Finite Element Model for Axial Stiffness of Metal-Plate-Connected Tension Splice Wood Truss Joint

Size: px

Start display at page:

Download "Finite Element Model for Axial Stiffness of Metal-Plate-Connected Tension Splice Wood Truss Joint"

Edward Robbins
5 years ago
Views:

1 Finite Element Model for Axial Stiffness of Metal-Plate-Connected Tension Splice Wood Truss Joint Jose M. Cabrero Assistant Professor University of Navarra, Department of Structural Analysis and Design, School of Architecture Navarra, Spain Kifle G. Gebremedhin Professor Department of Biological and Environmental Engineering, Cornell University Ithaca, NY, 14853, U.S.A. Abstract A finite element model that predicts stiffness for metal-plate-connected (MPC) tension splice joint of wood trusses is developed. The commercial software ABAQUS was used in developing the model. The model is two-dimensional, and the properties of the wood and metal plate are assumed to be linearly isotropic. Contacts between wood and teeth of the metal plate are modeled with finite sliding formulation. The contact elements model the slip behavior that occurs at the wood-tooth interface. The tangential contact properties are set to a specified coefficient of friction while the normal contact properties are set to a hard contact formulation, allowing for a possible separation of the nodes after contact is achieved. Contact elements represent the stiffness of the interface, and stiffness is lost once the contact elements are disengaged due to tooth withdrawal. Model predictions are validated against experimentally measured stiffness values obtained in the literature. The data covers two wood species and three levels of modulus of elasticity (MOE). The model predicts within 5 percent of the experimentally measured stiffness values. 1. Introduction Conventional methods of design of metal-plate connected (MPC) wood truss joints assume that connections between the metal-plate connector and wood are either pinned or rigid. In reality, these joints exhibit a semi- rigid behavior, i.e., not purely pinned or rigid but somewhere in-between [1,2,3]. Therefore, the challenge is to determine the stiffness of these joints so that their semi rigidity could be accounted for in design of MPC wood trusses. Modeling the behaviour of the connector in the truss member is complicated by the composite nature of the metal and wood and the configuration of the system (a row of teeth embedded in wood and a gap existing between the wood elements). The metal plate connection is the lease understood in truss design. The simplified approach of truss design is to assume truss joints to be pin connected, which means no moment is transferred between adjacent members. This assumption violates the continuity of chord members at the joints. To account for the indeterminacy of a truss when analyzed as pin-joined approximations, the Truss Plate Institute (TPI) has provided empirically-based Q-factors to modify the bending moment or the buckling length of truss members [4]. The Q-factors were developed based upon many years of experience of design and extensive simulated investigation of wood trusses of standard configurations using the Purdue Plane Structures Analyzer (PPSA) [5]. The PPSA is a matrix method of structural analysis that determines the axial forces and bending moments of truss-frame models. The

2 tabulated Q-factors provided by TPI do not cover all ranges and combinations of loading conditions, spans, and geometry. Therefore, theoretical models that provide realistic treatment of joints are needed so that forces and moments can be predicted with greater accuracy. Because of the wide application of MPC wood trusses in commercial, industrial, residential and agricultural buildings, even a reasonably small improvement in characterization of truss joints may result in significant cost savings. The main focus of this research is to develop a finite element model for the wood-tooth interface of MPC tension-splice joint based on fundamental principles of contact mechanics that, apart from basic material properties, does not require empirical corrections. Linear elastic finite elements represent the metal plate, teeth, and wood; and contact elements are virtual (imaginary) spring elements that transfer compressive and frictional forces between the wood and the teeth of the metal plate as the joint is externally loaded. The commercial software package ABQUS is used to develop the contact elements. Modeling the interface using contact elements can have wide engineering applications such as in modeling the bondage between steel and concrete in reinforced concrete structures, the transfer of frictional forces between piles and soil in pile foundations, and modeling rotational stiffness of MPC wood joints. 1.1 Objectives The specific objectives of this study were: 1. To develop a finite element model for the wood-tooth interface of metal-plate connected tension-splice joint of wood trusses using linear contact elements. 2. To predict the stiffness of a tension-splice joint. 3. To validate the predicted stiffness against measured values. 2. Literature Review A thorough literature review of experimental and theoretical studies conducted on MPC wood-truss joints are reported in Amanuel et al. [1]. The reader is referred to that study for extensive literatura review. 3. Model Formulation A bi-dimensional finite element (FE) model that predicts stiffness of MPC tension-splice joints is developed using the ABAQUS software. 3.1 Assumptions 1. Since the main deformation arises from the axial force in the x-direction, the deformation along the z-direction (perpendicular to the direction of the axial force) is assumed to be zero. Because of this assumption, the model is reduced to a plane strain model. 2. The behavior of the joint is governed by teeth-wood contacts and the resulting deformation of the teeth.

3. The stress distribution in the connection is rather complex because of plate geometry and nonlinearity of the behavior of the wood-tooth interface.

