Reinforced concrete beam under static load: simulation of an experimental test

Transcription

1 Reinforced concrete beam under static load: simulation of an experimental test analys: nonlin physic. constr: suppor. elemen: bar cl12i cl3cm compos cq16m interf pstres reinfo struct. load: deform weight. materi: crack elasti expone harden isotro multil parabo plasti rotati soften strain totstr vonmis. option: arclen direct groups linese newton normal regula select units update. result: cauchy crack crkwdt displa force green moment princi reacti strain stress total.

2 Outline 1 Description 2 Finite Element Model 2.1 Units 2.2 Geometry Definition 2.3 Properties Concrete beam Steel plates Interfaces Reinforcement Composed line element 2.4 Boundary Conditions 2.5 Loads 2.6 Meshing 3 Nonlinear Static Analysis 3.1 Analysis Commands 3.2 Results Displacements Crack widths Principal stresses Longitudinal reinforcement Transversal reinforcement Composed elements: shear forces and bending moments RC beam: simulation of an experimental test 2/68

3 1 Description This example presents a numerical simulation of an experimental test on a reinforced concrete (RC) beam under increasing static load until failure. The example is test VS-C3 from the series of experiments carried out in the University of Toronto by Vecchio and Shim (2004) 1. These series of tests were a reproduction of the experiments made by Bresler and Scordelis (1963) 2, which are classical benchmarks extensively used for validation of numerical models for concrete structures. The beam has a total length of m, a depth of m, and a width of m. The geometry, reinforcement, loading, boundary conditions and experimental setup are presented in [Fig. 1]. The bottom longitudinal reinforcement is extended outside the beam and welded to thick plates. The beam exhibited a flexural-compressive failure mode [Fig. 2]. The measured peak load was P exp = 265 kn at a deflection of 44.3 mm. Figure 1: Characteristics of the Toronto beam test VS-C3 [1] Figure 2: Toronto beam test VS-C3 at ultimate load [1] 1 Vecchio F. J. and Shim W. (2004). Experimental and analytical reexaminations of classic concrete beam tests, Journal of Structural Engineering 130(3): Bresler B. and Scordelis A. C. (1963). Shear strength of reinforced concrete beams, Journal American Concrete Institute, 60(1): RC beam: simulation of an experimental test 3/68

4 This experimental test was also simulated in Belletti et al. (2016) 3, being a reference for the finite element model presented here. The finite element model is 2D with plane stress elements for concrete and embedded truss elements for longitudinal and transversal reinforcement [Fig. 3]. Due to symmetry, only half of the beam is modeled. The concrete response is simulated with a total strain rotating crack model. The reinforcement steel is modeled with hardening plasticity. The steel plates for load application and support are also modeled with linear elastic material properties. Interface elements are used between the steel plates and the concrete beam. A static nonlinear analysis is performed with increasing imposed displacement until failure. The experimental and numerical results are compared in terms of load-displacement curve and cracking pattern at failure. Figure 3: Model of the Toronto beam test VS-C3 3 Belletti B., Damoni C., Hendriks M.A.N., de Boer A. (2016). Validating the Guidelines for Nonlinear Finite Element Analysis of Concrete Structures. Rijkswaterstaat Technisch Document, RTD :2016, RWS GPO, Utrecht, Netherlands. RC beam: simulation of an experimental test 4/68

5 Most of the material properties are available in the original publication [1]. When a parameter is not specified, the value is estimated according to the Model Code 2010, following the same procedure as in [3]. The material properties used in the model are listed in [Table 1]. Concrete Young s modulus E Poisson s ratio ν N/mm 2 Compressive strength f cm 43.5 N/mm 2 Tensile strength f tm 3.13 N/mm 2 Fracture energy in compression G c N/mm Fracture energy in tension G F N/mm Mass density ρ 2.4E-9 T/mm 3 Reinforcement steel M10 Diameter φ 11.3 mm Young s modulus E N/mm 2 Yielding strength f ym 315 N/mm 2 Ultimate strength f um Ultimate strain ε su N/mm 2 Reinforcement steel M25 Diameter φ 25.2 mm Young s modulus E N/mm 2 Yielding strength f ym 445 N/mm 2 Ultimate strength f um Ultimate strain ε su N/mm 2 Reinforcement steel M30 Diameter φ 29.9 mm Young s modulus E N/mm 2 Yielding strength f ym 436 N/mm 2 Ultimate strength f um Ultimate strain ε su N/mm 2 Reinforcement steel D4 Diameter φ 5.7 mm Young s modulus E N/mm 2 Yielding strength f ym 600 N/mm 2 Ultimate strength f um Ultimate strain ε su N/mm 2 Steel for plates Young s modulus E N/mm 2 Poisson s ratio ν 0.3 Table 1: Material properties RC beam: simulation of an experimental test 5/68

