Modeling

Soft pneumatic actuators are designed to handle large deformations and large mechanical strains. At these high values of strain, the actuator behavior is highly unpredictable. The materials employed to fabricate these actuators exhibit complex hyperelastic, viscoelastic non-linear behavior. Furthermore, fabricating soft pneumatic actuators is time consuming and it is helpful to know the performance characteristics obtainable a priori. Thus, numerical models using the finite element method (FEM) are developed to predict actuator behavior at large deformation values so as to design more efficient actuators and soft robotic components. 

A set of four demos is presented in this section to guide the user step-by-step through the process of creating and testing a numerical model for the actuators using the commercial FEM software AbaqusTM . The software interfaces with the python scripts provided in the design tool and enables the automation of the design procedure by providing capabilities for geometry and material variation as input design parameters. 

The following demos are provided:

Demo 1: Modeling Multi-Chamber Linear Actuators

Demo 2: Modeling Multi-Chamber Bending Actuators

Demo 3: Modeling Single-Chamber Shell-Reinforced Linear Actuators

Demo 4: Modeling Single-Chamber Shell-Reinforced Bending Actuators

Demo 1: Multi-Chamber Bending SPA

1. ACTUATOR GEOMETRY

The script create_geom.py is used to create both linear as well as bending actuators. In this case, the script is run to create a 4-chambered bending actuator as shown below. The bending actuator achieves bending motion due to a thin un-stretchable layer attached at the bottom of the structure. Due to the symmetry of the structure, only half the portion of the entire actuator is created and modeled.

The geometric parameters of the actuator, such as the height, width and the length of a chamber, and the height and width of the inlet tunnel, the wall thickness, along with the number of chambers can be customized using the script. Further details on the input parameters are described in the script.

As an example, the following geometry is generated in Abaqus CAE when the script is run using the parameters shown below:

Example: create_geom.py actuator bnd U ogden3.mat outfile.cae 0.05 200 4 --mesh_size 2.0 --chamber 8 8 2 --wall 7


2. MATERIAL CONSTITUTIVE MODEL

The elastomers typically used to create soft actuators exhibit hyperelastic behavior. The design tool provides the ability to model this behavior using several well-established constitutive laws (for a complete list, please see the scripts section). In addition, the user has the option to include viscoelastic behavior as well to capture any time dependent effects. For this example, the chambers are made in Exoflex-30 material while the thin un-stretchable layer is made of silk. The material Ecoflex-30 is modeled using a hyperelastic model while silk is modeled using a linear elastic model, as shown in image below. A matfile containing the material parameters is provided as an input to the script. A 3-term Ogden model is used for Ecoflex-30 in this example, with the following coefficients:

mu1 = 0.001887; alpha 1 = -3.848; mu2 = 0.02225; alpha2 = 0.663; mu3= 0.003574; alpha 3 = 4.225; D1 = 2.93; D2 = 0; D3 = 0



3. PRESSURE LOADS

The input loads are also specified as one of the parameters in the script above. In this example, an input pressure of 50 kPa was specified on the chamber and passage walls.  The following figure shows the corresponding load application in the Abaqus CAE file generated using the script.



4. BOUNDARY CONDITIONS

The boundary conditions include half symmetry, as mentioned previously, and no translation for the inlet portion. These are also applied by default in the CAE file generated using the script. The corresponding images are shown below.



5. MESH GENERATION

The input and CAE files generated are ready to run for obtaining output and post-processing as they also include a mesh definition. In this case, due to the hyperelastic behavior of the materials used to create the actuators,  standard quadratic elements are used with hybrid formulation and reduced integration. This ensures that any issues associated with shear or volumetric locking are avoided and that large deformations are permitted, as is expected in the case of the materials implemented for these actuators. The following image shows the mesh generated using the script, using a default element size of 2.0. The mesh size can be controlled as an input parameter through the script.



6. OUTPUT ANALYSIS

A variety of analysis can be performed using the design tool, including evaluation of the actuator performance under free and blocked loading conditions. This is specified in the script using the 'test' input parameter. Either 'U' or 'F' can be specified, signifying a free displacement test or a blocked force test, respectively.

Abaqus ODB result plots for bending motion generated are shown below for the free displacement condition, in which actuator images before and after pressurization are superposed. Plots for bending angle obtained vs. input pressure can also be generated using the script, as shown below.

Further, the actuators can also be tested under blocked end conditions using the scripts provided. For this the 'test' parameter in the script would be modified to the value 'F' instead of 'U' for the example shown above.

Demo 2: Multi-Chamber Linear SPA

The following demo shows how to use the scripts to create and model a 4-chambered linear SPA using the design tool. 

1. ACTUATOR GEOMETRY

The script create_geom.py is used to create both linear as well as bending actuators. In this case, the script is run to create a 4-chambered linear actuator as shown below. Due to the symmetry of the structure, only a quarter portion of the entire actuator is created and modeled.

