Validation Report: Additional Data Mapping to Structural Analysis Packages

Transcription

1 Autodesk Moldflow Structural Alliance 2012 Validation Report: Additional Data Mapping to Structural Analysis Packages Mapping process-induced stress data from Autodesk Moldflow Insight Dual Domain and 3D meshes to a structural analysis mesh Mapping coefficients of thermal expansion from Autodesk Moldflow Insight and Autodesk Moldflow Adviser Dual Domain and 3D meshes to a structural analysis mesh Workflow and settings Comparison validation of warpage prediction and thermal stress analysis with DS Simulia Abaqus Comparison validation of warpage prediction with Autodesk Simulation Multiphysics after mapping

2 Contents Introduction... 3 Background... 3 Different mesh focus... 3 Mapping strategy... 4 Workflow and Settings... 5 Workflow... 5 Autodesk Moldflow Structural Alliance with DS Simulia Abaqus 6.9 and Create Anchor Points for Warpage Analysis... 7 Autodesk Moldflow Structural Alliance built-in Export Wizard... 8 Autodesk Moldflow Structural Alliance built-in Import Wizard Autodesk Moldflow Structural Alliance with Autodesk Simulation Multiphysics and Simulation Mechanical Create Anchor Points for Warp Analysis Plastic Material Selection Export to Autodesk Moldflow Validation Examples Process-induced stress mapping validation Validation with DS Simulia Abaqus Validation with Autodesk Simulation Multiphysics Conclusion Mapping validation for Coefficients of Thermal Expansion (CTE) Validation with DS Simulia Abaqus

3 Introduction The Autodesk Moldflow Structural Alliance 2012 release supports additional important data sets which can be mapped to a structural analysis mesh, to enable a structural analysis package to predict injection molding process-induced deformation, such as warpage, final residual stress within the molded plastic part; and thermal stresses based on the correct property data predicted by Autodesk Moldflow Adviser and Autodesk Moldflow Insight. In-cavity residual stress for Dual Domain mesh models and initial stress for 3D mesh models are among these new data sets which can be mapped to a structural analysis mesh. These process-induced stresses are the driving factor for plastic part warpage after ejection. The stresses will find a new equilibrium state in an unconstrained condition and become part of the final stress remaining in a molded plastic part, which can be calculated in a structural analysis. Coefficient of thermal expansion (CTE) data is another new data set which can be mapped to a structural analysis mesh. This data mapping enables a structural analysis to account correctly for a distributed CTE due to fiber orientation of a fiber-filled material across a molded plastic part. (Future work is planned to handle distributed CTE due to crystalline morphology of a semi-crystalline material.) Although the process-induced stress data sets are always essential to both non-fiber-filled and fiber-filled materials for a warpage prediction and a further stress analysis in a structural analysis package, the CTE data are mainly for injection molded fiber-filled composites in which the CTE tensor is distributed non-uniformly across the molded part due to fiber orientation. When even a single set of anisotropic CTE data is measured and introduced for a non-fiber-filled material, the first principal direction is changing during the polymer melt flow before it solidifies due to cooling from mold halves. These CTE data, coupled with the mechanical properties of the molded part, are used to calculate the incavity residual stress or initial stress (depending on mesh type) induced by the molding process. The mechanical properties have been mapped in previous releases of Autodesk Moldflow Structural Alliance software. Now the mechanical properties will be coupled with processinduced stress and/or CTE data in a structural analysis. In this release, the mapping of these additional data sets is implemented according to the same approach, which will be explained in the next section, with some consideration of various tensor conventions in different structural analysis packages. Background Different mesh focus In order to catch the high gradient changes across the part thickness in a flow analysis of the injection molding process, multiple layers are used in Autodesk Moldflow s mesh models, as shown in Figure 1. A midplane triangular element is similar to a 3-node shell element with thickness as a geometric property, whereas a Dual Domain mesh is characterized with two matching triangular elements on the top and bottom surfaces with multiple layers in between. In a symmetric cooling condition, the number of layers is reduced to half for more efficient calculation. 3