6 2 Finite Element Model For the modeling session we start a new project. This will be a two dimensional model and we will dominantly use quadratic hexagonal elements. Main menu File New [Fig. 4] Figure 4: New project dialog RC beam: simulation of an experimental test 6/68

7 2.1 Units We use millimeter for the unit length and Newton for force. Model Window Reference system Units [Fig. 5] Property Panel [Fig. 6] Figure 5: Model window Figure 6: Property Panel - Units RC beam: simulation of an experimental test 7/68

8 2.2 Geometry Definition We start the model by making a polyline in Y = 0 and Z = 0 with the length of the beam and including the vertexes correspondent to the positions of the loading and support plates; the X coordinates for the vertexes are [Fig. 7]: 0, 145, 220, 295, 3345, Afterwards we extrude that line 552 mm in the Y -direction, that corresponds to the height of the beam [Fig. 8] [Fig. 9]. Main Menu Geometry Create Add polyline [Fig. 7] Main Menu Geometry Modify Extrude shape [Fig. 8] Figure 7: Geometry - Add polyline Figure 8: Geometry - Extrude polyline RC beam: simulation of an experimental test 8/68

9 Figure 9: View of the model - Beam RC beam: simulation of an experimental test 9/68

10 We do the same procedure with the support and load plates. For the support plate we create the line coincident with the beam edge and extrude it for -35 mm in the Y -direction (which corresponds to the thickness of the plates) [Fig. 10] [Fig. 11]. For the load plate we create the line coincident with the beam edge and extrude it 35 mm in the Y -direction [Fig. 12] [Fig. 13]. This procedure is performed to have a regular mesh. Main Menu Geometry Create Add polyline [Fig. 10] [Fig. 12] Main Menu Geometry Modify Extrude shape [Fig. 11] [Fig. 13] Figure 10: Geometry - Add line support plate Figure 11: Geometry - Extrude line support plate RC beam: simulation of an experimental test 10/68

11 Figure 12: Geometry - Add line load plate Figure 13: Geometry - Extrude line load plate RC beam: simulation of an experimental test 11/68

12 Figure 14: View of the model - Beam and plates for support and load RC beam: simulation of an experimental test 12/68

13 We define 3 lines for the longitudinal reinforcement (see [Fig. 1]): i) line for 2xM30 bars for one level of bottom reinforcement, ii) line for 2xM25 bars for other level of bottom reinforcement, iii) line for 3xM10 bars for the top reinforcement. Main Menu Geometry Create Add polyline [Fig. 15] - [Fig. 17] Figure 15: Geometry - Add line for 2xM30 bars Figure 16: Geometry - Add line for 2xM25 bars Figure 17: Geometry - Add line (3xM10 bars) RC beam: simulation of an experimental test 13/68

14 Figure 18: View of the model - Longitudinal reinforcement RC beam: simulation of an experimental test 14/68

15 We define the lines for the stirrups. Stirrups are predominantly distanced of 168 mm. This distance decreases to 52 mm in the loading and support areas (see [Fig. 1]). We define the first stirrup line from the bottom to the top reinforcements and at a distance of 52 mm from the edge of the beam. Main Menu Geometry Create Add line [Fig. 19] Figure 19: Geometry - Add Stirrup 1 RC beam: simulation of an experimental test 15/68

16 We copy that line 4 times with a distance of 84 mm [Fig. 20]. We copy the last stirrup 17 times with a distance of 168 mm [Fig. 21]. Finally we copy the last created line 2 times at a distance of 84 mm [Fig. 22]. Main Menu Geometry Modify Array copy [Fig. 20] - [Fig. 22] Figure 20: Geometry - Array copy stirrups Figure 21: Geometry - Array copy stirrups Figure 22: Geometry - Array copy stirrups RC beam: simulation of an experimental test 16/68

