Prediction method of linear expansion coefficient of glass fiber reinforced mechanical structure based on ANSYS Workbench

Abstract

The present invention discloses a method for predicting the linear expansion coefficient of a glass fiber reinforced mechanical structure based on ANSYS Workbench. The method obtains the fiber orientation information of the mechanical structure through mold flow software calculation, imports it into ANSYS Workbench, maps the fiber orientation information through the Material Designer and Injection Molding Data modules, solves the problem after setting the load and boundary conditions in Static Structural, processes and calculates the deformation results through MATLAB, and then predicts the average linear expansion coefficient of a specific position. The present invention can predict the average linear expansion coefficient of anisotropic materials while avoiding the complex characteristics of conventional calculation models. The algorithm is simple and flexible, and can calculate the linear expansion coefficients of different positions, which is convenient for subsequent use in application scenarios with high accuracy requirements for the prediction of the linear expansion coefficient.

Description

Technical Field

[0001] The present invention relates to the field of mechanical thermodynamics simulation, and in particular to a method for predicting the linear expansion coefficient of a glass fiber reinforced mechanical structure. Background Art

[0002] Fiber-reinforced materials are composite materials based on high-performance fibers and a resin matrix. From early natural fiber reinforcements to current high-performance fibers such as carbon fiber, glass fiber, and aramid fiber, the research and development of fiber-reinforced materials has progressed significantly, with continuous technological innovation and a broadening range of applications. These materials, with their excellent mechanical properties, lightweight construction, and corrosion resistance, are widely used in aerospace, automotive, construction, and other fields.

[0003] Glass fiber reinforced mechanical structures are generally injection molded from fiber reinforced materials. During this process, the fibers and matrix flow in the mold cavity and are affected by factors such as the melt temperature, injection pressure, and the shape of the mold cavity. Different microstructures are present at different locations in the molded mechanical structure, leading to anisotropic thermodynamic properties. In many application scenarios, high accuracy requirements are placed on the linear expansion coefficient. In the aerospace field, the material of the device is affected by extreme temperatures when flying at high speeds, and its linear expansion coefficient needs to be accurately predicted to simulate the thermodynamic properties of the mechanical structure under such conditions. In the field of optics, the linear expansion coefficient of mechanical structures such as lens barrels affects the thermal stability of the optical system. An accurate linear expansion coefficient helps to achieve athermal design in the optical design stage. The anisotropy caused by injection molding makes the inherent linear expansion coefficient of the material unreliable, and corresponding fiber orientation analysis is required for specific mechanical structures to obtain accurate linear expansion coefficient prediction results.

[0004] In order to accurately demonstrate the performance of anisotropic structures in thermodynamic analysis, the fiber orientation can be mapped to the ANSYS Workbench grid for overall thermodynamic analysis. However, due to the complex field distribution of anisotropic materials, this analysis method is often very time-consuming, especially in complex assembly analysis, where it consumes a large amount of computing resources. Therefore, a single, accurate linear expansion coefficient as a material parameter can help improve analysis efficiency. Existing linear expansion coefficient prediction models are generally based on regular layered fiber distributions, and the calculation model is simple. If they are to be applied to the complex fiber orientation distribution caused by the injection molding process, a complex calculation model must be established, and the algorithm is difficult to write and requires a large amount of calculation. Summary of the Invention

[0005] The purpose of the present invention is to address the shortcomings of the existing technology and provide an ANSYS Workbench-based method for predicting the linear expansion coefficient of glass fiber reinforced mechanical structures. The method can be applied to anisotropic materials, and the algorithm is simple and flexible. It can also calculate the average linear expansion coefficient at any position, which can then be used in subsequent analysis.

[0006] The object of the present invention is achieved through the following technical solutions:

[0007] A method for predicting the linear expansion coefficient of a glass fiber reinforced mechanical structure based on ANSYS Workbench includes the following steps:

[0008] Step 1: Import the geometric model of the glass fiber reinforced material structure into the mold flow software for injection molding analysis to obtain the distribution of fibers in the structure, and export the mesh information file and fiber orientation file corresponding to the distribution;

[0009] Step 2: Create a Static Structural module in ANSYS Workbench, and import the geometric model containing the glass fiber reinforced material structure described in step 1 into the Geometry of the module;

[0010] Step 3: Create a Material Designer module in ANSYS Workbench. In the Engineering Data section of this module, select the matrix material and fiber material corresponding to the glass fiber reinforced material described in Step 1 and set the corresponding parameters. After modeling is completed, link Material Designer to the Engineering Data section of the Static Structural module described in Step 2.

