Problem: Using Marc, Find the vertical displacement imposed by the load P for the linear load case. The load P is 6000 lb. The length L of the beam is 100 in. The dimensions of the beam Section A-A (a x b) are 1.0 in x 2.0 in. The Young's Modulus is 30 x 106 and the Poisson's Ratio is 0.3.

Horizontal spacer

1) Click on File. Then, Click on Save As....

2) Under File name:, enter tip_load and click Save.

(Note: Do not use spaces in directory or file names, instead use underscores, "_".)

1) Click on the Geometry & Mesh Tab and click on Geometry & Mesh.

2) Under Points:, click Add and in the Dialog menu / Command, enter 0 for Enter point coordinates (x) and hit enter, enter 0 for Enter point coordinates (Y) and hit enter, and enter 0 for Enter point coordinates (Z) and hit enter. Repeat for the following coordinates (100, 0, 0), (100, 2, 0), and (0, 2, 0).

3) Click on FILL on the View toolbar to make all the points visible on your screen.

4) Create a surface based on the 4 points by clicking on the drop down menu under Surfaces in the Geometry & Mesh tab and choose Quad and click Add.

5)Click OK.

6) Enter quad points 1 2 3 4 in the Dialog menu / Command.

1) Under Operations, click Convert.

2) Under Divisions, enter the number of convert divisions in U and V: 8 and 1 and hit enter.

3) Click Surface To Elements.

4) Now, click the All Existing icon. The surface will now be divided into meshes 8 x 1.

1) Click on the Material Properties tab and click on New - Standard.

2) Under Name, enter steel. Then click on Structural under Data Categories.

3) Enter 3e7 for the Young's Modulus and 0.3 for the Poisson's Ratio. Then click OK.

4) Return to the Material Properties tab, and click on General. Enter 0.00074 for the Mass Density and click OK.

5) Assign the properties to the geometry by clicking on Add under Elements and then select all the elements on the screen and click on End List.

1) Under Geometric Properties click on New, then click on Planar and then Plane Stress.

2) Under Name:, enter beam_geom and hit enter.

3) Click on Properties and enter 1 for the Thickness and hit enter. Make sure Assumed Strain is checked. Then click OK.

4) Click Add under Elements.

5) Click on the All Existing icon and then click on End List.

1) Click on the Boundary Conditions tab and then click on New (Structural) then Fixed Displacement.

2) Enter boundary condition Name: as fixed then hit enter.

3) Click on Properties and then make sure Displacement X and Displacement Y are checked and click OK.

4) Under Nodes, click on Add.

5) Select the left edge nodes as shown and then click on End List.

6) To create the Force Table, under Table & Coord. Syst., click New and go to 1 Independent Variable.

7) Enter Name: as Force_Table.

8) Click Type and then click time.

9) Then click Data Points and click Add.

10) Enter independent variable V1 value: 0 0 and hit enter. Then enter independent variable V1 value: 1 1 and hit enter.

Note: To switch back to the Beam Model from the Force Table, go to Window and switch to Model (View 1).

1) In the Boundary Conditions tab, click on New/Point Load.

2) Enter tip_load for the Name and and then click on Properties.

3) Make sure Force Y is checked and enter a value of -6000 for y. Click Table for Force Y and select Force_Table.

4) Click Add under Nodes: and select the top right corner node as shown.

5) Click End List.

1) Click on the Loadcases tab and click on New - Static.

2) Enter the Name as my_linear, and click on Properties.

3) Click on Loads and make sure that both fixed and tip_load loads are selected. Click OK.

4) Enter the # Steps as 10. Click OK.

1) Click on the Jobs tab and then click on New - Structural.

2) Click on Properties.

3) Under Available, select my_linear.

4) Under Analysis Dimension, select Plane Stress.

5) Make sure Linear Elastic Analysis is checked.

6) Click on Analysis Options.

7) Click on Advanced Options and make sure Assumed Strain is checked. Click OK and OK.

8) Under Element Types tab select Analysis Dimension. Select Planar and click Solid.

9) Click 114 (Plane Stress Reduced Integration 4-noded QUAD). Click OK.

10) Click on the All Existing icon and click on Id Types to ensure that all the elements are labeled as 114.

1) Under Jobs, click Show Menu.

2) Enter Name as linear_job1 and click Run.

3) Click Save Model and Submit(1).

4) Click Monitor.

5) Then click Status File after "Complete" appears in the status box.

6) Click Open Post File.

1) Click on the Results tab and click on Model Plot.

2) Under Deformed Shape set style to Deformed & Original.

3) Under Scalar Plot set the style to Contour Bands. Click Scalar and select Displacement Y. Click OK.

4) Click Play and click FILL.

5) You can create the deformed shape with the undeformed shape by setting the style under Model Plot Results to Deformed & Original.

1) In the Result File Navigation, click on Rewind Result File.

2) Click Fill.

3) Under the Results tab, click Path Plot.

4) Click Node Path.

5) Select the two nodes on the top edge as shown.

6) Click End List

7) Click Add Curves.

8) Click Add curve, then click Arc Length, then click Displacement Y.

9) Finally click Monitor Result File and then click Fit.

1) Under the Results tab click on History Plot.

2) Then click on Set Location.

3) Click the node shown at the beam tip end and click on End List.

4) Click on All Incs and then click Add Curves.

5) Click on Single Location and then click on Node 18.

6) Under Global Variables click Time and under Variables at Locations click Displacement Y. Click OK.

The maximum Y deflection of the beam can be read directly from the displayed spectrum/range. The largest value corresponds to a magnitude of 99.64, which is in fair agreement with a manual calculation of 100. You may still improve this by remeshing using two elements over the high of the section instead of just one as you have it now. (You will be asked to do this after you have run a nonlinear analysis using the present mesh.)