17 Figure 23: View of the model - Transversal reinforcement RC beam: simulation of an experimental test 17/68

18 In order to be able to output cross-section forces and bending moments in the beam we will use composed line elements. These elements are used for post-processing purposes only and do not have mechanical properties, so they do not influence the behaviour of the model. The stresses in the elements are integrated over the cross-section plane normal to the reference line. We create a line along the mid-height of the beam to create the composed line elements. Main Menu Geometry Create Add line [Fig. 24] Figure 24: Geometry - Add line for composed elements RC beam: simulation of an experimental test 18/68

19 The geometry definition of the model is complete. Figure 25: View of the model - Geometry RC beam: simulation of an experimental test 19/68

20 2.3 Properties Concrete beam To model the concrete we use a total strain rotating crack model with exponential softening in tension and parabolic behavior in compression. The parameters used for the definition of the material are listed in [Table 1]. Main Menu Geometry Analysis Property assignments [Fig. 26] Shape assignment Add new material [Fig. 27] [Fig. 28] - [Fig. 31] Figure 26: Assign beam properties Figure 27: Add new material - Concrete Figure 28: Concrete material properties RC beam: simulation of an experimental test 20/68

21 Figure 29: Concrete material properties Figure 30: Concrete material properties Figure 31: Concrete material properties RC beam: simulation of an experimental test 21/68

22 We use membrane elements with the thickness equal to the width of the beam (152 mm). We define the local element axes to ensure that these are the same in all elements. We add a new data for the beam in order to change the default number of integration points. If we define the geometry directly through the Shape property assignments dialog box [Fig. 32] will not appear; otherwise we have to define it as presented. Shape assignment Add new geometry [Fig. 33] Shape assignment Add new data [Fig. 34] Figure 32: Beam - Add new geometry Figure 33: Beam - Edit geometry Figure 34: Beam - Add new data RC beam: simulation of an experimental test 22/68

23 In the beam data we increase the number of integration points from default to high. We do this to increase the accuracy of the results as we are doing a nonlinear analysis until failure and comparing with experimental data. Geometry browser Element data Beam [Fig. 35] Properties Panel Description Drop-down list (INTEGR Numerical integration scheme) [Fig. 36] Properties Panel Value HIGH [Fig. 37] Figure 35: Element data Figure 36: Properties panel Figure 37: Set integration scheme RC beam: simulation of an experimental test 23/68

24 2.3.2 Steel plates We assign the properties of the steel plates of the support and loading positions. Steel is linear elastic with the properties listed in [Table 1]. Main Menu Geometry Analysis Property assignments [Fig. 38] Shape assignment Add new material [Fig. 39] [Fig. 40] Figure 38: Assign plates properties Figure 39: Add new material - Steel Figure 40: Steel material properties RC beam: simulation of an experimental test 24/68

25 We also use membrane elements with the thickness equal to the width of the beam (152 mm). We add a new data for the plates to set the same integration scheme as the one used for the beam. Shape assignment Add new geometry [Fig. 41] [Fig. 42] Shape assignment Add new data [Fig. 43] Figure 41: Plates - Add new geometry Figure 42: Plates - Edit geometry Figure 43: Plates - Add data RC beam: simulation of an experimental test 25/68

26 We increase the number of integration points from default to high. Geometry browser Element data Plate [Fig. 44] Properties Panel Description Drop-down list (INTEGR Numerical integration scheme) [Fig. 45] Properties Panel Value HIGH [Fig. 46] Figure 44: Element data Figure 45: Properties panel Figure 46: Set integration scheme Note: instead of defining a new data set for the plates we could also assign the data set of the beam to the loading and support plate shapes; so all these parts of the model would have the same integration scheme. RC beam: simulation of an experimental test 26/68

27 2.3.3 Interfaces We include an interface between the steel plates and the beam. The element class is Structural Interfaces and for the material definition the properties were based on the reference [3]. We start with the support plate interface (see [Fig. 3]). Main Menu Geometry Analysis Connection property assignments [Fig. 48] [Fig. 47] Connection property assignment Add new material [Fig. 49] [Fig. 50] - [Fig. 51] Figure 47: Edge selection for interface properties assignement Figure 48: Assign interface properties Figure 49: Interface - Add new material RC beam: simulation of an experimental test 27/68

28 Figure 50: Interface - Material properties Figure 51: Interface - Material properties RC beam: simulation of an experimental test 28/68

29 The thickness of the interface is equal to the width of the beam (152 mm). It is a line interface element. We add a new data because we will use an integration scheme and number of integration points different from the default. If we define the geometry directly through the Connection property assignments dialog box [Fig. 52] will not appear; otherwise if we do it afterwards we have to define it as presented. Connection property assignment Add new geometry [Fig. 53] Shape assignment Add new data [Fig. 54] Figure 52: Interface - Add geometry Figure 53: Interface - Edit geometry Figure 54: Interface - Add new data RC beam: simulation of an experimental test 29/68

30 Following the same procedure used in [3] we use Reduced Lobatto integration which means 3 integration points with Lobatto integration scheme. Geometry browser Element data Interface [Fig. 55] Properties Panel Description Drop-down list (INTEGR Numerical integration scheme) [Fig. 56] Properties Panel Value Reduce [Fig. 57] Properties Panel Description Drop-down list (NUMINT Integration scheme name) [Fig. 58] Properties Panel Value Lobatto [Fig. 59] Figure 56: Properties panel Figure 58: Properties panel Figure 55: Element data Figure 57: Set integration scheme Figure 59: Set integration scheme RC beam: simulation of an experimental test 30/68

31 We assign the same properties to the load plate interface. Main Menu Geometry Analysis Connection property assignments [Fig. 60] [Fig. 61] Figure 60: Assign interface properties Figure 61: Beam model with interfaces RC beam: simulation of an experimental test 31/68

32 2.3.4 Reinforcement We now define the properties of the reinforcement and we start with the longitudinal reinforcement. There are three types of reinforcement - M10, M25 and M30 (see [Fig. 1] and [Table 1]). We need to define the different material properties and sectional areas for each type of reinforcement. We use embedded reinforcement elements and element by element discretization method. We start with the top longitudinal reinforcement of 3xM10 bars. We define the material properties as listed in [Table 1]. Main Menu Geometry Analysis Reinforcement property assignments [Fig. 62] Reinforcement property assignment Add new material [Fig. 63] [Fig. 64]- [Fig. 65] Figure 62: Assign reinforcement properties 3xM10 bars Figure 63: Add new material - M10 reinforcement Figure 64: Material properties - M10 reinforcement RC beam: simulation of an experimental test 32/68

33 Figure 65: Material properties - M10 reinforcement Figure 66: Strain stress diagram - M10 reinforcement RC beam: simulation of an experimental test 33/68

34 And we define the cross section of the bar as 3 times the area of the steel M10 ( = mm 2 ). Shape assignment Add new geometry [Fig. 67] Figure 67: Add new geometry - M10 reinforcement Figure 68: Model view - selection bar topm10 RC beam: simulation of an experimental test 34/68

35 We assign the material properties to the bottom reinforcement of 2xM30 bars according to [Table 1]. Main Menu Geometry Analysis Reinforcement property assignments [Fig. 69] Reinforcement property assignment Add new material [Fig. 70] [Fig. 71] - [Fig. 72] Figure 69: Assign reinforcement properties 2xM30 Figure 70: Add new material - M30 reinforcement Figure 71: Material properties - M30 reinforcement RC beam: simulation of an experimental test 35/68

36 Figure 72: Material properties - M30 reinforcement Figure 73: Strain stress diagram - M30 reinforcement RC beam: simulation of an experimental test 36/68

37 And we define the cross section of the bar as 2 times the area of the steel M30 ( = mm 2 ). Shape assignment Add new geometry [Fig. 74] Figure 74: Add new geometry - M30 reinforcement Figure 75: Model view - selection bar botm30 RC beam: simulation of an experimental test 37/68

38 We define the bottom reinforcement of 2xM25 bars. We define the material properties as listed in [Table 1]. Main Menu Geometry Analysis Reinforcement property assignments [Fig. 76] Reinforcement property assignment Add new material [Fig. 77] [Fig. 78]-[Fig. 79] Figure 76: Assign reinforcement properties 2xM25 Figure 77: Add new material - M25 reinforcement Figure 78: Material properties - M25 reinforcement RC beam: simulation of an experimental test 38/68

39 Figure 79: Material properties - M25 reinforcement Figure 80: Strain stress diagram - M25 reinforcement RC beam: simulation of an experimental test 39/68

40 And we define the cross section of the bar as 2 times the area of the steel M25 ( = mm 2 ). Shape assignment Add new geometry [Fig. 81] Figure 81: Reinforcement M25 - Add new geometry Figure 82: Model view - selection bar botm25 RC beam: simulation of an experimental test 40/68

41 We now define the transversal reinforcement with stirrups of 2xD4 bars. We need to define the material properties and the area of the cross section. We also use embedded reinforcement and element by element discretization method. We define the material properties of reinforcement steel D4 as listed in [Table 1]. Main Menu Geometry Analysis Reinforcement property assignments [Fig. 83] Reinforcement property assignment Add new material [Fig. 84] [Fig. 85]-[Fig. 86] Figure 83: Assign reinforcement properties 2xD4 Figure 84: Add new material - D4 reinforcement Figure 85: Material properties - D4 reinforcement RC beam: simulation of an experimental test 41/68

42 Figure 86: Material properties - D4 reinforcement Figure 87: Strain stress diagram - D4reinforcement RC beam: simulation of an experimental test 42/68

43 And we define the cross section of the bar as 2 times the area of the steel D4 ( = 51.4 mm 2 ). Shape assignment Add new geometry [Fig. 81] Figure 88: Add new geometry - D4 reinforcements Figure 89: Model view - selection stirrups RC beam: simulation of an experimental test 43/68

44 2.3.5 Composed line element We define the properties of the composed line element. We need to define the maximum distance of the elements considered for the integration of forces in the post-processing. The maximum distance is 552 mm, which corresponds to the height of the beam. We define the element axes with z-local axis coincident with Z-global axis. Main Menu Geometry Analysis Property assignments [Fig. 90] Shape assignment Add new geometry [Fig. 91] Figure 90: Assign composed line properties Figure 91: Define new geometry - composed line Figure 92: Model view - selection composed line RC beam: simulation of an experimental test 44/68

45 2.4 Boundary Conditions We restrict the translation in the Y -direction in the mid point of the support plate. Main Menu Geometry Analysis Attach support [Fig. 93] Figure 93: Add point support Figure 94: View of the model - Point support RC beam: simulation of an experimental test 45/68

46 Due to the symmetry condition we restrict the translation in the X-direction in the symmetry edges of the beam and loading plate. Main Menu Geometry Analysis Attach support [Fig. 95] Figure 95: Add line support Figure 96: View of the model - Symmetry support RC beam: simulation of an experimental test 46/68

47 The load will be applied by imposed deformation, so we add a support in the location of the point load with restriction in the Y -direction (direction of the applied load). Main Menu Geometry Analysis Attach support [Fig. 97] Figure 97: Add point support Figure 98: View of the model - Support for imposed deformation RC beam: simulation of an experimental test 47/68

48 2.5 Loads As we will impose incremental load to the beam until failure, the effects of the dead weight can be neglected. We define the point load as a prescribed deformation of translation in the Y -direction with the value of -0.1 mm. We impose a prescribed deformation instead of force to replicate the experimental test that is controlled by displacements. We define a small value of displacement because we will impose small increments in the nonlinear analysis. Main Menu Geometry Analysis Attach load [Fig. 99] Figure 99: Point load Figure 100: Model view - Point load RC beam: simulation of an experimental test 48/68

49 2.6 Meshing We set the element size as 25 mm and generate the mesh. Main Menu Geometry Analysis Set mesh properties [Fig. 101] Main Menu Geometry Generate mesh [Fig. 102] Figure 101: Mesh properties Figure 102: Model view - Mesh RC beam: simulation of an experimental test 49/68

50 For an easier manipulation of output results we create two groups of reinforcement sets, one for the longitudinal reinforcement and other for the stirrups. Mesh browser Mesh Reinforcement sets < select all the longitudinal reinforcements > New group of reinforcement sets [Fig. 103] Mesh browser Mesh Reinforcement sets < select all the stirrups > New group of reinforcement sets [Fig. 104] < Rename (F2 or ) the reinforcement groups accordingly > [Fig. 105] Figure 103: New reinforcement group - longitudinal rebars Figure 104: New reinforcement group - stirrups Figure 105: Reinforcement groups RC beam: simulation of an experimental test 50/68

