Getting started with abaqus

Harvard University – SEAS ES227
Last Updated: 21-Jan-2013 Created by: Panos Polygerinos – January 2013
1
Getting Starting with Abaqus 6.11
Basic Guide for Fluid-Structure Interaction problems
In this guide we will go through the steps required to simulate a soft pneumatic actuator using Abaqus.
This actuator consists of 4 parts: the main body of the actuator and its two thin bottom layers that
enclose a piece of paper.

2
Start Abaqus 6.11 CAE software.
Import the parts (.STEP files from your CAD software, e.g. SolidWorks)
Note: All parts are imported as Solids except the piece of paper. This one will be designed later within
the Abacus environment as a Shell.

3
Create the MATERIALS and set their properties. We need two materials: (a) the elastomer (called
Elastosil), and (b) the piece of paper.

4
Create one SECTION for each of the materials. The (a) elastomer is set as solid and the (b) paper
as shell.
(a) 
(b) 

5
Now, go back to the parts you have imported and for each one of them assign a material property. To do
this, you will have to click on the Section Assignment option and select the entire part geometry.

6
Select all the instances to be imported into the assembly section. Assembly the parts creating
constraints.
Note: Before the assembly process, return to the part list and under the part ‘Bottom Layer B’
create a Surface by selecting one of its two major faces. This surface geometry will be used to
create a skin that acts as the inextensible layer (paper) of the soft actuator.

7
Under the assembly section, click Merge/Cut Instances and select the entire assembly. A new part, the
merged part, will be created in the parts list.
Select the newly created part and click to create a Skin. The software will ask you to select the entity on
which it will create the skin. We want to select the surface of the ‘Bottom Layer B’ that we created in
the previous page. To do so, you will have to go to: Tools - > Display Group -> Manager.

8
The ‘Part Display Group Manager’ will appear – select Create. The ‘Create Display Group’ will
now come up – select ‘Surfaces’ and click on the created surface from the list and then
‘Replace’ and ‘Dismiss’.
Select the top surface to create the skin.

9
While at the Megred part, click on the ‘Section Assignment’. There you should already have three
sections. To create a new section for the paper double click the ‘Section Assignment’ and then select the
region to be assigned a property by clicking again on the top surface. The ‘Edit Section Assignment’
window will appear where you should select the Paper as the Section. Make sure the Type is ‘Shell,
Homogeneous’. Click OK. You have successfully created one more section assignment for the paper.
Continuing on the same part from the parts list, click on the ‘Mesh’ module. Under the ‘Mesh Controls’
select all the parts of the assembly and then click the option ‘Tet’.

10
Seed the part with an ‘Approximate global size’ equal to 3 and Mesh the part.
Note: Because we are using a hyperelastic material, a Hybrid element type for the mesh should be use.
Go to: Mesh -> Element type and activate the tick on ‘Hybrid Formulation’ for all the hyperelastic parts.
Click on Steps to create the first step that accounts for the gravity acting on the actuator. Select a ‘Static,
General’ procedure type and in the next window turn ON the Nlgeom option.

11
Under Step-1, select ‘Loads’ and activate Gravity as the selected type for the step. Set the gravity value
on the negative Y axis.
Click on BCs (Boundary conditions), and select symmetry. Continue and click on the face of the part that
is going to be fixed. Select ‘Encastre’ to fix the surface.

12
Create a second step. This step will have all the attributes of the previous step propagated to it and the
pressure inside the cavity of the actuator will be enabled here. To do so, we will have to go back to the
merged part and create a Set. From the Parts list, click on the ‘Merged’ part and by holding the Shift Key
select all the internal faces of the cavity that will interact with the air.
Note: to help facilitate this, use the Cross Section views provided from the View Cut Manager.

13
Within the second step, create a Pressure load. To pick the internal cavity click at the bottom right
corner the button ‘Surfaces’ and select the Surf-Cavity. At the next window provide the pressure value
to be applied in the cavity.

14
Now, we are ready to submit the Job and run the simulation. Click on Jobs to create a new job. Right
click on the newly created job and select submit. You have the option to select to monitor the progress
of the simulation by selecting ‘Monitor…’.

15
Once the simulation finishes, you can observe and analyze the results by right clicking at the created job
and selecting ‘Results’.

Getting started with abaqus

Recommended

Recommended

More Related Content

Similar to Getting started with abaqus

Similar to Getting started with abaqus (20)

Recently uploaded

Recently uploaded (20)

Getting started with abaqus