Creating an equation based load in FEMAP

Equation Based Loading

Overview

To demonstrate the creation of equation-based loading we’ll use a water tank quarter model. Prior to load application a local coordinate system positioned at the expected water level has already been defined and the wall surfaces have been split at the corresponding level to allow a group of wetted surfaces to be created.

Water level
      
     equation-based-loading-1

The hydrostatic pressure (P) is a function of the fluid density (rho), acceleration due to gravity (g), and fluid depth (h). For water, and using the mm/tonnes/s consistent set of units in this model, this simplifies to:
  1. P = rho * g * h
Note that “!z” is the Femap variable that represents the depth of water in the equation.

Instructions

Please follow these step-by-step instructions:
  1. Create a new load definition by opening the Model section in the Model Info tree and right clicking Loads.
  2. Select New and enter a Title in the New Load Set dialog, then click OK.
  3. Expand the Loads section of the Model Info tree and right click Load Definitions and select On Surface. You should now select the surfaces that represent the wetted area of the model in the Entity Selection dialog.
  4. In the Create Loads on Surfaces dialog, select Pressure as the load type.
  5. In the Load section of the form, enter 1 as the Pressure.
  6. In the Coord Sys box, select the local coordinate system that is positioned at the water level (this needs to have been defined previously).
  7. In the Method section of the form, select Variable, then click the Advanced button. load editor, variable
  8. In the Advanced Load Methods dialog select Equation and enter the equation 9.79e-6*!z in the Equation box.
  9. Click OK and OK again. 
     Advanced load method dialog
  10. The surface load markers are now visible, but to see the actual element loads that have been created select Model | Load | Expand in the menu.
  11. In the Expand Geometry Loads dialog, click the Convert to Node/Elem checkbox and click OK, then Yes in the confirmation dialog. The elemental loads are then displayed.
            
visualized hydrostatic load

Video Demonstration


    • Related Articles

    • Temperature Loading Import from Excel

      Overview Sometimes element or nodal temperature distributions that are created by thermal solvers are only available in the form of a spreadsheet. We would like to take these values and turn them into a load case for subsequent analysis, so let’s see ...

    • Load Spreading in Femap

      What is in this webinar? This webinar will explain how to spread loads on your model using data surfaces through the Data Surface Editor. The following topics will be covered: What is load spreading? How external data, such as a pressure map, can be ...

    • Model Bounding Box

      What is the Femap Model Bounding Box, and why is it important? The Femap Model Bounding Box is a hexahedral cuboid constructed from planes that bound the model in the x, y, and z axes. The longest diagonal of the model bounding box is used to ...

    • An Advanced Overview of Freebodies in Femap

      Introduction This guide provides an in-depth overview of freebodies in Femap. If you would like to see the breakdown of each particular step and get a better understanding of freebodies, view the accompanying webinar hosted by Russ Hilley. What is a ...

    • UI Layout and Views

      Overview Once you have the Femap user interface set the way you like it, with the desired arrangement of windows, panes and view attributes, you can save both the layout and the view so that you can easily reset them should the need arise. User ...