51 3 Nonlinear Static Analysis 3.1 Analysis Commands We perform a structural nonlinear analysis until failure by increasing the load. Analysis browser New analysis [Fig. 106] Analysis browser Analysis1 Add command Structural Nonlinear [Fig. 107] [Fig. 108] <Rename (F2 or ) the execute block as Load > Figure 106: Analysis window Figure 107: Add command Figure 108: Analysis tree RC beam: simulation of an experimental test 51/68

52 As we are performing an analysis until failure we don t consider the self weight as it would have negligible influence. The point load is applied incrementally until failure by imposed deformation. We set the properties of the iterative procedure in order to ensure a stable and efficient analysis that converges throughout the nonlinear path of the structural response until failure. If we use default settings we will find problems of convergence from early load steps. Load is applied in 120 increments with a factor of 5 [Fig. 109]. We activate the Arc length control to follow the path of response with automatic scale of load steps. We use the Updated normal plane method with regular control, which are the default arc length options [Fig. 110]. We add a new set of control to chose the nodes and direction considered in the Arc Length [Fig. 111]. Analysis browser Analysis1 Structural nonlinear Load Load steps [Fig. 109] Properties - LOAD Arc length control Settings [Fig. 110] Regular arc length control settings Control sets Add new [Fig. 111] Figure 109: Load steps Figure 110: Arc length control settings Figure 111: Arc length new control set RC beam: simulation of an experimental test 52/68

53 In the Regular arc length control settings we consider the translations in the Y -direction because it is the direction of loading [Fig. 112]. To control the Arc length we choose all the nodes of the concrete beam (without the support and loading steel plates). For that we select the Beam in the Mesh browser [Fig. 113] [Fig. 114]. Regular arc length control settings DOF selection Node numbers [Fig. 112] Mesh browser Element sets Beam Select [Fig. 113] [Fig. 114] Figure 112: Arc length control Figure 113: Arc length control - node selection Figure 114: Arc length control settings RC beam: simulation of an experimental test 53/68

54 For the equilibrium iteration procedure we use the Newton-Raphson method with a maximum of 25 iterations. We use Line search with default settings to speed up convergence. For the convergence norms we use energy convergence with 10 3 and force convergence with tolerance of We choose to continue the analysis even if convergence is not achieved within the maximum number of iterations. The characteristics of the analysis were based on the reference [3]. The analysis runs until the final step, which is already in the post-peak response. Analysis browser Analysis1 Structural nonlinear Load Equilibrium iteration [Fig. 115] Properties - ITERAT Energy - Settings <Convergence tolerance = 0.001; no convergence - continue> [Fig. 116] Properties - ITERAT Force - Settings <Convergence tolerance = 0.01; no convergence - continue> [Fig. 117] Figure 115: Equilibrium iterations settings for load Figure 116: Energy convergence norm Figure 117: Force convergence norm RC beam: simulation of an experimental test 54/68

55 With the user selection we choose to output results of displacements, support reactions, crack strains and openings, total strains and stresses and forces and bending moments in the composed elements. Finally we run the analysis. Analysis browser Analysis1 Structural nonlinear Output Edit properties [Fig. 118] Properties - OUTPUT Result User selection Modify [Fig. 119] [Fig. 120] Analysis browser Analysis1 Run analysis Figure 118: Edit output properties Figure 119: Selection of results Figure 120: Output user selection RC beam: simulation of an experimental test 55/68

56 3.2 Results Displacements We start the presentation of results with the curve of applied load vs. displacement at mid-span and comparison with experimental data. For that we create a graph with the reaction force versus displacement in Y -direction in the bottom part of the beam at mid-span. Model Nodal selection <Select the node located at mid-span at coordinates(3420, 0, 0) mm > [Fig. 121] Result browser Output Nodal results Total Displacements TDtY Show table <Copy the data to Excel> [Fig. 122] [Fig. 123] Figure 121: Selected node for displacements Figure 122: Show table Figure 123: Table of total displacements RC beam: simulation of an experimental test 56/68

57 Select the node located at middle of the support plate. We copy the reactions from to Excel. Model Nodal selection <Select the node located at middle of the support plate at coordinates (220, -35, 0) mm> [Fig. 124] Results browser Output Nodal results Reaction Forces FBY Show table <Copy the data to Excel> [Fig. 125] [Fig. 126] Figure 124: Selected node for reaction force Figure 125: Show table Figure 126: Table of reaction forces RC beam: simulation of an experimental test 57/68