[0011] Step 4: Create an Injection Molding Data module in ANSYS Workbench, import the mesh information file and fiber orientation file described in step 1, link it to the Model of the Static Structural module described in step 2, and update it;

[0012] Step 5: Enter the Mechanical tab of the Static Structural module created in Step 2, select the material for the geometric model described in Step 2, specify the corresponding fiber orientation distribution field, set the load and boundary conditions, and then solve the problem. Export the deformation results to a result file.

[0013] Step 6: Use MATLAB to read the result file described in step 5 to obtain the deformation variable ΔL, temperature change ΔT, and initial length L. According to the calculation formula: Calculate the average linear expansion coefficient at the desired location.

[0014] Furthermore, the step three is implemented through the following sub-steps:

[0015] (3.1) Create a new Material Designer module in ANSYS Workbench and open Engineering Data.

[0016] (3.2) In Engineering Data Source, select the matrix material and fiber material corresponding to the glass fiber reinforced material described in step 1;

[0017] (3.3) Enter the Material Designer module and select Analytical Model from the Short Fiber Composite drop-down menu to calculate the homogenized mean field parameters.

[0018] (3.4) Set the volume content and fiber aspect ratio in Setup. Check Compute Coefficient of Thermal Expansion and Compute Thermal Conductivity in Settings to calculate the expansion coefficient and thermal conductivity of the glass fiber reinforced material.

[0019] (3.5) Select Variable Material in Analyses, edit the material that can vary with the region, select Sampling Strategy as custom, enter Short Fiber Wizard and set the number of sampling points;

[0020] (3.6) Click "Update" to complete the calculation of the homogenized mean field parameters;

[0021] (3.7) After completing the modeling, link it to the EngineeringData of the Static Structural module described in step 2. Open EngineeringData to see the basic data of the glass fiber reinforced material.

[0022] Furthermore, the step 5 is implemented by the following sub-steps:

[0023] (5.1) Open the Model of the Static Structural module created in step 2 and enter Mechanical;

[0024] (5.2) Select the glass fiber reinforced material imported in step 3 for the geometric entity;

[0025] (5.3) Click the Imported Element Orientation branch under the Geometry branch, select the corresponding geometry in the details, set Mapping Control to Manual, turn on Orientation Realignment, right-click Element Orientation under the branch, and select Import Element Orientation to complete the import of the element orientation vector;

[0026] (5.4) Click the Imported Material Field branch under the Materials branch. In the Details section, select the corresponding geometry and the material field to be imported. Right-click the corresponding material field and select Import Material Field to complete the import of the fiber direction distribution field.

[0027] (5.5) Set the Thermal Condition load, that is, select the geometry to which the load is to be applied and set the uniform temperature condition to be simulated;

[0028] (5.6) Set the Displacement load, that is, select the end face to be constrained and set the direction of the movement suppression to 0; click Analysis Settings, and turn on Weak Springs in the details to prevent the geometry from being under-constrained and causing solution problems, while not limiting the expansion dimension of the geometry;

[0029] (5.7) Perform calculations, view the deformation results, and select Export Text File to export the deformation results.

[0030] The beneficial effect of the present invention is that, with the help of the commonly used finite element analysis software ANSYS Workbench, the calculation of the anisotropic material field distribution based on fiber orientation is completed, and the anisotropic expansion results are obtained through simulation. A simple algorithm is used for data processing to calculate the average linear expansion coefficient of the corresponding mechanical structure. This coefficient can be input into the material properties of the engineering data in subsequent thermodynamic analysis, thereby avoiding the increased computational complexity caused by introducing anisotropic field distribution in more complex assembly analysis, saving computing resources and improving analysis efficiency. At the same time, the algorithm used in the present invention is simple and flexible, does not require the establishment of a complex mathematical model, and can meet the needs of calculating the linear expansion coefficient at different positions, can adapt to a variety of application scenarios, and facilitate subsequent analysis. BRIEF DESCRIPTION OF THE DRAWINGS

[0031] Figure 1This is a flow chart of the linear expansion coefficient prediction method for glass fiber reinforced mechanical structures based on ANSYS Workbench.

[0032] Figure 2 This is a schematic diagram of the links between the various modules of ANSYS Workbench.

[0033] Figure 3 This is the A11 fiber orientation distribution field cloud map.

[0034] Figure 4 This is the A22 fiber orientation distribution field cloud map.

[0035] Figure 5 This is a schematic diagram of thermal deformation results in ANSYS Workbench. DETAILED DESCRIPTION

[0036] The present invention will be described in detail below with reference to the accompanying drawings and preferred embodiments, and the purpose and effects of the present invention will become more apparent. It should be understood that the specific embodiments described herein are only used to explain the present invention and are not intended to limit the present invention.

