## Quick Overview

You may have to define a load or a boundary condition that not only varies as a function of spatial coordinates, but also with time, temperature, or frequency. This Tips & Trick shows how to use Simcenter 3D to create a 4D field, which allows you to model a functional expression of the form:

**f = f(x1,x2,x3,α)**

where x1, x2, and x3 represent a set of cartesian, cylindrical, spherical, or parametric spatial coordinates, and α represents a non-spatial variable like time, temperature, or frequency.

If the 4D functional relationship can be expressed as a closed-form mathematical expression, you can create the 4D field as a formula field. When Simcenter 3D evaluates the formula field for a given set of spatial and non-spatial values, it simply evaluates the expression that relates the independent and dependent domains at the given values.

If the 4D functional relationship can be approximated by a set of tabular data that relates the independent and dependent domains, you can create the 4D field as a table field. When Simcenter 3D evaluates the table field for a given set of spatial and non-spatial values at which a tabular data point does not exist, it interpolates the tabular data to obtain the corresponding dependent domain value. You can select the interpolation method that the software uses to look up values.

In this example we will show how to use a 4D formula field in Simcenter 3D to model the footprint pressure of a roller traveling on a track.

*Figure 1: Model the foot print pressure of a roller travelling on a track.*

*Figure 2: Varying pressure with spatial coordinates and time.*

## Steps

Let’s assume that the roller travels at a speed of 3 mm/sec and has a foot print pressure of 9 mm length (in the X axis) with a maximum pressure of 45 MPa.

**1. Create a field of varying spatial coordinates with time **

Since the roller is moving at a constant speed of 3 mm/sec, the roller’s central location can be simply calculated using the following function:

**X = 3*t**

To create this field, in the **Simulation Navigator** right click on the **Fields** node and select **New Field**, **Formula**.

*Figure 3: Create a formula field.*

In the **Formula Field** dialog, under the **Name** group, enter a meaningful name, for example, X_Center. Then under the **Domain** group, set the **Independent** to time and **Dependent** to Cartesian.

Since in our model the position of the roller changes only along the X axis, under the **Expression** group, select **x** and in the **Rule Formula** box type:

**3[mm/sec]*time**

*Figure 4: Create a formula field for position of the roller with respect to time.*

By end of this step, we defined the varying position of the roller with respect to time. So, we can now proceed to define the pressure field.

**2. Create a field for the pressure**

We assume that the roller footprint pressure is maximum at its center and linearly decreases toward the fore and aft edges of the foot print, in the X direction. The pressure is constant in the other direction on the surface.

*Figure 5: Roller footprint pressure distribution.*

To define a field for the pressure, in the Simulation Navigator right click on the **Fields** node and select **New Field**, **Formula**.

In the **Formula Field** dialog, under the **Domain** group, set the **Independent** to **time,Cartesian** and **Dependent** to **Pressure**. You will notice that the independent variables and the field created in the step1 are listed under the **Expression** group.

We assumed the roller foot print pressure has a length of 9 mm. So, the the pressure formula can be defined as

**if ( abs(x-fd(“X_center”,“x”))<=4.5) Then (10*(4.5-abs(x-fd(“X_center”,“x”)))) Else (0)**

where x is the independent variable, and X_center is the position of the roller, which is varying with time according to the field defined in step 1. Note that to use a value from another field, you need to use the fd(“Fieldname”,”value”) command.

*Figure 6: Define a formula field for the roller foot print pressure.*

**3. Define the pressure load**

To define the pressure load, in the **Simulation Navigator**, right click on Loads, and select **Pressure**.

*Figure 7: Define the pressure load.*

*Figure 8: Pressure dialog.*

In the **Pressure** dialog, under the **Model Objects** group, select the track bed face as the location where the pressure should be applied. Under the **Magnitude** group, click on the equal sign, and then choose **Select Existing Field.**

*Figure 9: Fields dialog.*

In the **Fields** dialog, select the Formula Field, which was defined in Step 2. Click **OK** on all dialogs.

**4. Verify the defined pressure (Optional)**

By the end of step 3, the varying pressure with respect to spatial coordinates and time is already defined and can be used in a solution. Simcenter 3D allows you to plot and animate the applied load to verify whether it is correctly defined and applied to the model.

To plot the varying pressure load, in the **Simulation Navigator**, right click on the pressure load and select **Plot Contours.**

*Figure 10: Plot load contours of the applied pressure.*

*Figure 11: Boundary Condition Contour Plot dialog.*

In the **Boundary Condition Contour Plot** dialog, under the **Selected Boundary Conditions** group select the pressure load. Then under the **Plot Options** group set the **Plot Type** to Animation, and **Independent Variable** to Time. Set the Start, Stop, and Number of Frames to 0, 100, and 33, respectively. Click on the **Plot** icon.

*Figure 12: Contour plot of the applied pressure.*