Deep Beam With Web Opening Name: Path: Keywords: DeepBeamWithWebOpening/deepbeam /Examples//DeepBeamWithWebOpening/deepbeam analys: linear static. constr: suppor. elemen: cq16m ct12m pstres. load: force node. materi: elasti isotro. option: direct units. post: binary ndiana. pre: dianai. result: cauchy displa extern force green reacti strain stress total.
Outline 1 Description 2 Finite Element Model 2.1 Units 2.2 Geometry definition 2.3 Boundary conditions 2.3.1 Constraints 2.3.2 Vertical load 2.4 Properties 2.5 Meshing 3 Structural linear static analysis 3.1 Analysis commands 4 Results 4.1 Reaction forces FBY 4.2 Contour plot Total displacements DtXYZ 4.3 Contour plot Stress field SXX 4.4 Contour plot Stress field SYY 4.5 Contour plot Stress field SXY 4.6 In-plane principal components Stress field SXX 4.7 Diagram Stress field SXX 4.8 Diagram Stress fields SYY and SXY 0 http://dianafea.com 2/27
1 Description We analyze a concrete continuous deep beam with web openings presented in (Ashour and Rishi) 1 and here shown in [Fig. 1]. The beam is 3 meters long, 625 mm height and 120 mm thick. The web opening is of 250 x 250 mm. Due to symmetry we model one half of the beam. Supports and loading plate are made of steel. The material properties are listed in [Table 1]. P Concrete Steel Young s modulus Poisson s ratio 25000 0.2 210000 0.2 N/mm 2 Table 1: Concrete and steel properties. 625 187.5 250 The nodal force P is equal to 4e+05 N. 250 We will study the elastic response of the beam by performing a linear elastic static analysis. y z x 137.5 100 120 500 200 500 80 1500 Figure 1: Schematic representation of the model (units are in millimeters). 1 A. F. Ashour and G. Rishi, Tests of Reinforced Concrete Continuous Deep Beams with Web Openings, ACI Structural Journal, 2000. 1 http://dianafea.com 3/27
2 Finite Element Model For the modeling session we start a new project for structural analysis [Fig. 2]. The dimensions of the domain for the 2D model are set equal to 10 m. We will use quadratic quadrilateral finite elements. Main menu File New [Fig. 2] Figure 2: New project dialog 2.0.0.0 http://dianafea.com 4/27
2.1 Units We choose millimeter for the unit Length, ton for Mass, Newton for Force. Geometry browser Reference system Units [Fig. 3] Property Panel [Fig. 4] Figure 3: Geometry browser Figure 4: Property Panel - Units 2.1.0.0 http://dianafea.com 5/27
2.2 Geometry definition We create a sheet for the beam. We will change the viewpoint to a top view, fit the shape in the Workspace window and hide the working plane. Main Menu Geometry Create Add polygon sheet [Fig. 5] Viewer Hide workingplane Viewer Viewpoints Top View Viewer Fit all [Fig. 6] Figure 5: Add Beam polygon sheet Figure 6: Top view of the Beam 2.2.0.0 http://dianafea.com 6/27
Similarly, we create a sheet for the left and right supports and the loading block. For the left support an additional vertex is created at (160, -40, 0) mm to account for the constrain we will apply along the Y -direction. Similary, we add a vertex at (820, 665, 0) mm to the loading bloack where to apply the nodal vertical force. Main Menu Geometry Create Add polygon sheet (3X) [Fig. 7] [Fig. 8] [Fig. 9] Viewer Fit all [Fig. 10] Figure 7: Add Left support polygon sheet Figure 8: Add right support polygon sheet Figure 9: Add Loading block polygon sheet Figure 10: Top view of the model 2.2.0.0 http://dianafea.com 7/27
We create a sheet for the web opening. Main Menu Geometry Create Add polygon sheet [Fig. 11] Figure 11: Add Opening polygon sheet Figure 12: Top view of the model 2.2.0.0 http://dianafea.com 8/27
We subtract the sheet Opening from the sheet Beam. Main Menu Geometry Modify Subtract shapes [Fig. 13] Figure 13: Subtract shapes Figure 14: Top view of the model 2.2.0.0 http://dianafea.com 9/27
2.3 Boundary conditions 2.3.1 Constraints We support the right edge (i.e., the centerline) of the beam in X-direction to get the symmetry condition. Main Menu Geometry Analysis Attach support [Fig. 15] [Fig. 16] Figure 15: Apply symmetry boundary conditions Figure 16: Symmetry boundary conditions 2.3.1.0 http://dianafea.com 10/27
