Static Analysis of Plastic Clip

Transcription

1 Static Analysis of Plastic Clip Zpracoval: Petr Žabka Jaroslav Beran Pracoviště: Katedra textilních a jednoúčelových strojů TUL

2 In-TECH 2, označuje společný projekt Technické univerzity v Liberci a jejích partnerů - Škoda Auto a.s. a Denso Manufacturing Czech s.r.o. Cílem projektu, který je v rámci Operačního programu Vzdělávání pro konkurenceschopnost (OP VK) financován prostřednictvím MŠMT z Evropského sociálního fondu (ESF) a ze státního rozpočtu ČR, je inovace studijního programu ve smyslu progresivních metod řízení inovačního procesu se zaměřením na rozvoj tvůrčího potenciálu studentů. Tento projekt je nutné realizovat zejména proto, že na trhu dochází ke zrychlování inovačního cyklu a zkvalitnění jeho výstupů. ČR nemůže na tyto změny reagovat bez osvojení nejnovějších inženýrských metod v oblasti inovativního a kreativního konstrukčního řešení strojírenských výrobků. Majoritní cílovou skupinou jsou studenti oborů Inovační inženýrství a Konstrukce strojů a zařízení. Cíle budou dosaženy inovací VŠ přednášek a seminářů, vytvořením nových učebních pomůcek a realizací studentských projektů podporovaných experty z partnerských průmyslových podniků. Délka projektu:

3 Abstract In recent years, safety of parts of automobiles have become of great concern to consumers and the general public. In light of this, this research study seeks to determine the deformation and the stress caused by a force of 300N acting on two different clips used in vehicles. Finite Element Analysis (FEA) is used in this study. The 3D models of each clip is designed in Pro/Engineer and then static analysis is ran on each clip to obtain the displacement, Von Mises Stress, Maximum Principal stress and the contact pressures on these clips. The results show that the model stress on each model is relatively lower than the yield stress of the material used for each clip. That notwithstanding, certain places on each clip had relatively high stress. The aim of the study is to analyze possibilities of optimization of the clips in order to reduce the stress at these critical places. Introduction This study deals with the design of 3D models of two clips and the Finite Element Analysis of the models using Pro Engineer. The research study seeks to find the deformation of the two clips and the stress cause by a force of 300 N acting on each clip. This chapter presents the introduction of the subject matter. This includes the introduction, why the use of the finite element method and Pro Engineer and the description of the clips. Finite Element Method In the field of Engineering Design, we are usually challenged with complex problems whose mathematical formulation are tedious and often than not impossible to be solved by analytical methods. Therefore, we resort to numerical techniques. The Finite Element Method (FEM), its practical application often known as Finite Element Analysis (FEA), is a numerical technique for finding approximate solutions of partial differential equations (PDE) as well as of integral equations. This has proven to be powerful tool for getting the numerical solution of a wide range of engineering problems. There are numbers of CAD software for FEA. Their difference usually lies the type of variable order used by their solvers, thus whether H-Element (the original and classic element) or P- Element (the p is for polynomial). The most basic issues relate to accuracy and speed. Unlike the H- Element method that requires users to vary meshing parameters to obtain desired accuracy, the P- Element method uses a constant mesh (usually coarser than an H-Element mesh). The P-Element method then uses a variable polynomial level to obtain the results (such as displacements, stresses or strains) to achieve a user-specified accuracy. In this case Mechanica (an application in Pro/Engineer CAD software) is used for the FEA of the two clips. Mechanica uses the P-Element method.

4 Descriptions of the two clips Figure 1.1 Model of Clip1 Figure 1.2 Model of Clip2 The model of clip 1 is shown in figure 1.1 and clip 2 can be seen in figure 1.2. These two clips have a lot in common. Each is used for holding a tube and the red oval part shown, are positions for holes where screws will be put through in order to assemble the clip to the car body. They are made of the same material and their front- ends for holding the tube have the same dimensions. But Clip 1 is twice as wide as Clip 2 at the back-end. Also Clip 1 has rib features for extra support. In order to get better identification of parts or surfaces on each model been talked about, the labels shown in figure 1.3 will be used when the need arises. These labels apply to both clips respectively. Part A Part B Surface A Part C Contact surface B Contact surfaces A

5 Surface B Surface C Surface D Surface F Figure 1.3 Labels of parts and surfaces of clip The design of each clip is provided and based on its dimensions 3D models of its parts are created and assembled into one component in Pro/Engineer standard module. In the original designs given, the edges of Contact surfaces A are not rounded. But these edges are rounded in the 3D models for the FEA. This is done in order to get stress results comparable to real life situation. And also since the clips are made from plastic, in plastic moulding edges are rounded to various radii. In this case, a radius of 0.1mm is used for the edges of Contact surface A. A 3D model of a tube of outer diameter 8.4mm, thickness 2mm and length 30mm is used for the contact analysis. The tube and labels of its surfaces is shown in figure 1.4. Surface G Figure 1.4 Labels of Tube Surface H (This applies to the opposite end too)

