SCIA stands for scientific analyser. The C in SCIA Engineering is not pronounced. Note that the first c in science is not pronounced either.

Transcription

1 Design of a reinforced concrete 4-hypar shell with edge beams P.C.J. Hoogenboom, 22 May 2016 SCIA stands for scientific analyser. The C in SCIA Engineering is not pronounced. Note that the first c in science is not pronounced either. This handout shows linear elastic analysis, linear buckling analysis and design of reinforcement. Start SCIA Engineer and start a new project. Double click on Analysis. Select General XYZ. Select Concrete C30/37. 1

2 Also select Dynamics and Stability. The others we do not need today. By selecting the functionality we add things to the menu things that we later need. The left column is a tree that makes many of the commands available. Look around in the tree. It is roughly organised in 3 parts: 1) Modelling, 2) Analysis, 3) Studying the results. (Most structural analysis programs and finite element programs are organised in this way.) In addition the program can design dimensions, perform code checking and help you write a report. 2

3 We will model a 4-hypar shell with a span of 50 m. ( 25, 0,10) (0, 0,11) ( 25,25,0) (0, 25,10) z ( 25, 25, 0) (0, 25,10) (25, 0,10) y x (25,25,0) (25, 25, 0) Double click on Structure -> 2D member -> Shell. Enter the thickness of 90 mm. Note that in this box we can also change the z axis of the local coordinate system (LCS) (inwards or outwards). Perhaps we need to do this later. 3

4 We enter one of the four hypars by typing the corner coordinates x, y, z on the command line. A command can be ended by clicking right and on end. If you want to get out of a command then press esc three times. The other three hypars can be entered in the same way. 4

5 For entering edge beams we first need to define a cross-section. 5

6 To add an edge beam to the model, click on a node and then on another node. 6

7 Repeat this for all edges including the interior edges. The shell is simply supported in 4 nodes. 7

8 Click in the drawing on a support point four times. We can check the supports by toggling them on and enlarging them. There is only self-weight on the shell. So one load case and one load combination. 8

9 Let s perform a linear elastic analysis. Note that the mesh is generated automatically. 9

10 Note that the software has done an equilibrium check for us. Since the load and the support reactions are in equilibrium the equations have been solved accurately. Let s look at the computation results. 10

11 All parts are connected properly. The element size in the hypar middles is good. At the edges the elements are probably too large. We can improve this later. The deformation at the supports is correct. The top of the shell moves up, which is unexpected but possible. The displacement of 214 mm is large. But there is no practical reason why it is too large. Of course, when we add creep, wind load and snow load the deformation will be very large. Probably too large. But it is not easy to define too large for shell structures. 11

12 Normal forces in the edge beams and interior beams. There is tension in the top, due to the camber. Perhaps there is no need for the interior beams. First principal stress in the top of the shell. (The minus sign refers to the negative side of the local z axis.) Note the edge disturbances. 30 N/mm 2 tension / 500 x 100 = 6 % reinforcement. This might not fit. Since it is due to an edge disturbance we can also let it crack. 12

13 Smallest principal stress in the top of the shell. Minus refers to the surface on the negative side of the local z axis. If the stress is not symmetrical you need to change the z axis of the local coordinate system. 59 N/mm 2 is too large. It is very local. Probably a singularity due to the point support. In reality this point support is distributed over some area. We better check the stresses at the support with a simple hand calculation instead of by finite element analysis. Let s have a look at the directions of the principal normal forces. The shell edges help the edge beams. Around the top there is a compression-tension system that seems to load itself. This calls for design improvements. (Not now.) 13

14 Directions of the principal moments. The moments in the edge disturbances are in the expected direction. Marieke Vergeer has made a small program that displays the strain energy in shells. Let s see of this works. The name of the program is b17_strain_energy_check.clc. It can be downloaded from (23 KB) The *.clc program needs to be copied to the folder C:\Users\Documents\ESA16\OpenChecks\ We need to load the program in SCIA. 14

15 15

16 The quantity α is the ratio of the membrane strain energy and the bending strain energy. Where α = 1 the load is carried in by membrane forces. Where α = -1 the load is carried by moments. It gives in one contour plot an overview of the shell behaviour. There is a lot of moment in the hypars. Mostly at the interior beams. We cannot do much about these because they are due to edge disturbances. You can write your own programs in SCIA with a tool called design forms builder. (Not know) You can use not only computation results but also model data such as node coordinates. This program (*.CLS) is first compiled (*.CLC) and then loaded into SCIA. 16

17 Let s design reinforcement. We first need to align the element coordinate systems in the reinforcement directions. The element coordinate systems are in the diagonal directions of the hypars. However, we want the reinforcement in parallel to the edge beams. Therefore, we need to rotate the coordinate systems. (We would need much less reinforcement if the bars are in the principal directions of the membrane forces. However, this would be difficult to build.) ` 17

18 Select a hypar by clicking on the edge. Rotate the LCS angle over 45 o (local coordinate system). We do this for all four hypars. (You might want to rotate some -45 o.) We need to do a new computation because the program forgets the calculation results when we rotate coordinate systems. (This can be programmed smarter.) When we zoom in we see that now the element coordinate systems are in the correct direction. Now we can display the reinforcement requirements. nxd and nyd are the membrane forces per length that the reinforcement needs to carry in the x direction and the y direction, respectively (nxd = nxx + nxy ). The moments are neglected. Only tension is important. ncd is the membrane force per length that the concrete needs to carry. 18

19 mxd and myd are the moments per length that the reinforcement needs to carry in the x and the y direction, respectively. The membrane forces are neglected. For most of the shell a mesh of 12 mm bars spaced 200 mm is sufficient. 500 N/mm 2 /1.15 x π/4 x (12 mm) 2 x 1000 mm / (200 mm) = N/m = 245 kn/m. 19

20 Let s check stability. 20

21 21

22 The first buckling mode has a buckling load factor of This means that the shell buckles at a load of 90% of its self-weight. Note that the buckling mode can be shown up or down. (Like a column can buckle to the left or to the right.) This critical load clearly is not sufficient. The deformation shows that we need stiffer edge beams. Have a look at the other buckling modes too. The number of buckling modes that are computed can be set in can be selected in Solver Setup. You can also change the finite element size in Mesh Setup. Half the element size, perform the analysis again and if the important results do not change much than the element size is sufficiently small. 22