We support the center of both support blocks in Y -direction. Due to the symmetry boundary condition (the center bottom point of the Right support has already been supported in X-direction), we now have a roller under the center of the left support and we pinned the center of the right support. Main Menu Geometry Analysis Attach support [Fig. 17] [Fig. 18] Figure 17: Apply vertical (Y -direction) boundary conditions Figure 18: Vertical (Y -direction) boundary conditions 2.3.1.0 http://dianafea.com 11/27
2.3.2 Vertical load We apply a nodal force of -4e+05 N to the center of the loading block. Main menu Geometry Analysis Attach load [Fig. 19] [Fig. 20] Figure 19: Apply vertical nodal force Figure 20: Vertical nodal force 2.3.2.0 http://dianafea.com 12/27
2.4 Properties We assign the element class and the material and geometrical properties to the beam. We use regular plane stress finite elements. The material is linear elastic. Regarding the geometry, we need to specify the thickness of the beam (120 mm). Main Menu Geometry Analysis Property assignments [Fig. 21] Property assignments Add new material [Fig. 22] [Fig. 23] Property assignments Add new geometry [Fig. 24] Figure 23: Material properties Figure 21: Property assignments Figure 22: Add new material Figure 24: Geometrical properties 2.4.0.0 http://dianafea.com 13/27
We assign the element class and the material and geometrical properties also to the supports and the loading block. We also use regular plane stress finite elements. The material is linear elastic. The thickness is equal to that of the beam (120 mm), thus we do not need to specify a new Geometry set. Main Menu Geometry Analysis Property assignments [Fig. 25] Property assignments Add new material [Fig. 26] [Fig. 27] Figure 25: Property assignments Figure 26: Add new material Figure 27: Material properties 2.4.0.0 http://dianafea.com 14/27
2.5 Meshing We set the mesh properties with an element size of 50 mm and we generate the mesh. Main Menu Geometry Analysis Set mesh properties [Fig. 28] Main Menu Geometry Analysis Generate mesh [Fig. 29] Figure 28: Mesh properties Figure 29: Finite element mesh 2.5.0.0 http://dianafea.com 15/27
3 Structural linear static analysis 3.1 Analysis commands We will perform a linear structural analysis. Main Menu Analysis New Analysis Analysis browser Right click ( ) Analysis1 Rename Linsta [Fig. 30] Analysis browser Right click ( ) LinSta Add command Structural linear static [Fig. 31] [Fig. 32] Main Menu Analysis Run Analysis Figure 30: Analysis window Figure 31: Add command Figure 32: Analysis tree 3.1.0.0 http://dianafea.com 16/27
4 Results 4.1 Reaction forces FBY To validate the results we check that the reaction forces are in equilibrium with the applied load. Since the load has only vertical component, we check only the reaction forces along the Y -axis (FBY). Results browser Output Nodal results Reaction Forces FBY Right click ( ) Show table [Fig. 33] [Fig. 34] Figure 33: Output browser - show table Figure 34: Nodal reaction forces FBY The summation of all nodal reaction forces along the Y -axis is equal to 400 kn, in equilibrium with the total applied load P = 400 kn. 4.1.0.0 http://dianafea.com 17/27
4.2 Contour plot Total displacements DtXYZ We make a contour plot of the total displacements DtXYZ [Fig. 36]. Results browser Output Nodal results Total Displacements DtXYZ [Fig. 35] [Fig. 36] Figure 35: Output browser Figure 36: Total displacement (DtXYZ) As expected, the highest total displacements DtXYZ are located near the applied nodal force and in the proximity of the opening [Fig. 36]. 4.2.0.0 http://dianafea.com 18/27
In order to have a smooth contour plot, we choose a continuous color scale [Fig. 38]. Property panel Result view settings Contour plot settings [Fig. 37] [Fig. 38] Figure 37: Output settings Figure 38: Total displacement (DtXYZ) 4.2.0.0 http://dianafea.com 19/27
4.3 Contour plot Stress field SXX We create a contour plot for the stress SXX [Fig. 42]. We only display the Element set Beam. We change the colorscale to specified values with minimum value equal to -12 N/mm 2 and maximum value 4 N/mm 2 (this provides a better understanding of the stress field in the beam). Mesh browser Element sets Beam Right click ( ) Show only [Fig. 39] Result browser Output linear static results Element results Cauchy Total Stresses SXX [Fig. 40] Property panel Result view settings Contour plot settings [Fig. 41] Figure 39: Show only Beam Figure 40: Output browser Figure 41: Output settings 4.3.0.0 http://dianafea.com 20/27
Figure 42: Stress field SXX Due to the bending of the beam, the stress component SXX takes the highest values (in tension) at the bottom part of the beam between the two supports and at the top-right (the center of the full beam). High values of SXX are also noticed at the bottom-left and top-right corner of the opening. On the contrary, negative values (compression) of SXX are observed at the other two corners. 4.3.0.0 http://dianafea.com 21/27
4.4 Contour plot Stress field SYY We create a contour plot for the stress SYY [Fig. 44]. Result browser Output linear static results Element results Cauchy Total Stresses SYY [Fig. 43] Figure 43: Output browser Figure 44: Stress field SYY The highest absolute values of SYY are located close to the supports and the loading block. Highest concentration of stresses are also noticeable at the opening s corners as observed for the case of SXX. 4.4.0.0 http://dianafea.com 22/27
4.5 Contour plot Stress field SXY We create a contour plot for the stress SXY [Fig. 47]. The colorscale limits are changed to the minimum and maximum values of SXY that correspond to -4 N/mm 2 and 4 N/mm 2, respectively. Result browser Output linear static results Element results Cauchy Total Stresses SXY [Fig. 45] Property panel Result view settings Contour plot settings [Fig. 46] [Fig. 47] Figure 45: Output browser Figure 46: Output settings Figure 47: Stress field SXY The contour plot shows that the highest absolute values of SXY are in two regions with an inclination of 45 starting from the loading block. It is interesting to observe how the stresses redistribute around the opening. 4.5.0.0 http://dianafea.com 23/27
4.6 In-plane principal components Stress field SXX We create a vector plot of the in-plane principal components of the SXX stresses. Result browser Output linear static results Element results Cauchy Total Stresses Right click ( ) SXX [Fig. 48] [Fig. 49] Figure 48: Output browser Figure 49: In-plane components of SXX 4.6.0.0 http://dianafea.com 24/27
4.7 Diagram Stress field SXX We create diagrams of the stress field along a vertical cut at X = 1050 mm (450 mm from the symmetry line). Therefore, we create a probe-curve. Property panel Result view settings Probing curve setting Add Curve [Fig. 50] Property panel Result view settings Probing curve setting probe-curve Number of intervals between points 20 [Fig. 51] Property panel Result view settings Probing curve setting probe-curve add Point coordinates [Fig. 52] Property panel Result view settings Probing curve setting probe-curve Point coordinates [Fig. 53] Figure 50: Add curve Figure 51: Rename curve and interval number Figure 52: Add coordinates Figure 53: Point coordinates 4.7.0.0 http://dianafea.com 25/27
We now create a diagram of SXX along the vertical cut at X = 1050 mm [Fig. 55]. Results browser Output Element results Cauchy Total Stresses Right click ( ) SXX Show contour probe [Fig. 54] [Fig. 55] Figure 54: Show contour probe Figure 55: Stress SXX along the cut at X = 1050 mm The diagram clearly shows that at the bottom of the beam we have positive stresses (tension) that become negative (compression) while moving toward the top. Nevertheless, close to the top surface (near the loading plate) the stress becomes again positive. 4.7.0.0 http://dianafea.com 26/27
4.8 Diagram Stress fields SYY and SXY Similarly, we create a diagram of SYY and SXY along the vertical cut at x = 1050 mm [Fig. 56] [Fig. 57]. Results browser Output Element results Cauchy Total Stresses SYY [Fig. 56] Results browser Output Element results Cauchy Total Stresses SXY [Fig. 57] Figure 56: Stress SYY along the cut at X = 1050 mm Figure 57: Stress SXY along the cut at X = 1050 mm 4.8.0.0 http://dianafea.com 27/27