ANSYS Multiphysics 11 is used here for the analysis
of Reinforced Concrete Beam. In ANSYS, all the units should be converted to a
same unit and just use the value.
For modeling concrete structure in ANSYS, Solid65
element type is used. This solid is capable of cracking in tension and crushing
in compression [1]. In this tutorial, the use of value -1 for uniaxial crushing
stress removes crushing capability and cracking of the concrete control the
failure of the finite element model [2]. The shear transfer coefficient
describes the ability of an open or closed crack to transfer loads. These
coefficients can vary from 0 to 1, with 0 indicating a very smooth crack and 1
indicating a rough crack surface [3]. Here, open shear transfer coefficient is
considered as 0.3 and closed shear transfer coefficient is 1. Uniaxial cracking
stress is 3.6e6 Pa. Elastic modulus and
Poisson’s ratio for concrete and steel used here are respectively 3e10 Pa, 2e11
Pa and 0.2, 0.3. Beam dimension: Length (X)=15, Height (Y)=5, Width (Z)=6
Ø File
- Change Job name: RCC beam
Ø File
– Change title : RCC beam
Ø Preprocessor
– Element type - Add/edit/delete – Add – Solid Concrete 65 (Click Apply) –
Shell Elastic 4 node 181 ( Click Apply) – Beam 3D finite strain (Click Ok) -
Close
Ø SAVE_DB
Ø Preprocessor
– Real constants – Add/edit/delete – Add – Type 1 Solid 65 – Ok – Real constant
set No. 1 – Ok - Close
Ø Here,
Material 1: Concrete, Material 2: Steel, Units used in Pascal (Pa)
Ø Preprocessor
– Material Props – Material Library – Select Units
Ø Preprocessor
– Material props – Material models – Material model number 1 – Structural- Linear
– Elastic – Isotropic – EX 3e10 – PRXY 0.2 – Ok – Nonlinear – Inelastic –
Non-metal plasticity – Concrete – Open Shear Transfer Coef 0.3 – Closed Shear
Transfer Coef 1 – Uniaxial Cracking Stress 3.6e6 –
Uniaxial Crushing Stress (-1) – Ok
Ø Material
– New model – Define material ID 2 – Ok
Ø Preprocessor
– Sections – Beam – Common sections – (fill it as shown in the picture) – Apply
– Ok
Ø Preprocessor
– Modeling – Create – Area – Rectangle – By 2 corners – WP X=0, WP Y=0,
Width=15, Height= 5 – Apply – Ok
Ø Preprocessor
– Meshing – Mesh Tool – Lines Set – (4 lines are selected) - Apply – No. of
element divisions 5 – Apply – Ok
Ø Preprocessor
– Meshing – Mesh Tool – Global Set – Element type number 2 SHELL181 – (leave
the others as they are) – Ok
Ø In
Mesh Tool; Shape: Quad, Mapped – Mesh – Click onto the rectangle – Apply – Ok (Close
the Mesh Tool)
Ø Preprocessor
– Modeling – Operate – Extrude – Elem Ext Opts – Element type number 1 SOLID65
– No. Elem divs 4 – Clear area after ext Yes – Ok
Ø Preprocessor
– Modeling – Operate – Extrude – Areas – By XYZ Offset – Click onto the
rectangle – Ok – Offsets for extrusion 0, 0, 6 – Ok
Ø Isometric
View – Plot – Elements
Ø Plot
– Nodes – Oblique View
Ø Preprocessor
– Modeling – Create – Elements – Elem Attributes – Element type number 3
BEAM188 – Material number 2 – Ok
Ø Preprocessor
– Modeling – Create – Elements – Auto Numbered – Thru Nodes – (select nodes and
after selecting every two nodes click Apply, then a line will be created
between those two nodes. Do the same until all nodes are selected. At last
click Ok.)
Ø Select
– Entities – Elements – By Attributes – Min, Max Inc 2 – Plot – Ok
Ø PlotCtrls
– Style – Size and Shape – Display of element On
Ø Select
– Everything – Plot – Elements – Isometric view
Ø Front
view
which is in front view – Apply – All DOF – Apply –
In the dialogue box click on ‘Box’ – Drag the mouse pointer and select the full
element – Ok – Unpick All DOF and pick ROTY – Ok
Ø Isometric
view
Ø Solution
– Define loads – Apply – Structural – Force/Moment – On Nodes – Select a node –
Ok – In the dialogue box, Direction of force/mom FZ – Value 8000 – Ok
Ø Solution
– Analysis Type – Sol’n Controls – Fill the dialogue box as shown – Ok
Ø Solution
– Solve – Current LS – Ok – (Sometimes a warning is shown. Don’t WORRY about it
if it is telling about ‘1 warning’. May be there is a minor mistake.) – Wait
some time and it will show ‘Solution is Done’.
Ø General
Postproc – Plot Results – Contour Plot – Nodal Solu – DOF Solution - Displacement vector sum – Scale Factor True
Scale – Ok
Ø General
Postproc – Plot Results – Contour Plot – Nodal Solu – Stress – von Mises stress
– Scale factor True Scale – Ok
References:
- http://mostreal.sk/html/elem_55/chapter4/ES4-65.htm
- http://www.oregon.gov/odot/td/tp_res/docs/reports/finiteelementmodeling.pdf
- MacDonald, Bryan J., 2011, Practical Stress Analysis with Finite Elements (2nd Edition), Glasnevin Publishing, 388 p.
- https://www.youtube.com/watch?v=OxAg8bg40H4
- https://www.youtube.com/watch?v=8glTmwLk59c