4 Even with a 3D solid mesh, the number of layers of tetrahedral elements across the thickness should be controlled; six layers are used by default, whereas for fiber orientation calculation, it is suggested to double the default number of layers in order to catch the profiled fiber tensor changes. Figure 1. Autodesk Moldflow s midplane and Dual Domain triangular element with multiple layers (left), and default number of layers of tetrahedral elements in a solid 3D mesh (right). These mesh models can be and have been directly passed to structural analysis packages in the past, but they triggered many warning messages indicating that the element aspect ratios were too high and they were not suitable for accurate structural analysis. On the other hand, major structural analysis packages have many high-order and multi-layered element types that are capable of handling profiled variables within each element, as shown in Figure 2. Their element types are developed for different purposes, and the number of element types grows with required research in the finite element method. However, a common requirement for most structural analysis element types is that the aspect ratio needs to be kept low. Figure 2. Element types of typical structural analysis that require low aspect ratio. Mapping strategy The difficulty in interfacing between Autodesk Moldflow analyses and all of these structural packages was to keep up with all these element types without violating their basic aspect ratio requirement for accuracy. A clear strategy would be mapping the distributed values from one type of mesh to another. However, what could be a generic approach that fits most of the element types? In reviewing these element types, it is found that most of the element types have integration points inside their element domain, as illustrated in Figure 3. These are Gauss integration points used for increasing the accuracy by capturing the distribution within the element domain. In order to develop a generic approach suitable for most the structural analysis packages without going into the details of each element type, the method selected was to map the required values to these integration points of a target mesh. 4

5 Figure 3. Gauss integration points in a hex element of a structural analysis. Having this mapping strategy, the remaining work is to calculate all of these distributed data, which are mostly tensor data, at those Gauss integration points. However, most structural analysis packages do not take input at Gauss integration points, and even if a special arrangement can be made for taking these data from input files, the amount of data would be huge. Therefore this mapping strategy needs to be coupled with an Application Programming Interface (API) in order to achieve seamless and smooth data transfer. This API has been implemented as a dynamic linking library, that is, the Autodesk Moldflow Structural Alliance package, which can be connected to any structural analysis software. DS Simulia Abaqus User Defined Subroutines (UDS) and ANSYS User Programmable Features (UPF) were among the first used with this Autodesk Moldflow Structural Alliance feature. Autodesk Simulation Mechanical and Simulation Multiphysics (formerly Autodesk Algor Simulation products) are the first structural packages to have this feature directly enabled along with the material database from Autodesk Moldflow, which contains thermo-mechanical properties data for thousands of commercial plastic grades. Workflow and Settings Workflow Autodesk Moldflow Structural Alliance 2012 has been implemented in DS Simulia Abaqus 6.9 and 6.10, and within Autodesk Simulation Multiphysics (formerly Algor s MES) and Autodesk Simulation Mechanical (formerly Algor s LSS). The workflow is illustrated in Figure 4; a user should start a model of a structural part or assembly in a structural analysis package, import a model from a CAD system and set up necessary boundary conditions there, then export the geometry to Autodesk Moldflow Insight or Autodesk Moldflow Adviser. Any design-related change should be handled in a CAD system, such as Autodesk Inventor or Autodesk Inventor Fusion, prior to import into a structural analysis package, or by iterative change between a CAD system and the structural analysis package to make sure the structural integrity and performance for the design are reasonable before exporting the component(s) to Autodesk Moldflow for plastic flow and fiber orientation analyses. At least a trial analysis with a set of isotropic mechanical properties can be performed without any major problem, and it is suggested to have an equivalent set of isotropic mechanical properties for such a trial analysis as a reference before using Autodesk Moldflow-produced anisotropic and distributed mechanical properties for the same part in a structural analysis. 5

6 Any injection molding process-related changes should be handled in the Autodesk Moldflow product. These changes include feed system design, cooling system design, and process conditions, among others. Even the meshing of the CAD geometry should be handled in the Autodesk Moldflow product for accuracy reasons, as mentioned previously. Any change to the part exported from a structural analysis should be done with the original CAD model and in the structural analysis package. A limitation must be pointed out that a rotation or translation of the exported geometry within the Autodesk Moldflow environment, such as to optimize the layout for molding, would destroy the connection to the original structural analysis model, because the geometry model in Autodesk Moldflow would not then coincide with the original model for mapping. Figure 4. Workflow between a structural analysis and Autodesk Moldflow product. 6