The geometric parameters of the actuator, such as the height, width and the length of a chamber, and the height and width of the inlet tunnel, the wall thickness, along with the number of chambers can be customized using the script. Further details on the input parameters are described in the script. 

As an example, the following geometry is generated in Abaqus CAE when the script is run using the parameters shown below:

Example: create_geom.py actuator lin U ogden3.mat outfile.cae 0.05 200 4 --mesh_size 2.0 --chamber 8 8 2 --wall 7

 

2. MATERIAL CONSTITUTIVE MODEL

The elastomers typically used to create soft actuators exhibit hyperelastic behavior. The design tool provides the ability to model this behavior using several well-established constitutive laws (for a complete list, please see the scripts section). In addition, the user has the option to include viscoelastic behavior as well to capture any time dependent effects. For this example, the material Ecoflex-30 is modeled. A matfile containing the material parameters is provided as an input to the script. A 3-term Ogden model is used in this example, with the following coefficients:

mu1 = 0.001887; alpha 1 = -3.848; mu2 = 0.02225; alpha2 = 0.663; mu3= 0.003574; alpha 3 = 4.225; D1 = 2.93; D2 = 0; D3 = 0

3. PRESSURE LOADS

The input loads are also specified as one of the parameters in the script above. In this example, an input pressure of 50 kPa was specified on the chamber and passage walls.  The following figure shows the corresponding load application in the Abaqus CAE file generated using the script. 

4. BOUNDARY CONDITIONS

The boundary conditions include quarter symmetry, as mentioned previously, and no translation for the inlet tunnel. These are also applied by default in the CAE file generated using the script. The corresponding images are shown below. 

5. MESH GENERATION

The input and CAE files generated are ready to run for obtaining output and post-processing as they also include a mesh definition. In this case, due to the hyperelastic behavior of the materials used to create the actuators,  standard quadratic elements are used with hybrid formulation and reduced integration. This ensures that any issues associated with shear or volumetric locking are avoided and that large deformations are permitted, as is expected in the case of the materials implemented for these actuators. The following image shows the mesh generated using the script, using a default element size of 2.0. The mesh size can be controlled as an input parameter through the script. 

6. OUTPUT ANALYSIS

A variety of analysis can be performed using the design tool, including evaluation of the actuator performance under free and blocked loading conditions. This is specified in the script using the 'test' input parameter. Either 'U' or 'F' can be specified, signifying a free displacement test or a blocked force test, respectively.

Abaqus ODB result plots for displacement and Von Mises stress are showed below for the free displacement condition, from which plots for displacement vs. input pressure can be generated. 

The stress plots are helpful in identifying the stress concentration regions within the actuator, such as in the narrow passage walls between chambers in the image above. The actuator can then be better designed given a specific application. 

Displacement plots as a function of input air pressure, such as the one shown below, can be easily generated using the script run_tests, and used to evaluate the actuator motion profile. 

Similarly, the actuator can be simulated under blocked conditions to generate plots as shown below. 

 

Demo 3: Shell-Reinforced Bending SPA

1. ACTUATOR GEOMETRY

The models for bending shell-reinforced actuators are available open-source here

In these actuators, a single air chamber is modeled for providing enhanced mechanical reliability of the actuator by eliminating stress concentrations at narrow passage walls. Furthermore, the cross-section of the air chamber is circular in this case as compared to the square cross-section for multi-chamber actuators described in other demos. The bending actuator achieves bending motion due to a thin un-stretchable layer attached at the bottom of the structure. Due to the symmetry of the structure, only half the portion of the entire actuator is created and modeled.

The geometric parameters of the actuator, such as the length and diameter of the chamber, the wall thickness, and the cut spacing on shell surface can be customized using the models provided.

As an example, the following geometry is generated in Abaqus CAE for a bending actuator with an outer diameter of 4 mm, wall thickness of 2 mm and total length of 40 mm. The number of cuts on shell surface is 7, at a cut spacing of 1 mm.



2. MATERIAL CONSTITUTIVE MODEL

The elastomers typically used to create soft actuators exhibit hyperelastic behavior. The design tool provides the ability to model this behavior using several well-established constitutive laws (for a complete list, please see the scripts section). In addition, the user has the option to include viscoelastic behavior as well to capture any time dependent effects. For this example, the chamber is made in Exoflex-30 material while the thin un-stretchable shell layer is made of a plastic material such as PET. The material Ecoflex-30 is modeled using a hyperelastic model while the shell is modeled using a linear elastic model (due to stresses in shell not exceeding elastic range). A 3-term Ogden model is used for Ecoflex-30 in this example, with the following coefficients:

mu1 = 0.001887; alpha 1 = -3.848; mu2 = 0.02225; alpha2 = 0.663; mu3= 0.003574; alpha 3 = 4.225; D1 = 2.93; D2 = 0; D3 = 0

3. PRESSURE LOADS

In this example, an input pressure of 50 kPa was specified on the chamber walls.  The following figure shows the corresponding load application in the Abaqus CAE file generated.



