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

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:

- P = rho * g * h

Note that “!z” is the Femap variable that represents the depth of water in the equation.

Please follow these step-by-step instructions:

- Create a new load definition by opening the
**Model**section in the*Model Info*tree and right clicking**Loads**. - Select
**New**and enter a**Title**in the*New Load Set*dialog, then click**OK**. - 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. - In the
*Create Loads on Surfaces*dialog, select**Pressure**as the load type. - In the
*Load*section of the form, enter**1**as the*Pressure*. - In the
*Coord Sys*box, select the local coordinate system that is positioned at the water level (this needs to have been defined previously). - In the
*Method*section of the form, select**Variable**, then click the**Advanced**button. - In the
*Advanced Load Methods*dialog select**Equation**and enter the equation**9.79e-6*!z**in the*Equation*box. - Click
**OK**and**OK**again.

- 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. - 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.

# 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 ...## Element Visual Inspection

Overview When FEMAP finishes meshing a model, a brief report of the mesh quality is written to the Messages pane. It's often desirable to visually inspect the worst elements of the mesh, and review their shape, and location in the model, an action ...