Simple Cantilever Beam
1) Click on New from the File menu or from the Defaults Toolbar as shown. Type the name of the new database as Cantilever_Beam and click OK.
2) Type the name of the new database as Cantilever_Beam and click OK.
1) Under the Geometry tab, click on Surface and select XYZ.
2) Input the vector of <12 1 0> in the Vector Coordinates List and click Apply. There are no units in Patran, and therefore it is important to stay consistent in units.
1) Under the Properties tab, select Isotropic.
2) Input steel as the Material Name and then select Input Properties ....
3) Input 30×106 as the Elastic Modulus and 0.3 as the Poisson's Ratio. Click OK and Apply.
1) Click on Shell under the 2D Properties section.
2) Input 2D_plate as the Property Set Name and then click on Input Properties ....
3) Click on Select Material and select steel. Enter 0.1 as the Thickness. Click OK.
4) Click on Select Application Region and then click on the Select Members box. Screen pick the surface. Click Add, OK then
Step 5 - Create boundary conditions: Constrain all translational degrees of freedom and the y-axis rotation degree of freedom along the left end of the beam.
1) Under the Load/BCs tab, select Displacement Constraint.
2) Input fixed_edge as the New Set Name and then click on Input Properties ....
3) Input <0,0,0> for Translations (to prevent any translational movement) and < ,0, > for Rotations (to prevent rotation in the y-direction). Click OK.
4) Click on Select Application Region and then click on the Select Geometry Entries box. In the selection toolbar, select Curve or Edge. Screen select the left edge of the surface. Click Add, OK then Apply.
1) Click on Distributed Load under the Element Uniform section.
2) nput z_load as the New Set Name and set the Target Element Type to 2D.
3) Click on Input Data... and input <0,0,-10> as the Edge Distr Load. Click OK.
4) Click on Select Application Region and then click on the Select Surface Edges box. Screen select the right edge of the surface. Click Add, OK then Apply.
1) Under the Meshing tab, click on Surface Meshers.
2) Click on the Select Surface List box. Screen click the surface. Click Apply.
1) Under the Analysis tab, select Entire Model. Ensure that the Job Name box is filled with a name and click Apply.
Step 9 - Attach results file, then create fringe and deformation plots. Record maximum displacement and stresses.
1) Click on XDB under the Access Results submenu.
2) Ensure the appropriate Job Name is selected and click Apply.
3) Under the Results tab, select Fringe/Deformation.
4) Plot Stress Tensor and Displacements, Translational. Click Apply.
1) Substitute: P=10 lb, L=12 in, E=30e6 psi, I=[1×(0.1)3]/12 in the equation below.
2) Results: δmax = 2.304 inches MD Nastran results = 2.286995E+00 inches (You can open the 'Cantilever_Beam.f06' file with Notepad to view your results)
To make the answers more precise, local shear effects must be taken into account.