Transcript
Topology Optimization R18.0 Feature and Usage Highlights Additive Manufacturing Application
1
© 2016 ANSYS, Inc.
March 12, 2017
Contents Introduction • Background • Capabilities Overview
New Topology Optimization System • Optimization Feature Set • UI Exposure and Usage Design Validation Workflow • Project Schematic Setup • Editing Optimized Geometry in SpaceClaim • Validating New Design • Export Optimized Model for Manufacture
2
© 2016 ANSYS, Inc.
March 12, 2017
Introduction Why Additive Manufacturing? •
Geometry complexity is free! • Leverage full geometric freedoms, including lattice structures, in designs
•
Minimize number of parts
•
Reduce material waste, improve durability, etc., …
Why simulation is key to realizing full potential of Additive Manufacturing?
• Enables superior designs via physics-driven free-form design optimization methods • E.g., Topological Optimization
• Allows for optimized designs to be validated • Set up and check optimized part for manufacture
3
© 2016 ANSYS, Inc.
March 12, 2017
GE Aviation new fuel nozzle: • 25% lighter • 5 times more durable • 1 vs. 20 parts • Lower cost
Capabilities Overview
R18.0 offers new physics-based design optimization technologies and supporting workflows aimed at realizing the full potential of Additive Manufacturing
•
New Topology Optimization System for Mechanical Physics • • • •
•
Design Validation Workflow • • • • •
4
Link to Static Structural or Modal System Define Optimization Objectives and Constraints Observe evolution of optimized shape as solution progresses Inspect optimized shape Launch system to perform design validation Original and optimized geometry transferred to validation system Edit optimized geometry in SpaceClaim Perform validation analysis on optimized design Export optimized geometry file for 3D printing
© 2016 ANSYS, Inc.
March 12, 2017
Workflow Overview NEW
Print Export Optimized Geometry
Static Structural (or Modal) Problem Set up
Original Assembly
5
© 2016 ANSYS, Inc.
March 12, 2017
Design Optimization
Optimized Part
Design Validation
Validate Design
Topology Optimization System
6
© 2016 ANSYS, Inc.
March 12, 2017
Capabilities Overview • Mechanical Physics • • • • •
Linear Static Structural Modal Steady State Linear Bonded Contact Solid Bodies only (2D and 3D)
• Optimization Objectives • • • •
7
© 2016 ANSYS, Inc.
Minimize Compliance (Maximize Stiffness) • Single and multiple loads Maximize Natural Frequencies • Single and multiple frequencies Minimize Mass Minimize Volume
March 12, 2017
• Response Constraints • • • • •
Mass Volume Global (von-Mises) Stress Displacement (Beta) Natural Frequency
• Manufacturing Constraints • • •
Minimum Member Size Maximum Member Size Pull Out Direction (Beta)
Accessing the Topology Optimization System (1)
Drag and drop new Topology Optimization System from Project Schematic Toolbox on top of Solution Cell of Static Structural or Modal System NOTE: Only one upstream feeder system (Static Structural or Modal) is supported in R18.0.
8
© 2016 ANSYS, Inc.
March 12, 2017
Accessing the Topology Optimization System (2) Linking the Topology Optimization System to a Static Structural or Modal System introduces a new “Topology Optimization” object in the Mechanical Project Outline New default types are added to the Topology Optimization object: • Analysis Settings: Exposes various solver settings and controls • Solution Selection: Indicates the upstream analysis system • Optimization Region: Defines the Design Region as well as Exclusions Regions (regions where material should not be removed) • Response Constraints: Defines limits for mass or volume, or maximum stress during optimization • Objective: Defines the goal of the optimization, such as minimizing compliance or maximizing natural frequencies Additional types may optionally be inserted from the Topology Optimization object
9
© 2016 ANSYS, Inc.
March 12, 2017
Defining the Optimization Region The Design Region can be scoped by: • Geometry • May be an entire assembly, a subassembly, or a multi- or singlebody part • Named Selection • May be any geometry, or grouping of mesh elements Exclusion Regions can de defined by: • Boundary Conditions • Geometry Selection • Named Selection
10
© 2016 ANSYS, Inc.
March 12, 2017
Defining the Design Optimization Objectives Following Design Optimization Objectives can be defined for Static Structural and Modal analyses • Static Structural: Single or Multiple Load steps • Minimize Compliance • Minimize Volume • Minimize Mass • Modal: Single or Multiple Natural Frequencies • Maximize Frequency • Minimize Volume • Minimize Mass Use worksheet to apply different weights to different load steps in Static Structural analyses, or different weights to different modes in Modal analyses
11
© 2016 ANSYS, Inc.
March 12, 2017
Defining Response Constraints Following Response Constraints can be defined for Static Structural and Modal analyses • Static Structural: • Mass (Default set to 50%) • Volume (Default set to 50%) • Displacement (Beta in R18.0) • Global von-Mises Stress • Tabular option available for applying different Global Stress constraint for each load step
• Modal: • Mass (Default set to 50%) • Volume (Default set to 50%) • Natural Frequency • Max/Min frequency range can be added to each mode
12
© 2016 ANSYS, Inc.
