Using topology optimization

1: Setup

On your desktop or the appropriate network drive, create a folder named topology_optimization.

Click the link below:

Download the part

Note:

The part files require about 1.4 GB of free disk space and might take some time to download.

Extract the files to your topology_optimization folder.
Start Simcenter 3D or NX.
Open Bracket 02_sim1.sim.

This model represents a bracket that will be affixed to two surfaces with four screws. Since the bracket is intended to be symmetrical, you will optimize only half of the model to reduce processing time.

2: Reset dialog box memory

The options you select in dialog boxes are preserved for the next time you open the same dialog box within a given session. Restore the default settings to ensure that the dialog boxes are in the expected initial state for each step of the activity.

File

Preferences→User Interface

Options

Reset Dialog Memory

OK

3: Examine the model and modal solution

You want the bracket to be as stiff as possible while reducing its weight and constraining one of its modes to not go below a specified frequency. To determine the constraints to impose, you must examine the model's existing weight and the frequency of its modes. A solved Simcenter Nastran SOL 103 Real Eigenvalues solution is provided to enable you to view the frequencies.

Solid Properties Check (Home tab→Checks and Information group→More list)

Drag a selection box around the entire model

OK

The Information window indicates that the total mass is about 9.6E-03 lbf-s²/in.

the Information window

Simulation Navigator

Test Normal Modes→Results
Structural

Post Processing Navigator

Test Normal Modes→Structural

Observe the frequencies of each mode. Mode 7 has a frequency of about 24228 Hz.

4: Create a topology optimization solution

For this solution, you will specify 35 design cycles, and indicate that a linear relationship exists between the material density and the Young's Modulus.

Simulation Navigator

Bracket 02_sim1.sim
New Solution

Name

TO Statics and Modes

Solution Type

SOL 200 Topology Optimization

Bulk Data

Maximum Number of Design Cycles (DESMAX)

35

Penalty Law (DMRLAW)

Linear

Create Modeling Object (Parameters)

AUTOMPC

YES

OK

all dialog boxes

5: Create a normal modes subcase

The frequency design constraint should be applied to a normal modes subcase.

Simulation Navigator

TO Statics and Modes
New Subcase

Step

Nastopt - Normal Modes

OK

6: Add the load and constraints to the solution steps

Simulation Navigator

Constraint Container
Fixed

Ctrl

+ Symmetric

TO Statics and Modes→Nastopt - Statics1→Constraints

Repeat this procedure to add the constraints to the Nastopt - Normal Modes 1 subcase as well.
Load Container
Force(1)
TO Statics and Modes→Nastopt - Statics1→Loads

7: Create the design objective

The design objective is to minimize compliance in the structure (that is, maximize stiffness). This procedure creates a design objective modeling object and a design response quantities modeling object simultaneously, and adds the design objective to the statics subcase. Objectives that are specific to a subcase should appear at the subcase level.

Simulation Navigator

TO Statics and Modes→Nastopt - Statics 1
Design Objective
New or Replace Design Objective

Name	Minimize Compliance

Response Type

Compliance (CMPLNCE)

Optimization Method

MIN

OK

8: Create the design area

To ensure that elements are not removed near the screw holes, the model includes a mesh around each hole, and a separate mesh for the rest of the solid body. You will limit the design area to the mesh for the rest of the body.

Simulation Navigator

TO Statics and Modes
Design Area
New Design Area

Name

Optimization Area

Area Type

Optimization Area

Label

DA1

Element Selection Method

Specified Elements

Type Filter (Top Border bar)

Mesh

OK

9: Create a weight design constraint

Without a weight constraint, the software would use as much material as possible to fulfill the objective of minimizing compliance. You can define weight constraints only at the solution level. In this case, you want the optimized part to weigh between 10–30% of the original weight, which you previously determined to be about 9.6E-03 lbf-s²/in.

Simulation Navigator

TO Statics and Modes
Design Constraint
New Design Constraint

Name	Weight Constraint

Response Type

Total Model Weight (WEIGHT)

Lower

0.001 lbf-s²/in

Upper

0.003 lbf-s²/in

Note:

Be sure to change the unit of measurement to lbf-s²/in.

OK

10: Create a frequency constraint

As the optimization process removes material, the structure becomes more flexible. You will set the lower boundary for the frequency of mode 7 to 8000 Hz.

Simulation Navigator

TO Statics and Modes→Nastopt - Normal Modes 1
Design Constraint
New Design Constraint

Name	Frequency Constraint

Response Type

Normal Modes (FREQ)

Normal Modes Mode Number

7

Lower

8000

OK

11: Specify the topology optimization results

Since this model takes a long time to solve, you can use the provided results with your solution.

Simulation Navigator

TO Statics and Modes→Results
Structural
Specify
Browse (Results File Name)

Files of type

Nastran Results Files (*.op2)

File name

bracket_02_sim1-to_statics_and_modes.op2

OK

all dialog boxes

12: Adjust and export the model

You will adjust the results of the final design cycle to show only the elements with a material density value of 0.7 or higher. You will also smooth the results and export the model as a faceted STL file.

Simulation Navigator

TO Statics and Modes→Results
Structural

Post Processing Navigator

TO Statics and Modes
Structural
Material Density Results

Result is automatically set to Design Cycle 35, which is the last design cycle.

Lower Bound

0.7

Tab

Smooth (Nodal Average)
Facets in STL Format
Facets in Nastran BDF Format

Export

the Information window

Close

13: Import the STL file

Importing the STL file into the original part file can help you visualize the optimized part in the Modeling application. You can also mirror the display to see the entire part.

Simulation Navigator