7 Autodesk Moldflow Structural Alliance with DS Simulia Abaqus 6.9 and 6.10 Create Anchor Points for Warpage Analysis For a warpage analysis, a local coordinate system determined by three anchor points must be used to constrain the rigid body movement for a plastic part. These anchor points are used to constrain a total of six degrees of freedom (DOF) as shown in Figures 5 and 6. Figure 5. Set up anchor points boundary conditions and use Autodesk Moldflow Structural Alliance export wizard. Figure 6. Setting up three anchor points for constraining the rigid body movement. By clicking Create (or Edit if it is already defined) in the CSYS-1 line, then selecting the three points in the right order, as so: the point on which ux, uy, uz are fixed must be selected first; then the second point is selected and its uy and uz are fixed; then the third point is selected and its uz is fixed, as shown in Figure 6. A name for the local coordinate 7

8 system just defined may be given, as shown in Figure 7, then return to the individual boundary condition points to select the local coordinate system. These three point boundary conditions must propagate to Step-1, as shown in Figure 8. Figure 7. Name the newly defined local coordinate system. Figure 8. Make sure the anchor point BCs are propagated to step-1. After specifying these boundary conditions, one can submit a job in Abaqus to see if it indicates any error. Typically, it would complain about no loading specified, or produce zero displacement result, as the specified boundary conditions are only for fixing the rigid body movement, and the expected loading from Autodesk Moldflow will not be there until Autodesk Moldflow flow analysis is complete. Autodesk Moldflow Structural Alliance built-in Export Wizard After specifying boundary conditions, one can use the built-in Autodesk Moldflow Structural Alliance Export Wizard to export the model to the Autodesk Moldflow product, or even in STL file format. In an assembly situation, multiple components from an assembly can be picked to export from a list of the components. There is also a wizard pane for selecting the units option, as shown in Figures

9 Figure 9. Autodesk Moldflow Structural Alliance built-in Export Wizard to guide export steps. Figure 10. Autodesk Moldflow Structural Alliance Export Wizard to pick a component from an assembly. 9

10 Figure 11. Autodesk Moldflow Structural Alliance built-in Export Wizard pane for file format. Figure 12. Autodesk Moldflow Structural Alliance built-in Export Wizard pane for model units. Autodesk Moldflow Structural Alliance built-in Import Wizard After exporting the Abaqus model to Autodesk Moldflow Insight or Autodesk Moldflow Adviser, it can be loaded into the Autodesk Moldflow product for meshing, material selection, process condition setup, and so on. If a fiber-filled material is selected, launching a flow analysis will run the fiber analysis by default, if the required Autodesk Moldflow license is valid. After the flow analysis is complete, the Autodesk Moldflow Structural Alliance Import Wizard built into Abaqus can be used to load in needed results for structural analysis. The Import Wizard pane for graphically checking if the component part is matching the targeted geometry is shown in Figure

11 Figure 13. Autodesk Moldflow Structural Alliance Export Wizard pane for graphically checking if the Moldflow model picked is matching the structural component, from the file names listed. Figure 14. Autodesk Moldflow Structural Alliance Export Wizard pane for additional result option to pick for a structural analysis. These two options are the newly added result data sets for mapping in the Autodesk Moldflow Structural Alliance 2012 release. Autodesk Moldflow Structural Alliance with Autodesk Simulation Multiphysics and Simulation Mechanical The Autodesk Moldflow Structural Alliance toolkit has been implemented in Autodesk Simulation Multiphysics (Algor s MES) and Autodesk Simulation Mechanical (Algor s LSS). To do a structural analysis of an injection molded plastic part that is to be analyzed with Autodesk Moldflow, the material model in the Element Definition dialog must be selected as Moldflow, as shown in Figure

