ANSYS Workbench-based linear expansion coefficient prediction method for glass fiber reinforced mechanical structure

Abstract

The invention discloses a method for predicting a linear expansion coefficient of a glass fiber reinforced mechanical structure based on ANSYS Workbench. According to the method, mechanical structure fiber orientation information is obtained through calculation of mold flow software, the mechanical structure fiber orientation information is imported into ANSYS Workbench, mapping is carried out on the fiber orientation information through a Material Designer module and an Injection Molding Data module, solving is carried out after load and boundary conditions are set in Station Stratum, a deformation result is processed and calculated through matlab, and then the average linear expansion coefficient of a specific position is predicted. According to the method, the average linear expansion coefficient of the anisotropic material can be predicted, meanwhile, the characteristic that a conventional calculation model is complex is avoided, the algorithm is simple and flexible, the linear expansion coefficients of different positions can be calculated, and subsequent application to application scenes with high precision requirements for prediction of the linear expansion coefficients is facilitated.

Description

Technical Field

[0001] The 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 resin matrices. From early natural fiber-reinforced materials to today's high-performance fibers such as carbon fiber, glass fiber, and aramid fiber, the research and development of fiber-reinforced materials has come a long way, with continuous technological innovation and expanding application areas. This type of material is widely used in aerospace, automobile manufacturing, construction engineering and other fields due to its good mechanical properties, lightweight, corrosion resistance and other advantages.

[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 melt temperature, injection pressure, and the shape of the mold cavity. Different microstructures are presented at different positions of the molded mechanical structure, which leads 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 will be affected by extreme temperatures when it is flying at high speed, and its linear expansion coefficient needs to be accurately predicted to simulate the thermodynamic properties of the mechanical structure under such conditions; in the optical field, the linear expansion coefficient of mechanical structures such as lens barrels affects the thermal stability of the optical system, and 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 make the anisotropic structure accurately express its performance in thermodynamic analysis, the fiber orientation can be mapped to the grid of ANSYS Workbench 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, which takes up a lot of computing resources. Therefore, a single accurate linear expansion coefficient as a material parameter is conducive to improving the efficiency of the analysis. The existing linear expansion coefficient prediction model is generally based on regular layered fiber distribution, and the calculation model is simple. If it is applied to the distribution of complex fiber orientation caused by the injection molding process, it is necessary to establish a complex calculation model, and the algorithm is difficult to write and the calculation is large. Summary of the invention

[0005] The purpose of the present invention is to address the deficiencies of the prior art and provide a method for predicting the linear expansion coefficient of a glass fiber reinforced mechanical structure based on ANSYS Workbench, which can be applied to anisotropic materials, has a simple and flexible algorithm, and can calculate the average linear expansion coefficient at any position, which can then be used in subsequent analysis.

[0006] The objective 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 comprises the following steps:

[0008] Step 1: Import the geometric model of the structure containing the glass fiber reinforced material into the mold flow software for injection molding analysis, obtain the distribution of the fibers in the structure, and export the grid 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, select the matrix material and fiber material corresponding to the glass fiber reinforced material in step 1 in the Engineering Data of the module, and set the corresponding parameters. After modeling is completed, link the Material Designer to the Engineering Data of the Static Structural module 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 in the Static Structural module created in step 2, select the material for the geometric model described in step 2, and specify the corresponding fiber orientation distribution field. Set the load and boundary conditions and then solve. Export the deformation results as 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 by the following sub-steps:

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

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

[0017] (3.3) Enter the Material Designer module and select Analytical Model in 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, and check Compute Coefficient of Thermal Expansion and Compute Thermal Conductivity in Setting 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 to 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 Engineering Data 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 as 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, select the corresponding geometry and the material field to be imported in the details, right-click the corresponding material field, select Import Material Field, and 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, set the direction of the movement suppression to 0; click Analysis Settings, turn on Weak Springs in the details to prevent the geometry from being under-constrained and causing solution problems, and do not limit 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 the fiber orientation is completed, and the anisotropic expansion result is obtained by simulation, and the data is processed by a simple algorithm 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 the subsequent thermodynamic analysis, thereby avoiding the situation where the amount of calculation increases due to the introduction of anisotropic field distribution in more complex assembly analysis, and can save computing resources and improve analysis efficiency. At the same time, the algorithm used in the present invention is simple and flexible, does not need to establish a complex mathematical model, and can meet the needs of calculating the linear expansion coefficients of different positions, can adapt to a variety of application scenarios, and is convenient for subsequent analysis. BRIEF DESCRIPTION OF THE DRAWINGS

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

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

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

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

[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 based on the accompanying drawings and preferred embodiments, and the purpose and effects of the present invention will become more clear. It should be understood that the specific embodiments described herein are only used to explain the present invention and are not used to limit the present invention.