[0037] like Figure 1 As shown, the linear expansion coefficient prediction method for glass fiber reinforced mechanical structures based on ANSYS Workbench of the present invention includes the following steps:

[0038] Step 1: Import the geometric model of the glass fiber reinforced material structure into the mold flow software for injection molding analysis to obtain the distribution of fibers in the structure. Then, export the mesh information file and fiber orientation file corresponding to the distribution. These two files should be in a file format recognizable by the Injection Molding Data module of ANSYS Workbench.

[0039] In this example, the mold flow software used is MoldFlow, the mechanical structure is a lens mount, and the glass fiber reinforcement material is a composite material with a PA66 matrix and a glass fiber content of 30%. After completing the fiber orientation analysis in MoldFlow, run the strintf3d macro command to export the corresponding mesh information file and fiber orientation file. The suffixes are .pat and .xml, respectively, which are file formats recognized by the InjectionMolding Data module (used in step 4).

[0040] Step 2: Create a Static Structural module in ANSYS Workbench and import the lens base geometry model obtained in step 1 into the Geometry section of the module.

[0041] Step 3: Create a Material Designer module in ANSYS Workbench. In the Engineering Data section of this module, select the matrix material and fiber material corresponding to the glass fiber reinforced material in Step 1, and set the volume content and fiber aspect ratio. After modeling is completed, link Material Designer to the Engineering Data section of the Static Structural module in Step 2 to transfer the generated glass fiber reinforced material to the engineering data of Static Structural. This step is divided into the following sub-steps.

[0042] 1) Create a new Material Designer module in ANSYS Workbench and open EngineeringData.

[0043] 2) In Engineering Data Source, select Resin Polyamide / Nylon 66 (the base material) and E-Glass (the fiber material) corresponding to the glass fiber reinforcement material in step 1.

[0044] 3) Enter the Material Designer module and select Analytical Model from the Short Fiber Composite drop-down menu to calculate the homogenized mean-field parameters.

[0045] 4) In Setup, set the volume fraction to 30 and the fiber aspect ratio to 20. In the settings, check Compute Coefficient of Thermal Expansion and Compute Thermal Conductivity to calculate the expansion coefficient and thermal conductivity of the glass fiber reinforced material.

[0046] 5) Select Variable Material in Analyses, edit the material that can vary with the region, select Sampling Strategy as custom, and enter the Short Fiber Wizard to set the number of sampling points.

[0047] 6) Click "Update" to complete the calculation of the homogenized mean field parameters.

[0048] 7) After completing the modeling, link it to the Engineering Data of the Static Structural module in step 2. Open Engineering Data to see the basic data of the glass fiber reinforced material, named Variable Short FiberResin Polyamide / Nylon66 / E-Glass.

[0049] Step 4: Create an Injection Molding Data module in ANSYS Workbench, import the mesh information file and fiber orientation file obtained in step 1, link it to the Model of the Static Structural module in step 2, and update it. The final link relationship between the modules is as follows: Figure 2 shown.

[0050] Step 5: Enter the Mechanical tab in the Static Structural module created in Step 2, select the material for the geometric model in Step 2, specify the corresponding fiber orientation distribution field, set the load and boundary conditions, and solve the model. Export the deformation results as a result file. This step is divided into the following substeps.

[0051] 1) Open the Model of the Static Structural module created in step 2 and enter Mechanical;

[0052] 2) Select the glass fiber reinforced material Variable Short Fiber ResinPolyamide / Nylon 66 / E-Glass imported in step 3 for the geometric entity;

[0053] 3) Click the Imported Element Orientation branch under the Geometry branch, select the corresponding geometry in the details, set Mapping Control to Manual, turn on Orientation Realignment, right-click Element Orientation under the branch, and select Import Element Orientation to complete the import of the element orientation vector;

[0054] 4) Click the Imported Material Field branch under the Materials branch, select the corresponding geometry and the material field to be imported in the details, right-click the corresponding material field, and select Import Material Field to complete the import of the fiber direction distribution field. The A11 fiber orientation distribution field is as follows: Figure 3 As shown, the A22 fiber orientation distribution field is as follows Figure 4 As shown;

[0055] 5) Set the Thermal Condition load. That is, select the entire lens base geometry and set the uniform temperature condition to be simulated to 60°C.

[0056] 6) Set the Displacement load. Specifically, select the bottom surface of the lens mount as the constrained end surface and set the direction of movement suppression to 0. This example aims to obtain expansion results along the optical axis, i.e., the x-axis, so the x-direction is set to 0. Click Analysis Settings and, in Details, enable Weak Springs to prevent underconstrained geometry from causing solution problems. This also does not restrict the geometry's expansion dimension.

[0057] 7) Perform calculations and check thermal deformation results, such as Figure 5 As shown in the figure, select Export Text File to export the deformation results. The data format includes the number, position and displacement of each node.

