Abaqus simulation process demo
Preface
This example explains in detail the operation process of using abaqus to achieve shape optimization of the connecting rod and Abaqus simulation process demo.
1. Create a model
1. Create geometric components
- Geometry
In the PART module, import the connecting rod isolated mesh part: a single isolated mesh part meshed with linear tetrahedral (C3D4) elements. The connecting rod is symmetric about the X–Y plane.
2. Define material properties
In the PROPERTY module, create the Elastic_Mat material: an elastic material with a density of 7.81E-09 tonne/mm3, a Young’s modulus of 210000 MPa, and a Poisson’s ratio of 0.3. 
Create a Section-Solid section: solid, homogeneous, material: Elastic_Mat.
Assign the section: assign the Section-Solid section to the entire solid part.
3. Create assembly entities
In the ASSEMBLY module, create the instance.
4. Create analysis steps
In the STEP module, create two static general analysis steps.
- Create step-1 analysis step
- Create step-2 analysis step
5. Create interactions
In the INTERACTION module, create a kinematic coupling constraint: couple the motion of a set of (slave) nodes on a face to the motion of a reference node.
- Create Constraint-1 motion coupling constraint
- Create a Constraint-2 kinematic coupling constraint
6. Create boundary conditions and loads
Create boundary condition 1 (first analysis step): Fix all degrees of freedom of the large-end control point m_Set-ControlPt2: U1=U2=U3=UR1=UR2=UR3=0.
Create load 1 (first analysis step): Apply a concentrated force of 25000N along the positive direction of the Z axis at the small-end control point m_Set-ControlPt1.
Create boundary condition 2 (second analysis step): Restrict all degrees of freedom of the large-end control point m_Set-ControlPt2 except U2: U1=U3=UR2=UR3=0, UR1=0.04.
Create boundary condition 3 (second analysis step): Restrict all degrees of freedom of the small-end control point m_Set-ControlPt1 except U2 and UR1: U1=U2= UR2=UR3=0.
Create load 2 (second analysis step): Apply a concentrated force of 2000N along the negative direction of the Z axis at the small-end control point m_Set-ControlPt1.
Create load 3 (second analysis step): Apply a concentrated force of 1750N along the positive direction of the Y axis at the large end control point m_Set-ControlPt2.
7. Create an analysis job and submit the analysis
In the JOB module, create a Job-1 analysis job and submit the analysis.
8. Visualization Post-Processing
In the Job Manager, click Results to enter the visualization module.
2. Setting Optimization
1. Create an optimization task
In the OPTIMIZATION module, create a condition-based shape optimization task, where the design region is the surface nodes and the smoothing region is the elements with an area larger than the design region.
2. Create a responsive design
Create Design Response 1: Maximum von Mises stress in the design region during the first analysis step.
Create Design Response 2: Maximum von Mises stress in the design region during the second analysis step.
Create Design Response 3: Total volume of elements in the design region.
3. Create the objective function
Create an objective function: The objective function determines which of the two design responses results in the maximum von Mises stress in the design node. The objective function then attempts to minimize the maximum von Mises stress for that design response.
4. Create constraints
Create constraints: limit the volume of the model to remain unchanged after optimization.
Create geometric constraint 1: limit the right part of the optimized model to be demolded from the forging die along the positive direction of the x-axis.
Create geometric constraint 2: limit the left part of the optimized model to be demolded from the forging die along the negative direction of the x-axis.
5. Create an optimization process
In the JOB module, create an optimization process and set the maximum number of loops to 15. Click Submit in the Optimization Process Manager to perform analysis.
3. Execution Optimization
1. Monitor optimization progress
Click Monitor in the Optimization Process Manager to monitor the optimization progress.
Click Results in the Optimization Process Manager to view the optimization results.
- Comparison of maximum stress before and after optimization in the first analysis step (138.1 VS 126.7)
- Comparison of maximum stress before and after optimization in the second analysis step (123.9 VS 121.8)
Link:
