Generate a Load-Displacement Plot

A load-displacement curve is generated and the simulated strength is compared to the experimental strength.

Load-displacement plots are commonly used as tools to determine the global stiffness response of a structure. They are particularly useful for progressive failure analyses as they are a simple means of determining how the structure behaves as failure initiates and progresses. To generate a load-displacement plot, data must be extracted from the output file.

  1. Select Tools > Data > Create. In the dialog box that appears, select the ODB field output option and click Continue.
  2. In the dialog box that appears, select Unique Nodal for the Position and check the RF2 and U2 checkboxes. On the Elements/Nodes tab, click Node sets and select LOAD_NODE.

    Note: Due to the equation constraint defined earlier, the total reaction force can easily be determined from just the load node.
  3. Click Save.
  4. Select Tools > XY Data > Manager. In the dialog box that appears, there will be two sets of data. To write this data to a file, it must be renamed using the Rename button.
  5. After the data is renamed, it can be output to a text file by selecting Report > XY. The data can then be plotted using a variety of tools such as Microsoft Office Excel.

The plot of the load-displacement curve is given in below. The sharp drop in stiffness at a displacement of 0.0462 corresponds to ultimate failure of the plate. The simulated ultimate load is 10,769 lbs and the strength is 49.9 ksi. The experimental [1] strength of the plate is given in the table below as 50.5 ksi. The ultimate strength predicted by Helius PFA and the experimental strength differ by just 1.2%.