[0058] Step 6: Use MATLAB to read the result file of step 5 and obtain the deformation variable ΔL, temperature change ΔT, and initial length L. According to the calculation formula: Calculate the average linear expansion coefficient at the desired location. The deformation ΔL and length L are related to the location of the target surface. The algorithm screens node coordinates to identify nodes within the target plane (or within a very small range) and averages the displacements of these nodes as the displacement of the target plane. The average linear expansion coefficient at the target plane location is then calculated using the formula.

[0059] Those skilled in the art will understand that the foregoing descriptions are merely preferred embodiments of the invention and are not intended to limit the invention. Although the invention has been described in detail with reference to the foregoing examples, those skilled in the art will still be able to modify the technical solutions described in the foregoing examples or substitute equivalents for some of the technical features therein. Any modifications, equivalent substitutions, etc. made within the spirit and principles of the invention shall be included within the scope of protection of the invention.

Claims

1. A method for predicting the linear expansion coefficient of a glass fiber reinforced mechanical structure based on ANSYS Workbench, characterized in that: The following steps are involved: Step 1: Import the geometric model of the glass fiber reinforced material structure into the mold flow software for injection molding analysis to obtain the distribution of fibers in the structure, and export the mesh information file and fiber orientation file corresponding to the distribution; Step 2: Create a Static Structural module in ANSYS Workbench, and import the geometric model containing the glass fiber reinforced material structure described in step 1 into the Geometry of the module; Step 3: Create a Material Designer module in ANSYS Workbench. In the EngineeringData of this module, select the matrix material and fiber material corresponding to the glass fiber reinforced material described in Step 1 and set the corresponding parameters. After modeling is completed, link Material Designer to the EngineeringData of the Static Structural module described in Step 2. Step 4: Create an Injection Molding Data module in ANSYS Workbench, import the mesh information file and fiber orientation file described in step 1, link it to the Model of the Static Structural module described in step 2, and update it; Step 5: Enter the Mechanical tab of the Static Structural module created in Step 2, select the material for the geometric model described in Step 2, specify the corresponding fiber orientation distribution field, set the load and boundary conditions, and then solve the problem. Export the deformation results to a result file. Step 6: Use MATLAB to read the result file described in step 5 to obtain the deformation variable ΔL, temperature change ΔT, and initial length L. According to the calculation formula: Calculate the average linear expansion coefficient at the desired location.

2. The method for predicting the linear expansion coefficient of a glass fiber reinforced mechanical structure based on ANSYS Workbench according to claim 1, characterized in that: Step 3 is implemented through the following sub-steps: (3.1) Create a new Material Designer module in ANSYS Workbench and open EngineeringData; (3.2) In Engineering Data Source, select the matrix material and fiber material corresponding to the glass fiber reinforced material described in step 1; (3.3) Enter the Material Designer module and select Analytical Model from the Short Fiber Composite drop-down menu to calculate the homogenized mean field parameters. (3.4) Set the volume content and fiber aspect ratio in Setup. Check Compute Coefficient of Thermal Expansion and Compute Thermal Conductivity in Settings to calculate the expansion coefficient and thermal conductivity of the glass fiber reinforced material. (3.5) Select Variable Material in Analyses, edit the material that can vary with the region, select Sampling Strategy as custom, enter Short Fiber Wizard and set the number of sampling points; (3.6) Click "Update" to complete the calculation of the homogenized mean field parameters; (3.7) After completing the modeling, link it to the Engineering Data of the Static Structural module described in step 2. Open Engineering Data to see the basic data of the glass fiber reinforced material.

3. The method for predicting the linear expansion coefficient of a glass fiber reinforced mechanical structure based on ANSYS Workbench according to claim 1, characterized in that: The step 5 is implemented by the following sub-steps: (5.1) Open the Model of the Static Structural module created in step 2 and enter Mechanical; (5.2) Select the glass fiber reinforced material imported in step 3 for the geometric entity; (5.3) Click the Imported Element Orientation branch under the Geometry branch, select the corresponding geometry in the details, set Mapping Control to Manual, turn on Orientation Realignment, right-click Element Orientation under the branch, and select Import Element Orientation to complete the import of the element orientation vector; (5.4) Click the Imported Material Field branch under the Materials branch. In the Details section, select the corresponding geometry and the material field to be imported. Right-click the corresponding material field and select Import Material Field to complete the import of the fiber direction distribution field. (5.5) Set the Thermal Condition load, that is, select the geometry to which the load is to be applied and set the uniform temperature condition to be simulated; (5.6) Set the Displacement load, that is, select the end face to be constrained and set the direction of the movement suppression to 0; click Analysis Settings, and turn on Weak Springs in the details to prevent the geometry from being under-constrained and causing solution problems, while not limiting the expansion dimension of the geometry; (5.7) Perform calculations, view the deformation results, and select Export Text File to export the deformation results.

Images