6 Defining of analyses (Pre-processing) The 3D Models are brought to Mechanica module where they are meshed, loaded and the boundary conditions applied appropriately. Three different static analyses are done on each model. Analysis A: Analysis B: Analysis C: Static analysis on the bonded clip without the tube. Static analysis on the clip taken into account contact interfaces between the tube and the Contact surfaces A on Part B. Static analysis on the clip into account contact Analysis B and the contact interface between Part C and Contact surface B on Part B. Therefore the major difference between each of the static analyses is the contact interfaces considered. Coordinate system All loads and constraints to both clips are applied using the coordinate system shown in figure 2.1. The Z-axis is vertical and the Y-axis is perpendicular to Surface D. Z X Y Figure 2.1 Coordinate system Material Assignment The materials used are STEEL of standard properties and POLYAMID 66 of the following properties; density-1.14e-9 tonnes/mm3, Poisson's ratio-04 and Young's Modulus 3000MPA. Which material goes with which part is listed in table 2.1.

7 Table 2.1 Material Assignment PART MATERIAL ASSIGNED Part A STEEL Part B POLYAMID 66 Part C POLYAMID 66 Tube STEEL Boundary conditions The boundary conditions describe fixation to the frame in a way similar to the real fixation. The setting is shown in table 2.2 and in figure 2.2. Table 2.2 Boundary Conditions Surface B, Surface C Surface F Surface D Surface H X Fix Fix Y Fix Fix Z Fix Figure 2.2 Boundary Conditions for Analyses Load Application For Analysis A, a force of 300N is applied on Surface A in the negative Z-direction as shown in figure 2.3. For Analysis B and Analysis C, a force of 300N is applied in the negative Z-direction on two equal surface regions on top of the tube as shown in figure 2.4.

8 Figure 2.3 Load Applications for Analysis A Figure 2.4 Load Applications for Analysis B and Analysis C Contact interfaces Figure 2.5 Contact interfaces for Analysis B Figure 2.6 Contact interface for Analysis C

9 Mesh The mesh of the each clip for the FEA is automatically generated by the Pro/Mechanica. But in order to get better stress results at certain places like the Contact Surface A and its edges, the maximum element size at these places should be redefined. The figure 2.7 shows these places and the values set. Figure 2.7 Mesh refinement Results and Discussion (Post-Processing) In this chapter, the results obtain from the static analyses on the two clips are represented and discussed. In the discussion, stresses on places on the clip that are of importance are brought to notice. Results of Displacement Results of displacement from all analyses are displayed in figures 3.1 to 3.6. The results show that the simplified Analysis A returns significantly lower displacement values. Therefore its results should be treated as unreliable. It must be noted that the displacement values obtained is for the worse situation. In the reality there will be a gap between contact surfaces of Part B and Part C. Therefore Part C will experience little or no stress.

10 Figure 3.1 Results of displacement of Clip 1 Analysis A Figure 3.2 Results of displacement of Clip 1 Analysis B Figure 3.3 Results of displacement of Clip 1 Analysis C

11 Figure 3.4 Results of displacement of Clip 2 Analysis A Figure 3.5 Results of displacement of Clip 2 Analysis B Figure 3.6 Results of displacement of Clip 2 Analysis C

12 Results of Stresses The pictorial views of the Von Mises Stress on each clip are shown in figures 3.7 to Von Mises Stress refers to a theory called the "Von Mises - Hencky criterion for ductile failure". For an elastic body that is subject to a system of loads in 3 dimensions, Principal Stresses acting in the x, y, and z directions are calculated at any point on the body. The Von Mises criteria is a formula for combining these three(3) stresses into an equivalent stress, which is then compared to the yield stress of the material. The yield stress is a known property of the material, and is usually considered to be the failure stress. In our case the yield stress is 85 MPa. According to Maximum Principal Stress theory, a material will fail when one of the principal stresses exceeds the yield strength in tension. It's good for brittle materials (like cast iron), but not ductile ones (like aluminium). Figure 3.7 Von Mises Stress - Clip 1 - Analysis B Figure 3.8 Von Mises Stress - Clip 2 - Analysis B

13 The analyses revealed several potentially hazardous places. The two most critical places are shown in figure 3.9 and These places are identified as Place 1 and Place 2. From the results, the stresses on Clip 1 around place 1 are relatively lower than that on Clip 2. This can be associated with the advantages of the rib features of Clip 1. But since both clips have stress values at this place relatively lower than the yield stress, the place is in good condition for both clips. Figure 3.9 Critical Place #1 Figure 3.10 Critical Place #2 Results of Contact Pressure The result of contact pressure for the Clip 2 is shown in figure Although the contact pressure exceeds the yield stress in narrow areas, it is not very significant issue, as the pressure will drop significantly with even small plastic deformation.

14 Figure 3.11 Results of contact pressure on Clip 2 Analysis B