March 12, 2017
Defining Manufacturing Constraints Following Manufacturing Constraints can be defined • Minimum Member Size • Maximize Member Size • Pull Out Direction (Beta)
Minimum and Maximum Member Sizes are Program Controlled by default but can also be specified manually Notes on Minimum Member Size: • The Minimum Member Size may be viewed as both a Manufacturing Constraint as well as a numerical filter to ensure there is adequate mesh resolution to accurately capture the smallest features in the optimized design • The default Program Controlled value for Minimum Member Size is 2.5 times the typical mesh element size which is the minimum resolution required to capture the smallest features. Where possible (typically where medium or finer meshes are being used), it is recommended to manually set a larger Minimum Member Size, e.g., 4 to 5 times the typical mesh element size.
13
© 2016 ANSYS, Inc.
March 12, 2017
Optimization Solution Set up • Guidelines for meshing upstream Static Structural or Modal Systems • Set Physics Preference to Mechanical • Use quadrilateral elements (i.e., Mid Side Notes Kept) • Where possible, use a constant element size
• Analysis Settings • Inspect or change settings such as Convergence Accuracy • Program Controlled or default settings
• Launching Topology Optimizer • Right-click on the Solution object under Topology Optimization and select “Solve” • NOTE: Both shared memory parallel (SMP) and distributed memory parallel (DANSYS) options are available which can use up to the maximum number of available physical cores. Select these options from Tools Solver Process Settings… Advanced…
14
© 2016 ANSYS, Inc.
March 12, 2017
Optimization Solution Monitoring Different ways to monitor solution progress • Solver printouts and convergence charts • Accessible from Details view of Solution Information • Charts allow monitoring of objectives and response constraints • Topology Density Tracker • Visualize evolution of shape during solution • Both Nodal Averaged (Default) and Elemental Topology Density Results may be tracked • User may stop solution at any time (say if shape has stabilized visually) and have results available for inspection 15
© 2016 ANSYS, Inc.
March 12, 2017
Postprocessing Optimization Results Visualize and inspect Nodal Averaged (Default) or Elemental Topology Densities •
•
16
Topology Density values range from ~0 to 1.0 • Higher values indicate material that must be kept, lower values indicate redundant material that can be removed Retained Threshold • User can alter the Retained Threshold value and use intuition to decide on “best” topology • The default value of 0.5 represents the reference optimized topology • Color legend provides general guidance to determine final choice of Retained Threshold • Higher values lead to more “slender” models (more aggressive designs), lower values lead to “chunkier” models (more conservative designs) • Volume and mass of the optimized topology are computed for the selected Retained Threshold value and contrasted with the original volume and mass to further help the user determine “best” topology © 2016 ANSYS, Inc.
March 12, 2017
Design Validation Workflow
17
© 2016 ANSYS, Inc.
March 12, 2017
Sequence of Steps to Launch Design Validation Workflow 1. First ensure that Export Topology (STL File) option is set to Yes 2. Launch design validation system from Results Cell of Topology Optimization System • A Duplicate of the upstream feeder system is created and placed downstream of the Topology Optimization System • A data transfer link is established between the Results Cell of the Topology Optimization System and the Geometry Cell of the Design Validation System (System C) 3. “Update” the Results Cell of the Topology Optimization System 4. “Refresh” the Geometry Cell in the Validation System • The STL file of the optimized geometry as well as the original CAD model are transferred to the Geometry Cell of the Validation System • The Geometry application is automatically set to SpaceClaim
18
© 2016 ANSYS, Inc.
March 12, 2017
Edit STL File (Optimized Geometry) in SpaceClaim (1) • • • •
19
Launch SpaceClaim from the Geometry Cell of the Design Validation System STL geometry of optimized model as well as original CAD model are imported into SpaceClaim IMPORTANT: The imported STL file is not suitable for performing validation analysis. It must be edited and converted to a solid geometry Following editing operations are performed in SpaceClaim • Smooth and coarsen facets on the “organic” surfaces • Optionally add more material around bolt holes, contact surfaces, etc. • Accurately capture the “prismatic” surfaces of the original CAD model on which boundary or other conditions are applied • Convert the edited STL geometry to solid geometry
© 2016 ANSYS, Inc.
March 12, 2017
Edit STL File (Optimized Geometry) in SpaceClaim (2) •
•
20
The Facets capability in SpaceClaim is used to edit the STL geometry • A wide range of editing tools are available
IMPORTANT: • A separate license is required to use the Facets capability • Activate the Facets tab in the GUI via SpaceClaim Options as follows: • File SpaceClaim Options License • Check STL Prep checkbox
© 2016 ANSYS, Inc.