12 Figure 15. Element Definition dialog: select Moldflow as the material model. Create Anchor Points for Warp Analysis If one plans to use Autodesk Simulation Multiphysics or Simulation Mechanical to do a warpage analysis with Autodesk Moldflow Structural Alliance, three anchor points must be defined, with the local coordinate system defined by the anchor points. Figure 16. Select three points to define a LCS for anchoring the part to do warpage analysis. These three anchor points are used to constrain the rigid body movement for the plastic part to be analyzed. A total of six DOF must be constrained, and it is suggested that the first anchor point should constrain the three displacement DOF, as shown in Figure 17, and the second anchor point should be constrained by two of the three displacement DOF, and only one displacement DOF should be fixed on the third anchor point. 12

13 Figure 17. Setting up anchor points with the LCS defined for warpage analysis. Plastic Material Selection After finishing the boundary conditions setup, a Moldflow material can be selected from the database built into Autodesk Simulation Multiphysics or Simulation Mechanical, as shown in Figure 18. Please note that Current Material may not be the Select material when a switch of the material is being done. After clicking OK and returning to the dialog, they will be the same. Figure 18. Selecting a plastic material in Autodesk Simulation Multiphysics. It must also be noted that if a fiber-filled composite material is selected, the modulus of elasticity and the Poisson ratio shown in the Element Material Selection dialog is an 13

14 average into isotropic set of the original anisotropic mechanical properties. The original anisotropic set values can be viewed in Autodesk Moldflow Insight or Moldflow Adviser. Export to Autodesk Moldflow Choose Export to Autodesk Moldflow Insight or Autodesk Moldflow Adviser for Moldflow analysis, as shown in Figure 19. Figure 19. Export to Autodesk Moldflow from Autodesk Simulation Multiphysics or Simulation Mechanical. Validation Examples Process-induced stress mapping validation The key to validating the mapping of process-induced stress is to see if the predicted warpage by another structural analysis with the mapped stress distribution can produce the same warpage as predicted by the Autodesk Moldflow Insight Warp solver. The validation tests have been performed with DS Simulia Abaqus and Autodesk Simulation Mechanical. The following examples have been performed: Simple Box with an unfilled material, Dual Domain and 3D meshes in Autodesk Moldflow Insight to map to HEX element mesh in Abaqus Simple Box with a fiber-filled material, 3D mesh in Autodesk Moldflow Insight to map to the same 3D mesh in Abaqus, and to a Hex mesh in Abaqus Camera model with a fiber-filled material, 3D mesh in Autodesk Moldflow Insight to map to Abaqus mesh 14

15 Validation with DS Simulia Abaqus In the following examples, DS Simulia Abaqus 6.10 has been used for this purpose, to compare the warpage prediction by Autodesk Moldflow Insight 2011 for the same geometry model with the same material properties. 1. The first example is a simple box case meshed with Dual Domain mesh, with an unfilled material for which mechanical properties are isotropic. It will not have the complication with distributed mechanical properties across the part so that it can purely test the process-induced stress mapping. The mesh in DS Simulia Abaqus is a high-order hexagon element mesh, completely different from the mesh in Autodesk Moldflow Insight, which is a Dual Domain, 3-node triangle element mesh with 12 layers in between the matching top and bottom surface elements. Figure 20. Autodesk Moldflow Insight Warp predicted warpage shape and magnitude based on a Dual Domain mesh for an unfilled material. Figure 21. DS Simulia Abaqus predicted warpage with Autodesk Moldflow Structural Alliance mapping of the process-induced stress: in-cavity residual stress produced from Autodesk Moldflow Insight flow solver for the Dual Domain mesh. It readily can be seen that the warpage shape and the magnitude are in very good agreement between Autodesk Moldflow Insight Warp prediction and DS Simulia Abaqus prediction with Autodesk Moldflow Structural Alliance mapped in-cavity residual stress. 15

