condition along the line .

Set the conditions at the outer free surface (BOUNDARY2).

The free surface boundary condition in contact detection problems is different from their simulations in Polyflow Classic. In blow molding problems, a free surface comes into contact with a solid mold. Polyflow Classic applies a contact detection algorithm at each location of the surface to detect the occurrence of the contact.

You need to specify the following for the free surface on BOUNDARY2:

1. Select Zero wall velocity (vn=vs=0) along BOUNDARY2 and click Modify.

2. Click Free surface.

3. Specify the contact detection problem.

   1. Click Contact (blow mold).

   2. Click Create a new contact problem.

   3. Specify where the free surface will contact the mold.

      Polyflow Classic uses the definition of the contact wall in the determination of the penetration distance (into the mold) of every point of the free surface (BOUNDARY2).

      Click Select a contact wall.

   4. Select Mold 1 : Contact along BOUNDARY5 and click Select.

      As shown in Figure 2.2: Boundary Set for the Problem, the free surface (BOUNDARY2) of the preform comes into contact with the mold (BOUNDARY5).

   5. Define the slipping coefficient.

        Modify slipping coefficient

      Retain the default value of 1e+12 and click OK.

      With such a high value of the slipping coefficient, the fluid will stick to the contact wall.

   6. Define the penalty coefficient.

        Modify penalty coefficient

      Retain the default value of 1e+12 and click OK.

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

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

   In contact detection problems, abrupt changes in the velocity field occur at the contact points between the fluid preform and the mold. Polydata gives the warning message shown below. Since the prediction of the velocity field in such cases destroys the prediction scheme, you can continue by clicking OK.

   

5. Click OK to accept the warning and continue.

Set the conditions at the top part of the preform (BOUNDARY3).

1. Select Zero wall velocity (vn=vs=0) along BOUNDARY3 and click Modify.

2. Click Normal velocity and tangential force imposed ( vn, fs ).

3. Click Upper level menu to accept the default value of 0 for the normal velocity, .

4. Click Upper level menu to accept the default value of 0 for the tangential force, .

Set the conditions at the inner free surface (BOUNDARY4).

This boundary of the preform is subjected to pressure by the application of a normal force, so specify a normal force along this boundary.

1. Select Zero wall velocity (vn=vs=0) along BOUNDARY4 and click Modify.

2. Click Free surface.

3. Specify the normal force.

   1. Click Normal force.

   2. Select Constant.

      Polydata prompts for the new value of the normal force.

      

   3. Enter -2e06 as the New value and click OK.

   4. Click Upper level menu.

4. Click Upper level menu to return to the Flow boundary conditions menu.

Click Upper level menu to return to the blow molding menu.

The Global remeshing menu item is highlighted.

Specify the region where the remeshing is to be performed (SUBDOMAIN_1).

  1–st local remeshing

Click Upper level menu to accept the default selection of SUBDOMAIN_1.

Click Lagrangian on the border only.

For information on remeshing techniques, see Appendix.

1. Click Accept the current setup in the Element distortion check menu.

   In blow molding simulations, the finite-element mesh can undergo great deformations. The Element distortion check menu deals with the detection of all possible distortions of the elements. In this problem, you can accept the default options and proceed to the next step.

2. Click Upper level menu two times to return to the F.E.M. Task 1 menu.

Specify the parameters for the iterative scheme in the calculation of the free surface.

  Modify the transient iterative parameters

For information on time marching scheme, see Appendix.

1. Specify the time limit.

   This option specifies the time at which the solution procedure stops.

     Modify the upper time limit

   Polydata prompts for the new value of the time limit.

   Enter 0.1 [units: s] as the New value and click OK.

2. Specify the initial value of the time step.

   This option is used to define the initial time step, which is used for the calculation of the next two time steps. After that, the step size is automatically calculated by Polyflow Classic. This first time step should be set according to the characteristic time scale of the process considered.

     Modify the initial value of the time-step

   Enter 1e-03 [units: s] as the New value and click OK.

3. Specify the minimum value for the time step.

   If a calculated value for the time step falls below the minimum for the time step at any point in the calculation, the iterative scheme stops since this might be a symptom of calculation difficulties.

     Modify the min value of the time-step

   Enter 1e-07 [units: s] as the New value and click OK.

4. Specify the maximum value for the time step.

   In order to guarantee accuracy of the time-marching scheme and to avoid useless calculations (rejection of inaccurate time steps), you can limit the growth of the time increment.

     Modify the max value of the time-step

   Enter 1e-03 [units: s] as the New value and click OK.

5. Specify the tolerance for time marching.

   The tolerance is the admissible error between the predicted solution and the exact solution at a particular time step. A very small value of the tolerance can result in large computational costs and a very large value can result in wrong solution.