58 We make the graph in Excel. Load is the reaction force FBY multiplied by 2 and deflection is the displacement TDtY multiplied by -1. We can observe a good agreement between the numerical and experimental results. Figure 127: Load vs. Displacements RC beam: simulation of an experimental test 58/68

59 3.2.2 Crack widths We represent the crack widths in the beam. For that we want to display only the mesh that belongs to the beam. We make a contour plot of principal crack width at peak load (load step 90). Mesh browser Mesh Element sets Beam Show only [Fig. 128] Results browser Output Element results Crack-widths Ecw1 [Fig. 129] [Fig. 130] Figure 128: Show only beam mesh Figure 129: Result tree - crack widths Figure 130: Crack widths at peak load RC beam: simulation of an experimental test 59/68

60 We observe that the computed crack pattern is similar to the experimental observation and that the failure is due to bending. Figure 131: Crack patterns at failure: numerical and experimental results RC beam: simulation of an experimental test 60/68

61 3.2.3 Principal stresses We present the minimum principal stresses in the beam at peak load. We can observe crushing of concrete near the load application area. Results browser Output Element results Cauchy Total Stresses S2 [Fig. 132] [Fig. 133] Figure 132: Result tree - principal stresses Figure 133: Minimum principal stresses at peak load RC beam: simulation of an experimental test 61/68

62 3.2.4 Longitudinal reinforcement We present the strains in longitudinal reinforcement at peak load (Load-step 90). For that we show only in the mesh the longitudinal reinforcement group. Mesh browser Mesh Reinforcement group Long Reinforcement Show <or tick in the box> [Fig. 134] Results browser Output Reinforcement results Reinforcement Total Strains EXX [Fig. 135] [Fig. 136] Figure 134: Show longitudinal reinforcement Figure 135: Result tree - EXX in reinforcement RC beam: simulation of an experimental test 62/68

63 We can see that the reinforcement is yielded at peak load as the yielding strain is 2.18E-3 for M30 and 2.02E-3 for M25. Figure 136: Strains EXX in longitudinal reinforcement at peak load RC beam: simulation of an experimental test 63/68

64 3.2.5 Transversal reinforcement We present the strains in transversal reinforcement at peak load (Load-step 90). For that we hide the longitudinal reinforcement from the mesh and show the stirrups group. Mesh browser Mesh Reinforcement group Long Reinforcement <take the tick in the box> Mesh browser Mesh Reinforcement group Stirrups <tick in the box> [Fig. 137] Results browser Output Reinforcement results Reinforcement Total Strains EYY [Fig. 138] [Fig. 139] Figure 137: Show stirrups Figure 138: Result tree - EYY in stirrups RC beam: simulation of an experimental test 64/68

65 We can see that the stirrups are yielded in some areas of the beam as the yielding strain is 3.0E-3. Figure 139: Strains EYY in transversal reinforcement at peak RC beam: simulation of an experimental test 65/68

66 3.2.6 Composed elements: shear forces and bending moments In order to illustrate the advantage of using composed elements we output the diagrams of sectional shear forces and moments in the beam for the peak load. First we hide the stirrups and show only the Line with the composed elements in the mesh. We display line diagrams for shear forces Qy and moments Mz. Mesh browser Mesh Reinforcement group Stirrups <take the tick in the box> Mesh browser Mesh Element sets Line Show only [Fig. 140] Results browser Output Element results Cross-section Forces Qy Show line diagram [Fig. 141] [Fig. 143] Results browser Output Element results Cross-section Moments Mz Show line diagram [Fig. 142] [Fig. 144] Figure 140: Show only composed line in the mesh Figure 141: Result tree - Qy Figure 142: Result tree - Mz RC beam: simulation of an experimental test 66/68

67 Figure 143: Cross section forces Qy Figure 144: Cross section moments Mz RC beam: simulation of an experimental test 67/68

68 DIANA FEA BV Delftechpark 19a 2628 XJ Delft The Netherlands T +31 (0) F +31 (0) DIANA FEA BV Vlamoven TN Arnhem The Netherlands T +31 (0) F +31 (0)