16 2. The second example is the same geometry but meshed with Autodesk Moldflow Insight 3D mesh, with an unfilled material. The target mesh in DS Simulia Abaqus is still the high-order hexagon element mesh. Autodesk Moldflow Structural Alliance in DS Simulia Abaqus can automatically produce the initial stress needed for Abaqus structural analysis. Comparing the warpage prediction by Autodesk Moldflow Insight as shown in Figures 22 and 23, a very good agreement has been achieved by Autodesk Moldflow Structural Alliance mapping of the initial stress. Figure 22. Autodesk Moldflow Insight Warp3D predicted warpage shape and magnitude for an unfilled material with 3D mesh. Figure 23. DS Simulia Abaqus predicted warpage with Autodesk Moldflow Structural Alliance mapping of the process-induced stress --- initial stress produced from Autodesk Moldflow Insight Warp3D solver for the 3D mesh mentioned above. 3. The third example is the same geometry of the simple box but with a fiber-filled material. Fiber orientation analysis was performed to get the distributed mechanical properties, as shown in Figure

17 The warpage predictions from Autodesk Moldflow Insight and Abaqus are shown in Figures 25 and 26, for Dual Domain mesh to 3D tetra mesh mapping. They are in very good agreement. Figure 24. Autodesk Moldflow Insight fiber orientation result. Figure 25. Autodesk Moldflow Insight warpage prediction of the simple box with a fiber-filled material. 17

18 Figure 26. DS Simulia Abaqus prediction of a solid tetra mesh, with mapped mechanical properties and residual stress from Autodesk Moldflow Insight Dual Domain mesh. 4. The same simple box case with a fiber-filled material is then meshed with Autodesk Moldflow Insight 3D mesh, and the mesh in DS Simulia Abaqus is changed to a highorder hexagon mesh, as shown in Figures 27 and 28. It indicates that mapping between dissimilar meshes is very good. Figure 27. Autodesk Moldflow Insight Warp3D prediction of tetra mesh. 18

19 Figure 28. DS Simulia Abaqus prediction of a solid hex mesh, with mapped mechanical properties and initial stress from Autodesk Moldflow Insight 3D tetra mesh. 5. Camera case with a fiber-filled material. The Autodesk Moldflow Insight mesh and fiber orientation result are shown in Figures 29 and 30. Very good agreement between the two software packages has been achieved. Figure 29. Autodesk Moldflow Insight Mesh of camera model. It is finer than the Abaqus mesh shown in Figure

20 VALIDATION REPORT: ADDITIONAL DATA MAPPING TO STRUCTURAL ANALYSIS PACKAGES Figure 30. Autodesk Moldflow Insight fiber orientation result with Dual Domain mesh. Figure 31. Autodesk Moldflow Insight warpage prediction with Dual Domain mesh. 20

21 Figure 32. DS Simulia Abaqus mesh and warpage prediction with mapped in-cavity residual stress and mechanical properties by Autodesk Moldflow Structural Alliance. Validation with Autodesk Simulation Multiphysics The Autodesk Moldflow Structural Alliance toolkit has been implemented in Autodesk Simulation Multiphysics and Simulation Mechanical, and a number of tests have already been done in the past with Abaqus as it is the same code in Autodesk Moldflow Structural Alliance. However, a simple test is performed with Autodesk Simulation Multiphysics to validate the implementation, as shown in Figures Figure 33. A simple plate molded with a fiber-filled plastic is used to validate the implementation. 21

22 After specifying the boundary conditions and exporting to Autodesk Moldflow Insight as explained in the previous section, flow (including fiber orientation) analysis has been performed in Autodesk Moldflow Insight, as shown in Figure 34. Figure 34. Fiber orientation result by Autodesk Moldflow Insight. Figure 35. Warpage prediction by Autodesk Moldflow Insight. Since both initial stress and fiber-filled composite properties are mapped with Autodesk Moldflow Structural Alliance to Autodesk Simulation Multiphysics, it is a comprehensive validation. The following plot from Autodesk Simulation Multiphysics indicates that a good agreement with Autodesk Moldflow Insight warpage prediction has been achieved, but a small difference can be observed in color shading and in the gating end of the plate where 22