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

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

[0039] In this embodiment, mold flow software is moldflow, the mechanical structure is a lens base, and the glass fiber reinforced material is a composite material with PA66 as the matrix and 30% glass fiber content. After completing the fiber orientation analysis in moldflow, run the strintf3d macro command to export the corresponding mesh information file and fiber orientation file, with the suffixes .pat and .xml respectively, which are file formats recognizable by the InjectionMolding Data module (for use in step 4).

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

[0041] Step 3: Create a Material Designer module in ANSYS Workbench, select the matrix material and fiber material corresponding to the glass fiber reinforced material in step 1 in the Engineering Data of this module, and set the volume content and fiber aspect ratio. After completing the modeling, link Material Designer to the Engineering Data of the Static Structural module in step 2 to complete the transfer of 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 the matrix material Resin Polyamide / Nylon 66 and the fiber material E-Glass corresponding to the glass fiber reinforced material in step 1.

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

[0045] 4) In Setup, set the volume content to 30 and the fiber aspect ratio to 20. In setting, 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 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 the 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 in the Static Structural module created in step 2, select the material for the geometric model in step 2, and specify the corresponding fiber orientation distribution field. Set the load and boundary conditions and then solve. Export the deformation results as a result file. This step is divided into the following sub-steps.

[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 orientation 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, that is, select the bottom surface of the lens base as the constrained end surface, and set the direction of the movement suppression to 0. This embodiment aims to obtain the expansion result in the direction of the optical axis, that is, the x-axis direction, so the x-direction is set to 0. Click Analysis Settings, turn on Weak Springs in the details to prevent the geometry from being under-constrained and causing solution problems, and do not limit the expansion dimension of the geometry;

[0057] 7) Perform calculations and check the thermal deformation results, such as Figure 5 As shown, 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 get the deformation variable ΔL, temperature change ΔT, and initial length L, according to the calculation formula: Calculate the average linear expansion coefficient of the required position. The deformation variable ΔL and length L are related to the position of the target surface. The algorithm needs to screen the node coordinates to determine the nodes within the target plane (or within a very small range), and take the average of these node displacements as the displacement value of the target plane, and then calculate the average linear expansion coefficient of the target plane position according to the formula.

[0059] Those skilled in the art can understand that the above are only preferred examples of the invention and are not intended to limit the invention. Although the invention is described in detail with reference to the above examples, those skilled in the art can still modify the technical solutions recorded in the above examples or replace some of the technical features therein with equivalents. Any modification, equivalent replacement, etc. made within the spirit and principle of the invention shall be included in the protection scope 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 structure containing the glass fiber reinforced material into the mold flow software for injection molding analysis, obtain the distribution of the fibers in the structure, and export the grid 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, select the matrix material and fiber material corresponding to the glass fiber reinforced material in step 1 in the EngineeringData of the module, and set the corresponding parameters. After modeling is completed, link the Material Designer to the EngineeringData of the Static Structural module 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 in the Static Structural module created in step 2, select the material for the geometric model described in step 2, and specify the corresponding fiber orientation distribution field. Set the load and boundary conditions and then solve. Export the deformation results as 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: The step three is implemented by the following sub-steps: (3.1) Create a new Material Designer module in ANSYS Workbench and open EngineeringData; (3.2) Select the matrix material and fiber material corresponding to the glass fiber reinforced material described in step 1 in Engineering Data Source; (3.3) Enter the Material Designer module and select Analytical Model in 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, and check Compute Coefficient of Thermal Expansion and Compute Thermal Conductivity in Setting 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 to 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 the Engineering Data to see the basic data of the glass fiber reinforced material.

3. The linear expansion coefficient prediction method of 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 as 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, select the corresponding geometry and the material field to be imported in the details, right-click the corresponding material field, select Import Material Field, and 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, set the direction of the movement suppression to 0; click Analysis Settings, turn on Weak Springs in the details to prevent the geometry from being under-constrained and causing solution problems, and do not limit 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