4. BOUNDARY CONDITIONS

The boundary conditions include half symmetry, as mentioned previously, and no translation or rotation for the inlet portion. The corresponding images are shown below.

5. INTERACTION

To achieve bending motion profile, a thin strip portion at the bottom of the shell is attached to the core surface using an adhesive. The shell is permitted to slide over the surface of the actuator and guide its trajectory in the remaining portions. To implement this condition in Abaqus, a tie constraint is imposed at the thin unstretchable portion while a contact property is defined to include finite sliding in tangential orientation with a specified coefficient of friction in the remaining portions, as shown below.



6. MESH GENERATION

In this case, due to the hyperelastic behavior of the material used to create the actuator core,  standard linear 3-D stress elements are used with hybrid formulation and reduced integration. This ensures that any issues associated with shear or volumetric locking are avoided and that large deformations are permitted, as is expected in the case of the materials implemented for these actuators. For the shell structure, standard linear shell elements with reduced integration are used. The following image shows the mesh generated for the shell, as an example.

7. OUTPUT ANALYSIS

A variety of analysis can be performed using the design tool, including evaluation of the actuator performance under free and blocked loading conditions. Abaqus ODB result plots for linear extension motion generated are shown below for the free displacement condition.

 

Demo 4: Shell-Reinforced Linear SPA

1. ACTUATOR GEOMETRY

The models for linear shell-reinforced actuators are available open-source here.

In these actuators, a single air chamber is modeled for providing enhanced mechanical reliability of the actuator by eliminating stress concentrations at narrow passage walls. Furthermore, the cross-section of the air chamber is circular in this case as compared to the square cross-section for multi-chamber actuators described in other demos. The linear actuator achieves linear motion due to the corresponding shell pattern discussed earlier in the design section. Due to the symmetry of the structure, only half the portion of the entire actuator is created and modeled.

The geometric parameters of the actuator, such as the length and diameter of the chamber, the wall thickness, and the cut spacing on shell surface can be customized using the models provided.

As an example, the following geometry is generated in Abaqus CAE for a linear actuator with outer diameter of 4 mm, wall thickness of 2 mm and total length of 40 mm. The number of cuts on shell surface is 13, at a cut spacing of 0.5 mm.



2. MATERIAL CONSTITUTIVE MODEL

The elastomers typically used to create soft actuators exhibit hyperelastic behavior. The design tool provides the ability to model this behavior using several well-established constitutive laws (for a complete list, please see the scripts section). In addition, the user has the option to include viscoelastic behavior as well to capture any time dependent effects. For this example, the chamber is made in Exoflex-30 material while the thin un-stretchable shell layer is made of a plastic material such as PET. The material Ecoflex-30 is modeled using a hyperelastic model while the shell is modeled using a linear elastic model (due to stresses in shell not exceeding elastic range), as shown in images below. A 3-term Ogden model is used for Ecoflex-30 in this example, with the following coefficients:

mu1 = 0.001887; alpha 1 = -3.848; mu2 = 0.02225; alpha2 = 0.663; mu3= 0.003574; alpha 3 = 4.225; D1 = 2.93; D2 = 0; D3 = 0


3. PRESSURE LOADS

In this example, an input pressure of 50 kPa was specified on the chamber walls.  The following figure shows the corresponding load application in the Abaqus CAE file generated.



4. BOUNDARY CONDITIONS

The boundary conditions include half symmetry, as mentioned previously, and no translation or rotation for the inlet portion. The corresponding images are shown below.

5. INTERACTION

In this design, the shell is permitted to slide over the surface of the actuator and guide its trajectory. To implement this condition in Abaqus, a contact property is defined to include finite sliding in tangential orientation with a specified coefficient of friction, as shown below. 

Surface-to-surface contact is then defined between the shell and the actuator surface using the contact property defined above, as shown in the image below.



6. MESH GENERATION

In this case, due to the hyperelastic behavior of the material used to create the actuator core,  standard linear 3-D stress elements are used with hybrid formulation and reduced integration. This ensures that any issues associated with shear or volumetric locking are avoided and that large deformations are permitted, as is expected in the case of the materials implemented for these actuators. For the shell structure, standard linear shell elements with reduced integration are used. The following image shows the mesh generated for the shell, as an example.



7. OUTPUT ANALYSIS

A variety of analysis can be performed using the design tool, including evaluation of the actuator performance under free and blocked loading conditions. Abaqus ODB result plots for linear extension motion generated are shown below for the free displacement condition.

It is seen that the stress concentration occurs at the notches in the shell structure. This stress can be reduced by increasing the number of cuts on the shell surface. The following image shows reduction in stress obtained for the case of an actuator with 21 cuts on shell surface, as an example.