Blow Molding Analysis with SIMULIA ABAQUS CAE

Blow molding analysis with SIMULIA ABAQUS CAE 

Blow molding is a widely used manufacturing process for producing hollow plastic  components such as bottles, containers, and automotive ducts, where the final product quality  is strongly influenced by material behaviour, thermal history, and process parameters.  Predicting thickness distribution during the inflation stage is particularly challenging due to  large deformations, nonlinear viscoelasticity, and evolving material properties. Advanced finite  element tools like Abaqus enable detailed simulation of such processes, offering insights into  deformation patterns and thickness variation. 

In this blog, two simulation approaches are presented for blow molding. The first uses a  standard GUI-based setup, which provides a straightforward implementation but has  limitations in capturing complex material physics. The second approach incorporates a  VUHYPER user subroutine, where crystallization evolution is modelled to account for changes  in material stiffness during deformation. By coupling the mechanical response with  crystallization kinetics, this method more realistically represents polymer behaviour during  stretching and cooling, ultimately enabling improved control over thickness distribution and  achieving a more uniform final product. 

The blow molding process is simulated using an Explicit Dynamics procedure in Abaqus to  accurately capture the large deformations involved. Refer to images given below for the  components involved in blow molding. 

Prefoam, rigid rod and bottle die

Assembly

In this approach, a rigid rod is first displaced to stretch the preform, representing the initial  elongation stage. Subsequently, cavity pressure is applied to inflate the preform until it expands  and conforms to the mold geometry. To enhance thickness uniformity, crystallization evolution  is incorporated into the material model, allowing the polymer stiffness to evolve during  deformation. This behavior is implemented through a VUHYPER user subroutine, enabling a  more realistic representation of material response and improved control over the final shell  thickness. 

The preform material is modeled as a hyperelastic polymer using the Mooney–Rivlin strain  energy potential to accurately capture its nonlinear elastic response under large deformation.  The material constants are defined as input properties and passed into the VUHYPER user  subroutine within Abaqus, enabling customization of the constitutive behavior, including the  incorporation of crystallization effects. To ensure numerical stability during the explicit  simulation, appropriate damping is introduced. The material density is taken as 1020 kg/m³,  representing typical polymer characteristics used in blow molding applications.

Hyperelastic material model

Crystallinity is modeled as an evolving internal variable that depends on the deformation state  of the material, increasing only under tensile and shear loading conditions. Its value is  constrained within the physical bounds of 0 ≤ ���� ≤ 1, ensuring realistic representation  throughout the simulation. As crystallinity increases, the material exhibits progressive  stiffening, capturing the strain-induced solidification behavior typical of polymers during  processing. To reflect this effect within the constitutive model, both Mooney–Rivlin  coefficients are scaled as functions of the evolving crystallinity, enabling the material response  to adapt dynamically with deformation.

VUHYPER interface 

Crystallinity evolution with stretch

Dependency of hyperelastic parameters on crystallinity

The simulation is carried out using the Dynamic Explicit procedure in Abaqus, which is well  suited for problems involving large deformations and severe geometric nonlinearity, as  encountered in blow molding. To improve computational efficiency, mass scaling is applied to  the entire model with a target time increment of 5 × 10−6s, effectively increasing the stable  time step and reducing CPU time. Although blow molding is inherently a quasi-static process,  its highly nonlinear nature makes the explicit approach advantageous. With controlled mass  scaling, the method efficiently captures the forming behavior while maintaining a reasonable  balance between accuracy and computational cost. 

Explicit dynamic step definition 

In the blow molding simulation, two key interactions are defined within Abaqus to accurately  capture the physics of the process. The first interaction involves defining the contact behavior  between the expanding preform and the rigid mold (blow mold cavity). As shown in the image,  a contact property named IntProp-2 is created under the Normal Behavior category, where  the pressure-overclosure relationship is set to “Hard” Contact with the constraint  enforcement method left as Default, and the option to Allow separation after contact is  enabled. This ensures that when the preform inflates and comes into contact with the mold  walls, it does not penetrate through the rigid surface while still being able to separate if needed.  The second interaction defines the Pneumatic Fluid Cavity, which simulates the air pressure  driving the blow molding process. interaction is essential as it replicates the internal air pressure  that inflates the preform outward against the mold, forming the desired shape during the blow  molding process.

Pneumatic fluid cavity

Results and discussion

The expansion of prefoam at different time steps can be seen in figures below. The left side  shows procedure without crystallinity and right side shows the process in which crystallinity is  taken into consideration.

t=0.02 s

t=0.1 s 

t=0.4 s

The irregular stress regions are visible where crystallinity is not taken into consideration. Now  lets take a look at the uniform shell thickness.

Shell thickness distribution

It can be observed that the shell thickness is more uniform when crystallinity evolution is  incorporated. It can be inferred from simulation that, crystallization introduces  strain-dependent hardening that suppresses localized thinning. Redistributes  deformation to softer regions and naturally leads to a more uniform shell thickness. 

The usage of VUHYPER and many more user subroutines in ABAQUS CAE makes it  highly customizable and powerful FEA simulation software, which can handle any kind of  non-linear structural scenarios.

We Urge You To Call Us For Any Doubts & Clarifications That You May Have. We Are Eager to Talk To You

Call Us: +91 7406663589