     Modify the tolerance

   Retain the default value of 0.01 and click OK.

6. Specify the maximum number of successful steps.

   This option is used to select the maximum number of converged steps. If this value is reached, the calculation stops, even if the upper time limit has not been reached.

     Modify the max number of successful steps

   Retain the default value of 200 and click OK.

7. Enable Use of the implicit Euler method.

Click Upper level menu three times to return to the top-level Polydata menu.

Click Output Triggering.

1. Click Enter the number of steps.

   Polydata prompts you for the number of steps.

2. Enter 4 as the New value and click OK.

Click Upper level menu twice.

Specify the system of units.

1. Click Modify system of units.

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

Click Upper level menu twice to return to the top-level Polydata menu.

Create a new sub-task.

  Create a sub-task

1. Click No when asked whether you want to copy an existing sub-task.

2. Click Postprocessor.

3. Enter parison thickness as the New value for the title and click OK.

Click Parison thickness.

Click parison #01.

Click OK twice to accept the warnings about defining the borders.

You will have to define these borders at a later stage.

Specify the region where the postprocessor sub-task applies.

  Domain of the sub-task

Accept the default of SUBDOMAIN_1 by clicking Upper level menu.

Specify the boundary sets representing the starting and ending borders to be used in the thickness calculation.

Polyflow Classic evaluates the distance between these borders at a point between them to determine the thickness at that location.

  Borders for thickness calculation

1. Select BOUNDARY2: not used and click Modify.

2. Click Starting border.

3. Select BOUNDARY4: not used and click Modify.

4. Click Ending border.

Click Upper level menu five times to return to the top-level Polydata menu.

Click Accept.

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 the Polyflow Classic format results file is (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 system.

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

Align the view as shown in the following figure.

Display contours of thickness in the fluid region (SUBDOMAIN_1).

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

2. In the box that opens, click OK to accept the default name (Contour 1) and display the details below the Outline tree.

   

3. Specify the following settings under the Geometry tab:

   1. Select SUBDOMAIN_1_surf from the Locations drop-down list.

   2. Select estim. THICKNESS from the Variable drop-down list, or click the ellipsis button ( ) on the right and select estim. THICKNESS.

   3. Click Apply.

4. Annotate the display.

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

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

   3. Enable Embed Auto Annotation under the Definition tab.

   4. Select Time Value from the Type drop-down list.

   5. Click Apply.

Figure 2.3: Contours of Thickness at the Final Time-step t = 0.1 s

Show contours of thickness on the full blown bottle.

1. Double-click Default Transform in the Outline tree tab, under User Locations and Plots (or right-click Default Transform and select Edit).

   

2. Disable Instancing Info From Domain under the Definition tab in the details of Default Transform.

3. Enable Apply Reflection, and select YZ Plane from the Method drop-down list.

4. Retain the default value of 0.0 m for X.

5. Click Apply.

6. Click the   button to center the view.

Figure 2.4: Contours of Thickness on the Full Blown Bottle at t = 0.1 s

Display contours of thickness at various timesteps.

Display the results at several time steps to see the shape and thickness of the parison during the blow molding process.

Tools → Timestep Selector or click the   button.

1. Select the 20 ^th timestep and click Apply.

2. Select the 40 ^th timestep and click Apply.

3. Select the 60 ^th timestep and click Apply.

4. Select the final timestep and click Apply.

   The thickness decreases as the parison inflates. At the final time step, the thickness is smallest where the parison has been the most extended, (in the corner of the bottle). It is largest at the top where the deformation was much less important due to the small diameter here.

   Figure 2.5: Contours of Thickness at the 20th Timestep

   
   
   

   Figure 2.6: Contours of Thickness at the 40th Timestep

   
   
   

   Figure 2.7: Contours of Thickness at the 60th Timestep

   
   
   

   Figure 2.8: Contours of Thickness on the Full Blown Bottle at t = 0.1 s

   
   
   

Create and save an animation.

1. Click the Tools menu and select Animation or click the   button.

2. Enable Timestep Animation in the Animation dialog box.

   

3. Enable Save Movie to save the animation as a file.

4. Disable   to save only one cycle of animations.

5. Click the start button  .

Display contours of velocity in the fluid region.

1. Double-click Contour 1 under the Outline tab to display the details view.

2. Select VELOCITIES from the Variable drop-down list and click Apply.

   There is zero velocity at the contact between the parison and the mold, but the velocity magnitude is still important where the fluid does not yet touch the mold. At the final time of the simulation, the velocity is near zero, which indicates that the contact is completed. The residual value originates from the penalty formulation used for the contact, as explained in 3D Thermoforming of a Blister.

   Figure 2.9: Final Velocity Distribution