23 a curved shape is observed. The small difference in warped shape may be due to the higher order element type used in Autodesk Simulation Multiphysics. Figure 36. Autodesk Simulation Multiphysics predicted warpage. Conclusion Scenarios incorporating unfilled and fiber-filled materials, Dual Domain mesh to 3D mesh mapping, dissimilar mesh mapping, low density to high density mesh mapping, and high density to low density mesh mapping have been tested in comparisons between Autodesk Moldflow Insight and DS Simulia Abaqus, and between Autodesk Moldflow Insight and Autodesk Simulation Multiphysics. In all of the preceding examples, good agreement in warpage predictions has been demonstrated, which proves that the process-induced stress mapping has been implemented correctly. Mapping validation for Coefficients of Thermal Expansion (CTE) Validation of mapping of CTE data is not done with comparison between two structural analysis solutions; rather, it is done with the same package with either averaged thermomechanical properties or with bounding approach, as shown in this section. Constant isotropic set of thermo-mechanical properties in an unfilled material would not be used in this validation as it is equivalent to be a set of input material properties that is normally done for a metal material without Autodesk Moldflow Structural Alliance. Validation with DS Simulia Abaqus The first example is a simple cantilever plate that is injection molded with a fiber-filled material. The fiber orientation results predicted by Autodesk Moldflow Insight are shown in Figures 37 and 38, corresponding to two gating scenarios: one gate in the middle of the free end two gates, one in the middle of each end Clearly there is a difference in fiber orientation distribution in these two scenarios, and the CTE distributions are different also, so that under the same temperature loading condition, the response from these two scenarios should be different. 23

24 However, it is better to first look at what deflection a constant isotropic set of thermomechanical properties can cause. The constant isotropic set is a set of the mechanical properties averaged from the original anisotropic set of the material, shown in Figure 39, that is, E=7320, v=0.44; whereas the isotropic CTE value is picked from one of the two principal directional CTE values of the material. Figure 37. Fiber orientation result of one gate on the free end of a cantiliver plate. Figure 38. Fiber orientation result of one gate on each end of a cantiliver plate. 24

25 Figure 39. Thermo-mechanical properties of the fiber-filled material used in the cantiliver plate. Figure 40. Scenario one: isotropic mechanical properties with constant CTE = 3.716e-05. Here are the highlights of the boundary conditions: Initial temperature: 80C Boundary condition: end encastre (cantilever plate) Load: temperature reduced to 20C It can be readily seen that the cantiliver plate shrinks quite uniformly due to the constant CTE value, and it deflects linearly with a change of the CTE constant. The only exception is in the encastre end where deformation in the width (X) direction is also constrained, as shown in both Figure 40 and Figure

26 However, with an injection molded fiber-filled polymer composite, the deformation magnitude should be similar to the ones with constant CTE values, but non-uniformly, as shown in Figure 42. Figure 41. Scenario two: isotropic mechanical properties with constant CTE = 1.887e-05. Figure 42. Scenario three: anisotropic fiber-filled composite properties, distributed due to fiber orientation, gated on the free end only. 26

27 It can be also seen from Figure 42 that in the longitudinal direction, in which fiber orientation is dominant in the flow direction, the shrinkage is less than the smaller, constant value isotropic scenario shown in Figure 41, whereas in the cross-flow direction, the shrinkage is higher than with the constant CTE. These non-uniform and anisotropic shrinkages are due to the mapped CTE distribution by Autodesk Moldflow Structural Alliance. Figure 43. Scenario four: anisotropic fiber-filled composite properties, distributed due to fiber orientation, injection gates on both free end and the fixed end. It is also interesting to see how a two-gate injection molded cantiliver plate shrinks with the same fiber-filled material, and the same processing and boundary conditions. From Figure 43 it can be seen clearly that the cantiliver plate deflected up due to higher shrinkage on the top than in the bottom. This is because the CTE values on the top side are less, and the weld line area is weaker because of the gating positions on the top, as shown in Figure 44. Figure 44. The first principal directional CTE distribution viewed on top (left) and on bottom (right). 27

28 Autodesk and Moldflow are registered trademarks or trademarks of Autodesk, Inc., and/or its subsidiaries and/or affiliates in the USA and/or other countries. All other brand names, product names, or trademarks belong to their respective holders. Autodesk reserves the right to alter product and services offerings, and specifications and pricing at any time without notice, and is not responsible for typographical or graphical errors that may appear in this document Autodesk, Inc. All rights reserved. 28