Md Monjurul Hasan's Blog: RC Beam Analysis With ANSYS Step by Step

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 Material model number 2 – Structural – Linear – Elastic – Isotropic – EX 2e11 – PRXY 0.3 – Ok – Material – Exit

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

Ø Solution – Define loads – Apply – Structural – Displacement – On Nodes – In the dialogue box click on ‘Box’ – Drag the mouse pointer from the left corner of the element

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’.