Modulus of elasticity for steel is assumed to be 203,000 N/mm 2 and Poisson ss ratio is 0.3. These material properties correspond to those reported by Riley and Gebremedhin [6]. 5.

3 3. The stress distribution in the connection is rather complex because of plate geometry and nonlinearity of the behavior of the wood-tooth interface. In this study, force distribution in each row of teeth is assumed to be the same. 4. Both wood and steel are modeled as elastic materials. Isotropic behavior is assumed for both materials. Modulus of elasticity for steel is assumed to be 203,000 N/mm 2 and Poisson ss ratio is 0.3. These material properties correspond to those reported by Riley and Gebremedhin [6]. 5. Even though wood is an orthotropic material, an isotropic formulation is adequate for this model because the joint is modeled as a plane strain model. Poisson' 's ratio of wood is assumed to be 0. 4 and MOE values used are the same values obtained experimentally by Riley and Gebremedhin [6]. 3.2 Boundary Conditions Since both sides of the member are symmetrical, only one side of the member is modeled. Because of symmetry, rollers are defined at the bottom of the wood to allow movement in the x-direction (direction of the axial load). The metal plate is fixed along its left edge, which corresponds to the centerline of the plate. All displacements are restricted along the centerline. In the y-direction, displacement restriction was imposed to avoid rigid-body motion. 3.3 Load Application Axial tension force was applied at the free end of the member, and is applied as a uniform pressure. In order to provide uniform load distribution and avoid local stress concentration, the load was applied 50 mm away from the last row of teeth. 3.4 Geometrical Model Wood lumber species used in this study weree 2 x 4 Spruce-Pine-Fir and Southern Yellow Pine. The actual size of the lumber was 38-mm thick and 89-mm wide. Plates were 20 gages, and weree 76.2 mm by 102 mm in size. Thesee are the same species, dimensions and gage thatt were used in the experimental study of Riley and Gebremedhin [6]. A representation of the actual geometry of the metal plate is shown in Figure 1. (a) (b )

4 (c) Figure 1. (a and b) Axial joint considered in this study and tested by Riley and Gebremedhin [6] and (c) geometry and teeth layout of the metal plate. Some simplifications were made in modeling the geometry of the plate. The slots created because of punched teeth were not considered in modeling. The teeth are twisted and tapered toward the end but are modeled as flat rectangular surfaces having a thickness equal to the nominal thickness of the plate. Because of symmetry, one-fourth of the joint is used as the computational domain for the model (Figure 1c). The hole in the wood is 0.01 mmm smaller than the thickness of the tooth. This would allow good initial contact between the wood and the plate. From the start, good contactt is established by relocating the nodes on the wood (initially inside the steel) to the metal-plate surface. This is accomplished inside the software. 3.5 Element Used in the Model The element used in the model is CPE3 available in the ABAQUS library [7]. The element adapted for the plane strain model is solid continuum 3-node triangular element. Each node has two degrees of freedom translation in the x and y directions. Because of its triangular shape, it is less sensitive to geometrical distortions, which could potentially happen to the teeth due to bending. The mean size of the element is fixed at 0.5 mm. This size assures, at least, two layers of elements for the teeth in bending. The same mesh density was used for both parts of the joint (wood and steel). The resulting mesh is shown in Figure 2. (a) (b) Figure 2. Finite element model, (a) meshed metal plate, (b) meshed wood member.

5 3.6 Contact Load transfer between teeth and wood occurs at the contact interfaces. Contact interface is defined by two surfaces, one for the wood and the other for the metal plate. The required contact elements are internally defined by the software. ABAQUS requires that one of the surfaces to be defined as master and the other surface as slave. The specification of the surfaces is critical because of the way the surface interactions are discretized. For each node on the slave surface, ABAQUS attempts to find the closest point on the master surface of the contact pair where the normal of the master surface passes through the node on the slave surface. The interaction is then discretized between the point on the master surface and the slave node. In the model, the surface corresponding to the metal plate is defined as master, and the wood is defined as the slave (see Figure 3 for definition of contact surfaces). Figure 3. Definition for contact surfaces. A hard contact formulation is employed for the properties of the contact elements. This relationship minimizes the penetration of slave nodes into the master surface and does not allow transfer of tensile stress across the interface. The classical Lagrange multiplier method was applied to enforce no penetration between the surfaces. When the surfaces are in contact, any contact pressure can be transmitted between them. When the contact pressure reduces to zero, the surfaces separate. Once contact is achieved, the related nodes are allowed to separate again. In addition to pressing on the wood, the teeth may also slip and transmit tangential forces. A basic isotropic Coulomb friction model with a coefficient of friction equal to 0.5 was used. In this model, for the sake of simplicity, the same static and kinetic friction coefficients were assumed. No shear limit is indicated, therefore, any tangential force could be transferred. A finite sliding model formulation is applied. This formulation allows the defined contact surfaces to separate and slide with finite amplitude and arbitrary rotation. As mentioned previously, the hole in the wood is made a little bit smaller (by 0.01 mm) than the thickness of the idealized tooth. This assures an initial contact between wood and tooth. The initial contact is adjusted automatically by the finite element program by moving the over passing nodes to the exact contact position. This technique assures the necessary initial contact. 4. Results and Discussion The predicted results were compared against test results of Riley and Gebremedhin [6]. The test results were based on two wood species (Southern Yellow Pine and Spruce Pine Fir). Riley and Gebremedhin [6] experimentally obtained the modulus of elasticity of these species