March 12, 2017
Edit STL File (Optimized Geometry) in SpaceClaim (3) • • •
The main objective is to accurately represent the optimized geometry with an optimal number of facets There are countless ways in which the combination of tools in SpaceClaim can be used to obtain a high quality faceted representation of the optimized model The Shrinkwrap tool is one such tool that may be used to good effect for this purpose. It allows the user: • To capture the “organic” surfaces with coarser facet sizes. •
•
To accurately capture “prismatic” surfaces and other important geometric features with high resolution using smaller facets • •
•
•
21
Use the “Gap size” to set the desired coarse facet size
Use the ”Secondary size” to set the desired smaller facet size Use the “Select Tight-Fit Faces of Facets” option to select faces from the original CAD model (highlighted in blue in image) which will be wrapped with the smaller facet size Use the “Angle threshold” to set the desired angle below which features will be preserved
Select the Facets object only in the SpaceClaim Structure tree and then click the green check mark to wrap the optimized STL geometry
© 2016 ANSYS, Inc.
March 12, 2017
Edit STL File (Optimized Geometry) in SpaceClaim (4) • • • • •
22
It is possible to optionally add material around selected regions of the optimized model such as bolt holes, lugs, etc. Material is typically added to the original STL geometry before the model is shrink wrapped Surfaces from the original CAD model can be used to create material around selected regions The selected surfaces are copied from the CAD model and pasted on top of the faceted geometry Where appropriate, only portions of some of these surfaces may be used by clipping off extraneous areas – e.g. the surface attached to one of the lugs
© 2016 ANSYS, Inc.
March 12, 2017
Edit STL File (Optimized Geometry) in SpaceClaim (5) • • •
23
The “Pull” tool under the Design tab is used to create solid regions around the bolt holes and lugs The “Merge” tool under the Facets tab is used to merge the solid regions into the optimized STL geometry The merged geometry is then shrink wrapped using the Angle threshold, Gap and Secondary size settings
© 2016 ANSYS, Inc.
March 12, 2017
Convert Model to Solid Geometry and Prepare for Transfer to Design Validation System •
It is recommended to create a copy of the Shrinkwrap object •
•
Select Shrinkwrap object in SpaceClaim model tree • •
•
Right-click and select Convert to solid Merge faces Solid model is created
Preparing for Transfer • •
•
24
This will be needed later for exporting to a 3D printer
It’s important to ensure only intended geometric objects are transferred to the design validation system To do this select original CAD part - and any additional solid and/or faceted geometries that you may have created during your geometry editing operations - right click and select “Suppress for physics” Exit SpaceClaim
© 2016 ANSYS, Inc.
March 12, 2017
Perform Design Validation (1) • • • •
25
Double click Model Cell of validation system (System C) in project schematic to launch the validation system Click “Yes” to import the optimized solid model into the validation system On start up, the original CAD model is replaced with the new optimized solid model Note that associativity of all problem set up attributes, such as material properties, boundary conditions, mesh sizing, etc. are lost. These will need to be reapplied manually and the optimized geometry re-meshed before the validation analysis can be performed
© 2016 ANSYS, Inc.
March 12, 2017
Perform Design Validation (2) •
•
26
As a first step it is recommended to “Generate Virtual Cells” using default settings of “Automatic” Method combined with “Low” Behavior • While not strictly necessary, this reduces the number of surface patches in the model and leads to more optimal meshes It is also helpful to further group into virtual surfaces all surface patches on boundaries where Loads, Supports, or other BCs are to be applied • The “Extend to Limits” group selection tool can be used to facilitate selecting boundary surfaces with a large number of small faces • Right-click and Insert Virtual Cell
© 2016 ANSYS, Inc.
March 12, 2017
Perform Design Validation (3) • • • •
Re-associate Material and related properties to the optimized geometry Reapply Loads, Supports, and any other boundary conditions Reapply and readjust as needed any mesh sizings and re-mesh the optimized model Guidelines for re-meshing optimized model: •
• • • •
27
Use same Mechanical Physics preference, quadrilateral elements, and where possible constant element sizing as used for meshing the original CAD model in the upstream analysis system (see slide 14) The preferred meshing method is the default Patch Conforming Method Due to the organic nature of optimized model shape, tetrahedral elements are the preferred choice of elements for such geometries Use the default Mechanical “Adaptive” Size Function If difficulties are encountered meshing the model with the Patch Conforming Method, use the Patch Independent Method
© 2016 ANSYS, Inc.
March 12, 2017
Perform Design Validation (4) • •
28
Solve and inspect the solution on the optimized geometry to determine if the design objectives have been met The solutions on the original and optimized models may be compared
© 2016 ANSYS, Inc.
March 12, 2017
Prepare and Export Optimized Geometry for 3D Printing •
After the optimized design has been validated, return to SpaceClaim to prepare and export the optimized geometry for additive manufacture •
•
The Shrinkwrap geometry can be exported directly as an STL file for import to a 3D printer
•
Prior to exporting you may optionally choose to further smooth the optimized geometry using the Smooth command under the Facets tab: • • •
29
Recall that a copy of the Shrinkwrap object was made for this purpose
Select the Approximate Smooth type option Enter a desired Angle threshold (default is 60o) This smoothing operation increases the number of facets
© 2016 ANSYS, Inc.
March 12, 2017
