# 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

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.