6 and reported: 8.49 MPa for Spruce Pine Fir, and and MPa for Southern Yellow Pine. The same values were used in the model herein. The displacement of the joint was calculated at two locations. These two locations are identifiedd by the two nodes shown in Figure 4. Node N A is located along the axis of symmetryy below the last tooth, and the second node (N B ) is located at the tip end of the last tooth. Figure 4. Model definition and node locations wheree stiffness values were calculated. The predicted node displacement ( Δ h ) is equal to one-half the displacement of the joint. The corresponding force ( F h ) is equal to the reaction force at the node. The effectivee stiffness is, therefore, calculated by dividing F h by Δ h. The predictedd and measured [6] stiffness values are compared in Table 1. Table 1. Measured and predictedd stiffness values for metal-plate connected tension splice wood truss joint. The values in the parenthesis are the percent difference from the measured values. Lumber Species Spruce Pine Fur Southern Yellow Pine Southern Yellow Pine From [6] Wood MOE (MPa) 8.49 Measured stiffness 1 (kn/mm) Predicted stiffness at specified nodes (kn/mm) N A (+4%) (-0.4%) (+2%) N B (-9%) 26.7 (-10%) (-7%) The calculated stiffness values for the two nodes ( N A and N B ) are reasonably close to the measured stiffness values. The stiffness at Node N A is within 2% difference and that of N B is within 8. 7% difference of the measured values. The location of Node N A accounts for deformation due to bending of all teeth, axial extension of the plate, and deformation of the wood. The other node location, however, does not take all these components into account. The load-displacement relationships for the three MOE values are given in Figure 5. The relationship is almost linear. The plots show that good contact between wood and teeth of the metal plate was established from the very beginning.

7 Figure 5. Load-displacement curves for three MOE values of the tension-splice joint. The calculated stress distributions in the wood and metal plate are shown in Figures 6 and 7, respectively. As the row of teeth approaches the joint gap, the magnitude of the stress decreases. The teeth closest to the gap are thus least loaded. That is why the predicted displacement at this location (N A A) was not accurately predicted. A diagonal stress field is formed in the wood between teeth holes when there are two adjacent rows of teeth. This non- uniform distribution of stress in the teeth does not invalidate the assumption made in formulation of the model. The model only assumed that the force distribution in each row of teeth to be the same. Figure 6. Stress distribution in the wood for MOE = MPa (scale of the deformed shape = 50).

8 Figure 7. Stress distribution in the metal plate for MOE =15.17 MPa (scale of the deformedd shape = 50). 5. Conclusionss A simple and accurate finite element model that predicts stiffness values for metal-plate connected tension-splice joints of wood trusses was developed using the ABAQUS commercial computer software. The model is bi-dimensional and accounts for good contact of the interface of wood and tooth of the metal plate connector. The predicted stiffness values were compared against experimentally measured values and compare within 5 percent. 6. References [1] Amanuel S., Gebremedhin K.G., Boedo S., and Abel J.F., Modeling the interface of metal-plate-connected tension-splice joint by finite element method, Trans. of ASAE, 43(5), 200, pp [2] Gupta R., and Gebremedhin K.G. Destructive testing of metal-plate-connected wood truss joints, Journal of Structural Engineering 116, 1990, pp [3] Riley G.J., Gebremedhin K.G., and White R.N. Semi-rigid analysis of metal plateconnected Wood trusses using fictitious members, Trans. of ASAE 36(3) ), 1993, pp [4] Truss Plate Institute, Inc. (TPI), National design standard for metal-plate-connected wood truss construction, ANSI/TPI Truss Plate Institute, Madison, Wisconsin. [5] Purdue Research Foundation, Purdue Plane Structures Analyzer, 1993, Departmentt of Forestry and Natural Resources, Purdue University. [6] Riley G.J., and Gebremedhin K.G. Axial and rotational stiffness model of metalplate connected Wood truss joints, Trans. of ASAE 42(3), 1999, pp [7] ABAQUS. Version 6.5. Html documentation.

Modelling Flat Spring Performance Using FEA

Modelling Flat Spring Performance Using FEA Blessing O Fatola, Patrick Keogh and Ben Hicks Department of Mechanical Engineering, University of Corresponding author bf223@bath.ac.uk Abstract. This paper